Problem! Open drawing, views replaced by crossed boxes!

[hititfaster]

I've just opened a drawing, which was sent to a client a week ago and was fine (showing four views of a part) to find that all my views are now just dashed boxes with a cross through! What has gone wrong?! Part is in the same folder as before (all parts and drawings are in one folder) and although I did re-name before sending to the client, I thought I'd done it through SW, not just windows.

Help required asap! Thanks guys!

 

[MadMango]

Check your drawing's references to ensure the drawing is referencing the correct model.

"Art without engineering is dreaming; Engineering without art is calculating."


Have you read faq731-376 to make the best use of these Forums?

 

[hititfaster]

Ok, I just right clicked on one of the views and clicked open - it still seems to be looking for the part on our server and I now have the models/parts on a memory stick. How can I point SW to look for the part on the stick, not the server?

 

[CorBlimeyLimey]

Re-link the files via the File > Open > References function.

 

[hititfaster]

Where do you both live, I want to come and buy you both a pint.

Crisis averted!

 

[ctopher]

You can also do this in SolidWorks Explorer.
Also in SWE you can make a copy of the dwg and point to another model.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[SnowCrash]

Couldn't he also save as an unreferenced drawing which would not need to see the part?

--
Hardie "Crashj" Johnson
SW 2011 SP 4.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580

 

[ShaggyPE]

Re: SnowCrash's point. SolidWorks calls that a "detached drawing." Basically it is a drawing file that was purposely saved in a manner that breaks the link to the model file.

I don't believe this results in X'ed out views. The intent is to maintain all the views and just disassociate the model... maybe for really large models or something... never really found a use for them.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[SteveJJH]

Just for future reference when people find this thread, we have a lot of drawings here that are crossed out even when they haven't lost the references. Just right click on the view and select "show". I know it's not your issue, but for something so simple, you wouldn't think I'd get asked it about twice a week.

 

[hititfaster]

Great feedback on this everybody - I'm back in the office today, and have already found a use for this. I have two similar parts, so having already created one drawing, a did a save as copy, opened the new drawing, changed the references to be the similar part, and all but a couple of the dimensions stuck where I wanted them to, thus saving me quite a chunk of time.

I love the fact that after using SW for over a year continuously, and on/off before that, I'm still finding new and often better ways to do things.

 

[moon161]

Yes hititfaster. If you have standard names for views, configs, etc, you can stretch a drawing quite a bit before it breaks.

 

[SnowCrash]

This has been a helpful reminder. Last night I had three similar parts but had to create the drawing only once. I just reloaded with replaced references and did a "Save as.." for the two subsequent parts.

--
Hardie "Crashj" Johnson
SW 2011 SP 4.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580