Thread: First attempt at an inlay : FAIL

Damien,

Watch this video and see where you went wrong
The VCarve Inlay Technique - YouTube

Rick

That bevel technique is interesting.

When I had the laser, I simply told it to OFFSET by the width, with was 0.1mm on the inner piece.

Made another and discovered that the inlay is significantly smaller than the pocket resulting in to much movement during the glue up process. Could tell that the glue up was going to be a complete fail so binned the whole thing.

I am using F-Engrave which is free and exceptionally easy to use so not sure where the issue is.

Damian,
Did you see the video on the F-carve website ?
V-Carve Inlay Using F-Engrave - YouTube

Rick

Yes thanks Rick.

I watched it about 6 times now and read the online manual end to end.

Damian,

If you have followed the video you should end up with a cross section like this

20211014_195755.jpg

Yours looks like this

20211014_195813.jpg

My suggestion would be to follow the video exactly and see how you get on (he was using inches so do the same)

Rick

Got the following reply from the developer overnight.

********
Most of the time the problem you are describing is caused by the v-bit not cutting to a true point, so when it is zeroed on the top pf the material the bit is too low. That causes the v-carved side to be too big and the inlay side to be too small. This can be compensated for by zeroing the z-axis with the bit above the work piece (so that the theoretical tip of the bit is at the top of the material)

The other solution is to buy a bit that cuts to a true point. Bits that cut to a true point will specifically advertise that that is the case.
*******

Makes sense to me and aligns with Rick’s illustrations

Test results this time are better however far from good enough.

This time I did both the pocket and the inlay in one pass (other attempts have been 2 passes). I also set the Vbit slightly above the piece as recommended by Scorch.

There is a lot of vibration in the system when the vBit is running and cutting so thinking I need to invest in a quality vBit. (Any one got any recommendations?)

Also wondering if I need to switch from the hardwoods that I am using to some softwoods?

The lack a parallel in the top line also suggests that my bed is not flat. I did test this and it appears to be flat across that span to a tolerance of around 1/100th of a mm. The cut suggests it is out by way more.

Carbatec for bits.

I get a bit of vibration on larger v bits, try a smaller one to minimise it. Unlikely the issue though.

At the risk of telling you how to suck eggs, you did surface your spoilboard to ensure it is level with respect to the machine?

At the time of my original post I had not surfaced the spoil board as it is a long process and I didnt think it was that far off flat.

I have since done it and another inlay test and the results were actually worse.

I think my $10 vbit is the issue so will stop any further testing until I can get a new bit.

Ordered the Amana Tools 8 piece set. Apparently it will be here from the USA by Friday


Sent from my iPhone using Tapatalk

This v bit technique seems like a headache to me. Whenever I've done CNC inlays I just use the same shape to generate the inlay and the recess, cut out with a 2mm straight bit, clean up pointy bits with a chisel then hammer the inlay in with glue.

I've played around with offsets but in the end I just chamfered the top of the inlay, either with a v bit or with sandpaper, before tapping it in. I'm usually inlaying into Tas Oak so it's soft enough.

This process avoids issues with v bit depth because you're cutting vertical sides - just like when you do a hand-cut inlay (which I've done plenty of too!).

Maybe two things I'd suggest, looking at the second photo the inside corners of the inlay piece (not the writing, the squarish shape) seem rounded and looking at the shape I'm guessing they should be square, not rounded. This might upset the clamping process as the inlay doesn't go in as far as it should, which is what it looks like is happening.

I don't use F engrave so you may need to read up a bit, but I've found that the constant contouring trajectory planner (well with what I am using - Linuxcnc) can shortcut corners like that, Ive seen it when milling circuit boards, the inside angles get rounded but not the outside.

The way I fixed it was to include a G64 in my post processor, which is rounding, so something like this G64 P0.03 will keep the path within 0.03mm and not shortcut. That is actually the setting I use, you may need to experiment to make it suit your machine.

The next thing is it could be the depth setting when you do the inlay, as per Warrick's photo the inlay should push into the vcarved base and there should be a gap between the two pieces of timber.

In VCarve that setting is just the start depth, but F engrave uses prismatic overcut by the looks of it, so that sounds like it sets the whole job down by an amount you set, I usually use 3mm, so the overlap is 3mm which gives a bit of space for glue expansion/squeeze out, if that makes sense. I only do that on the inlay piece, if you did that on the vcarve base piece as well then it won't work.

Good luck, maybe try some small pieces just to save a bit of time and effort, then once its sorted move to bigger stuff.

Russell.

Oh yes definitely softer woods make life easier, or at least a softer wood for the inlay piece with a harder wood for the base, easier to sand down the inlay and keep the surface nicely flat.

Also I just use the cheap ebay 60 degree bits, for around 3-4 bucks each, fling them when they get blunt.

Another trick is to use eurethane glue, it will hide a few sins, this is one I did ages ago, both timbers are pretty hard, the base is Black Bean, dunno what the white inlay was but it was quite hard so the inlay wasn't anywhere near perfect but the missus was happy.

Russell.