I build a CNC I'm using Carbide Create Pro

[notaquitter (douglas)]

OK I have 2 by 6 laying around I wanna cut it three quarter inch pocket into it but on the front edge I want it sloped for easy part removal How would I do this

[WillAdams (William Adams (Carbide 3D))]

Could you post a drawing/sketch of what you are trying to achieve? Ideally w/ dimensions?

[notaquitter (douglas)]

Here are some pictures

Of course they’re upside down oh I got a headache

[Tod1d (Tod (with 1 'd'))]

OK, so they aren’t dimensioned so I’m just guessing on the pockets
Starting with this

To create a 3D fillet / half-round, you have to make a full round & only machine half of it. It will also round the ends so you need to make the model longer than necessary. And a 2x6 is actually 1.5 x 5.5, so I’ll increase the size of the stock to 5.5 x 16, and move my geometry over 1"

Now create a boundary for a round shape we can subtract from the model. Make it at least 0.75 longer than the pockets. I’ll go an inch longer. And center it on the bottom edge of your existing pocket.

We’ll use the 5.5 x 15 rectangle to create a flat component, and the 1.5 x 16 rectangle to create a round component that we’ll subtract from the flat component.

Now you need to define where the tool is going to run within that shape. A 3D path runs “ON” the boundary. The center of the tool will cut to the boundary, so the radius of the tool will cut that much larger.
I’m guessing you used a 1/4 end mill for the pockets, so we’ll just use the same tool for the fillets. I need to make the left & front edges of my boundary 1/8" smaller than the area to be cut, and to overlap the new path with the existing pocket I’ll make the top/back part of the boundary 1/8" larger.

For display only, I’ll cut out the pockets.
Then I’ll run a rough & finish 3D path on the smaller boundaries.
For the finish path, I’ll run the tool at 90° so the flat of the tool is cutting up the fillet for a better finish

[notaquitter (douglas)]

thanks i do appreciate your help