Hi there, I am new to xcarve, ugcs, and arduino. I’m super excited to have my machine “up and running”.
I have been using xcarve to created my models, and UGCS to send the commands to my machine. I am working on a simple name sign for my nephew. Here is the issue that I have. It is responding to the code, but it seems that there are 3 or 4 passes of the same layer with no cutting, just the motions of cutting. It’s been on this M for 15 minutes. What have I done incorrectly, or were there settings that I didn’t pay attention to? Thanks for any help!
Edit: I totally misread the above. Nevermind…
Was the first layer actually cutting wood?
I will assume that the first cut was correct and cutting wood, then the next few passes (where the tool should have been lowered into the material) were not cutting any new material.
There are a few things that can cause this behavior. The simplest is that the bit is not tight in the collet and it is simply sliding up. Easy to fix, just be sure the collet is tight (and you are using the correct collet for the shank size of your bit).
The next possible issues is that the Depth of Cut (DOC) is set to small, so that each pass is only moving down a very tiny amount. Check to be sure your DOC is between 10% and 50% the diameter of the cutting tool.
Lastly, your Z axis may have a mechanical issues. If the threaded rod is binding, or the Z pulley is slipping on the motor shaft then the Spindle will not move down as expected. You can check for binding by removing the Z drive belt and turning your threaded rod by hand, it should turn smoothly for the spindles entire range of motion. If it feels tight or difficult to turn, find out why.
If the set screws in the Z pulley are loose (or missing) then the pulley will slip and not be able to provide enough torque to move the spindle downward.
The last possible issue to check in the voltage being sent to the Z motor from the Grbl shield. You may need to adjust the voltage potentiometer slightly. There are many very good explanations of how to do this on the forum.
Thank you, the bit is not loose in the collett, the thickness of the carve was consistent across the piece. The first pass did cut wood. I will check out your other solutions and report back. I had assumed it was a problem with the way the UGCS processed the file, or some setting that I either ignored or was ignorant of adjusting.
It very well could be a toolpath issue. I have never had any problem with UGCS not doing exactly what the gcode told it to do. So if there is a toolpath issues it is most likely from your CAD/CAM program. An example of that type of problem would be that the DOC was set way to small.
What software are you using to create the gcode (toolpath)?
If you used Easel, check the toolpath in the 3D view to make sure the layers are there and they go down the way they should. You may have to get very close up to the paths on a very shallow angle to see this. I would also check “hide material” so that you just see the toolpath.
Alternatively you could use a program like OpenSCAM which will read a Gcode file and run it virtually so you can see the piece being carved in real time and get an idea whether or not it’s done right.
If the code looks ok, check the machine. Do a simple shape like a small circle. Watch the pulley on the Z Axis stepper. after each layer, you should see it go about a quarter to a half turn. If it turns but the spindle doesn’t go down, check that the grub screws in the pulleys are tight, and that the belt is not slipping on them.
If the machine is dialed in, and the code is right, but the z axis is still not moving down, check the grbl configuration. Depending on what Z axis screw you have the configuration will be different. Look at line $102. If you have the Acme screw it should say 188.95 or thereabouts. If you have the M8 screw, it should be 302. If it says something wildly different, re-run your setup routine through easel to reset the machine to the correct numbers.
1 Like
I’m using Vcarve Pro 8. This is a newbie questions, but what is a DOC?
I understand about half of what you are saying 
I really appreciate the help, and will definitely get to the root of this problem after my kiddo goes to bed today. My machine isn’t dialed in, i still don’t have the permanent home for the machine set up…My housewifery and mommyawesomeness is suffering due to preoccupation with the xcarve.
The DOC is just the depth of cut or “pass depth”. It is the amount the bit will cut into the wood on each pass. The larger the DOC the more material is removed with each pass. The DOC is set in Vcarve for each operation you create.
For example if you are making a profile cut (cutting around the edge of a vector) that will cut a hole all the way though your wood and your wood is 1/2 inch thick you would not want to try to cut the the full half inch deep in one pass.
Determining how deep each pass should be depends on four things, how hard the material is, how large your bit is and how fast your feedrate is and finally how smooth you want your finish cut to be.
Typically a good rule of thumb is to keep your depth of cut to about half the width of your bit. So if you are using a .125 inch diameter cutting tool then the DOC would be .06 inches. If you wanted your feedrate to be faster than normal then you could reduce the DOC to .03 or you could decide you wanted a deeper cut each pass of .08 inches and slow down the feed rate a bit.
The trade off is that the smaller your DOC the more passes an operation will take and that can dramatically increase the amount of time a project will take.
Here is a screen shot from Vcarve showing a profile cut though material that is .25 inches thick. I am using a .125 inch diameter endmill and the DOC is set to .06 for that tool. So Vcarve is telling me it will take 5 passes to cut through the material
You can override the DOC for each pass in Vcarve (if you want to) by clicking the “Edit Passes” button. Then you will see a complicated looking screen that lets you set the DOC for each pass to just adjust the total number of passes that you want. This is sometimes useful if the last pass is very small.
Typically you will define the DOC for each tool in your Vcarve tool library and then just leave it alone.
Here I have the pass depth set to 0.07 for this particular bit.
1 Like
Thank you so much! This is the most thorough explanation of how to determine the DOC that I have seen. I think that was my issue!!! I truly appreciate it.
After my carve finished, I realized my safe Z height was set to .13 by default, I am unable to change it, without an error. When I reset to home in UGCS, do I raise Z to .13 to begin with? On the same sign, I observed that letter profile depth had been set to .1 in. and in reality, the calipers read .23 I, had assumed that I need to raise my Z by .13 to begin with so that I would be accurate. This would also explain why it seemed like after the first pass, it slowed down, when in actuality, that was the proper DOC for the pass.
In Vcarve you can change the safe Z height by clicking the “Set” button at the top of the Toolpath form on the right side of the screen.
Then enter the height you want in the “Clearance (Z1)” box.
Always set your Z0 to the top of your work surface (unless you change the home position in Vcarve). Also, be sure that all your coordinate values in UGCS are zero for work and machine positions before you click send.
When you click the Send button in UGCS the spindle will immediately move up to the Z Clearance (Z1) value you set in Vcarve. Then the spindle will move to the starting X/Y location and lower to the work surface minus the first pass depth and begin cutting.
1 Like