Good day to everyone,
I have a problem with drawings in SW 2017 SP2.
I have a sheet metal part and I make a drawing out of it with a flat pattern view. I save the file and close the drawing.
When I open again the drawing an message apears and tells me that my flat pattern isn't found so the progra will put a regular view instead.
Can you tell me how to overcome this problem?
Thank you!
This is the error:
Can you upload the part?
Yes
Try this - In the configuration marked below select the flatten icon
That wouldn't make the drawing think the configuration doesn't exist though. It would just give you a un-flattened flat-pattern.
I think it's one of 2 things, the flat-pattern view was created while the part was in read-only therefore losing the config as soon as it was closed. or
Someone has deleted the config in the mean time.
It worked here -
I'm not sure which release it started to be an issue, thinking 2013 - where you would need to insert all the other views and then go and insert the Flat Pattern, then it would stay as set otherwise it would always do what Eugen's part did..
Fair enough then. I've not seen that so I've learnt something new here I'm sure I'll now see a lot of.
I do find it curious that the dialog Eugen posted states a completely different config name to the one you fixed.
I did what I mentioned above - which would have been the same if I would have picked one of his configurations. That part file doesn't recognize flat patterns apparently like the older version files. Since this has been an on going issues from years ago, I always just inserted the other views and then the Flat Pattern selection, otherwise it'll work sporadically....
I find this is the "normal" behavior of sheet metal part:.
1. Part is created but the flat pattern derived configuration is not automatically created.
2. Insert the part in a drawing and create a flat pattern view. (Make sure part file is also open.) Then save the drawing.
3. Look at the part files and you will see that the flat pattern derived configuration has been added. Save the part file!
4. Now you can open the drawing without errors.
That's my interpretation of 'normal' sheet metal behaviour also.
I think that is why I have to have check-out both of them: the part and the drawing to automaticaly create me the flat pattern in the part when I save the drawing.
Thank you!
The thing is like this. I work in PDM too. I made the part with all the things I needed. Then I check in it and all the parts become read only. After that I made the drawing for the part. I save it and when I opened again my flat pattern dissapears. When I made the drawing for the part I added the flat pattern view last.
I discovered that I have to check out the part I want to make the drawing for and then check in again both of them, the drawing and the part. In this way the flat pattern remains there.
I agree with Eugen, this issue is caused when the part file is read-only (not checked out in PDM) when the drawing is created. So when the flat configuration is created(view placed into the drawing), it is not saved into the part along with the drawing. Then next time you open the drawing, it can't find the part configuration it created when it was saved. Eugen Lupascu
I find this is the "normal" behavior of sheet metal part:.
1. Part is created but the flat pattern derived configuration is not automatically created.
2. Insert the part in a drawing and create a flat pattern view. (Make sure part file is also open.) Then save the drawing.
3. Look at the part files and you will see that the flat pattern derived configuration has been added. Save the part file!
4. Now you can open the drawing without errors.