I believe you will need to draw in the circles again, but otherwise it all sounds reasonable — I’d try a test cut in a piece of easily cut scrap before committing to alu.
1 Like
Finally got time to try cutting out a version in wood, and I’m running into a strange issue. Work file is attached, it always says 2 minutes estimated time to do a full contour or pocket into 1/2" thick wood. I triple checked all the settings and switched everything around in many ways. Any advice on what went wrong?
problem.c2d (80 KB)
This is a very small part.
I was able to get a time of 16 minutes:
by reducing the feed rate from 65 IPM to 16:
1 Like
Hmm I’ve been playing around with things but I’m getting confused. I think my design is a bit unintentionally overly-complex… but it’s forcing me to learn.
Here’s the current issue I’m facing. Running step 1 (contour path) is easy, but then once it comes to pocketing the gripper areas things get extremely confusing. I’ve been trying to make some kind of workaround but it’s not clicking what I need to do.
You need one (or more) piece of geometry for each sort of toolpath which you are trying to cut.
See:
Things aren’t clicking for me. I don’t understand why an offset was added, or why the nodes were edited in the example. For me it would make sense to just create the shapes to be pocketed with capped ends (and correct channel dimensions). I think my brain maybe trying to cheat and find an easy solution instead of actually understand lol.
I thought of using a contour for one of the grip handles, but it creates issues at the bottom of the handle:
The offset was added and the nodes edited because there were two different outlines, an upper one:
and a lower one:
You need separate geometry for each level at which a design will be cut.
Consider cutting a Ziggurat:
First level is:
Second level is:
Third level is:
and when we preview this we see the need for the offset geometry and larger stock:
So:
Apply
Edit all the toolpaths to use the offset geometry instead of the original outer, then add:
which previews as:
So obviously the outer geometry should be larger w/ dog bones:
1 Like
Something like this?
Circle has an inner contour (it seems to have many sides for some reason rather than a perfect circle)
Custom poly shape would be a pocket.
If you will post the .c2d file and also a side view drawing which shows the various depths we should be able to walk through making this with you.
Really appreciate your efforts to help me out. Wish I was picking up on it a bit faster, I think once I see the result it will all make sense.
Files are attached.
c2dfile.c2d (160 KB)
Your most recent SVG contained 6 paths (some of which could be broken into separate paths themselves)
I took the path that defined the outline and combined it with a circle with the same diameter as your center to achieve the SVG I shared above. It’s not perfect because the diameter of the center portion on your original was inconsistent (not a perfect circle).
2 Likes
First, simplify things down to just what is needed and a matching stock size:
Then select the largest part geometry and offset by endmill diameter plus 10%:
Apply
Add the circle to the selection:
Assign a pocket to a depth of 3mm:
Select the outer part geometry and the offset geometry:
Assign a toolpath which starts at the bottom of the previous pocket and cuts down as deep as is needed:
which previews as:
Machine a mirror imaged negative of this as a fixture, insert the part into it, the cut the first toolpath registered w/ the fixture to complete things.
1 Like
Thanks, you guys are a huge help!!
I managed to recreate it:
Honestly, never would have figured that out so I really appreciate you taking the time. It makes sense now that I seen how it applies to my project. I should be able to apply the technique to new projects in the future 
Would you mind sharing speeds and feeds for a 60 degree vbit? I’d need to add it to my tool library for both wood and aluminum. It’s this these ones here: Amazon.ca
Machine a mirror imaged negative of this as a fixture, insert the part into it, then cut the first toolpath registered w/ the fixture to complete things.
What do you mean by first toolpath registered with the fixture?
I can predict I’m going to have issues zeroing the part once it’s in the fixture. Any ideas on the best way to proceed?
We have feeds and speeds for a 60 degree tool we sell for use in wood/plastics in Carbide Create:
Most V tooling is too delicate for aluminum, unless one avoids engaging the tip and only cuts using the edge.
The idea is:
- mount a piece of stock of a reasonable thickness (greater than 3mm)
- make a greater than 3mm circular hole in it which is large enough for the circle to fit into:
- cut that in a suitably stable piece of stock securely clamped in place
It may be helpful to make the origin the center:
With the stock in place, clamp the cut part in place so that it is secure.
Set up a toolpath which uses a mirror image of the offset geometry and has the sides cut away so as to admit the clamps:
Then subtract this shape from the outline:
OK
Assign a 3mm deep toolpath:
1 Like
Thanks again Will for coming through with some amazing instructions. I’m going to have a few questions once I get going on that (tomorrow).
Today I just had a bit of time to play with the vbits. It’s important that I can get them to work with aluminum because pretty much everything I’ll be making and selling requires it.
I did some quick tests and have some promising things to share (attached).
The more conservative depth per pass seems a bit nicer on the machine (less noise). It’s not really making chips very well at that DOC but it seems to work anyway lol.
The bit seemed to hold up well after the small test. Whats seen in the image that looks like a rounded over edge is actually just aluminum that I was able to pick off. No heat on the bit at all.
I did an initial pass then a clean up pass to remove all the build up.
Videos of the test cuts:
I’ve run into a problem and it’s a bit confusing. Been playing with it for a few hours and I’m not sure if there’s anything I can do to fix it.
When I create the offset at 0.125" (exact measurement of endmill) the edges of my design stay nice and sharp and crisp. When I add the 10% it starts to round over. That 10% is directly impacting the material being cut away from my edges leading to rounded grips (see attached image).
It seems there must be a solution to this but I’m unable to find it.
I assume the 10% is added to prevent slotting around the entire workpiece causing premature wear to the endmill. I could reduce it to 2-5% and the rounding would be less, but it’s still negatively impacting the design. Any solution to this?
10% also ensures that the calculation will be certain of admitting the tool.
