Loading ...
Sorry, an error occurred while loading the content.
 

Re: Newfangled Wizard Stand Alone, some thoughts

Expand Messages
  • ozzie34231
    Jeff, I fully agree. But I add: Wizards eliminate the need to ever draw the part and so in some cases speed the process. I actually machined the part with the
    Message 1 of 30 , Apr 28 10:50 AM
      Jeff, I fully agree.
      But I add:
      Wizards eliminate the need to ever draw the part and so in some cases speed the process.
      I actually machined the part with the Mach 3 Wiz, then found the new edition would not have been so expeditious.
      Ozzie

      --- In mach1mach2cnc@yahoogroups.com, "Jeffrey Birt" <birt_j@...> wrote:
      >
      > Ramping angle is part of the machining strategy not a tool property. For
      > example knowing what a certain ¼" end mill's feed/speed for aluminum should
      > be does not tell you the ideal machining strategy for doing a pocket with a
      > certain level of finish; that is part of the machining strategy. What I mean
      > to say is that it seems to me that a Tool Library should only incorporate
      > those properties that are inherent to the tool, not things are a properties
      > of the machining strategy. (The machining strategy does incorporate a tool
      > and its properties however.)
      >
      >
      >
      > In a program like CamBam you can define tools in your Tool Library and you
      > can also set up a Style Library (CAM Styles) for more of the machining
      > strategy related settings. A Style might include all the common settings for
      > a particular operation in a particular material. For example, I do a lot of
      > cutting in 6061 aluminum with the same tool so I have a Style set up with
      > those settings for that tool. So you could have a Style set up for ramping
      > and a separate for plunging down if you want. There is somewhat of an
      > overlap between Tool Library and Styles Libraries, i.e. the RPM/federate per
      > material for a particular material, but everything else if more of a
      > machining strategy not a tool property.
      >
      >
      >
      > In your example of a pocket with an open bottom. I would set that up in two
      > or more operations. The first would be a pocketing operation and the second
      > would be a profile operation to finish the sides. Then if I decide I want to
      > cut the pocket with a larger tool to save time I can set up the finish
      > pass(es) to use a smaller tool. There is not `one' pocketing operation that
      > can account for every variable in possible machining strategies.
      >
      >
      >
      > Just me 2 pence…
      >
      >
      >
      > Jeff Birt
      >
      > Soigeneris.com
      >
      >
      >
      > From: mach1mach2cnc@yahoogroups.com [mailto:mach1mach2cnc@yahoogroups.com]
      > On Behalf Of ozzie34231
      > Sent: Sunday, April 28, 2013 10:59 AM
      > To: mach1mach2cnc@yahoogroups.com
      > Subject: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
      >
      >
      >
      >
      >
      >
      >
      > Ron,
      > I understand that there are many ways to do machining and therefore write
      > wizards. And I appreciate all the time it must have taken to write the new
      > product. But please look at these couple issues with an open mind.
      > Some end mills cannot plunge, but all end mills that can plunge can also
      > ramp. So to make ramp angle part of the tool description, eliminates the
      > possibility to plunge. Lead-ins are part of a milling strategy. Cambam,
      > Solidcam, Mastercam, and others all agree with that.
      > Does it make a difference? I think yes. In the example I already sighted, my
      > pocket is a through hole, it has no bottom. And because of the rounded
      > corners I must use a mill of a size that is relatively small compared to the
      > dimensions of the pocket.(3/8" mill, Pocket almost 2" X 3".) Using the
      > wizard the pocket cuts fine, but then we get to a finish cut.
      > In the Mach 3 version, although the main cuts were done with a ramp angle,
      > in the finish cut the tool plunges down full depth, through air at a place
      > away from the pocket wall, then moves to the wall and makes a trip around
      > taking away the last couple thou.
      > In the new version, (standalone), the tool goes to the ramp down place,
      > spirals down slowly, (it doesn't know it's cutting air), and then proceeds
      > to cut the non-existent bottom away. This take quite a while even with a
      > step-over of 75%. Then finally the last few lines of code make the finish
      > cut.
      > I don't think this an unusual example.
      > So my plea is to make the new operations more like the old. Put finishing on
      > the operation page, put ramp and plunge there also.
      > All the other things you've added are great
      > Thanks for your consideration
      > Ozzie
      >
      > --- In mach1mach2cnc@yahoogroups.com
      > <mailto:mach1mach2cnc%40yahoogroups.com> , Ron Ginger <ronginger@> wrote:
      > >
      > >
      > > > Ya, i second this also. The wizards are nice, but some things i think
      > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
      > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
      > spiral down in CW or CCW and not both. Both directions or back and forth can
      > cause undesired tool deflections.
      > >
      > > Brian changed that yesterday- circles now ramp down in the same
      > > direction, taking as far around the circle as needed to get get to
      > > depth, then finishing that pass at a constant depth. Actually that was
      > > how I had it at first, then Brian figured out his zig-zag cut and we
      > > changed it.
      > >
      > > Pockets do a spiral down to step depth in the center of the pocket, then
      > > cut that step at a constant depth.
      > >
      > > > IMHO ramping IS NOT at tool function, but rather part of a machining
      > strategy. In the new program if I want to use the same tool for a ramped
      > entry and the later in the same feature to plunge feed, I must create two
      > tools, and have to deal with the machine thinking there is a tool change
      > when none is needed.
      > >
      > >
      > > I believe the ramp angle is a tool property- some tools will not plunge-
      > > think an insert mill, or non-center cutting end mills. Yes, there are
      > > tools that can do both, but there are plenty that cannot. Ramping always
      > > gives a better cut than plunge.
      > >
      > > > Then there is the problem of not having a finish pass without using a
      > separate operation. The pocket I was making was about 2" X 2" with .25"
      > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that
      > a single down step, and then a new pocket size to cut the last couple thou
      > away. The problem is that I cut air seemingly endlessly to get to actually
      > cut. Another way to finish is cutting the inside of a rectangle to make a
      > final cut. Well that works, but if you've been using a ramped entry for the
      > first operation, the tool wanders back and forth until it reaches full
      > depth.
      > >
      > > If you are doing a pocket you can apply the finish amount to both the
      > > side and bottom of the pocket. Set the step depth to the same as the
      > > finish depth on your second pocket and you will never cut air. You can
      > > now have a Ztop value lower that 0, so you could do a finish cut with
      > > Ztop at you finish depth minus total depth.
      > >
      > > One of the problems of writing wizards is that every operation can have
      > > multiple solutions. I have tried to give lots of options, but in the end
      > > I can only program some of the options. I am sorry this cannot be the
      > > solution to every case, but wizards are supposed to offer the simple,
      > > common needs.
      > >
      > > Thanks for the feedback, I try to look at it all and will continue to
      > > make changes and additions when it seems like it will improve the wizards.
      > >
      > > ron ginger
      > >
      >
      >
      >
      >
      >
      > [Non-text portions of this message have been removed]
      >
    • Terry Parker
      Actually IT ONLY allows you to do operations not really complete parts. What is missing is the ability to hand program contours such as outer contours and
      Message 2 of 30 , Apr 28 5:51 PM
        Actually IT ONLY allows you to do operations not really complete parts. What is missing is the ability to hand program contours such as outer contours and special function not done with the wizards. ADD that and you have something.

