CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

CFX-Pre takes forever to open

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes
  • 2 Post By ghorrocks
  • 1 Post By ghorrocks
  • 1 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 22, 2021, 02:36
Default CFX-Pre takes forever to open
  #1
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 407
Rep Power: 14
Светлана is on a distinguished road
Hello! I have around 10 million mesh elements. The CFX-Pre window takes over 10-20 minutes to open. What's worse, it appears to be using only one CPU core out of 8 (Windows) or 16 (Linux). 16GB RAM (Windows) or 96GB RAM (Linux) available. The .cfx file size being only 3GB. What could possibly take it so long? Any tips? Thanks!
Светлана is offline   Reply With Quote

Old   September 22, 2021, 03:32
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
CFX-Pre does take a very long time to load some times. It is only a single threaded application so it will only ever run on a single CPU. So you cannot fix that.

But here are some things to do to speed CFX-Pre up:
1) Run it stand-alone, not in workbench. You get a lot more control over things stand-alone.
2) Before you load your file, turn off some options (under Edit/Options) which can take forever:
a) CFX-Pre/General/Auto Generation - turn off auto default interfaces
b) CFX-Pre/Graphics Style - Object highlighting - change to bounding box.
c) CFX-Pre/Render - Turn off Draw Faces and Specular lighting. Note you won't see anything if you do this! If you are really desperate you can turn visibility off. You won't see anything, but for some really big models it is required
d) CFX-Pre/Labels and Markers/Labels - turn Show Labels off.
e) CFX-Pre/Labels and Markers/Boundary Markers - turn Show Boundary Markers off.

You might have to close and reopen CFX-Pre to make these options take effect.

But try loading your file then and hopefully it will be much faster. But it will not look as pretty, that is the price you pay.
AtoHM and aero_head like this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   September 22, 2021, 17:27
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,788
Rep Power: 31
Opaque will become famous soon enough
Which version are you running?

What operating system are you using? Windows 10? Linux?

Sometimes is not only about the mesh, but the physics details, say 100's of domains, domain interfaces, boundaries, etc.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   September 22, 2021, 18:22
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Opaque's comments remind me - a common source of this problem is geometries with thousands of surfaces. ANSYS meshing by default creates an individual surface on each one, and that can overwhelm CFX-Pre. If you generate your mesh in ANSYS Meshing, then load it into ICEM (or any other good mesh editor) and merge all the surface groups you do not need into one big surface group. Then import the ICEM mesh into CFX-Pre and you should only have the surface groups you need, and CFX-Pre will run much better.
Opaque likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   September 23, 2021, 05:39
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,818
Rep Power: 27
Gert-Jan will become famous soon enough
The fact that your .cfx file is 3Gb, while you have only 10 million elements, tells me something is wrong, or at least different from standard. With 10million elements, I usually end up with a file size of around 100 Mb.

So I guess, Glenn is right, the geo might be too complex with too many named surfaces.
Opaque likes this.
Gert-Jan is offline   Reply With Quote

Old   October 24, 2021, 22:10
Default
  #6
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 407
Rep Power: 14
Светлана is on a distinguished road
Thank you! 2a helped the most.
Светлана is offline   Reply With Quote

Old   October 24, 2021, 22:12
Default
  #7
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 407
Rep Power: 14
Светлана is on a distinguished road
It's 2021R1, problem with in Linux and Windows. Agreed that there is too many faces named F3445.435 etc in CFX-Pre. Would be very interested to know a few short tips about how to merge surface groups in ICEM.
Светлана is offline   Reply With Quote

Old   October 24, 2021, 23:09
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
ICEM is very different to ANSYS-Mesh. You will need to do the tutorials with ICEM to understand it. If all you are doing is just renaming faces so you can group them together and reduce the face count then the key areas you need to look at are parts and adding and removing items to parts. This is all in the ICEM tutorials. A lot of the tutorial will cover generating meshes - this is not relevant to this case.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 25, 2021, 18:24
Default
  #9
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,818
Rep Power: 27
Gert-Jan will become famous soon enough
- How did you generate the mesh?
- In ICEM, you need to create parts. To each part, you can add elements by picking, or box select, or ..... many more options...... When finished, export the mesh to ANSYS-CFX (.cfx5-file), and import it as ICEM-file in Pre.
Gert-Jan is offline   Reply With Quote

Reply

Tags
cfx, slow simulation

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM.com] swak4foam compiling issues on a cluster saj216 OpenFOAM Installation 5 January 17, 2023 17:05
OpenFoam "Permission denied" and "command not found" problems. iyidaniel@yahoo.co.uk OpenFOAM Running, Solving & CFD 11 January 2, 2018 07:47
[swak4Foam] groovyBC in openFOAM-2.0 for parabolic velocity bc ofslcm OpenFOAM Community Contributions 25 March 6, 2017 11:03
interFoam & decomposition method: scotch MacGyver OpenFOAM Running, Solving & CFD 2 May 23, 2012 08:00
Problem installing on Ubuntu 9.10 -> 'Cannot open : No such file or directory' mfiandor OpenFOAM Installation 2 January 25, 2010 10:50


All times are GMT -4. The time now is 01:15.