Hi Guys,
I am trying to make a bulkhead with two edge flanges, but Solidworks is keeping me from my sanity.
The material is .050" aluminum with 5/8" flanges on inner and outer edges.
**FILE ATTACHED TO POST FOR HELP**
Attachment 6381
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Hi Guys,
I am trying to make a bulkhead with two edge flanges, but Solidworks is keeping me from my sanity.
The material is .050" aluminum with 5/8" flanges on inner and outer edges.
**FILE ATTACHED TO POST FOR HELP**
Attachment 6381
Hi - I wasn't able to open your SLDPRT file for some reason - probably because I'm using SW 2013 and yours is probably more advanced.Quote:
Originally Posted by rkirk77
If so, please save it as a STEP file (File>Save As>*.STP,*STEP.), and re-post it.
Is the bulkhead exactly circular? Maybe you could do so a simple work-around by producing it using a single "Revolved Boss" or "Swept Boss" feature?
One way or another, please describe exactly what problem you encountered.
My issue is that I cannot flange the inside of the ellipse, however it will let me do it to the outside.
PS, I re-saved the file as STEP.
At first I thought the problem might be the offset spline used for the inner edge so I changed it to an ellipse. That didn't help, it still would not create an edge flange on the inside. I then made the base part as one half, intending to mirror it after forming the flange but it would not let me mirror the part. It did however form the half inner flange. I added the other half of the base using another extrusion and flanged the inside of that edge. Worked fine. The outer edge took the edge flange with no issues so the part is complete,,,, except the flat pattern shows an error because of the inner flange. Notice in the image below the the two halves of the inner flange are not tangent for some reason.
So, I was able to do it but the sheet metal part is not happy. Not sure why. I'm also not sure why there's a 97K file size limit on ZIP files -- I can't upload my revised file for you to look at............Bill
Attachment 6385
If you interrupt the inner edge the flange works as it should. Sounds like a SWx bug to me;
Attachment 6386
Attachment 6387
Attachment 6388
No Bill - you are completely wrong - there is no such thing as a SWx bug:mad: It's called a SWx feature.;)Quote:
Originally Posted by cwilliamrose
Otherwise I grudgingly admit that you're right. There is a limitation in SW sheet metal flanges that says you can't flange a split face.
http://eaaforums.org/images/attach/jpg.gif
The secret is to model one half of the bulkhead, flange it in SWx sheet metal (one edge at a time), and then mirror the final result.
Interesting set of limitations. I'm not at all sure what they mean by 'split faces' unless they're talking about what you do to a molded part to allow draft to be applied. I put a 'split' through the part on the inner edge as a workaround.
I tried mirroring the half part and SWx told me I can't mirror sheet metal features and to mirror the body instead. OK, I tried that it it wouldn't let me pick a face/plane to mirror around. I did the tests in SWx 2016 and the only way I found to could get a valid sheet metal part was to put a slit through the inner edge. I didn't try older versions or SWx 2017. I also didn't try the EAA version, I only have that loaded on my laptop at home and with no SpaceExplorer and no hot key assignments I find it nearly impossible to use. Color me spoiled......