Flat pattern in part controls flat pattern in drawing? 1

[KirbyWan]

Howdy all,

I have created a simple sheet metal part with two bends. I can create a flat pattern in a drawing, but the flat pattern is linked to the part. If I suppress the flat pattern in my part, the part is displayed in the formed condition. If I unsuppress the flat pattern so the part is now flattened, the part shows up in my drawing as a flat pattern. If I want to display the flat pattern of a part in a drawing I expect it to be the flat pattern regardless of the state the part is in. Is there some flag I've missed or is this a known error. It doesn't happen to all my drawings, just some. Here is an example:

http://files.engineering.com/getfil...0a-484f-9598-79ed5aed0e22&file=example.SLDDRW

http://files.engineering.com/getfil...a6-44cd-894e-7e53ac4a6492&file=example.SLDPRT

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[TheTick]

Configurations!

 

[Updraft]

KirbyWan,

You do not have to create a separate configuration for a flat pattern. SWX automatically does that for you when you create a drawing of a sheet metal part.

Our practice has been to show the detailed formed part on sheet one and for reference only show the flat pattern on sheet two complete with the information used to generate it (actual material thickness, IBR, K-factor). We hold the vendor responsible for the finished part, not the flat pattern.

- - -Updraft

 

[KirbyWan]

I compared the a part that behaves correctly (or at least as I expect it to) and a part that behaves by what I'll call the stupid behavior I described and they both have the same configurations and the same link display states to configuration box checked....

Went back and checked the properties for the flat-pattern1 and this was suppressed for both the default configuration and the flat-pattern configuration. I unspressed the flat-pattern1 in the properties dialong for this configuration when I had the flat pattern config selected and that corrected the problem.

Thanks for you help, Tick, brief though it was.

-Kirby

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[Russell67]

Creating seperate configurations is a quick way to get into trouble. Create sheet metal and let it do the work for you, this will ensure that your bend notes appear correctly. If someone monkeys with the configurations it might not update the flat pattern or vice versa. Depending on what you control and what the vendor is responsible is a key factor. Personnally if the vendor wants to carve my finished part from a solid block that is his choice, i want the folded part that i created.

 

[DesignerGuy16]

In the drawing, if you select the view you want for the flat pattern and select "flat pattern" it will automatically create a derived configuration as NameSM-FLAT-PATTERN (Name = your configuration name). That derived config will be your normal configuration with the flat pattern feature unsupressed. That way it allows you to use the bent original configuration wherever needed and create the drawing normally without any issues.

James Spisich
Design Engineer, CSWP