I figure for Tool path 1 I’d cut the small hole at the top. Then cut out the whole shape with Tool path 2. And finally for Tool path 3, chamfer only the outer perimeter. I plan on using a 90 degree chamfer end mill.
My questions:
How do I isolate the tool path for just the outer perimeter I need to chamfer?
Do I need to set an offset?
My stock thickness is 3mm. I would like to chamfer exactly half way through so to a depth of 1.5mm. Do I just set the the maximum depth of cut to 1.5mm and leave it at that?
My hope is to chamfer the other side of the object as well. I understand I will need to add tabs correct?
You would need to do a bit of vector editing to isolate just that portion of the path, then expand it to a closed region with rounded ends, then do a V carving which cuts that path.
I’d suggest offsetting a bit so that the tip of the V endmill is to the outside of the part edge.
If you could post an original I could work up instructions on doing this — unfortunately Carbide Create won’t allow one to change a closed path to an open, so to do it there you’d need to re-draw it.
I use MOI3D to model, then export to Illustrator where I save the file as an .svg. I have now created an additional path 0.8mm away from the perimeter (based on Stephen’s method). Would this work?
If you use a 0.08" offset, the depth of cut for your vbit will have to be 0.08 before the bit touches the corner of your material (presuming you’re using a 45° vbit). Add to the depth of cut what ever amount you want to chamfer. I usually go with 0.05" to just break the edge but you may want more. Just be careful you don’t exceed the cutting height of your vbit. I usually use a 0.03" offset, as I often use a 1/4" 90 deg vbit with a cutting height of 0.125, so with an 0.08 DOC I’m cutting right in the middle of the edge.
You’d need to do the math (or just draw things up) to determine how wide the expanded stroke would need to be to get the desired chamfer. The specifics would depend on which application you’re using.
To get the desired 1.5mm chamfer we start by drawing a 1.5mm circle on the point:
Will thank you for breaking this down for me. It really helps a great deal.
Could you please explain what you mean by: “We select the lines which make up the chamfer and expand that stroke by that dimension with a rounded cap”.
Also, what kind of end mill would you suggest for this?
I used a #301 and a #122 in the Carbide Create file — I think the #122 might not have sufficient flute length — please check that before committing to anything.
Will, although I changed a few dimensions, I followed your instructions and used Inkscape to create the chamfer tool path. When I import the saved svg file into CC, there is always one path that remains open. Can’t figure out why? I checked it in Inkscape and it appears closed but in CC it appears as a few pink lines.
Could you please let me know what I’m missing? Thanks
You can see that the paths in Inkscape are not closed by selecting the shape and filing it. (again, Inkscape allows it to be filled, which is wrong).
You need to identify where the path nodes are not connected and join them.
If you have difficulty someone more experienced with Inkscape should be able to assist, or perhaps you could do it in Illustrator — it does have tools for this sort of thing after a fashion.
If you’re inclined, it ought to be simple in Serif’s Affinity Designer which is modeled on Freehand, in which application this is a simple checkbox.
The odd little extra movements are caused by Carbide Create converting everything into polylines and said lines not always matching up. Vectric Vcarve can emit G2/G3 arcs, and keeps things internally as curves, so does a better job if you’re interested in a commercial option.
