Author Topic: Inlay using V-Engrave  (Read 59479 times)

Offline macbob

  • Storm Trooper
  • ***
  • Posts: 186
    • View Profile
    • Bob Mackay
Inlay using V-Engrave
« on: March 12, 2014, 17:50:01 pm »
Hi There,

I wanted to have a go at making an inlay, using the V-Engrave plugin to cut a beveled edge to the inlay and the substrate.  This allows the pattern to have sharp corners, which is not possible with a simple milling cutter, doing a vertical cut.  Although this must be old hat for most of you, it turns out to be sufficiently complex that I needed to make notes of the procedure.  I thought I would put these out on the forum in case they were of use to anyone.

The aim is to make a sandwich of the inlay material and the substrate, where the inlay penetrates into the substrate, and then, after the glue has set, to mill away the entirety of the inlay material and perhaps a little of the substrate, to leave a smooth surface.  Quite different from the approach used in marquetry, where you simply cut a hole and fill it with a flat piece of the appropriate size.

The point is that the inlay piece should fit really snugly round the edges.  Looking at a section through the sandwich,

- on top there is the block of inlay;
- below that is an air-gap, to allow for slop (A);
- below that is the thin surface of the substrate that is going to get sanded or milled off (S);
- then there is the inlay material that is going to be left behind (I);
- below which is a glue-filled gap (G)
- and finally the underlying substrate material.  See picture!

The air gap and glue gap are there to allow for errors in the cutting.  It is important not to ground the inlay into the bottom of the substrate pocket, so that the tight fit is obtained at the sloping edges.

The starting pattern consists of a number of closed polylines or, possibly, regions. The V-Engrave cut goes around the inside of the pattern for the substrate and around the outside of the pattern for the inlay.  This is then followed by a conventional pocket with a milling cutter to hog out the centers of each region.  The inlay is the mirror image pattern of the substrate.


My procedure was to make four complete copies of the pattern, each in a separate layer.  The third and fourth copies are mirror images of the original pattern.

0 - The original pattern.  Good to keep around!

1 - For the substrate V-Engrave, the ‘Offset’ tool in the Edit menu, specifying a negative offset, creates a new set of polylines inside the existing pattern.  The offset specified should be -tan (theta / 2) * (I + G) * 2, where theta is the angle of the cutter (e.g. 60 degrees) and I and G are the chosen depths for the inlay and the glue gap.  Then, select everything on the layer and ‘Convert to Regions’.  Parts that are so small that the ‘Offset’ tool did nothing, remain polylines.  These can be V-Engraved as they stand.

[Note:  If the pattern includes Regions, and their offsets overlap, it may be necessary to do some manual tweaking using the Subtract tool.]

2 - The second layer is just a copy of the original pattern and will be used to rough out the larger areas of the substrate.

3 - For the inlay V-Engrave, the ‘Offset’ tool is used with a positive offset, creating a new set of polylines outside the existing pattern.  The offset specified should be +tan (theta / 2) * (S + A) * 2, where S and A are the chosen depths for the sanding layer and the air gap.  With the newly added polylines still selected (only), this must be followed by ‘Convert to Region’ and then the ‘Union’ tool, which joins them together just as needed.  Something of a “suddenly a miracle happens” step!  Then, select everything on the layer and ‘Convert to Region’ again.

[Note: If the pattern includes parts that surround other parts (e.g. a border) with a gap that is less than the offset, the border must be handled separately, since the ‘Union’ operation fails - this is due to the procedure generating a Region with two enclosed, overlapping holes, where ‘Union’ does the wrong thing for our purpose.]

4 - In the fourth layer, add an enclosing rectangle around everything, to be used to constrain the outer inlay pocket. 

Note that tan (60/2) = 1/sqrt (3) = 0.577.  tan (90/2) = 1.


OK, that takes care of the layers. On to machining!

We need four MOPS: Substrate V-Engrave and Pocket and Inlay V-Engrave and Pocket, each based on the geometry above.

1 - The Substrate V-Engrave follows the regions in the first layer.  It is convenient to specify a Stock Surface as -S, the Sanding depth.  This allows the cutter to be zeroed at the actual original surface.  The tool diameter should be 0 for V-Engrave.

2 - The Substrate Pocket follows the polylines in the second layer and should specify: a Stock Surface of 0; a Target Depth of -(S + I + G) and a Roughing Clearance of tan (theta / 2) * I, or perhaps a bit less if there are tight corners to get into.

3 - The Inlay V-Engrave follows the regions in the third layer.  The Stock Surface should be -I.

4 - The Inlay Pocket follows the polylines in the fourth layer, including the outer rectangle.  It should specify a Stock Surface of 0; a Target Depth of -(I + S + A) and a Roughing Clearance of tan (theta / 2) * (A + S), or less if there are tight corners to get into.

