[RobertW]

Dear All,

I prepare a model for 2D airflow analysis in Fluent.
Air flows through inlet -> air zone -> porous media -> air zone -> outlet

I am not sure whether I should define somehow the interface between porous media and 'air zone'.

Also I have another question related to selection of walls in my analysis. Please see the drawing attached.

I would be grateful for your help.
Thank you.
Regards

[vinerm]

Fluent does not require an interface between fluid and porous zone since both are fluid zones. So, you can create a mesh where all internal boundaries are interior.

As far as SpaceClaim is concerned, use Share option under Workbench Tab. That will share the topology only on the boundaries that are touching and rest will automatically become walls. You can then do the name selection in Meshing.

[RobertW]

@vinerm
Thank you for you kind reply. I am grateful.

I asked about these interfaces because Fluent confuses me in terms of definition of zones in the model.

I predefine some zones in Meshing Section (inlet zone, porous zone, outlet zone).
In Setup Section however, I get a mess in Cell Zone Conditions. Please refer to the attached figure. Certainly I do something wrong but I do not know what it could be. I would be grateful for any tip.

Thank you.
Regards.

[AlexanderZ]

form my point of view easiest way is to make name selections in workbench design modeler

space clam - create geom
workbench design modeler - import geom, make name selections
export geom to mesher

[vinerm]

First of all, remove the Contacts under Connections in the Mesh. Then, regenerate the mesh. After importing in Fluent, if it shows a cell zone as solid, just right click > Type > Fluid. Once that is done, look for wall and wall-shadow pair. Select one of those boundaries and change type to interior. Finally, you will end up with what you wanted.

[RobertW]

@vinerm
Thank you for your answer.
I have followed the recommendations. I am not sure whether I did everything right. Could you have a look on the attached figure please. Thank you again.

@AlexanderZ
I have started implementing this rule.
Thank you.

[vinerm]

Since you removed contacts in Meshing, it appears that you no longer have any interfaces or wall-shadow pairs; all the zones are fluid zone. So, just go ahead and run the simulation. No need to convert any zone into interior. It's all good now.

[RobertW]

@vinerm
Thank you for your reply.

Unfortunately, there is no interaction (airflow) between inlet zone-porous zone, porous zone-outlet zone. The air is entrapped between the inlet and porous zone (in inlet zone).

I would be very grateful if you could have a look on a couple of screenshots sent attached.
I have no idea were the problem is.

Thank you.
Regards

[vinerm]

The image you sent is not very clear, however, if there is no communication across the zones then that means you have multiple parts instead of single part. Open Meshing tool and then under Geometry, you should see a part and then all three bodies under the part. If all three bodies are listed directly under the Geometry then you have multiple parts, which is not good. There should be a part under Geometry and then all three bodies under the part. You have to go back to CAD, make a single part, remesh, and then open Fluent.

[RobertW]

@vinerm
Thank you for your answer.

I have checked Geometry section of Ansys Workbench and I am not sure how should I group 3 bodies under 1 part.

I created a geometry in SpaceClaim.
I have tried a few things in order to get 1 part and 3 bodies in Ansys Workbench Geometry:

- I kept 3 surfaces (inlet zone, porous zone, outlet zone) in 3 separate folders (in Spaceclaim) and as such I imported them to Ansys Workbench Geometry (File -> Import External Geometry File). Outcome - 3 parts, 3 bodies. I tried to allocate all three bodies to 1 part (in Ansys Workbench Geometry) but I did not figure out how I can do that.

- I kept 3 surfaces (inlet zone, porous zone, outlet zone) in 1 folder (in Spaceclaim) and as such I imported them to Ansys Workbench Geometry. Outcome - 3 parts, 3 bodies.

- I 'merged' 3 surfaces (inlet zone, porous zone, outlet zone) into 1 surface having separate 'regions', i.e. when I clicked on e.g. inlet zone then only this region was highlighted (in Spaceclaim) and as such I imported them to Ansys Workbench Geometry. Outcome - 1 part, 1 body.

In some tutorials that present similar scenarios, there are 3 parts and 3 bodies (1m50sec).
https://www.youtube.com/watch?v=1pxvdwEWc5Q&t=30s

Thank you.
Regards

[vinerm]

In SpaceClaim, you need to go to Workbench tab and then click on Share. It will show all the faces that will be shared across bodies. Click on Green Tick and then close SpaceClaim. Open Meshing and you will see now that all bodies belong to one part. Mesh and run the simulation.

[RobertW]

@vinerm
Thank you for your reply.

Unfortunately, I do not have the Workbench tab or Share command in Properties of group of elements (in SpaceClaim).

I have also tried neutral file (STP saved in SpaceClaim). What I get in Ansys Workbench meshing section is 1 surface.

I guess that before SpaceClaim joined Ansys, such 'share' feature could be resolved in some way. I clicked on various icons in Ansys, but I could not find anything relevant. Search in web also did not produce anything.

Thank you.
Regards

[vinerm]

Which version are you using? If you do not have current or rather new version of SpaceClaim, then you can either bring in a parasolid or step file in DM and then create single part in DM. Or you will have to create connections in Meshing and somehow maintain same number of nodes on both sides of the connections. Once in Fluent, you have to fuse these connected boundaries. However, fusion is possible only if the number of nodes on each side are equal and at approximately equal gap.

[RobertW]

@vinerm
Thank you for your answer.
I have SpaceClaim 2016.

Thank you.
Regards

[vinerm]

v2016 does not having Share option. So, I'd suggest you write a parasolid or step file from spaceclaim, open it in DM, provided you have license for DM, and then just form a new part. That's the only thing DM is required to do. If you do not have DM license, then the only option to make a conformal mesh is using connections in Meshing to ensure that number of faces on adjacent boundaries of two zones are same. If the model is 2D, then you can assign same sizing to both coincident edges, i.e., edges lying at exactly same location at the junctions of body 1 and body 2 and similarly body 2 and body 3.

[RobertW]

@vinerm
I eventually managed with 1 part 3 bodies problem.
I have created in SpaceClaim (2016) 1 surface (as entire 2D simulation domain). This surface is split into 3 sub-regions (I would call them as inlet zone, porous zone, outlet zone).
Ansys does not list these regions as bodies. In the tree, in meshing section, I have only 1 surface listed (in Geometry). But in Named Selections, I click on porous zone, and name it as 'porous zone'.
Model seems to be working ok.

Thank you.
Regards