[Mfaizan]

Hi Glenn,

I totally agree with you but there is something happening beyond my control and I can not change it as it is locked. I share with you as how I developed the mesh.

1. First I developed the nozzle,hpgas and air geom on designmodeler all together.
2. Then I hide 2 items and save as separate nozzle file. separate hpgas and air file.
3. Then I call three different files one by one on icem using ansys workbench and assembled them.
4. Then I created the mesh of all three domains in assembled form using blocking method. I used O-grid as well.
5. Then I separated the mesh files separately as nozzle, hpgas and air.
6. Then I exported each file into ansys cfx format separately as nozzle, hpgas and air.
7. Then I called these three files into ansys workbench one by one and throw them into cfx-setup on workbench.
8. I got three different domains in cfx-pre.
9. Then I connect the overlapping face of three domains using interface option called GGI.
10. then I started the solver and got this mesh statistics.

Now the mesh quality (Ortho, exp factor and aspect ratio) I generated in ICEM is different from what I got in CFX- Solver. Since solver running, I can not change the mesh at all. It's an automatic connection of nodes and mesh among three domains in CFX Solver which is beyond my control.

I hope I explained the things and you can understand now as why I think the mesh first generated is OK for supersonic flow at high conditions.

Now please suggest what should U do smartly to overcome convergence. Moreover is there any option available called dynamic or adaptive mesh in CFX-Pre/Solver which can fix mesh dynamically.

Please suggest. thanks for your guidance.

kind regards,

Faizan

[ghorrocks]

The FAQ I posted previously describes what you can do in this situation: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Let me explain what I mean by mesh quality more completely. Your list describes the basic steps of setting up your simulation. I am referring to exactly how you do the meshing step only. The quality of the mesh you define here is critical.

Please post an image of your mesh. Pay particular attention to the mesh around the shock waves. If we see your mesh I suspect we will be able to be more specific.

[Mfaizan]

Hi Glenn,

Please suggest which mesh file would you wish to review. ICEM Mesh Images or the CFX-Solver (Finally running) mesh images. I explained you the situation earlier that cfx-solver is changing it automatically. So which one would be important for you to review? I will post images of mesh you are suggesting.

Kind regards,

Faizan

[ghorrocks]

Images of the mesh is all I want to see. Some cross sections would be good, also some of the external mesh. The area around the shock wave is the critical area so in the area of the shock please.

[Mfaizan]

Hi Glenn,

I am sending the mesh pics of currently running CFD case.

Please have a look and suggest. If you need more images, please suggest.

Look forward to hear from you,

Regards,

Faizan

[Mfaizan]

one more pic

[Mfaizan]

x section mesh images

[Mfaizan]

one more x sec pic

[ghorrocks]

I am not surprised you have a problem with convergence with that mesh. It has massive jumps in mesh size in several locations. Below is some marked up comments.

image.jpg

Image2.jpg

[ghorrocks]

Another point:

Can you model this as 2D axisymmetric? That will make it run much faster.

Are you modelling the solid which forms the nozzle as well? If so, why? Do you want to know the temperature profile of the nozzle?

[Mfaizan]

Hi Glenn,

Thanks a lot for identifying the mesh related issues.

I developed big mesh prior to this. I am posting the cross section of big mesh at throat area. Please suggest if it is OK.

I am performing a 3D analysis so 2D axis symmetric study is out of question.

Yes I need to study the temperature variation within the nozzle wall during the flow. As I mentioned it is a 3D study.

I did refinement at nozzle exit because at this thin plane high velocity nitrogen is mixing with atmospheric air. It's a 3D multicomponent model study. As I told you I import three mesh files in CFX-Pre. And this condition at interface is beyond my control. It's auto.

If I send you the ICEM nodes seeding of my three different domains nozzle,hpgas and air. Would you suggest me the best distribution of nodes. I used bigeometric for nodes distribution. Can you suggest any better rule to develop mesh which can support supersonic flow convergence.

Look forward to hear from you,

Regards,

Faizan

[ghorrocks]

Don't do mesh refinement when you are still getting the basic model working. Start with a coarse mesh with even element sizes. Once that is working then you start refining the mesh.

[Mfaizan]

No this big mesh was also a failure. Not working and always giving error code 1.

[ghorrocks]

You need your mesh fine enough to capture the basic physics of what is going on. If it is too coarse then it will fail with strange errors. So you need to be finer than that. But the mesh you showed was too fine with far too much mesh grading.

[Mfaizan]

Hi Glenn,

Thanks. Can you guide me on ICEM. Should I send you the pic of hpgas mesh first showing no. of nodes for grids.

Pl. suggest. I would truly appreciate your support at this crunch point.

Regards,

Faizan

[ghorrocks]

Try the Geometry and Meshing forum for advice on ICEM.

But to start you off I would remove the mesh grading you currently have, or at least reduce it. Your aim is to make sure the size of any 2 adjacent elements is the same with 20%, or 10% if you can.

[Mfaizan]

Hi Glenn,

As you suggested in your last response. I am trying to read between the lines as stated "size of any 2 adjacent elements is the same with 20%, or 10% " means the the ratio should be 1.2 or 0.2. As I stated earlier that i used bigeometric option and node distribution growth was 1.2.

Please suggest if I am thinking on right path or wrong path under your instructions.

thnaks

regards

Faizan

[quangthanh94]

cacn you help me with this wrong? thank you

[Mfaizan]

The solution component is unable to find the file from CFX-Pre cell. Right click on solution cell and click on the option suggesting read file from CFX-Pre cell. The solution would be updated. Thanks.

[Mfaizan]

Hi Glenn,

I would like to use this platform to thank you that my 3D supersonic model is running successfully on coarse mesh. I also performed grid independency test by further reducing nodes to 50% with the existing one. I observed the velocity at nozzle exit and the difference in velocity is 0.13%. It means the coarser mesh has no significant effect on the outcome or variables of 3D model.

Thanks for your timely support. I appreciate. I also thank other people who contributed to resolve the matter.

Cheers,

Faizan