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

RE: [SherlineCNC] Re: True 3D milling using rotary table

Expand Messages
  • Andy Wander
    Kevin:You may be correct, but I am pretty sure that SheetCAM, for instance, is described as a 2-1/2D CAM program, and it can do 3-axis interpolation with no
    Message 1 of 17 , Feb 6, 2009
    • 0 Attachment
      Kevin:

      You may be correct, but I am pretty sure that SheetCAM, for instance, is described as a 2-1/2D CAM program, and it can do 3-axis interpolation with no problem.

      ______________________________________
      Andy Wander

      -----Original Message-----
      From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com] On Behalf Of Kevin Martin
      Sent: Friday, February 06, 2009 11:09 PM
      To: SherlineCNC@yahoogroups.com
      Subject: RE: [SherlineCNC] Re: True 3D milling using rotary table

      Hmmm. Not how I recall it.
      The stuff you describe, undercuts and side pockets, are 4D+ as they involve rotating the part or the spindle axis as well as needing three linear motions.

      If you can see it all from above it is 3D.

      If you can see it all from above and each "top" surface you see is at a constant Z, *that* is 2-1/2D; essentially the machine can move in the third dimension (Z) but cannot do so smoothly (or proportionately to X and Y motion) so any sort of ramps or contours are impossible and all cutting motion must occur at constant Z.
      -Kevin Martin

      -----Original Message-----
      From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com] On Behalf Of Andy Wander

      2-1/2D is anything you can do with a standard vertical mill, using only the X-Y table, and the Z(spindle) moving up and down.

      No pockets on the underside, holes in the sides of the part, or anything else that would require a rotation of the part or one of the axes.

      Another way to look at it, if you can see all of the features of the part that need machining, by looking at it from above, then you can do it with 2-1/2D.


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

      Yahoo! Groups Links



      This communication including any attachments, are intended
      for the exclusive use of the addressee(s) and contains
      confidential or copyrighted materials. Duplication,
      distribution or reproduction is strictly prohibited by law
      without written permission of Verrex
    • Neil Albert
      I have come to understand (or look at) 2-1/2D milling as even more restrictive than that, specifically being able cut pockets in the z direction of an object,
      Message 2 of 17 , Feb 6, 2009
      • 0 Attachment
        I have come to understand (or look at) 2-1/2D milling as even more
        restrictive than that, specifically being able cut pockets in the z
        direction of an object, or cut a curved path in the material at some
        Z depth, but not having sufficient coordinate independence to machine
        any curved 3D surface which could "fall away" on more than 1 axis.
        Thus a linearly sloped ramp would be possible and possibly also a
        a curved hump of uniform width, but NOT anything like a hemisphere.
        This definition may only be a result of the CADCAM software I own,
        though. I'm not sure. It is possible, that in practice, it can mean a
        number of things, always a product which cannot handle a full set of
        NC generation to create any shape at will.
        --- In SherlineCNC@yahoogroups.com, Andy Wander <awander@...> wrote:
        >
        > 2-1/2D is anything you can do with a standard vertical mill, using
        only the X-Y table, and the Z(spindle) moving up and down.
        >
        > No pockets on the underside, holes in the sides of the part, or
        anything else that would require a rotation of the part or one of the
        axes.
        >
        > Another way to look at it, if you can see all of the features of the
        part that need machining, by looking at it from above, then you can do
        it with 2-1/2D.
        >
        > ______________________________________
        > Andy Wander
        >
        > -----Original Message-----
        > From: SherlineCNC@yahoogroups.com
        [mailto:SherlineCNC@yahoogroups.com] On Behalf Of tony_dspglobal
        > Sent: Friday, February 06, 2009 8:52 PM
        > To: SherlineCNC@yahoogroups.com
        > Subject: [SherlineCNC] Re: True 3D milling using rotary table
        >
        > Hi Neil,
        >
        > I'm new to CAM so I was wondering what is meant by
        > "2-1/2D"? I understand 2D and 3D, but what does the 1/2D
        > refer to?
        >
        > Thanks
        > Tony
        >
        >
        > --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
        > >
        > > What is available in the way of routines that might generate G-Code
        > > to run an X,Y,Z,A setup to render complex surfaces.
        > > Do I really have to write the code line by line? I don't have an
        > > immediate projects in mind, but I was wondering if anyone has come up
        > > with any solutions to streamline the process. Someone had
        > > asked my about making parts, and I mistakenly told him that I had a 3D
        > > CADCAM setup when I only have TurboCADCAM which is 2-1/2D. (I hadn't
        > > used the stuff in a while.)
        > > --Neil
        > >
        >
        >
        >
        >
        > ------------------------------------
        >
        > Yahoo! Groups Links
        >
        >
        >
        > This communication including any attachments, are intended
        > for the exclusive use of the addressee(s) and contains
        > confidential or copyrighted materials. Duplication,
        > distribution or reproduction is strictly prohibited by law
        > without written permission of Verrex
        >
      • montanaaardvark
        ... Neil, Now that the discussion on 2 1/2D CAD is done, I think your question was actually about CAM programs. There are many options out there, including
        Message 3 of 17 , Feb 7, 2009
        • 0 Attachment
          --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@...> wrote:
          >
          > What is available in the way of routines that might generate G-Code
          > to run an X,Y,Z,A setup to render complex surfaces.
          > Do I really have to write the code line by line? I don't have an
          > immediate projects in mind, but I was wondering if anyone has come up
          > with any solutions to streamline the process. Someone had
          > asked my about making parts, and I mistakenly told him that I had a 3D
          > CADCAM setup when I only have TurboCADCAM which is 2-1/2D. (I hadn't
          > used the stuff in a while.)
          > --Neil
          >
          Neil,


