Help with machining a display panel

[Damon Nabors]

can someone explain to me how to cut a part like the one posted. I took a display panel into ecab and then took it to the parts editor and tried several different methods, but non of them worked. Rather than machining around the center panel, it machined the entire panel. I am trying to take a 3/4 piece of plywood and mill the outer edges down 1/4" so that it will fit into another part. It looks simple and should be simple, but I can't figure out what I am doing wrong. The top and bottom (or left and right as it is shown in the picture) have a 1 9/16 wide by 1/4" deep rabbit, and the sides are 1 1/16" x 1/4" rabbit.

Thanks,
Damon

[David Hall]

As you have discovered, CN does not recognize islands.

I would do this using a DXF file, creating at least two pockets (one "U" shaped pocket for three sides, and the second pocket for the 4th side) making sure the pockets don't share any verticies with each other, or the part outline.

If you must use ecabs, then try the two pocket method described above and cut one pocket .002" deeper than the other.

Alternatively you could profile model this, but that's more work.

Regards,
Dave

[jerry johnson]

Damon, if I am understanding you correctly you do not want the router to outline the panel. If that is the case after you load the file and before you write to cnc open the settings page at the controller and check off outline cuts. Hope this helps.

[Damon Nabors]

I want a flat center panel for a project that I am working on and do not want to make it out of 1/4" material. I need it to feel solid. I have decided to make them out of 3/4" material but I need to cut a 1/4" of the material around the outer edge to create a raised center panel. This way the 3/4 material will slip into the 3/4 rails and styles and leave me with 1/2" depth to apply a molding.

I can draw it up in ecab several different ways, but non of them will allow me to create that recess around the panel

[Damon Nabors]

let me show the picture in a different angle

[Ryan Hochgesang]

Are you getting a tooling error at the Control side? Because the pict. your displaying should certainly nest and cut on machine. You may want to check your Pocket Tool Setup in SETTINGS.

[Justin Melhiser]

Damon
To achieve what you are wanting, you will have to go about it a different way. In the part editor, pocket routines recognize one boundary. Therefore if you draw two boundaries on your part and try to pocket in between them, it will try to pocket from one side of boundary 1 to the other side of boundary 1.
See Pic 1
Now to make this work, what you can do is draw a line that will intersect both boundaries. Offset that line at .001” and trim all the lines.
Now this will create one boundary that is in the shape of a C. Since there is a gap of .001”, it can cut this out as one pocket.
See Pic 2 and 3
Once you have this created you will right click and go to exit then right click again and cut/pocket using closed contour.
If you have any questions on how to do this feel free to call me.

[Dan Voges]

Just curious, do you have the profile modeler on your CNC controller set up?

[Justin Melhiser]

It will not work in the PM because there are no part editor cuts in it.