Having just built my ooznest ox cnc machine i am having problems getting it to cut the correct depths, when using a file made in cut2d desktop. Not sure i am saving as the right type of gcode file as the machine is not listed. I have tried xcarve and shapecko.mm along with Grlb and still get the same result. The machine depth works perfectly when i use the machine control. Many thanks doc
It is also important to make sure that the material/cut settings you choose in Cut2D matches the workflow you are using. For example, I have homing switches on X, Y, an Z axes and when the Z-axis is at 0, it is just touching the bed. All of my material and cutting is done above zero. But other people manually set the Z-axis zero to the top of the material and the material itself and cutting area is all below zero. Cut2D can handle both kinds of workflows, but you have to set it properly. Other Z-axis issues, like the material not being cut through, or the material being cut too aggressively, or the bit digging into the spoilboard have other causes. But since you don't specify exactly what issue you are having, it is hard to assess. FYI, I use Cut2D myself and specify the 'grbl' post-processor and it works for me. So I'd do that as a starting point and then start tweaking other values. -Jonathon Duerig
i zeroed the machine on top of the material 12mm ply and tried to make a 50mm straight line 1mm deep to see how deep it was cutting 7mm deep i have set the material up in cut 2d the same as what i have been using. I also tried in 6mm mdf and had the same problem. I will try zeroing it on the machine bed later and see what happens. Many thanks doc
A good next step is to look at the actual gcode output. Open it up in a text editor and search for 'Z'. You should get a sense of what coordinates it is sending. If the coordinates look like '-7' instead of '-1' then you know that the problem is how Cut2D is setup and generating gcode so you'll want to check the settings and toolpaths. If the coordinates look like '-1', then the problem is the machine itself and either you are not zeroing where you think you are or your distances are badly miscallibrated. Note that you can also remove the actual board you are cutting as well to pin down the cause precisely. Zero your machine, measure the distance from the tip to the bed, run the code in 'air', but pause it partway through (when it has lowered) and measure it in air again. This will let you know whether it is the movements of the machine itself or if the bit itself is being pulled down into the material by the action of cutting. -Jonathon Duerig
I think i may have fixed it somewhat. I tried the whole air idea and found the z was going to high when starting to send the file. So i have adjusted the router up to match where the z axis does not top out. I do not know if i am doing this right.
So here is what I think you mean: (1) The Z-axis is zeroed on the top of the workpiece (2) You start the program. (3) The Z-axis moves up to the top of its travel, grinds for a moment (skips steps) because it has hit the limit, then moves down. (4) The Z-axis then moves down to the work piece but it is now systematically lower by however many steps it missed. If this is the case, then one solution is just as you said. Adjust your machine to ensure that there is enough room above the workpiece to avoid hitting the edge of your travel. The settings that this interacts with are the 'starting position' and 'safe rapids height' options in Cut2D. If either one is high enough above the piece to hit the limit of movement, that will cause this problem. OTOH, you need to ensure that the safe rapids height had good clearance on the entire workpiece and any clamps you are using so it won't hit them while it moves between cuts. In the longer term, getting limit switches (the cheap microswitches on the OBPS work great) and installing them is both cheap and easy. And in addition to helping to avoid the skipped steps like you have seen, they also act as homing switches so you can use fixed stops on your spoilboard and not spend 10 minutes jogging the machine to find just the right zero point. Best of luck on your project either way. -D
Gotcha found the safe rapid height and its set at 20mm which to me sounds way way to high will try with 5mm. Many thanks for all the help and will look into getting limit switches.
