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

Re: Bit life in steel

Expand Messages
  • mattdbartlett
    I don t have any experience with SGS. It s probably better than the unmarked import mills in any case. You re using flood coolant, is it a good stream? IE, can
    Message 1 of 26 , Nov 23, 2012
    • 0 Attachment
      I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.

      You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.

      I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.

      I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)

      One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.

      Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.

      --- In mill_drill@yahoogroups.com, "brianpimm@..." <brianpimm@...> wrote:
      >
      >
      >
      >
      >
      >
      >
      >
      >
      > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
      > >
      > > Couple things that would be interesting to know
      > >
      > > * Is this a ball end mill, or a square end mill. You are talking >about waterline milling, which makes me ask.
      >
      > Square end mill.
      >
      > > * Is this an uncoated mill?
      >
      > Uncoated
      >
      > > * Are you running coolant, or an air blast to clear chips?
      >
      > Flood coolant
      >
      > >
      > > A few generic tips. Chatter is usually not caused by backlash, but >properly. Backlash tends to lead to broken tools if you have a lot >of it, and you are trying to climb mill. This is especially true >with smaller cutters.
      > >
      > > Dull cutters usually have a couple causes.
      > >
      > > 1) Spindle speed too high
      > > 2) Cheap, low quality cutter (they dull faster, nothing's free).
      > > 3) Feed rate too low (causes rubbing, heating, destroys the edge)
      > > 4) Chip re-cutting
      > >
      > > It sounds like you may be slotting (cutting the full width of the
      >
      > Yes
      >
      > >cutter. This is one of the harshest things you can do with an end >mill. GWizard has steered you in the direction of lower speeds and >feeds, which is necessary, but the other thing you want to take into >account is chip re-cutting. This happens when the chips hang around >near the cut, and get pulled back in by the mill. It's really hard >on end mills, cause they are doing double or triple the work they >normally would. It can cause catastrophic failures (snapping the end >mill in two) if the chips get packed in there. You can deal with >this with flood cooling, or an air blast. I have also followed the >cutter around with a shop vac, sucking up the trailing chips as I >went. Works well, but is tedious.
      > >
      > > I don't think a 4 flute is necessarily going to last longer, but >it's going to be stronger (less deflection) and you will be able to >increase your feed rate by 100%. I would recommend 4flute end mills >for steel.
      > >
      > > -Matt
      >
      > I have some 4 flute end mills on order.
      >
      > The endmill I used was bought on fleebay it is a SGS marked mill, is that good, bad or ugly? What brands of cutters are good?
      >
      >
      > Thanks
      > Brian
      >
      >
      > >
      > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
      > > >
      > > > What can I expect for bit life cutting steel?
      > > > The mill is a Grizzly G1007 converted to CNC before I bought it.
      > > >
      > > > I bought the mill a little over a year ago as a learning tool, I thought I could teach myself some basic machining with it but I finally came to the realization that I needed to learn how to rebuild the mill before I could expect good results. I mainly work Aluminum and had fair to poor results a lot of chatter among plenty of other things. I tried to cut a tool out of steel and it just mauled the bit. After much reading I decided it was partially due to backlash and slop in general. So I embarked on a journey of learning how to reload the ball screw balls with larger balls and now have gone from .013 combined backlash (ball screw and thrust bearing without any method of adjustment) in both X and Y to .000 in Y and .003 in the X, I also got the Z down to .002. I am going to order more balls and see if I can get X and Z to 0.000 also.
      > > >
      > > > Last night I ran the part again and had much better results but it still dulled the bit to the point it's a throw away after one part. I also tried GWizzard for the first time and found the feeds were much slower than any other calculator I have tried.
      > > >
      > > > This was a HSS 3/16" 2 flute bit which is probably not a good choice but it was the only 3/16" I had.
      > > >
      > > > I guess I'm looking to find out what the expected bit life would be under "perfect conditions" on this mill. The part was cut from 1/4" mild steel, I used mesh cam to generate the Gcode using just waterline finish for a minimum width cut, the cut length was 271" at .020" depth full width cut. Feed rate was 1.4 IPM at 1220 RPM this gave a chip load of 0.0006 according to Gwizzard.
      > > >
      > > > This part lays out nicely with 4 parts per run and I'm hoping I can cut it with 1 bit once I get the backlash tightened up a bit more.
      > > >
      > > > Would a 4 or 5 flute bit last longer, how about a deeper cut so I use more of the cutting edge?
      > > >
      > > > Looking for advise.
      > > >
      > > > Brian
      > > >
      > >
      >
    • brianpimm@rocketmail.com
      ... Yes it s a good stream, I have trouble containing the spray, ;) I m using the waterline finish pass to minimize the amount of material removed, if I use
      Message 2 of 26 , Nov 23, 2012
      • 0 Attachment
        --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@...> wrote:
        >
        > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
        >
        > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.

        Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.


        >
        > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.

        1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(

        >
        > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
        >
        > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
        >
        > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.

        It looks dull to me, here are some comparison pics of new and worn, and the part in question.

        Dull End mill Pic
        http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg

        New End mill Pic
        http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg

        Tool Pics
        http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
        http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
        http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
        http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
      • mattdbartlett
        The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate
        Message 3 of 26 , Nov 24, 2012
        • 0 Attachment
          The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.

