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VeryLarge Assemblies


New member
Hi everybody,

I am working with an Automotive company here in India making Commercial Vehicles. We have been using Pro/Engineer for Product development. Currently we are running Pro/E 2001 and Intralink 2.0.

We are facing issues with handling large assemblies. The assemblies ( data size ~ 1.2 GB) takes about 30 min to 1 hour to open in Pro/Engineer (if opened in geometry rep). In the master rep these assemblies don't open at all and Pro/E crashes.

We are using Windows NT based systems. Pentium 4 / 1GB RAM/ 64 MB graphics

We are also aware of the large assembly management tools in Pro/E like simplified reps.

I would like to know how other companies are handling such a large data. Do they need to open the entire vehicle assembly at all? What is the best working methodology in such scenario?


New member
The best methodology is using simplified reps like you mentioned.

All assemblies have those three pre-defined reps built in. It sounds like you are indeed opening them by using the Open Rep button in the File Open dialog box. But you can also create a simplified rep on the fly when you open the assembly. After you choose Open Rep, there's a checkbox for creating a new rep. Pro retrieves the model tree information and you can pick and choose how much detail you want to retrieve for each component.

Another option is to make non-associative shrinkwrap parts of your large assemblies, if the work that you're doing can still be satisfied. A shrinkwrap part will be typically 60-90% than the original assembly.

And it's recommended that you have 3 times as much RAM as the size of the assembly you're trying to open. That way you won't have to use swap space on your hard drive, which can be incredibly slow.

David Martin

Torgon Industries


New member
I am also searching for the best possible solution to large assembly management. Simplified reps at the assembly level seem to be the only solution as a Geometry rep. I am also looking into simplifed part reps and substitution. Shrinkwrap seems to be out of the question. Shrinkwrap requires storage of new data external to the part or assembly. I also cannot find the option to make the shrinkwrap dependant upon the original model. I am using 2001. It seems the software does not have the definitive solution to large assembly management? Any expert feedback on this subject would be appreciated.


To create an associative shrinkwrap feature (as opposed to a shrinkwrap export model), look in the Data Sharing features.

Shrinkwrap export model:

Creates a separate part model not associated to the original. Options include Faceted Solid, Merged Solid, and Surface Subset

Shrinkwrap feature:

Creates a surface subset of an assembly as a single feature. This surface subset is associative back to the original source geometry. This feature will reference the currently active top-level assembly (even if the feature is being added to a sub-sub-sub-part of that assembly using modify-modify-part).

External Shrinkwrap feature:

Does the same thing as the regular Shrinkwrap feature, but you must specify the source model.

Here is one case for usage:

1. UserA designing a vehicle frame

2. UserB designing a wiring harness that must be routed through the frame.

3. UserB would like to reference a lot of gemetry from UserA, but doesn't want his assembly tied directly to the frame.

4. UserA creates a part in his frame assembly (the very last part) and populates it with a single feature while in assembly mode - a shrinkwrap feature which will reference the entire frame assembly (I call this a publish part).

5. UserB then takes this part and assembles it into his wiring harness assembly and uses it as needed for references

6. As UserA updates his frame, the frame publish part is updated and gets checked in with the frame (no extra work required).

7. UserB sees that the frame publish part is out of date, so he grabs the latest one and keeps on routing his harness around the latest frame geometry.

The idea here is that UserB does not ever need to check out or pull up the frame assembly in order to do his work. If certain frame parts are not required, the shrinkwrap feature can be easily redefined to exclude certiain components.

...Just one idea

-Brian Adkins


New member
try this:

change first the level detail to a smaller value

View/Display settings/Performance/Level detail

and than open the .asm


New member
The problem (crashing) that you have is probably related to upper limit for addressing memory. Teoretically it is 2 GB, but it depends on application and software writers. Pro/E usually crashes at around 1.6 or 1.7 GB (ansys crashes earlier at 1.2 GB) and if you take a look at PTC tech support this is described somewhere. By that information, you should make a patch on Pro/E and this is something that no one does.

