I have a part that was converted to sheetmetal. This process did not create a flat pattern configuration, and thus there is no flat pattern view in the drawing file. Is there a way to fix this?
I do current have a configuration to display the flat pattern set-up. However, it does not display the bend line notes in the view.
Thank you,
Jim Walsh
SW2016 SP3.0
Windows 7
Hi, Try this, it sometimes works by completely regenerating a new flat pattern (Don't click flatten during this process until the end):
Delete all flat pattern configurations and derived configurations in the part.
Save as new part.
In the new part, without clicking flatten, Create a new drawing from part.
Drag the flat pattern in (assuming it is there)
Go back to part, check if the flat pattern configuration is there and is working.
Try flattening.
Olly
Mr. Olly:
Thanks for the suggestion. However, the flat pattern view is still not available in the drawing.
This worked great. It even worked when I had it all dim out
Hi James,
Once you've got the flat pattern configuration as Olly so beautifully explained, make sure the "bend lines" sketch in the part is visible (expand the flatten feature in the tree and you should see that sketch")
Hi James,
Sorry I did not notice your reply. Did you get this sorted? If not can you please upload the part file if possible?
Olly
Looks like the flat was added as a config rather than a derived config, therefore the flat config needs to be selected when inserting the view before a flat-pattern can be selected.
EDIT:
That's not the type of behavious I'd expect. when doing a drawing of a sheetmetal part it usually creates the flat-pattern config automatically, as it does when you select the flat config in the model James attached.
Hi James,
I have had this behaviour frequently. I used to make a config with the flat such as you have but have found another "workaround".
In the main config I change the part to the flat model by selecting the flatten command.
Then I go to the drawing and insert new part, (which shows up flattened), and select the flat pattern which, by magic, is now available. The new view is the proper flat pattern.
Then I go back to the part and deselect the flatten command.
The proper derived config of the flat pattern is now in place and all is right with the world.
Bizarre but works... Thanks for posting your files. It helps a lot!
Frank Bos - thanks. I think that is what Oliver Washington wanted me to do too, I just missed a step in the process.
Hi James,
I have had this behaviour frequently. I used to make a config with the flat such as you have but have found another "workaround".
In the main config I change the part to the flat model by selecting the flatten command.
Then I go to the drawing and insert new part, (which shows up flattened), and select the flat pattern which, by magic, is now available. The new view is the proper flat pattern.
Then I go back to the part and deselect the flatten command.
The proper derived config of the flat pattern is now in place and all is right with the world.
Bizarre but works... Thanks for posting your files. It helps a lot!