          --- In mill_drill@yahoogroups.com, "brianpimm@..." <brianpimm@...> wrote:
          >
          >
          >
          >
          >
          >
          >
          >
          > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
          > >
          > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
          > >
          > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
          >
          > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
          >
          >
          > >
          > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
          >
          > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
          >
          > >
          > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
          > >
          > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
          > >
          > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
          >
          > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
          >
          > Dull End mill Pic
          > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
          >
          > New End mill Pic
          > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
          >
          > Tool Pics
          > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
          > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
          > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
          > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
          >
        • brianpimm@rocketmail.com
          Entry is a plunge at .7 IPM. What should I be looking for as a cause for the breakage if it s not the plunge rate. I still have .003 backlash in the X axis and
          Message 4 of 26 , Nov 24, 2012
          • 0 Attachment
            Entry is a plunge at .7 IPM.

            What should I be looking for as a cause for the breakage if it's not the plunge rate. I still have .003 backlash in the X axis and .002 in the Z axis, would those contribute to the problem?

            I'm assuming that unwanted motion of the part vs the end mill is the source of the problem. Am I correct in my assumption?

            Brian


            --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@...> wrote:
            >
            > The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.
            >
            > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
            > >
            > >
            > >
            > >
            > >
            > >
            > >
            > >
            > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
            > > >
            > > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
            > > >
            > > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
            > >
            > > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
            > >
            > >
            > > >
            > > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
            > >
            > > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
            > >
            > > >
            > > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
            > > >
            > > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
            > > >
            > > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
            > >
            > > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
            > >
            > > Dull End mill Pic
            > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
            > >
            > > New End mill Pic
            > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
            > >
            > > Tool Pics
            > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
            > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
            > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
            > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
            > >
            >
          • mattdbartlett
            The feed rate seems ok. How does it sound when it touches down? 2-3 thou backlash is not that much.. I ve got about 12 on my knee mill, though it has more mass
            Message 5 of 26 , Nov 24, 2012
            • 0 Attachment
              The feed rate seems ok. How does it sound when it touches down? 2-3 thou backlash is not that much.. I've got about 12 on my knee mill, though it has more mass in the bed. How loose are your gibs? If they are really loose, your backlash is going to have more effect, though they would have to be pretty loose for a 3/16" endmill to start throwing things around. I'm guessing it's having some issues with the entry method, can you set it to a 2d or 3d entry rather than a straight plunge (not sure, never used meshcam). Another thing you might double check is the tram of your head, if it is off, then one side of the cutter is going to touch down first, and that can set up some nasty vibrations when plunging.

              --- In mill_drill@yahoogroups.com, "brianpimm@..." <brianpimm@...> wrote:
              >
              >
              >
              > Entry is a plunge at .7 IPM.
              >
              > What should I be looking for as a cause for the breakage if it's not the plunge rate. I still have .003 backlash in the X axis and .002 in the Z axis, would those contribute to the problem?
              >
              > I'm assuming that unwanted motion of the part vs the end mill is the source of the problem. Am I correct in my assumption?
              >
              > Brian
              >
              >
              > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
              > >
              > > The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.
              > >
              > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
              > > >
              > > >
              > > >
              > > >
              > > >
              > > >
              > > >
              > > >
              > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
              > > > >
              > > > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
              > > > >
              > > > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
              > > >
              > > > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
              > > >
              > > >
              > > > >
              > > > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
              > > >
              > > > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
              > > >
              > > > >
              > > > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
              > > > >
              > > > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
              > > > >
              > > > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
              > > >
              > > > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
              > > >
              > > > Dull End mill Pic
              > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
              > > >
              > > > New End mill Pic
              > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
              > > >
              > > > Tool Pics
              > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
              > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
              > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
              > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
              > > >
              > >
              >
            • brianpimm@rocketmail.com
              I couldn t hear the touchdown over the machine noise, the gibs are tight, using a large screwdriver almost as tight as I can get them, I wanted to make sure
              Message 6 of 26 , Nov 25, 2012
              • 0 Attachment
                I couldn't hear the touchdown over the machine noise, the gibs are tight, using a large screwdriver almost as tight as I can get them, I wanted to make sure they weren't adding to the backlash measurements then never backed them off, the steppers don't seem to mind. I think strait plunge is my only option with meshcam, I'll look again. I trammed it to less than .001 in 12" but then moved the head and now it's around .007 in 12", if my math is correct that's .000109" in a 3/16 tool, is that enough to cause problems?

                Could the spindle bearings be causing this problem? I haven't checked them other than by hand feeling for play which I don't feel any by hand. What is the proper procedure for checking the spindle bearings?

                I was running at 1220 RPM, would a higher RPM help or hurt? Just thinking maybe 1220 hits a resonance in the machine and upping it by a bit might move it out of resonance?

