Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: SailFl on September 12, 2009, 08:03:56 PM
-
I am having a problem with chatter on my cuts. There are members of another forum were I built my machine that think the chatter is caused by the kernal not being set at a high enough rate or that the Dell Pentium III machine is having a problem processing the files. I ran the test program that comes with Mach and the computer passed the test. Is there anther way to check for kernal speed or a computer problem with regards to the kernal.
I am starting to question that it might be the computer. I am cutting a diamond shape that has 2" length legs with the diamond sitting on a point so the cuts are at a diagonal. I am cutting solid surface material with .5" O Flute End Mill. When I cut this small pattern, there is considerable chatter. Tonight I cut a small 45 degree 4" cut and there was chatter marks but the cut was smooth.
The last cut makes me wonder if I am having a computer problem and the bad chatter I am getting is the result of the computer not being able to process the cut commands and is skipping.
I would appreciate some input or suggestions.
Thanks
-
more likely to be mechanical issues, if you do a straight cut along an axis do you see problems?
Hood
-
Hood,
After the two test I just described, I don't think it is mechanical. The diamond cuts are at a 45 degree angle and the chatter is bad at a slow 35 IPM. The 4" 45 degree had chatter marks but the cut was smooth.
So I don't think it is chatter. Straight cut are okay.
I have been over my machine and it is tight.
-
What kernel do you have it set at and what are your velocities and steps per unit?
Hood
-
What kind of drives are you using? Can you post a video? does the machine sound rough?
Also, why are you cutting so slow. With a sharp spiral bit, you can easily cut solid surface at 300ipm.
-
My Opinion... this is a CV Issue. I have been noticing the same issues with a large Foam Band saw I recently built. I have tried playing around with the CV settings but optimize this but IMHO, due to the fact that the machine is large and has a lot of mass (therfore really slow accels) there is a large speed differential between my X & Y axis (X is belt driven & Y is lead screws) there is simply not enough ability to equalize the CV in order to compensate for one axis being so much slower.
I wish some one had an answer to this. Just my $.02
Sid
-
Sid,
I think you are on to some thing with the CV issue. I lookd over the document on CV and I wish the author would have included some number examples for settings. Also it would be nice to know what the values mean.
The default for Distance Tolerance is 180 and I set my to 100. I also set my Stop CV Angle to 90. My look ahead to 200.
I recut my test Diagonal cuts at 35 and 70 IPM and things were smooth but when I cut at 100 IPM my chatter was back.
So I think that these parameters are making an impact.
If any one has some experiencing with these setting please post your settings or what your experience has been.
Ger21: I am cutting at these speeds because I am getting chatter. I would love to be able to cut at 300 IPM with no chatter. But chatter doesn't go away when you cut faster, it only cuts faster. At least that is what I am experiencing.
I will be happy to report my experience and settings when I have done some more testing.
Thanks for the suggestion.
-
Just for 'Grins'- perhaps you can try to cut in Exact Stop mode and see if you are able to reach your 300 IPM target and NOT get the chatter? This eliminates the chatter for me but changes my cut in an undesireable way so I am kinda locked into using CV.
-
If you have cutter chatter I don't think you will find it is a software problem. Chatter is generated from a component NOT rigid enough to hold it in place. It flexes then jumps back into place and flexes ,etc,etc.
Could be DOC too large for the machine or material or too fast feedrate for the cut. OR spindle speed too slow for cutter specs and feedrate.
I have never seen software CAUSE tool chatter in itself. I always had to help it occur (;-)
Just some thoughts, (;-) TP
-
VMAX-
Respectfully, I have to disagree.
If you have a machine with a lot of mass and the accel rate is set too high then a rapid acel will cause your machine to jerk, then this will result in what I am interpreting as chatter. Perhaps I am mistaken or using the incorrect terminology. If so, I apologize in advance.
While what you say is partially true because the "chatter" it is due to the mass limitations of the machine, the software allows us to slow down our accels to a point where things become smooth.
CV takes this away from us to a certain extent because Mach now want to control velocity on it's own terms (well sort of) but we certainally do not have the same speed/accel control as in exact stop mode. If 2 or more of your axis are dissimilar in terms of their tuning profile, you will see Mach slowing down one axis a lot more rapidily than the other in an attempt to keep things "Constant" this struggle can result is Jerky motion (exactly what CV is supposed to prevent). CV is a double edged sword under these circumstances.