Once everything has been cut, cleaned, glued and dried, the inlay layer needs to be milled off, down to the level of the Sanding depth on the substrate, if any.  This requires a straight polyline with length equal to the height of the substrate and with Cut Width equal to its width.  Standard stuff!


I hope that these notes are of practical use to someone!

Bob

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8277
    • View Profile
Re: Inlay using V-Engrave
« Reply #1 on: March 12, 2014, 19:15:53 pm »
Ahh... I understand, now, Bob.

Back "in the day", I was a woodworker, doing fine period reproduction pieces -- for our own use.  Mostly mahogany and cherry, in deeply dyed piano lacquer finishes.  French rubbed.

When we did inlays and marquetry then, we cut the pieces with a tapered cutter to obtain the same result you're doing with a Vee-cutter, except our taper was a scant degree-or-so.

I think the very shallow taper has an advantage, in that the inlay really 'jams' into the substrate tightly (when well cut! <G>), any small differences being taken up by the compression of the wood; and thus the edges are very sharp and clean.   We'd usually cut the inlay portion a small bit thicker than the pocket, then scrape or plane it level with the substrate.  Done well, there wasn't a sign of a joint anywhere.  Except for grain mis-matches, which couldn't be avoided, it looked like the substrate simply changed color at the unions.

LLoyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline macbob

  • Storm Trooper
  • ***
  • Posts: 186
    • View Profile
    • Bob Mackay
Re: Inlay using V-Engrave
« Reply #2 on: March 12, 2014, 21:46:35 pm »
But a one-degree cutter could not get into corners, unless it was ten feet long, maybe!

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8277
    • View Profile
Re: Inlay using V-Engrave
« Reply #3 on: March 12, 2014, 22:37:55 pm »
'pends on its diameter, Bob!  I had several, but one a mere 1/64" in diameter.  At 40Krpm, it cut like any other bit, though slowly.

Even with a Vee-cutter, you're limited to a corner radius equal to the tool's.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline billt

  • Droid
  • **
  • Posts: 90
    • View Profile
Re: Inlay using V-Engrave
« Reply #4 on: April 21, 2014, 01:45:08 am »
Bob -
Really nice work, and thanks for the detailed cambam-specific explanation.
The Vectric site has a good description and video tutorial on v-carve inlay in case you had not found this yet.
http://www.vectric.com/support/training-material/bonus/vinlay.html
Now that cam-bam has v-carve I may give this a shot!
Cheers - BillT

Offline macbob

  • Storm Trooper
  • ***
  • Posts: 186
    • View Profile
    • Bob Mackay
Re: Inlay using V-Engrave
« Reply #5 on: May 26, 2014, 21:48:20 pm »
Here is a better example of using the V-engrave approach.  The pattern was thin enough that no substrate roughing was needed, since a V-cutter could reach across the pattern with no need to clear a central area.  Otherwise the approach was as described.

Note: My sister believes that these characters represent her name, or perhaps sound like it.  Please do not disabuse us of this notion unless you really have to - I don't read Chinese!  8)

Bob

Offline Dragonfly

  • CNC Jedi
  • *****
  • Posts: 2310
    • View Profile
Re: Inlay using V-Engrave
« Reply #6 on: May 27, 2014, 09:18:37 am »
How thin a layer you left on the darker part and how did you cut the glyphs? I suppose there is still need for some sanding of the surface after the insets are fitted.

Offline macbob

  • Storm Trooper
  • ***
  • Posts: 186
    • View Profile
    • Bob Mackay
Re: Inlay using V-Engrave
« Reply #7 on: May 28, 2014, 03:04:56 am »
No, No!  The idea is to glue the whole thing up in one go, not to cut out each little piece.  See the picture below.

Have another look at the diagram I drew above.  The walnut inlay is probably 20mm thick.  It fits into the bamboo substrate but is constrained by the 45 degree edges of the shapes, leaving an air-gap between the main inlay plank and the bamboo surface, in this case of 2mm.  There is also an air-gap below the pattern, i.e. the inlay does not 'bottom' in the hole.  Probably full of glue though.  In terms of the diagram, A=2, S=1, I=3 and G=2.  90 degree V-cutter.

In this example, the actual pattern is set up to be 1mm below the surface of the substrate.

The final operation, after the glue has set, is to use a 12mm milling cutter with a single line cut with cut-width equal to the width of the bamboo plank, taking down the walnut inlay 3mm at a time until a final depth of 0.5mm into the substrate, i.e. just skimming the surface.  I had to do a little filling with walnut wood filler, and then some sanding with a disk-sander to take the surface down a further fraction of a mm, bringing the pattern to the surface (or the surface to the pattern, if you will).