          Now that the discussion on 2 1/2D CAD is done, I think your question
          was actually about CAM programs. There are many options out there,
          including writing your own G-code, but I think there are limits to how
          intricate you might want to go. For example, I've got Gcode files
          that are hundreds of k-bytes, or megabytes, thousands of lines. I
          have no desire to do that by hand!

          I would say to look at, in no particular order: Deskproto and
          Protowizard (popular in jewelry and other intricate 3D shapes), Vector
          (has CAD and CAM), BobCAD/CAM and DeskCNC. I'm currently running
          Deskproto, and do jewelry, which is what generates the huge files, up
          to several megabytes. It's what happens when you're moving a .003"
          diameter cutter around a complex design.

          What I'd like to see is real simultaneous use of all four axes of an
          X, Y, Z, A CNC mill. I have not seen any that do.



          Hope that helps,
          Bob
        • Fred Smith
          ... This simultaneous X-Y-Z-A is called 4 axis machining, and is usually not used, rather a 5th axis is included to assure that enough reach is available
          Message 4 of 17 , Feb 7, 2009
          • 0 Attachment
            --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@...> wrote:
            >
            > What is available in the way of routines that might generate G-Code
            > to run an X,Y,Z,A setup to render complex surfaces.
            > Do I really have to write the code line by line?

            This simultaneous X-Y-Z-A is called 4 axis machining, and is usually
            not used, rather a 5th axis is included to assure that enough "reach"
            is available through the software. This software will provide
            services such as the ability to insert a complex tool and holder into
            a "bottle" shape, carve out the inside, and not permit the tool shank
            or tool holder to come in contact with the mouth of the bottle.
            Another service is to keep a constant tangential angle between a ball
            nosed cutting tool and the angle of a swept surface. This permits
            maximum feed rates and yields the best surface finish because the
            center of the tool ( spinning at 0 SFM) is never used for cutting.
            The complexity of these kind of tasks, the few potential
            installations, and the heavy product support requirement make for
            expensive software costs. Usually in excess of $10,000, plus hefty
            annual maintenance charges.

            There are many sub-optimal ( compared to the above examples)
            solutions that provide nearly the same results at a much lower cost.

            1) 3D surface machining is free to inexpensive, depending on the
            level of control you want to accept.

            For example there is a free version of 3D surface machining called
            Freemill from Mecsoft ( $$$$ Rhino Cam, $$$$ Visual Mill). It will
            only make finish passes of rectangular patches, to get you to buy the
            more expensive software.

            3D surface machining is usually done with a ball nosed cutter, which
            is used to carve a 3D shape from a solid block of material. In
            jewelry making ( of wax casting patterns), the ball nosed cutter is
            replaced with a Sharp V-tipped cutter with a small flat on the end (
            think .005-.010 inch). A great many small incremantal passes are
            made and the shape "appears" as if it had been embedded in the
            substrate.

            With some shapes, it is possible to machine the top and bottom,
            utilizing indexing pins or vises ( or a rotary indexer that can
            position 180 degrees on command). Attachment tabs are needed to
            control the time that the part breaks free from the surrounding
            material. Some programs provide this automatically, but it is also
            very simple to add these to a 3D model.

            Most hobby class 3D machining CAM programs use STL files, which are
            triangulated approximations ( but accurate) of the mathematical
            curves of the surfaces. Some use "polygonized" DXF files too. A few
            can directly process nurbs surfaces in iges or Rhino 3dm files ( like
            Vector cad-cam).

            If you want to do 3D surface machining, you have to have 3D models.
            These can be obtained from a couple of service bureaus, some freely
            downloaded from the internet, can be created from 3D surface scanned
            data, or designed with 3D cad programs. You can also combine these
            techniques to create your model.

