CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Needing an approach for using ICEM mesh in FSI (

anno_x December 29, 2010 15:50

Needing an approach for using ICEM mesh in FSI
Dear Friends,
I am working on 2d FSI problem with ansys workbench. I performed the meshing in ICEM. I know how to import 2d mesh from ICEM to CFX, but in FSI modeling (Oscillating plate in cfx tutorial as reference of modeling) I can't import the mesh. I don't know if it is possible to use ICEM mesh in ansys workbench FSI problem.


PSYMN December 30, 2010 12:05

Workbench Simulation requires the geometry for applying bocos... So you can't just import the ICEM CFD mesh.

However, if you go in thru ANSYS Meshing, you can use ICEM CFD interactive to generate a mesh in ICEM CFD and suck it back into ANSYS Meshing where it is automatically associated with the geometry...

Depending on your needs, you may even be able to get what you want directly from ANSYS Meshing.

ICEM CFD interactive finally got useful at R13, so hopefully you are up to date. Otherwise send an image of your mesh and maybe I can help you get similar in ANSYS Meshing (Workbench)...

backside March 5, 2013 13:13


I'm having the same probelm. I want to create a mesh in ICEm, that afterwards I can use in ANSYS to do a 2-way FSI analysis (workbench).

For that I started with the geometry, which is just made of curves and points. The geometry is a 2D hydrofoil in a control volume. I proceeded with the blocking and defined the mesh params. If I pre-mesh it, everything looks fine. Then I created by premesh>>convert to unstructured mesh the .uns file.
As a last step selected the solver (ANSYS CFX) and wanted to write the file. But then a get this:

Running ICEMCFD - CFX5 Interface Vers. 14.0.0

Error : no volume elements found.child process exited abnormally

It's clear that I shouldn't have volumes as I try to model a 2D Case. Where I have to fix my problem?

Best Regards,

Far March 5, 2013 14:11

did you choose the 2d option? is your mesh in x-y plane?

backside March 5, 2013 14:22

where can I choose this? If it's for the blocking, yes 2D blocking was selected, but my mesh is in X-Z plan. Maybe there is the problem

backside March 5, 2013 15:03

1 Attachment(s)
I rotated the geometry and the blocking in the XY-plane. But I got the same error message.
Attached you can find the geoemtry and teh blocking. The mesh is very poor at the moment, I just want to try to import like this before I waste time to create a better mesh..

By the way thanks for your help :)

Far March 5, 2013 15:11

1 Attachment(s)
Find attached files. Try them...

backside March 5, 2013 15:43

In fact you deletet my solid blocks (the 2 blocks in the blade moved to VORFN) and changed the flow solver from ANSYS CFX to ANSYS Fluent, where now one can choose 2D are 3D mesh. Is this correct? (At least it functions very well to import into Fluent)

But as I do a FSI (fluid-solid interaction) I can't erase the meshing of my hydrofoil. I need it to do a transiant structural analysis (ex. an initial displacmenet or pressure for 0.5secondes). So I have to keep both, fluid- and structure-mesh.

Far March 5, 2013 21:44

In that case you need to change the material to solid . Right click on parts and make new part. Choose the last option (material) and select the blocks inside the hydrofoil and name it solid. Generate unstructured mesh and go to output tab and select "2d" option and you are done.

And now import Fluent mesh (.msh) into cfx-pre and it will extrude mesh by one element. You have now 3d mesh !!!

backside March 19, 2013 21:29

1 Attachment(s)
I found a very good way to do the 2 way FSI.
In the transiant structural, at the model, one can choose as a insert mesh methode a multizone. In the advanced settings one can choose to create a ICEM CFD interactive mesh. (for more infos see: Video sample)

I have done that for the solid as for the fluid part. At the last stage of my settings, one has do define the boundary conditions for the fluid ( control volume) in the Fluid CFX. But there suddenly I have like defaults in my geometry. I checked my blocking as well as the mesh generation, they seem to be correct in ICEM. I even ensured that every face of the blocking is correctly projected on the surface.
Because of these defaults (see attached picture) I can't create the right boundary conditions. At the outlet for example this creates reflow, as the little box (red circle) is also attributed to the outlet...

Why I got these defaults? Could it be an error because of tolerances between ICEM and Workbench?

backside April 10, 2013 22:10

I could manage my problem with the mesh creation.

Initialy you start from the basic 2-way setup with a part for the solid (Transiant structural) coupled with the fluid (CFX). You can create or import a geomtry in Design Modeller after making/choosing the material. Then it comes to the meshing (Model for structur, Mesh for Fluid). The approach is for both the same, so I will explain the procedur for the solid part.

1.Double Click Model, so that Mechincal is opening.
2.Geometry-Hide the body you dont use. Check if right material is associated.
3.Mesh - Insert Method - MutliZone. There select advanced options. Now you can choose Write ICEM CDF Files: Interactive , ICEM CFD Behavior: Postprocessing.
4,Update Mesh. Now ICEM should open. Sometimes it is usefull to create a script (Link in further post). Be carrefull: When you create your own blocking it must have the same name as before to be regognized by Workbench (Usually it is called CREATED_MATERIAL).
5. When the premesh is done->export mesh as unstructured block.

Note: I changed the triangulation tolerance (ICEM-Settings-Model-Triangulation-Tolerance) to get rid of my mesh default of the further post

That's it.

Hope this will help you

mvoss April 12, 2013 03:57

If you´re using ANSYS 14.5 you can use an extra ICEM-Meshing container within the project schematic. It makes the whole scripting/blocking/updating process way more flexible and accessible.


Far April 13, 2013 09:36


an extra ICEM-Meshing container within the project schematic
where it is located ?

mvoss April 16, 2013 03:31

sorry for the delay.
The icem-container is.... at least in my installation, right below the Geometry component system.
I think it strongly depends on the licences you´ve got.

All times are GMT -4. The time now is 14:40.