Machine accuracy

Latest round of testing and even more confusion. I did a couple of different preliminary test cuts, ultimately finishing with a 1" square centered in a 2" square. Had two copies of that configuration and cut one as a pocket toolpath (pocketed the gap between the squares) and one as a profile toolpath (both selected so inside the 2" and outside the 1"). All done with Vcarve. Did a test cut and found my 1/8" bit cuts a 0.125" kerf. But ended up running .115" tool settings as .125" results were too big (bigger than what I will report for the .115"). Ran the cut. With the pocket toolpath, the inner squares outer dimensions were 1.01"x1.001" (x by y) and the outer squares inner dimensions were 1.996" x 1.993". With the profile toolpath, the inner squares outer dimensions were 1.027" x 1.020" and the outer squares inside dimesions were 1.969" x 1.979". First, is not the only difference between pocket and profile the fact that the gap in between is cleaned out? Second, should not the inside and outside squares outside and inside toolpath have been the same and thus the same dimensions??? So confused. Trying to upload a picture, will see it works.
[Uploading Cut.png…]

I have noticed the same thing as well. Those are the same numbers I get when I try to do a 2" square. Have you Pocketed and profiled a small circle, less than .50 inch. The reason i ask is im having trouble getting a perfect circle and wondering if the two issues are connected. I wonder if there is a problem with the Vcarve post processor or something to that effect for the Xcarve.

Xcarve and the post processor work perfectly for every one else. Way more likely to be a problem with something on your side.

If you carve the same square as a shallow cut (.05 in) with a vbit I bet the dimisions are spot on.

I think I mentioned earlier, that yes, the gcode run with a vbit and tool path ON the line is dead on accurate, which makes this other more puzzling. Assuming the pocket and profile paths are also accuate, 1) why are they different like shown in the picture. Even if the tool size was off, should not both pairs of squares be off the same? and 2) what else could it be??? I have calibrated, checked and tensioned belts, checked and adjusted pots, squared everything, and made sure all the vwheel are not free spinning or too tight. Surely there is something simple I am missing but after a week of trying to figure it out, I am out of ideas. Not being able to get accurate pocket and profile cuts pretty much kills this thing for the projects I have in mind.

I just wanted to point out that vCarve is putting the center of the tool exactly where you are asking it to be.

Tell vCarve that you are using your .125 end mill but actually load the vbit and do the shallow cut so you can see exactly where the tool center is positioned for the cut.

If you asked Vcarve to do an outside profile then the center of the tool should be exactly .0625 outside of the boundary of the square so measuring side to side on the thin tool center line should be 2.125 inches apart for a 2 inch square.

If that distance is exactly 2,125 then you will know that the problem lays with the bit you are using.

So ive been in boat as Bradley for about a month now, so if i have built a box torsion table, true and flat, squared the machine from corner to corner and that is dead on, steel plate in the x axis, y axis bracing, squared and shimed the z axis, milled the wast board, calibrated the SPU, swiched steepers to different axis, cut and wires and reattach, adjusted pots, tighten belts, loosened belts, tighten v wheels, lossened v wheels, changed out some v wheels, Dewalt spindle, precision bits.com collet, invetables .125 end mill, Vcarve pro and a new Toshiba laptop.

What else is there? Why does the issues still exist? Why cant it cut a circle the same diameter all the way around? If the issues happen the same way in different parts of the bed of the Xcarve i cant help to think its not mechanical. And buy the way customer support at inventables said not to change any settings to keep it at 40.00 on X and Y.

Im not trying to be a PITA but im frustrated and tired of playing around and adjusting the XCARVE.

Couple things I want to add, are you using X-Carve post processor mm or inch for V Carve, If you are this is the Grbl configuration I have and don’t have any problems. Please check line by line to see if something different.
(And one more reminder, Don’t use your Dewalt on max speed. Brush expected life time on full speed is 50 Hrs. which is 27000 RPM. Go slower like 3 or 4.)

Grbl 0.9i [’$’ for help]
[’$H’|’$X’ to unlock]

$$
$0=10 (step pulse, usec)
$1=255 (step idle delay, msec)
$2=0 (step port invert mask:00000000)
$3=3 (dir port invert mask:00000011)
$4=0 (step enable invert, bool)
$5=0 (limit pins invert, bool)
$6=0 (probe pin invert, bool)
$10=3 (status report mask:00000011)
$11=0.050 (junction deviation, mm)
$12=0.002 (arc tolerance, mm)
$13=0 (report inches, bool)
$20=0 (soft limits, bool)
$21=0 (hard limits, bool)
$22=1 (homing cycle, bool)
$23=3 (homing dir invert mask:00000011)
$24=25.000 (homing feed, mm/min)
$25=750.000 (homing seek, mm/min)
$26=250 (homing debounce, msec)
$27=1.000 (homing pull-off, mm)
$100=40.000 (x, step/mm)
$101=40.000 (y, step/mm)
$102=188.900 (z, step/mm)
$110=8000.000 (x max rate, mm/min)
$111=8000.000 (y max rate, mm/min)
$112=500.000 (z max rate, mm/min)
$120=500.000 (x accel, mm/sec^2)
$121=500.000 (y accel, mm/sec^2)
$122=50.000 (z accel, mm/sec^2)
$130=790.000 (x max travel, mm)
$131=790.000 (y max travel, mm)
$132=100.000 (z max travel, mm)
ok

1 Like

Let me guess. The outside square you were machining in a counter clockwise direction, right.

