Diverging simulation
 

Hi, my simulation is diverging. I've tried increasing nNonOrthogonalCorrectors up to 10, and also introducing residualControl in fvSolution, but nothing helps. My checkMesh log is as follows.

The boundary conditions are similar to my other case, which runs perfectly. I have only changed the velocity at the inlet and with a slightly different geometry.

May I know if the "number of severely non-orthogonal faces" is the cause? Otherwise, how can I solve the diverging problem?

hi czhongrong

By looking at your checkMesh Log, it is seen that the Max Skewness for your mesh is 3.314. This could be the problem why your simulations are diverging. The skewness of the mesh is an indication of the optimum cell size. For accurate solution, the maximum skewness for Hex mesh should not go beyond 0.7 or 0.85. In general, the mesh with max skewness of 0 is considered to be perfect and it should not go beyond 1 in order to have accurate solution or convergence in solution.

So i recommend you to change your mesh and run the simulations once again.

All the best

Hi vishal3,

My geometry is a cylinder with a protruded top on its surface(see attached). I just can't seem to be able to decrease the max skewness. May I know what parameters I could try editing? Below is my blockMeshDict.

If you have an STL of your geometry use snappyHexMesh.

Hi akidess,

I can't get my STL to work, that's why I use blockMeshDict to mesh my geometry.

The problem is in non-orthogonality, in fact OpenFOAM's implementation of FVM will not work with non-orthogonality larger then 60-70 degrees

So I would need to reduce the "Mesh non-orthogonality Max" to be below 60-70? If so, how can I do that? Do I still need to care about the max skewness?

Yes

You must locate cells where non-orthogonality is high and change geometry of corresponding blocks in blockMeshDict. To locate this cells, run:
then
Yes, but in most cases, improvement of non-orthogonality leads to improvement of skewness

Hi mkraposhin,

Is there any rule of thumb or guideline that we can follow to avoid high non-orthogonality? As seen from my geometry in my previous reply #3, I find it difficult to change the geometry of the block. Attached is the schematic sketch diagram of my meshing and what "foamToVTK -faceSet nonOrthoFaces" has shown me in ParaView.

It can be seen that lines 5-23 and 4-22 are the causes of this problem.

Hey czhongrong

Why don't you try to create a mesh in other applications like GMSH / SALOME / GAMBIT / ANSYS WORKBENCH / HYPERMESH etc. ? I dont have any idea whether blockmeshdict is that much capable of handling this. Just give it a try. There you have a good control over your mesh when you are using other applications.

All the best!

I would propose another a bit more complex configuration of blocks - see attachment

Thanks for the layout, but just a few questions, I couldn't quite visualise properly:o:

1) I see 2 circles, do I have to model that outer circle? If yes, is the area in-between the 2 circles considered as hex blocks as well?

2) Are the 2 horizontal lines on the right needed?

3) "With this line non-orthogonality can be adjusted" - meaning the BLACK diagonal line on the right?

By the way, I've tried to mesh in a different layout. See attached for layout. But I keep getting the following error from blockMesh - "face 3 in patch 2 does not have neighbour cell face: 4(3 4 7 8)". I can't find the cause of the problem. My blockMesh is as follows.

Hi,
I think that with the descretization shown above, you will also get mesh with high non-orthogonality. I made another version of block geometry (see attachment).

Grey regions are blocks

In this geometry you can adjust non-orthogonality with the vertical position of point 6 and horizontal position of point 5.

Hi mkraposhin,

Yes, indeed my discretisation still yields 88 deg of non-orthogonality.

1) Are points 4, 6, 8, 9, 13, 14 all arbitrary points on the circle which I can choose on my own?

2) I will need to follow this discretization on the upper left half of the geometry too right (i.e. mirror on the left)?

Yes, this was expected result, because you must take care of planar angles between edges in each block - they all should be near 90 degrees

Yes, they are arbitrary, and with their position you can adjust non-orthogonality.
For the first iteration, you can assume that line 2-5 have length equal or slighly larger then line 3-2. Line 13-8 inclined to line 12-10 with angle ~ 30 degrees


Yes, you need to mirror upper right blocks on the upper left to get upper part of your geometry. Then, you must creat lower part of geometry. For this you can look at tutorial tutorials/stressAnalysis/solidDisplacementFoam/plateHole

For the lower part of my geometry, can I just model it like how I used to, in my earlier posts? By the diagonals 0-12 and 13-1?

Yes, you can, but if you will do lower part of mesh like in example tutorials/stressAnalysis/solidDisplacementFoam/plateHole
or like the top part, you will get better mesh quality, i think.