                Thanks
                Brian

                --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@...> wrote:
                >
                > The feed rate seems ok. How does it sound when it touches down? 2-3 thou backlash is not that much.. I've got about 12 on my knee mill, though it has more mass in the bed. How loose are your gibs? If they are really loose, your backlash is going to have more effect, though they would have to be pretty loose for a 3/16" endmill to start throwing things around. I'm guessing it's having some issues with the entry method, can you set it to a 2d or 3d entry rather than a straight plunge (not sure, never used meshcam). Another thing you might double check is the tram of your head, if it is off, then one side of the cutter is going to touch down first, and that can set up some nasty vibrations when plunging.
                >
                > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                > >
                > >
                > >
                > > Entry is a plunge at .7 IPM.
                > >
                > > What should I be looking for as a cause for the breakage if it's not the plunge rate. I still have .003 backlash in the X axis and .002 in the Z axis, would those contribute to the problem?
                > >
                > > I'm assuming that unwanted motion of the part vs the end mill is the source of the problem. Am I correct in my assumption?
                > >
                > > Brian
                > >
                > >
                > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                > > >
                > > > The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.
                > > >
                > > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                > > > >
                > > > >
                > > > >
                > > > >
                > > > >
                > > > >
                > > > >
                > > > >
                > > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                > > > > >
                > > > > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
                > > > > >
                > > > > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
                > > > >
                > > > > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
                > > > >
                > > > >
                > > > > >
                > > > > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
                > > > >
                > > > > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
                > > > >
                > > > > >
                > > > > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
                > > > > >
                > > > > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
                > > > > >
                > > > > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
                > > > >
                > > > > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
                > > > >
                > > > > Dull End mill Pic
                > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
                > > > >
                > > > > New End mill Pic
                > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
                > > > >
                > > > > Tool Pics
                > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
                > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
                > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
                > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
                > > > >
                > > >
                > >
                >
              • brianpimm@rocketmail.com
                What about vertical deflection of the workpiece, it was a piece of 1/4 plate 5 wide and was clamped at each end probably a 10 span. I m thinking that could
                Message 7 of 26 , Nov 26, 2012
                • 0 Attachment
                  What about vertical deflection of the workpiece, it was a piece of 1/4" plate 5" wide and was clamped at each end probably a 10" span. I'm thinking that could be a cause of the chipping cutting edge. I'm thinking of using a piece of plywood as a sacrificial support, I just don't like the idea of wood shavings and flood coolant. Any thoughts?

                  Brian

                  --- In mill_drill@yahoogroups.com, "brianpimm@..." <brianpimm@...> wrote:
                  >
                  > I couldn't hear the touchdown over the machine noise, the gibs are tight, using a large screwdriver almost as tight as I can get them, I wanted to make sure they weren't adding to the backlash measurements then never backed them off, the steppers don't seem to mind. I think strait plunge is my only option with meshcam, I'll look again. I trammed it to less than .001 in 12" but then moved the head and now it's around .007 in 12", if my math is correct that's .000109" in a 3/16 tool, is that enough to cause problems?
                  >
                  > Could the spindle bearings be causing this problem? I haven't checked them other than by hand feeling for play which I don't feel any by hand. What is the proper procedure for checking the spindle bearings?
                  >
                  > I was running at 1220 RPM, would a higher RPM help or hurt? Just thinking maybe 1220 hits a resonance in the machine and upping it by a bit might move it out of resonance?
                  >
                  > Thanks
                  > Brian
                  >
                  > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                  > >
                  > > The feed rate seems ok. How does it sound when it touches down? 2-3 thou backlash is not that much.. I've got about 12 on my knee mill, though it has more mass in the bed. How loose are your gibs? If they are really loose, your backlash is going to have more effect, though they would have to be pretty loose for a 3/16" endmill to start throwing things around. I'm guessing it's having some issues with the entry method, can you set it to a 2d or 3d entry rather than a straight plunge (not sure, never used meshcam). Another thing you might double check is the tram of your head, if it is off, then one side of the cutter is going to touch down first, and that can set up some nasty vibrations when plunging.
                  > >
                  > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                  > > >
                  > > >
                  > > >
                  > > > Entry is a plunge at .7 IPM.
                  > > >
                  > > > What should I be looking for as a cause for the breakage if it's not the plunge rate. I still have .003 backlash in the X axis and .002 in the Z axis, would those contribute to the problem?
                  > > >
                  > > > I'm assuming that unwanted motion of the part vs the end mill is the source of the problem. Am I correct in my assumption?
                  > > >
                  > > > Brian
                  > > >
                  > > >
                  > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                  > > > >
                  > > > > The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.
                  > > > >
                  > > > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                  > > > > >
                  > > > > >
                  > > > > >
                  > > > > >
                  > > > > >
                  > > > > >
                  > > > > >
                  > > > > >
                  > > > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                  > > > > > >
                  > > > > > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
                  > > > > > >
                  > > > > > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
                  > > > > >
                  > > > > > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
                  > > > > >
                  > > > > >
                  > > > > > >
                  > > > > > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
                  > > > > >
                  > > > > > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
                  > > > > >
                  > > > > > >
                  > > > > > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
                  > > > > > >
                  > > > > > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
                  > > > > > >
                  > > > > > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
                  > > > > >
                  > > > > > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
                  > > > > >
                  > > > > > Dull End mill Pic
                  > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
                  > > > > >
                  > > > > > New End mill Pic
                  > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
                  > > > > >
                  > > > > > Tool Pics
                  > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
                  > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
                  > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
                  > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
                  > > > > >
                  > > > >
                  > > >
                  > >
                  >
                • mattdbartlett
                  Yeah, that could do it, the thing would be flexing pretty bad in the middle. Are you supporting it on parallels? I would contemplate a backer, or adding more
                  Message 8 of 26 , Nov 26, 2012
                  • 0 Attachment
                    Yeah, that could do it, the thing would be flexing pretty bad in the middle. Are you supporting it on parallels? I would contemplate a backer, or adding more parallels/clamps around the perimeter.

                    If you are worried about wood chips, you might try a piece of acrylic (plexiglass). It's dimensionally accurate, and and chips should not cause rusting or contamination issues with the coolant.

