Duplicating V-Carve toolpath

[tKC]

So I’m trying to cut out the male piece out of Wenge which is hard as a damn rock. I already busted 1 bit on it, so spending more time with the toolpaths before I lose anymore money.

I have went the route of pocketing out the clearance areas in particular zones that won’t mess with the 60 Degree VBit and allows me to make several shallow passes. Using a Start depth of .1 and a Flat depth of .1 I pocket down to .2 and everything looks great in Vectrics generation.

Though the problem is with the 1/4 60 Degree V-Bit, it is sharp as all get out but something tells me if it goes plunging directly in at .1 depth into this wenge I’m going to have a broken or dull bit. So I was wondering if I could duplicate the V-Carve and get the Same results for instance running one at .05 start depth and .05 Flat depth then run the next one at the true .1/.1 I am aiming for? The Preview in the cut looks identical in Vectric software (compared to just clicking v-carve with the settings and the bit), but I suspect there could be some real world problems I might not be considering? Or maybe someone has already tried this to limit the depth of plunge and can speak from experience in it’s effectiveness?

Thanks for your Time and consideration.

[DCK (Dan)]

You can edit the cutter parameters for the 60 degree v-bit so that the pass depth is 0.05". Don’t need to change the flat depth or make two toolpaths to do this.

[tKC]

Well as the Start depth is 0.1 and though the pass cut in the tool setting set to .05, my understanding is then your first plunge will be .15 into the wood as it ignores the first .1 as you have set that as your start depth. I have read that on the vectric forums but correct me if I’m wrong.

[DCK (Dan)]

Honestly, I probably missed a bit in your original post. Sort of zeroed in on the last paragraph and thought it to be a simpler issue. I’d take the advice of the people on the Vectric forum over me, since I barely use their software. I have Aspire, but I pretty much only use it for laser stuff, anymore, and rarely do v-carving that’s not straightforward.

Dan

[tKC]

Yeah I haven’t found any clear guidelines in Regards to duplicate V-Carve toolpaths on Vectric forums as of yet, and as I have been trying to get register for the forums for 3 months now with no responses to activate my account its pretty clear the forums are kind of a cool kids club, so that’s why I’m hoping someone over here might have tried it.

I was looking at the Amana Tool 45730 that has a pass depth of .25 and looks pretty well built, but wenge strenth and brittle ness combined still concerns me when it comes to plunging metal at .15

[Geige (Tom Wert)]

Your post is hard to understand. You should use the same words as the software.

I don’t understand what the flat depth and the surface depth are.

I would recommend to learn what pass depth, step over and clearance pass stepover in VCarve mean. I suggest a google search that will bring you on the VCarve website.

I am not too familiar with vcarves, I don’t of signs.

For my STL files I use a roughing toolpath and a finishing toolpath. The amount of material the finishing toolpath has to remove is determined by the machining allowance in the roughing toolpatth plus a little extra cause by the difference in the geometry between the tools I used for each toolpath.

[tKC]

@Geige

olpatth plus a little extra cause by the difference in the geometry be

The post would be confusing to anyone who does not do V-Carve Inlays and has not studied the method of using the V carve toolpath to do so. I did however make a mistake In the first post exchanging the word “start” for “surface” however anyone familiar with the V carve Inlay process most likely wouldn’t have noticed. As they know very well I am referring to with these Numbers (Hence the Male Inlay)

I am well aware of what Pass depth is, I even figured it in the math in my second post in which I used the proper Definitions of Start & Flat depth, as for clearance and stepover that is completely irrelevant in this scenario. We are discussing a block of wood that is hard as a rock, and telling the machine to start at .1 depth below the top surface of the material so the machine completely ignores that top .1" of the material. When it starts there is when your Pass depth and stepover apply, yet we just plunged a bit to .1" which is what I am trying to avoid.

