how do you reduce file size w/ using patterns

Does anyone know any tricks to keep file size down and stillusepatterns in a part?

RobSolidworksParts And Features
Comments 8
SF
SF 2007-02-24
Rob,

Using patterns does not increase file size more than other methods.There are a lot of factors. What you pattern (how complex), whatoptions you select (geometry vs non-geometry), how many, whetheryou exclude instances, etc. Just saving a file twice can double thefile size due to a bug in the Windows OLE. What is the concernhere? According to the SolidWorks reps I have talked with (asrecently as SolidWorks World 2007), file size does not representthe amount of memory required when the part is open. It doessomehow affect opening the file across a network. My main concernwith file size is server storage space only(by opening and doing asave as I was able to reclaim 4GB of space on 3500 files and thatwas only the tip of the iceberg). Is there something else I shouldthat SolidWorks is not admitting to?

SA

PS Here is something to try. Enclose your model inside a cube andsee how much it reduces your file size. Depending on the model, itcan be quite a lot.
AW
AW 2007-02-24
Rob,

Is file size the issue or the time it takes to resolve a pattern?

Large patterns can really kill SolidWorks performance.

A few more specific details on what you are experiencing and wewill all be able to give you a better answer.

Regards,
AL
AL 2007-02-24
Regarding Patterns. Here is something I do, which does notnessesarily affect file size, but does impact performance.
If I have a part, which is used in an assembly, that has a patternthat will eventually need to be described or shown in a drawing, Iwill make at least two configs for that part. One with, and onewithout the pattern.
The config without the pattern I use as the default config and itis used everywhere. But when I need to show the applied pattern ina drawing, I will use the pattern config just in the view(s) I needit in, in the drawing.
This saves a great deal in performance.
JS
JS 2012-03-08

Are you patterning features, sketches or parts? It could be my own perception, but I think that patterned features load faster than patterned sketches. Therefore if I have a feature that I know will be a pattern I make the initial sketch, perform the feature (boss,cut) then pattern the feature.

SF
SF 2012-04-27

Jody,

It is not just your perception. Matt Lombard and some other people have done tests that show that feature patterns are "usually" significantly faster than sketch patterns. I believe someone, it may have been Matt again, has done some tests that show that in certain instances sketch patterns are faster, but I believe those are pretty limited.

Jerry Steiger

AV
AV 2012-04-27

Even better, pattern bodies not features (if possible).

And even faster than that is patterning components inside assemblies.

Watch this video for an example were patterning bodies turns a long rebuild into a very short one.

CLICK HERE or click on the picture below:

SF
SF 2012-04-28

Alin,

That's awesome! Now, if we just convince someone at SolidWorks that they need to make the patterning of bodies in a multi-body part work as quickly as the patterning of parts in an assembly, we wouldn't have to try and remember this trick.

Jerry Steiger

SF
SF 2012-04-28

Rob,

A complex geometric pattern will always be bigger in size(due to a lot of info contained in). Is the total memory size of file a probllem? or facing prb while working on SW having complex geometries up in design tree. two methods for later case:

1.suppress those complex geometries as you work down the design tree and correspondingly unsuppress afterwards.

2. if working in assembly mode, you can alo set that part to "Lighweight"(and then again set to resolved mode), it's effective with heavy files.