CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > ANSA

Batch Meshing and OpenFOAM 3.0

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 15, 2017, 20:06
Default Batch Meshing and OpenFOAM 3.0
  #1
New Member
 
hernan
Join Date: Mar 2013
Posts: 8
Rep Power: 11
tesorieri is on a distinguished road
Dear all,

I'm working on a 3D mesh using the Batch Mesh Manager. I've already worked my way around layer and volume meshing in rather simple 3D geometries but reached a dead end. I'll try to explain the issues I have in a general way, I can provide files and more detailed information if that helps.

I'm facing two problems:

1. When I try to output mesh data to FOAM, I find that patch faces aren't there (I have one inlet and one outlet which should appear in polymesh/boundary). The patch faces appear in PID's tab in ANSA; everything seems as the catalyst tutorial.

2. When working on a more complex geometry (where layers are collapsed or excluded), volume mesh generation fails (error message "Errors in volume boundary definition"). However, if I don't generate layers, volume mesh is OK. I've checked the auto-generated volume and it seems fine.

Any ideas will be welcomed!

Thanks!
tesorieri is offline   Reply With Quote

Old   May 16, 2017, 05:00
Default openfoam
  #2
New Member
 
demirel suleyman
Join Date: Apr 2017
Location: Turkey
Posts: 28
Rep Power: 7
dmirel is on a distinguished road
Hello,

1. Regarding the first question I can't help, I work with other solvers...

Did you tried to play with the paramaters from Options List before generating the volume(ex. Max. growth rate, Criterion. etc)? Another thing for the volume generation problem, did you re-defined the volume after creating the layers?

Hope this helped!
Mirel
dmirel is offline   Reply With Quote

Old   May 16, 2017, 13:14
Default
  #3
New Member
 
hernan
Join Date: Mar 2013
Posts: 8
Rep Power: 11
tesorieri is on a distinguished road
Hi Mirel, thanks for your reply!

1. Which solver do you use? I can try to export the mesh in that format and then convert it with mesh conversion tools of foam.

2. I think my problem is related to volume definition, as you said. In the simple 3D case layers are generated in one session and are put in a new part called "LAYERS". The remaining volume is put in a part called "Auto Detected Volume" when running the volume scenario. This last step seems to go wrong in the complex model.

For the complex model, I have several sessions in the layer scenario, so many parts and volumes are generated. I joined the layer parts in one big layer part, it still didn't work. I also see in the properties tab that several volumes are defined for the layers. I've been trying to join them before performing the volume meshing, but I still haven't figured out how to do this (maybe this is the volume redefinition you mentioned?)

The only thing that worked so far is to make a shell mesh with the batch manager and then use the MESH deck to generate layers and volume mesh. It's not what I want, as I'd prefer to use the batch manager to control layering differently in different parts of my geometry.

I'll post any update on the model.
tesorieri is offline   Reply With Quote

Old   May 17, 2017, 04:23
Default
  #4
New Member
 
demirel suleyman
Join Date: Apr 2017
Location: Turkey
Posts: 28
Rep Power: 7
dmirel is on a distinguished road
Hi,

1. I work in ANSYS Fluent and others.

2. Until now I didn't used the Batch Mesher to create layers and generate Volumes. My working steps are like this:
- I use the Batch Mesher for mesh ONLY
- I create the Layers from Volume Mesh Deck manually
- ONLY AFTER I generate the Layers I define the volumes remained.


If you first create the Volume Mesh and after that you are generating the layers, ANSA creates your solid mesh starting from the Shell mesh, not keeping count of your layers, so the layers and the solids are overlapping. So, if you can setup you batch mesher to first create your layers and only after to generate the Volume mesh maybe this will work. Sincerely I never use batch mesher for layering, only for meshing, so I dunno how helpful is my answer
dmirel is offline   Reply With Quote

Old   May 17, 2017, 04:43
Default
  #5
New Member
 
demirel suleyman
Join Date: Apr 2017
Location: Turkey
Posts: 28
Rep Power: 7
dmirel is on a distinguished road
Hello again,
I did a test with Batch Mesh Layering and I didn't found how to control layering differently in different parts, so I think you can't do that, you have to separate the parts manually.
dmirel is offline   Reply With Quote

