Tips on reducing file size (Feel free to add to this) 1

[davidinindy]

This was brought up on another board.
"which will reduce the file size? (which one to prefer

1. revolve
2. extrude "

The reply
"I assume your asking about a cylindrical part, if the cylinder has mutliple steps etc. then the revolve will be faster. generaly data in a sketch can be rebuilt faster than multiple features. Ie. a cylindrical part with multiple steps would take several features that could all be defined in a single revolve sketch. Hope this helps"

I have tried this on a very complex part I'm working on.
It consisted of two drafted, stepped diameter features extruded from a face, that was linear patterned 150 times.
I simply redrew the features as two seperate sketches and revolved it, and then linear patterned the same as before, and the file size went from 20mb to 15mb, with no other changes.
I also, on the original file, changed the linear pattern to geometry patterns where possible. That seemed to reduce the file size some also, even before doing the above.
Anyway, Just thought I'd share this.

 

[aamoroso]

Extrude a single bounding block over your entire model after all your features are done, so the model looks like an ice cube and everything is inside of it. This too will reduce file size, to view your model, suppress the extrude.

 

[SBaugh]

Saveing the model as a new name will help bring down the size, but once you resave that model the size will return. This is a good way to help in sending files out to customers.

All and all there is no great way, because there is data that is added to the file via MicroSoft. But there are ways to help get around it.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[macPT]

As a base rule for the use of actual 3D CAD we have the design intent. Depending on the type of industry/product, manufacturing capabilities, know-how,..., this can de achived by different strategies (design for manufacturing, design for assembly,...). The design intent make us build models in a way that file size or rebuild time are far from being optimized.

But now, as technology and markets evolves, we are facing other challanges as our models grows in size and complexity.

Should we consider a design for file size or a design for rebuild time? Can this be as important as other design intents? (for me it's not, but I ear more and more complaints from my IT guys about the need for new disks or faster servers).

Regards

 

[davidinindy]

I design for rebuild time, which may or may not be related to file size. Haven't worked with it enough to make that connection yet. I hate making a minor change to the model, and then waiting 5 minutes for it to rebuild. It's hard to look like you're working when your boss walks by, and you're sitting back waiting for the model to rebuild!

 

[MadMango]

Good point [blue]macPT[/blue].

I don't desing parts for file size, but I do try to structure my top-level assemblies so they rebuild faster. FIle size isn't that important, as it comes at a price of about $2 a gig.

[green]"But what... is it good for?"[/green]
Engineer at the Advanced Computing Systems Division of IBM, 1968, commenting on the microchip.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[PDMAdmin]

I agree, file size isn't terribly important, but memory usage can be a show-stopper after your assembly becomes large enough. For large, complicated assemblies, it may be a good idea to formulate a plan for simplifying the "heavy hitters" for purposes of displaying them in the assembly. One of the biggest weaknesses of SolidWorks, IMHO, is how it handles large assemblies. I suppose that could be a separate discussion entirely.

 

[MadMango]

I handle the slow models by saving them as parasolids if I need them for display reasons.

[green]"But what... is it good for?"[/green]
Engineer at the Advanced Computing Systems Division of IBM, 1968, commenting on the microchip.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[engAlright]

IMO, it's important to differentiate between file size and performance - they aren't necessarily related.

I create complex features (fillets, chamfers) as seperate features wherever possible, then I can create a simplified configuration in which those complex features are suppressed. This simplified configuration is what gets used in the assembly to improve the assembly's performance.

Also - exporting and re-importing as a parasolid as MadMango has suggested gives you essentially a "dumb solid", which in my experience is the best case for rebuild/save/open performance (not necessarily the best case for graphics performance).

 

[DesignSmith]

The feature Parts for Publication in

http://www.swcommunity.com

confirms your finding that a revolve is more efficient than stepped bosses or other methods.
When making parts that get used dozens of times in hundreds of assemblies, part file size and performance, can become as important as design intent.
If your custom end stop will never be sold to another customer, then you are free to create it any which way.
-----
Some other tricks to more efficient part modeling:
1. In general, more complex sketches and a shorter feature tree are better than multiple features from simple sketches.
2. Thin extrudes are better than shells or double profile sweeps as the path gets longer.
3. Using part equations is better than putting more and more columns in a design table.
4. Making a complex patterned feature (turbine fan blade) as a separate body (in the same part), and then patterning that; is more efficient than patterning the fully merged feature. (join the pattern and base later)



DesignSmith

http://www.DesignSmith-Services.com