                    --- In mill_drill@yahoogroups.com, "brianpimm@..." <brianpimm@...> wrote:
                    >
                    > What about vertical deflection of the workpiece, it was a piece of 1/4" plate 5" wide and was clamped at each end probably a 10" span. I'm thinking that could be a cause of the chipping cutting edge. I'm thinking of using a piece of plywood as a sacrificial support, I just don't like the idea of wood shavings and flood coolant. Any thoughts?
                    >
                    > Brian
                    >
                    > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                    > >
                    > > I couldn't hear the touchdown over the machine noise, the gibs are tight, using a large screwdriver almost as tight as I can get them, I wanted to make sure they weren't adding to the backlash measurements then never backed them off, the steppers don't seem to mind. I think strait plunge is my only option with meshcam, I'll look again. I trammed it to less than .001 in 12" but then moved the head and now it's around .007 in 12", if my math is correct that's .000109" in a 3/16 tool, is that enough to cause problems?
                    > >
                    > > Could the spindle bearings be causing this problem? I haven't checked them other than by hand feeling for play which I don't feel any by hand. What is the proper procedure for checking the spindle bearings?
                    > >
                    > > I was running at 1220 RPM, would a higher RPM help or hurt? Just thinking maybe 1220 hits a resonance in the machine and upping it by a bit might move it out of resonance?
                    > >
                    > > Thanks
                    > > Brian
                    > >
                    > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                    > > >
                    > > > The feed rate seems ok. How does it sound when it touches down? 2-3 thou backlash is not that much.. I've got about 12 on my knee mill, though it has more mass in the bed. How loose are your gibs? If they are really loose, your backlash is going to have more effect, though they would have to be pretty loose for a 3/16" endmill to start throwing things around. I'm guessing it's having some issues with the entry method, can you set it to a 2d or 3d entry rather than a straight plunge (not sure, never used meshcam). Another thing you might double check is the tram of your head, if it is off, then one side of the cutter is going to touch down first, and that can set up some nasty vibrations when plunging.
                    > > >
                    > > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                    > > > >
                    > > > >
                    > > > >
                    > > > > Entry is a plunge at .7 IPM.
                    > > > >
                    > > > > What should I be looking for as a cause for the breakage if it's not the plunge rate. I still have .003 backlash in the X axis and .002 in the Z axis, would those contribute to the problem?
                    > > > >
                    > > > > I'm assuming that unwanted motion of the part vs the end mill is the source of the problem. Am I correct in my assumption?
                    > > > >
                    > > > > Brian
                    > > > >
                    > > > >
                    > > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                    > > > > >
                    > > > > > The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.
                    > > > > >
                    > > > > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                    > > > > > >
                    > > > > > >
                    > > > > > >
                    > > > > > >
                    > > > > > >
                    > > > > > >
                    > > > > > >
                    > > > > > >
                    > > > > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                    > > > > > > >
                    > > > > > > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
                    > > > > > > >
                    > > > > > > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
                    > > > > > >
                    > > > > > > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
                    > > > > > >
                    > > > > > >
                    > > > > > > >
                    > > > > > > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
                    > > > > > >
                    > > > > > > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
                    > > > > > >
                    > > > > > > >
                    > > > > > > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
                    > > > > > > >
                    > > > > > > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
                    > > > > > > >
                    > > > > > > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
                    > > > > > >
                    > > > > > > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
                    > > > > > >
                    > > > > > > Dull End mill Pic
                    > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
                    > > > > > >
                    > > > > > > New End mill Pic
                    > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
                    > > > > > >
                    > > > > > > Tool Pics
                    > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
                    > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
                    > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
                    > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
                    > > > > > >
                    > > > > >
                    > > > >
                    > > >
                    > >
                    >
                  • Jerry Durand
                    ... I use acrylic all the time for fixturing, mostly with our small CNC mill. It s cheap (I get 1/4 stuff free from a supermarket that uses it as food
                    Message 9 of 26 , Nov 26, 2012
                    • 0 Attachment
                      On 11/26/2012 11:26 AM, mattdbartlett wrote:
                      > Yeah, that could do it, the thing would be flexing pretty bad in the middle. Are you supporting it on parallels? I would contemplate a backer, or adding more parallels/clamps around the perimeter.
                      >
                      > If you are worried about wood chips, you might try a piece of acrylic (plexiglass). It's dimensionally accurate, and and chips should not cause rusting or contamination issues with the coolant.
                      >

                      I use acrylic all the time for fixturing, mostly with our small CNC
                      mill. It's cheap (I get 1/4" stuff free from a supermarket that uses it
                      as food dividers until it gets scratched) and it's easy to cut into shape.

                      I wouldn't use it for holding down anything that needs serious milling,
                      but as a backer and for light milling it works fine.

                      --
                      Jerry Durand, Durand Interstellar, Inc. www.interstellar.com
                      tel: +1 408 356-3886, USA toll free: 1 866 356-3886
                      Skype: jerrydurand
                    • brianpimm@rocketmail.com
                      I like that idea, doesn t compress like wood would.
                      Message 10 of 26 , Nov 26, 2012
                      • 0 Attachment
                        I like that idea, doesn't compress like wood would.

