Need help with cutting accuracy!
So up until now I've been mostly tinkering with the cuts I’ve made. Not really paying too much attention to the size of the cuts. Mostly just getting used to programming and running this machine. Well, I’ve gotten to the point where I’m pretty comfortable with programming and the machine. I’m also at the point where I have to make some pretty exact hole sizes (within .0015” or so) for some parts that need to be press fit. I’m using Mastercam. Attached is a pic of the first prototype I made.
So here’s the problem: I went to create a .786” dia by .5” deep hole in 6061 aluminum. I was doing this by ramp machining it. 3% per pass, at a feedrate of 12, 4100 rpm, climbmilling. The plan was to rough it out using a 3/8” 3 flute flat endmill for aluminum cutting and finish with the boring head. When I checked the dia after the rough cut, it was .810”. Way oversize. I checked the program over and over, recreated it and even tried different sizes. Each time the hole is being cut from .015-.035” oversize. The sizes were never this far off, otherwise the other components in the assembly I was making would not have fit.
I checked the runout on the spindle, the tool holder (TTS collet), and the end mill shank, and nothing more than .001” from what I could see. Certainly not something that would throw it that far off. I also did a really slow manual plunge cut of 2 brand new 3/8 center cutting endmills, one rougher and a finish endmill. Just to see if maybe there was something in the program that was screwed up. Tried 5 cuts and the dia ranged from .383 - .410”. I spent about 6 hours yesterday chasing this problem and have no idea what to check next or what to do. I’m dead in the water until I could figure this out. Why is the accuracy so far off. One thing to mention, when I first got the machine the z axis would drift down an inch or 2 when I shut it off. It doesn’t do that now. I’ve only got a handful of hours of actual machining time on the machine so far. Any suggestions on what is causing this and how to fix it? Thanks for your help.
Rob in CT
Similar Threads:
Last edited by 98vert; 08-15-2007 at 11:23 AM.
Rob, Nices parts.
If you can put your Mastercam file too, I can take a loof at it.(I know Mastercam very well). As I looked at your code, I'd see that your code is linear. You should use the filter option in Mastercam to get 3 axis arcs. I can't understand how you can get .386"-.410" passes with a 3/8 end mill. Did you measured your end mill diameter? Does your .810” hole is perfectly round?
Would it make sense to try the same sort of cutting using one of the Mach wizards as a test? If that comes out to size, you can eliminate the mill as the source of error and focus on the CAM side.
Mike
Hi Rob,
I just looked at your program and I believe I have found at least part of your problem:
The numbers don't add up correctly, the last ramp in your program ends at:
X-.2035Y-.0286 Z-.1
then the next line is
G3X.2035Y-.0286R.2055
The R value needs to be the same as the movement in this case, you have a .004 total difference of diameter between the R value and the actual movement you are trying to achieve. What is happening is you are getting a larger radius in a shorter distance, so you are actually creating an out of round condition. You could try this instead:
X-.2035Y-.0286Z-.1
G3I.2055
This will give you a complete circle with a radius point in the X plus direction.
Sean
CutViewer shows the supplied gcode to cut correctly. The toolpath makes a 1.5 turn spiral down, then a half turn at full depth, then a small arc to put the cutter on the Y axis, then a final half turn at full depth to produce a flat bottom.
Also (2 * .2055 radius) + .375 cutter diameter = .786 hole diameter so mathematically it jives.
I know the PCNC software (customized Mach) to accurately render gcode (I am using PCNC3,) so the out-of-round problem must be mechanical.
Best regards,
Randy
Rob, my machine did that for a while, it seems in cooler weather, and I adjusted the Z axis gib a couple of times. But the machining itself has always been fine, good surface finish, etc. so I just got to putting a length of 2x2 under the spindle nose when I powered down the machine, but it hasn't drifted down for a couple months now. My Tormach is in the garage ("California basement") which can get pretty hot (but it helped a lot when I installed an insulation kit on the sheetmetal garage door...) so I'll see if the drifting down returns with cooler weather.Originally Posted by 98vert
But I don't expect the drifting down alone to be a cause of your problem.
Nice looking piece, Rob. It looks like all the sides are contoured. How did you hold it while machining? That's my part of the learning curve now--how to hold more contoured pieces while I machine them...
Best regards,
Randy
Hey Randy,
I don't mean to be rude but the finish position of X-.2035 plus the X.2035 from the nex line equals .407 and .407+.375=.782 not .786 so it can't be correct with the R.2055. To be correct either both of the X numbers need to be .2055 or the R value needs to be .2035.
Sean
Rob,
Try these numbers, I have posted out a program using Sprutcam and am attaching it to this post.
Sean
Sean, you're not being rude, just a little inaccurate in your calculation.Earlier you pointed out
The spiral ramp ends a little above the Y axis on the negative X side (the Y value is actually positive in the gcode), but at the correct radius. Pythagoras will clarify sqrt(-.2035^2 + .0286^2) = .2055 Then the first G3 makes a half circle to just below the Y axis on the positive X side, but again at the correct radius, then the second G3 makes a little arc to bring the toolpath to the positive Y axis, then the last G3 makes a not-quite-half circle back to just above the negative Y axis. But all are at the correct .2055 radius from the circle center.
The original gcode as supplied is OK. Not exactly how I'd have done it, but OK mathematically.
Best regards,
Randy
Last edited by zephyr9900; 08-19-2007 at 04:26 AM.
Yes Randy I was incorrect and I apologize. I did miss the Y+ versus the Y-, I now digress.
Not a problem, Sean. I actually took the lazy way myself and viewed the toolpath in CutViewer Mill (which does recognize the final hole to be round and will give the diameter) and saw that it looked OK, then I went back and analyzed it. CutViewer is a great tool for debugging problems when I hand-write gcode too.
Best regards,
Randy
Posting Permissions
Reply with Quote