Batch Meshing and OpenFOAM 3.0
 

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!

openfoam
 

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

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.

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 :(

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.

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.

Glad to hear that the things are working.
Have fun!

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

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!

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.

Glad it worked out for you!