            Look at MOI - Moment of Inspiration for an inexpensive 3D solid
            modeler. It currently sells for under $200, and has lots of features
            and capabilities that were previously only available at much higher
            prices ( Rhino 3D at $600-$800 was a popular 3D modeling program), or
            with very limited capabilities or cryptic interfaces.

            2) Now for rotary axis uses: On a Sherline about the most complicated
            that you will find in general use is rotary 4th axis machining.
            (There are a couple of 5 axis machines around, I know of one for sure
            that appeared at last years CNC-Workshop.) This consists mostly of 2
            1/2 axis machining interspersed with rotary indexing. Drill some
            holes, mill a flat, pocket a shape, index 90 or 180 degrees and then
            drill some more holes, mill a flat, pocket a shape, etc. Indexing
            consists of a single command A90.000 or A180.000, so most people
            don't need any special cam software to use this kind of setup. You
            can use this method to mill features on the surface of hex stock, or
            even to make hex stock.

            The next most popular rotary axis application is engraving on a
            cylinder. This is easily accomplished by wiring the rotary axis(A)
            to the Y motor and cutting a flat layout 2 1/2 axis program. Some
            mathmatical scaling is involved to set up your machine, but it's not
            rocket science and you do NOT need any special CAM software.

            For Sherline machines, probably the next most popular application is
            to cut gears or sprocket shapes for power transmission. These are
            usually a simple set of g-code commands that are repeatedly run
            between indexes, equal to one tooth of motion. A bevel gear requires
            2 simultaneous axes of motion ( X and A, like a thread) , but not 4

            For those making jewelry with a rotary axis, DeskCNC ( $250) has a
            routine that zig-zags back and forth along the rotational axis ( X-Z
            contouring) between tiny angular indexes of an stl file, creating a
            3D shape.

            The next step up would be to cut a 3D surface with climb milling
            only, and using rotary contouring. An example part would be a liquid
            flow device that required a high polish and toolmarks only in the
            direction of a helix. Examples are injection molder screws, jet
            engine impellors, and maybe a couple of others. You can create a
            helix shaped toolpath using the Totem pole function in StlWork,and
            then create 3 axis( X-Z-A) rotary toolpaths with Vector cad-cam for
            under $1000.

            As you can see the rotary applications are very part specific and
            most Sherline users will never use more than one or two of the
            methods.

            One last thing about rotary axis machining. Generally it is better
            to mount your part onto the table of a mill than between a rotary
            table and tailstock, because the part is more stable. This means
            that you can take heavier cuts and worry less about chatter, tool
            breakage, and part movement from cutting tool pressure.

            3) 2 1/2 axis machining, generally refers to the ability of a CAM
            program to produce X-Y contouring code, inter mixed with Z plunges
            and retractions. It usually refers to drilling, flat( planar)
            contouring ( like engraving), and pocketing. The processes usually
            can have multiple cuts to the final depth. There should be no lines
            of G-code that contain X, Y, and Z simultaneous motion. ( non-modal
            code however will have all three address words on the same line, even
            though one or more may not be moving)

            That having been said, Sheetcam is a 2 1/2 axis program. It does
            have a couple of 3D machining funcitons like corner sharpening and
            tapered tabbing, but it does NOT create 3D surface machining of
            sculpted surfaces with ball nosed end mills.

            Another thing that tends to differentiate 2 1/2 axis machining from 3
            axis machining is the actual tools used for the two processes. Again
            generally, if you are using a square cornered tool like an end mill
            or an angled tool like a drill or engraving bit or corner chamfering
            tool, this will be referred to as 2 1/2 axis. If you are using a
            full radius cutter to carve out a sculpted 3D surface, this would be
            3 axis machining, even though the g-code may consist entirely of 1 or
            2 axis motion per line. Most 3D surface machining consists of zig-
            zag, raster patterns with X-Z codes for the contours interspersed
            with small Y movements for each pass back and forth.

            In most cases the original part design can be represented by a flat
            drawing with no Z depth, and the programmer adds the desired Z-depth
            to the g-code as part of the programming process. With 3 axis
            programming, the original model is a 3D surface, and the toolpaths
            are developed based on te programmer providing the radius of the ball
            nosed tool tip.

            Fred Smith - IMService
            http://www.imsrv.com
          • Neil Albert
            Thanks Bob. My thought was based on the notion that if programs were specifically designed for X,Y,Z,A CAM that certain shapes could be distilled down to
            Message 5 of 17 , Feb 7, 2009
            • 0 Attachment
              Thanks Bob.

              My thought was based on the notion that if programs were specifically
              designed for X,Y,Z,A CAM that certain shapes could be distilled
              down to relatively simple routines, when the desired goal was a
              carefully chosen subset of the whole specrum of possible shapes.
              Certainly, it seems easier to me to write G-Code by hand to machine a
              hemisphere, for example, if one of the axes were rotary. Your work on
              jewelry sounds like you accomplish some pretty fancy stuff, and I will
              indeed look into DeskProto, DeskCNC, etc.