Also, please note, that in any case you will need to save blocks between outer and inner cylinders

See attachment

Save blocks?

I attached file with lower part of mesh

Thanks so much! I will give it a try and update again!

Hi mkraposhin,

HELP! I've created the mesh and encountered some error in blockMesh as follows. I'm not sure if my labelling sequence in hex blocks are correct. :confused: Attached is my schematic layout, and blockMeshDict.

In the schematic layout, blue ink corresponds to the hex block numbers in blockMeshDict for better reference.

Hi,

i think, you must start by adding blocks one by one to find which block causes error. Also, you must disable all patches at this step

Erm, how can I disable patches?

Just comment everything in boundaries section

I mean here:

Thanks a lot! I'll try it out soon...

blockMesh crashed while "creating topology patches" after I blocked out "boundary", and had the following error:

Hi, i checked your blockMeshDict and i can propose next changes

1) If you want to comment something between '(' and ')' brackets, use two slashes, for example:
2) The problems with blocks, with which you faced several days before are result of incorrect specification of directions of blocks. Each block in OpenFOAM uses next specification of directions:

• direction e1 - between point 1 and 2 of block
• direction e2 - between point 2 and 3 of block
• direction e3 - normal to the plane of e1 and e2 (e3 = e1^e2)

When you specified block 10 as
it means, that e1 direction specified from point 22 to point 43, e2 direction specified from point 43 to 52 and direction e3 is orthogonal to e1 and e2. It means, that all edges that belongs to e1 will be partitioned in 30 parts, all edges that are belongs to e2 direction will be partitioned in 20 parts and all edges that are belongs to e3 direction will be partitioned in 20 parts

But in block 11
You specified e1 to be from point 53 to 4 and direction e2 to be from point 4 to 52. Their partitions are 30 and 20, consequently. This means, that edge 43-52 will have 30 part in block 11 as it's a direction e1. But in block 10 edge 43-52 will have 20 parts, because you specified it to belong to direction e2.

So, you need to correct directions for all blocks with errors
For example - see attached file

I've done according to what you've instructed, but now I encountered another error.:confused: Apparently, blockMesh said I have undefined faces, which I couldn't figure out as I have listed all the faces. Subsequently, checkMesh stated "Number of edges not aligned with or perpendicular to non-empty directions: 1208760".

Attached is my schematic layout (i've re-numbered my points), and my blockMeshDict.

Because you introduced new block, that is not connected to others. You must split this block to connect to point 4, 59, 60, 61, 62, 1. See attached jpg for example, new points are marked with red color

Also, i see that your mesh have a very large aspect ration
OpenFOAM's checkMesh says that it's OK, but from my experience i can tell you that you must reduce it with at least 10 times, lets say to 58.0

How can I reduce the max aspect ratio? Would simpleGrading help? Because now I'm just testing the mesh with simpleGrading (1 1 1), to see if it works...

You must inrease number of discretization points in z direction for all blocks and number of discretization points for large blocks in x and y directions - blocks like 38-59-4-58.

Or, you can decrease number of discretization points in radial direction and azimuthal directions (blocks in the circle and blocks in the cross)

Thanks!! I've managed to solve the undefined patches! Now I'm trying to lower the max aspect ratio...

Thank you so much! It is of indeed great help for my project!

Hi,
did your simulation converged with the new mesh?

The core processors are idling though, I will update once I got it to run...

UPDATE: The simulation seems to be running well! Thanks a lot!

Hi mkraposhin,

I've encountered some problem with my simulation. It keeps getting this error. See attached for log(only an extract). It looks like it suddenly diverges. Is it a problem with my mesh?

checkMesh as follows(I can only reduce my max aspect ratio to 76.8):

Hi, i think that your mesh is good.

As i undestrand, you are using transient solver (pimpleFoam?)

Try next:

1) Set momentumPredictor in fvSolution->PIMPLE to false
2) Set nCorrectors to 2
3) Reduce time step at least 4 times (set maxCo to 0.5)

Yes, I'm using pimpleFoam.

1) I do not have a "momentumPredictor" entry in fvSolution. Attached is my fvSolution file.

2) nCorrectors was initially 2.

3) Currently my deltaT is 1E-4 in controlDict, so decrease by 4x right?

From the log i saw that your Co number is larger then 2. This value is acceptable for pimpleFoam, but i would recommend you to decrease time step at least 4 times. When you will be sure that stability is not dependent on time step, you can increase deltaT again (or maxCo)