[flotus1]

Is this a picture of the actual mesh you are using?
If yes, add at least prism layers at the walls.

What mach number do you expect in your simulation? How high is the pressure at the inlet and outlet respectively?

Edit: Am I right assuming that the prism layers you added are so thin compared to the tet elements that they cannot be seen in the picture of your last post?

[victoryv]

Originally Posted by flotus1

Is this a picture of the actual mesh you are using?
If yes, add at least prism layers at the walls.

What mach number do you expect in your simulation? How high is the pressure at the inlet and outlet respectively?

I have added prism layers at the bottom wall.The Mach no is around 0.3. The pressure at the inlet is 103000 Pa and the outlet is what I have to find by comparing the exp results.

[flotus1]

Since you are experiencing convergence issues, I would try a simulation with a velocity or mass flow inlet, at least to get better initial values for the following simulations.

Getting back to the prism layers, are you sure that the volume jump is better this time?

Additionally, I strongly recommend to use a hexa mesh, especially since the whole geometry basically consists of one hexaeder. A good mesh is one thing less to worry about in CFD
This could even be done with the Ansys mesher.

[victoryv]

Originally Posted by flotus1

Since you are experiencing convergence issues, I would try a simulation with a velocity or mass flow inlet, at least to get better initial values for the following simulations.

Getting back to the prism layers, are you sure that the volume jump is better this time?

Additionally, I strongly recommend to use a hexa mesh, especially since the whole geometry basically consists of one hexaeder. A good mesh is one thing less to worry about in CFD
This could even be done with the Ansys mesher.

I know the stagnation pressure and stagnation temp at inlet. Thats why I am using preesure inlet. yes, the volume jump is far better now. Yeah, i will try improving the mesh . If that does not succeed , I will try multizone mesh.

[Far]

instead of symmetry , specify them as slip wall.

Extend domain by some unit lengths at inlet and outlet

[victoryv]

Originally Posted by Far

instead of symmetry , specify them as slip wall.

Extend domain by some unit lengths at inlet and outlet

Is there other option than symmetry for modeling slip walls?. Also, but if we extend the domain at the inlet and outlet, it changes the parameters (velocity, pressure) inside the domain right?

[Far]

Specify extended walls as slip so you will not have any boundary layer development or pressure loss.

You can define as slip wall by specifying shear stress = 0. It will have same effect as symmetry. Moreover symmetry condition has some special purpose and it has different mathematical definition.

[victoryv]

Originally Posted by Far

Specify extended walls as slip so you will not have any boundary layer development or pressure loss.

You can define as slip wall by specifying shear stress = 0. It will have same effect as symmetry. Moreover symmetry condition has some special purpose and it has different mathematical definition.

Oh, i totally forgot that we can specify shear stress in "wall" boundary condition. Thanks man . Also, i will try extending the the inlet and outlet.

[flotus1]

Originally Posted by Far

You can define as slip wall by specifying shear stress = 0. It will have same effect as symmetry. Moreover symmetry condition has some special purpose and it has different mathematical definition.

This is the first time I heard of this. Are you sure? Where exactly is the difference?

[Far]

I always face convergence problems with symmetry, which is not the case with slip wall.

Originally Posted by ghorrocks

This is described in the documentation.

Symmetry enforces zero normal gradient to all parameters, and a slip wall does not necessarily do this. But for most normal simulations they are equivalent.

And a symmetry plane is required to be planar, but a slip wall can be any shape.

Originally Posted by Martin Hegedus

In general, slip and symmetry are much the same, if not exactly the same. But, sometimes it is implementation dependent. For example one could have p(-1)=p(1) for symmetry but p(0)=p(1) for wall. Also, the turbulence model boundary conditions could be different. OK, I don't know what it means to have a slip turbulence model, but I guess that depends on what someone is trying to do. Also, a turbulence model could depend on the distance from a surface. So it's possible that setting a far field condition to a wall will affect the turbulence model.

But, the answer, to first order, is that they are the same.

http://www.cfd-online.com/Forums/mai...condition.html

[Far]

https://dl.dropbox.com/u/68746918/CFDNotes06.ppt

Refer to slide 54 and 57. Why two lateral boundaries are set as symmetry and top and bottom as slip-wall? What will be effect if two side (lateral ) boundaries are set to slip-wall or periodic? What will happen if top and bottom walls are defined as symmetry or periodic?

Edit : Some notes from CFX

[RodriguezFatz]

Hi, you should switch off energy equation and try to run the simulation. If that diverges too, please switch the inlet to velocity inlet and try if it works. Pressure inlet and outlet are not the easiest choice.

[hossam_ali]

hi i think the problem in ur mesh skewness

u should remesh and decrease the skeness to be less than now and this will decrease the squinsh of the mesh (to be less than 0.9)

[RodriguezFatz]

Originally Posted by hossam_ali

hi i think the problem in ur mesh skewness

u should remesh and decrease the skeness to be less than now and this will decrease the squinsh of the mesh (to be less than 0.9)

Maybe (or belike) the mesh is the problem, but normally meshing is also the most time consuming part of the whole process, so rather than remeshing I would try to spot the problem before starting...

[victoryv]

I have tried extending boundaries and slip walls. No use. Still it is diverging.
I will try incompressible flow and velocity inlet and simulate once again.

[RodriguezFatz]

Originally Posted by victoryv

I have tried extending boundaries and slip walls. No use. Still it is diverging.
I will try incompressible flow and velocity inlet and simulate once again.

You also had compressible flow? That's too much, you should really try to get simple settings running before switching on all additional equations...
Also, if you explain your case in a thread, please tell people everything about it and don't wait until post #50 to do so...

[victoryv]

Originally Posted by RodriguezFatz

You also had compressible flow? That's too much, you should really try to get simple settings running before switching on all additional equations...
Also, if you explain your case in a thread, please tell people everything about it and don't wait until post #50 to do so...

I have written in the heading above the first post itself that I am doing steady state compressible. I am doing compressible because i have compressible results to compare with. Sorry for the confusion.

[RodriguezFatz]

My bad! I didn't know that posts have captions. Anyway, switch off all these additional equations when something does not work and try to run it.

[victoryv]

I am facing a new problem now. I got rid of all the previous problems. The solution was taking a lot of time and many iterations to reach steady state. So I have used FMG initialization and pseudo transient method( time step 0.001) to make the convergence faster. When I was trying to find mesh independent solution, after 3rd refinement, the solution (pressure and velocity) started oscillating where it was supposed to reach state.

How did the mesh refinement led to oscillations?
If mesh is not the problem, what could be the problem?

[Far]

Originally Posted by victoryv

I am facing a new problem now. I got rid of all the previous problems. The solution was taking a lot of time and many iterations to reach steady state. So I have used FMG initialization and pseudo transient method( time step 0.001) to make the convergence faster. When I was trying to find mesh independent solution, after 3rd refinement, the solution (pressure and velocity) started oscillating where it was supposed to reach state.

How did the mesh refinement led to oscillations?
If mesh is not the problem, what could be the problem?

Because refined mesh is capturing some unsteady flow phenomena which was not being captured in coarse mesh.