CNC Router consistently off by 1/16"

Could be some backlash in your X and Y axes. Since you said home built we don't know if your axes are belt driven or screw driven or gear driven the kind used would make a big difference.
4D

Have you calibrated your machine? How large is it? Whatever your Y length is you can use the MDI window to enter the code, say G01 F100 Y24.0 and that will move from Y0 to 24". Measure how far it moves and if it's not 24" then it needs calibrating. Same with X and Z. Mach3 has a built in calibration tool.

Photos always help.

It could also be your tooling or how you set up the file in F360. Are you cutting inside the line, outside the line, on the line, etc. and is your tooling exactly what you think it is? I have a 1/4" bit that measures 0.245" so that's how I set it up in F360.

Are you climb cutting or conventional cutting? Did you take a finishing pass?

Lots of good questions. The x access is belt driven, the x and y-axis are acme threads with anti-backlash. I am confident in the calibration since I can drill hole patterns accurately and jog the machine manually accurately. I also have excellent repeatability, since the walls of the cuts of perfectly vertical. I thought it was missing the finishing passes, but they are selected and I can see the paths in F360. The weirdest part is that when I simulate in cutviewer and measure, it is accurate. I have tried climbing and standard compensation with no difference.

Welcome to the forum.

Double check the connections between stepper motors and the drive. I notice on my CNC a weird action when the machine reversed direction in the Y axis. Turned out I had a loose coupler set screw on one side which led to that action. Tightened the screw and all problem disappeared.

besides all of the great responses above... the best way to calculate and adjust for actual tooling dimensions is to perform a straight line cut, preferrably in the same material you are using, and the same feeds and speeds. measure the width with calipers as accurately as possible. then enter that value for that specific tool cutting diameter.

unfortunately i do not use mach3 to tell you where that is, but i am sure there is a tool page where the tool diameter can be entered. have your tried the same box test with a different tool? is there an allowance or offset in the program?

TimPa said:

unfortunately i do not use mach3 to tell you where that is, but i am sure there is a tool page where the tool diameter can be entered. have your tried the same box test with a different tool? is there an allowance or offset in the program?

Click to expand...

That would be handled in Fusion 360, not in Mach3, but the same principle applies there.

TimPa said:

besides all of the great responses above... the best way to calculate and adjust for actual tooling dimensions is to perform a straight line cut, preferrably in the same material you are using, and the same feeds and speeds. measure the width with calipers as accurately as possible. then enter that value for that specific tool cutting diameter.

unfortunately i do not use mach3 to tell you where that is, but i am sure there is a tool page where the tool diameter can be entered. have your tried the same box test with a different tool? is there an allowance or offset in the program?

Click to expand...

TimPa You nailed it. I cut two grooves and measured .216” with a 1/4” spiral down cut bit. I had measured the bit and a drill hole previously at .25” Changed my tool diameter in F360 and got accurate results. Thank you for solving this mystery!

That is quite a difference, if it is a new bit it might be a 7/32" bit with a 1/4" shank. Or an old bit that has been re-sharpened.

SteveC said:

TimPa You nailed it. I cut two grooves and measured .216” with a 1/4” spiral down cut bit. I had measured the bit and a drill hole previously at .25” Changed my tool diameter in F360 and got accurate results. Thank you for solving this mystery!

Click to expand...

im glad it worked out for you. i just repeated something that i have read tho, no credit here...

I'm a bit late to this and it sounds like you solved your problem but there is another possibility. I would check my F360 CAM setup - there is a "stock to leave" option that is on by default (at least, it was a year ago). It leaves a little stock to allow for a light finishing pass. Also, it is hard to accurately measure a groove for width and 34 thou is waaay off. Even bits made of Chinesium aren't usually that bad. I think (based on what you said) your original test was an inside cut. Have you tested an outside cut?

If the measurements are off only when the gantry is moving and not when drilling I would check for racking of the gantry. I also would try making passes near each end of the table and in the middle. If you have racking the distances from one pass to another will be different.

PhilBa said:

I'm a bit late to this and it sounds like you solved your problem but there is another possibility. I would check my F360 CAM setup - there is a "stock to leave" option that is on by default (at least, it was a year ago). It leaves a little stock to allow for a light finishing pass. Also, it is hard to accurately measure a groove for width and 34 thou is waaay off. Even bits made of Chinesium aren't usually that bad. I think (based on what you said) your original test was an inside cut. Have you tested an outside cut?

Click to expand...

Thanks everyone for the good comments. I have been doing additional troubleshooting. I declared victory too quickly. I changed my spiral downcut bit to straight flute and measured the cut. It is 1/4". Ran additional tests and came up with similar issues in both axis. Both bits are Whitehead solid carbide. I would like to still rule out that the issue is not with F360. Could someone be so kind as to share a G code file that they created with a simple square recess(say 6x6"x1/2" deep grooves in a 12X12"x 3/4" stock). That way I can confirm it's the machine and not the G code. Thank you. Steve

G-code that I generate in F360 very likely won't work on your machine. Our Post Processor choices are going to be different and our tool library different. Post your f3d file somewhere that we can download it and view what you've done in F360 (you might be able to zip it and upload it here).

difalkne;
Please find attached 3 files to use for testing. The first few lines are setup for my machine and will need to be modified to use with your machine. Just use Notepad++ or some other text editor to add the necessary files for your machine. This G-code is in absolute coordinates not relative so if your generating relative coordinates that could be a source of your problem. One file cuts a 12X12X.5 box another file cuts a 8X8X.5 box and the 3rd file cuts both. These files were generated using V-Carve pro 10 with a standard G-code post processor.
Doc

Doesn't look like the files attached. I am changing the files to .TXT format and retry. Looks like they are going this time. Just change the file extension to whatever your machine uses and you should be good to go

wyzarddoc said:

that could be a source of your problem.

Click to expand...

I think you're missing the point, Doc. I'm not having an issue with my machine; Steve is having an issue with his. He's using Fusion 360 and asking questions about accuracy.

Sorry for the wrong name attached to post. thanks for the correction