        (;-) TP


        --- In mach1mach2cnc@yahoogroups.com, "ozzie34231" <OzzieII@...> wrote:
        >
        > Jeff, I fully agree.
        > But I add:
        > Wizards eliminate the need to ever draw the part and so in some cases speed the process.
        > I actually machined the part with the Mach 3 Wiz, then found the new edition would not have been so expeditious.
        > Ozzie
        >
        > --- In mach1mach2cnc@yahoogroups.com, "Jeffrey Birt" <birt_j@> wrote:
        > >
        > > Ramping angle is part of the machining strategy not a tool property. For
        > > example knowing what a certain ¼" end mill's feed/speed for aluminum should
        > > be does not tell you the ideal machining strategy for doing a pocket with a
        > > certain level of finish; that is part of the machining strategy. What I mean
        > > to say is that it seems to me that a Tool Library should only incorporate
        > > those properties that are inherent to the tool, not things are a properties
        > > of the machining strategy. (The machining strategy does incorporate a tool
        > > and its properties however.)
        > >
        > >
        > >
        > > In a program like CamBam you can define tools in your Tool Library and you
        > > can also set up a Style Library (CAM Styles) for more of the machining
        > > strategy related settings. A Style might include all the common settings for
        > > a particular operation in a particular material. For example, I do a lot of
        > > cutting in 6061 aluminum with the same tool so I have a Style set up with
        > > those settings for that tool. So you could have a Style set up for ramping
        > > and a separate for plunging down if you want. There is somewhat of an
        > > overlap between Tool Library and Styles Libraries, i.e. the RPM/federate per
        > > material for a particular material, but everything else if more of a
        > > machining strategy not a tool property.
        > >
        > >
        > >
        > > In your example of a pocket with an open bottom. I would set that up in two
        > > or more operations. The first would be a pocketing operation and the second
        > > would be a profile operation to finish the sides. Then if I decide I want to
        > > cut the pocket with a larger tool to save time I can set up the finish
        > > pass(es) to use a smaller tool. There is not `one' pocketing operation that
        > > can account for every variable in possible machining strategies.
        > >
        > >
        > >
        > > Just me 2 pence…
        > >
        > >
        > >
        > > Jeff Birt
        > >
        > > Soigeneris.com
        > >
        > >
        > >
        > > From: mach1mach2cnc@yahoogroups.com [mailto:mach1mach2cnc@yahoogroups.com]
        > > On Behalf Of ozzie34231
        > > Sent: Sunday, April 28, 2013 10:59 AM
        > > To: mach1mach2cnc@yahoogroups.com
        > > Subject: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
        > >
        > >
        > >
        > >
        > >
        > >
        > >
        > > Ron,
        > > I understand that there are many ways to do machining and therefore write
        > > wizards. And I appreciate all the time it must have taken to write the new
        > > product. But please look at these couple issues with an open mind.
        > > Some end mills cannot plunge, but all end mills that can plunge can also
        > > ramp. So to make ramp angle part of the tool description, eliminates the
        > > possibility to plunge. Lead-ins are part of a milling strategy. Cambam,
        > > Solidcam, Mastercam, and others all agree with that.
        > > Does it make a difference? I think yes. In the example I already sighted, my
        > > pocket is a through hole, it has no bottom. And because of the rounded
        > > corners I must use a mill of a size that is relatively small compared to the
        > > dimensions of the pocket.(3/8" mill, Pocket almost 2" X 3".) Using the
        > > wizard the pocket cuts fine, but then we get to a finish cut.
        > > In the Mach 3 version, although the main cuts were done with a ramp angle,
        > > in the finish cut the tool plunges down full depth, through air at a place
        > > away from the pocket wall, then moves to the wall and makes a trip around
        > > taking away the last couple thou.
        > > In the new version, (standalone), the tool goes to the ramp down place,
        > > spirals down slowly, (it doesn't know it's cutting air), and then proceeds
        > > to cut the non-existent bottom away. This take quite a while even with a
        > > step-over of 75%. Then finally the last few lines of code make the finish
        > > cut.
        > > I don't think this an unusual example.
        > > So my plea is to make the new operations more like the old. Put finishing on
        > > the operation page, put ramp and plunge there also.
        > > All the other things you've added are great
        > > Thanks for your consideration
        > > Ozzie
        > >
        > > --- In mach1mach2cnc@yahoogroups.com
        > > <mailto:mach1mach2cnc%40yahoogroups.com> , Ron Ginger <ronginger@> wrote:
        > > >
        > > >
        > > > > Ya, i second this also. The wizards are nice, but some things i think
        > > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
        > > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
        > > spiral down in CW or CCW and not both. Both directions or back and forth can
        > > cause undesired tool deflections.
        > > >
        > > > Brian changed that yesterday- circles now ramp down in the same
        > > > direction, taking as far around the circle as needed to get get to
        > > > depth, then finishing that pass at a constant depth. Actually that was
        > > > how I had it at first, then Brian figured out his zig-zag cut and we
        > > > changed it.
        > > >
        > > > Pockets do a spiral down to step depth in the center of the pocket, then
        > > > cut that step at a constant depth.
        > > >
        > > > > IMHO ramping IS NOT at tool function, but rather part of a machining
        > > strategy. In the new program if I want to use the same tool for a ramped
        > > entry and the later in the same feature to plunge feed, I must create two
        > > tools, and have to deal with the machine thinking there is a tool change
        > > when none is needed.
        > > >
        > > >
        > > > I believe the ramp angle is a tool property- some tools will not plunge-
        > > > think an insert mill, or non-center cutting end mills. Yes, there are
        > > > tools that can do both, but there are plenty that cannot. Ramping always
        > > > gives a better cut than plunge.
        > > >
        > > > > Then there is the problem of not having a finish pass without using a
        > > separate operation. The pocket I was making was about 2" X 2" with .25"
        > > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that
        > > a single down step, and then a new pocket size to cut the last couple thou
        > > away. The problem is that I cut air seemingly endlessly to get to actually
        > > cut. Another way to finish is cutting the inside of a rectangle to make a
        > > final cut. Well that works, but if you've been using a ramped entry for the
        > > first operation, the tool wanders back and forth until it reaches full
        > > depth.
        > > >
        > > > If you are doing a pocket you can apply the finish amount to both the
        > > > side and bottom of the pocket. Set the step depth to the same as the
        > > > finish depth on your second pocket and you will never cut air. You can
        > > > now have a Ztop value lower that 0, so you could do a finish cut with
        > > > Ztop at you finish depth minus total depth.
        > > >
        > > > One of the problems of writing wizards is that every operation can have
        > > > multiple solutions. I have tried to give lots of options, but in the end
        > > > I can only program some of the options. I am sorry this cannot be the
        > > > solution to every case, but wizards are supposed to offer the simple,
        > > > common needs.
        > > >
        > > > Thanks for the feedback, I try to look at it all and will continue to
        > > > make changes and additions when it seems like it will improve the wizards.
        > > >
        > > > ron ginger
        > > >
        > >
        > >
        > >
        > >
        > >
        > > [Non-text portions of this message have been removed]
        > >
        >
      • jeremywillson
        You already have that program, it is called Notepad [:)] ... parts. What is missing is the ability to hand program contours such as outer contours and
        Message 3 of 30 , Apr 28 9:36 PM
          You already have that program, it is called 'Notepad' [:)]


          --- In mach1mach2cnc@yahoogroups.com, "Terry Parker" wrote:
          >
          >
          > Actually IT ONLY allows you to do operations not really complete
          parts. What is missing is the ability to hand program contours such as
          outer contours and special function not done with the wizards. ADD that
          and you have something.
          >
          > (;-) TP
          >
          >
          > --- In mach1mach2cnc@yahoogroups.com, "ozzie34231" OzzieII@ wrote:
          > >
          > > Jeff, I fully agree.
          > > But I add:
          > > Wizards eliminate the need to ever draw the part and so in some
          cases speed the process.
          > > I actually machined the part with the Mach 3 Wiz, then found the new
          edition would not have been so expeditious.
          > > Ozzie
          > >
          > > --- In mach1mach2cnc@yahoogroups.com, "Jeffrey Birt" wrote:
          > > >
          > > > Ramping angle is part of the machining strategy not a tool
          property. For
          > > > example knowing what a certain �" end mill's feed/speed for
          aluminum should
          > > > be does not tell you the ideal machining strategy for doing a
          pocket with a
          > > > certain level of finish; that is part of the machining strategy.
          What I mean
          > > > to say is that it seems to me that a Tool Library should only
          incorporate
          > > > those properties that are inherent to the tool, not things are a
          properties
          > > > of the machining strategy. (The machining strategy does
          incorporate a tool
          > > > and its properties however.)
          > > >
          > > >
          > > >
          > > > In a program like CamBam you can define tools in your Tool Library
          and you
          > > > can also set up a Style Library (CAM Styles) for more of the
          machining
          > > > strategy related settings. A Style might include all the common
          settings for
          > > > a particular operation in a particular material. For example, I do
          a lot of
          > > > cutting in 6061 aluminum with the same tool so I have a Style set
          up with
          > > > those settings for that tool. So you could have a Style set up for
          ramping
          > > > and a separate for plunging down if you want. There is somewhat of
          an
          > > > overlap between Tool Library and Styles Libraries, i.e. the
          RPM/federate per
          > > > material for a particular material, but everything else if more of
          a
          > > > machining strategy not a tool property.
          > > >
          > > >
          > > >
          > > > In your example of a pocket with an open bottom. I would set that
          up in two
          > > > or more operations. The first would be a pocketing operation and
          the second
          > > > would be a profile operation to finish the sides. Then if I decide
          I want to
          > > > cut the pocket with a larger tool to save time I can set up the
          finish
          > > > pass(es) to use a smaller tool. There is not `one' pocketing
          operation that
          > > > can account for every variable in possible machining strategies.
          > > >
          > > >
          > > >
          > > > Just me 2 pence�
          > > >
          > > >
          > > >
          > > > Jeff Birt
          > > >
          > > > Soigeneris.com
          > > >
          > > >
          > > >
          > > > From: mach1mach2cnc@yahoogroups.com
          [mailto:mach1mach2cnc@yahoogroups.com]
          > > > On Behalf Of ozzie34231
          > > > Sent: Sunday, April 28, 2013 10:59 AM
          > > > To: mach1mach2cnc@yahoogroups.com
          > > > Subject: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some
          thoughts
          > > >
          > > >
          > > >
          > > >
          > > >
          > > >
          > > >
          > > > Ron,
          > > > I understand that there are many ways to do machining and
          therefore write
          > > > wizards. And I appreciate all the time it must have taken to write
          the new
          > > > product. But please look at these couple issues with an open mind.
          > > > Some end mills cannot plunge, but all end mills that can plunge
          can also
          > > > ramp. So to make ramp angle part of the tool description,
          eliminates the
          > > > possibility to plunge. Lead-ins are part of a milling strategy.
          Cambam,
          > > > Solidcam, Mastercam, and others all agree with that.
          > > > Does it make a difference? I think yes. In the example I already
          sighted, my
          > > > pocket is a through hole, it has no bottom. And because of the
          rounded
          > > > corners I must use a mill of a size that is relatively small
          compared to the
          > > > dimensions of the pocket.(3/8" mill, Pocket almost 2" X 3".) Using
          the
          > > > wizard the pocket cuts fine, but then we get to a finish cut.
          > > > In the Mach 3 version, although the main cuts were done with a
          ramp angle,
          > > > in the finish cut the tool plunges down full depth, through air at
          a place
          > > > away from the pocket wall, then moves to the wall and makes a trip
          around
          > > > taking away the last couple thou.
          > > > In the new version, (standalone), the tool goes to the ramp down
          place,
          > > > spirals down slowly, (it doesn't know it's cutting air), and then
          proceeds
          > > > to cut the non-existent bottom away. This take quite a while even
          with a
          > > > step-over of 75%. Then finally the last few lines of code make the
          finish
          > > > cut.
          > > > I don't think this an unusual example.
          > > > So my plea is to make the new operations more like the old. Put
          finishing on
          > > > the operation page, put ramp and plunge there also.
          > > > All the other things you've added are great
          > > > Thanks for your consideration
          > > > Ozzie
          > > >
          > > > --- In mach1mach2cnc@yahoogroups.com
          > > > , Ron Ginger wrote:
          > > > >
          > > > >
          > > > > > Ya, i second this also. The wizards are nice, but some things
          i think
          > > > need tweeking. Maybe this is why its in Beta.Another thing i liked
          with the
          > > > NFW for Mach3 concerning ramping, is when doing a circle, the tool
          would
          > > > spiral down in CW or CCW and not both. Both directions or back and
          forth can
          > > > cause undesired tool deflections.
          > > > >
          > > > > Brian changed that yesterday- circles now ramp down in the same
          > > > > direction, taking as far around the circle as needed to get get
          to
          > > > > depth, then finishing that pass at a constant depth. Actually
          that was
          > > > > how I had it at first, then Brian figured out his zig-zag cut
          and we
          > > > > changed it.
          > > > >
          > > > > Pockets do a spiral down to step depth in the center of the
          pocket, then
          > > > > cut that step at a constant depth.
          > > > >
          > > > > > IMHO ramping IS NOT at tool function, but rather part of a
          machining
          > > > strategy. In the new program if I want to use the same tool for a
          ramped
          > > > entry and the later in the same feature to plunge feed, I must
          create two
          > > > tools, and have to deal with the machine thinking there is a tool
          change
          > > > when none is needed.
          > > > >
          > > > >
          > > > > I believe the ramp angle is a tool property- some tools will not
          plunge-
          > > > > think an insert mill, or non-center cutting end mills. Yes,
          there are
          > > > > tools that can do both, but there are plenty that cannot.
          Ramping always
          > > > > gives a better cut than plunge.
          > > > >
          > > > > > Then there is the problem of not having a finish pass without
          using a
          > > > separate operation. The pocket I was making was about 2" X 2" with
          .25"
          > > > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron
          suggests that
          > > > a single down step, and then a new pocket size to cut the last
          couple thou
          > > > away. The problem is that I cut air seemingly endlessly to get to
          actually
          > > > cut. Another way to finish is cutting the inside of a rectangle to
          make a
          > > > final cut. Well that works, but if you've been using a ramped
          entry for the
          > > > first operation, the tool wanders back and forth until it reaches
          full
          > > > depth.
          > > > >
          > > > > If you are doing a pocket you can apply the finish amount to
          both the
          > > > > side and bottom of the pocket. Set the step depth to the same as
          the
          > > > > finish depth on your second pocket and you will never cut air.
          You can
          > > > > now have a Ztop value lower that 0, so you could do a finish cut
          with
          > > > > Ztop at you finish depth minus total depth.
          > > > >
          > > > > One of the problems of writing wizards is that every operation
          can have
          > > > > multiple solutions. I have tried to give lots of options, but in
          the end
          > > > > I can only program some of the options. I am sorry this cannot
          be the
          > > > > solution to every case, but wizards are supposed to offer the
          simple,
          > > > > common needs.
          > > > >
          > > > > Thanks for the feedback, I try to look at it all and will
          continue to
          > > > > make changes and additions when it seems like it will improve
          the wizards.
          > > > >
          > > > > ron ginger
          > > > >
          > > >
          > > >
          > > >
          > > >
          > > >
          > > > [Non-text portions of this message have been removed]
          > > >
          > >
          >