Sid
-
VMAX-
Respectfully, I have to disagree.
If you have a machine with a lot of mass and the accel rate is set too high then a rapid acel will cause your machine to jerk, then this will result in what I am interpreting as chatter. Perhaps I am mistaken or using the incorrect terminology. If so, I apologize in advance.
While what you say is partially true because the "chatter" it is due to the mass limitations of the machine, the software allows us to slow down our accels to a point where things become smooth.
CV takes this away from us to a certain extent because Mach now want to control velocity on it's own terms (well sort of) but we certainally do not have the same speed/accel control as in exact stop mode. If 2 or more of your axis are dissimilar in terms of their tuning profile, you will see Mach slowing down one axis a lot more rapidily than the other in an attempt to keep things "Constant" this struggle can result is Jerky motion (exactly what CV is supposed to prevent). CV is a double edged sword under these circumstances.
Sid
"If you have a machine with a lot of mass and the accel rate is set too high..." - And how is that a software problem?? Is the software supposed compensate for you setting the acceleration too high?
I agree with Terry. This is a machine problem, not a software problem.
Regards,
Ray L.
-
Hey Ray,
Thanks for chiming in.
Perhaps I could have been more clear. In my previous post, I was using accel being set to high as an example of how chatter could occur.
Of course software can not compensate for incorrect settings. However, it has been my experience when Mach is runing in CV, the speed blending which occurs to create the 'Constant' somehow overides the acel parameters in tuning in its attempt to run every axis at the same speed. This causes undesirable effects.
Yes- I could adapt my machine so that the Axis were more similar in terms of the tuning profile but, it sure would be nice (read easier) to have some more control over CV (maybe like a CV axis scalling factor) to help smooth things out.
Sid
-
Hey Ray,
Thanks for chiming in.
Perhaps I could have been more clear. In my previous post, I was using accel being set to high as an example of how chatter could occur.
Of course software can not compensate for incorrect settings. However, it has been my experience when Mach is runing in CV, the speed blending which occurs to create the 'Constant' somehow overides the acel parameters in tuning in its attempt to run every axis at the same speed. This causes undesirable effects.
Yes- I could adapt my machine so that the Axis were more similar in terms of the tuning profile but, it sure would be nice (read easier) to have some more control over CV (maybe like a CV axis scalling factor) to help smooth things out.
Sid
Sid,
I don't believe that's true, and it's easy enough to test - set the accel on one axis artificially low. I think you'll see that ALL "blended" operations slow down accordingly. If Mach ignored the accel on even one axis, we'd having servos faulting and steppers losing steps randomly, but that does not happen, even when there are wide disparities in the capabilities of different axes. One of my machines runs an accel of 125 on two axes, with a max speed of 270 IPM. The third axis has an accel of only 5, and a max speed of 30 IPM, and those settings are right on tha hairy edge of what it's capable of without losing steps. On blended moves, the thing crawls, because of the third axis, but it does not lose steps.
Regards,
Ray L.
Regards,
Ray L.
-
OK, I'm not workin today but I'll give it a go tomorrow.
-
Actually the CV helps to maintain a constant feedrate AND that is a desired effect when milling. IT will make a smoother more consistant cut with proper CV. AND the mach cv is normally BEST left in the default state with 200 lines look ahead(;-)
THe jerk is caused by improper axis tuning for the machine specifications OR a non ridgid machine that creates the jerk on axis reversals.
Mass has little to do with it and rigidity is not always a function of mass. Mass can help you OR hurt you depending on the design of the machine and WHAT you are trying to do with it.
SO back to the software chatter (;-) For the most part I don't think so.
Cutter chatter is normall a function of the machine process verses the rigidity/mass ratio of the machine AND the proper cutter selection and feed/speeds and DOC, tool length ratio. The list goes on and on. Get it right and smooth as glass get it wrong and CHITTY CHITTY bang bang.
R what you are calling chatter is not what I call chatter(;-) It could be Gouging is what you are seeing???
