I am trying to model a part that basically looks like the attached BMP file.
I am having no luck getting the full radius on the area of the part where it goes up at an angle.
Can anybody give me some ideas on what to do?
How do the two views relate to each other?
If the upper view is the section being extruded, the bevels at the top LH corner of the angled portion will not be do-able in a SM part.
Not really it. The part is only .03 thick sheet. bent around a 2.44 R I have tried drawing the flat and doning a sketched bend and there is always part of the part that stays flat. I tried calculating the length of a 180 degree part figuring I could cut away the excess but that isn't working, at least not the way I am doing it. I have done a thousands of machined parts but very little sheet metal, so you'll need to walk me through it.
That did it thanks.
Now I see the key was creating the fixed face (Extrude2) that you cut away later.
I still wouldn't have known how to do the following steps, this was an excellent tutorial for me.
I think in 2008 and I know in 2009 you can select an edge to create a sheetmetal part instead of a face.
Not necessarily easier ... just a different method.
Old method = make a solid first, then convert to Sheet Metal.
New method = create Sheet Metal part as the first feature.
Each method has its merits.
I will laser the blank and then roll form. I only neeed 30 pieces.
Thanks but I'm still in SW 2007, couldn't open your part.
I appreciate your trying help, as I said I'm really weak in sheet metal.
I have some questions for everyone here.
1. Why are you, Tony & Kelvin, putting the extra flat extrude on at the beginning? I suspect it's because there used to be a limitation, but that's not necessary any more. I just put in the arc as a single line, then create the base extrude straight from that single arc. Then insert the unfold by selecting the end edge as the reference, make the shape cut, and then fold. Done. Kelvin, you basically did that as I would do except you added the flat nose on it and then cut it off.
2. When I open Tony's part in SW2010 and hit the Flatten button, I get an error that I can't seem to fix after that unless I suppress the Cut-Extrude5 at the end. Then it will flatten ok, but of course that leaves the part wrong. I presume it works fine in 2007 (correct?) where it was created. I would like permission from Tony and James to work on this some more and then submit this to SW Beta to see if we can figure out why I get this failure in an "old" part.
3. And related to that permission, I would like to have your Okey-dokey to use this in my sheet metal presentation. I know, it's basically public here, but I like to have the owner's permission before it's published in my presentation.
Just another thought for you. If you are going to roll these parts, which makes sense, are you going to use a tripod roller? If so, you may want to leave an extension on each end and then trim that off after rolling. Otherwise you will have a flat section on each end. Or you can hit both ends with a form die to preform the ends, or you could do it after rolling, or you could roll on a urethane roller. Just some thoughts.
I just figured out that I can get the Tony part to work if I suppress the cut at the end, then hit the flatten button, then unsuppress the cut. At that point I can hit the flatten button to go back to the formed view and then use it at will. Works fine after that.
If I edit the Flat-Pattern1 feature after that, I see that it has selected the lower edge as the fixed face. I find it interesting that if I try to pick the upper edge it won't let me. I can pick the edge face of the material but then it will fail. It has to be the lower edge. And if I manually go in and pick that edge to start with, the part will still fail. Interesting, eh?
Wayne ... I added the flat portion because it wouldn't let me select an edge for the Unfold feature (at home). I was surprised as I thought I had done similar before, but was too tired to look into it.
I just tried it here at work and it works fine. I will check again when I get home.
I would use the first option, but that will be up to my vendor. We don't do sheet metal in house but I do know that one that has this part has roll form equipment and I can't see them doing it any other way. Most places I have dealt with in the past would take your first suggestion since there are follow on operations where holding the part by the extensions makes the most sense. Thanks for the reply. I have gained some insight to what the newer versions of SW will do and some knowledge about current/past versions that will solve issues in the future.
AKA pyramid roll. For such a low run, just use a waste piece (backing sheet) which is longer than the part. You run them together with the waste piece underneath the desired part. If you're really frugal, you can reverse roll the waste piece back to flat and reuse later.
I like your answer and Fig.
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