          [Non-text portions of this message have been removed]
        • Ron Ginger
          ... In this case I would make it just a rectangle cut- if you are taking the pocket all the way through the material, just cut a rectangle and let the center
          Message 4 of 30 , Apr 29 4:56 AM
            > In the Mach 3 version, although the main cuts were done with a ramp angle, in the finish cut the tool plunges down full depth, through air at a place away from the pocket wall, then moves to the wall and makes a trip around taking away the last couple thou.
            > In the new version, (standalone), the tool goes to the ramp down place, spirals down slowly, (it doesn't know it's cutting air), and then proceeds to cut the non-existent bottom away. This take quite a while even with a step-over of 75%. Then finally the last few lines of code make the finish cut.

            In this case I would make it just a rectangle cut- if you are taking the
            pocket all the way through the material, just cut a rectangle and let
            the center block fall out, why cut it in chips?

            If it is necessary to cut as a pocket, then make the finish cut a simple
            rectangle, that will not do any bottom finish.

            I worry about restricting the finish cut to one full depth pass,
            although that is probably the most common operation. If I get convinced
            that a one depth finish pass is Ok I can add the finish pass.

            I am going to Brians today to plan our next few changes or additions, we
            will review this one carefully.

            > Posted by: "Terry Parker" vmax549@... vmax549
            > Date: Sun Apr 28, 2013 5:51 pm ((PDT))
            >
            >
            > Actually IT ONLY allows you to do operations not really complete parts. What is missing is the ability to hand program contours such as outer contours and special function not done with the wizards. ADD that and you have something.
            >
            > (;-) TP

            I have been thinking about a polyline operation. You would see a
            spreadsheet style input box for X,Y values- just like the one for list
            of holes. You could either type in values, or load them from a cvs file
            generated by a spreadsheet, or a program.

            The cut path would move to the first entry, plunge down to Zdepth (or
            use the zig-zag ramp), then follow point to point down the line- Unless
            I force it to be a closed path I cannot do inside/outside, so I have to
            follow the line.

            Would this be a useful operation?

            I am planning to add a Gcode Operation where you can simply enter your
            line of code. You could make it a startup block, an end block, or
            between any other operations.

            I am thinking about a blank text box you fill in, but also some kind of
            library of code snips you select from. I have not quite figured out how
            I want to do the library part yet. Suggestions?

            ron ginger
          • Terry Wellman
            We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual Mill ported into Rhino as a plug-in. It has a good tool library function. Is there a way
            Message 5 of 30 , Apr 29 8:55 AM
              We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual Mill ported into Rhino as a plug-in. It has a good tool library function. Is there a way to import the tool library from Rhino Cam into Mach so that I don't have to recreate the whole thing? We have a bunch of tooling listed there already. It would be great if I could do that. Then again, I haven't gone back to the manual and might be violating RTFM Code 1. ;-)

              Thanks,
              Terry Wellman
            • Henrik Olsson
              Hi Terry, The short answer is no, not really (at least not in Mach3, I don t know about Mach4). The long answer is that Mach3 doesn t have any functionality
              Message 6 of 30 , Apr 29 10:32 AM
                Hi Terry,

                The short answer is no, not really (at least not in Mach3, I don't know
                about Mach4).



                The long answer is that Mach3 doesn't have any functionality built in to do
                this but it does have scripting capability so it might be possible to write
                a simple importer that reads the tool library file and stuffs the info into
                Mach3's tooltable. Obviously the possible success of such an effort depends
                on if the format of the tool library, as exported from Rhino, is published
                and/or if it's simple text files so one can figure it out by just looking at
                the file.



                Over the years the issue of exporting the tooltable FROM Mach3 have been
                covered numerous times on this list but I can't remember importing tools
                being discussed. Do you have any info on the actual format of the tool
                library file you want to import?



                /Henrik.



                _____

                ---Original message---

                We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual Mill
                ported into Rhino as a plug-in. It has a good tool library function. Is
                there a way to import the tool library from Rhino Cam into Mach so that I
                don't have to recreate the whole thing? We have a bunch of tooling listed
                there already. It would be great if I could do that. Then again, I haven't
                gone back to the manual and might be violating RTFM Code 1. ;-)

                Thanks,
                Terry Wellman



                [Non-text portions of this message have been removed]
              • Freeman P. Pascal IV
                Personally, I would love to see Mach 4 support a tool library format that was standard between many CAD/CAM packages. I hate having to maintain my tool
                Message 7 of 30 , Apr 29 1:04 PM
                  Personally, I would love to see Mach 4 support a tool library format that
                  was standard between many CAD/CAM packages. I hate having to maintain my
                  tool library across multiple packages. Ideally, it would be nice if I could
                  point all my software to a common data source.



                  A quick google did not reveal any standard tool library formats, but I
                  wouldn't be surprised if there was something that was industry supported.
                  If there isn't, perhaps an XML scheme could be devised to provide such
                  support, at least between Mach 4 (possibly Mach 3) and NFW external wizards.
                  You would be surprised how simply publishing an exchange format would
                  promote its use.





                  -Freeman



                  _____

                  From: mach1mach2cnc@yahoogroups.com [mailto:mach1mach2cnc@yahoogroups.com]
                  On Behalf Of Henrik Olsson
                  Sent: Monday, April 29, 2013 11:33 AM
                  To: mach1mach2cnc@yahoogroups.com
                  Subject: Re: [mach1mach2cnc] Can I import a tool library into Mach3 or soon
                  4?





                  Hi Terry,

                  The short answer is no, not really (at least not in Mach3, I don't know
                  about Mach4).

                  The long answer is that Mach3 doesn't have any functionality built in to do
                  this but it does have scripting capability so it might be possible to write
                  a simple importer that reads the tool library file and stuffs the info into
                  Mach3's tooltable. Obviously the possible success of such an effort depends
                  on if the format of the tool library, as exported from Rhino, is published
                  and/or if it's simple text files so one can figure it out by just looking at
                  the file.

                  Over the years the issue of exporting the tooltable FROM Mach3 have been
                  covered numerous times on this list but I can't remember importing tools
                  being discussed. Do you have any info on the actual format of the tool
                  library file you want to import?

                  /Henrik.

                  _____

                  ---Original message---

                  We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual Mill
                  ported into Rhino as a plug-in. It has a good tool library function. Is
                  there a way to import the tool library from Rhino Cam into Mach so that I
                  don't have to recreate the whole thing? We have a bunch of tooling listed
                  there already. It would be great if I could do that. Then again, I haven't
                  gone back to the manual and might be violating RTFM Code 1. ;-)

                  Thanks,
                  Terry Wellman

                  [Non-text portions of this message have been removed]





                  [Non-text portions of this message have been removed]
                • Brian Barker
                  No standards at this time.. I think what we write should become the standard ;) We are going to make it so you can save and load a tooltable.. So you should be
                  Message 8 of 30 , Apr 29 1:07 PM
                    No standards at this time.. I think what we write should become the
                    standard ;)

                    We are going to make it so you can save and load a tooltable.. So you
                    should be able to make a converter program...

