I was wondering if there are any v carve pro experts out there. When doing a deep pocket path, I was wondering if there was a way to have the Z not always feed from Z+.02 for every depth pass and like feed from Z+.02 from the previous finished cut… It would save an unimaginable amount of cycle time. I know we do it with our cnc machines at work.
Are you saying that the bit is raising .2 after each pass and then moving down to make the next pass? If so that’s not in v-carve maybe it’s in the post processor that you are using, or something in the Cad.
Do a virtualization in vcarve, look at it at supper slow speed from the edge and see if the bit is moving up, if not it’s definitely the post process.
Are you sure about that? I looked into this, and I am seeing the same thing. I don’t see anything in the post-processors that would cause it. It raises to the “Safe Z” height prior to each pass.
I have used each version since 7.5 and it’s never done that with me. You have the safe z height that the bit will travel above the work piece but that’s the only setting I can think of, that’s why I suggested to do a virtualization in v-carve and looking at the cut first. Is there something goofy in the tool table settings?
I do not think there is any way to stop Vcarve from pulling the tool up to the Z safe height between passes. For simple rectangular pockets this seems wasteful, but for complex pocket shapes it is easy to see how a collision could occur if the tool was not at the Z safe height when rapiding back to the start point of the pocket.
You can reduce the time a small amount by setting the Z2 value that allows the tool to rapid move from the Z1 Safe Height to the Z2 distance above the material.
I’m gonna have to look at that tomorrow while I’m messing with the ATC Allen, I have never noticed that. Maybe I have my setting running real tight, it’s been forever since I set them up.
I saw your ATC posting, that is some very impressive upgrading. Are you using the standard GRBL motion controller? If so how did you mod the software to enable the ATC? Or do you need to include the ATC actions in the Gcode?
Pocket toolpath will retract to safety height. Profiles won’t.
I think there’s 2 different Z retract heights (Z1 and Z2) but I can’t remember the difference between them.
One is the safe Z retract height and two is the feed height (height it will rapid to before slowing to plunge feedrate).
I’m using a controller that supports ATC (Planet-CNC)
So yes. There are 3 Z height parameters. There’s the home/start position which is how high the bit starts at. Then there is a Z1 and Z2. Z1 is the clearance for rapid travel in the x and y. Z2 is the plunge distance, which I have set to .02". So for example, if I’m doing a pocket that is 2" deep, with a pass depth of .1", it will always start feeding down at .02 above my z zero point for every pass depth cut. Well, if I only have a plunge feed, of let’s say 2 ipm, it will have to feed from .02 above zero to -1.9" of cutting air just to cut the last pass depth. Wasting a lot of time …
Of course you can always edit the gcode to remove the z axis command that lifts the tool to the z1 safe height.
This is a bit risky since any error made when you manually edit gcode will almost certainly result in a tool break.
Yea, I’ve edited the code before for other things, but if you had several passes, this alone would take quite a bit of time. Assuming that I don’t make a mistake that is…
Well, I guess there is no way. I emailed Vectric and that’s the way the cookie crumbles… I think that’s usually one of the most common gripes with programming software is tool path selection… Vectric included.
I will say if you upgrade to a linear Z axis, you can increase your rapid speeds by about a factor of 3 or 4 and it makes that process way less painful to watch.
Applies for acceleration value aswell which can safely be increased to 250. (Xcarve default $122=50)
Not that important for safe height retraction/plunge speed but have great impact on 3D carve times.
I edit like that all the time just using cut and paste in the text editor. Works well and reliably.
250 is still low. I’m running 750 and easily recommend 400 when upgrading.
Yes, I do have the z upgrade and have the rapid turned up. My issue is doing more with metal where the plunge can’t be quite as fast as wood, and DOC is quite a bit less then wood as well, making for more passes, increasing that z plunge air cut time.