If that is the case you can see the problem in the photo. Look at the 4 corners. Do you see what looks like over run of the end mill. That is not over run that is the end mill cutting where it is suppose to. Then when it starts to cut the next side the end mill is deflecting to the inside of the square and cutting under size.

I’ll also bet you are cutting the inside square in a clock wise direction. The deflection is now away from the inside square so it is over size.

If your software will let you do a roughing cut that leaves .01" material on the square. Machine in a conventional direction. Then do a finish pass and remove that .01" using climb milling. Now measure the results and see what you get.

Hope this helps

Dave

3 Likes

@DavidSohlstrom I’ve been noticing an occasional divot in some of my projects, that makes a lot of sense. I’m working solely through Easel, maybe they’ll give an option soon to do a clean-up pass.

1 Like

I will give that a shot tomorrow. Thanks for a the advice. Sounds like a combination of these things will get me where I want to be. I will report back the results.

Is your power supply output clean and stable? I’m not suggesting a connection problem here, simply a power supply that is not delivering enough “on demand” current–or a dirty signal. This is, of course if all the physical variables check out OK. I see this happen occasionally with the switching supplies.

The only difference is that my junction deviation settings is .02 and not .05 and my $100 and $101 are a little different based on my calibration runs. And I am now running my dewalt at max of 2 or 3 on the speed setting.

Gave that a shot and still seeing differences from the 1" and 2" it should be of .02 to .05" (the difference still between pocket and profile toolpaths.

The power supply is clean and stable, as far as I know (which is to say, it is whatever it is :slight_smile: ).

I did some tests cuts like before and measured the width of the toolpath, as well as the inside and outside edges for a difference to determine an accurate cut width and over maybe a dozen measurements get a 0.127" cut. Used that for the same test as earlier with slower cuts and am getting a 0.95x0.97" inner square and 2.025x2.02" inner square (the top profile cutout like in the earlier image) and a 1.02x1.02" inner square and 1.97x1.97" outer square (pocket toolpath like the bottom earlier image).

So, I feel like I am getting closer, but think changing actual tool cutting widths like I was doing earlier is not the way forward. This seems like it is as good as I am able to get things. My biggest concern is that I still think the error between pocket and profile should be the same (and I am pretty close), even if I am off with the toolbit cut size a bit…right?

Not trying to get overly picky here but errors like these really make cutting holes for stuff to fit into, or a hex nut insert, or anything similar, becomes an iteration exercise.

I will keep trying…something. Thanks again for all the helpful feedback. I will report back if something finally works.

On the profile cuts did you program a roughing cut and a finish cut. On the pocket cut I see that the tool path appears to traverse back and forth from left to right and then right to left.

Most true CAM programs will start at the outside edge of the inside square and travel around the square in ever increasing squares until it reaches the inside of the outer square. You can set this up to do conventional milling or climb milling. each have there good points and there bad points.

If a machine is set up correctly with no slop and your steps per unit of travel are correct and you have checked your machine seven ways from Sunday and appear to be right.

The one thing that can be biting you is tool deflection.

Hope this helps

Dave

I have been trying to cut some pockets over the last 2 days and have been noticing the same issue, I made a 50mm pocket using a 6.4mm 2 flute cutter. On measuring the pocket with a vernier calliper it reads 49.58 mm. I haven’t had any time to try and resolve this yet, my first thoughts were to come on here and see if there was something simple I have missed.

I also spent quite some time trying to measure my cutter accurately, simply because the stated size of the cutter from the manufacturer was not accurate (6.85mm), but even after adjusting it to the correct size my cuts are still off.

As far as I can tell they are perfect circles, just not accurate in their diameter.

I am using Fusion 360 with Universal gCode sender.

I did do a finishing cut, with the same result. I switched to a 1/2" bit, trying to solve the deflection issue, with the same result (of course I edited tool sizing and such in the software). I plan to go back to basics, yet again, and confirm that things are dead one accurate, belts and pulleys are tight, machine is square, etc… Hopefully something will click.

What spindle are you using that allows a 1/2 inch bit (I assume it has a 1/2 inch shank)?

:smirk:

2 Likes

I prefer the old kick start spindles, electric start is for kids.

1 Like