              Thanks again,
              Neil
              --- In SherlineCNC@yahoogroups.com, "montanaaardvark"
              <boblombardi@...> wrote:
              >
              > --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
              > >
              > > What is available in the way of routines that might generate G-Code
              > > to run an X,Y,Z,A setup to render complex surfaces.
              > > Do I really have to write the code line by line? I don't have an
              > > immediate projects in mind, but I was wondering if anyone has come up
              > > with any solutions to streamline the process. Someone had
              > > asked my about making parts, and I mistakenly told him that I had a 3D
              > > CADCAM setup when I only have TurboCADCAM which is 2-1/2D. (I hadn't
              > > used the stuff in a while.)
              > > --Neil
              > >
              > Neil,
              >
              >
              > Now that the discussion on 2 1/2D CAD is done, I think your question
              > was actually about CAM programs. There are many options out there,
              > including writing your own G-code, but I think there are limits to how
              > intricate you might want to go. For example, I've got Gcode files
              > that are hundreds of k-bytes, or megabytes, thousands of lines. I
              > have no desire to do that by hand!
              >
              > I would say to look at, in no particular order: Deskproto and
              > Protowizard (popular in jewelry and other intricate 3D shapes), Vector
              > (has CAD and CAM), BobCAD/CAM and DeskCNC. I'm currently running
              > Deskproto, and do jewelry, which is what generates the huge files, up
              > to several megabytes. It's what happens when you're moving a .003"
              > diameter cutter around a complex design.
              >
              > What I'd like to see is real simultaneous use of all four axes of an
              > X, Y, Z, A CNC mill. I have not seen any that do.
              >
              >
              >
              > Hope that helps,
              > Bob
              >
            • Dennis Cranston
              One of the issues, it seems to me, that is confusing the discussion is the Subject: True 3D using the rotary table . 3 Dimensional milling means machining
              Message 6 of 17 , Feb 7, 2009
              • 0 Attachment
                One of the issues, it seems to me, that is confusing the discussion is the
                Subject: 'True 3D using the rotary table'. 3 Dimensional milling means
                machining with moves in 3 axis. These are usually the x, y, and z axis. The
                rotary table adds an axis, not a dimension. In certain situations, the y
                axis is mapped to the rotary, this is still 3D, X, A, and Z, again 3 axis
                moving. There is true 4 axis machine as well as 5 axis units. There are
                some interesting youtube videos of 5 axis machining.
                Now the problem is for 3 axis machining, there are many CAM programs
                to generate the G Code. However, a CAM package that generates true 4 axis G
                code, is usually outside the budget range of a Sherline CNC user. I have
                seen small shop packages in the past that advertises they supply 4 axis
                moves, but usually in small print, there is a disclaimer that it is
                'underdevelopment'. I would like to be proven wrong. Now once up in the
                commercial area, $4,000 and up (way up) there are many CAM programs
                available.
                I do some '4 axis' machining on a CNC mill (Tormach) by mounting a
                part blank on a rotary table and performing 3 axis machining on one face of
                the part then rotating the part, doing some more machining, rotating the
                part, etc. Technically this is 3 and 1/2 axis machining and is done by
                concatenating chunks of code for each face into one long part program.