                    On 4/29/2013 4:04 PM, Freeman P. Pascal IV wrote:
                    > Personally, I would love to see Mach 4 support a tool library format that
                    > was standard between many CAD/CAM packages. I hate having to maintain my
                    > tool library across multiple packages. Ideally, it would be nice if I could
                    > point all my software to a common data source.
                    >
                    >
                    >
                    > A quick google did not reveal any standard tool library formats, but I
                    > wouldn't be surprised if there was something that was industry supported.
                    > If there isn't, perhaps an XML scheme could be devised to provide such
                    > support, at least between Mach 4 (possibly Mach 3) and NFW external wizards.
                    > You would be surprised how simply publishing an exchange format would
                    > promote its use.
                    >
                    >
                    >
                    >
                    >
                    > -Freeman
                    >
                    >
                    >
                    > _____
                    >
                    > From: mach1mach2cnc@yahoogroups.com [mailto:mach1mach2cnc@yahoogroups.com]
                    > On Behalf Of Henrik Olsson
                    > Sent: Monday, April 29, 2013 11:33 AM
                    > To: mach1mach2cnc@yahoogroups.com
                    > Subject: Re: [mach1mach2cnc] Can I import a tool library into Mach3 or soon
                    > 4?
                    >
                    >
                    >
                    >
                    >
                    > Hi Terry,
                    >
                    > The short answer is no, not really (at least not in Mach3, I don't know
                    > about Mach4).
                    >
                    > The long answer is that Mach3 doesn't have any functionality built in to do
                    > this but it does have scripting capability so it might be possible to write
                    > a simple importer that reads the tool library file and stuffs the info into
                    > Mach3's tooltable. Obviously the possible success of such an effort depends
                    > on if the format of the tool library, as exported from Rhino, is published
                    > and/or if it's simple text files so one can figure it out by just looking at
                    > the file.
                    >
                    > Over the years the issue of exporting the tooltable FROM Mach3 have been
                    > covered numerous times on this list but I can't remember importing tools
                    > being discussed. Do you have any info on the actual format of the tool
                    > library file you want to import?
                    >
                    > /Henrik.
                    >
                    > _____
                    >
                    > ---Original message---
                    >
                    > We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual Mill
                    > ported into Rhino as a plug-in. It has a good tool library function. Is
                    > there a way to import the tool library from Rhino Cam into Mach so that I
                    > don't have to recreate the whole thing? We have a bunch of tooling listed
                    > there already. It would be great if I could do that. Then again, I haven't
                    > gone back to the manual and might be violating RTFM Code 1. ;-)
                    >
                    > Thanks,
                    > Terry Wellman
                    >
                    > [Non-text portions of this message have been removed]
                    >
                    >
                    >
                    >
                    >
                    > [Non-text portions of this message have been removed]
                    >
                    >
                    >
                    > ------------------------------------
                    >
                    > www.machsupport.com - Web site AccessYahoo! Groups Links
                    >
                    >
                    >
                    >
                  • quadconversions
                    A In a message dated 29/04/2013 21:07:48 GMT Daylight Time, brianb@machsupport.com writes: No standards at this time.. I think what we write should become the
                    Message 9 of 30 , Apr 29 2:25 PM
                      A


                      In a message dated 29/04/2013 21:07:48 GMT Daylight Time,
                      brianb@... writes:

                      No standards at this time.. I think what we write should become the
                      standard ;)

                      We are going to make it so you can save and load a tooltable.. So you
                      should be able to make a converter program...

                      On 4/29/2013 4:04 PM, Freeman P. Pascal IV wrote:
                      > Personally, I would love to see Mach 4 support a tool library format that
                      > was standard between many CAD/CAM packages. I hate having to maintain my
                      > tool library across multiple packages. Ideally, it would be nice if I
                      could
                      > point all my software to a common data source.
                      >
                      >
                      >
                      > A quick google did not reveal any standard tool library formats, but I
                      > wouldn't be surprised if there was something that was industry
                      supported.
                      > If there isn't, perhaps an XML scheme could be devised to provide such
                      > support, at least between Mach 4 (possibly Mach 3) and NFW external
                      wizards.
                      > You would be surprised how simply publishing an exchange format would
                      > promote its use.
                      >
                      >
                      >
                      >
                      >
                      > -Freeman
                      >
                      >
                      >
                      > _____
                      >
                      > From: mach1mach2cnc@yahoogroups.com
                      [mailto:mach1mach2cnc@yahoogroups.com]
                      > On Behalf Of Henrik Olsson
                      > Sent: Monday, April 29, 2013 11:33 AM
                      > To: mach1mach2cnc@yahoogroups.com
                      > Subject: Re: [mach1mach2cnc] Can I import a tool library into Mach3 or
                      soon
                      > 4?
                      >
                      >
                      >
                      >
                      >
                      > Hi Terry,
                      >
                      > The short answer is no, not really (at least not in Mach3, I don't know
                      > about Mach4).
                      >
                      > The long answer is that Mach3 doesn't have any functionality built in to
                      do
                      > this but it does have scripting capability so it might be possible to
                      write
                      > a simple importer that reads the tool library file and stuffs the info
                      into
                      > Mach3's tooltable. Obviously the possible success of such an effort
                      depends
                      > on if the format of the tool library, as exported from Rhino, is
                      published
                      > and/or if it's simple text files so one can figure it out by just
                      looking at
                      > the file.
                      >
                      > Over the years the issue of exporting the tooltable FROM Mach3 have been
                      > covered numerous times on this list but I can't remember importing tools
                      > being discussed. Do you have any info on the actual format of the tool
                      > library file you want to import?
                      >
                      > /Henrik.
                      >
                      > _____
                      >
                      > ---Original message---
                      >
                      > We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual
                      Mill
                      > ported into Rhino as a plug-in. It has a good tool library function. Is
                      > there a way to import the tool library from Rhino Cam into Mach so that I
                      > don't have to recreate the whole thing? We have a bunch of tooling listed
                      > there already. It would be great if I could do that. Then again, I
                      haven't
                      > gone back to the manual and might be violating RTFM Code 1. ;-)
                      >
                      > Thanks,
                      > Terry Wellman
                      >
                      > [Non-text portions of this message have been removed]
                      >
                      >
                      >
                      >
                      >
                      > [Non-text portions of this message have been removed]
                      >
                      >
                      >
                      > ------------------------------------
                      >
                      > www.machsupport.com - Web site AccessYahoo! Groups Links
                      >
                      >
                      >
                      >


                      ------------------------------------

                      www.machsupport.com - Web site AccessYahoo! Groups Links






                      [Non-text portions of this message have been removed]
                    • quadconversions
                      blessed laptops... As a user of Rhino and Rhinocam ... why would you want to use wizards? If you re a Rhino user it would be a quick job to draw any of the
                      Message 10 of 30 , Apr 29 2:51 PM
                        blessed laptops... As a user of Rhino and Rhinocam ... why would you want
                        to use wizards? If you're a Rhino user it would be a quick job to draw any
                        of the simple operations in the wizards and run them though Rhinocam. The
                        wizards are for the people who don't want to invest in the software like
                        Rhino. Ron said he wasn't trying to re-create Solid Works. I agree it would
                        be good if the tool libary was an industrial standard. But, Rhino to Mach
                        wizards? If you're lucky enough to have several advanced Cam programs why
                        would you want Brian waste his time making wizard tool libraries compatable?


                        In a message dated 29/04/2013 22:25:14 GMT Daylight Time,
                        _qcoanvers@..._ (mailto:qcoanvers@...) writes:

                        A


                        In a message dated 29/04/2013 21:07:48 GMT Daylight Time,
                        brianb@... writes:

                        No standards at this time.. I think what we write should become the
                        standard ;)

                        We are going to make it so you can save and load a tooltable.. So you
                        should be able to make a converter program...

                        On 4/29/2013 4:04 PM, Freeman P. Pascal IV wrote:
                        > Personally, I would love to see Mach 4 support a tool library format
                        that
                        > was standard between many CAD/CAM packages. I hate having to maintain
                        my
                        > tool library across multiple packages. Ideally, it would be nice if I
                        could
                        > point all my software to a common data source.
                        >
                        >
                        >
                        > A quick google did not reveal any standard tool library formats, but I
                        > wouldn't be surprised if there was something that was industry
                        supported.
                        > If there isn't, perhaps an XML scheme could be devised to provide such
                        > support, at least between Mach 4 (possibly Mach 3) and NFW external
                        wizards.
                        > You would be surprised how simply publishing an exchange format would
                        > promote its use.
                        >
                        >
                        >
                        >
                        >
                        > -Freeman
                        >
                        >
                        >
                        > _____
                        >
                        > From: mach1mach2cnc@yahoogroups.com
                        [mailto:mach1mach2cnc@yahoogroups.com]
                        > On Behalf Of Henrik Olsson
                        > Sent: Monday, April 29, 2013 11:33 AM
                        > To: mach1mach2cnc@yahoogroups.com
                        > Subject: Re: [mach1mach2cnc] Can I import a tool library into Mach3 or
                        soon
                        > 4?
                        >
                        >
                        >
                        >
                        >
                        > Hi Terry,
                        >
                        > The short answer is no, not really (at least not in Mach3, I don't know
                        > about Mach4).
                        >
                        > The long answer is that Mach3 doesn't have any functionality built in
                        to
                        do
                        > this but it does have scripting capability so it might be possible to
                        write
                        > a simple importer that reads the tool library file and stuffs the info
                        into
                        > Mach3's tooltable. Obviously the possible success of such an effort
                        depends
                        > on if the format of the tool library, as exported from Rhino, is
                        published
                        > and/or if it's simple text files so one can figure it out by just
                        looking at
                        > the file.
                        >
                        > Over the years the issue of exporting the tooltable FROM Mach3 have been
                        > covered numerous times on this list but I can't remember importing
                        tools
                        > being discussed. Do you have any info on the actual format of the tool
                        > library file you want to import?
                        >
                        > /Henrik.
                        >
                        > _____
                        >
                        > ---Original message---
                        >
                        > We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual
                        Mill
                        > ported into Rhino as a plug-in. It has a good tool library function. Is
                        > there a way to import the tool library from Rhino Cam into Mach so that
                        I
                        > don't have to recreate the whole thing? We have a bunch of tooling
                        listed
                        > there already. It would be great if I could do that. Then again, I
                        haven't
                        > gone back to the manual and might be violating RTFM Code 1. ;-)
                        >
                        > Thanks,
                        > Terry Wellman
                        >
                        > [Non-text portions of this message have been removed]
                        >
                        >
                        >
                        >
                        >
                        > [Non-text portions of this message have been removed]
                        >
                        >
                        >
                        > ------------------------------------
                        >
                        > www.machsupport.com - Web site AccessYahoo! Groups Links
                        >
                        >
                        >
                        >


                        ------------------------------------

                        www.machsupport.com - Web site AccessYahoo! Groups Links






                        [Non-text portions of this message have been removed]



                        ------------------------------------

                        www.machsupport.com - Web site AccessYahoo! Groups Links






                        [Non-text portions of this message have been removed]
                      • chuck
                        Dave, are the video files anywhere they can be downloaded instead of streaming from youtube? nice work by the way thank you, Chuck ... From: qconvers@aol.com
                        Message 11 of 30 , Apr 29 3:34 PM
                          Dave,
                          are the video files anywhere they can be downloaded instead of streaming from youtube?
                          nice work by the way thank you,
                          Chuck
                          ----- Original Message -----
                          From: qconvers@...
                          To: mach1mach2cnc@yahoogroups.com
                          Sent: Sunday, April 28, 2013 8:45 AM
                          Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts



                          I have uploaded the final cut of Ron's wizards video. I think it makes it
                          more engaging to watch.

