Currently working on the very large assemblies (tractor).I have made the simplefied reps also,still it takes a very large time for regeneration,Include,exclude and substitute reps.
Assembly opening takes 20 min time.working on the 24 GB system...please help or suggest any technique.
Simplified reps should certainly help, but also based on some recent benchmarking I am very leery of the "workstations" most vendors are selling for top dollar. I don't know about the Z800 series of workstations for certain, but we recently tested the newest Z440, our prior standard Z420 and the Z230. The Z230 was about 36% faster than the older Z420 and 25% faster than the Z440 using the OCUS benchmark (www.proesite.com). I know in the past there were definite performance enhancements by using the Xeon processors, but right now for Creo 2, the i7 processor in the cheaper Z230 blew the Xeon away. Also we are seeing real improvements with Solid State Drives. The Z230 can take up to 32 Gb RAM. Remember also, than RAM does NOT necessarily mean speed. As long as you have enough RAM, adding more doesn't speed anything up.
Does your open process include a workspace connected to Windchill? (a big impact on performance is cache folder size)
Are you calling for objects from a windchill server on the fly? (are all the objects in your workspace)
Are there family tables included in any of the sub-assemblies? (regenerate generic- PTC would recommend Instance Accelerators)
What version of Creo? (some versions are better than others)
All of these are worthy to check.
I have been hoping for a magic config option to prevent regeneration of family tables when opening simp reps for a long time!
Did you consider using family table instance accelerators ? in majority of cases their presence will eliminate instance generation upon retrieval, and reduce time dramatically. Lately we increased robustness of their usage vs. older Wildfire versions. They are mostly recommended for finished parts of design, but can be used on in-work stages as well, though less efficient as they will need to recreate upon Save after instance is modified.
Currently working with Creo-2 version. Not working on the wind chill and the related all files(part and assemblies) are on the local drive itself.
Yes some components, mostly hardware's are having the family tables.
Thanks & Regards,
When dealing with slow retrieval times, you have to consider a few different things... Network Speed (if remote storage is used), Wind Chill Server speed, or the Hardware on the Workstation itself. Since your last message says you doing everything local... You'll need to look at your hardware specs not just model number and amount of RAM. Z800 and 24GB tells us very little...
I don't want to turn this into a plug for my company, but to Robert's point, I have worked with many companies who have been disappointed with the off-the-shelf "workstations" that some companies are trying to sell for top dollar. It boils down to these companies are trying to sell a "workstation" that fits everyone so that they can sell high volumes off an assembly line. The fact is that if you want Creo to run as fast as possible, then you need to understand how Creo works and build a machine that allows the software to do what it wants to do. Really, this is true no matter what the software... CAD, Photo-Rendering, or FEA... each type of software has different needs and a specific "workstation" should be different for each.
I would start first with what you have told us. Very Large assembly and 24GB. - Check your task manager when the full assembly is in session. Are you pulling in more than your 24GB physical limit? If so, then your in "swap space" and being in swap really slows the performance of the machine. In this case, (if you can) simply add more RAM to your machine and you should notice an improvement.
Beyond that, we'll need to know some more details. Creo is still largely a single threaded software, so CPU, Motherboard, RAM, and Hard drive speed all have a huge impact on performance. Its time to do some homework...
CPU: Intel or AMD?... if Intel- Xeon or i5 or i7?... speed (in Ghz)?... Overclocked or not?...
MOBO: Workstation/Server class board, (supports Xeon CPU's) - or Workstation/Gaming class board (supports i7 CPU's)?
RAM: How much do you really need? (keep the machine out of swap) Whats the RAM speed? (in Mhz) (1033, 1600, 2133, 2400, etc)
Hard Drive: mechanical disc, or SSD? if mechanical whats the RPM speed? (5200, 7200, 10K)
There are other details you can look at within these categories as well. for example: Whats the latency of the RAM? or whats the seek time and data transfer rates of the hard drive? etc... In general though, the information gathered on the items listed above will go a long way toward telling you where the problem is.
Owner / Design / Builder
PTC needs to have the customer's experiencing success with instance accelerator's in a Windchill environment to start proclaiming how great they are!
Have you used Creo View connected to Windchill with extremely large assemblies? It does circles around Parametric with large assemblies in regards to loading, searching and selecting. Parametric can only load one configuration at a time...View can load 16 simplified reps concurrntly into 16 views from one top level assembly and it doesn't have to regenerate.
I really wish the Parametric team chose to use the PVZ/OL files for the lightweight graphics rep functionality instead of using the PVT files in Windchill. I personally think you would have hit a home run with an OL strategy in the long run. I'm sure PTC has their reasons...but I can still hope and voice my opinion!
Please elaborate on any specific problem you see on Windchill with instance accelerators - we definitely shall know if we have some. Accelerators are a suggested performance improvement method and is desired to work smooth with Windchill, being a "secondary content" to each generic.
.xpr files are definitely not any miracle - they simply prevent instance parts / assemblies from generating upon retrieval, taking finished geometry from accelerator model, but this means respectively reducing retrieval time. Mentioned time saving is relevant for the case when instance is in Master Rep, as well as in Geom / Graphics rep.
I do not argue Creo View retrieval performance if far superior to Creo Parametric - though you can barely compare the two, considering amount of data that Creo Parametric brings with it. And yes, please be sure - we do put continuous effort on improvement of retrieval performance, this is on high priority of respective development department. Not sure if you attended latest (January) TC where it was discussed in quite a details. If not - watch out for June event, I guess (hope, cross fingers 🙂 that you will get good news on this topic.
Any chance for instrumenting Creo - number of CPU cycle per feature, memory consumed per feature, GPU used? It's difficult to determine what the best method is with scanty feedback and difficulty separating out file system, network, PDM, and model interpreter performance. I've seen people complain about how long things take and am lead to believe it's delays from Windchill traffic or poor hardware choice, not actual model interpretation performance. The last place I worked I would sometimes hit save and the software would stall for 30 minutes. Make some more changes, hit save and it's 30 seconds. No way to debug.
Creo is a software development system, but without the tools most software developer access for profiling to improve performance.
That's a good point, David. Hope product management watches this thread ...