CAD Forum

I am trying to model a complex sheetmetal-type part but I am finding Sheet Metal function very limiting.

I am wondering if I should move towards surfacing instead.

I am forming foil bearings with wings that are pressed out (See photo). They are very precise and small.
Currently I am piecing together wings and web with sheet metal, cutting out the negative, etc.
I need a final flat pattern for etc.
Solidworks is so bad at this. Design changes are a nightmare.
Has anyone used the "FLATTEN SURFACE" command with SW premium? I don't have premium, and I don't even know if this will work.
Any advice is appreciated. I am getting pretty frustrated with this.

Don't get me wrong. Modeling the part is "easy", either with traditional solids or sheet metal. The hard part is knowing what the part will look flat.

VTmechie wrote: ↑Wed May 19, 2021 2:22 pm Has anyone used the "FLATTEN SURFACE" command with SW premium? I don't have premium, and I don't even know if this will work.
Any advice is appreciated. I am getting pretty frustrated with this.

You don't need SW Premium to use the Surface Flatten feature. See this link from the old forum

JSculley wrote: ↑Wed May 19, 2021 2:35 pm You don't need SW Premium to use the Surface Flatten feature. See this link from the old forum

As far as I know, flatten surface is only available for Solidworks Premium. I have SolidWorks Professional 2021 and the Surface Flatten feature is greyed out.

VTmechie wrote: ↑Wed May 19, 2021 3:27 pm As far as I know, flatten surface is only available for Solidworks Premium. I have SolidWorks Professional 2021 and the Surface Flatten feature is greyed out.

Read the link I provided. Essentially, you can take any file that has a surface flatten feature already in it (see the seed file attached in the linked forum post), insert your part into that file, edit the definition of the Surface-Flatten, deselect the existing face and select the faces of your part. The flatten will now flatten your part and you can delete the original boss extrude from the seed file. you do not need SW Premium to do this. It is a loop hole that has existed for many years.

see this help file
http://help.solidworks.com/2021/english ... urface.htm

Unless you know a work-around...

I would draw the part (sheet-metal) in its flattened state. I would imagine that the wings would be formed (forming tool) while in this state anyway. Also, it would difficult to roll from the part without crushing the wings. I guess if it is thin material, roll-forming wouldn't be necessary.

Surface flatten will be very slow. Basically it mesh the surface then flatten it. Also it's not accurate because of the mesh. It will be close but not exact.
For your part, you just need to model one "slot/tab" or two and pattern it.
I don't see anything that need to be precise.
Laser cut 3 edge for the tab and punch the shape. Or punch shear and form the tabs in one shot.
Unless you're designing the punch, there is nothing you need to model precisely.

VTmechie wrote: ↑Wed May 19, 2021 2:22 pm I am trying to model a complex sheetmetal-type part but I am finding Sheet Metal function very limiting.

Not typically what I call sheet metal, at least not for what most CAD systems are designed to create which is press brake formed parts. This is more like a roll/stamping operation.

Looks like the material is very thin. This means you will get very little material stretch as there just isn't much there. If flatten surface is not available to you, I would draw the flat separate. You can measure the formed tab curve total length to get the length to draw it in 2d. Might take some trial and error.

If the entire part consists of cylinders and planes with no compound bends, it ought to flatten with sheet metal.

You don't need to model with sheet metal features. (I wouldn't in this case). Maintain constant thickness and you can convert to sheet metal and flatten.

Make sure the spring leaves don't intersect when flattened. Best to try a small sample area out first.

JSculley wrote: ↑Wed May 19, 2021 3:38 pm Read the link I provided. Essentially, you can take any file that has a surface flatten feature already in it (see the seed file attached in the linked forum post), insert your part into that file, edit the definition of the Surface-Flatten, deselect the existing face and select the faces of your part. The flatten will now flatten your part and you can delete the original boss extrude from the seed file. you do not need SW Premium to do this. It is a loop hole that has existed for many years.

Thanks JSculley, I understand it now, I was trying to read that too late in the day ha.

I programmed a part like that before for a Amada vipros 357 queen.

Back in 2015 I did not have access to any flattening, so we ran the small features on the punch press operation before the perimeter cutting op.
It would cut the feature in 3 hits and then use form punch to bend it out. The rolling was done in a second operation with custom tooling on the amada press brake.

I am curious if there is a machine that can punch/form/roll in one shot?
If not I would not bother making the part out sheetmetal in SW, it gives zero benefit. All of the Amada programming is done in Amada AP100US.