                Dennis in Houston

                > -----Original Message-----
                > From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com]
                > On Behalf Of Neil Albert
                > Sent: Saturday, February 07, 2009 5:24 PM
                > To: SherlineCNC@yahoogroups.com
                > Subject: [SherlineCNC] Re: True 3D milling using rotary table
                >
                > Thanks Bob.
                >
                > My thought was based on the notion that if programs were specifically
                > designed for X,Y,Z,A CAM that certain shapes could be distilled
                > down to relatively simple routines, when the desired goal was a
                > carefully chosen subset of the whole specrum of possible shapes.
                > Certainly, it seems easier to me to write G-Code by hand to machine a
                > hemisphere, for example, if one of the axes were rotary. Your work on
                > jewelry sounds like you accomplish some pretty fancy stuff, and I will
                > indeed look into DeskProto, DeskCNC, etc.
                >
                > Thanks again,
                > Neil
                > --- In SherlineCNC@yahoogroups.com, "montanaaardvark"
                > <boblombardi@...> wrote:
                > >
                > > --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
                > > >
                > > > What is available in the way of routines that might generate G-Code
                > > > to run an X,Y,Z,A setup to render complex surfaces.
                > > > Do I really have to write the code line by line? I don't have an
                > > > immediate projects in mind, but I was wondering if anyone has come up
                > > > with any solutions to streamline the process. Someone had
                > > > asked my about making parts, and I mistakenly told him that I had a 3D
                > > > CADCAM setup when I only have TurboCADCAM which is 2-1/2D. (I hadn't
                > > > used the stuff in a while.)
                > > > --Neil
                > > >
                > > Neil,
                > >
                > >
                > > Now that the discussion on 2 1/2D CAD is done, I think your question
                > > was actually about CAM programs. There are many options out there,
                > > including writing your own G-code, but I think there are limits to how
                > > intricate you might want to go. For example, I've got Gcode files
                > > that are hundreds of k-bytes, or megabytes, thousands of lines. I
                > > have no desire to do that by hand!
                > >
                > > I would say to look at, in no particular order: Deskproto and
                > > Protowizard (popular in jewelry and other intricate 3D shapes), Vector
                > > (has CAD and CAM), BobCAD/CAM and DeskCNC. I'm currently running
                > > Deskproto, and do jewelry, which is what generates the huge files, up
                > > to several megabytes. It's what happens when you're moving a .003"
                > > diameter cutter around a complex design.
                > >
                > > What I'd like to see is real simultaneous use of all four axes of an
                > > X, Y, Z, A CNC mill. I have not seen any that do.
                > >
                > >
                > >
                > > Hope that helps,
                > > Bob
                > >
                >
                >
                >
                >
                > ------------------------------------
                >
                > Yahoo! Groups Links
                >
                >
                >
              • Neil Albert
                Fred, Thank you for such a marvelous tutorial. I am going to copy it right away to my PC for my reference. An extremely valuable piece I would say, your
                Message 7 of 17 , Feb 7, 2009
                • 0 Attachment
                  Fred,

                  Thank you for such a marvelous tutorial. I am going to copy
                  it right away to my PC for my reference. An extremely valuable
                  piece I would say, your explanation.

