[victoryv]

I am doing a external flow simulation on a wall. In my meshing , I have a huge aspect ratios (order of 10^5). I have prism layers along the boundary (first layer thickness around 10^-7). The unstructured mesh outside the boundary layer has parameters- patch conforming,proximity and curvature, min size 10^-4, max face size 0.250m and tet size 0.17m . I am using kw sst model, implicit solver, upwind schemes, green gauss node method. The solution is diverging.

I have tried following methods. But they were of no use.

1. Reducing CFL number. Reduced it upto 0.05.

2. Starting with First order scheme and then switching to 2nd order. The residuals get reduced to 10^-1 after 30 iterations. But when I switch to Second order upwind scheme, they start diverging again.

3.Reducing relaxation factors. Reduced them to 0.3.

4. Refining. I have refined the grid from 0.05 M nodes to 0.2 M nodes.

What else can be done to stop divergence?

Also,

1. Is it a good mesh?

2.I wanted to know if meshes with such high aspect ratios will result in divergence ?

3. Is volume mesh adaption a good option for such meshes?

I would really appreciate if someone would respond.

[victoryv]

I have a stopped the simulation when it is diverging and saw the contours. The edge shown here( between inlet and bottom wall) has abnormal values.
Is this the reason for divergence?
What could be the problem the mesh or geometry?
I would really appreciate anyone's suggestion.

[victoryv]

I have remeshed it and also redrew the geometry.Also, changed the turbulence parameters at the inlet. The residuals are high but constant for sometime and then start to diverge.Also, I am getting these statements after every iteration.

reversed flow in 392 faces on pressure-inlet 5.

absolute pressure limited to 1.000000e+00 in 9 cells on zone 10009

How can you have reversed flow at the inlet? Any suggestions are welcome.

[PSYMN]

Originally Posted by victoryv

reversed flow in 392 faces on pressure-inlet 5.

absolute pressure limited to 1.000000e+00 in 9 cells on zone 10009

How can you have reversed flow at the inlet? Any suggestions are welcome.

If the inlet or outlet is too close to the area of interest, things can start to reverse. It is common to extend the model by 6 to 10 diameters to ensure that the inlet or outlet is far enough away. Often this is done by extruding the mesh on the inlet and outlet to make a pipe...

You can probably find posts about this elsewhere on CFD-Online...

[victoryv]

The inlet and outlet are far apart. My geometry is a windtunnel. Also, can you please see earlier divergence issues I pointed out.

[Far]

Is it a good mesh?

Without looking at mesh, I am not able to comment.

I wanted to know if meshes with such high aspect ratios will result in divergence ?

Normally not. Turn on double precision

Is volume mesh adaption a good option for such meshes?

Yes. But I prefer to get the good mesh from preprocessor.

[victoryv]

I have turned on double precision.
My mesh quality

Applying quality criteria for tetrahedra/mixed cells.
Maximum cell squish = 9.99997e-01
Warning: maximum cell squish exceeds 0.99.
Maximum cell skewness = 7.60320e-01
Maximum aspect ratio = 2.75799e+06

Its empty wind tunnel. The mesh looks like this. It has boundary layers along the wall at the bottom.

[PSYMN]

The converging duct starts right up near the inlet... It doesn't matter how far apart the inlet and outlet are, it matters how far the inlet and outlet are from things getting interesting...

I think your inlet is too close to your converging section...

[PSYMN]

Also, from your mesh image, I can see that the volume jump between your top prism and the adjacent tetra is huge... The solver probably doesn't like that at all...

You either need more layers so it has time to transition to the larger size...

Or you need a smaller tetra size,

or you need a larger initial size.


Regardless of your Y+ calc, just try out a larger (5 or 10x) initial height and see what happens in the solver.

[victoryv]

Originally Posted by PSYMN

Also, from your mesh image, I can see that the volume jump between your top prism and the adjacent tetra is huge... The solver probably doesn't like that at all...

You either need more layers so it has time to transition to the larger size...

Or you need a smaller tetra size,

or you need a larger initial size.


Regardless of your Y+ calc, just try out a larger (5 or 10x) initial height and see what happens in the solver.

You are right. I tried with BL 100x initial size . It did not diverge. The residuals got reduced to 10^-3 and were fluctuating there but by monitoring other parameters i could say it reached steady state. But I need y+ ~1 . So I will try increasing the no of layers, keeping earlier size.