                          http://www.youtube.com/watch?v=jFBAm151JRY

                          Regards Dave

                          In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                          ronginger@... writes:

                          > Ya, i second this also. The wizards are nice, but some things i think
                          need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                          NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                          spiral down in CW or CCW and not both. Both directions or back and forth can
                          cause undesired tool deflections.

                          Brian changed that yesterday- circles now ramp down in the same
                          direction, taking as far around the circle as needed to get get to
                          depth, then finishing that pass at a constant depth. Actually that was
                          how I had it at first, then Brian figured out his zig-zag cut and we
                          changed it.

                          Pockets do a spiral down to step depth in the center of the pocket, then
                          cut that step at a constant depth.

                          > IMHO ramping IS NOT at tool function, but rather part of a machining
                          strategy. In the new program if I want to use the same tool for a ramped entry
                          and the later in the same feature to plunge feed, I must create two tools,
                          and have to deal with the machine thinking there is a tool change when
                          none is needed.

                          I believe the ramp angle is a tool property- some tools will not plunge-
                          think an insert mill, or non-center cutting end mills. Yes, there are
                          tools that can do both, but there are plenty that cannot. Ramping always
                          gives a better cut than plunge.

                          > Then there is the problem of not having a finish pass without using a
                          separate operation. The pocket I was making was about 2" X 2" with .25"
                          rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                          single down step, and then a new pocket size to cut the last couple thou
                          away. The problem is that I cut air seemingly endlessly to get to actually cut.
                          Another way to finish is cutting the inside of a rectangle to make a final
                          cut. Well that works, but if you've been using a ramped entry for the
                          first operation, the tool wanders back and forth until it reaches full depth.

                          If you are doing a pocket you can apply the finish amount to both the
                          side and bottom of the pocket. Set the step depth to the same as the
                          finish depth on your second pocket and you will never cut air. You can
                          now have a Ztop value lower that 0, so you could do a finish cut with
                          Ztop at you finish depth minus total depth.

                          One of the problems of writing wizards is that every operation can have
                          multiple solutions. I have tried to give lots of options, but in the end
                          I can only program some of the options. I am sorry this cannot be the
                          solution to every case, but wizards are supposed to offer the simple,
                          common needs.

                          Thanks for the feedback, I try to look at it all and will continue to
                          make changes and additions when it seems like it will improve the wizards.

                          ron ginger

                          ------------------------------------

                          www.machsupport.com - Web site AccessYahoo! Groups Links

                          [Non-text portions of this message have been removed]





                          [Non-text portions of this message have been removed]
                        • Paul
                          ... I would definitely like and use a text format tool table. I have a lot of tools set up and would like to be able to more easily backup and edit the tool
                          Message 12 of 30 , Apr 29 3:45 PM
                            > If you're lucky enough to have several advanced Cam programs why
                            > would you want Brian waste his time making wizard tool libraries compatable?

                            I would definitely like and use a text format tool table. I have a lot of tools set up and would like to be able to more easily backup and edit the tool offsets outside of Mach. Right now they are stored in a binary .dat file and the only way to edit them or look at them is from within Mach and the editing tools that table are constraining.

                            Paul T.
                            www.springtest.com
                          • tmday7
                            Chuck, If you use Firefox, there is a nice addon that will add a download button below the YouTube video you are watching. This is the addon i use....
                            Message 13 of 30 , Apr 29 5:05 PM
                              Chuck,
                              If you use Firefox, there is a nice addon that will add a download button below the YouTube video you are watching.
                              This is the addon i use....
                              https://addons.mozilla.org/en-US/firefox/user/ialc/?src=api

                              HTH,
                              Troy

                              --- In mach1mach2cnc@yahoogroups.com, "chuck" <chuckels@...> wrote:
                              >
                              > Dave,
                              > are the video files anywhere they can be downloaded instead of streaming from youtube?
                              > nice work by the way thank you,
                              > Chuck
                              > ----- Original Message -----
                              > From: qconvers@...
                              > To: mach1mach2cnc@yahoogroups.com
                              > Sent: Sunday, April 28, 2013 8:45 AM
                              > Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                              >
                              >
                              >
                              > I have uploaded the final cut of Ron's wizards video. I think it makes it
                              > more engaging to watch.
                              >
                              > http://www.youtube.com/watch?v=jFBAm151JRY
                              >
                              > Regards Dave
                              >
                              > In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                              > ronginger@... writes:
                              >
                              > > Ya, i second this also. The wizards are nice, but some things i think
                              > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                              > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                              > spiral down in CW or CCW and not both. Both directions or back and forth can
                              > cause undesired tool deflections.
                              >
                              > Brian changed that yesterday- circles now ramp down in the same
                              > direction, taking as far around the circle as needed to get get to
                              > depth, then finishing that pass at a constant depth. Actually that was
                              > how I had it at first, then Brian figured out his zig-zag cut and we
                              > changed it.
                              >
                              > Pockets do a spiral down to step depth in the center of the pocket, then
                              > cut that step at a constant depth.
                              >
                              > > IMHO ramping IS NOT at tool function, but rather part of a machining
                              > strategy. In the new program if I want to use the same tool for a ramped entry
                              > and the later in the same feature to plunge feed, I must create two tools,
                              > and have to deal with the machine thinking there is a tool change when
                              > none is needed.
                              >
                              > I believe the ramp angle is a tool property- some tools will not plunge-
                              > think an insert mill, or non-center cutting end mills. Yes, there are
                              > tools that can do both, but there are plenty that cannot. Ramping always
                              > gives a better cut than plunge.
                              >
                              > > Then there is the problem of not having a finish pass without using a
                              > separate operation. The pocket I was making was about 2" X 2" with .25"
                              > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                              > single down step, and then a new pocket size to cut the last couple thou
                              > away. The problem is that I cut air seemingly endlessly to get to actually cut.
                              > Another way to finish is cutting the inside of a rectangle to make a final
                              > cut. Well that works, but if you've been using a ramped entry for the
                              > first operation, the tool wanders back and forth until it reaches full depth.
                              >
                              > If you are doing a pocket you can apply the finish amount to both the
                              > side and bottom of the pocket. Set the step depth to the same as the
                              > finish depth on your second pocket and you will never cut air. You can
                              > now have a Ztop value lower that 0, so you could do a finish cut with
                              > Ztop at you finish depth minus total depth.
                              >
                              > One of the problems of writing wizards is that every operation can have
                              > multiple solutions. I have tried to give lots of options, but in the end
                              > I can only program some of the options. I am sorry this cannot be the
                              > solution to every case, but wizards are supposed to offer the simple,
                              > common needs.
                              >
                              > Thanks for the feedback, I try to look at it all and will continue to
                              > make changes and additions when it seems like it will improve the wizards.
                              >
                              > ron ginger
                              >
                              > ------------------------------------
                              >
                              > www.machsupport.com - Web site AccessYahoo! Groups Links
                              >
                              > [Non-text portions of this message have been removed]
                              >
                              >
                              >
                              >
                              >
                              > [Non-text portions of this message have been removed]
                              >
                            • chuck
                              thanx Troy, I will try it Chuck ... From: tmday7 To: mach1mach2cnc@yahoogroups.com Sent: Monday, April 29, 2013 8:05 PM Subject: [mach1mach2cnc] Re: Newfangled
                              Message 14 of 30 , Apr 29 5:18 PM
                                thanx Troy,
                                I will try it
                                Chuck

                                ----- Original Message -----
                                From: tmday7
                                To: mach1mach2cnc@yahoogroups.com
                                Sent: Monday, April 29, 2013 8:05 PM
                                Subject: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts



                                Chuck,
                                If you use Firefox, there is a nice addon that will add a download button below the YouTube video you are watching.
                                This is the addon i use....
                                https://addons.mozilla.org/en-US/firefox/user/ialc/?src=api

                                HTH,
                                Troy

                                --- In mach1mach2cnc@yahoogroups.com, "chuck" <chuckels@...> wrote:
                                >
                                > Dave,
                                > are the video files anywhere they can be downloaded instead of streaming from youtube?
                                > nice work by the way thank you,
                                > Chuck
                                > ----- Original Message -----
                                > From: qconvers@...
                                > To: mach1mach2cnc@yahoogroups.com
                                > Sent: Sunday, April 28, 2013 8:45 AM
                                > Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                >
                                >
                                >
                                > I have uploaded the final cut of Ron's wizards video. I think it makes it
                                > more engaging to watch.
                                >
                                > http://www.youtube.com/watch?v=jFBAm151JRY
                                >
                                > Regards Dave
                                >
                                > In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                                > ronginger@... writes:
                                >
                                > > Ya, i second this also. The wizards are nice, but some things i think
                                > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                                > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                                > spiral down in CW or CCW and not both. Both directions or back and forth can
                                > cause undesired tool deflections.
                                >
                                > Brian changed that yesterday- circles now ramp down in the same
                                > direction, taking as far around the circle as needed to get get to
                                > depth, then finishing that pass at a constant depth. Actually that was
                                > how I had it at first, then Brian figured out his zig-zag cut and we
                                > changed it.
                                >
                                > Pockets do a spiral down to step depth in the center of the pocket, then
                                > cut that step at a constant depth.
                                >
                                > > IMHO ramping IS NOT at tool function, but rather part of a machining
                                > strategy. In the new program if I want to use the same tool for a ramped entry
                                > and the later in the same feature to plunge feed, I must create two tools,
                                > and have to deal with the machine thinking there is a tool change when
                                > none is needed.
                                >
                                > I believe the ramp angle is a tool property- some tools will not plunge-
                                > think an insert mill, or non-center cutting end mills. Yes, there are
                                > tools that can do both, but there are plenty that cannot. Ramping always
                                > gives a better cut than plunge.
                                >
                                > > Then there is the problem of not having a finish pass without using a
                                > separate operation. The pocket I was making was about 2" X 2" with .25"
                                > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                                > single down step, and then a new pocket size to cut the last couple thou
                                > away. The problem is that I cut air seemingly endlessly to get to actually cut.
                                > Another way to finish is cutting the inside of a rectangle to make a final
                                > cut. Well that works, but if you've been using a ramped entry for the
                                > first operation, the tool wanders back and forth until it reaches full depth.
                                >
                                > If you are doing a pocket you can apply the finish amount to both the
                                > side and bottom of the pocket. Set the step depth to the same as the
                                > finish depth on your second pocket and you will never cut air. You can
                                > now have a Ztop value lower that 0, so you could do a finish cut with
                                > Ztop at you finish depth minus total depth.
                                >
                                > One of the problems of writing wizards is that every operation can have
                                > multiple solutions. I have tried to give lots of options, but in the end
                                > I can only program some of the options. I am sorry this cannot be the
                                > solution to every case, but wizards are supposed to offer the simple,
                                > common needs.
                                >
                                > Thanks for the feedback, I try to look at it all and will continue to
                                > make changes and additions when it seems like it will improve the wizards.
                                >
                                > ron ginger
                                >
                                > ------------------------------------
                                >
                                > www.machsupport.com - Web site AccessYahoo! Groups Links
                                >
                                > [Non-text portions of this message have been removed]
                                >
                                >
                                >
                                >
                                >
                                > [Non-text portions of this message have been removed]
                                >





                                [Non-text portions of this message have been removed]
                              • Dave
                                Hello chuck. What file format would you like them in? Windows. Android. . I ll sort that tomorrow for you. Regards Dave.
                                Message 15 of 30 , Apr 29 5:42 PM
                                  Hello chuck. What file format would you like them in? Windows. Android. . I'll sort that tomorrow for you. Regards Dave.

