I have created this body as a lid for another part. But, recently discovered that it needs to be made in sheet metal. I can make the top face and the planar sides into sheet metal by converting but I can't convert the rounded corners. Can any one help me figure this one out?
You'll have to model (sorry you can't convert into sheet metal with those corners) that as sheet metal (and use swept flange option) to get that part as sheet metal.
Have you tried cutting the corners out, turn the remainder into sheet metal, then add back the corners as flanges?
This looks more like something that should be formed
Are you designing this part for high volume production or a limited run? Attached is the best that I could come up with for a producible part in a limited run. I created the main part and added flanges to the straight sections, I tried several methods but found the only way that I could create a part that would convert to sheet metal properly was to create a flat extrusion and add a sketched bend and then trim off the excess. If you are producing it with a stamping process and can draw the corners up with progressive forming dies, I was able to convert a base extrusion and create flanges all of the way around the base part after converting it to Sheet Metal, and flatten it out to get a good blank.
I hope this is helpful.
Thank you for that help that is great. That was exactly the kind of idea I had and now that I know how to do it I can reproduce it in the future. MY next problem is with flattening the model. How do I go about that?
select the sheet metal menu and there will be several options available at the top menu, select convert to sheet metal and a dialog box will appear, click on the main body and then click the collect bends icon, then click ok. A flat pattern icon should appear at the bottom of the design tree, it is suppressed, if you expand it there will be a 2nd flat pattern icon and if you unsuppress that it will flatten the part. The rounded corner is a little trickier, attached is a new model that works better that the last one, I made it using a revolve and then in the sheet metal menu, I selected insert bends icon, selected the edge of one of the outside corners and unchecked the use default box, I then had to enter the radius of 1.375 in to the radius dialog box. If you roll back the design tree you will be able to see the steps that I took to build it. Hopefully this helps!
Thank you very much for that help. It looks awesome. I can see what you did there. That is a great help. Thank you
Grant,
I work at a precision sheet metal shop. We get models similar to this all the time from our customers. I have modified your model in a way we would typically do it so that we could obtain a useable flat....see attached file.
Hey there, thanks for doing that and creating that file. Do I need to open it a certain way? I keep getting an error message when I try to open your file.
Bob is using 2015, I have the same problem opening it as my administrator has not updated our system to 2015 yet. You cannot open a newer file with an older version of Solid Works.
Thank you for all the help you gave me on this. It helped me along so much.
Grant,
I will save the file as a parasolid (step doesn't work) so that you can see it. You should be able to use the edge flange tool to add bends. Use .208 as a bend deduction initially. After it is sheetmetal, go in and change the large radius bends to K-factor = .447.....it should unfold.
Duh, why don't I just give you the 2014 part? I originally modified it in 2015. Exported a step and found that 2014 just crashed when trying to open it. I tested the parasolid with 2014 and it worked. I don't know why I didn't think of just saving that as a part and posting it....it's early...
That is exactly what I was thinking of. That looks perfect, and I can see exactly how you did it. Thank you so much for the help.
Duh, why don't I just give you the 2014 part? I originally modified it in 2015. Exported a step and found that 2014 just crashed when trying to open it. I tested the parasolid with 2014 and it worked. I don't know why I didn't think of just saving that as a part and posting it....it's early...