Drawing detail of weldment part body - only one face

[brrian]

We do a lot of weldment parts which are primarily wire. If it's a complex weldment, we'd typically want to break out views of individual cut list items (bodies). I know to insert drawing views with the "Relative to Model" option to get just the body I want; however wire parts usually have only one face for reference (the command needs two).

Is there any other way to select and orient a body for a drawing of a weldment body--other than selecting two faces? Planes don't work. I know that I could build a very small cut or extrude into the body to add a face, but that's a workaround that I'd rather not use. Has SolidWorks considered this--is there another way? Thanks in advance,

Brian

 

[CorBlimeyLimey]

The "small flat" method you mention is the only way I know of.

Helpful SW websites faq559-520
How to get answers faq559-1091

 

[TheTick]

Temporarily create flats on your part. Use "normal to" orientation with the planes selected. Then save the view and insert the saved view into the drawing.

If you select 2 planar faces and hit "normal to", the 2nd face is used to orient the top of the view.



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[TheTick]

One thing I miss about Pro/E: "relative to model" type view could used more types of entities, and would update orientation in the drawing if orientation of the entities changed in the model.

 

[Adrian2]

Dear Brian;

Just open the cut list and highlight the solid you want, right click and "Insert into new part".

Create your drawing view from the new part file which will have standard planes automatically added to aid in view placement.

I use this frequently for round parts with no second face for "relative to model" views.

Works great !

Adrian Dunevein

http://www.aaadrafting.com