                  Thanks again,
                  Neil
                  --- In SherlineCNC@yahoogroups.com, "Fred Smith" <imserv@...> wrote:
                  >
                  > --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
                  > >
                  > > What is available in the way of routines that might generate G-Code
                  > > to run an X,Y,Z,A setup to render complex surfaces.
                  > > Do I really have to write the code line by line?
                  >
                  > This simultaneous X-Y-Z-A is called 4 axis machining, and is usually
                  > not used, rather a 5th axis is included to assure that enough "reach"
                  > is available through the software. This software will provide
                  > services such as the ability to insert a complex tool and holder into
                  > a "bottle" shape, carve out the inside, and not permit the tool shank
                  > or tool holder to come in contact with the mouth of the bottle.
                  > Another service is to keep a constant tangential angle between a ball
                  > nosed cutting tool and the angle of a swept surface. This permits
                  > maximum feed rates and yields the best surface finish because the
                  > center of the tool ( spinning at 0 SFM) is never used for cutting.
                  > The complexity of these kind of tasks, the few potential
                  > installations, and the heavy product support requirement make for
                  > expensive software costs. Usually in excess of $10,000, plus hefty
                  > annual maintenance charges.
                  >
                  > There are many sub-optimal ( compared to the above examples)
                  > solutions that provide nearly the same results at a much lower cost.
                  >
                  > 1) 3D surface machining is free to inexpensive, depending on the
                  > level of control you want to accept.
                  >
                  > For example there is a free version of 3D surface machining called
                  > Freemill from Mecsoft ( $$$$ Rhino Cam, $$$$ Visual Mill). It will
                  > only make finish passes of rectangular patches, to get you to buy the
                  > more expensive software.
                  >
                  > 3D surface machining is usually done with a ball nosed cutter, which
                  > is used to carve a 3D shape from a solid block of material. In
                  > jewelry making ( of wax casting patterns), the ball nosed cutter is
                  > replaced with a Sharp V-tipped cutter with a small flat on the end (
                  > think .005-.010 inch). A great many small incremantal passes are
                  > made and the shape "appears" as if it had been embedded in the
                  > substrate.
                  >
                  > With some shapes, it is possible to machine the top and bottom,
                  > utilizing indexing pins or vises ( or a rotary indexer that can
                  > position 180 degrees on command). Attachment tabs are needed to
                  > control the time that the part breaks free from the surrounding
                  > material. Some programs provide this automatically, but it is also
                  > very simple to add these to a 3D model.
                  >
                  > Most hobby class 3D machining CAM programs use STL files, which are
                  > triangulated approximations ( but accurate) of the mathematical
                  > curves of the surfaces. Some use "polygonized" DXF files too. A few
                  > can directly process nurbs surfaces in iges or Rhino 3dm files ( like
                  > Vector cad-cam).
                  >
                  > If you want to do 3D surface machining, you have to have 3D models.
                  > These can be obtained from a couple of service bureaus, some freely
                  > downloaded from the internet, can be created from 3D surface scanned
                  > data, or designed with 3D cad programs. You can also combine these
                  > techniques to create your model.
                  >
                  > Look at MOI - Moment of Inspiration for an inexpensive 3D solid
                  > modeler. It currently sells for under $200, and has lots of features
                  > and capabilities that were previously only available at much higher
                  > prices ( Rhino 3D at $600-$800 was a popular 3D modeling program), or
                  > with very limited capabilities or cryptic interfaces.
                  >
                  > 2) Now for rotary axis uses: On a Sherline about the most complicated
                  > that you will find in general use is rotary 4th axis machining.
                  > (There are a couple of 5 axis machines around, I know of one for sure
                  > that appeared at last years CNC-Workshop.) This consists mostly of 2
                  > 1/2 axis machining interspersed with rotary indexing. Drill some
                  > holes, mill a flat, pocket a shape, index 90 or 180 degrees and then
                  > drill some more holes, mill a flat, pocket a shape, etc. Indexing
                  > consists of a single command A90.000 or A180.000, so most people
                  > don't need any special cam software to use this kind of setup. You
                  > can use this method to mill features on the surface of hex stock, or
                  > even to make hex stock.
                  >
                  > The next most popular rotary axis application is engraving on a
                  > cylinder. This is easily accomplished by wiring the rotary axis(A)
                  > to the Y motor and cutting a flat layout 2 1/2 axis program. Some
                  > mathmatical scaling is involved to set up your machine, but it's not
                  > rocket science and you do NOT need any special CAM software.
                  >
                  > For Sherline machines, probably the next most popular application is
                  > to cut gears or sprocket shapes for power transmission. These are
                  > usually a simple set of g-code commands that are repeatedly run
                  > between indexes, equal to one tooth of motion. A bevel gear requires
                  > 2 simultaneous axes of motion ( X and A, like a thread) , but not 4
                  >
                  > For those making jewelry with a rotary axis, DeskCNC ( $250) has a
                  > routine that zig-zags back and forth along the rotational axis ( X-Z
                  > contouring) between tiny angular indexes of an stl file, creating a
                  > 3D shape.
                  >
                  > The next step up would be to cut a 3D surface with climb milling
                  > only, and using rotary contouring. An example part would be a liquid
                  > flow device that required a high polish and toolmarks only in the
                  > direction of a helix. Examples are injection molder screws, jet
                  > engine impellors, and maybe a couple of others. You can create a
                  > helix shaped toolpath using the Totem pole function in StlWork,and
                  > then create 3 axis( X-Z-A) rotary toolpaths with Vector cad-cam for
                  > under $1000.
                  >
                  > As you can see the rotary applications are very part specific and
                  > most Sherline users will never use more than one or two of the
                  > methods.
                  >
                  > One last thing about rotary axis machining. Generally it is better
                  > to mount your part onto the table of a mill than between a rotary
                  > table and tailstock, because the part is more stable. This means
                  > that you can take heavier cuts and worry less about chatter, tool
                  > breakage, and part movement from cutting tool pressure.
                  >
                  > 3) 2 1/2 axis machining, generally refers to the ability of a CAM
                  > program to produce X-Y contouring code, inter mixed with Z plunges
                  > and retractions. It usually refers to drilling, flat( planar)
                  > contouring ( like engraving), and pocketing. The processes usually
                  > can have multiple cuts to the final depth. There should be no lines
                  > of G-code that contain X, Y, and Z simultaneous motion. ( non-modal
                  > code however will have all three address words on the same line, even
                  > though one or more may not be moving)
                  >
                  > That having been said, Sheetcam is a 2 1/2 axis program. It does
                  > have a couple of 3D machining funcitons like corner sharpening and
                  > tapered tabbing, but it does NOT create 3D surface machining of
                  > sculpted surfaces with ball nosed end mills.
                  >
                  > Another thing that tends to differentiate 2 1/2 axis machining from 3
                  > axis machining is the actual tools used for the two processes. Again
                  > generally, if you are using a square cornered tool like an end mill
                  > or an angled tool like a drill or engraving bit or corner chamfering
                  > tool, this will be referred to as 2 1/2 axis. If you are using a
                  > full radius cutter to carve out a sculpted 3D surface, this would be
                  > 3 axis machining, even though the g-code may consist entirely of 1 or
                  > 2 axis motion per line. Most 3D surface machining consists of zig-
                  > zag, raster patterns with X-Z codes for the contours interspersed
                  > with small Y movements for each pass back and forth.
                  >
                  > In most cases the original part design can be represented by a flat
                  > drawing with no Z depth, and the programmer adds the desired Z-depth
                  > to the g-code as part of the programming process. With 3 axis
                  > programming, the original model is a 3D surface, and the toolpaths
                  > are developed based on te programmer providing the radius of the ball
                  > nosed tool tip.
                  >
                  > Fred Smith - IMService
                  > http://www.imsrv.com
                  >
                • Hamilton Elliott
                  Hi Guys, I have been using a Sherline lathe (manual not CNC) for a few months and am now interested in getting a mill as I now see that a lathe on its own has
                  Message 8 of 17 , Feb 8, 2009
                  • 0 Attachment
                    Hi Guys,

                    I have been using a Sherline lathe (manual not CNC) for a few months and am
                    now interested in getting a mill as I now see that a lathe on its own has a
                    limited area of work.