[Far]

If you need Y+ = 1 , try hexa

[victoryv]

Originally Posted by Far

If you need Y+ = 1 , try hexa

But we do not have inflation layers in hexa right?
Also, do you think we can have proper mesh if we have complex body in the tunnel later on?
I thought unstructured mesh is best for complex geometry. So, is hexa good enough for curved bodies?

[Far]

Hexa is good for every problem. In Hexa you can get inflation (aka boundary layer) through edge mesh parameters or more conviently through Ogrid. Thats very simple.

[RodriguezFatz]

I am confused. How do pictures from post #2 and #5 fit together? Could you please post a picture of your complete domain, with all surfaces described and also what kind of inlets and outlets you have?

One additional thing: Did you check in Fluent, if "General->Scale..." shows the correct size values?

[PSYMN]

Originally Posted by Far

Hexa is good for every problem. In Hexa you can get inflation (aka boundary layer) through edge mesh parameters or more conviently through Ogrid. Thats very simple.

In the hands of an expert user, ICEM CFD Hexa is great. It is certainly the best way to efficiently capture a boundary layer... It would probably work very well for this model, depending on what you wanted to put into that test section...

But I just wanted to temper Far's comment... on some models (or for some users), hexa is not worth the hassle ;^), which is when tetra/prism or polyhedral meshing kicks in.

[victoryv]

Originally Posted by RodriguezFatz

I am confused. How do pictures from post #2 and #5 fit together? Could you please post a picture of your complete domain, with all surfaces described and also what kind of inlets and outlets you have?

One additional thing: Did you check in Fluent, if "General->Scale..." shows the correct size values?

They are the same. In #2 only bottom and inlet are shown where I found abnormal values. The flow is in +x direction. BC are bottom wall, pressure inlet , pressure outlet, other faces are taken as symmetry. It is actually half section of a wind tunnel.I have also checked the scaling. They are right.

[victoryv]

Originally Posted by PSYMN

In the hands of an expert user, ICEM CFD Hexa is great. It is certainly the best way to efficiently capture a boundary layer... It would probably work very well for this model, depending on what you wanted to put into that test section...

But I just wanted to temper Far's comment... on some models (or for some users), hexa is not worth the hassle ;^), which is when tetra/prism or polyhedral meshing kicks in.

Originally Posted by Far

Hexa is good for every problem. In Hexa you can get inflation (aka boundary layer) through edge mesh parameters or more conviently through Ogrid. Thats very simple.

I have been using unstructured grids in 3D since I started using Fluent. I have never used ICEM CFD. Though I have heard its really good for meshing. But I read somewhere that its features have already been added in Ansys Meshing application in workbench. That is the reason I haven't learned it . I will probably give a shot at ICEM CFD and hexa once I finish this work.

[PSYMN]

A lot of the ICEM CFD technology has been exposed... Even ICEM CFD hexa is in ANSYS Meshing as "MultiZone".

But MultiZone is really an automated, almost patch conforming bottom up version of ICEM CFD hexa... Very different from the top down, powerful, flexible tool that ICEM CFD users love, but a great tool in its own right.

[RodriguezFatz]

Originally Posted by victoryv

They are the same. In #2 only bottom and inlet are shown where I found abnormal values. The flow is in +x direction. BC are bottom wall, pressure inlet , pressure outlet, other faces are taken as symmetry. It is actually half section of a wind tunnel.I have also checked the scaling. They are right.

1) So the left of the yellow part is the inlet and the right yellow part with the little teal area shows the bottom?
2) It looks like you use energy equation. What are your boundary conditions?
3) Does your simulation converge without the temperature stuff?
4) So top is also symmetry? How can this curve be symmetric?
5) How can this be "half of" something, when you have 3 of 6 faces with a symmetry boundary condition?

Again: Please post an clearly arranged picture of your domain and mark all faces with their meaning.

[victoryv]

Originally Posted by RodriguezFatz

1) So the left of the yellow part is the inlet and the right yellow part with the little teal area shows the bottom?
2) It looks like you use energy equation. What are your boundary conditions?
3) Does your simulation converge without the temperature stuff?
4) So top is also symmetry? How can this curve be symmetric?
5) How can this be "half of" something, when you have 3 of 6 faces with a symmetry boundary condition?

Again: Please post an clearly arranged picture of your domain and mark all faces with their meaning.

Please see the pic. I have added the names.

1.Yes, you are right.
2.Yes, I am using energy equation. It started to diverge again. I am using compressible flow.
3. The left is symmetry - half section plane. The other two boundaries are symmetry due to slip condition.
4.Bottom wall is no-slip wall and other boundaries are pressure inlet and pressure outlet.