Question on carving inlays

[Jan.vanderlinden]

I V carve my bottom at .15 deep.
When I carve the top (inlay) why do I have to set the depths at a start of .1 and a finish of .1?
Why cant I just set my start depth to 0 and my finish depth at .2?
Currently with a start depth of .1 with a .25 EM, it causes what I consider to much stress on the machine, and also I have to be very carful or my EM will start to suck out of the collet.
If I could start with a 0 depth, then I could take lighter cuts.
I hope I explained that right.

[adze_cnc]

Jan.

For the top (inlay — a.k.a. plug, male) if you set the start depth at 0.0 and the flat depth at 0.2 the inlay wouldn't go into to the bottom (it would effectively be a mirror image of the bottom...sort of).

In the image above A is your start depth (0.1 in your case) which is the amount of material to go into the bottom. B (also 0.1 in your case) is the gap between the two pieces—commonly used for ensuring a good fit and to slip a bandsaw blade to go between to cut the two apart.

FixitMike has a more detailed image here: viewtopic.php?p=202721#p202721

At the risk of some shameless self-promotion give this gadget a try. It creates "roughing" toolpaths to eliminate the material above the starting depth for the inlay top: viewtopic.php?f=51&t=38767

Steven

[Jan.vanderlinden]

Hi Steven,
Thank you for the reply.
I took a quick read but I only have the desktop version.
However, I do understand you explanation.
Maybe I have to upgrade to the pro version.

Edit.
So now I'm thinking.
Can I just set a boundary (say .25 or .5) around the inlay to get rid of the bulk and then run the normal inlay program?

[martin54]

The software doesn't know there is material above your start depth which is why the bit plunges so far, if you are using desktop & don't have gadgets then you could set up & run a pocket toolpath to get rid of that extra material

Not something I have tried but I would think you could also set your z zero position above the material surface by the same amount as your start depth, that is just me sat here thinking so I might not have thought that through properly

[adze_cnc]

Jan,

You can manually do what the gadget does.

Let’s pretend you want a start depth (SD) of 4mm and a flat depth (FD) of 2.5mm. The pretend bits are 60 deg V with stepdown of 2mm and 1/8 square-end with stepdown of 1.5mm:

• find the largest stepdown of the two bits: 2mm
• create a “VCarve / Engraving Toolpath” (VCE) with SD = 0mm; FD = 2mm
• create a VCE with SD = 2mm; FD= 2mm
• create your regular tapered inlay VCE toolpath with SD = 4mm; FD = 2.5mm

If you regularly use the same settings you could save this as a toolpath template.

The FD for the roughing toolpath is the largest stepdown of the two bits. The SD for each roughing path is the accumulated depth so far. e.g. for inlay SD = 6; FD = 3; max tool stepdown 1.75mm then the toolpaths would have the following values: (SD, FD):

1. 0.0, 1.75
2. 1.75, 1.75
3. 3.5, 1.75
4. 5.25, 0.75
5. 6.0, 3.0

Note that toolpath four’s FD is smaller than the other 1.75 values. This is so that we don’t exceed the final toolpath’s SD of 6.

Steven

[Jan.vanderlinden]

Hi Steven,
That's fantastic information.
I'm going to give it a try.
Thank you for all your help.

[Tex_Lawrence]

You can manually do what the gadget does....

... Let’s pretend you want a start depth (SD) of 4mm and a flat depth (FD) of 2.5mm. The pretend bits are 60 deg V with stepdown of 2mm and 1/8 square-end with stepdown of 1.5mm: ...

I'm curious about what you meant by "stepdown"? Are you referring to what Vectric calls "Pass Depth" in the Tool Database?

[adze_cnc]

Tex,

"Pass Depth" ... yes. Sorry about that. The gadget API refers to it as "stepdown".

It's funny that both the API and the externally facing tool database both use the term "stepover" though.

[Jan.vanderlinden]

Thank you Steven (adze-cnc) for your help.
Your directions worked flawlessly and did exactly as I wanted.
Project is now in the glue up stage.
I will post pictures when its done..

[adze_cnc]

Glad to hear it (both that things worked out and that I might see what you've done),

[Jan.vanderlinden]

As promised, my first inlay.
Not perfect, but overall I'm pleased.
Thanks again for your help adze

[scottp55]

Came out Nice Jan!
Always like cutting off the waste...Kinda like opening a Christmas present...
and finding out if you got socks...or something Really Special!
Congrats!!
scott

[adze_cnc]

I agree it's quite good. Choosing text for your first go is like stepping into the deep end of a swimming pool. If you keep your head above water and can make it over to the exit ladder you've got it mastered.