# Frustrating accuracy issue

I’ve run into an issue with my x-carve where designed objects are smaller than they should be by ~2/64ths in x and y directions. If I draw a 2" square in easel, and make sure it is set to outside cut and it’s short in both directions. I don’t hear anything strange when cutting, I don’t think I am missing steps. All tests were done in MDF w/ 1/8" 2 flute upcut but @ 40" feed rate.

• I’ve calibrated both the x and y directions to be accurate within 1/128th" over 30" by using UGCS (g0 x30). I’ve checked this twice. Maybe use G1 x30 f40?
• I’ve played with the stepper motor voltage pots. I’m pretty sure I have them dialed in correctly.
• I’ve adjusted the voltage output of the main power supply from 24.3 to 24.0. - I saw in one video incorrect voltage could cause missing steps.
• I’ve ensured the belts are tight, but not too tight.
• I’ve verified the v-wheels can barely be spun by one finger - I’m pretty strong, so the average person could move it with 2 fingers.

This inaccuracy is very consistent on both axis. I even wrote a gcode file to cut a square to see if Easel was the issue without any difference. I have a older x-Carve pre-2016 with the g-shield. I’m using a dewalt 611 for my spindle and I’ve stiffened the gantry. Z axis is rock solid.

Any help is much appreciated!

Is the discrepancy equal for a 2x2" and 5x5" square?

If the amount off is equal, its due to backlash.
Backlash is the amount of motion the machine need to do before motion in the opposite direction take place.

During your calibration routine you also need to make sure backlash isnt a factor in the calculation.
You achieve this by jogging say to the far left side, then do a small jog in the opposite direction - then measure a single long jog with a ruler.

Aslo try a single slot carve for the 1/8" and measure the path width, is it exactly 1/8" or a smidge off?

1 Like

Have you calibrated your steps per millimeter after checking for belt tightness? I’ve found that you can get pretty close but these machines aren’t really capable of extremely tight tolerances. +/-.010 is about what you can expect realistically. You need a real accurate measuring device to do this well.

See post 3 here:

Calibrating my X-carve 1000 - X-Carve - Inventables Community Forum

Or an oversized endmill. Does the same issue occur with a different endmill?

True

@NateStovall:
The Xcarve presicion is stated to be, on a fine-tuned machine, in the 0.7-0.13mm range

Not only the diameter of the bit, but also the precision of the collet.
If the bit is off slightly, and the collet this will accumulate the error.

Indeed, this is called run-out.
To factor in this component a single slot carve should be performed and its width measured, this will give you a “true” diameter to use.

Yes, I’ve calibrated this a half-dozen times. And again if I mess with the belt tension.

I’ll try the backlash test tonight. I’m assuming I move 15" right then .25 left then another 15" to the right?
Yes, the bit cuts a 1/8" wide slot. Thx!

Yes, it’s aboutthe same with a 1/4" bit. I also verified that the bits are 1/8" and 1/4". Damn the metric system!

I scratched run-out off the list because the slot is exactly 1/8" wide - the same as the bit. I’m using a high-quality collet, not some cheap crappy one. At 10,000 RPM I don’t screw around with cheap tools or bits.

Say you want to check the X-axis:

• Jog to the far left side, then one small jog towards the right in order to take out backlash.
• Measure in the right direction, one large jog. This is your actual travel you´d use for step/mm calculations. What do you get?

Measuring your 1/8" to carve exactly 1/8" is good because then you have ruled out that possibility from the mix

Have you tried a 2x2" and 10x10" square test?
Is the discrepancy equal between the two?

How rigid is your machine? There are a few things needed for accuracy, rigidity, sharp tools, proper direction of cut for final pass, no backlash, properly trammed z axis, tool tooth engagement, speeds and feeds and many other things that relate to accuracy.

Run a scratch test on your job with a liner bit or a super fine graphic pen. Then measure results. Something with no drag. If the dimensions are correct, then it’s structural issue, not electrical or code.

I bet it’s machine twist and deflection. I had the same problem - constantly cutting slightly under size. When I put a .01 pen in and ran the machine as basically a plotter, dimensions were correct.

Once I replaced the Z and reengineered the X/Y to stiffen the whole thing up, it gained the missing accuracy.

It’s a flimsy machine, poorly designed, particularly for the 500-1000mm sizes.

Overall, it’s not a 25k machine. It’s never going to be 100% accurate. I say this after driving myself insane, trying to make it be what it is not.

I did myself a favor and learned to love it 98% of the time and forgive it when it is not what it is not.

1 Like

Sorry for the late reply. I get very frustrated and before I smash the damn thing I work on other stuff for a while. I (mainly) bought this machine to do inlays. If it is off by 1/64th of an inch here and there they are not going to look good enough.

I have stiffened the X and Y axis on my machine.

Today I went through the entire machine. Checked all bolts to make sure they are not loose. Belt tension and potentiometer settings. V-wheel tightness. Verified the machine is square in all directions. Last week I surfaced the wasteboard to make 100% sure the bit is perpendicular to the surface. Re-Calibrated the machine. Used G0 and G1 commmands to calibrate – just in case the machine acts a little differently between fast and normal travel. I’m dead accurate over 30" of travel.

I measured no backlash in the X or Y directions. The bit is basically brand new & still sharp enough to mark my fingernail.

I’ve tried 2" 3" 4" & 5" squares, and they are all off by 1/64th of an inch… Always smaller than they should be. So the 5" test measures 4 63/64 by 4 63/64ths. The 2" test measures 1 63/64 by 1 63/64ths. This is consistent across the entire side. So the carvings are dead straight along the X and Y Axis - the box isn’t twisted. In Easel, I’m drawing a box, and setting it to cut “outside the line”

What’s vexing me is that is always off by a 64th regardless of the size of the cut. It would make more sense for me if it was off .01" on a 1" square and .1" on a 10" square. It’s always a 64th of an inch. I can’t simply change the \$100 and \$101 values in the machine’s firmware to make up the difference.

NEXT:

• I’ll tell Easel to cut inside the line and see if it makes any difference.
• I’ll write a Gcode program to cut squares and use GCS to run it.
• I’ll try TravisBrown1’s idea of using a pen to test. The smallest I have is .05mm
• Bite the bullet and try a test inlay and see how fugly it looks.

A huge THANK YOU to the community for giving me a hand. I’ll post my results.

You have to adjust the \$101 and \$100 settings multiple times to get more accurate, but there’s a point where you can’t go any further due to the limitations of a hobbiest machine. A machine with a solid framework, ballscrews , and supported linear guides would get you closer, but it’s still not going to be perfect.

That is indicative of some degree of tool/machine deflection and some component of backlash.
There is not a single CNC-machine out there without some component of backlash present.

Have you measured the actual width of the bit by carving a single slot and measure width?
This give you a “true” diameter which also take into account run-out of the router. Thou’s are lost here aswell.

Regarding inlays, are you using straight bits or V-bits?
V-bits offer some advantages in terms of material inconsistencies that might be easier to deal with.

1 Like