The clearing out with Pocket tool paths only works in zones of the piece away from where the VBit would touch as it’s the 30/60/90 degree angles that shape the piece so obviously the wood can not be flattened and then expected to be shaped from thin air with the V-Bit.

So the entire thing I’m trying to ask is if anyone attempting to avoid plunging a Vbit directly to the “start” depth of a hard piece of wood has ever instead attempted to set the start and flat depths in increments to simulate a pass depth, having the Vbit run the same paths each time but a little lower and had the male piece (plug) of the inlay come out correctly and fit in the female piece, or have they had troubles with the resulting shape of what the Vbit just cut.

[Geige (Tom Wert)]

The tool will only go as deep as specified in the pass depth in the field that you highlighted.
You could reduce the pass depth to below 1mm or 0.3 inch. That number indicates the deepest that tool will plunge ever.

Path depth and Flat depth have nothing to do with the depth of each cut. The only define the final depth. Vcarves are indeed interesting as I noticed that both roughing and finishing are covered.

In the preview toolpath tab you will see a preview of your cut as well as as every single toolpath (the blue lines).

You will notice that the blue lines will be closer to each other if you reduce pass depth and as well as stepover.

As far as I remember the clearance pass stepover is indeed important for vcarves, in all other cuts (pocket, profile, roughing and finishing) it will be disregarded, so please check it is not too big.

As I mentioned before, roughing and finishing are both covered in a vcarve toolpath, so it seems the clearance pass stepover is basically the stepover in the roughing portion of the toolpath.

[tKC]

Ok so I did some Testing and in short to answer my own Question, Yes it will work.

Those working with V-Carve Inlays understand that if we set our Start Depth at .1 and Flat Depth at .1 as Seen below

The CNC machine is going to ignore the first .1" of our Material and Say if we set our “Pass Depth” to 0.05" The bit will be plunged down 0.15" into the Material before cutting. With our parameters set above it would mean that 2 Passes would be made and the result would be the surface depth at 0.2" deep.
Working with Wenge; I do not want to cut down 0.2" into the surface let alone 0.1" due to breaking bits, but rather take smaller passes so This is how I achieved it.

I first did a Pocket cut, The end result needed to be 0.2" Deep so I did this with 4 Passes using a 1/4 EM DC, and 1/8" EM DC bits.

This allowed for roughly 0.05" passes, while it does take longer my Bits Survived and cut nicely

Now in the Next Step I found the Areas inside the Logo that would use a larger Clearing bit, and i applied the Same logic going after those Areas as well with a Pocket Cuts at 0.2" Deep in 4 Passes with the 1/8" & 1/4" Bits.

These Tool Paths were Sent to the CNC and sure enough everything cut smoothly and no bits breaking.

Now finally to What my initial Question Was, I know i need the V-Carve to be .1 Start Depth & .1 Flat Depth, I know I don’t Want The V Bit To Plunge that far into the surface so What if I try .05 SD & .05 FD, first then running the right tool path will the Shape still come out the Same?
Here is the Results from the First Cut:

Notice inside the nose and brim of hat it has an abrupt stop, that is 0.1" below the surface as we told the bit to start at .05" below the Surface (Z) and it cut down from there .05

With the Final Pass we don’t need to Touch anything or Home The z, I simply ran the Next pass at the desired 0.1 Strat Depth & .01 Flat Depth resulting in the carve being at the final 0.2" depth.

As you can see the results came out excellent and look exactly as they should but here is the Question; Will it Fit Into the Female Piece!?!?!

So I set the Female Piece at 0.0" Start Depth and 0.15" Flat Depth, The Pass Depth is 0.125" so The Bit needs to make 2 Passes to reach the desired depth, The wood is Walnut so I’m perfectly fine leaving these settings:

Now Time For the Glue up & final Result

As you Can See Everything Came out as Expected with the little details such as the Stars Eyes making their appearance. So as mentioned above to my original Post & Question the Answer is Yes for anyone pondering attempting the Same scenario