There is 64 bit version of Pro/E, but it works 30% slowly than 32 bit one.

have a closer look at:




I hope that you have access to tech. support.

It is nice to hear that someone uses Pro/E together with Pro/I on such large assemblies. The biggest Pro/E assy that I have seen contains over 350.000 parts (windows platform) but was done without the use of Intralink.

There was also an upper limit in Pro/I regarding the number of items inside Pro/I database, but this was recently fixed. I do not know if this is true for your version of Intralink.



New member
I would like to thank everyone for their expert advice. I have been playing with options, simplified reps and shrinkwrap. The smallest asm of components seems to be shrinkwrap. Attached are part_a, part_b which both have accelerated simplified reps, box_pin.asm which has both a simplified rep and shrinkwrap as a feature. Note, when assembling the shrinkwrap to the upper level asm, the upper level asm is smaller than the original asm. I do wish I could create a relational shrinkwrap at the part level. I have tried Publish Geom. At the part level, do I have any options so that when I assemble, I can replace the component with something other than a simplified rep? Banging my head off the wall, but getting somewhere :)


New member
One place almost always overlooked by users when trying to control database size is at the part level. We can create large amounts of feature geometry quickly in a part (usually by patterning) and then we tend to create a family table part with fewer features. What most people don't understand is when retrieving an instance of the family table, the generic data is always brought into session. We create our large pattern parts and then use a small repeat number in the generic and use the family table to expand to the full pattern. We swap out the family tabled part only when we need to show the full pattern for display purposes. Parts can also have simplified reps to reduce memory use. Keep parts used in the assembly as simple as possible.

Our assemblies use simplified reps and shrinkwraps to help control the assembly size.

For drawings, create a rep that shows only what is necessary for the drawing purpose and use it to create the drawing views. Shrinkwraps do not work well on drawings and should be avoided.

I spent 6 months developing our large assembly management techniques - the hard part is getting people to use them.


Lots of good advice here.

Here is my 2 cents worth from my experiences.

1)You need a better video card. At least 128 MB.

2) You need more ram 2GB for Large assembly but at a minimu you need enough memory to completely load your model into memory with enough left over for the rest of your applications.

3) Use skeletons to build the assembly.

4) Shrinkwrap sub-assemblies. Surfaces are smaller than solids.

5) Use simp reps extensively even at the part level to reduce detail.

6) always open a simp rep.

7) reduce/eliminate external references.

8) Make sure all componets are loaded locally and not on the network.

9) use top down design to reduce the top assembly to a small set of sub-assemblies instead of hundreds of parts and small sub-assemblies.

I took a multi GB model that took over 4 hrs to come up on an Ultra 60 with 2GB ram and ELite 3d card and it came up in 12 minutes and was easliy used and manipulated.

Good luck


New member

The biggest problem with shrinkwraps on drawings is you end up with empty space on any cross-section views cutting thru the shrinkwrap. You also need to use the Quilt HLR option when doing the view cosmetics and these seem to take a very long time to regen the first time the sheet is opened or if a change is made to the view.


I agree on the cross section thing...

I guess we don't use them enough to notice the problem with the QuiltHLR option... It works good enough for now.

It might be cool if there was an option to define a section view to grab the section geoemtry from the parent of a shrinkwrap feature. It would take longer to regen, but it might be worth it for some people.

-Brian Adkins


New member
Here is a trick for opening any assembly, no matter how large, on any Pro/E terminal. When opening the assembly, there is an option for Simplified Rep on the bottom panel, choose Open Rep, check the radio button Create New Simplified Rep, give it a name, choose Exclude Comp, then add components you would like to see. There is also an option for Geometry Rep whose default it to Exclude all components. One setback is a Geometry Rep for a component cannot be created if the file is Pro/E Rev 17 or earlier.