I am trying to cut word inlays with my Shapeoko. I have seen the videos for the advanced v-carve, I have to watch more to learn that better. However I want to just create an inlay with words using a 1/8" straight cut bit. I can’t seem to get the sizing correctly. I am pocketing the one side so the word is read backwards. The other side I am pocketing just the word, and they do not fit inside each other. I am not understanding why if the words are the same size when they are created in carbide create the inlay doesn’t fit inside the other side. I have been messing with the size of the letters but I feel like I can’t be the only one who has tried to do this. Any help I would greatly appreciate!
How far off is it?
It’s not as simple as just making a pocket and a profile. Your endmill has a radius…it can not cut an internal corner with a radius less than that.
Can you share a screenshot of your font?
I don’t need to be belittled for asking a question. I am obviously not as knowledgeable or talented with the machine as you. I am simply looking for help and trying to give as much information as I have about the problem I am having right now. I understand there needs to be room so the inlay actually fits in. I didn’t know if there was a way to do that. I tried the offset but wasn’t sure how much the offset needed to be with out the inlay being too loose.
so one trick with straight inlays is that you need to make sure that all corners are “round enough” for your bit.
Since you have an 1/8" bit you can ensure that with the following steps in carbide create:
Use the offset tool to create an outer offset of 0.0625, and group the result of that.
Use the offset tool to create an inside offset of 0.125 of the result of step 1 and group that
Use the offset tool to create an outer offset of 0.0625 of the rsult of step 2 and group that
the result of these steps has the same size as the original (you grew it by 1/16h, then shrunk it by 1/8th then grew it by 1/16th) with one key difference: All corners, both inside and outside, now will fit your 1/8th bit without leaving the “round bit leaves stuff in the corner issue” making it useful for inlays
so the key is the sharp corners, ilke in the top of the “d”. Your round bit can’t do those perfectly on the bottom cut, and will leave a bit of wood behind.
On the top cut, it can do that corner perfectly… but that little bit left behind will cause the piece to not fit.
if you follow the 3 steps of contours I posted, it will round off those edges so that there is nothing left behind… and the fit will be a lot better.
Making the inlay part a little smaller in addition can help, but frankly,. that’s by far a secundary problem compared to the “round corner” problem.
(before I figured out how to do V based inlays I did quite a few straight inlays… and never did an inside contour for the fit, just the 3 steps to deal with he round corner problem… if there was too tight a fit it was never much and a tiny bit of sanding with sandpaper would take care of that)
I will be honest, that made no sense to me but I did it and it seemed to work. I lost the center in my d, but I can see the rounded corners you spoke of. I am curious, is there a better font I can use that’s already rounded over?
Also, now for programming my actually inlays, do I still need to reduce the size of the male side to fit into the female side?
it depends on how much you hate sanding
reducing a tiny tiny bit, say 0.005 or 0.01 makes the fit easier, but you run the risk of too loose fit.
basically what you’re compensating with this reduction is the size of the bit maybe not being a perfect 1/8"… but only very close.
One thing you can do is to cut first the inlay part, and only then the “socket” part… and leave the socket part on the CNC, and do a test fit. If it’s too tight you can always then recut the socket a tiny bit larger… (since you kept the zero position/etc in tact)…
I really appreciate all the help, thank you so much. I never would have thought reducing then enlarging and then reducing would have help round the letters over like it did.
Say for a cut out, not words, like a heart shape or animal shape, do I have to do the same thing?
yeah it’s a generic trick… I do it for other shapes too. Not all shapes have sharp corners of course… but it doesnt hurt the cases where there are no sharp corners.
Note that if a detail is too small to cut, it will disappear with this… but it’s too small anyway and will never fit., at least you’ll see it before you cut it out,
Inlay is the prime reason I got a Nomad. I’m not an adherant of the v-carve inlay method, it’s all straight end mills for me.
I use the same lines for both the inlay and the field, I don’t create offsets. But when I mill out the field, I use a phony bit entry, based on the bit I intend to use, that I specify as being slightly smaller than the bit really is. This will result in a “fat” cut, making the pocket a tad larger than the inlay. I typically resize the bit’s diameter by 0.05 mm but that may vary depending on scale and materials.
