[anand32]

Hi there


I recently meshed a model in ICEM CFD and imported the mesh in ANSYS FLUENT.
On importing, I found out that the boundary conditions had been wrongly assigned.
Specifically, there is a box. Currently the whole box is a single Part and has been assigned the same boundary condition throughout. However, ideally one of the surfaces should have a different boundary condition than the other 5.
How do I ensure that?

Is it as simple as going back to ICEM and creating a new part of this surface, and let the original part have only 5 surfaces?

I am concerned because the mesh has been generated and so the part will have mesh information with it. Will moving the one surface from one part to another will be enough in this case?

Please let me know.

Thank you

[kad]

There are different ways of doing this. In general it is enough to load only the mesh in ICEM. For assigning boundary conditions for a specific surface it has to be in its own part. You can access the different operations (e.g. creating one) via RMB over parts in Display tree. In the "selection menu" toggle on the tools for mesh selection (to the very right of it). There are some very helpful functions available in the selection menu like "pick all elements up to an angle" for selecting the appropriate surface elements.

Another approach is to do this via geometry modification by assigning the surface to a new part. One obvious possibilty then is to do a full re-mesh of your model. This is not neccessary in general. You can also reassociate an existing mesh to a modified geometry. You can find this function under "Repair mesh" -> Associate. Make sure to make associations only for shell/surface elements.

[anand32]

Thank you Kad for this help.

I tried the second option; wherein I created a new part for the lone surface and did Repair Mesh -> Associate Mesh (Surface elements).

When I imported the mesh in FLUENT, the surfaces were in different boundary zones.

Thank you

[anand32]

Originally Posted by kad

There are different ways of doing this. In general it is enough to load only the mesh in ICEM. For assigning boundary conditions for a specific surface it has to be in its own part. You can access the different operations (e.g. creating one) via RMB over parts in Display tree. In the "selection menu" toggle on the tools for mesh selection (to the very right of it). There are some very helpful functions available in the selection menu like "pick all elements up to an angle" for selecting the appropriate surface elements.

Another approach is to do this via geometry modification by assigning the surface to a new part. One obvious possibilty then is to do a full re-mesh of your model. This is not neccessary in general. You can also reassociate an existing mesh to a modified geometry. You can find this function under "Repair mesh" -> Associate. Make sure to make associations only for shell/surface elements.

Kad,

Could you tell me how to do the same thing inside FLUENT?

Thank you

[kad]

I am not really shure about this one. I think it is possible in Fluent but I only have access to an older version and I do not use it very often. You might try the Separate function under Mesh. Check the manual for this one.

[hello-fluenttt]

Originally Posted by anand32

Thank you Kad for this help.

I tried the second option; wherein I created a new part for the lone surface and did Repair Mesh -> Associate Mesh (Surface elements).

When I imported the mesh in FLUENT, the surfaces were in different boundary zones.

Thank you

Hello

Could you explain how you solved this problem.?

My problem is-
I generated geometry and then i created parts. but once meshing is done, these parts get modified automatically, for example. initially the whole circle(surface) is inlet but later a part of circle is only inlet and remaining part is assigned to some other part say outlet. If thats the same problem as yours, plz. explain how do i solve this. Can i edit the parts after meshing or avoid the altercation ??

Thankyou

[anand32]

Originally Posted by hello-fluenttt

Hello

Could you explain how you solved this problem.?

My problem is-
I generated geometry and then i created parts. but once meshing is done, these parts get modified automatically, for example. initially the whole circle(surface) is inlet but later a part of circle is only inlet and remaining part is assigned to some other part say outlet. If thats the same problem as yours, plz. explain how do i solve this. Can i edit the parts after meshing or avoid the altercation ??

Thankyou

Yes I could.

There are two ways to change the parts associated to mesh elements in ICEM, after the mesh has been created:

1. Method 1: After the generation of mesh, go to "Edit Mesh" ==> "Repair Mesh" ==> Associate Mesh to Geometry. In the selection toolbar which opens up, select the penultimate (last but one) option- All Surface elements.

When you do that, ICEM automatically assigns surface elements to the nearest surface part.
However, this method is automatic and we do not have much control over the surface part to which the mesh elements are being assigned. There is a manual method too.

2. Method 2: Right Click on the part name in the "Display Tree". Select "Add to Part". Select the mesh elements which you want to add to this part (select "mesh elements" tab should be switched on). And you are done!

This method affords the use much more control since you are manually associating the elements to the corresponding surface parts. However, this method is slower if you want to associate elements to many parts one at a time.

Thank you

Vish

----------------------
Subsribe to my YouTube Channel to learn ICEM from Scratch:

A First Course in ICEM Hexa

[Far]

Excellent