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Procedure for sheet metal

Procedure for sheet metal

Procedure for sheet metal

(OP)
Is there an order to go in when constructing sheet metal parts? I get my part modeled and then have problems when I get to the drawing view and spend a long time folding/undfolding creating unfolds, watching my hole patterns or mirrors not function any longer. It has something to do with the patterns referencing the flat pattern and then it not being there when folded but I have to have it flat to dimension holes.

RE: Procedure for sheet metal

Basically ...
Create the formed shape
Unfold (only where necessary)
Add the holes
Fold

Can you post a problem part for review?

RE: Procedure for sheet metal

(OP)
I was working on a u-shaped part and was patterning holes from one side to the other in flat, then when I folded it they would dissapear w/ errors. Anyway, I found a workaround by just keeping it in fold and extending the first hole through both walls - so it's basically one hole. For some reason SW likes that as it works in flat as well. I don't think it likes when you reference and edge in flat that will eventually be folded (it will be missing). Sheet metal feature seems very finicky.

RE: Procedure for sheet metal

EaZiE,

Usually, I start off my sheet metal parts are regular parts. There always is the possibility I will convert it to a machined part. At the end of the design, I rip the corners and convert to sheet metal.

On the drawing, I do not unfold the part unless I have to. The flat layout is the fabricator's job.

--
JHG

RE: Procedure for sheet metal

^This.

For sheet metal specifically, I build a block model of the shape I want and the use the "Convert to Sheet metal" Option; choosing a base-line-face. and then the corresponding corners for folds. Doing it this way
gives you very tight dimensioning and quickly letting you switch from inside to outside dimensioning. Mark all holes on the this model and let Solidworks do the work for unfolding.

RE: Procedure for sheet metal

As I have been learning here lately Sheet metal designing is a science. Anyone can make it in Solidworks, but what get in the real world it's not always the same thing. We have been using Bend tables to control the Bending K-factor to get the parts in SW to real world components. If that's not an issue then what we do is we usually make it in a partial formed shape either in a U shape or and L shape and added Edge Flanges as needed. When I need to add hole and varying on the requirement I will usually flatten the SM part using the Unfold icon. When done I will use the Fold icon and re fold the part. Whatever you do not build any features after the Flat-Pattern feature, because when you flatten the part your features will be suppressed, which I assume is what is happening for you.

Other times I will use the Convert To Sheet metal. I think there is a time and a place for either "Convert to SM" and/or "Base Flange". When place your model in the drawing that is when you get your Flat-pattern configuration in the part... strange I know and agree, but its been like this for years. When you place a view into the drawing you get the option on the right and on the left to select Flat Pattern. Drag that view into the drawing and that is how you get the Flat Pattern Config.

Folding and unfolding is simple when you find the Fold and unfold SM features. I have showed this to a former employer and they thought it like God gave them a special gift... haha.

Anyway I hope that helps,

Scott Baugh, CSWP pc2
Gryphon Environmental
www.2gryphon.com

Quote:

"If it's not broke, Don't fix it!"
FAQ731-376: Eng-Tips.com Forum Policies

RE: Procedure for sheet metal

I start with a base flange feature, either the primary profile of the part or the primary face. Then add edge flanges or other features using the sheet metal tools. Many of the needed hole features can be included in the edge flanges and remain well behaved when revising material, thickness, bend radii, etc. My back ground is primarily sheet metal fabrication so the SW tools makes sense functionally, and I have been modelling sheet metal in SW for 17 years. The software tools are robust when used as intended. If you find yourself having to add too many steps in the feature tree, or lookind for work-rounds you may want to review the help files for the sheet metal tools. I'm in that same situation when working with swoopy parts using surfaces, having to go back and review the standard tools and not add features just to tweak something.

Diego

RE: Procedure for sheet metal

Check out YouTube for some sheet metal tutorials.
Link

Chris, CSWA
SolidWorks '15
SolidWorks Legion

RE: Procedure for sheet metal

(OP)
Thanks for the tips! Yes, rule #1 of sheet metal is don't create a feature after the flat pattern. Usually don't post until I fought it for awhile. Good to have a place I can ask questions and refer back to when I need to.

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