Old   May 18, 2017, 12:41
Default
  #6
New Member
 
hernan
Join Date: Mar 2013
Posts: 8
Rep Power: 11
tesorieri is on a distinguished road
Hi, I got some updates:

1. I solved the output issue. It took me three steps:
a. I opened the Part manager and enabled the visibility of the geometry, layers and auto detected volume.
b. Then, I exported the mesh as a fluent mesh, selecting "Output: all" and Ascii format.
c. Finally, used fluentMeshToFoam to make the conversion.
2. Yes Mirel, as you say, creating the mesh with the batch manager and then using the layers and volume mesh in the volume deck (in that order) works fine. It is possible to create layers separately (manually). For that, you need to have different PID's for each geometry feature you want to layer separately, and then create several sessions for each PID under the same Layer Scenario. Of course, I think it is only useful if you want the layers to grow differently.

Well, now that I have a working mesh, I'll continue with the simulation. If anybody has similar issues, I'll be happy to help.
tesorieri is offline   Reply With Quote

Old   May 19, 2017, 05:43
Default
  #7
New Member
 
demirel suleyman
Join Date: Apr 2017
Location: Turkey
Posts: 28
Rep Power: 7
dmirel is on a distinguished road
Glad to hear that the things are working.
Have fun!
dmirel is offline   Reply With Quote

Old   May 23, 2017, 08:12
Default
  #8
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
Hi to all

Just to clarify something. If you want to grow layers with different parameters from different PIDs, you must not create several Layers scenarios or sessions.
You must instead create One Scenario, with One session and underneath it create a new Layers Area. You put in different Layer Areas different PIDs and then
ANSA grows all Layer areas simultaneously and hence the are all connected together and connected propetly with the rest of the domain.

If you grow layers in different scenarios or session they grow sequentially one after another and hence they are not connected together. As a result the volume definition afterwards goes wrong and volume meshing fails

Look for more info under Help>ANSA online documentation index
ANSA for CFD Brief User Guide

Hope this helps

Vangelis
vangelis is offline   Reply With Quote

Old   May 24, 2017, 15:47
Default
  #9
New Member
 
hernan
Join Date: Mar 2013
Posts: 8
Rep Power: 11
tesorieri is on a distinguished road
Thanks Vangelis,

It helps a lot. I thought that my problem was related to volume definition and to how I created layers. I'll give a try your solution and update on results.

Cheers!
tesorieri is offline   Reply With Quote

Old   May 24, 2017, 16:40
Default
  #10
New Member
 
hernan
Join Date: Mar 2013
Posts: 8
Rep Power: 11
tesorieri is on a distinguished road
Update:

I've followed Vangelis suggestions and got everything working. By assigning PID's to different areas you get a single Layer Volume. Then the auto detection works just fine for the rest of the mesh.
tesorieri is offline   Reply With Quote

Old   May 25, 2017, 03:10
Default
  #11
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
Glad it worked out for you!
vangelis is offline   Reply With Quote

Reply

Tags
batch mesh, openfoam

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
Map of the OpenFOAM Forum - Understanding where to post your questions! wyldckat OpenFOAM 10 September 2, 2021 06:29
OpenFOAM 4.0 Released CFDFoundation OpenFOAM Announcements from OpenFOAM Foundation 2 October 6, 2017 06:40
NEW OpenFOAM GUI (WIN/LIN) & AUTOMATIC MESHING WORKFLOW: cfSuite (try it for FREE) Creative Fields, Ltd. OpenFOAM Announcements from Other Sources 0 June 8, 2014 11:31
New OpenFOAM Forum Structure jola OpenFOAM 2 October 19, 2011 07:55
[Other] CastNet: modeling and meshing tool for OpenFOAM ulli OpenFOAM Meshing & Mesh Conversion 7 May 31, 2011 02:14


All times are GMT -4. The time now is 09:29.