Saving .sldasm ---> .sldprt

[matrix027]

Hello,

with solidworks 2003 it is possible now to save a assemly
to a part.
I want to use tis to save the assembly who don't change.
so the memory of the part will be the half size of the assembly
and also the mates will be reduced to max 3.

this has to affect the loadspeed.

does anyone have experience with this ?

 

[TateJ]

I'm 90% sure that - if you do this - you loose the functionality of the assembly.
The feeling I get is that saving an assembly as a part is handy if you want to send it to a client for approval - for example.
But if you still want to spec each part seperately in the BOM - you just blew it.
Without knowing exactly what you're needs are - let me suggest looking into an ENVELOPE part.
For example - we designed our own specialized bearings for our equpment. We buy thrust & roller bearings from SKF and have our housings machined and everything assembled at a local machine shop. So I have models and assemblies for all these parts, but I don't want/need all these pieces to show up in my equipment layout for a given project. So after designing and modeling the bearing, I made an ENVELOPE part in which all the geomentry is defined in context to the bearing assembly. Now I can insert the ENVELOPE into my equipment assembly. The bearing now shows up as a single part in my equipment BOM and I still have all my parts in the BOM for the bearing assembly that goes out to my machine shop.
I get the impression that you real concern is the size of you assembly files. This will solve that problem too.
Let me know if this is what you're loooking for.

H[sub]o[/sub][sup]3[/sup]
tatej@usfilter.com​

 

[MadMango]

You can also use the Join command to join parts of an assebly into a single part, then Save As a parasolid file. After this, save it back as a SLDPRT. We do this at my company for purchased parts that do not change (like motors and hydraulic components). Usually, the file sizes are smaller (but not always). "The attempt and not the deed confounds us."

 

[RawheadRex]

"I'm 90% sure that - if you do this - you loose the functionality of the assembly. The feeling I get is that saving an assembly as a part is handy if you want to send it to a client for approval - for example."

I believe the What's New manual for SW2003 says pretty much exactly what TateJ is alluding to above. His subsequent suggestion to use an Envelope part is the best way to handle things if his assumption is correct. I've used both Envelope and Join (which function similarly) but the performance of Envelope parts seemed better to me.

Might I also suggest a defrag utility such as ECOSqueeze if file size is a problem. It works quite well and is a free download.

Chris Gervais
Mechanical Designer
American Superconductor

 

[matrix027]

I am agree that saving a ssemly to a part , i loose the functionality.
But i have also the original assembly in the database.
I only use the converted part in my total model to save speed and memory while loading.
For the BOM i don't want to now the name of the parts in the assembly because they are dumb parts.
The name of the converted part have the article name (for example a motor )

I only want to use converted part (from assemblies) if they
don't change and the parts in the assembly ar dumb parts.

thanks guys.

 

[TateJ]

If the parts never change - then you're good to go.
I would still investigete the ENVELOPE PART strategy.
This way, both the part & assembly are linked - and minor changes to the assembly will show up in the part too.

H[sub]o[/sub][sup]3[/sup]
tatej@usfilter.com​

 

[RawheadRex]

A word of caution, creating dummy part files to represent your assemblies is something that can potentially come back to bite you because the link to the original parent doesn't exist. At the very least if you never have problems keeping track of what's what you will have a bit of tedious work ahead of you re-creating the dummy files whenever a change occurs to a parent assembly. We tried working this way for a time in my group and found that keeping up with things in this manner was more trouble than it was worth (at least to us). On the other hand, if the parent assembly files NEVER change then maybe this won't be a big deal for you.

Just curious but do you use lightweight parts/large assembly mode? This, we found was the best way to deal with performance issues in terms of loading, etc. for the way we work. I personally used to avoid this functionality like the plague because of one or two misconceptions that I had which someone set me straight on. Now we're able to open our top-level assembly files (~2000 parts) in rather short order (~1-2 minutes).

Our VAR did a seminar for our group on large-assembly management which helped us out significantly with our speed issues. If I'm not mistaken the core presentation looked as though it was prepared at SolidWorks in Concord, MA (not very far from where I'm at). It might be worth calling your VAR to check and see if they can do something like that for you if you're having major problems with speed. Also if you're running over a network that could be a significant source of your grief as well (it was definitely part of our problem). Run test cases between loading models locally and over the network. If there's a big difference (there should be at least some difference) then beat on your network guys for help.

Chris Gervais
Mechanical Designer
American Superconductor

 

[TateJ]

RawheadRex:
Been there - done that - bought a T-shirt. Lightweight Parts - doing it. Over a network - yes - we have all the speed we can get from it. The only way we've brought our speed up to something reasonable is to use ENVELOPE PARTS.

My ENVELOPE PART features are all defined in-context with the actual assembly. They are linked - intimately - the ENVELOPE part is in the assembly, but hidden. So, if the assembly parts change, the ENVELOPE changes. Sure, there's a few quirks, but it works for us. If you create a dummy part - outside the assembly - then I would agree with you.

H[sub]o[/sub][sup]3[/sup]
tatej@usfilter.com​

 

[matrix027]

tatej

i have a question about those enveloppe parts.

if i save a assembly t a part , i have for example 100 mates
reduced to max. 3 mates.
i think that mates also have an impact on load and calculate speed.

*** does enveloppe parts also have 3 mates ? ***


And i also use the lightweight mode .

 

[TateJ]

An ENVELOPE PART is only one part - so the only mates you'll have are the few that locate it in your assembly.
All the features of my ENVELOPE PART are defined in-context with the assembly it represents.

H[sub]o[/sub][sup]3[/sup]
tatej@usfilter.com​

 

[BBJT]

I may have missed something from the above post but envelopes do not show up ina BOM or for all that goes in the DRW either. BBJT CSWP

 

[TateJ]

True, but what happens if you insert your orignal assembly - with all the parts hidden - and your ENVELOPE PART visible?
You should get all your BOM data from the hidden parts, and only see your ENVELOPE PART.
I'm 95% sure this will work.

H[sub]o[/sub][sup]3[/sup]
tatej@usfilter.com​

 

[BBJT]

TateJ,

I am trying to understand the envelope thing.

What are you gaining by doing the envelope. If you hide and not suppress the assembly how is that going to help the performance of the assembly? Also how do you create a detail drawing? BBJT CSWP