                                  chuck <chuckels@...> wrote:

                                  >Dave,
                                  >are the video files anywhere they can be downloaded instead of streaming from youtube?
                                  >nice work by the way thank you,
                                  >Chuck
                                  > ----- Original Message -----
                                  > From: qconvers@...
                                  > To: mach1mach2cnc@yahoogroups.com
                                  > Sent: Sunday, April 28, 2013 8:45 AM
                                  > Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                  >
                                  >
                                  >
                                  > I have uploaded the final cut of Ron's wizards video. I think it makes it
                                  > more engaging to watch.
                                  >
                                  > http://www.youtube.com/watch?v=jFBAm151JRY
                                  >
                                  > Regards Dave
                                  >
                                  > In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                                  > ronginger@... writes:
                                  >
                                  > > Ya, i second this also. The wizards are nice, but some things i think
                                  > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                                  > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                                  > spiral down in CW or CCW and not both. Both directions or back and forth can
                                  > cause undesired tool deflections.
                                  >
                                  > Brian changed that yesterday- circles now ramp down in the same
                                  > direction, taking as far around the circle as needed to get get to
                                  > depth, then finishing that pass at a constant depth. Actually that was
                                  > how I had it at first, then Brian figured out his zig-zag cut and we
                                  > changed it.
                                  >
                                  > Pockets do a spiral down to step depth in the center of the pocket, then
                                  > cut that step at a constant depth.
                                  >
                                  > > IMHO ramping IS NOT at tool function, but rather part of a machining
                                  > strategy. In the new program if I want to use the same tool for a ramped entry
                                  > and the later in the same feature to plunge feed, I must create two tools,
                                  > and have to deal with the machine thinking there is a tool change when
                                  > none is needed.
                                  >
                                  > I believe the ramp angle is a tool property- some tools will not plunge-
                                  > think an insert mill, or non-center cutting end mills. Yes, there are
                                  > tools that can do both, but there are plenty that cannot. Ramping always
                                  > gives a better cut than plunge.
                                  >
                                  > > Then there is the problem of not having a finish pass without using a
                                  > separate operation. The pocket I was making was about 2" X 2" with .25"
                                  > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                                  > single down step, and then a new pocket size to cut the last couple thou
                                  > away. The problem is that I cut air seemingly endlessly to get to actually cut.
                                  > Another way to finish is cutting the inside of a rectangle to make a final
                                  > cut. Well that works, but if you've been using a ramped entry for the
                                  > first operation, the tool wanders back and forth until it reaches full depth.
                                  >
                                  > If you are doing a pocket you can apply the finish amount to both the
                                  > side and bottom of the pocket. Set the step depth to the same as the
                                  > finish depth on your second pocket and you will never cut air. You can
                                  > now have a Ztop value lower that 0, so you could do a finish cut with
                                  > Ztop at you finish depth minus total depth.
                                  >
                                  > One of the problems of writing wizards is that every operation can have
                                  > multiple solutions. I have tried to give lots of options, but in the end
                                  > I can only program some of the options. I am sorry this cannot be the
                                  > solution to every case, but wizards are supposed to offer the simple,
                                  > common needs.
                                  >
                                  > Thanks for the feedback, I try to look at it all and will continue to
                                  > make changes and additions when it seems like it will improve the wizards.
                                  >
                                  > ron ginger
                                  >
                                  > ------------------------------------
                                  >
                                  > www.machsupport.com - Web site AccessYahoo! Groups Links
                                  >
                                  > [Non-text portions of this message have been removed]
                                  >
                                  >
                                  >
                                  >
                                  >
                                  >[Non-text portions of this message have been removed]
                                  >
                                  >
                                  >
                                  >------------------------------------
                                  >
                                  >www.machsupport.com - Web site AccessYahoo! Groups Links
                                  >
                                  >
                                  >
                                • chuck
                                  Dave, thank you. I guess windows or even mp4 would be great. thanx for your hard work getting these done. Chuck ... From: Dave To:
                                  Message 16 of 30 , Apr 29 5:45 PM
                                    Dave,
                                    thank you.
                                    I guess windows or even mp4 would be great.
                                    thanx for your hard work getting these done.
                                    Chuck

                                    ----- Original Message -----
                                    From: Dave
                                    To: mach1mach2cnc@yahoogroups.com
                                    Sent: Monday, April 29, 2013 8:42 PM
                                    Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts



                                    Hello chuck. What file format would you like them in? Windows. Android. . I'll sort that tomorrow for you. Regards Dave.

                                    chuck <chuckels@...> wrote:

                                    >Dave,
                                    >are the video files anywhere they can be downloaded instead of streaming from youtube?
                                    >nice work by the way thank you,
                                    >Chuck
                                    > ----- Original Message -----
                                    > From: qconvers@...
                                    > To: mach1mach2cnc@yahoogroups.com
                                    > Sent: Sunday, April 28, 2013 8:45 AM
                                    > Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                    >
                                    >
                                    >
                                    > I have uploaded the final cut of Ron's wizards video. I think it makes it
                                    > more engaging to watch.
                                    >
                                    > http://www.youtube.com/watch?v=jFBAm151JRY
                                    >
                                    > Regards Dave
                                    >
                                    > In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                                    > ronginger@... writes:
                                    >
                                    > > Ya, i second this also. The wizards are nice, but some things i think
                                    > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                                    > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                                    > spiral down in CW or CCW and not both. Both directions or back and forth can
                                    > cause undesired tool deflections.
                                    >
                                    > Brian changed that yesterday- circles now ramp down in the same
                                    > direction, taking as far around the circle as needed to get get to
                                    > depth, then finishing that pass at a constant depth. Actually that was
                                    > how I had it at first, then Brian figured out his zig-zag cut and we
                                    > changed it.
                                    >
                                    > Pockets do a spiral down to step depth in the center of the pocket, then
                                    > cut that step at a constant depth.
                                    >
                                    > > IMHO ramping IS NOT at tool function, but rather part of a machining
                                    > strategy. In the new program if I want to use the same tool for a ramped entry
                                    > and the later in the same feature to plunge feed, I must create two tools,
                                    > and have to deal with the machine thinking there is a tool change when
                                    > none is needed.
                                    >
                                    > I believe the ramp angle is a tool property- some tools will not plunge-
                                    > think an insert mill, or non-center cutting end mills. Yes, there are
                                    > tools that can do both, but there are plenty that cannot. Ramping always
                                    > gives a better cut than plunge.
                                    >
                                    > > Then there is the problem of not having a finish pass without using a
                                    > separate operation. The pocket I was making was about 2" X 2" with .25"
                                    > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                                    > single down step, and then a new pocket size to cut the last couple thou
                                    > away. The problem is that I cut air seemingly endlessly to get to actually cut.
                                    > Another way to finish is cutting the inside of a rectangle to make a final
                                    > cut. Well that works, but if you've been using a ramped entry for the
                                    > first operation, the tool wanders back and forth until it reaches full depth.
                                    >
                                    > If you are doing a pocket you can apply the finish amount to both the
                                    > side and bottom of the pocket. Set the step depth to the same as the
                                    > finish depth on your second pocket and you will never cut air. You can
                                    > now have a Ztop value lower that 0, so you could do a finish cut with
                                    > Ztop at you finish depth minus total depth.
                                    >
                                    > One of the problems of writing wizards is that every operation can have
                                    > multiple solutions. I have tried to give lots of options, but in the end
                                    > I can only program some of the options. I am sorry this cannot be the
                                    > solution to every case, but wizards are supposed to offer the simple,
                                    > common needs.
                                    >
                                    > Thanks for the feedback, I try to look at it all and will continue to
                                    > make changes and additions when it seems like it will improve the wizards.
                                    >
                                    > ron ginger
                                    >
                                    > ------------------------------------
                                    >
                                    > www.machsupport.com - Web site AccessYahoo! Groups Links
                                    >
                                    > [Non-text portions of this message have been removed]
                                    >
                                    >
                                    >
                                    >
                                    >
                                    >[Non-text portions of this message have been removed]
                                    >
                                    >
                                    >
                                    >------------------------------------
                                    >
                                    >www.machsupport.com - Web site AccessYahoo! Groups Links
                                    >
                                    >
                                    >




                                    [Non-text portions of this message have been removed]
                                  • Dave
                                    Hello chuck. The file format from youtube might only play on the latest media player or vlc player. I ll sort a download for you tomorrow. Dave
                                    Message 17 of 30 , Apr 29 5:46 PM
                                      Hello chuck. The file format from youtube might only play on the latest media player or vlc player. I'll sort a download for you tomorrow. Dave

                                      chuck <chuckels@...> wrote:

                                      >thanx Troy,
                                      >I will try it
                                      >Chuck
                                      >
                                      > ----- Original Message -----
                                      > From: tmday7
                                      > To: mach1mach2cnc@yahoogroups.com
                                      > Sent: Monday, April 29, 2013 8:05 PM
                                      > Subject: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                      >
                                      >
                                      >
                                      > Chuck,
                                      > If you use Firefox, there is a nice addon that will add a download button below the YouTube video you are watching.
                                      > This is the addon i use....
                                      > https://addons.mozilla.org/en-US/firefox/user/ialc/?src=api
                                      >
                                      > HTH,
                                      > Troy
                                      >
                                      > --- In mach1mach2cnc@yahoogroups.com, "chuck" <chuckels@...> wrote:
                                      > >
                                      > > Dave,
                                      > > are the video files anywhere they can be downloaded instead of streaming from youtube?
                                      > > nice work by the way thank you,
                                      > > Chuck
                                      > > ----- Original Message -----
                                      > > From: qconvers@...
                                      > > To: mach1mach2cnc@yahoogroups.com
                                      > > Sent: Sunday, April 28, 2013 8:45 AM
                                      > > Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                      > >
                                      > >
                                      > >
                                      > > I have uploaded the final cut of Ron's wizards video. I think it makes it
                                      > > more engaging to watch.
                                      > >
                                      > > http://www.youtube.com/watch?v=jFBAm151JRY
                                      > >
                                      > > Regards Dave
                                      > >
                                      > > In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                                      > > ronginger@... writes:
                                      > >
                                      > > > Ya, i second this also. The wizards are nice, but some things i think
                                      > > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                                      > > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                                      > > spiral down in CW or CCW and not both. Both directions or back and forth can
                                      > > cause undesired tool deflections.
                                      > >
                                      > > Brian changed that yesterday- circles now ramp down in the same
                                      > > direction, taking as far around the circle as needed to get get to
                                      > > depth, then finishing that pass at a constant depth. Actually that was
                                      > > how I had it at first, then Brian figured out his zig-zag cut and we
                                      > > changed it.
                                      > >
                                      > > Pockets do a spiral down to step depth in the center of the pocket, then
                                      > > cut that step at a constant depth.
                                      > >
                                      > > > IMHO ramping IS NOT at tool function, but rather part of a machining
                                      > > strategy. In the new program if I want to use the same tool for a ramped entry
                                      > > and the later in the same feature to plunge feed, I must create two tools,
                                      > > and have to deal with the machine thinking there is a tool change when
                                      > > none is needed.
                                      > >
                                      > > I believe the ramp angle is a tool property- some tools will not plunge-
                                      > > think an insert mill, or non-center cutting end mills. Yes, there are
                                      > > tools that can do both, but there are plenty that cannot. Ramping always
                                      > > gives a better cut than plunge.
                                      > >
                                      > > > Then there is the problem of not having a finish pass without using a
                                      > > separate operation. The pocket I was making was about 2" X 2" with .25"
                                      > > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                                      > > single down step, and then a new pocket size to cut the last couple thou
                                      > > away. The problem is that I cut air seemingly endlessly to get to actually cut.
                                      > > Another way to finish is cutting the inside of a rectangle to make a final
                                      > > cut. Well that works, but if you've been using a ramped entry for the
                                      > > first operation, the tool wanders back and forth until it reaches full depth.
                                      > >
                                      > > If you are doing a pocket you can apply the finish amount to both the
                                      > > side and bottom of the pocket. Set the step depth to the same as the
                                      > > finish depth on your second pocket and you will never cut air. You can
                                      > > now have a Ztop value lower that 0, so you could do a finish cut with
                                      > > Ztop at you finish depth minus total depth.
                                      > >
                                      > > One of the problems of writing wizards is that every operation can have
                                      > > multiple solutions. I have tried to give lots of options, but in the end
                                      > > I can only program some of the options. I am sorry this cannot be the
                                      > > solution to every case, but wizards are supposed to offer the simple,
                                      > > common needs.
                                      > >
                                      > > Thanks for the feedback, I try to look at it all and will continue to
                                      > > make changes and additions when it seems like it will improve the wizards.
                                      > >
                                      > > ron ginger
                                      > >
                                      > > ------------------------------------
                                      > >
                                      > > www.machsupport.com - Web site AccessYahoo! Groups Links
                                      > >
                                      > > [Non-text portions of this message have been removed]
                                      > >
                                      > >
                                      > >
                                      > >
                                      > >
                                      > > [Non-text portions of this message have been removed]
                                      > >
                                      >
                                      >
                                      >
                                      >
                                      >
                                      >[Non-text portions of this message have been removed]
                                      >
                                      >
                                      >
                                      >------------------------------------
                                      >
                                      >www.machsupport.com - Web site AccessYahoo! Groups Links
                                      >
                                      >
                                      >
                                    • chuck
                                      cool.. thanx ... From: Dave To: mach1mach2cnc@yahoogroups.com Sent: Monday, April 29, 2013 8:46 PM Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand
                                      Message 18 of 30 , Apr 29 5:50 PM
                                        cool.. thanx

                                        ----- Original Message -----
                                        From: Dave
                                        To: mach1mach2cnc@yahoogroups.com
                                        Sent: Monday, April 29, 2013 8:46 PM
                                        Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts



                                        Hello chuck. The file format from youtube might only play on the latest media player or vlc player. I'll sort a download for you tomorrow. Dave

                                        chuck <chuckels@...> wrote:

                                        >thanx Troy,
                                        >I will try it
                                        >Chuck
                                        >
                                        > ----- Original Message -----
                                        > From: tmday7
                                        > To: mach1mach2cnc@yahoogroups.com
                                        > Sent: Monday, April 29, 2013 8:05 PM
                                        > Subject: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                        >
                                        >
                                        >
                                        > Chuck,
                                        > If you use Firefox, there is a nice addon that will add a download button below the YouTube video you are watching.
                                        > This is the addon i use....
                                        > https://addons.mozilla.org/en-US/firefox/user/ialc/?src=api
                                        >
                                        > HTH,
                                        > Troy
                                        >
                                        > --- In mach1mach2cnc@yahoogroups.com, "chuck" <chuckels@...> wrote:
                                        > >
                                        > > Dave,
                                        > > are the video files anywhere they can be downloaded instead of streaming from youtube?
                                        > > nice work by the way thank you,
                                        > > Chuck
                                        > > ----- Original Message -----
                                        > > From: qconvers@...
                                        > > To: mach1mach2cnc@yahoogroups.com
                                        > > Sent: Sunday, April 28, 2013 8:45 AM
                                        > > Subject: Re: [mach1mach2cnc] Re: Newfangled Wizard Stand Alone, some thoughts
                                        > >
                                        > >
                                        > >
                                        > > I have uploaded the final cut of Ron's wizards video. I think it makes it
                                        > > more engaging to watch.
                                        > >
                                        > > http://www.youtube.com/watch?v=jFBAm151JRY
                                        > >
                                        > > Regards Dave
                                        > >
                                        > > In a message dated 28/04/2013 13:08:12 GMT Daylight Time,
                                        > > ronginger@... writes:
                                        > >
                                        > > > Ya, i second this also. The wizards are nice, but some things i think
                                        > > need tweeking. Maybe this is why its in Beta.Another thing i liked with the
                                        > > NFW for Mach3 concerning ramping, is when doing a circle, the tool would
                                        > > spiral down in CW or CCW and not both. Both directions or back and forth can
                                        > > cause undesired tool deflections.
                                        > >
                                        > > Brian changed that yesterday- circles now ramp down in the same
                                        > > direction, taking as far around the circle as needed to get get to
                                        > > depth, then finishing that pass at a constant depth. Actually that was
                                        > > how I had it at first, then Brian figured out his zig-zag cut and we
                                        > > changed it.
                                        > >
                                        > > Pockets do a spiral down to step depth in the center of the pocket, then
                                        > > cut that step at a constant depth.
                                        > >
                                        > > > IMHO ramping IS NOT at tool function, but rather part of a machining
                                        > > strategy. In the new program if I want to use the same tool for a ramped entry
                                        > > and the later in the same feature to plunge feed, I must create two tools,
                                        > > and have to deal with the machine thinking there is a tool change when
                                        > > none is needed.
                                        > >
                                        > > I believe the ramp angle is a tool property- some tools will not plunge-
                                        > > think an insert mill, or non-center cutting end mills. Yes, there are
                                        > > tools that can do both, but there are plenty that cannot. Ramping always
                                        > > gives a better cut than plunge.
                                        > >
                                        > > > Then there is the problem of not having a finish pass without using a
                                        > > separate operation. The pocket I was making was about 2" X 2" with .25"
                                        > > rounded corners using a 3/8" mill. And it's deep, 1 5/8". Ron suggests that a
                                        > > single down step, and then a new pocket size to cut the last couple thou
                                        > > away. The problem is that I cut air seemingly endlessly to get to actually cut.
                                        > > Another way to finish is cutting the inside of a rectangle to make a final
                                        > > cut. Well that works, but if you've been using a ramped entry for the
                                        > > first operation, the tool wanders back and forth until it reaches full depth.
                                        > >
                                        > > If you are doing a pocket you can apply the finish amount to both the
                                        > > side and bottom of the pocket. Set the step depth to the same as the
                                        > > finish depth on your second pocket and you will never cut air. You can
                                        > > now have a Ztop value lower that 0, so you could do a finish cut with
                                        > > Ztop at you finish depth minus total depth.
                                        > >
                                        > > One of the problems of writing wizards is that every operation can have
                                        > > multiple solutions. I have tried to give lots of options, but in the end
                                        > > I can only program some of the options. I am sorry this cannot be the
                                        > > solution to every case, but wizards are supposed to offer the simple,
                                        > > common needs.
                                        > >
                                        > > Thanks for the feedback, I try to look at it all and will continue to
                                        > > make changes and additions when it seems like it will improve the wizards.
                                        > >
                                        > > ron ginger
                                        > >
                                        > > ------------------------------------
                                        > >
                                        > > www.machsupport.com - Web site AccessYahoo! Groups Links
                                        > >
                                        > > [Non-text portions of this message have been removed]
                                        > >
                                        > >
                                        > >
                                        > >
                                        > >
                                        > > [Non-text portions of this message have been removed]
                                        > >
                                        >
                                        >
                                        >
                                        >
                                        >
                                        >[Non-text portions of this message have been removed]
                                        >
                                        >
                                        >
                                        >------------------------------------
                                        >
                                        >www.machsupport.com - Web site AccessYahoo! Groups Links
                                        >
                                        >
                                        >




                                        [Non-text portions of this message have been removed]
                                      • Terry Wellman
                                        That s an easy one. Not everyone in our shop uses Rhino and RhinoCam. Believe it or not, we still have some folks who are really good with their hands but not
                                        Message 19 of 30 , Apr 29 9:43 PM
                                          That's an easy one. Not everyone in our shop uses Rhino and RhinoCam. Believe it or not, we still have some folks who are really good with their hands but not the greatest CNC machinists. With several mills here, if they were able to work with wizards while getting their chops up to speed on software, they could still make stuff. Sometimes it is actually faster to use wizards to prep stock while we're still working out the nuances on a 3D model in Rhino.