                        --- In mill_drill@yahoogroups.com, Jerry Durand <jdurand@...> wrote:
                        >
                        >
                        > On 11/26/2012 11:26 AM, mattdbartlett wrote:
                        > > Yeah, that could do it, the thing would be flexing pretty bad in the middle. Are you supporting it on parallels? I would contemplate a backer, or adding more parallels/clamps around the perimeter.
                        > >
                        > > If you are worried about wood chips, you might try a piece of acrylic (plexiglass). It's dimensionally accurate, and and chips should not cause rusting or contamination issues with the coolant.
                        > >
                        >
                        > I use acrylic all the time for fixturing, mostly with our small CNC
                        > mill. It's cheap (I get 1/4" stuff free from a supermarket that uses it
                        > as food dividers until it gets scratched) and it's easy to cut into shape.
                        >
                        > I wouldn't use it for holding down anything that needs serious milling,
                        > but as a backer and for light milling it works fine.
                        >
                        > --
                        > Jerry Durand, Durand Interstellar, Inc. www.interstellar.com
                        > tel: +1 408 356-3886, USA toll free: 1 866 356-3886
                        > Skype: jerrydurand
                        >
                      • brianpimm@rocketmail.com
                        Yes it s on parallels on the ends so the middle is unsupported. I ll add a backer and see what happens.
                        Message 11 of 26 , Nov 26, 2012
                        • 0 Attachment
                          Yes it's on parallels on the ends so the middle is unsupported. I'll add a backer and see what happens.

                          --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@...> wrote:
                          >
                          > Yeah, that could do it, the thing would be flexing pretty bad in the middle. Are you supporting it on parallels? I would contemplate a backer, or adding more parallels/clamps around the perimeter.
                          >
                          > If you are worried about wood chips, you might try a piece of acrylic (plexiglass). It's dimensionally accurate, and and chips should not cause rusting or contamination issues with the coolant.
                          >
                          > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                          > >
                          > > What about vertical deflection of the workpiece, it was a piece of 1/4" plate 5" wide and was clamped at each end probably a 10" span. I'm thinking that could be a cause of the chipping cutting edge. I'm thinking of using a piece of plywood as a sacrificial support, I just don't like the idea of wood shavings and flood coolant. Any thoughts?
                          > >
                          > > Brian
                          > >
                          > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                          > > >
                          > > > I couldn't hear the touchdown over the machine noise, the gibs are tight, using a large screwdriver almost as tight as I can get them, I wanted to make sure they weren't adding to the backlash measurements then never backed them off, the steppers don't seem to mind. I think strait plunge is my only option with meshcam, I'll look again. I trammed it to less than .001 in 12" but then moved the head and now it's around .007 in 12", if my math is correct that's .000109" in a 3/16 tool, is that enough to cause problems?
                          > > >
                          > > > Could the spindle bearings be causing this problem? I haven't checked them other than by hand feeling for play which I don't feel any by hand. What is the proper procedure for checking the spindle bearings?
                          > > >
                          > > > I was running at 1220 RPM, would a higher RPM help or hurt? Just thinking maybe 1220 hits a resonance in the machine and upping it by a bit might move it out of resonance?
                          > > >
                          > > > Thanks
                          > > > Brian
                          > > >
                          > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                          > > > >
                          > > > > The feed rate seems ok. How does it sound when it touches down? 2-3 thou backlash is not that much.. I've got about 12 on my knee mill, though it has more mass in the bed. How loose are your gibs? If they are really loose, your backlash is going to have more effect, though they would have to be pretty loose for a 3/16" endmill to start throwing things around. I'm guessing it's having some issues with the entry method, can you set it to a 2d or 3d entry rather than a straight plunge (not sure, never used meshcam). Another thing you might double check is the tram of your head, if it is off, then one side of the cutter is going to touch down first, and that can set up some nasty vibrations when plunging.
                          > > > >
                          > > > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                          > > > > >
                          > > > > >
                          > > > > >
                          > > > > > Entry is a plunge at .7 IPM.
                          > > > > >
                          > > > > > What should I be looking for as a cause for the breakage if it's not the plunge rate. I still have .003 backlash in the X axis and .002 in the Z axis, would those contribute to the problem?
                          > > > > >
                          > > > > > I'm assuming that unwanted motion of the part vs the end mill is the source of the problem. Am I correct in my assumption?
                          > > > > >
                          > > > > > Brian
                          > > > > >
                          > > > > >
                          > > > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                          > > > > > >
                          > > > > > > The tips of those flutes are broken off. I know the look well. What kind of entry move are you using? If you are plunging straight in, make sure the feed rate is appropriate, as it's hard on the bits. That kind of damage I usually see from running into something hard, or introducing the cutter to the work too quickly. The tips are very delicate. I would say, try 40 thou depth, its about 2x what you are doing now, and it may spread the load on the flutes out better.
                          > > > > > >
                          > > > > > > --- In mill_drill@yahoogroups.com, "brianpimm@" <brianpimm@> wrote:
                          > > > > > > >
                          > > > > > > >
                          > > > > > > >
                          > > > > > > >
                          > > > > > > >
                          > > > > > > >
                          > > > > > > >
                          > > > > > > >
                          > > > > > > > --- In mill_drill@yahoogroups.com, "mattdbartlett" <mattdbartlett@> wrote:
                          > > > > > > > >
                          > > > > > > > > I don't have any experience with SGS. It's probably better than the unmarked import mills in any case.
                          > > > > > > > >
                          > > > > > > > > You're using flood coolant, is it a good stream? IE, can you tell if chips are being flushed effectively? I also find it a little strange that you are using a waterline with a square end mill. Waterline is usually used on profiled surfaces, the kind of thing you would use a ball mill for. I don't have much experience with different cam software though, so that could just be the way that Meshcam does things. In AlibreCAM for example, I would use a profile pass with a square end mill.
                          > > > > > > >
                          > > > > > > > Yes it's a good stream, I have trouble containing the spray, ;) I'm using the waterline finish pass to minimize the amount of material removed, if I use the roughing pass it cuts the path twice as wide for clearance, but half of that is full width cutting anyway and I'm just cutting out a part from flat stock. A CNC Plasma table would be a better fit but I have the mill. There is 1 place where the thickness is milled down but it's a small area compared to the whole part. Plus Meshcam is a 3D program and I'm fudging it use it as a 2D.
                          > > > > > > >
                          > > > > > > >
                          > > > > > > > >
                          > > > > > > > > I ran your situation through GWizard, and I get slightly different numbers that you reported, but nothing significant. You say you are running 4 parts. How much cutting are we talking about here? Maybe you are just pushing the cutter past its limits.
                          > > > > > > >
                          > > > > > > > 1 part was 270" of full width cut so 4 would be 1080" @ .020 deep. If I bump up the depth of cut it would shorten the length of cut. Gwizzard seemed to want .062 deoth of cut but I was afraid to try it, to many broken end mills in the pile. :(
                          > > > > > > >
                          > > > > > > > >
                          > > > > > > > > I can't give you a number for how long these things should last, as I have never worn an end-mill out, I always break them before that happens ;)
                          > > > > > > > >
                          > > > > > > > > One thing you might try, especially if you are removing lots of material, is a roughing end mill. They should let you take a deeper pass, with less chatter.
                          > > > > > > > >
                          > > > > > > > > Another thing you can do is to take a look at the end mills with a magnifier and see if they are really dull, or if you are chipping the cutting edge. This is more common with carbide than HSS, but I have done it to my fair share of HSS tools too.
                          > > > > > > >
                          > > > > > > > It looks dull to me, here are some comparison pics of new and worn, and the part in question.
                          > > > > > > >
                          > > > > > > > Dull End mill Pic
                          > > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6101.jpg
                          > > > > > > >
                          > > > > > > > New End mill Pic
                          > > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6100.jpg
                          > > > > > > >
                          > > > > > > > Tool Pics
                          > > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6093.jpg
                          > > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6096.jpg
                          > > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6095.jpg
                          > > > > > > > http://i101.photobucket.com/albums/m57/bdpimm/Mill/IMG_6094.jpg
                          > > > > > > >
                          > > > > > >
                          > > > > >
                          > > > >
                          > > >
                          > >
                          >
                        • Jerry Durand
                          I even make hold-down clamps out of acrylic as part of some fixtures. Works great for acetyl (Delrin) and ABS panels. ... -- Jerry Durand, Durand Interstellar,
                          Message 12 of 26 , Nov 26, 2012
                          • 0 Attachment
                            I even make hold-down clamps out of acrylic as part of some fixtures.
                            Works great for acetyl (Delrin) and ABS panels.

