Problems with Cavity feature

[mkmech]

Let's say I have a cuboidal hollow box with some features on one face. Now I want to create a door that will replicate those features (as cavity) so that the dorr will close on the box. I used cavity to create the female version of these features on the door. Now I can create a cavity only once I have an assembly with the door and the box mated to each other. The problem is that I once I have the cavity created in the dorr, I want the door to be free so that I can put it wherever I want. But since the cavity was created AFTER I mated the door and the box, if I suppress those mates, the cavity is not valid anymore.

I would appreciate if sopmeone can help me out with this.

Thanks to all

PS: Also, I have some problems with creating the cavity itself. I get a message that SW can't create zero-thickness geometry...

 

[Theophilus]

There are some work-arounds you can use to solve your problem.

First, you need your in-context cavity feature to be stable, so the parts used in making the cavity feature need to stay where they are and not move.

From this point, you can save this part as a parasolid and bring it back into SolidWorks, but you will lose associativity to any changes you make to the original part. If you don't want that to happen, you can save the solid body from your original part--Insert > Features > Save Bodies. This will maintain an associative link to your original part, while creating a new part file. So if you update your original part, your descendant new part (saved body) will update also.

The net effect is that you leave your original part in the assembly (hidden if you like), reinsert the new part for movement, and your cavity feature will remain stable.

Regarding the zero-thickness geometry, what is happening is there are coincident faces (or edges) somewhere that bring the thickness to zero. There isn't a way to figure out the geometry from a logical perspective, so SW doesn't know what you want it to do. Check your geometry and get rid of the coincident faces/edges. For instance, if you try to subtract a smaller cube from a larger cube, and one of the faces are coincident on each cube, simply add some material (extrude) to your smaller cube to fully "escape" the bounds of the larger cube and the error will go away.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.