CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Fine mesh make CFX-Pre react too slow (

Anna Tian July 28, 2012 07:41

Fine mesh make CFX-Pre react too slow

When I change coarse mesh to fine mesh, the CFX react very very slow. It even takes a lot time to press a button. But I have to work with fine mesh. May I ask how to solve this problem?

Best regards,

monkey1 July 31, 2012 03:26

The finer the mesh the bigger the files CFX pre has to load and the more Work it has to do...this is kind of normal. But I might guess you could solve your problem partially by getting more RAM.
For example a file with approx. 5.8 Mio Cells consumes around 400 mb RAM (260 MB PreEngine + 140 MB PreGUI_ogl) on my machine. When I load a nearly 15 Mio Cells file it increases to 840 mb RAM (595 MB PreEngine + 235 MB PreGUI_ogl) consumption.

ghorrocks July 31, 2012 06:45

Fine mesh means long run time. That is a fact of life.

So before running a fine mesh simulation:
* Do a sensitivity check to make sure you actually need the fine mesh
* Do all the debugging on a coarse mesh to make sure everything works as expected.

And when you run the big mesh make sure you Use a multi-processor option to speed things up.

Doginal August 1, 2012 14:11

If your having issues just in pre, along with the idea of doing all your debugging on a course mesh. I dont see any reason why you cant just set up your model in pre using a course mesh then switch to a fine mesh and just update your model with it.

singer1812 August 1, 2012 16:49

Second what Dog said. Just use a bogus coarse mesh for setup then dump fine mesh in when setup is complete.

Anna Tian August 2, 2012 09:08

May I ask what do you mean by using 'multi-processor'? I never heard about that. Does it mean I could use two computers to run my simulation at the same time?

monkey1 August 2, 2012 09:30

Not necessarily two (or more) computers. If you have a multicore CPU (e.g: Intel Core i7 Quad or similar) CFX is able to use the 4 (or more) cores for solving instead of doing a single core calculation.

Doginal August 2, 2012 12:56


Originally Posted by Anna Tian (Post 375039)
May I ask what do you mean by using 'multi-processor'? I never heard about that. Does it mean I could use two computers to run my simulation at the same time?

Ansys by default runs on serial processor setting. As in it will only run off of 1 processor (or 1 processor core).

In the case that you have multiple cores on the processor your using then you can using the MPI Parallel settings when trying to start the simulation to using more processors. Can speed up the run time drastically depending on the model you are running.

The only catch is you need to make sure your licensing can handle it. I believe your license need to enable the MPI setting and also each additional core uses another license.

The setting can be found when defining the run. Using the Platform MPI Local Parallel setting in the run mode option. Then select the number of processors/cores under the partitions setting below the run mode.

The local parallel mode is used when all cores/processors are on the local machine....the distributed i believe is when your are trying to link multiple computers together.

Also as a note to the original topic. If you use a course mesh to define everything in Pre then switch to a fine mesh. Be sure not to change your geometry file at all as you switch meshes. May result in changing some of the names of the geometry features and force you to redefine all your boundries in pre.

good luck


urosgrivc April 15, 2016 07:33

I had big problems with CFXpre oppening large mesh files:

Reducing mesh size changes opening time by a small fraction.

Biggest problems are (conections made in mesher) if these have a lot of surfaces, opening time can be in hours.

I had over 3000 surfaces in contact (fluid-solid) opening time went from
1.5 h to 5 min, just by deliting contacts in mesher.

All times are GMT -4. The time now is 13:17.