CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Remeshing problem (http://www.cfd-online.com/Forums/cfx/122570-remeshing-problem.html)

Roland R August 22, 2013 07:38

Remeshing problem
 
Hello,

I would like to complete a remeshing process manually. There is a body which is in motion. I create the mesh files for five positions of the body. While the simulation is running I change the mesh files continously. Finally I have 5 res file which I have to read in post but I get the next notice:

Cannot add timestep. Number of nodes is different in result files.

How can I avoid this error?

Regards
Roland

brunoc August 22, 2013 10:11

Two options come to mind.

Option 1 - Remeshing setup:
Set your problem as a regular remeshing problem. When it asks for a script file for remeshing, just use an empty batch file (or a batch file that only displays a message - whatever). On the field for the resulting mesh, enter the name of the mesh you already have. All mesh files must have the same domain and BC names.

Option 2 - Regular multiconfiguration setup:
Load all your meshes into CFX-Pre. For each mesh, generate a separate 'Flow Analysis'. On 'Simulation Control', create one configuration for each 'Flow Analysis' and tie them together through their results, such that when on Flow Analysis ends another one starts (the manual has a tutorial for that). You'll be left with a .mdef file to run. After the simulation, you'll have a .mres file that contains you complete set of results.

Roland R August 22, 2013 11:03

Quote:

Originally Posted by brunoc (Post 447466)
Two options come to mind.

Option 1 - Remeshing setup:
Set your problem as a regular remeshing problem. When it asks for a script file for remeshing, just use an empty batch file (or a batch file that only displays a message - whatever). On the field for the resulting mesh, enter the name of the mesh you already have. All mesh files must have the same domain and BC names.

Option 2 - Regular multiconfiguration setup:
Load all your meshes into CFX-Pre. For each mesh, generate a separate 'Flow Analysis'. On 'Simulation Control', create one configuration for each 'Flow Analysis' and tie them together through their results, such that when on Flow Analysis ends another one starts (the manual has a tutorial for that). You'll be left with a .mdef file to run. After the simulation, you'll have a .mres file that contains you complete set of results.


Thank for your quick answer.
The first solution is OK, but where can I define a regular remeshing process in CFX 12?

Thanks a lot
Roland

brunoc August 22, 2013 11:20

I'm not sure about 12.0, but on 12.1 it is under 'Configurations' on its second tab.

The manual for 12.1 has a Remeshing Guide. Take a look at that.

Roland R August 23, 2013 11:03

Quote:

Originally Posted by brunoc (Post 447489)
I'm not sure about 12.0, but on 12.1 it is under 'Configurations' on its second tab.

The manual for 12.1 has a Remeshing Guide. Take a look at that.

I tried to apply your idea but I always get the next notice:

Unable to find "empty.bat" on the PATH. Please ensure that all required software is correctly installed.

(Empty.bat is an empty file)

Roland

Roland R October 11, 2013 10:30

Hello,

I have found the solution to my previos problem...

Now, I would like to make a remeshing simulation where I dont know the positions of the moving body so I can not generate the *.tin files previously. The solver should export the current geometry to ICEM.
Well, how can I this realize? Based on help, I didnt understand...

Thansks a lot

Roland

brunoc October 13, 2013 15:17

Quote:

Originally Posted by Roland R (Post 456373)
Now, I would like to make a remeshing simulation where I dont know the positions of the moving body so I can not generate the *.tin files previously. The solver should export the current geometry to ICEM.

It's doable, but it takes some extra steps.

First, you'll need to import the intermediate res file generated by the solver and open it on CFX-Pre. This will give you essentially the same case you had before, but with a deformed mesh. Generate a new def file with this deformed mesh and import this file into ICEM.

Now you have your deformed, updated mesh inside ICEM. With this you can recreate the geometry (I don't remember the exact command, but it's something to do with creating faceted surfaces based on the mesh). Once you have the geometry, regenerate the mesh as you wish and them update you CFX project with the new mesh. Then restart the simulation from where it last stopped.

In terms of your CFX setup, your remeshing script will have to handle all these steps: import the res file in Pre (which in turn requires a simple script for Pre); export a new def file; import the new def in ICEM; extract the geometry and generate a new mesh. The only steps that are automatically handled are the second mesh update on Pre and the solver restart.

Your ANSYS contact has an example that does that. Get in touch with them and ask for those files.

Cheers.

Roland R October 14, 2013 10:49

Helllo Brunoc,

thanks for your help. I solved the problem till "import the def file to ICEM". Now, I have a mesh in ICEM, but I dont know how can I change the mesh to geometry. You mentioned the faceted surfaces (or something same one) but I didnt find the solution. Could you remember perhabs the exact method to convert the mesh to geometry?

Thank a lot
Roland

brunoc October 14, 2013 13:37

Quote:

Originally Posted by Roland R (Post 456864)
Helllo Brunoc,

thanks for your help. I solved the problem till "import the def file to ICEM". Now, I have a mesh in ICEM, but I dont know how can I change the mesh to geometry. You mentioned the faceted surfaces (or something same one) but I didnt find the solution. Could you remember perhabs the exact method to convert the mesh to geometry?

Thank a lot
Roland

On the Menu, 'Edit > Mesh -> Facets'.

Cheers.

Roland R October 15, 2013 10:27

Quote:

Originally Posted by brunoc (Post 456897)
On the Menu, 'Edit > Mesh -> Facets'.

Cheers.

OK, I found it. Thanks a lot for your help!! :)


All times are GMT -4. The time now is 19:56.