                            On 11/26/2012 12:36 PM, brianpimm@... wrote:
                            > I like that idea, doesn't compress like wood would.
                            >

                            --
                            Jerry Durand, Durand Interstellar, Inc. www.interstellar.com
                            tel: +1 408 356-3886, USA toll free: 1 866 356-3886
                            Skype: jerrydurand
                          • wjhaasman
                            Just a thought,Is the end mill a centercutting end mill? If not the tool will bog down and snap crackle pop. Your problem is not due to backlash either way.
                            Message 13 of 26 , Nov 26, 2012
                            • 0 Attachment
                              Just a thought,Is the end mill a centercutting end mill? If not the tool will bog down and snap crackle pop. Your problem is not due to backlash either way.
                            • brianpimm@rocketmail.com
                              They were advertised as center cutting, but that s fleebay so who knows. Can you tell by the pics?
                              Message 14 of 26 , Nov 26, 2012
                              • 0 Attachment
                                They were advertised as center cutting, but that's fleebay so who knows. Can you tell by the pics?

                                --- In mill_drill@yahoogroups.com, "wjhaasman" <brianomcp@...> wrote:
                                >
                                >
                                >
                                > Just a thought,Is the end mill a centercutting end mill? If not the tool will bog down and snap crackle pop. Your problem is not due to backlash either way.
                                >
                              • brianpimm@rocketmail.com
                                I ran another one today, increased the spindle RPM to 1600, feed rate to 2.1 IPM still plunged at .7 IPM I used plywood as a backer to stop the flex in the
                                Message 15 of 26 , Nov 26, 2012
                                • 0 Attachment
                                  I ran another one today, increased the spindle RPM to 1600, feed rate to 2.1 IPM still plunged at .7 IPM I used plywood as a backer to stop the flex in the middle of the part and it ate the bit just as bad as the previous one.
                                • Goran Hosinsky
                                  Hello, I have to remove rather a lot of steel for a couple of toolholders. I have no facility for sharpen endmills, getting new ones takes time as I have to
                                  Message 16 of 26 , Nov 27, 2012
                                  • 0 Attachment
                                    Hello,

                                    I have to remove rather a lot of steel for a couple of toolholders. I
                                    have no facility for sharpen endmills, getting new ones takes time as I
                                    have to order from abroad. I am thinking that the best policy is to take
                                    as deep cuts as my mill permits, the idea being that the wear of the
                                    cutting edge is a function of the number of cuts, a few heavy cuts wears
                                    the edges less than many light ones. The mill is manual.

                                    Am I right thinking this?

                                    Goran, Canary Islands
                                  • Robert Broughton
                                    Before you get to max depth of cut, you need to look at both rigidity and power at the spindle (it is about 50 to 70% of the motor s rated power) to make sure
                                    Message 17 of 26 , Nov 27, 2012
                                    • 0 Attachment
                                      Before you get to max depth of cut, you need to look at both rigidity and power at the spindle (it is about 50 to 70% of the motor's rated power) to make sure you can remove the amount of material for your setup. Then you will need to look at the material you are cutting. As part of the rigidity, you will need to use the largest diameter end mill you can use for the project (and that your machine can still drive) because the larger the diameter, the more rigid the tool bit will be. Another factor is the type of end mill you are using as HSS is able to deflect more than Carbide. Finally, the greater the depth of cut, the greater the end mill deflection to the point that the end mill will finally break.

