Show Model Items in Flat Pattern View

[ssmithdigilab]

Is there a trick to showing model dimensions in a flat pattern view? I have a sheet metal part with several cuts that go across bends. So, in the model, I unfolded the part, created my cuts, and then folded the part.

In the drawing, I have created a flat pattern view. For some reason, in this view I cannot show the model dimensions related to the cuts that go across the bends. These dimensions will however, show up in other views where the part is bent, which doesn't make any sense. The witness lines for these dimensions in the bent part view go off into space (as if the part were flat).

Has anyone run across this problem? I hate creating dimensions within the drawing when I have already created them in the model, but it seems like that is my only option here. I have even tried showing the dimensions in a bent view and dragging them to the flat view, but I get the red circle with a slash through it.

For your reference, I have attached a Word document with some screenshots of what I am describing. Please help!

 

[ssmithdigilab]

Bueller? Bueller? Bueller?

 

[CorBlimeyLimey]

My names not Bueller, but ...

Its working fine for me with SW2010-SP2 on XP Pro x32 ... and always has with other versions of SW.

Try inserting the dimensions to the flat pattern view before any other views.

In Tools > Options > System Options > Drawings there is an option to Eliminate duplicate model dimensions on insert. If that is checked, and other views are dimensioned before the flat pattern, that would prevent the dimensions being added.

 

[ssmithdigilab]

I believe I figured out the problem. It seems that the problem existed in the flat-pattern feature in the model.

When I initially created the base flange, SolidWorks automatically created a flat pattern. The fixed face it chose for the flat pattern seemed to cause the problem.

I edited the flat-pattern feature and chose a different plane for the fixed face, and suddenly I could insert the model dimensions for those features into the flat-pattern view.

Hopefully this info will help someone else down the road, although it doesn't sound like anyone else has ever had this problem.

 

[CorBlimeyLimey]

The flat pattern is not usually created till a drawing of the part is created.

 

[ssmithdigilab]

That's not true. If you create a sheet metal part using:

Insert>Sheet Metal>Base Flange

as soon as you complete the feature, the following 3 items are listed in the model tree:

Sheet-Metal1
Base-Flange1
Flat-Pattern1

The user enters the values that create "Sheet-Metal1" and "Base-Flange1". But SolidWorks automatically creates "Flat-Pattern1". If you edit that feature, you see that SolidWorks automatically chose a "Fixed face".

As I said previously, the face that SolidWorks automatically chooses could affect the way dimensions show up in the flat pattern view that you later create in the drawing. In my case, solidworks somehow chose a fixed face that was on the far side of the part with reference to the direction that the flat pattern view appeared in the drawing. I don't know why that mattered, but most of the dimensions would not show up in this flat pattern view. Once I edited the flat pattern feature in the model tree and selected the plane that was on the near side in the flat pattern view in the drawing, all dimensions showed up.

 

[CorBlimeyLimey]

Ahh yes ... you are correct. I haven't used that method since the new method was introduced.

 

[DiegoLGraves]

Creating the sheet metal part puts the sheet metal Flat-Pattern1 in the feature tree. Adding any view of the sheet metal part to a drawing creates the DefaultSM-FLAT-PATTERN derived configuration in the part file.

details, Diego

 

[ssmithdigilab]

CorBlimeyLimey,

What new method are you talking about?

 

[CorBlimeyLimey]

[sigh] Just ignore me today. I have been re-arranging the office and workspaces all week, and am totally knackered. Taking a break for lunch and skimming the posts.

The "new" method I referred to is in fact the method you are using. I skim-read and misinterpreted your Insert > Sheet Metal steps as the old Insert Bends method.

Diego's post explains what I originally meant.

I'm going for a sleep now.