Dear CFD user

I produced a 15degree pie to model flow inside a 170mm diameter pie. I did this meshing with ICEM. I have a problem with the BC (boundary condition) when I define my CFX case.

To avoid simulating the whole 360 degree of the pipe I modeled only a small 15 degrees angle pie. I defined each of the vertical plane of my cylinder as symmetry plane when I defined the BC. Unfortunalty when I try to run this case the CFX solver give me an error that my two plane are not parellel and the solver cannot solve the problem...

Is there something I defined wrong in the BC? Should I change something to my ICEM mesh?

Thanks in advance for your help

Hi Jonathan,

Check your mesh on these faces. ICEM CFD is notorious for producing errors like this because it assigns faces to regions (parts) by finding the surface it projects closest to. You will probably find that at the edges you have a few faces which are non-planar.

If it is a simple model, consider meshing it in the ANSYS Meshing app instead. You can define a sweep method on the body and assign the two sides as the start and end of the sweep. Also, if it is perfectly axisymmetric you can reduce you wedge to ~3 degrees and specify only one element in the sweep direction.

Regards, Robin

Hi Robin,

Thanks a lot for your help. I chose ICEM CFD because I wanted to mesh with hexa element (I mean full cubic types, with 6 faces volumes). So is there a way to mesh with CFX MESH (workbench) and get this kind of element? I know that CFX mesh is much more convenient for easy application.

By the way I am simulating the mixing cold flow of a bluff body burner.

Regards, Jonathan

You cannot generate a pure hex mesh with the CFX-Mesh method, but you can with the sweep method. However, the topology is much more limited than with Hexa. That said, I wouldn't worry too much about getting a pure hex mesh. A revolved mesh with inflation will be very accurate too (it will result in hexes where you have inflation and prisms through the rest). The main thing is to make sure you have sufficient mesh where you need it.

I hadn't realized you were using Hexa. In that case I would stick with ICEM CFD. The problem in that case is most likely that you have not properly projected your edges to all of the curves around the plane, projected your vertices to the points at the corners and/or projected the faces to surfaces. Small misalignments in these projections will lead to a non-planar face.

Regards, Robin

Hello,

I am bit skeptical here. Did you apply "symmetry" BC or "rotational periodicity"... I hope the later one best suits your problem...

Regards Anantha

Hi Anantha

I simply applied a Symmetry boundary condition as it is shown in the CFX tutorial of Reacting flows in a mixing tube. Would you inform me about this "rotational periodicity" BC? Never heard about that in CFX.

Regards. Jonathan

Hi Robin

I would ask your help for something is ICEM. Thanks to your advice I associated the faces of my blocks to the different surfaces. I either associate point with vertex. Do you know if it possible to associate more then one vertex to a point?

Another useful information I would need. How do I manage my surfaces in ICEM so they could be recognize by CFX when it is coming the time to define the region of my BC?

I am getting confuse with two other things. Sometimes when I choose my region for BC in CFX, their is two available regions similar to each other. One has the mesh of the face only and the other region has the mesh plus the contour. What is the difference for those regions?

I am a beginner in ICEM so thanks a lot for your precious help.

Hi Jonathan,

I'll do my best to answer your questions, but I suggest you go through some of the tutorials as well.

I would ask your help for something is ICEM. Thanks to your advice I associated the faces of my blocks to the different surfaces. I either associate point with vertex. Do you know if it possible to associate more then one vertex to a point? Yes. You can assign multiple vertices to a point, but be careful that you don't collapse a block by doing so.

Another useful information I would need. How do I manage my surfaces in ICEM so they could be recognize by CFX when it is coming the time to define the region of my BC? Before you generate your mesh, group surfaces into "Parts" by right clicking on the Part object and creating new parts. These parts will then appear in Pre as separate regions.

I am getting confuse with two other things. Sometimes when I choose my region for BC in CFX, their is two available regions similar to each other. One has the mesh of the face only and the other region has the mesh plus the contour. What is the difference for those regions? I'm not sure what the answer is. I haven't seen such a problem so this may be a result of what you have done specifically in ICEM. What do you see in terms of regions under your mesh object in Pre?

Regards, Robin

Hi Robin

Thanks for the tips. I did several tutorial on ICEM but it seems I missed something. Anyway your help is really appreciated

About producing part in ICEM a already did that including surfaces in my parts. The thing is when I open CFX-PRE, all those part defined previously in ICEM are not there, some ones are missing. So should I change something when exporting? I thought ICEM was either exporting all the primitive 2D surfaces to CFX-Pre. Unfortunatly it is not my case. I currently use as solver ANSYS CFX an it produce a .cfx5 mesh file.

About those region in CFX that you have not understand, I will work on that to resolve that issue.

Hehehe Ok Thank you professor Regards

Hi Robin

Thanks you so much for your help. It has been great help!! My meshing is now running in CFX..

Hi Jonathan,

I think I know why you don't have all your faces in PRE. In ICEM, start with creating/importing your 2D geometry. Then, as Robin suggested, name every part you want to use in PRE (inlet line, outlet line, symmetry plane, etc..). Next, create your 2D Planar blocks.

The following step was probably missing and is very important. **Assign every block's face, edges and vertex to their corresponding geometry**. This will allow the mesh elements to take the name of the corresponding part. If you then convert the Pre-Mesh to an Unstructured mesh, you should see Line elements in the Inlet part, for example.

Finally, when you extrude the mesh, leave the "new side name" as "inherited", name the "new top name" symmetry2 and give a cool name to the volume part.

Save your mesh, export it and everything should be fine in PRE !

Regards, Felix