2D Drawing view placement / regen very slow

[awilson-2]

Does any one else have this issue.....

When I place a view on a 2D drawing and try to set it's orientation (say left view or front view) then click ok it can take up to 20 minutes to respond and update the view. This model is not a very complex assembly. In fact the entire model loads fairly quickly and regenerates just fine in the 3D world. Just hangs up badly when creating a drawing. This issue is not limited to this particular assembly. I see it in about 50% of my work.... I spend $$$ on a top end graphics adapter, maxed out my RAM to 16GB and have a not so shabby dual core workstation.

It's got to be a setting somewhere...

Can anyone help? I'm wasting hours a day just waiting for Creo to respond.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[StephenW]

Is it just when placing the view or does it continue slow on that drawing?

Our major drawings take a lot of time, graphics doesn't particularly help and more RAM only helps if you are actually running out of RAM.

I would first check your system. Make sure you aren't actually running out of RAM.

What video card?  Dual core only helps when running other stuff, not Creo.

If you use drawing templates, you may want to try starting the drawing without the template.

If you don't use templates, try removing (or renaming) the drawing setup file and creating the drawing so all drawing setup options are default.

You may want to try starting Creo with NO config.pro set. Rename your configs so they won't load. everything will be default. Try creating the drawing again.

[mender]

Very difficulty to say what might be going on without seeing the particular drawing/assembly, I would recommend filing an SPR and we can look into it.  One thing you might try is to update the drawing to all bug fixes with File>Prepare>Drawing Properties>Detail Options, 'update_drawing' for the name and 'all' for the value, and regen the drawing, then see if the problem no longer occurs.

[StephenW]

Would this be something you would want to do on the drawing template to clean it up?

[awilson-2]

Thanks for the posts...

This issue, when it happens, only seems to affect the parent view. I can place and modify projections just fine. Dimension, balloon, notes, etc. all fine. If I try to modify the properties of the parent view in any way it locks up for 10-20 minutes (not responding). The assembly does not seem to have any issues. It regenerates just fine and shows not regen errors. I have had this happen several times before. Starting over with a fresh drawing does not help, but I will try using a blank page with no template...

I am using a Quadro K4200 graphics adapter and custom drawing templates with tables.

[StephenW]

Definitely try Matthew's updated drawing setting. It fixes odd issues.

You've got an odd problem if its only happening on the parent view, not at all what I was expecting. 

[rreifsnyder]

You might try adding this to your config.pro display_in_adding_view minimal_wireframe

It prevents datums and several other entities from showing and because it is wireframe it does not have to do hidden line removal which is probably the biggest thing slowing down drawing views. Remember that the graphics card is not used for drawing views unless you use fasthlr_drawing set to yes. The problem with FastHLR for drawings is that it is not exactly WYSIWYG. Also, as far as the CPU remember that Creo is single threaded and therefore multiple cores does not help. I have found that Core-i7 based CPU's with high clock speeds especially from this list PassMark CPU Benchmarks - Single Thread Performance