A simple way to make inlays

[adze_cnc]

I have tried numerous sets of number for both male and female with different start depths and finish depths.

Please don't take this is in a bad way but this says to me that you might not quite understand the interplay among the three base values—inlay-material, air-gap, and glue-gap (A, B, and C in my post above). The B and C values in a way don't really matter at all. They could both be zero* and I could get an inlay to work properly no matter what angle v-bit I was using.
 

Star with both B & C (air-gap and glue-gap) set to zero set to be cut with a 90 degree v-bit

 
When glued together the plug and base will touch on all flat faces (at the surface and in the pocket),

* technically the "V-Carve / Engraving Toolpath" requires that the B value to be non-zero (e.g. 1/1000 of an inch).

Should the numbers be the same regardless of the VBit angle. I'm taking 15 degrees to 60 degreees.

Perhaps. It really depends on the design you are trying to do. For example if I were doing the following simple star using a 30 degree v-bit I'd get this result:
 

 
But if I were using a 90 degree v-bit I'd get the following result:
 

 
Both are using the same A, B, and C values. It may not look like it in the images but the flat depth of the star in the base and the flat area depth around the star for the inlay plug are both the same with both 30 and 90 degree v-bits.

Is one better than the other? Not really. But, I'm more likely to have a 90 degree v-bit. And the slope for the 90 degree v-bit provides a larger glue area which might prove usefull.

It seems to me the VBit engraving angle impacts the the cuttng depth numbers.

It depends. For the star above not much. For a design that has fine features the steeper the bit (smaller included angle) the more potential for material to fit into the base and the less potential for chipping of delicate material.

So it's better to say the the design might dictate the choice of the v-bit. Some of those cutting boards created by Stephan Forseilles need a seriously steep v-bit (small angle) for the tiny lettering and thin lines to have a reasonable amount of material inlaid into them.

The following design uses the same values for A, B, and C.

This one cut with a 90 degree v-bit has many areas on the plug (and in the base) where is details come to a sharp peak. If this was delicate material there could be much chipping. Also, some of those peaks might have less material than I want to inlay into the base.
 

 

 
This one cut with a 30 degree v-bit has far more flat areas on the plug allowing less chance of chipping and a better chance that the the full depth of material will inlay into the base.
 

 

[RHT9774]

I am having same issues as EMoloney. I have simplified the design to circle inlay. I am trying a deep inlay. I am using a 15 degree engraving bit with a bottom flat dimensions of .02. The circle vector is set up to be 3.75 inches. What I found is the diameter of the plug at the point where the plug is supposed to contact the pocket at the widest point is only 3.70 inches in diameter. I am consistently getting this kind of gap. The router tool inputs has the flat dimension in it. But I can’t help but think that some how the flat dimension of the engraving bit is not getting accounted for in the VCarve.

But that is just a last desperate grasp at straws. However, if that is the issue, is there a work around? Any other helpful tips are greatlt appreciated.

[adze_cnc]

Without images or a CRV file this is going to be well nigh impossible to diagnose.

But, having said that, if all you are doing is inlaying a circle into something why not do so using the builtin "Inlay Toolpath” with a square end cutter? See here.

[RHT9774]

I started with a more
complicated design but because of my own problems, I simplified things to try to self diagnose my problem. I can up load a crv file tomorrow. Thank you.

[RHT9774]

I want to say thanks again for the effort to help.

Here are two of the files. One is a rectangle, the other a circle. I know they are very simple shapes but I figure if I can't make this work, then no need to work on hard shapes.

[adze_cnc]

I've had a look at the circle file. As far as the rectangle goes, as FixitMike so ably points out at this post using an engraving bit (especially one with such a large flat) wouldn't work anyway.

The circle project would work as it doesn't have any sharp corners. Above you mention that it is a 3.75-inch circle. But, measuring the actual vector within the file I find that it is 3.79 inches in diameter.

But I can’t help but think that some how the flat dimension of the engraving bit is not getting accounted for in the VCarve

We're at version 11 of the software (more if you count the x.5 releases as being significantly different). You'd think that with the myriad of users and "The Johnsons Live Here” signs cut that someone would have noticed the omission.

