Hey guys, curious the best way to go about this project… I’m making a custom vent cover for a dehydrator / paint booth.
The image is of the outer cover. It’s 1/4" aluminum. The highlighted tabs need to be 1/8".
So I assume I need to create toolpaths where the tabs are merged with the body, run that, everything will be 1/4", then run a new file where the tabs are separate so I can target them for deeper milling to get them at 1/8" like I need?
If I get it in to my pea brain, You can create a toolpath to cut the 1/4 in tabs deeper to 1/8 in thickness without making a new file. If you have a C2D file we can work it up for you.
Sort of.
This was just covered at:
You need to cut out around the initial outline first, then around the outline plus tabs.
First, duplicate the rectangle:
Second, edit each tab so that it overlaps with the rectangle:
Done
Then select the rectangle, then shift-click on the edited rectangle so that it is the key object:
Boolean Subtract:
OK
Repeat for each corner.
Note that for the ones along the edges it will be necessary to add a node:
Done
OK
Eventually arriving at:
Note that you may want to add dogbones at the corners of the rectangle:
Assuming you are using a 1/4" tool, inset by 0.25 plus 10%:
Select the rectangle and the inset geometry and cut as a pocket to the 1/8" depth:
Then select the tab geometry and the inset and cut as a pocket starting at that depth:
Add geometry and toolpaths for the balance as appropriate:
Feeds and speeds were set up for aluminum, and it was assumed that workholding would not require tabs (see the above link for how to do tabs).
v7 file attached.
outer frame_v7.c2d (108 KB)
You’re the best, thanks for that. Extremely helpful!
Learned some really interesting tricks and techniques from your tutorial. Appreciate you sharing the file too. I’m going to try to follow along and see if I can get it done.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.
