F engrave inlay testing

I’m sure you’ve looked, but you can see the screens in the video here:

1 Like

It looks like your v-bit might not cut to a true point. This is common for hardware store v-bits. If this is true, when you zero on the top of the wood the bit is lower than it should be because the bit is missing the tip. (there may be a pointy tip but if it is off center it gives the same effect)

If the bit is zeroed too low the v-carves will be a little too wide and the prismatic side will be a little too narrow. That is what I think I see in your pictures.

If you send me the g-code files I can check if F-Engrave is at fault. (my e-mail address is in the help menu under, Help-About)

1 Like

I recieved your files. I will evaluate them tonight. Anything I say before that would be a guess.

The lines in your pictures should not be the same distance appart since the cutter is tapered.

1 Like

Is there a start depth option? I am yet still waiting for my x controller to ship to be able to actually get my machine fired up so I have not actually cut anything yet, but I have been messing around with v carve pro in the mean time and there is an option there called start depth which comes into play for inlays to help get the inlay to seat fully into the pocket and leave a small gap underneath for glue and such. Not sure if this is your problem, but it sounds like it could be relevant, I am just now sure how it would translate into f engrave as far as options.

Maybe it doesn’t matter and the void between the v and the flat bottom are to make sure the interface isn’t glue-starved? Isn’t the void buried inside the work so you won’t see it?

Phil, I took the g-code files you sent and ran them through CAMotics (Open source CAM simulator).
I used a sharp 60 v-bit and the results are shown in the first picture below.

The next picture shows those shapes exported to STL files and assembled in OpenSCAD. The fit-up is correct. I don’t see any problems with the way you made the g-code files. (It does look like F-Engrave missed a bit of cleanup above the “i”. (I am aware that sometimes this happens. I am planning to look into it soon.) The yellow cylinder in the picture was a visual aid for me to ensure the prismatic over cut was working correctly.

Based on these results it seems that F-Engrave is working correctly (with the exception of the cleanup issue).

I went on to introduce a small 0.030" flat on the tip of the v-bit cutter. The following results show what happens when the cutter does not cut a true point. The first picture shows the incorrect fit up that occurs. The second picture is an attempt to show the comparison between the sharp tip v-bit (yellow) and the v-bit that is cutting a small flat (orange). It is a little difficult to see but the orange parts exhibit the the same pattern as your pictures. The v-carved parts are wider than they should be and the prismatic parts are thinner than they should be resulting in an improper fit.

I don’t have any specific experience with the CMT bit that you are using but I do use a different CMT bit that does have a sharp point. CMT calls them “laser point” bits to differentiate them from the other bits. The laser point bits are more expensive about $25 vs $12. (CMT Laser Point Bit - Amazon Link)

1 Like

You may not see any flat on the bit. The bit may not be flat but it is cutting a flat.

If the point on the bit is not concentric with the shaft it will cut a flat. Also if the spindle has wobble the machine will cut a flat.

The best way to check it to start the spindle and slowly lower it until the bit starts to make contact with a piece of wood ay the point of initial contact there will either be a pin point spot or a spot with a diameter. It is best to use a piece of very flat finished wood or a piece of scrap from cheap partical board furniture so it is essy to see the point of contact.

I see your latest post now. Flat found without lowering the bit…

See my link above to the CMT Laser bit for s cheap bit. It is the cheapest I have found.

A flat tiped cutting bit can be used to make an inlay you just need to figure out what the diameter of the flat is and set the z=0 above the workpiece accordingly.

Zoffset = (D/2) / tan(bit_angle/2)
D=diameter of flat
bit_angle=v-bit tool angle

So when the bit is touching the top of the workpiece z = -Zoffset. The offset should be used on both the v-carve and prismatic cuts.

1 Like

I use them a lot:

If you need bigger I can’t recommend enough this guys:


1 Like

I might have linked you wrong thing, I’m not any close to my stuff I’m sure they have both directions available.

1 Like

Unless it has a reverse, a router spins clockwise.

1 Like

I like the WhiteSide Vbits


In any case, this is more about direction of chips load not necessarily cutting direction. I do 90% of my stuff in plywood and down cut bits give best results with decent dust collection.

1 Like

I love Whiteside bits for regular woodworking in my 3.25HP Hitachi M12V. You can find them locally at woodworking stores and better lumber yards.


I had an error in the formula I posted earlier. It should have been divide by tan() . I edited the post accordingly.

For a 60 for deg bit it is safe to just raise the bit the distance as the flat diameter. (Too much is better than too little)

1 Like

I just started experimenting with F-Engrave and generated a first set of normal, prism, cleanup and v cleanup files.

I then bring them in camotics and they seem as expected… only to realize a minute later that the (straight bit) cleanup takes place in a single pass!

My initial settings were
Cut Depth Limit: -4mm
Prismatic Overcut: -2mm
Cleanup Cut Diameter: 3.175mm
Cleanup Cut Step Over: 40%

That would require a 1/8" bit to clean up 6mm deep in one pass (and probably break). To correct this I guess I would have to use a combination (or all) of:

  • cut less deep
  • overcut less deep
  • cleanup with a larger bit
  • use lower step over

I was wondering whether there should be a “Cleanup Cut Step Down” setting as well…

Rrrright… so, how did 162% [ =(0.125+0.0625)/0.116 ] work for you? :smile:

My point is… it would be helpful if the cleanup in F-Engrave could be done in multiple passes with configurable step down. Otherwise one has to work around this limitation by cutting shallower and/or using a larger bit and/or smaller step over.

Yes, but this refers to the V-Carve toolpath. What I am talking about is the (straight bit) cleanup toolpath.

If you turn on V-Carve multipass, does the step down apply to the cleanup as well?

1 Like