(;-) TP
-
Based on my reading of the CV Notes, I made the following changes to my Mach configuration:
CV Look Ahead 200 lines.
CV Dist Tolerance 100 units
Stop CV on angles > 90 degrees.
After restarting, I cut my Diamond at both 35 and 70 IPM and the cuts were smooth. But when I cut at 100 IPM, I still had chatter.
I have since changed the CV Dist Tolerance to 50 Units. I recut the Diamond at 100 IPM and I still had the same amount of chatter.
My X and Y motors are tuned to 450 Velocity and 30 Acceleration and Z is 150 / 10.
I would like to hear more from those that have some experience with these configurations changes.
For those that don't think software has an effect. Yes, it does not cause chatter but it affects the way the machine operates. For example if you have CV set and you cut a rectangle and a very high say 400 IPM, you will get rounded corners. Changing to Stop will give you square corners.
-
WE never said it would NOT effect how your machine ran. But it has little to no effect on chatter.
What is your spindle speed? The faster you try to cut the faster the spindle speed has to be to maintain the proper chip load.
(;-) TP
-
Sail, give us more information on the material you are cutting, the axial and radial depth of cuts, the type of cutting tool and tool holder you are using, how far the cutting tool is extended from the holder, what spindle RPM you are using and what type of machine you have. This will make it easier to figure out what is causing the chatter.
Paul T.
-
As stated by Vmax & Titchener above, I agree that you are probably over stretching the Feed rate due to low RPM. Also, with such small sizes I wonder why 1/2" EM ? & O flute ? There has been no mention as to the work holding or the remains of the material during the So-Called Chatter. I would suspect that what you are calling Chatter is not really what or where your describing. Deflection might be in play as well. Or even dull cutter induced surface character. I didn't see what material your cutting, could be surface work hardening, or grain tearing, or chip re cutting ! It could be any number of things involved here and without a visual or better description, then you could be easily leading all who try to help, astray ! And you end up without a viable solution.
-
Paul,
I am cutting .5" solid surface material. I am using a .25" Solid Carbide UpCut Spiral O Flute Onsrud 63-775 bit. I am cutting .125" with each pass at 90 degrees to the surface of material. I am using a Milwaukee 5625 router in my machine and it has a standard .25" collet. The bit has a CEL of .75" and only the cutters are showing out of the collet. The router is set at 14,000. The machine is a MechMate.
I think I understand and have answered all your questions.
Thanks for you help.
Cruiser,
I am cutting with a bit that recommended by Onsrud for solid surface material. I need to use .25" bit for details.
The little piece missing is from a tab that broke off.
-
Use a 1/2" upcut 2 flute spiral. Also, measure the tool runout and make sure it's not excessive. I cut solid surface with these, with very good results. http://www.vortextool.com/index.cfm?fuseaction=category.display&category_id=13
-
Paul,
I am cutting .5" solid surface material. I am using a .25" Solid Carbide UpCut Spiral O Flute Onsrud 63-775 bit. I am cutting .125" with each pass at 90 degrees to the surface of material. I am using a Milwaukee 5625 router in my machine and it has a standard .25" collet. The bit has a CEL of .75" and only the cutters are showing out of the collet. The router is set at 14,000. The machine is a MechMate.
I think I understand and have answered all your questions.
Thanks for you help.
Cruiser,
I am cutting with a bit that recommended by Onsrud for solid surface material. I need to use .25" bit for details.
The little piece missing is from a tab that broke off.
You are running that very near the top end of it's recommended chip load, which will not always work well. Also, what I see in the picture is not what I would call "chatter", but rather indications of an over-loaded tool - you're feeding too fast, and the tool is flexing. Either reduce feed, or increase RPM, and I bet it works fine. I'd bet going to a stiffer tool (1/2", for example) would also help, as it would increase your SFPM, and allow a heavier chipload, albeit with more spindle power and higher feed force required.
Regards,
Ray L.
-
YEP I am in agreement with Ray on this one > Looks like the chip load is too high for conditions and the cutter is being pushed over when the flutes get loaded up and can no longer cut. THen the chips clear out and start cutting again. Either UP the spindle speed, slow the feedspeed or go to a 2 flute high helix cutter.
Hope that helps, (;-)TP