Cutting tolerance on an X3 CNC

[archerks]

I just finished up my X3 CNC conversion and did some test cutting in some MDF and aluminum. When cutting a 1 inch circle in the MDF, the Y axis diameter measures .998 and the Z axis diameter measures .989, a difference of .009 inch. The aluminum had a difference of .012 inch. Is the what I should expect or should I be able to get a perfect circle? What do I look for to correct it? Do I need to put a backlash setting in Mach 3? Both motors are set in Mach 3 at 10160 steps based on....
200 motor steps
x 10 driver micro steps
=2000 steps per revolution
/ 5 ball screw is 5mm
=400 steps to go 1 mm
*25.4 convert from 1mm to 1inch
=10160 steps per inch entered in Mach 3

[dneisler]

What conversion did you use? I used a CNC Fusion one, tweak my steps . inch and on my X and Y and I getting backlash of like .0002 Seems really good. I have tweaked in my Z yet.

[cyclestart]

Originally Posted by archerks Is the what I should expect or should I be able to get a perfect circle?

Are the ball screws preloaded? My X2 won't cut a "perfect" circle, but it will hold .001" on a hole that size.
Are there noticable jogs at 90/180/270 positions? This would indicate backlash.

If you are using rubbery couplers like lovejoys it is also possible to induce some of this behaviour with extremely tight gibs. Loose gibs are no help either.

What do I look for to correct it?

Place a dial indicator on that part of the table and take 2 measurements. One measurement for backlash and another to test that a 1" command moves exactly 1". The backlash measurement will likely provide the answer.

Do I need to put a backlash setting in Mach 3?

Maybe. Need to measusre the true backlash first and find the source. Best to remove as much mechanically as possible. Software compensation in the .010" range is an ugly kludge.

[thackman]

Archerks,
I have a Syil SX3 that I purchased already converted and I have the same results. I don't have backlash compensation on (you shouldn't need it if you have ball screws) but that's not the source of my issues. Try measuring your repeatability with an indicator.

Your issues could be caused by either backlash or other ridigity issues (including spindle) but I suspect it is ridgity in the head carriage. When I use a DTI on the table I get .0002" repeatability on the X and Y axis and .0005" on the Z axis. I have the gibbs on X and Y axis adjusted perfectly. I get 60ipm rapids and I can push, pull, and twist the table and there isn't any measurable slop.

The Z axis is just the opposite. With the head in the middle of the z travel I can put 20 lbs of force on the head in the X direction and it deflects .010". I've worked called tech support a few times and even put in a replacement Gib and it hasn't solved the problem.

If you have a backlash issue then it should be relativly consistant regardless of the material that you are cutting. Since your distortion increases with the hardness of the material I suspect that you either have a miss adjusted gib somewhere or an issue with the Z axis itself.

Try running your code several times on the same part and see what you get.

As a temporary solution when cutting AL I've been resorting to roughing at .005" oversize, a semi-finish pass to size and then three finish passes at the exact size. Plastic parts require two finish cuts and the mill chatters so much it's impossible to cut mild steel.

I'm waiting for a replacement Z-axis carriage to arrive. If anyone else has any other solutions I'd love to hear it.

[Crevice Reamer]

10,160 steps per inch is only a starting point. Try measuring a straight 1" cut on both X and Y directions--Then tweak the steps per inch up or down to adjust and try again. When you can cut a 1" straight cut in both axes that IS 1" long, then try to cut a 1" SQUARE. If square ok, try the circle again.

Once the SPI is set properly, any circular error will either be backlash or Z deflection. Measure and eliminate/compensate backlash then try square/circle again. Now any error could be Z deflection.

CR.

[Crevice Reamer]

By the way: You DO know there is a Z gibb adjusting screw on top--And ANOTHER on the bottom, right?

CR.

[philbur]

I don't understand, why would you need to fiddle with the steps per inch. It's simple math and surely there is only one right answer.

The problem is surely backlash somewhere in the system and should be easily traced with a DTI. I think backlash comp is a fudge and should be the last resort.

Just some thoughts and opinions
Phil

Originally Posted by Crevice Reamer 10,160 steps per inch is only a starting point. Try measuring a straight 1" cut on both X and Y directions--Then tweak the steps per inch up or down to adjust and try again. When you can cut a 1" straight cut in both axes that IS 1" long, then try to cut a 1" SQUARE. If square ok, try the circle again. Once the SPI is set properly, any circular error will either be backlash or Z deflection. Measure and eliminate/compensate backlash then try square/circle again. Now any error could be Z deflection. CR.

[wwendorf]

I've got a friend who run's a machine shop, and if he needs a hole done, he just does it with a boring bar. He says that on a mill its the only real good way to get a perfect hole as a mill just can't do it on it's own with an endmill. I have the SX3 and i've been following his advice and it works for me. Trying to mill a hole is just too imprecise.

Wade

[tauntdesigns]

Yea, I always bore holes after roughing them out with an end mill. Sometimes with holes that are for clearance only(no mating parts) I'll finish them with an end mill. I'll rough out the hole and then run a finish pass, then a spring pass at a higher feedrate. They usually come out pretty close(within .002").

Is the O P roughing his holes before a finish pass or just cutting to size in one pass?
What size cutter? DOC?
Backlash?

Did I miss this info?
Jack

[philbur]

That depends on how precise you need the hole and how well your mill is set up. Also boring a hole to size is a bit of a fiddly process and takes time setting up and checking.

Phil

PS: I think the OP may have been milling the circles as a check of mill performance, 0.012" out of round on a 1" hole needs looking at.

Originally Posted by wwendorf Trying to mill a hole is just too imprecise. Wade

[archerks]

Found a lot of the problem. When I set up the Mach3 for a 1 inch movement, my backlash was being put into it since I set it up using a test right, then test left, then test right, etc. So I always had the back lash in the 1 inch movement which is fine if you are going to only move 1 inch EVERY time. Thats why my .1 inch movement were off. With backlash enabled in Mach3 at .006 inch, I am now moving 1 inch and .1 inch movements correctly. Haven't tried cutting a circle yet to see what happens.
Thanks,
Dave