How can I reduce the size of large parts?

[marieke]

Does anyone has some tips for reducing the size of large parts?
In our company we use the parasolid conversion to reduce the size of our parts (we don't need the features anymore, just the surfaces and edges for mating). I am just wondering if there are other ways to facilitate the building of large assemblies (like factory and machinery layouts). In some Cad software it is possible to delete the "solid" information of the part and to save it as a set of surfaces. All tips about size reduction are very welcome and thanks in advance!

 

[MHendler]

Hi marieke,

In SolidWorks, the size of the files is controlled by the number of features of the part. If you can reduce the number of features, modeling in the best way (sometimes it's hard to find the best way), the parts will be smaller.
Another thing you can do, is create configuration of the parts to use in the assembly. You can suppress the unnecessary features to make the part smaller.
The procedure of export the parts in Parasolid extension is a good practice, once you don´t need the parametric information of the part.
Also, you can load the parts in lightweight mode. In the Open dialog box, check the LIGHTWEIGHT option. SolidWorks loads just the visual information of the parts. Once you click on the part, SolidWorks loads just the selected part.
Another thing you can do is create a configuration of the assembly. For example, if you are working if the left part of the machine, you can make a configuration named "Left" or "Motor" and suppress the parts you aren't using. It makes the assembly faster.

I hope it can helps.

Regards,

MHendler

 

[BBJT]

You may want to check out thread559-22063. We use Unfrag which can reduce hthe file size in half. Keep in mind that as soon as you do a save the file size will increase again. BBJT CSWP

 

[MadMango]

Parasolid conversion seems to be the best way to reduce the size of files while retaining the overall representation of the part. We do it all the time here for OEM parts that have been modeled to reduce the parts to "dumb parts".

If you are looking for performance gains in your larger assemblies (which is different that just reducing file size) there are several seetings that you can tweak in Tools>Options. You can also remove details like fillets, helix-based features, etc from your parts as these are major resource hogs. "The attempt and not the deed confounds us."

 

[marieke]

Thank you for the tips. In fact, in our company we are starting to investigate to the possibility of building complete factory layouts in Solidsworks. At the moment the layouts are still done in 2D, but a 3D layout will be nicer to watch (seperate machines are allready designed completely in 3D). For that reason, it will be important to find out how to handle and build those assy's in a decent way. If we find interesting things I will try to post them on this forum. Also, if anyone has any experience (positive or negative) with factory layouts (up to 30 machine units) in Solidworks (or any other 3D solid modeller), I would like to invite you to post that experience.

Marieke
P.S. Are there people that have investigated the impact of certain features on the size of the part? Because for me there was no directly need to do that, I haven't done it before, but I can imagine that there will be quite some differences (there are so many ways to create a final geometry and I sometimes get a littlebit spoiled by the amount of available memory space on me workstation)

 

[MadMango]

I forget the actual size, and I am not sure if it is still present in SW01+, but back in the days of SW99-00 there was a limitation on the physical size of parts. I think it was something near 1024 meters in X, Y and Z.

Can somebody please confirm this. "The attempt and not the deed confounds us."

 

[marieke]

Yeah, ik read something about the maximum physical size of a part...I have tried it and for our factory layouts it's large enough (luckily our factories aren't that big). I have done some experiments and I was able to reduce the (memory) size of a part 4 times by using a combination of parasolid conversion and the method of embedding the part into a large rectangular extrusion (wich can be supressed).

 

[linqur]

Quote from solidworks.com:
[tt]Question : What is the size of the "modeling space" in SolidWorks?
Answer : In order to maintain a high degree of accuracy, SolidWorks limits the area in which geometry can be created in parts and assemblies. The total space available in SolidWorks (part or assembly) is a 1000 meter cube, centered on the origin. Also, any linear or diameter dimension value must be less than or equal to 1000 meters. Radial dimensions must be less than or equal to 500 meters.[/tt]
BR