                                      Being manual control, you probably want to err on the side of caution as you can inadvertently feed the machine faster than you were expecting.

                                      Hopefully this gives you an idea of what you are looking at in your question.
                                      Bob

                                      From: Goran Hosinsky <hosinsky@...>
                                      To: mill_drill@yahoogroups.com
                                      Cc: hosinsky@...
                                      Sent: Tuesday, November 27, 2012 1:13 AM
                                      Subject: [mill_drill] Bit life, another aspect

                                       
                                      Hello,

                                      I have to remove rather a lot of steel for a couple of toolholders. I
                                      have no facility for sharpen endmills, getting new ones takes time as I
                                      have to order from abroad. I am thinking that the best policy is to take
                                      as deep cuts as my mill permits, the idea being that the wear of the
                                      cutting edge is a function of the number of cuts, a few heavy cuts wears
                                      the edges less than many light ones. The mill is manual.

                                      Am I right thinking this?

                                      Goran, Canary Islands


                                    • Goran Hosinsky
                                      Well, as I work manually, all the different aspects reduce to what sounds and feel right when I do the cut, vibrations, sound of motor etc. I should perhaps
                                      Message 18 of 26 , Nov 27, 2012
                                      • 0 Attachment
                                        Well, as I work manually, all the different aspects reduce to what sounds and feel right when I do the cut, vibrations, sound of motor etc. I should perhaps reformulate my question:

                                        I do a cut with the maximum depth that feels right. If I then do two cuts, each with half the cutting depth of the first cut I will remove the same amount of material. Which way is less dulling of the cutting edges of the mill? Two cuts with half dept or one cut with full depth?

                                        Goran

                                        On 2012-11-27 10:00, Robert Broughton wrote:
                                         
                                        Before you get to max depth of cut, you need to look at both rigidity and power at the spindle (it is about 50 to 70% of the motor's rated power) to make sure you can remove the amount of material for your setup. Then you will need to look at the material you are cutting. As part of the rigidity, you will need to use the largest diameter end mill you can use for the project (and that your machine can still drive) because the larger the diameter, the more rigid the tool bit will be. Another factor is the type of end mill you are using as HSS is able to deflect more than Carbide. Finally, the greater the depth of cut, the greater the end mill deflection to the point that the end mill will finally break.

                                        Being manual control, you probably want to err on the side of caution as you can inadvertently feed the machine faster than you were expecting.

                                        Hopefully this gives you an idea of what you are looking at in your question.
                                        Bob

                                        From: Goran Hosinsky <hosinsky@...>
                                        To: mill_drill@yahoogroups.com
                                        Cc: hosinsky@...
                                        Sent: Tuesday, November 27, 2012 1:13 AM
                                        Subject: [mill_drill] Bit life, another aspect

                                         
                                        Hello,

                                        I have to remove rather a lot of steel for a couple of toolholders. I
                                        have no facility for sharpen endmills, getting new ones takes time as I
                                        have to order from abroad. I am thinking that the best policy is to take
                                        as deep cuts as my mill permits, the idea being that the wear of the
                                        cutting edge is a function of the number of cuts, a few heavy cuts wears
                                        the edges less than many light ones. The mill is manual.

                                        Am I right thinking this?

                                        Goran, Canary Islands



                                      • wjhaasman
                                        ... The pics look like they are center cutting.Perhaps try to ramp in rather than plunge.
                                        Message 19 of 26 , Nov 27, 2012
                                        • 0 Attachment
                                          --- In mill_drill@yahoogroups.com, "brianpimm@..." <brianpimm@...> wrote:
                                          >
                                          > They were advertised as center cutting, but that's fleebay so who knows. Can you tell by the pics?
                                          >
                                          > --- In mill_drill@yahoogroups.com, "wjhaasman" <brianomcp@> wrote:
                                          > >
                                          > >
                                          > >
                                          > > Just a thought,Is the end mill a centercutting end mill? If not the tool will bog down and snap crackle pop. Your problem is not due to backlash either way.
                                          > >
                                          >
                                          The pics look like they are center cutting.Perhaps try to ramp in rather than plunge.
                                        • brianpimm@rocketmail.com
                                          ... The software I use doesn t have the ability to ramp. and I m not sure I could hand code that much... What ramp angle should I try if I go that way.
                                          Message 20 of 26 , Nov 27, 2012
                                          • 0 Attachment
                                            > The pics look like they are center cutting.Perhaps try to ramp in rather than plunge.
                                            >


                                            The software I use doesn't have the ability to ramp. and I'm not sure I could hand code that much... What ramp angle should I try if I go that way.
                                          • carlmciver
                                            I ve only been paying peripheral attention to this thread, so if I missed the suggestion previously, I apologize. Have you looked at roughing end mills for
                                            Message 21 of 26 , Nov 27, 2012
                                            • 0 Attachment
                                              I've only been paying peripheral attention to this thread, so if I missed the suggestion previously, I apologize. Have you looked at roughing end mills for first pass removal of lots of metal? These things are a real time saver for me.

