[stefank]

hello

I am quite new to cfd and I am trying for some weeks to simulate flow in parts of the following geometry:
variante1_geometry.jpg

The thin part in the middle (also seen on the next picture) is a fluid body and relevant for the simulation.
fluid.jpg
While trying to generate a mesh, I am wondering about the duration, the mesher needs to generate the mesh. Even generation of surface mesh on the cut surface (tagged light green) needs more than three hours. The small gap is siced with 0.1 mm and I set up properties as follows:

Advanced Size function: ON: proximity and curvature
Min. Size: 0.001mm
max. size: 0.01mm

This properties are for automatic mesh method. I was already trying with CFX-mesh, same problem here.

I am working with ANSYS 12.1 (ANSYS Academic Meshing Tools), memory of 16 GB and a Intel(R) Xeon(R) CPU with two processors with each about 2 GHz (both are assigned).
I am kind of helpless, I am working on the problem for weeks and I would be glad if anybody could help me. Do I have problems with the software or is the duration in a normal frame? If you need any other information, please let me know!!

[BrolY]

How many elements do you have at the end of the meshing process ?
Maybe you should increase your smallest element size.

More pictures (full geometry and mesh views) could also help to better understand your issue.

[stefank]

I was currently trying to mesh with

min size 0,02mm
max size 0,2mm

which is actually quite nonsense for what I want to reach. And there I have aroun 150000 elements. So I think if I mesh with the other settings, there will be definitly way too many elements. Is there any possibility that ANSYS is able to handle this? Or do I have to reduce the model extremly?

[jsm]

Hi,

Which meshing method are you using now?

For this kind of geometries, use sweep or multi zone method. It will reduce the mesh count and meshing time. Try with Ansys 13. In this multi zone method has much improvement that previous versions.

Other wise you can use ICEM CFD blocking. You have more interactive meshing options in ICEM CFD blocking method.

[BrolY]

ANSYS can handle much more elements than 150 000 !
Maybe you could post some pictures of the mesh, because 3 hours for only 150 000 elements if a little bit too long ...

[stefank]

Originally Posted by jsm

Hi,

Which meshing method are you using now?

For this kind of geometries, use sweep or multi zone method. It will reduce the mesh count and meshing time. Try with Ansys 13. In this multi zone method has much improvement that previous versions.

Other wise you can use ICEM CFD blocking. You have more interactive meshing options in ICEM CFD blocking method.

Hi,
Thanks for replying, I am using automatic meshing method and I already thought about using sweep method, but actually this quite simple modell should be kind of a basis to illsutrate how to use ANSYS. Finally I want to simulate a fluid geometry similar to the following picture (there I can't use sweep method, therefore I want to be on the right way already with the simple modell)
fluid_variante1_lamelle.jpg
(I hided the front faces for better visualisation)

As I am interested in pressure, velocity and shear stresses an very accurate mesh is needed in the narrow regions. This is way I tried to use the small meshing size in the first try.
I just got ANSYS 13 some minutes ago and it's getting installed right now. I'll try with multi zone method.
Do you have any suggestions what to do?

[stefank]

Originally Posted by BrolY

ANSYS can handle much more elements than 150 000 !
Maybe you could post some pictures of the mesh, because 3 hours for only 150 000 elements if a little bit too long ...

I was assuming this. 150000 Elements was with the coarse settings just as a try (0,02 and 0,2) and needed around 3-5 minutes. As you can see in the picture, the mesh is definitly bad, one element over the gap can't solve the flow in it appropriate.
fluid_variante1_mesh1.jpg

The narrow settings (0,001 and 0,01 mm) didn't come to a solution yet. After three hours, there was no progress in the mesh generation process at all, that's why I stopped it.

I think there must be a basic mistake in the way I handle this problem, and I don't know which it is.

[jsm]

Hi

For this kind of curvature geometry, multizone method may not be helpful. Because it is automatic blocking method. But you can try this.

If you are solving in Fluent, then you can try with cutcell method. This will give cartesian hexa elements with less element count.

Otherwise, first give the node distribution for all edges then mesh with patch dependent method. This may help you.

[PSYMN]

Stefank,

The problem isn't the method. The problem is that you only have one cell across the thickness. The velocity at the walls must be zero (no-slip wall), so with only one element and both sides set to zero, you can't possibly get a solution.

You need to get a number of cells across that gap.

If you go with Cutcell, the cartesian hexas will need to be uniform and that could kill your cell count to the third power. However, with the sweep mesher or mulitzone mesher, you could have higher aspect ratio elements that would be much more efficient.

Increase the number of nodes on the ends of your part and see what happens...

If you want Multizone to handle the corners better (miter), you could slice them with a 45 degree imprint... (sketch the line in DM and imprint it on the body)

If you go with full hexa, you would create a thin CGrid, and then delete the inner HGrid, associate the outer 3 blocks with your geometry and put the right number and distribution on the edges... It wouldn't take more than a few minutes (once you know how). Then you could add your more complicated clocking to later revisions... If you want to go this more difficult but higher quality route, I could help you out a bit.

[stefank]

Hi PSYMN,

sorry for the late reply. I still had problems with the first model and therefore I tried to mesh the second one with more complex geometry - which I actually thought would be even more complicated to mesh. Surprisingly I got a pretty good mesh for the second one in less time. (I removed the small gap in the second one. Better solution for me considering to the calculating time.
Thanks again for your help.

[Shashank Singh]

Hey all

I am a new user to ansys ICEM . I have to generate some around 600000 hexahedral cells. In geometry as given in the figure. In given figure the big cylinder is chimney and small one is burner,further square duct is the furnace and fluid is flowing inside the volume.I did multizone meshing but donot know that approach is better or not, I figured out that it could be done with multiblocking approach but I really donot know how to do multiblocking since the geometry is with three blocks . Could any one of you suggest which method is suitable along with the prodecure how to do particular meshing. It is extremely important. Thanks