What is question? From images it looks good mesh.
How to access Ansys Online Help Document
How to show full resolution image
Guidelines on the Student Community
How to use Google to search within Ansys Student Community
@kkanade, the questions are:
1- how to put a single element in the thickness? (if it is possible)
2- the boundary layer (picture 3 and 4) is not continuous on the walls of the ball and the sidewall, doesn't this cause a problem?
The calculation is static with compressible CO2, k-w sst turbulence model. I set all residuals to 1e-6 and it seems to have trouble converging at the first few iterations, should I be concerned?
The inflation won't fit into the narrow gap so it's compressing and then losing layers. If the ortho quality is good you don't need to do anything. There's not an option for forcing the mesh to extrude from one side to the other (yet) so you either need to reduce the surface facet size or number of inflation layers if the quality is poor.
@Rob Thank you for your clear answer! My ortho quality is correct, so 0.15, why don't the residues converge to the requested value in your opinion?
Looking at the residual curves it seems that it will never converge to 1e-6,
Have a look at the flow field. I'd focus on immediately downstream of the valve and also the step.
@Rob I would like to reduce the number of boundary layer on the balle which is a wall, but I notice the application of boundary layer is done at the same time on all walls, is there any way to do it on the walls and then on the ball?
it is applied directly to all walls.
How can I put two boundary layers on both walls?
Have a look in the Add Boundary Layer section, you look to be able to add multiple inflation sets using the surface labels.
@Rob I looked for the add boundary layer section, but there is none, I just have what is on the image below that allows you to add the boundary layer to all walls at once! I am on a 2019R3 version. Maybe there is an extra manipulation to do?
Hi, @Rob iIt seems that it is possible on the 2020R2 version and not the 2019. But I just ask about the minimum orthogonal quality, I think we should be at 0.1 and here I am at 0.06. But the output shows [Quality Measure : Inverse Orthogonal Quality]
---------------- 279911 cells were created in : 0.93 minutes
---------------- The mesh has a minimum Orthogonal Quality of: 0.07
---------------- The volume meshing of geometrie2d-1 is complete.
Is it a good mesh? Why is it different from the quality I had in the 2019 version yet it's the same features just the boundary layer changes?!?
In versions prior to 2020R2, when the cell aspect ratio within the boundary layer exceeds certain threshold, Fluent mesher splits the cells in two. This does not happen in the 202021 and 2021R1 versions, and it may be the cause of the variations that you are noticing.
@Aitor thank you for your answer. So the controlled mesh in the 2019 version would be more interesting? How could I then correct this on the 2020 version?
@Aitor it seems that the transition ration plays an important role, knowing that I put 15 elements on the boundary layer and I am in smooth-transition, how is calculated the height of the first boundary layer?@Rob
The boundary layer maths are covered in the manual, and cell height is generally a function of some of facet size, first cell height, last cell height and number of layers.
I personally prefer not to have the cells split in two.
Based on my experience, aspect ratio is not crucial in RANS simulations (of course, with some limits, even though I cannot imagine a good mesh in the outer region that has a maximum aspect ratio of 10.000 in the BL, for example). In the case of LES, there is something wrong if Fluent meshing performs the mentioned splitting (the initial mesh should have a maximum aspect ratio less than 10 and the correction should not be done).
In regards to the height of the first boundary layer, it depends on your application. The ideal situation is to have wall y+<1, although values between 1 and 10 are good for RANS simulations when no transitions model is used. In order to compute the height in dimensional variables, just type "y plus calculation" on the Internet and you will find some online calculators for your specific case.
@Aitor @Rob thank you for your reaction.
@Aitor the calculator will calculate the value of y necessary to have y+ = 1. I would like to know how to enter the value of y in the calculator because? Is it in function of transition ratio?
I see no option of choosing the height of the first layer in the smooth-transition offset method. Just number of layers, transition ratio and growth rate.
@Aitor ok, I'll try to see if there is a relation between all this!
So I remeshed and I got an orthogonal quality of 0.15, which seems good. So I restarted the static calculation but the residual continuity seems to have stabilized even though I asked for a residual value of 1e-4 and it stabilizes before. Should I exploit this result? Is there anything else that can be modified so that the residual continuity converges to the imposed value? @Rob said "Take a look at the flow field. I would focus on immediately downstream of the valve and also on the walk." How? It's a compressible gaz (so ideal gaz)
2e-4 for a time scale of 0.5 seems okay. Do you see something in the results that does not convince you?
@Aitor what bothers me is that the continuity residual does not reach the value of 1e-4
Which value is reached when you set time scale to 0.1?
Convergence is usually good if continuity residual is less than 1e-3.
Ansys customers with active commercial software licenses can access the customer portal and submit support questions. You will need your active account number to register.