                                              --- In mill_drill@yahoogroups.com, Robert Broughton <r.broughton@...> wrote:
                                              >
                                              > Before you get to max depth of cut, you need to look at both rigidity and power at the spindle (it is about 50 to 70% of the motor's rated power) to make sure you can remove the amount of material for your setup. Then you will need to look at the material you are cutting. As part of the rigidity, you will need to use the largest diameter end mill you can use for the project (and that your machine can still drive) because the larger the diameter, the more rigid the tool bit will be. Another factor is the type of end mill you are using as HSS is able to deflect more than Carbide. Finally, the greater the depth of cut, the greater the end mill deflection to the point that the end mill will finally break.
                                              >
                                              > Being manual control, you probably want to err on the side of caution as you can inadvertently feed the machine faster than you were expecting.
                                              >
                                              > Hopefully this gives you an idea of what you are looking at in your question.
                                              > Bob
                                              >
                                              > ________________________________
                                              > From: Goran Hosinsky <hosinsky@...>
                                              > To: mill_drill@yahoogroups.com
                                              > Cc: hosinsky@...
                                              > Sent: Tuesday, November 27, 2012 1:13 AM
                                              > Subject: [mill_drill] Bit life, another aspect
                                              >
                                              >
                                              >  
                                              > Hello,
                                              >
                                              > I have to remove rather a lot of steel for a couple of toolholders. I
                                              > have no facility for sharpen endmills, getting new ones takes time as I
                                              > have to order from abroad. I am thinking that the best policy is to take
                                              > as deep cuts as my mill permits, the idea being that the wear of the
                                              > cutting edge is a function of the number of cuts, a few heavy cuts wears
                                              > the edges less than many light ones. The mill is manual.
                                              >
                                              > Am I right thinking this?
                                              >
                                              > Goran, Canary Islands
                                              >
                                            • Corey Renner
                                              Goran, your theory is correct, and under CNC it is pretty easy to take advantage of this effect, however, when manual milling you normally do not have very
                                              Message 22 of 26 , Nov 27, 2012
                                              • 0 Attachment
                                                Goran,
                                                your theory is correct, and under CNC it is pretty easy to take advantage of this effect, however, when manual milling you normally do not have very precise control of your feed-rate and the efficiency gains made by engaging more of the tool are usually undone by the chatter&vibration caused by deep cuts and imprecise feeds.

                                                cheers,
                                                c

                                                On Tue, Nov 27, 2012 at 1:13 AM, Goran Hosinsky <hosinsky@...> wrote:

                                                 the idea being that the wear of the
                                                cutting edge is a function of the number of cuts, a few heavy cuts wears
                                                the edges less than many light ones. The mill is manual.

                                                Am I right thinking this?

                                                Goran, Canary Islands

                                              • Robert Broughton
                                                Under that setup, the single cut will be less dulling as long as you are removing the chips cut and not doing any re-cutting of swarf. Additional benefit would
                                                Message 23 of 26 , Nov 27, 2012
                                                • 0 Attachment
                                                  Under that setup, the single cut will be less dulling as long as you are removing the chips cut and not doing any re-cutting of swarf. Additional benefit would be to use a roughing cutter and some coolant mist, spray, or flood. Sometimes when you take deeper cuts, the swarf will not clear as well as a more shallow cut (depending on the cut profile and pocketing.)
                                                  Bob


                                                  From: Goran Hosinsky <hosinsky@...>
                                                  To: mill_drill@yahoogroups.com
                                                  Sent: Tuesday, November 27, 2012 3:34 AM
                                                  Subject: Re: [mill_drill] Bit life, another aspect

                                                   
                                                  Well, as I work manually, all the different aspects reduce to what sounds and feel right when I do the cut, vibrations, sound of motor etc. I should perhaps reformulate my question:

                                                  I do a cut with the maximum depth that feels right. If I then do two cuts, each with half the cutting depth of the first cut I will remove the same amount of material. Which way is less dulling of the cutting edges of the mill? Two cuts with half dept or one cut with full depth?

                                                  Goran

                                                  On 2012-11-27 10:00, Robert Broughton wrote:
                                                   
                                                  Before you get to max depth of cut, you need to look at both rigidity and power at the spindle (it is about 50 to 70% of the motor's rated power) to make sure you can remove the amount of material for your setup. Then you will need to look at the material you are cutting. As part of the rigidity, you will need to use the largest diameter end mill you can use for the project (and that your machine can still drive) because the larger the diameter, the more rigid the tool bit will be. Another factor is the type of end mill you are using as HSS is able to deflect more than Carbide. Finally, the greater the depth of cut, the greater the end mill deflection to the point that the end mill will finally break.

                                                  Being manual control, you probably want to err on the side of caution as you can inadvertently feed the machine faster than you were expecting.

                                                  Hopefully this gives you an idea of what you are looking at in your question.
                                                  Bob

                                                  From: Goran Hosinsky <hosinsky@...>
                                                  To: mill_drill@yahoogroups.com
                                                  Cc: hosinsky@...
                                                  Sent: Tuesday, November 27, 2012 1:13 AM
                                                  Subject: [mill_drill] Bit life, another aspect

                                                   
                                                  Hello,

                                                  I have to remove rather a lot of steel for a couple of toolholders. I
                                                  have no facility for sharpen endmills, getting new ones takes time as I
                                                  have to order from abroad. I am thinking that the best policy is to take
                                                  as deep cuts as my mill permits, the idea being that the wear of the
                                                  cutting edge is a function of the number of cuts, a few heavy cuts wears
                                                  the edges less than many light ones. The mill is manual.

                                                  Am I right thinking this?

                                                  Goran, Canary Islands





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