It seems more likely that a combination of factors could be at issue:

• what if the bit doesn't really have a 7.5 degree side angle?
• what if the flat is not exactly 0.02 inches?
• what if the router bit is not truly (or closely) perpendicular to the machine bed? i.e. it needs to be "trammed”.
• what if the material surface is not parallel to the machine bed? (Could be cupped, not held down flat, etc.)
• what if there is flex in the machine as things are cut?

Your toolpaths look logical. You are actually missing one. You go from start=0; flat=0.08 to start=0.16; flat=0.08. You are missing start=0.08; flat=0.08.

My only quibble with them is that you don't really need 8 toolpaths (your 7 plus the missing one). Your engraving bit has a pass depth of 0.08 and your 1/4" bit 0.125. You could base your start and flat depths for the toolpaths using the larger of the two values (0.125 in this case).

Using your tool specifications, your geometry, and your material settings I created the attached file as how I would do this if it were me. Rather than using a 0.125 pass depth I used 0.130 inches. The amount of material you want inlaid is 0.52 inches so by using 0.130 I can save one toolpath (0.52 / 0.130 = 4 ; 0.52 / 0.125 = 4.16 round up to 5). The extra depth is a sheet of paper in thickness. If your machine can't handle that I would be surprised.

I then ran those toolpaths after your toolpaths in simulation. They didn’t cut any extra material that your toolpaths did. I reversed the order simulating my toolpaths then yours. Again, they match nicely.

You're on the right track. Again, the toolpath creation method you are using is sound (pass depths not withstanding).

How about using the circle or square file and try to create things using a 60 or 90 degree included angle v-bit (not engraving bit) and see how that works?

Steven

PS. If this file is going to be cut then toolpaths in the CRV file need to be 1) verified that the bit settings are correct—I tried copying them over as best I could (even using tool #4 for the end mill) but I am fallible; 2) recalculated—they are not calculated to make the file size smaller (88,000 bytes versus 1.1 million).
 

[RHT9774]

Thank you Steven.

I will be working on it today.

[RHT9774]

Rather having to manually run each different toolpath, is there a way to have the software automatically batch together and run simultaneously all the same type of tool paths like clearing paths and then run all the same shaping paths?

[Adrian]

Rather having to manually run each different toolpath, is there a way to have the software automatically batch together and run simultaneously all the same type of tool paths like clearing paths and then run all the same shaping paths?

When you save the toolpaths you can choose the "Visible toolpaths to one file" option and all the toolpaths with a check mark next to them will be saved to one file. They must all be the same tool number and have the same geometry if your post processor doesn't support tool changing.

Another method (if you're using the Pro version not Desktop) is to use the Merge Toolpaths tool to create one toolpath from all the separate ones.

[RHT9774]

Just wanted to loop back and say thanks to those who helped me with the V Carve inlay suggestions. I finished my little project and could not have done it without them.

This may be repetitive but for me the most important basics I can reiterate are:

1) Engraving bits did not work in V Carve and provided me with endless headaches. Once I changed to a round nose end mill on the deep inlays, everything started fitting. Thank you.
2) The Dust boot will damage fine plug work. I stopped using it on the fine work. Another big time saver.
3) Plugs are mirror image. I know. Again, very basic but I made this mistake enough times even after telling myself not to, that it deserves repeating for those who are slow to learn like me.
4) When setting up a round nose end mill, Vectric inputs are for radius, not diameter. Another stupid mistake that cost me a few hours of frustration.
5) Group like tool paths into one g code. Again, another basics tip but it really saves time when layering multiple plug V Carve and clearing paths.

I attached the final product. And even though there are a few mistakes, it made it to the final gift phase.

Thanks again to those on this forum who helped.

[Custom carving]

great work that is a beautiful piece thanks for sharing

[larryh]

LithgowShredder: Thanks for the PDF file. The image on page three is really useful. To me, though, the top image on page one is still needlessly complex.