                                          Is there a problem using multiple tools to accomplish something?

                                          Terry

                                          On Apr 29, 2013, at 4:51 PM, qconvers@... wrote:

                                          > blessed laptops... As a user of Rhino and Rhinocam ... why would you want
                                          > to use wizards? If you're a Rhino user it would be a quick job to draw any
                                          > of the simple operations in the wizards and run them though Rhinocam. The
                                          > wizards are for the people who don't want to invest in the software like
                                          > Rhino. Ron said he wasn't trying to re-create Solid Works. I agree it would
                                          > be good if the tool libary was an industrial standard. But, Rhino to Mach
                                          > wizards? If you're lucky enough to have several advanced Cam programs why
                                          > would you want Brian waste his time making wizard tool libraries compatable?
                                          >
                                          >
                                          > In a message dated 29/04/2013 22:25:14 GMT Daylight Time,
                                          > _qcoanvers@..._ (mailto:qcoanvers@...) writes:
                                          >
                                          > A
                                          >
                                          > In a message dated 29/04/2013 21:07:48 GMT Daylight Time,
                                          > brianb@... writes:
                                          >
                                          > No standards at this time.. I think what we write should become the
                                          > standard ;)
                                          >
                                          > We are going to make it so you can save and load a tooltable.. So you
                                          > should be able to make a converter program...
                                          >
                                          > On 4/29/2013 4:04 PM, Freeman P. Pascal IV wrote:
                                          > > Personally, I would love to see Mach 4 support a tool library format
                                          > that
                                          > > was standard between many CAD/CAM packages. I hate having to maintain
                                          > my
                                          > > tool library across multiple packages. Ideally, it would be nice if I
                                          > could
                                          > > point all my software to a common data source.
                                          > >
                                          > >
                                          > >
                                          > > A quick google did not reveal any standard tool library formats, but I
                                          > > wouldn't be surprised if there was something that was industry
                                          > supported.
                                          > > If there isn't, perhaps an XML scheme could be devised to provide such
                                          > > support, at least between Mach 4 (possibly Mach 3) and NFW external
                                          > wizards.
                                          > > You would be surprised how simply publishing an exchange format would
                                          > > promote its use.
                                          > >
                                          > >
                                          > >
                                          > >
                                          > >
                                          > > -Freeman
                                          > >
                                          > >
                                          > >
                                          > > _____
                                          > >
                                          > > From: mach1mach2cnc@yahoogroups.com
                                          > [mailto:mach1mach2cnc@yahoogroups.com]
                                          > > On Behalf Of Henrik Olsson
                                          > > Sent: Monday, April 29, 2013 11:33 AM
                                          > > To: mach1mach2cnc@yahoogroups.com
                                          > > Subject: Re: [mach1mach2cnc] Can I import a tool library into Mach3 or
                                          > soon
                                          > > 4?
                                          > >
                                          > >
                                          > >
                                          > >
                                          > >
                                          > > Hi Terry,
                                          > >
                                          > > The short answer is no, not really (at least not in Mach3, I don't know
                                          > > about Mach4).
                                          > >
                                          > > The long answer is that Mach3 doesn't have any functionality built in
                                          > to
                                          > do
                                          > > this but it does have scripting capability so it might be possible to
                                          > write
                                          > > a simple importer that reads the tool library file and stuffs the info
                                          > into
                                          > > Mach3's tooltable. Obviously the possible success of such an effort
                                          > depends
                                          > > on if the format of the tool library, as exported from Rhino, is
                                          > published
                                          > > and/or if it's simple text files so one can figure it out by just
                                          > looking at
                                          > > the file.
                                          > >
                                          > > Over the years the issue of exporting the tooltable FROM Mach3 have been
                                          > > covered numerous times on this list but I can't remember importing
                                          > tools
                                          > > being discussed. Do you have any info on the actual format of the tool
                                          > > library file you want to import?
                                          > >
                                          > > /Henrik.
                                          > >
                                          > > _____
                                          > >
                                          > > ---Original message---
                                          > >
                                          > > We use Rhino Cam 2012 Pro for our cam programming. Rhino Cam is Visual
                                          > Mill
                                          > > ported into Rhino as a plug-in. It has a good tool library function. Is
                                          > > there a way to import the tool library from Rhino Cam into Mach so that
                                          > I
                                          > > don't have to recreate the whole thing? We have a bunch of tooling
                                          > listed
                                          > > there already. It would be great if I could do that. Then again, I
                                          > haven't
                                          > > gone back to the manual and might be violating RTFM Code 1. ;-)
                                          > >
                                          > > Thanks,
                                          > > Terry Wellman
                                          > >
                                          > > [Non-text portions of this message have been removed]
                                          > >
                                          > >
                                          > >
                                          > >
                                          > >
                                          > > [Non-text portions of this message have been removed]
                                          > >
                                          > >
                                          > >
                                          > > ------------------------------------
                                          > >
                                          > > www.machsupport.com - Web site AccessYahoo! Groups Links
                                          > >
                                          > >
                                          > >
                                          > >
                                          >
                                          > ------------------------------------
                                          >
                                          > www.machsupport.com - Web site AccessYahoo! Groups Links
                                          >
                                          > [Non-text portions of this message have been removed]
                                          >
                                          > ------------------------------------
                                          >
                                          > www.machsupport.com - Web site AccessYahoo! Groups Links
                                          >
                                          > [Non-text portions of this message have been removed]
                                          >
                                          >



                                          [Non-text portions of this message have been removed]
                                        • Brian Barker
                                          Hello Paul, The new tool table files will be simple text files.. You can check out the tool table file in the wizard and see how I did it if you would like.
                                          Message 20 of 30 , Apr 30 5:07 AM
                                            Hello Paul,
                                            The new tool table files will be simple text files.. You can check out
                                            the tool table file in the wizard and see how I did it if you would like.

                                            Thanks
                                            Brian


                                            On 4/29/2013 6:45 PM, Paul wrote:
                                            >> If you're lucky enough to have several advanced Cam programs why
                                            >> would you want Brian waste his time making wizard tool libraries compatable?
                                            > I would definitely like and use a text format tool table. I have a lot of tools set up and would like to be able to more easily backup and edit the tool offsets outside of Mach. Right now they are stored in a binary .dat file and the only way to edit them or look at them is from within Mach and the editing tools that table are constraining.
                                            >
                                            > Paul T.
                                            > www.springtest.com
                                            >
                                            >
                                            >
                                          • Rjreese29
                                            On the tool table import/ export for mach3, I was very surprised to get it when I purchased mach standard mill professional for the probing features. The
                                            Message 21 of 30 , Apr 30 7:09 AM
                                              On the tool table import/ export for mach3, I was very surprised to get it when I purchased mach standard mill professional for the probing features. The tooltable import export features were a surprise bonus for me.Though it doesn't necessarily work between cam and mach (no valueadd for me) I still like the feature and can see how useful it would be very useful for multiple mach3 seats.

                                              Rob

                                              On Apr 29, 2013, at 3:45 PM, "Paul" <pt@...> wrote:

                                              > > If you're lucky enough to have several advanced Cam programs why
                                              > > would you want Brian waste his time making wizard tool libraries compatable?
                                              >
                                              > I would definitely like and use a text format tool table. I have a lot of tools set up and would like to be able to more easily backup and edit the tool offsets outside of Mach. Right now they are stored in a binary .dat file and the only way to edit them or look at them is from within Mach and the editing tools that table are constraining.
                                              >
                                              > Paul T.
                                              > www.springtest.com
                                              >
                                              >


                                              [Non-text portions of this message have been removed]
                                            • Terry Wellman
                                              Exactly! I didn t put that in my original post but that s another issue that we face having several mach mills here. Terry ... [Non-text portions of this
                                              Message 22 of 30 , Apr 30 7:16 AM
                                                Exactly! I didn't put that in my original post but that's another issue that we face having several mach mills here.

                                                Terry

                                                On Apr 30, 2013, at 9:09 AM, Rjreese29 <rjreese29@...> wrote:

                                                > On the tool table import/ export for mach3, I was very surprised to get it when I purchased mach standard mill professional for the probing features. The tooltable import export features were a surprise bonus for me.Though it doesn't necessarily work between cam and mach (no valueadd for me) I still like the feature and can see how useful it would be very useful for multiple mach3 seats.
                                                >
                                                > Rob
                                                >
                                                > On Apr 29, 2013, at 3:45 PM, "Paul" <pt@...> wrote:
                                                >
                                                > > > If you're lucky enough to have several advanced Cam programs why
                                                > > > would you want Brian waste his time making wizard tool libraries compatable?
                                                > >
                                                > > I would definitely like and use a text format tool table. I have a lot of tools set up and would like to be able to more easily backup and edit the tool offsets outside of Mach. Right now they are stored in a binary .dat file and the only way to edit them or look at them is from within Mach and the editing tools that table are constraining.
                                                > >
                                                > > Paul T.
                                                > > www.springtest.com
                                                > >
                                                > >
                                                >
                                                > [Non-text portions of this message have been removed]
                                                >
                                                >



                                                [Non-text portions of this message have been removed]
                                              • Paul
                                                ... Brian that s great to hear, thanks again for your efforts to implement all these improvements. Paul T.
                                                Message 23 of 30 , Apr 30 9:19 AM
                                                  > The new tool table files will be simple text files.. You can check out
                                                  > the tool table file in the wizard and see how I did it if you would like.
                                                  >
                                                  > Thanks
                                                  > Brian

                                                  Brian that's great to hear, thanks again for your efforts to implement all these improvements.

                                                  Paul T.
                                                Your message has been successfully submitted and would be delivered to recipients shortly.