I’m not sure why or how, but my y axis scale seems to be off. I’ve been trying to CNC some keyboard plates and the holes, which are meant to be 14.7mm squares are coming out as rectangles. On the x axis, it measures 14.1mm, but on the y axis, it measures 13.5mm. Besides the measurement being off by 0.6mm on the x-axis, both axes seem to have completely different measurement differences. Is there a way for me to calibrate the different axes?
That’s a really big difference. How did you generate the gcode, what software are you using?
Did you select configure the right bit?
Differences like that can’t be just attributed to calibration, something else must be off.
If you can share your model & generated gcode that would help as well.
I used fusion360 to generate it.
Here’s the link to it.
Keyboard Plate Top - Pastebin.com
Not sure why this would suddenly happen though, I managed to CNC a test keyboard plate before and it worked. I’m pretty sure I was using the same settings.
It’s an open loop controller, so if for some reason the linear modules skip you’ll have these kinds of dimensional errors.
Try using the laser to make a square and it should come up with the right dimensions. If it doesn’t, you’ll need to adjust the steps per unit for each axis, otherwise you can try shallower cuts on the CNC to avoid putting too much strain on the linear modules and causing skips.
The generated gcode seems to be correct. At the least the squares are squares. The toolpath for the square is spaced at 13.2 mm, which would mean that the diameter of your milling bit is 1.5mm. Correct?
Did you do a cutout of the entire plate as well? Is everything scaled in the same way? It seems really weird that everything would be scaled exactly the same.
Have you been doing any calibration on your axis? (M92 command in gcode?) It’s not something you can do from the GUI, so you shouldn’t have done it by accident.
If you just execute the M92 command in the gcode console it will give you the current values. Normally those are at 400 for X, Y & Z axis.
Thanks for the recommendations. I think I’ll try with the laser engraver to see if my calibration is working. I’m only cutting 2mm which doesn’t seem like it should put too much strain on the linear module. How do I adjust the steps per unit if I need to?
Yes my drill diameter is 1.5mm and I did cut out the whole thing as well and the measurements outside are also wrong by different amounts. Though I’ve thrown the plate away now so I can’t measure by how much its off.
I didn’t make any changes to the M92 command. I’ve just been putting the cnc file into the thumb drive and running it from there. How would I get the gcode console to run commands directly? Can I just plug it in and the software will have a way to open a console?
If you connect your computer to the snapmaker through USB you can enter the gcode commands in the console like window on the left. But if you’re asking this question, the chance is very small you would have adjusted these values 
You can also enter the commands over wifi, but then you don’t get the response, just “ok”
You can try again by running the job in the air above your workpiece.
Depending on the material, a 2mm deep cut can be too much for the snapmaker to handle and can be a reason for it to skip steps. (and or break a bit). I usually step down 1mm per pass. Also depends on other parameters.
This thread has a lot of useful info for cnc (and laser): Some info on cnc tool changes and combo cnc/laser projects
I was cutting acrylic. I guess I just sort of assumed 2mm was not too bad. I’ve broken a few drill bits and I ended up having to buy new ones (though those were my fault I sent it back to workplace origin without realising I had something in the way). I’ll definitely try the 1mm thing, that seems like the most likely cause. I can only access the snapmaker next weekend though but I am pretty excited to try out these fixes! Thanks.
Hi guys, I have discovered the issue. It was not the gcode, and it wasn’t the 2mm deep acrylic. I was using the wrong drill bit. My original had snapped off and I bought a few different drill bits to try out.
Here’s a picture.
The one on the left is similar to the one that was provided by snapmaker, the one on the right is another 1.5mm bit I found. I had a pretty hard time finding a replacement bit and most of the bits I found online were similar to the right one. The left one has a sharp cutting edge that probably helps with cutting through the acrylic. The right one was likely unable to cut acrylic properly and hence wasn’t getting the right shape.
My snapmaker is still getting differences in measurements on the x and y axis, but they’re off by 0.4mm or so which I find much more acceptable.
I only discovered this by chance, after deciding to change the drill bit to a different one. I guess I still don’t know where to get more of these kinds of drill bits and what they’re even called.
The bit on the left looks like a single flute bit. The one on the right is a 4 flute bit (the flutes are the number of spirals/helixes) you see.
The 4-flute one might even be a down cutting bit, can’t see it good enough on the picture. The one on the left is cutting upwards. This means the direction the chips (parts you cut) try to escape.
Acrylic might melt if you’re cutting too slow, especially with high speed spindles like the one in the snapmaker. Due to the friction it just gets hot and melts. As such your bit might indeed get stuck in the acrylic.
4-flute bits will get hotter qs there is more friction and the chip you’re cutting away is smaller, so it’s more likely to melt faster. Resulting in a sticky situation (literally).
I haven’t really worked with acrylic myself yet, but from what I gather it is indeed recommended to use single flute bits and move fast enough at not too high spindle speeds to get the best results. All depending on the actual bit, how sharp it is, the material etc. obviously.
The proper bits for cutting acrylic have different tool geometries than those for cutting metal or wood. Search for “plastic-cutting end mill” to purchase products.
Thanks! I had so much trouble finding what I wanted. I was searching for drill bit, or cnc router bits but I kept getting other stuff that wasn’t exactly what I needed.
Would you happen to know what bit is required to cut carbon fibre? I was looking into getting a few carbon fibre plates to try out.
Not offhand. There are a number of sites out there, however, with fabrication advice for any number of materials. Just put the name of the operation and the material into a search engine. “CNC” is not the name an operation, but “milling”, “drilling”, and “sawing” all are.