I've posted variations of the following in answer to questions on other threads. I'm consolidating it here as it's getting tiresome trying to search for past posts to provide a link to when the question comes up again.

I am going to give values here for an imaginary inlay project. Substitute your own numbers for your own project/needs.
 
inlay.png
 
For the tapered inlay process you only need to determine three (3) numbers—the values for A, B, and C in the image above. From these all start and flat depths can be determined.

• A is the amount of material to inlay into the base
• B is "air gap": the amount to leave between the two pieces
• C is "glue gap": the amount for glue squeeze out and compensation for ill-fit

For my imaginary inlay project I'll use:

• A is 6mm
• B is 3mm (I'll separate the base and inlay with a 30" bandsaw that has a thick blade)
• C is 0.75mm (I'm thrifty with glue and my design shouldn't need a "fudge factor").

Now for the start and flat depths:

• Base/female start depth: 0mm (always*)
• Base/female flat depth: A + C (6.75mm)
• Inlay/male start depth: A (6mm)
• Inlay/male flat depth: B (3mm)

That's it.

Now, my bits might not be able to plunge all the way down to 6mm+ for the inlay/male piece. For that case I created a gadget the will create "roughing" toolpaths to eliminate material above the 100mm start depth. See: viewtopic.php?f=51&t=38767

If you are using VCarve Desktop then the gadget won't be available to you. See: viewtopic.php?p=282314#p282314 for a manual method to emulate the gadget.

Steven
 
 
* = I say that the base start depth is always zero (0) but if I was inlaying something in the bottom of an 8mm deep pocket for a tray I might set it to that depth. Let's master the simple case first though.

Ive used this method a dozen times or more and its served me well using vcarve desktop pro V10.5. Ive since upgraded and have V11 and V11.5 installed now as well. If there were every any issues it was due to mu belt driven machine. I solf off my old CNC and got a onefinity and now for the life of me cant get a good fit, all the plugs have noticeable slop. Im basically just trying to do a .2" deep inlay in the shape of a baseball diamond base lines. A triangle with an arched end and a center island. The whole thing about 8" across and reduced to a bare minimum of nodes.

Whats ironic is I recently did a test to the same depth with same bits that was only about 2" across and had a nice tight fit. So why would the 2 different shapes be giving me wildly different results? Thinking it may be something strange with the vectors I went so far as to create a new baseball field inlay vectors and tried again, still sloppy. This is all leading me to believe its either the post processor or the way vectric is generating the tool paths.

More testing is needed but has anyone ever encountered anything like it?

[Adrian]

More testing is needed but has anyone ever encountered anything like it?

The basic test to eliminate any possibilities of issues from version to version is to run a file with the same settings but generated from 10.5

My suspicions would be the different speeds and loads involved in running a 2" job compared to an 8" job. Movement will be much slower on the smaller piece unless you're running at a very low feed rate to start with.

[larryh]

Well, isnt that interesting. So I saved the SVG (basically just an outer loop and an inner loop)( out from V11.5 project. Imported it into a V10.5 project. Then I selected both vectors, copied to new layer and with both selected flipped horizontally. Then selected just the outer most loop/vector and created an offset of it to use as the area to clear when making the male plug. used vcarve tool paths for both the pocket and the plug, .250" end mill for clear and amana 6 degree TBN 6 for profile. The end result was a nice snug fit so there seems to be a difference in the way V10.5 and V11/11.5 create the tool paths.

[Adrian]

Well, isnt that interesting. So I saved the SVG (basically just an outer loop and an inner loop)( out from V11.5 project. Imported it into a V10.5 project. Then I selected both vectors, copied to new layer and with both selected flipped horizontally. Then selected just the outer most loop/vector and created an offset of it to use as the area to clear when making the male plug. used vcarve tool paths for both the pocket and the plug, .250" end mill for clear and amana 6 degree TBN 6 for profile. The end result was a nice snug fit so there seems to be a difference in the way V10.5 and V11/11.5 create the tool paths.

Now load the 10.5 project into 11.5, recalculate and save the toolpaths using exactly the same post processor that you used in 10.5.