                    I think that CNC is the way I should be thinking for the mill and I would
                    like some comments and advice on my shopping list.

                    5410A-CNC Mill
                    Gecko G540 controller
                    ?? Stepper motors
                    ?? CAD software

                    I have an early copy of Corel Draw (Ver 6) which I know reasonably well. Is
                    this the sort of thing that I need?.

                    I would like a European source for the Stepper Motors if possible for lower
                    shipping costs.

                    I have a range of possible laptops/Desktop computers as I am in that
                    business.

                    Is there anything else I should include? Any other accessories from Sherline
                    as its much cheaper to get it in one shipment.

                    Thanks for any help you can give me.

                    Regards,
                    Hamilton
                  • Neil Albert
                    Not to belabor the subject, but perhaps my question would have been better served had I said A,Y,Z which would be cylindrical coordinates. If programs which
                    Message 9 of 17 , Feb 9, 2009
                    • 0 Attachment
                      Not to belabor the subject, but perhaps my question would have been
                      better served had I said A,Y,Z which would be cylindrical coordinates.
                      If programs which maintained these axes in trigonometric (sin, cos,
                      etc.) relationships, then a means to create (some)3D surfaces could be
                      accomplished relatively mimimal resources.
                      --- In SherlineCNC@yahoogroups.com, "Fred Smith" <imserv@...> wrote:
                      >
                      > --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
                      > >
                      > > What is available in the way of routines that might generate G-Code
                      > > to run an X,Y,Z,A setup to render complex surfaces.
                      > > Do I really have to write the code line by line?
                      >
                      > This simultaneous X-Y-Z-A is called 4 axis machining, and is usually
                      > not used, rather a 5th axis is included to assure that enough "reach"
                      > is available through the software. This software will provide
                      > services such as the ability to insert a complex tool and holder into
                      > a "bottle" shape, carve out the inside, and not permit the tool shank
                      > or tool holder to come in contact with the mouth of the bottle.
                      > Another service is to keep a constant tangential angle between a ball
                      > nosed cutting tool and the angle of a swept surface. This permits
                      > maximum feed rates and yields the best surface finish because the
                      > center of the tool ( spinning at 0 SFM) is never used for cutting.
                      > The complexity of these kind of tasks, the few potential
                      > installations, and the heavy product support requirement make for
                      > expensive software costs. Usually in excess of $10,000, plus hefty
                      > annual maintenance charges.
                      >
                      > There are many sub-optimal ( compared to the above examples)
                      > solutions that provide nearly the same results at a much lower cost.
                      >
                      > 1) 3D surface machining is free to inexpensive, depending on the
                      > level of control you want to accept.
                      >
                      > For example there is a free version of 3D surface machining called
                      > Freemill from Mecsoft ( $$$$ Rhino Cam, $$$$ Visual Mill). It will
                      > only make finish passes of rectangular patches, to get you to buy the
                      > more expensive software.
                      >
                      > 3D surface machining is usually done with a ball nosed cutter, which
                      > is used to carve a 3D shape from a solid block of material. In
                      > jewelry making ( of wax casting patterns), the ball nosed cutter is
                      > replaced with a Sharp V-tipped cutter with a small flat on the end (
                      > think .005-.010 inch). A great many small incremantal passes are
                      > made and the shape "appears" as if it had been embedded in the
                      > substrate.
                      >
                      > With some shapes, it is possible to machine the top and bottom,
                      > utilizing indexing pins or vises ( or a rotary indexer that can
                      > position 180 degrees on command). Attachment tabs are needed to
                      > control the time that the part breaks free from the surrounding
                      > material. Some programs provide this automatically, but it is also
                      > very simple to add these to a 3D model.
                      >
                      > Most hobby class 3D machining CAM programs use STL files, which are
                      > triangulated approximations ( but accurate) of the mathematical
                      > curves of the surfaces. Some use "polygonized" DXF files too. A few
                      > can directly process nurbs surfaces in iges or Rhino 3dm files ( like
                      > Vector cad-cam).
                      >
                      > If you want to do 3D surface machining, you have to have 3D models.
                      > These can be obtained from a couple of service bureaus, some freely
                      > downloaded from the internet, can be created from 3D surface scanned
                      > data, or designed with 3D cad programs. You can also combine these
                      > techniques to create your model.
                      >
                      > Look at MOI - Moment of Inspiration for an inexpensive 3D solid
                      > modeler. It currently sells for under $200, and has lots of features
                      > and capabilities that were previously only available at much higher
                      > prices ( Rhino 3D at $600-$800 was a popular 3D modeling program), or
