Mesh generation in impinging jets
 

I have been working on a jet impingement problem for a while now. I was trying to do a 2-d simulation on CFX using geometry and mesh from ICEM. But I am encountering problems with mesh generation. I am attaching pics in this post, so you can see my problem. Since cfx does not support 2d simulation, i have extruded my geometry by 1 unit in the z direction. So basically, you can see the various parts in the geometry. Inlet is a small c/s diameter part, whereas the rest are as mentioned. The jet enters through the inlet and impinges on the wall (green). But when I pre-mesh the set up, my mesh is very bad quality. Please advise.

Hi
 

Instead of extruding the geometry, do the 2-D mesh(surface mesh) and extrude the mesh by 1 unit. I guess the mesh is getting distorted bcoz of some association problem and I also think that there is some problem with your inlet definition of the geometry. Why are you adding a small surface near the inlet, in "-ve y" direction?

Hi,

Thanks for the reply. I was wondering if I extrude the mesh from 2-d then how do I create parts to give the boundary condition later? Should I create parts with just the lines? As there will be no surfaces...please explain.

Yes create parts with lines, and while extruding the mesh see that you have checked on the lines in Mesh control tree.

Hi

I tried to do the 2d-surface mapping, but its not working properly. It says it needs to build topology with default tolerance, i clicked yes and then it makes block, but i am not able to define pre mesh params.

Also, in the 2d surface blocking, there are 3 methods, please advise on the best.

Hi
 

1. First create the 2D geometry with points and lines and then create the 2D surface.
2. Next create the parts with lines.
3. Next under blocking use 2D planar.
4. Create the mesh using blocks and then convert it to unstructured mesh.
5. Then in the display control tree you will find Mesh tree, under it check the lines.
6. Go to Edit mesh menu and extrude the 2D-mesh by giving your required "Z" spacing.
7. Finally output the mesh.

If you face any problems, post the problem.:)

Hi,

I followed all the steps correctly. Except since I am using structured mesh, I generated the mesh using the pre-mesh params. The mesh was created perfectly and I even got the output file. I gave the boundary conditions as per a paper (the pic is attached). But when I tried to run in CFX, I got the following error:

ERROR #002100048 has occurred in subroutine SU_BNEXT.
Message: All vertices for a fluid domain lie on boundaries. This is considered to be a fatal error because control volume gradients cannot be calculated, leading to serious discretization error. A common cause for this error is a mesh which is only one element thick, without symmetry or 1:1 periodicity on the lateral boundaries. If you have this situation, and the domain is two-dimensional, please change the lateral boundary conditions to symmetry or 1:1 periodicity. Alternatively, for three-dimensional simulations, please ensure that your mesh has at least two elements across. Execution is terminating. This error message can be bypassed by setting the expert parameter 'boundary vertex check = f', but be aware that doing so may lead to significant solution error

Please advise. I am attaching all the pictures such as boundary conditions followed and mesh generated etc. The hand drawn diagram is my geometry and I have given BCs as follows:

Entrainment - Opening BC. with static pres. entrain, zero gradient turbulence
Inlet - Vertical downward velocity, low intensity turbulence
Outlet - static pressure, relative pres= 0
Symmetry - usual symmetry
wall - no slip and smooth

I hope this information suffices.

Hi shashank
 

I see from the attached pictures that you got the mesh correctly:). Well the error message your getting from the solver is bcoz you have to give a boundary condition for the extruded faces. I guess your using CFX solver, in cfx if you dont mention the boundary condition, by default they will be wall's.

So in your case the extruded face and the original face should be given symmetry boundary condition.

I believe this correction should make your simulation going.

Hi,

Sorry for late reply, I did not have net. But you were right, I made the correction and the simulation worked properly. Thanks for the advice. I will write to you soon when I run 3-d simulations. I am sure your help will be valuable. :)

Hi,

I wanted to know how to calculate heat flux for my wall part using Ansys cfx. I am not able understand how to calculate it. Please help. :confused: