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

Remeshing problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 22, 2013, 07:38
Default Remeshing problem
  #1
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
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
Roland R is offline   Reply With Quote

Old   August 22, 2013, 10:11
Default
  #2
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
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.
brunoc is offline   Reply With Quote

Old   August 22, 2013, 11:03
Default
  #3
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
Quote:
Originally Posted by brunoc View Post
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
Roland R is offline   Reply With Quote

Old   August 22, 2013, 11:20
Default
  #4
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
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.
brunoc is offline   Reply With Quote

Old   August 23, 2013, 11:03
Default
  #5
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
Quote:
Originally Posted by brunoc View Post
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 is offline   Reply With Quote

Old   October 11, 2013, 10:30
Default
  #6
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
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
Roland R is offline   Reply With Quote

Old   October 13, 2013, 15:17
Default
  #7
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by Roland R View Post
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.
brunoc is offline   Reply With Quote

Old   October 14, 2013, 10:49
Default
  #8
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
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
Roland R is offline   Reply With Quote

Old   October 14, 2013, 13:37
Default
  #9
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by Roland R View Post
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.
brunoc is offline   Reply With Quote

Old   October 15, 2013, 10:27
Default
  #10
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
Quote:
Originally Posted by brunoc View Post
On the Menu, 'Edit > Mesh -> Facets'.

Cheers.
OK, I found it. Thanks a lot for your help!!
Roland R is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Remeshing in FSI problem tctczxh CFX 12 September 25, 2014 11:11
Problem with moving mesh and remeshing technique.. stephen__white CFX 2 April 4, 2011 08:42
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 23:46.