Lightweight Drawings 1

[rothers]

Are lighweight drawings only available for assembly drawings ?

We have a very large drawing of a complex single part done in fully resolved mode. Want to try changing to lightweight mode but on right clicking a view, Set Resolved / Set Lightweight is not there. Also Choosing lightweight when opening the drawing is ignored and the drawing opens fully resolved. This is with 2016.

 

[SBaugh]

Lightweight is only an assembly option. You can save the drawing as a "detached drawing".

It allows you to work on the drawing without the model loaded into memory. You may have to resolve the model to do certain functions, Per the help:
Resolving Models

If the referenced model is needed for you to complete an operation ina Detached drawing, you are prompted to load the model file. You can load the model by right-clicking a view and selecting Load Model. If the model is unavailable or fails to load, you cannot perform the selected operation. Model files are necessary when you want to: •Crop drawing views
•Break drawing views
•Create section views
•Flip or change section lines
•Insert alternate position and relative views
•Insert model items

Search the help for more information about Detached Drawings or maybe reduce the complexity of the part.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[rothers]

Many thanks Scott, had an experiment with detached drawings and it looks like it's a good way to go.

 

[CheckerHater]

You can try (if your PLM will allow it) to create "dumb" part by using "save body" or " split" command (depends on your part).
Resulting part will have same geometry, but smaller in file size.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[SBaugh]

That's a Possibility CheckerHater, but there are a lot of drawbacks to splitting the part and saving the body as a dumb solid. Even Dumb solids can be just as bad. If the model in general as a lot of fillets it will kill performance. Had a file imported from NX that the inside of the model was filled with super tiny fillets and the software was trying to generate each one. I finally resolved the issue, because in the end we didn't care about the inside so I extruded a body swallowing up all the tiny fillets, exported the part to Parasolid, and imported it back in and it reduced the size dramatically. Then it was a usable file.

Past history of splitting a part for me resulted in a loss of connection to the original file and changes were not able to be made. I will split a body into multiple bodies, but I refuse to split a part and save the body. That's just me.

Cheers Guys!

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[rothers]

2 other possibilities we're lookng at:

1. Create a 2nd part and insert the first complex part as a solid body only, create the drawing from this second part. This way even in resolved mode your only dealing with a dumb solid in drafting rather than the fully featured original however the drawing is still fully associative to the orginal part.

2. Detailing mode in Solidworks 2020.

 

[SBaugh]

It still has to load the model graphical data, even if there is no history.

See my reply above to CheckerHater

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376