mesh
 

I have a 3D meshing, unstructured. According to the histogram for quality and aspect ratio my mean value is 0.77. And for the skewness is about 0.99.

When I am using this mesh in fluent, it gave a fluctuating residual.

Has someone have an idea what kind of problem that I am dealing here and what is the solution?

Thank you very much

Arya

Re: mesh
 

Sorry, I forgot to tell you that my mesh was generated using ICEM CFD.

Thanks

Re: mesh
 

Hi Arya,

Not only the mean value is important but also (and maybe mainly) the minimums. What are your minimums for these parameters? Can you improve your mesh to eliminate them?

Cheers

Anderson

Re: mesh
 

Hi Anderson,

I think the minimum is between 0.3 and 0.4

I do not know how to improve them. So far I only use smooth mesh globally. And my mesh size is already big (around 1,7 million cells).

Do you have any suggestion

Thanks

Re: mesh
 

Hi Arya,

Normally I try to push my minimum for over 0.4

I don´t have experience with Fluent, but CFX gives you a warning message when the mesh present some cells which can couase convergence problems. Have you got any of these messages?

Smooth mesh globally should work. Try to push it gradually: For example: minimum 0,35, then minimum 0,40, then 0,45 ... And maybe try to improve more than one criterion (I use quality and skewness)

Another approach (time consuming but maybe better) is to click on the histogram of quality and ask it to show the worst elements. Then, manually, you can try to change the blocking (e.g. edge lenghts) to improve the overall quality in the worst zones.

Hope you have agood computer to deal with all those cells

Cheers

Anderson

Re: mesh
 

Hi Anderson,

No I don't get any error message. Usually after this step, I select an icon to check on the mesh. The only message I got is unconnected vertices.

I'll try your suggestions. I use 3 parameters (quality, skewness and aspect ratio). What is the common value that you give for the number of iterations and maximum value when you do the smoothing?

And I don't quite understand about fixing the worst mesh. Can you give a more detail explanation?

Thanks

Arya

Re: mesh
 

Hi Arya,

Convergence isn't always related to mesh quality, so it is worth you while to check how the solution is behaving in the regions that are not converging.

In terms of mesh quality, one option would be to convert the domain to Polyhedra from the Grid>Polyhedra menu, assuming the other options you are using are compatible with polyhedral elements. You can opt to convert the entire domain, or just the poor quality cells. This will create cells which are the mesh dual of the tetrahedral mesh (cells around the nodes of the current mesh). the procedure is described in the FLUENT 6.3 documentation. This should help convergence, but you may need a slightly finer grid to get the same accuracy.

CFX is less sensitive to mesh issues such as this because it is always solving on the mesh dual by way of its discretization, rather than converting the mesh itself.

You could also try using the coupled solver. Under Solution Controls, change the Pressure-Velocity Coupling to "Coupled".

-CycLone

Re: mesh
 

Hallo

In your histogram of quality, click on the column which refers to the worst cells (around 0,3, isn´t it?). With right bottom, click on Show. This will show in your mesh where the cells have quality values in that interval (width of the first colunm). These are your "bad guys". If they are concentrated in some area, maybe you can change the edges around it in order to improve them.

Regarding the values for number of iterations, I usually play with it a bit. I dont really know a good procedure to choose it, but normal values for me are 3 and 5.

hope it helps

Anderson

BTW, what is your case? is your geometry complex?

Re: mesh
 

Hi cyclone:

So basically I don't have to change anything in my mesh which is originated from icem cfd. I'll see what I can do tomorrow. I am using SIMPLE as my pressure-velocity coupling and I set all the discretization for QUICK. Do you have any suggestion for the disretization scheme? And one more thing I have this fluctuation problem as soon as I change from incompressible to compressible.

For anderson:

If you don't mind I can send a tiff file of my model. Because of time constraint to finish the project, I thought that unstructured approach would be the best option.

Thanks

Re: mesh
 

Hi Arya,

I wouldn't bother with QUICK, Second Order on Pressure and Second Order Upwind on Momentum and Energy should give you good results. QUICK can be highly non-linear and hard to converge and doesn't really offer than much of an improvement over Second Order (none if you cannot converge). Stick to First Order Upwind for Turbulent Kinetic Energy and Dissipation. Solving these second order can lead to non-physical values due to numerical over- and under-shoots. Turbulence is largely dominated by source terms so advection is a second order effect anyhow.

For pressure-velocity coupling you could also try SimpleC, which should provide some improvements over Simple. As for compressible vs. incompressible, a compressible flow will be more non-linear so it isn't surprising that it gives you more grief. The coupled solver will probably make a big difference.

-CycLone

Re: mesh
 

Hi Anderson,

I have sent you an email, if you have time please read. One more thing, what did you usually do for the global mesh setup (for the tetrahedral mesh)?

and for Cyclone, my project supervisor advise me to do some adjustment for the mesh, so I could not say anything about changing the setup for the fluent, because the same setup works for the mesh generated with centaur.

Thanks

Arya