Marquetry - Why Aren't These Two Toolpaths Identical?

[TimSchubach]

Hi all - apologies if this has been discussed and explained already.

I'm experimenting with marquetry on my machine doing pocket and inlay toolpaths. When I create a pocket, I use a 30 degree V and the biggest end mill that makes sense for a clearance bit. In general, the settings I use are Start Depth 0", Flat Depth 0.2". For the inlays, my settings are Start Depth 0.18", Flat Depth 0.1".

Since I don't like to abuse my bits too much, I was wondering if instead of using a Start Depth of 0.18" and a Flat Depth of 0.1" I could use a Start Depth of 0" and a Flat Depth of 0.28". In my head, which can be a dangerous place, it made sense. I created the two different sets of toolpaths in Aspire, and from my eye they looked to be identical. So I made a clearance test cut using Start Depth of 0", and then to satisfy myself that I was right, I ran the clearance toolpath with Start Depth of 0.18" on the same test piece. What I found is that they were NOT the same. The second clearance toolpath, with Start Depth of 0.18" actually cut a little wider that the one that started at 0". I created two other sets of toolpaths, and got the same results. The difference wasn't a lot, but it was noticeable.

I'm guessing that the reason they are different is painfully obvious to some of you, but I'm afraid I don't understand. Can someone please explain? In the future, I can see myself creating a more complex project where the pockets are deeper ( pockets inside of pockets inside of pockets, etc. ), and I don't want my inlay clearance bit hogging out that much in one pass.

Thanks in advance.
Tim

[adze_cnc]

If you are using a v-bit perhaps the following would be more useful than the pocket and built-in inlay toolpath: viewtopic.php?f=39&t=7241&hilit=inlay

[TimSchubach]

Thanks for your reply.

I am using the process described in the document authored by Paul Zank and Damien Durrant, just with different Start and Flat Depths. But that should not make a difference, and doesn't explain why my two toolpaths would not be the same.

[ger21]

With V Carve Inlays, Start Depth has some control over where the edge of the inlay is, changing it's size.

When V Carving, the edge of the tool cuts along the vector. When you change the start depth, you "project" that edge down to the start depth, and the tool follows the vector at that depth. This moves that actual cut edge at the material surface.

[ZipperHead55]

I don't think you have to worry about "abusing" your bits by using the suggested parameters (the suggested start/flat depths, etc). Since you would (should?!) use the large area clearance bits (usually an end mill), the v-bit is only shaving off what the end mill couldn't, so it's not like it's crashing headlong into your piece.

I have done about a dozen inlay projects using a 30degree Kyocera scoring blade/bit, and I haven't had any problems, and I use hardwoods exclusively (walnut, maple, padauk, cherry, purpleheart, oak, etc).

You are overthinking it, I suspect, and I have been there before. It helps to have a good supply of bits handy so that if you ruin one (with bad feeds/speeds) you aren't driving off to the store, or waiting days/weeks for a new bit to come in.

Allan

[TimSchubach]

Thanks Gerry. What you said makes sense, and that's obviously what I was experiencing. I guess my question is, Is there a way to create a toolpath that starts at 0 instead of having to use a Start Depth? So I kinda want to work backwards from a toolpath using a Start Depth to one that doesn't.

[TimSchubach]

Hi Allan, and thanks for your reply. Part of the "abuse" probably comes from a feed speed that's too fast for the depth - I'm still experimenting trying to find that sweet speed. And I definitely do use a larger end mill as a clearance bit. I run the clearance first, so the V-bit doesn't have such a big cut.

On top of this, there is a little "play" in my gantry when the machine takes a healthier cut. Mine is a NextWave machine, and I haven't found a way to beef up the gantry to eliminate that play. Depending on the cut, I can sometimes see the deflection, and that can just ruin your whole day not to mention some good wood. Off topic, but if there are any other NextWaver'ers who've modified the gantry, I'd really like to hear from you.

[ger21]

I guess my question is, Is there a way to create a toolpath that starts at 0 instead of having to use a Start Depth?

Use trigonometry, with the start depth and tool angle, to calculate the offset of the vector. Do the offset, and v carve the offset vector.

[FixitMike]

You can avoid excessive depth of cut for the male with two toolpaths. The first using a start depth of 0 and flat depth of .018. Then run a duplicate toolpath with a start depth of .1 and a flat depth of .28 to avoid making an initial pass that is at a greater depth that what is specified for the bit pass depth.

When you specify a start depth for a Vectric toolpath, it assumes that all of the material down to the start depth was previously removed with a pocket (or other) toolpath. This doesn't happen with the Zank inlay male inlay, so the initial pass of the V bit is made at the start depth plus the tool pass depth. This can be deeper that what you wish. The work around is what I have described above.

[TimSchubach]

the initial pass of the V bit is made at the start depth plus the tool pass depth

Hi FixitMike - Yes, this is exactly why I want to create a toolpath that starts at 0. But I was concerned more about the clearance cut, since it uses a bigger bit, than I am with the V-bit since I generally make the clearance cut first. Then the V-bit doesn't have to plow through as much material.