Importing 2D separated Hybrid mesh from PointWise to Ansys Fluent
 

Hi! I'm new in CFD Online, so I hope I post my message correctly.
I see you've made your mesh in "PointWise". I also work on simulation of a 2-element airfoil and I chose PointWise for meshing.
I try to create 10-20 steps extrusion around each airfoil (structured mesh) and for the rest of the domain I use triangular mesh (unstructured) so in total I have 3 separated domain. In PointWise it seems it's impossible to join structured to unstructured domains. Now my question is how you imported your hybrid mesh into Fluent?
Thanks in advance for your replay
Masoud

Hi Masoud,
Just make sure you make the grid in XY plane and they should be right handed pointing in the +Z direction. Obviously you can't join structured and unstructured grids. In Pointwise just select the domains in the tree and then export you grid.
For further details refer to this thread:
http://www.cfd-online.com/Forums/poi...t-problem.html

Thanks so much for the reply. You're definitely right. It follows the Right-Hand-Rule of "I-J-K" vectors. You should select all the structured domains that you want to check, then go to EDIT> ORIENT. Here you select each domain separately and observe the Red (I) & Yellow (J) arrows, and use the Right-Hand-Rule. If you don't get the " +K " vector, then reverse the direction of "I" or "J" (there's no difference).
Another point is that for exporting to FLUENT, in addition to set the "boundary conditions" you have to go to: CAE>SET VOLUME CONDITIONS> NEW & select all the domains (both structured and unstructured in 2D) and call it for instance "DOMAIN-1" and select the type as FLUID. You should do it only if you have one type of fluid, if not, create different volume conditions for each domain.

You can join the structured and unstructured block. What you need is defining an interface between them. Consequently using grid interface in fluent as well.

Mesh Interfaces option disabled in ANSYS Fluent
 

I did the same of importing separate case files of meshes into ANSYS Fluent, but after importing both meshes into Fluent, the 'Mesh Interfaces' option is disabled. What can be the cause of this case? Is it with appending the two case files of meshes? I am modeling a 2D VAWT to be solved using sliding mesh technique. The rotor and farfield are to be imported intro Fluent from Pointwise separately.

Thank you.

You can export them as a single Fluent .cas file. In Pointwise, go to the CAE, Set Boundary Conditions... menu. Click on "New" and assign a name to the new boundary condition. Under CAE Type, select "Interface." Check on "Select Connections" then select all the interfaces and check on "Set" in the row of the interface BC.

Now when you export the Fluent file they will show up as interfaces, and you can apply the appropriate boundary conditions.

Importing case files from Pointwise to Fluent
 

Thank you for this! I have yet to to do your suggested procedure as I resorted to a workaround I figured out later. It is by exporting the rotating and stationary domains separately as two (2) case files and appending these case files in Fluent. I created the interface in Fluent thereafter.

Thank you for the urgent and in-depth response to my query and to this thread.