Unwrapping a cylinder 2

[mlaro]

I have a model of a partial cylinder (a 90° arc) that has cell geometry on it. I want to unroll in to a flat pattern but have been unsuccessful. I know designing this as a sheet metal part is the obvious solution but I haven't been able to get this to work. Instead I've used the wrap feature to create the cylindrical model. The problem is that after wrapping it I then need to add material to represent the as cut geometry (the part is electropolished which removes a constant thickness from the entire part). I add this material by offsetting all of the surfaces and creating a new body. Now I'd like to simply "unwrap" the new body but there is no such feature in SolidWorks. Does anybody have a suggestion of a better way to model this or know of a thrid party software that may be able to do this?

Thanks,

mlaro

 

[DiegoLGraves]

I'd use sheet metal to do this. Make the profile with a flat area so you can insert a flat feature, then do your cut, then remove the flat area. Take a look at the attached file.

Regards, Diego

 

[vims]

no, just use the thickness of the part as the fixed surface. then select insert bends.

 

[mlaro]

Thanks for your reply, Diego. The model you sent is similar to what I've already explored. The problem lies in the surface offset I have to do after I wrap it.

 

[hendersdc]

I would start this part as blank sheetmetal and then cutout all the gaps rather then extrude the material. Then use sketched bend to make your partial cylinder. The part at this stage can be flattened. Then with the part flattened add your material with a offset entities sketch and a extude ofset from the surfaces to show your as cut part. When flat pattern is turned on your material is thicker, when it is off the extrude is supressed and you have your finished part. sketched bend is picky though so you need some flat material on the ends that don't get bent. You can remove this material after the bend is added to the part. See attached part.

 

[msjames1]

Have you tried sketching a 90 degree arc and extruding that as a base-flange. Then insert an "unfold" feature (use an edge of the base-flange as the "fixed face"), extrude your cut and insert a "fold" feature. With this method, you make your cut in the flat. Just make sure you don't try to make a multibody sheetmetal part.

 

[msjames1]

Sorry, just read Diego's post. My suggestion is along the lines of his, but you don't need "flat" area that will need to be removed.

 

[DiegoLGraves]

The flat area just helps you control how the part unfolds. With the flat area on or normal to a plane, when you unfold the part the curved area will flatten normal to the plane. You may be able to control the sketch easier, and make a print with normal projected views of the flattened part easier. And of course there are other ways of doing this too. To each his own - just make the part robust so when the changes start coming thru everything holds together thru your edits.

Regards, Diego