I was trying to use carbide create to do a v carve inlay. I created the.tool path with no issues and brought ot over to UGS again with no issues and ran the 1/8 inch pocketing bit first and then tried to change out the bit to the 60 degree v bit but I could not move the machine to reset my zero so it was my best guess as to try and set the depth of my v bit to match the pocketing bit. I never could get it to work. What am I doing wrong?
@fiveowoodworks4460 Not sure what you mean “could not move the machine”. Can you give a little more detail. Or pics maybe. Will be glad to help with more info.
I couldn’t jog the machine in any direction unless I manually spun lead screws or pulleys. So to change the bit I had to manually.spin the pulley the z axis carriage to.bring the router up to change.the bit then bring it back down to where I guessed the starting depth was.
@fiveowoodworks4460 Did the first gcode file completely finish? Router return to x0y0 and z safe height? Were the jogging controls greyed out? Trying to visualize in my mind.
@fiveowoodworks4460 I’m assuming that your job is done and you are looking to make sure this does not happen again.
I, too, am curious as to what was happening when it froze. Was the tool path finished? Did your gcode have a command in it to pause for a tool change? If it did, you can’t jog in that state. I don’t use carbide create so cannot help there. In VCarvePro, for example, I create a separate tool path for each bit. The “job” is complete when the tool path is run. Then, I change the bit, set Z0 and run the next tool path.
How do you create your tool paths in carbide create?
If your tool paths are separate by bit, try clicking on soft reset in UGS if this happens again.
With more info, I’m sure we can help you to get past this.
The controls were grayed out the router didnt return to x0y0. The machine stopped because in carbide create the “advanced v carve” does the flat pocketing and v carving as one g code and I do not know how to break it up or make it 2 separate tool paths.
@fiveowoodworks4460 - unfortunately i know nothing about carbide create. we need some CC users to chime in. Sounds like a CC issue. If CC stopped for a tool change it should have given you an opportunity to swap the bit which includes being able to jog. It almost sounds like the gcode just stopped. Did the flat pocketing look like it was finished?
@fiveowoodworks4460 Matt: Maybe this will help
If it does not, I searched on tool change in the group and got lots of hits. I’m sure one of them will solve your problem.
UGS was in what ill call Hold mode while I swapped the bit then when I pressed play it started again with the v bit carving. It sounds like becUse they design it to work with their own machine for which they have a bit depth setter they probably designed the g code to work within those parameters.
In carbide create do you have your post processor set to GRBL? Did you export your gcode for each bit separately? I’ve just started but I think you have to save each tool path separately and run the separately because of this. The work around might be to use depth stop collars so you can just place your bit and not have to worry about resetting the z zero.
I had a similar problem using Carbide Create. Apparently either CC doesn’t send the right gcode for a manual tool change or the LongMill doesn’t recognize it, but either way you can’t reset Z after changing the bit even if you manage to get it swapped.
As I recall I had to go in and manually edit the gcode file and split it in to two files - one for the first bit and one for the second bit. Then you run the first file to completion, perform the bit change and reset Z, then run the second file.
If you open the .rc file in a text editor, your can search for (Advanced …) to see the start of each section to find where to split it.
Not sure if there is a better way, but that was how I made it work.
@SteveInCO The link that I posted previously in this thread describes how to create separate gcode files in carbide create for each tool. That way, you do not need to edit the gcode.
Yes, it shows how to disable/enable steps to export to different files. That works for most of the toolpath types.
However, because the Advanced VCarve allows selecting two bits at once, you can’t separate them just by disabling steps. I was unable to find any way to “partially” disable a single step, hence the manual editing.
The other thing I will add is that I am using the free version of Carbide Create on Windows. The version in the article looks different. I don’t know if its because it’s the “Pro” version or because it is on a Mac or if it is just out of date.
Advanced v-carve will create the single file with the two bits and a tool change. The last command before the tool change is the command to move up to whatever height you have your carbide create set to for movement. The way I have worked around this is to open the g-code in a g-code editor and search for M0 command. Go to the correct one as there are usually 5 M0 commands in the file. I then increase the last Z command on the line before the M0 command to an appropriate height to be able to change the tool.
You could also do the advanced v-carve with the pocketing operation, save the g-code and do a second advanced vcarve and unselect the pocketing operation, save the g-code. Then run the first one stop the program when it gets to the tool change and then restart it with the non-pocketing operation after changing the bit and resetting the zero.
As another thought one might be able to do the pocketing operation in advanced v-carve and unselect the v carve operation, then do another toolpath with advanced vcarve and select only the v-bit. Then save each toolpath individually. I haven’t tried that and I don’t have carbide create in front of me so I can’t verify that would work.
At the moment Carbide Create pro license is free for a year.
So i downloaded a text editor and found the 5 M0 commands you talked about. I am extremely new to the CNC world and have some questions if you could help me. How do I know which one is the right MO command. And if I increase the Z height for the tool change will my zero remain the same without any further modification?
I had struggled with this before finding this post and solved it another way. Well actually the same way, just searching for another letter.
The T command is associated with tool changes in the code. It’ll look something like:
This is the start of tool 108.
In CC you can give the various tools numbers. When the tool changes, the new tool number will be there, that is how you can identify which M0 TXXX command is which.
You only need to do this with advanced V Carve, the other ones you can manually control the files as shown above. Export the G-Code, open it in some editor and look for the change in tool command. Delete from that point forward (I leave the M05 and M02, not sure if that is necessary) for the first file. Reopen the original file and delete between the two T lines and that is the second file. Run the first file, UGS should show idle/done. Jog as needed to change the bit. Use the touch plate to home Z only (or manually set Z) and run the second file. Worked well for me.