I am trying to get my inlays to work, so have setup some tests. And, off the bat I have some weird “drill holes” created. They are not in my design or preview toolpaths. Not entirely sure where to look to see what could have caused this?
Upload the file?
Could steps have been lost?
1 Like
Attached. Thanks Will. I may be doing something very wrong, I’m not experienced in this by any means.
Oak_Test_Holes.c2d (140 KB)
The holes don’t show up when the toolpaths are exported to G-code and plotted:
So this would seem to be a mechanical issue where towards the end of the file the machine lost steps, got off-position, and continued cutting just the picking/corner defining toolpaths.
Surprised that the tool didn’t break plunging into uncut material…
Is there a way to prevent this? Obviously don’t want random holes on my main piece, when I get my inlay settings right. Is there something else I can test/do to see why this happened?
Monitor the machine and ensure that steps are not lost.
Usual suspects:
- cord or hose interfering with motion
- insufficient lubrication of linear blocks and rails
https://carbide3d.com/hub/docs/maintenance/
c.f.,
2 Likes
Tell us what machine you are cutting this with.
It’s a Shapeoko 3 xl.
I think Will is correct, you lost a step, most likely it was lost while the TBN was clearing out the “N”.
I watched the Toolpath Simulation, and the toolpath doesn’t start “Pecking” at the corners until after the leftover material inside the “N”'s is done. My guess is that the far left side N caused the belt to skip.
You are only seeing some of the holes because the skipped belt moved everything down, and the pecking happened in Air (already carved away the material). I added the black dots and highlighted where they likely were, just cutting “air”.
Here is where the TBN is clearing out the “N”.
I suggest you fix the N so the Clearance tool can reach that area. See attached.
OLD N is highlighted. I just edited the Nodes a bit to enable the 6mm EM to clear that area. I also removed a few nodes to straighten the lines. You can see that the 6mm tool does the clearancing within the N now.
NOCH SD Guy Edit.c2d (136 KB)
.
3 Likes
I’m sorry, I don’t have anything useful to contribute (the gang has given some really good advice), but I almost laughed out loud at the leading image when my 55-years-ago German lessons made me think
NOCH einmal
NOCH einmal
NOCH einmal
NOCH einmal
(“again, again, again, again”)
I thought the vcarve toolpath doesnt support using a tapered ball nose bit
(Not where I can look at file, but that was what jumped out at me)
John
You are correct. Carbide Create does not support a TBN, but you can still use one.
You just don’t get the same effect as you would if the bit were supported.
I used a tool to generate the tool path, but then actually installed a different tool to run it.
For example, to make the lid of this Salt Vault, a V-Carve toolpath is used, but the tool is a Cove Bit.
In this example, I used a V Carve (vectric), but the tool I selected is a 1.5" Ball Nose Bit
For the Center hold, I used a pocket cut but used a .75 Ball Nose Bit.
4 Likes
Thank you all for your super insightful and quick replies. What a great community!! I will do some maintenance and adjust the shapes as mentioned!
1 Like
Ok, after continuing with my test, the result wasn’t terrible.
Of course the N was a bit broken. I went ahead and adjusted the lettering as suggested to give the main clearing tool space to do the bulk of the work and it seems like the pockets for the new piece worked great.
However, my plugs had some issues.
You can see the plugs have really weird dents. Is this likely from missed steps too? It’s very inconsistent, so it’s doesn’t feel to be a settings thing, but rather something mechanical, like missed steps. I’d love some insights.
Andy_Inlayboard_Inlay_V002.c2d (348 KB)
Here is the file, in case it helps. Thank you all!
1 Like
You are using a 3rd party V tool, one which seems to be quite acute and which I believe has a rounded tip.
Carbide Create only supports sharp-pointed V tools, and a slightly more obtuse angle actually helps in forming a good inlay because the angle is more forgiving.
Try again w/ a 60 degree #302?
See:
This is a good call and good idea, I’ll give this a go! Thanks Will!
Also for TBN bits you want to radius every inside corner to at least the radius of the Tip. i did both the inside and outside corners for consistency.
This a good practice for all inlays. I have found that if the female comes to a “thin sharp point” there is a higher probability that the male side will chip out/have a gap. The thinner the female side the shallower the carve and the shallow carve can give some problems with the male plug side.
Here is an example:
This is a VERY rough example but just to illustrate what I mean here is the updated image:
I believe the Radius for the SPE W01005 TBN is .25 MM, I suggest radius of .3-.5mm for all the corners.
I used a .5MM filet.
