Machine accuracy

I know this topic will have overlap with others already posted, but I am hoping for some inspiration from everyone here.
I have my 1000m Xcarve up and running. I still cannot connect to Easel with any of the 3 Mac notebooks I own, even with the advice of the forums and Inventables help desk (restarts, reinstalls, different browsers, reflashed grbl to my arduino, etc…), so have given up on that as everyone on the forums and help desk seem to have run out of solutions. Connects fine with a 6 year old pc notebook, but takes a week to but runs like molasses and I don’t want to buy another computer just for the Xcarve. I just use Vcarve and UGS.

My biggest issue now is accuracy of the cuts. I have checked, rechecked, checked and rechecked belt tensions, Vwheels and eccentric nut tightness, squared the machine, adjusted pots and calibrated steps per mm several times. My precision is great in than I can hit the same spot or spots dead on all day long. The calibrations (have done x and y from 100 up to 600 mm) get me where the movement is dead on. But, when I go to cut a simple 1"x1" or 2" x 2" square, or circle, of whatever, the actual cut dimensions are always about 5-7% smaller (0.94" square instead of 1") than drawn. I get perfectly shaped squares and circles, just too small. I have done this with both 1/8" and 1/4" bits and get the same result. The only thing I can narrow it down to now is that somehow the toolpaths generated with Vcarve are not what they should be. Or is this the level of accuracy that should be expected?

Any help or ideas on what to try next are greatly appreciated. I love this thing, just want to get it running as close to perfect as possible before I move forward.

What type of cut are you doing (profile/pocket) and how are you measuring it?

I would load a 30 deg vbit and carve a image like this that should be exactly 12 inches long and 1 inch high, then measure the vertical lines to see if they are correct

Thanks, I will give that a shot. I was cutting 3/4" plywood, and only 1/4" depth in 3 passes. And I measured with a pair of digital calipers, inside edge to inside edge.

With the figure, how deep of cut should I make? Cut on the line or inside or outside? Do I measure edge to edge or center of v groove to center of V groove?

Thanks again, I will get things ready to cut.

I would make the cuts as shallow as possible, so the lines are as thin as possible. Set a dept limit of .03 inch, if you vcarve a a set of vector like the picture you do not have a choice of inside/outside. It will always cut on the line.

Ok, so the cuts are absolutely dead on, which is great. But now makes me ask why the other cuts I made were off. I measured tools bits to insure the right tool size, so should not be that. My cut rates were 80 in/min, 0.1" depth per pass and I am using the DW611 at full rpm. The project started me down this road was making wooden knobs for some tools in my shop with a hex cutout and hole for a 5/16" bolt to fit in. Both the hole and hex recess were too small, thus my quest for accuracy. So, now that I know the machine is dead on, any suggestions on priority of things to try to make more accurate cuts. Thanks again! Has me feeling much more confident in all of the setup I have done and the Xcarve itself.

When you are cutting a part out (a profile cut) you do have a choice of inside/outside or on line. Depending on the bit size the choice you make really matters a lot for the the finished dimensions. You should probably be cutting outside if your drawing is exact size.

Also, there is really no need to ever have the Dewalt set above 4, for most cuts 2 is better than 4 (of course it all depends on the material, bit size, number of flutes, and feed rate. But within the range of what is normally cut on the X-Carve with .125 bits or even .25 bits 2 or 3 on the speed control will be better than 4 or 5.

Here is a small Excel sheet that you can enter your feed rate and it will show what speed setting on the Dewalt is needed to achieve a desired chip load.

CNC Speed Calculator.xlsx (14.6 KB)

So, I have done both. For the knob, I cut outside for the knob shape itself, but the recessed for the hex bolt head and the through hole were both inside the lines. I will keep experimenting with feed rates and such. Worse case, I guess I can fudge the drawing dimensions by the 5 or 6% I am off.

So, I have adjusted feed rates and confirmed that the squares are dead one. I have tried a number of pocket toolpath cuts (all generated in VCarve) for a recessed hex nut for a knob as well as test 1 and 2" squares and a 7/8" hole to test against a forstner bit. These pocket cuts are still 5-7% undersized, edge to edge. I did just a profile toolpath for a 3" circle, cutting on the line, dead on. Am I missing something with the pocket toolpaths?? confirmed bit sit, feed rates, machine steps/mm, and all the calibration tests show the thing is much closer than the error I am getting. Very, very confused and grateful for any clearing of the fog anyone can provide.

