I have a design i want to pocket.
At 1/4" end mill i am 12min
At 1/8" end mill i am 45min.
The 1/4 however misses a few spots.
My question is, if i do the pocket in 1/4 can i have the 1/8" do the missing portions. These missing portion can not be highlighted to make another toolpath. Is there a way the system recognizes the spots not done by 1/4". Running the program again in full in 1/8 would mean i should just do it in 1/8".
Any solutions?
rest machining is the term youâre looking for.
If you have CC PRO you can use REST option.
Search âcarbide create restâ and youâll find a tutorial.
If you donât have a copy of CC Pro you might want to try an inside or outside contour toolpath strategy with smaller bits.
example.c2d (80 KB)
What you are describing is called ârest machiningâ, and is available in CC PRO.
A trick that works in the free version is the âpocket / contourâ trick. Like rest machining, you use progressively smaller mills, but there is a limitation - at each step, the next smaller mill must be at least half the diameter of the previous.
So, you can go from 1/4" to 1/8", but not 1/4" to 1/16" inch. To get as small as 1/16", you need three steps - 1/4", 1/8", then 1/16". With real rest machining, you would be able to go directly from 1/4" to 1/16".
Hereâs how the âpocket / contourâ trick works:
This will do more works that real rest machining, but itâs much faster than pocketing with the smallest bit.
Hereâs three text blocks, each about 1.75"x1.25" (so pretty small) From top to bottom, we have here pocketing with 1/16", Pocket / Contour with 1/4":1/8":1/16", and finally Rest machining, 1/4":1/16". Notice you get the same result each time.
As a ridiculous example, I scaled up this test by 9 times - Each text block is now about 16"x11". Now the estimated machining times are:
On larger areas, the Pocket / Contour trick can save a lot of time, and is competitive with true Rest machining.
what is the tool path for the contour? How do you get it to follow the âvector the same wayâ?
Use the same toolpath you used for the pocket. Be sure that Offset Direction is set to Inside/Left (usually the default).
Oops, sorry. Same vector, two different tool paths.
Sorry, still not getting itâŚhow does the contour tool path run through the pocket?
You need two toolpaths - the pocket and the contour. Each toolpath uses the same set of vectors.
Here is a simple test piece. Normally the pocket and the contour would have the same depth. Just for this example, i made the contour a bit shallower, so you can easily see what areas the contour cleared that the pocket did not.
untitled.c2d (84 KB)
I seeâŚthanks. Here is my projectâŚwanting to ensure the bottom of the pocket is smooth. Thought of starting with 1/4 and moving to 1/8. It looks like i would need 2 full passes. Any recommendations appreciated.
wedding 2.c2d (532 KB)
You could also make a small curve like this & contour it at full depth with the 1/8" tool to clean out corners.
But your corners are already 1/8" radius, so you shouldnât need to clean them out with a smaller tool.
If youâre talking about the strip down the middle, just change the stepover to 0.120"
This topic was automatically closed after 30 days. New replies are no longer allowed.
