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**
Will you be required to offer a flat pattern of this part for fabrication to any suppliers? If not I would suggest that you don't model it as a sheet metal part. I would rather create a model using a swept sketch profile.
OOOPS! Meant to say Revolved sketch as opposed to swept.
Use the Sheet Metal Swept Flange feature for this....
Can you provide your part file? I just created a test piece and was able to create an edge flange of 5/8" long on both the inside and outside edges.
With a flat pattern?
Yes I created it out of sheet metal features (Base Flange/Tab feature and two separate Edge Flange features) . The only issue is, I know my shop guys would look at me crazy if I sent them this part to build because we don't have the capabilities to produce this with bends. I would have to make it out of three different pieces and have them welded together.
Same process as this..EAA Video Player - Your Source for Aviation Videos
Having the guys look at you crazy can be avoided by not sending this part to be fabricated internally when you're aware they can't do it in house. Clint Eastwood often remarked, "a mans got to know his limitations' in the Dirty Harry movies.
Hence why I said "IF" I sent this to the guys in the shop . I don't send anything out to the shop that I know can not be made here. If it can't be made here we simply just don't do the job.
Yes, it will need one.
Yes, it will be a sheet metal part that requires a flat pattern.
I also included the part i am trying to make
I meant the Solidworks part file that you are working with. But now that I see what the part exactly is suppose to be (aside form exact dimensions, its hard to see the TIFF File when zoomed in. The Ellipse shaped base flange part can not be created with any edge flanges on it. Solidworks just wont allow it. I tried an Ellipse shape and it gave me the same error. When I originally looked at your first jpeg I did not pay attention to the part being of an Ellipse shape. It will however create a Circular part with two edge flanges on each edge. The only way to get this drawing correct for production is to figure out the flat pattern/bend allowance yourself the oldschool way with a Calculator.
I was just thinking it might work if I cut the ellipse in half?
There is a lot going on in that tif file.. Nice. Like Dean, I did NOT have any issues with my test piece either using what looks like your settings are for the edge flange. I suggest you take a look at whatever you are using for a k-factor..
Edit:.. I ran the gamut with k-factors and still had no problems. Perhaps you are using something else???
Another Edit:... I get it now.. Your parts is an ellipse..
I can also do this process with circles, squares, etc.. but it seems to choke on the ellipse shape, or "non-lineral circles".
It will create edge flanges if the ellipse is cut in half.
Very Good Dean.. I was just fiddling with that myself. I tried to mirror it but it would fail to flatten then. This might be the best solution for the time being. I also tried converting to arcs but that didn't work out for me either. Then tried splines and still the same thing. Could get the outer edge to work but not the inner edge.
I would suggest trying the ellipse as you have it but putting a small split or cut in it to make it an incomplete full ellipse. Even a full through cut extrude that is just .001 wide.
I did the following1) Create the ellipse in Sketch2) Create the Offset3) Draw line down middle (top to bottom) and trim other side.4) Mirror the Ellipse and Offset5) Create Base / Flange Tab6) Create Edge Flange on inside (there will be two) and outside.
Here is what I got..
I only go this gap in the top and bottom.. so not bad!
Make it as an assembly. With three different pieces that are to be welded together. But you will need three flat patterns for this.
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