                      > with very limited capabilities or cryptic interfaces.
                      >
                      > 2) Now for rotary axis uses: On a Sherline about the most complicated
                      > that you will find in general use is rotary 4th axis machining.
                      > (There are a couple of 5 axis machines around, I know of one for sure
                      > that appeared at last years CNC-Workshop.) This consists mostly of 2
                      > 1/2 axis machining interspersed with rotary indexing. Drill some
                      > holes, mill a flat, pocket a shape, index 90 or 180 degrees and then
                      > drill some more holes, mill a flat, pocket a shape, etc. Indexing
                      > consists of a single command A90.000 or A180.000, so most people
                      > don't need any special cam software to use this kind of setup. You
                      > can use this method to mill features on the surface of hex stock, or
                      > even to make hex stock.
                      >
                      > The next most popular rotary axis application is engraving on a
                      > cylinder. This is easily accomplished by wiring the rotary axis(A)
                      > to the Y motor and cutting a flat layout 2 1/2 axis program. Some
                      > mathmatical scaling is involved to set up your machine, but it's not
                      > rocket science and you do NOT need any special CAM software.
                      >
                      > For Sherline machines, probably the next most popular application is
                      > to cut gears or sprocket shapes for power transmission. These are
                      > usually a simple set of g-code commands that are repeatedly run
                      > between indexes, equal to one tooth of motion. A bevel gear requires
                      > 2 simultaneous axes of motion ( X and A, like a thread) , but not 4
                      >
                      > For those making jewelry with a rotary axis, DeskCNC ( $250) has a
                      > routine that zig-zags back and forth along the rotational axis ( X-Z
                      > contouring) between tiny angular indexes of an stl file, creating a
                      > 3D shape.
                      >
                      > The next step up would be to cut a 3D surface with climb milling
                      > only, and using rotary contouring. An example part would be a liquid
                      > flow device that required a high polish and toolmarks only in the
                      > direction of a helix. Examples are injection molder screws, jet
                      > engine impellors, and maybe a couple of others. You can create a
                      > helix shaped toolpath using the Totem pole function in StlWork,and
                      > then create 3 axis( X-Z-A) rotary toolpaths with Vector cad-cam for
                      > under $1000.
                      >
                      > As you can see the rotary applications are very part specific and
                      > most Sherline users will never use more than one or two of the
                      > methods.
                      >
                      > One last thing about rotary axis machining. Generally it is better
                      > to mount your part onto the table of a mill than between a rotary
                      > table and tailstock, because the part is more stable. This means
                      > that you can take heavier cuts and worry less about chatter, tool
                      > breakage, and part movement from cutting tool pressure.
                      >
                      > 3) 2 1/2 axis machining, generally refers to the ability of a CAM
                      > program to produce X-Y contouring code, inter mixed with Z plunges
                      > and retractions. It usually refers to drilling, flat( planar)
                      > contouring ( like engraving), and pocketing. The processes usually
                      > can have multiple cuts to the final depth. There should be no lines
                      > of G-code that contain X, Y, and Z simultaneous motion. ( non-modal
                      > code however will have all three address words on the same line, even
                      > though one or more may not be moving)
                      >
                      > That having been said, Sheetcam is a 2 1/2 axis program. It does
                      > have a couple of 3D machining funcitons like corner sharpening and
                      > tapered tabbing, but it does NOT create 3D surface machining of
                      > sculpted surfaces with ball nosed end mills.
                      >
                      > Another thing that tends to differentiate 2 1/2 axis machining from 3
                      > axis machining is the actual tools used for the two processes. Again
                      > generally, if you are using a square cornered tool like an end mill
                      > or an angled tool like a drill or engraving bit or corner chamfering
                      > tool, this will be referred to as 2 1/2 axis. If you are using a
                      > full radius cutter to carve out a sculpted 3D surface, this would be
                      > 3 axis machining, even though the g-code may consist entirely of 1 or
                      > 2 axis motion per line. Most 3D surface machining consists of zig-
                      > zag, raster patterns with X-Z codes for the contours interspersed
                      > with small Y movements for each pass back and forth.
                      >
                      > In most cases the original part design can be represented by a flat
                      > drawing with no Z depth, and the programmer adds the desired Z-depth
                      > to the g-code as part of the programming process. With 3 axis
                      > programming, the original model is a 3D surface, and the toolpaths
                      > are developed based on te programmer providing the radius of the ball
                      > nosed tool tip.
                      >
                      > Fred Smith - IMService
                      > http://www.imsrv.com
                      >
                    Your message has been successfully submitted and would be delivered to recipients shortly.