The point about this is approach is firstly that you can have a pattern that has detail too fine to get a cylindrical cutter into and secondly that you can have a pattern with many separate parts, possibly fragile, without the need to cut out each part separately and glue each into place, as would be done with conventional marquetry.

My CNC router is made of wood and is not as rigid as it might be, but the results are quite adequate for artistic purposes.


Bob

Offline Dragonfly

  • CNC Jedi
  • *****
  • Posts: 2310
    • View Profile
Re: Inlay using V-Engrave
« Reply #8 on: May 28, 2014, 07:23:13 am »
Ah, I see now. Thank you for the explanation. I could see that the surface had been milled or sanded off to make it level but thought you implanted the letters one by one.

Walnut is a very good material. I recently did a 3D horse figure on a piece of walnut and after the fine pass very little had to be done to smooth and polish the surface.

Offline eastcoast

  • Ewok
  • *
  • Posts: 3
    • View Profile
Re: Inlay using V-Engrave
« Reply #9 on: April 19, 2015, 10:42:11 am »
with bob's help, I have developed a google form to assist anyone who would want to have a go at vcarving inlays.

the links below will take you to a form, and then a spreadsheet where the form will display.

(perhaps there is a way to embed the forms in to this forum?)

I'm still testing this, so I'll make a few notes to help others;-)

1. try something small first.. and make that something cut with as few moves as possible.. (a triangle or a square, would be good, dont be fancy like me and try to cut a star shaped inlay on your first go.)

2. consult your tooling;-) (i.e. check the capabilities of your v shaped bits, it would be nice to have an inlay that its .375 thick but.. I'll bet you dont have a bit to make it happen.


USE THIS FORM

https://docs.google.com/forms/d/1F7Tag-HhfSuXSTtziqFVRJcojuvl8kyoBgEiCKGDBnI/viewform

AND SEE RESULTS POSTED HERE!

https://docs.google.com/spreadsheets/d/1r8OJua8yqh3II8aWdFUZJD8lQxsgi2wrzb_rVZFMnEs/edit?usp=sharing
« Last Edit: April 19, 2015, 10:49:55 am by eastcoast »

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4378
    • View Profile
Re: Inlay using V-Engrave
« Reply #10 on: April 19, 2015, 11:14:13 am »
You don't need any of that Google stuff, a simple script in CamBam will do it.


Here's a quick one I made from another script, I'm a bit short on time just now so I'll tidy it up later.
I think it's doing the maths right.

Edit: added tidy version but just seen some more calcs need adding  :P

Edit2: Right, that's it, v1.2. To be used while reading the excellent info provided by Bob

Edit3: version 1.3 added later in this thread, fixed error with offsets being reversed.
« Last Edit: July 07, 2015, 18:19:40 pm by EddyCurrent »
Made in England

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 2933
    • View Profile
Re: Inlay using V-Engrave
« Reply #11 on: April 19, 2015, 16:54:29 pm »
Nice work Bob. My try this one day. :D
My 2¢

Win 10 64 bit, CB [1.0} rc 1 64 bit, Mach3, ESS, G540

Offline macbob

  • Storm Trooper
  • ***
  • Posts: 186
    • View Profile
    • Bob Mackay
Re: Inlay using V-Engrave
« Reply #12 on: April 19, 2015, 18:05:41 pm »
Not mine - this was eastcoast's doing.  It seems to work fine, although I don't think it should really expose email addresses!

Bob

Offline macbob

  • Storm Trooper
  • ***
  • Posts: 186
    • View Profile
    • Bob Mackay
Re: Inlay using V-Engrave
« Reply #13 on: April 19, 2015, 18:29:55 pm »
Hi Eddy,

I had ago at using your script too - It seems to work very nicely and the maths appears to be correct, given my simple testing.

What is the correct way to install plugins?  I unzipped your file and put the .vbs file into the scripts directory.  In CamBam, I used the Scripts >> open dialogue, which displayed the script code, and then chose Compile, which immediately ran it!  There must be a better way to make this more permanent!

I had a look at the code.  It is always interesting to see how things are written in other languages!  That is an amazing amount of boilerplate to put up a form, but I guess it only has to be written once.

Nice piece of work!

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4378
    • View Profile
Re: Inlay using V-Engrave
« Reply #14 on: April 19, 2015, 18:42:42 pm »
Bob, thanks, but it was easy once you did the calculations.
You are correct in what you said about running the script and making a form, the only way to make it easier as far as I know is to turn it into a Plugin. I can do it if you think it's worthwhile but it will be in C#

Also Bob I see you don't have v1.2 of the script (0 downloads as I write), I added the Target Depth values.
« Last Edit: April 19, 2015, 18:46:04 pm by EddyCurrent »
Made in England