"Geoffrey" wrote in message news:3f9f100a$ firstname.lastname@example.org... : Cannot belief nobody has responded to my original post. Still waiting for : help. Would really appreciate it if someone can give me some advice. I am : stuch and couldn't finish the model. : Geoffrey, there's a file that I uploaded to comp.binaries as an attachment. It will be the only message there as this is a totally unused NG. The file is called FLANGES.WRL. It is a VRML file exported from a part made to your specifications ~ two walls attached to sheetmetal sides at 135 degrees. It is in VRML format as this is a common standard, it's in 3D so it beats looking at jpegs, the viewers are readily available as browser plugins and using this format avoids all kinds of compatibility problems, e.g., you're on 2001 and I'm on Wildfire.
While there are several ways that might work to make the walls, I didn't try to make them attached to the first wall on a plane with it then bend the tabs to make the flanges. I created flat walls, one on each of the two sides that meet at 135 degrees. You can do this with 'Feature>Create>Sheetmetal>Wall>Flat' Pick Part bnd tbl and Inside rad, then pick one of the edges you want to attach the wall to. It will show you an indicator for a 90 degree bend which is what you want to accept it. Then, it will set up the adjacent surface to the first wall as a sketching plane and also give you two vertices at the ends of this edge as refernces. Now, just sketch three sides of the new wall, snapping the side edges to the two vertex references. (Do not make the sketch cross the sheetmetal face, but sketch away from the edge.) Select done and ok. Set the radius to 0 and this will give you a sharp inside corner on the wall. Using inside rad and sketching away from the attachment edge adds the wall to the outside of the box. If you use outside rad, it builds the walls within the perimeter of the first wall and subtracts from the space inside the box.
Do the same on the second wall and you're done. You don't even have to use corner relief because there remains a small gap between the edges. When you create an unbend feature and pick 'Unbend all', you will see that the walls and radiuses are to the outside of the sharp vertex at the 135 angle. On the other hand, if you had made this as one wall in a single feature, you wouldn't have been able to unbend it, except to 'flatten form' which would treat it as a formed feature. In other words, there are ways to produce this as a single feature, continuous wall. But, if you don't expect to make it that way in production, what would be the advantage of designing it that way?
BTW, the sheetmetal module is difficult and complicated enough to warrant getting some training. Even if you can't get to somewhere that offers the PTC course, at least try to get something from CADtrain or FroTime. Anything would be a help, seeing as how you didn't get very far before you got stuck.