As a quick follow-up, did a 1"x2" square, fill cut using Easel last night and the resulting square was 1/16" too short in both directions, so it does not look like it is something I am doing wrong in VCarve. There has to be something simple I am missing.

Do 1 more test, cut the same fill cut with w larger bit like a .25 or 6 mm (be sure you are using a flat bottom endmill) and measure it to see out much it is out.

Redid the test cut with a 1/4" flat bottom spiral cut bit. Made sure the bit was a full 1/4". My 1x2" square came out to 0.97x1.97. I re measured the 1x2" square cut with the 1/8" bit, it was 0.94x1.94". Seems like I am missing something somewhere related to tool size and path.

You don’t have a non zero value for the pocket allowance do you?

No, I made sure and double checked that in VCarve. I also did the same test carve in Easel and get basically the same result. And I don’t think Easel has an option like pocket allowance (at least not that I have seen). It is wired that cutting on a path is perfect, but cutting inside or outside is short. I think I have remeasured tool diameters at least half a dozen times. Figure whatever I am doing wrong will be something I will be one of those things I slap my head once (or if) I figure it out.

Have you checked your step/mm settings? It might require adjusting those to compensate for machine variations.

For instance, when I checked my SO2 using a circle-square-triangle test, it was off slightly. I then checked the accuracy over a longer distance and changed the settings as follows:
$100=40.040 (x, step/mm)
$101=40.040 (y, step/mm)

Your settings will be different from mine, but it might be worth checking.

WHen you find it please post the answer, because I am stumped also. It sure seems to be related to the bit size, but not by any fixed amount that I can see. It might be worth trying a different 1/8 bit to see if the error stays the same.

I have done the machine calibration a number of times, so am confident have that dialed in. I think I mentioned earlier, I did a 3" circle, cutting on the line, as well as the 12, 1" boxes suggested earlier and both of these tests show that the machine is dead on. It seems to just be cutting inside or outside the lines that cause problems. My next test will be a series of circles and squares cut on the line with a 30deg vbit to make sure it is still dead-on, the some shallow inside and outside line cuts next to the v cut to see where the edge of the tool is going. I will try to take some pictures and upload to see if anyone has any brilliant ideas. I am at a loss at this point.

It sounds to me that the program you are using to generate your Gcode has a problem with figuring tool diameter off sets.Your machine looks to be calibrated correctly when you do a cut that has zero tool diameter off set.

One thing you may want to try is down load a copy off CamBam where you can run 40 jobs before you have to buy a copy if you want to continue to use it. Use the CAD part of the program to generate your 2"x2" square. then do a outside profile with the tool of your choice. Set your feeds and speeds the same as you have been using.
Use the generic post processor to generate the Gcode.
load it to a thumb drive to load on the computer running your machine. run the code as an air cut with NO end mill in the machine and make sure it does what you want. then load a tool and run again and measure the results.
If all is well then you know that the software you have been using is the problem somewhere.

Hope this helps


I know for a fact that Vcarve generates accurate gcode that takes the tool geometry into account perfectly.

That being said, it is only as good as the tool description you give it. If you tell it you are using a .245 inch endmill and then actually use a .25 endmill the cuts will certainly be off. So you do need to verify that the tool selected accurately matches the tool being used.

No pictures to upload as they really did not show any thing useful. I am not sure I figured anything out, but my “fix” at this point was to modify my tool bit size. Increasing my 0.25" bit to 0.255" got the inside and outside cut where they are supposed to be. I figure if both Easel and Vcarve give me the same inside and outside toolpaths that are off like they have been, and the machine is properly calibrated and setup (belts, eccentric nuts, squared, etc…) and all other software settings are correct, the only other thing it can be (I think?) is tool size. Even though I think I am measuring the bits correctly, there must be something off. My thought moving forward with different bits is to use the test squares (with in and outside cuts) and “calibrate” the bit size in the software until my cuts are where they are supposed to be. I was surprised that .05" change in bit size had as much impact on the cut placement as it did. Anyway, maybe not the best solution, but I will see how it works.