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  #1  
Old 09-27-2001, 11:03 AM
Rick singer
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working with very large assemblies

greetings, we are struggling with the logistics of creating drawings of very large assemblies. Updates take 24+ hours, even with EconoFast; files are enormous (65+ MB) so store times into WorkManager are agonizing. I'm wondering how other users handle these issues. As a basis of comparison, assemblies are in the 10-50k range for number of parts and sub-assemblies (some shared but not an enormous percentage). Package files for the assemblies are on the order of 125 MB. Also, we are using UNIX, C3600's with 1 GB memory and 1 GB swap. Any of you out there doing similar things and having similar experiences? thanks.
  #2  
Old 09-29-2001, 06:41 AM
Stefano
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re: working with very large assemblies

we r using HP J5000 with 1GB memory and more then 1.5 GB swap, not using WorkManager. Our bigger one is made with more then 5k pieces and it makes a 150 mb package file, we use intensive shared parts. mi file is depending of number of view and sheets, normally they r near to 25 MB. We saw dramatic better in SD8 then 7.51. before we needed more them 10 hours and now it is near to 1 hour for each view. With SD8 we can use more than 1GB data and we r upgrading the system to 2 GB memory, I think this will help us. We try to create drawings with few views, better to create one drawing for each one of this large. Our system has two cpus but I think SD see only one and this could be a problem, often first cpu is on 100% and other to near 20% working only for the system I think. We try to ask remote update on the system itself and we saw 2nd cpu jump to 100%, I think this is better way but we didn't try it with this large one, exange file will be really big, but we will test it better with the upgrade system with more memory and HDs. I hope this can help you.
  #3  
Old 09-30-2001, 03:32 PM
sdf
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re: working with very large assemblies

sdfdf
  #4  
Old 10-05-2001, 12:40 AM
Claus Brod
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re: working with very large assemblies

Rick,

unfortunately, there is not a single easy answer to your question since the drawing generation performance (which is the part of the question I can address) depends on many things: used hardware, available memory, size and nature of the model, usage of shared parts, usage of library parts, EconoFast on/off, hidden line settings etc etc. Therefore, I can only give some general hints:

  • First of all, most of Stefano's hints mentioned above are right on.
  • In SD 9, switch off automatic center and symmetry line generation if you do not need it.
  • Use EconoFast where possible.
  • Use view component lists to remove insignificant or unimportant parts from views where possible.
  • Use remote server updates where possible.
  • Try modifying the drawing generation accuracy (contact CoCreate support for details)
  • Avoid sections, cutaways, detail views where possible
  • Isometric views are typically slower than standard views.
  • Make sure that the view direction is exactly perpendicular to the main faces in the model (and not slightly tilted).
  • Consider generating drawings on PCs. Today's PCs are often twice as fast as your current HP-UX hardware, sometimes even faster than that.
We are working on significant performance improvements in the drawing generation area for an upcoming release of SolidDesigner (unfortunately, not the immediate next release). We think this will be a major step forward again which should address the issues of customers who are dealing with very large assemblies.

Claus

  #5  
Old 10-11-2001, 06:09 AM
Dave Halseth
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re: working with very large assemblies

Avoid clashes. Annotation really doesn't like clashes, it will spend a lot of time trying to figure out where it should or shouldn't put lines. We've had problems where we have made simple representations of threaded parts (ball screws and nuts, fasteners, etc.). Check to be sure that your assemblies are free of interferences.
 


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