Tool pass depth vs. Vcarve Flat depth

[Solenberg]

I broke an expensive bit. I have the pass depth for my 1/16” upcut bit set to 1/16” (0.0625). I was doing a vcarve using that bit as a clearing bit with the clearing pass Flat Depth set to 1/8” (0.125). On that clearing pass the CNC plunged to 1/8” and after a few seconds, the bit snapped (I'm using the Amana recommended feeds & speeds for this bit). Why doesn’t the pass depth I set for the bit overrule the flat depth and simply require the bit to make two clearing passes? This is what I assumed would happen. Is there any way I can force it to do that?

(BTW, full disclosure, I was using three different clearing bits, a 1/4” bit, a 1/8” bit, and then the 1/16” bit. So I realize I could set the flat depth to 1/16” but that would add a ton of time to the cut when the other two bits don’t need a pass that shallow.)

[Rcnewcomb]

Can you upload your CRV file for us to review?

If it is too large to post here you can upload it to a free file sharing site such as drive.google.com, onedrive.com, or dropbox.com. Make the file shareable and then share the link here.

[Solenberg]

Outstanding idea! Here's a link to the file. I'm also open to any other tips if anyone sees anything wrong with it.

https://1drv.ms/u/s!Ak9iX-omcv-PsknHQx2 ... w?e=uP9uVy

[Adrian]

You've got a start depth set. The software assumes that you don't have any material above that depth so it will plunge much further than you might expect. It's the drawback of using the v-carve toolpath in a way it was never designed for with those inlays.

There is a gadget now that creates multiple toolpaths to get around that issue you might want to have a look at - viewtopic.php?f=51&t=38177

[Solenberg]

Thank you, Adrian. I will check out that gadget but I may be confused. The start depth on my first pass is zero with a flat depth of 1/16". The following paths start at the new level and go to a flat depth of 1/8" each. Did I misunderstand your answer?

[Adrian]

I did misunderstand what the issue is. It's not the usual one.

With so many bits (do you really need that many?) it's hard to see exactly what is going on in the preview wireframe but it certainly looks like it's doing two passes on all the full contact parts from what I can see.

[SteveNelson46]

Unless I'm missing something here, you don't need all of those toolpaths. As an example, set Vcarve 4 start depth to 0 and the flat depth to the full .4375 and recalculate. Turn on the animate preview and set the speed slider down to about half way. Run all four vcarve4 toolpaths in sequence starting with the largest diameter tool. You can see that the "depth per pass" on each tool will handle each toolpath appropriately and it doesn't cut air where the previous toolpath cut.

[Solenberg]

Unless I'm missing something here, you don't need all of those toolpaths. As an example, set Vcarve 4 start depth to 0 and the flat depth to the full .4375 and recalculate. Turn on the animate preview and set the speed slider down to about half way. Run all four vcarve4 toolpaths in sequence starting with the largest diameter tool. You can see that the "depth per pass" on each tool will handle each toolpath appropriately and it doesn't cut air where the previous toolpath cut.

I'm still trying to get my head around deep Vcarve inlays. If I do it with the multiple paths the way I did it originally, I get this: https://dm2306files.storage.live.com/y4 ... pmode=none

If I use zero as a start depth and .4375 as a flat depth I get this: https://onedrive.live.com/?cid=8FFF7226 ... 75&o=OneUp

Sorry, I don't know of a better way to embed screenshots.

[Solenberg]

With so many bits (do you really need that many?) it's hard to see exactly what is going on in the preview wireframe but it certainly looks like it's doing two passes on all the full contact parts from what I can see.

When I looked at the part that was being carved, the 1/16" bit was very obviously trying to cut a path that was 1/8" deep. Initially, I assumed I had set the pass depth of the bit wrong but when I went back to Vcarve and checked, I had it set correctly. I almost hate to try again to verify it without a better understanding of what's going on. $50 a pop for bits can start adding up after you snap a few.

[SteveNelson46]

Maybe I am missing something. I didn't realize it was an inlay. Never seen one that deep.

[adze_cnc]

I'm still trying to get my head around deep Vcarve inlays.

Have you looked at the gadget link Adrian posted above?

[Solenberg]

Have you looked at the gadget link Adrian posted above?

Not yet. I'm juggling these questions with the work I have to do for my actual job. But I definitely will. Sounds like it could possibly solve all my problems.

[Adrian]

When I looked at the part that was being carved, the 1/16" bit was very obviously trying to cut a path that was 1/8" deep. Initially, I assumed I had set the pass depth of the bit wrong but when I went back to Vcarve and checked, I had it set correctly. I almost hate to try again to verify it without a better understanding of what's going on. $50 a pop for bits can start adding up after you snap a few.

To clarify I had a look at the g-code for the "V-Carve 2[Clear 3]" toolpath and it looks fine to me. The first pass is done at 0.1250 below z-zero which is correct as the start depth is 0.0625 so that first pass is 0.0625. The second pass is at 0.18750 below z-zero which is also correct as that's 0.0625 more than the first pass.

[Solenberg]

To clarify I had a look at the g-code for the "V-Carve 2[Clear 3]" toolpath and it looks fine to me. The first pass is done at 0.1250 below z-zero which is correct as the start depth is 0.0625 so that first pass is 0.0625. The second pass is at 0.18750 below z-zero which is also correct as that's 0.0625 more than the first pass.

Ok, so if the flat depths are correct (1/16", 1/8", etc.), Shouldn't the pass depth for the tool still override the total depth per pass? Sorry, inlays are starting to make me feel pretty dense.

[Adrian]

Ok, so if the flat depths are correct (1/16", 1/8", etc.), Shouldn't the pass depth for the tool still override the total depth per pass? Sorry, inlays are starting to make me feel pretty dense.

That's what I'm saying. It's doing two passes at 1/16". If it's going 1/8" that's because there is material above the start depth. There's nothing wrong as far as the VCarve side of things goes. It's working as it's supposed to. Two passes of 1/16" starting at 1/16" below the z-zero.