[me3840]

I'm hoping someone can give me some help getting this solution to converge.
I'm using k-e with non-equilib. walls, velocity-inlet and pressure-outlet. The velocity is at a lowish 26m/s for now, but I'd like to bump it up later.

I can't seem to get any convergence with the default fluent relaxation factors or the suggested factors if your solution diverges. Using:
pressure=.2
mom, k, e=.5
I can get a solution that just kind of flat-lines instead of wildly diverging.

Right now turb. intensity is constant over the inlet and outlet. Should I stick with those?
I get lots of turbulent viscosity ratio limited messages during the solution. I read in a few other threads that shutting off momentum for a little while and iterating can help solve this, but it doesn't seem to help.
I should not that, right now, the car has no wheels at all. I wanted to take this one step at a time.
I don't have a boundary layer on the ground.
I've heard taking a looksee at the velocity vectors can tell you where your mesh may not be good, but I can't get a solution converged enough to plot any vectors.

Any help?

[me3840]

Anyone got a suggestion?

[shiren77]

Originally Posted by me3840

Anyone got a suggestion?

Hi,budy.I have met the same problem.The folloing is my suggestions.first，if there are more than one blocks in your model，the ratio of mesh size between two adjacent blocks does not exceed 1.2;second，you can change the farfield boundary into “symmetry boundary;lastly,choose the ”components“option，when you set input velocity.The above is my experience.good luck.
Stone

[nfspetronilho]

Hi!
Do you have Inflation?
What's the number of layers and their dimension?
Do you have any advanced sizing function?

[me3840]

What do you mean by inflation?
The sizing function for the surface mesh is 10 degrees, growth of 1.1, with a min size of 2mm I believe. I'm using 8 layers, first layer .1 with a growth of 1.3 or 1.2 (can't remember which).

[nfspetronilho]

My opinion is:
In the mesh control, add inflation. In the inflation's "definition" you'll see the "number of faces". Click there and select the faces where you want definition and where the main process ocours (faces of the car and bottom).
For the inflation option, select first layer thickness and give it 1 or 2mm. Growing rate of 1.1 or 1.2 and the number of maximum layers 12 to 15.
Thats what i mean by inflation control.

As for the sizing in the mesh menu:
I use an "advanced sizing function" on "proximity and curvature".

The number of nodes and elements will increase, but i believe you'll have better results.
Hope this helps...
Keep up the good work and good luck with the simulations

[me3840]

I should probably note that my surface mesher is ANSA and my volume mesher is Tgrid. I've never heard of the mesh control option you're talking about, though. I doubt it's in Fluent, so what mesher are you talking about?
I've had differing opinions from some experts on w the BL thickness, but I'll try it with those parameters.

[nfspetronilho]

I was talking of the mesher existing on Ansys Workbench, so it won't any helpfull for you.

[me3840]

Well, I do have access to Workbench, though I've never heard of it being used for CFD. Do you have experience with other meshers? Would you recommend Workbench?

[nfspetronilho]

I've seen the Algor mesher for CFD And i usually use workbench. I believe it's good because Ansys has Fluent and CFX for CFD calculations. I've seen and made several simulations with Ansys and the results are good.
I've also used another mesher, but for structural analisys...

[me3840]

Well, I can't seem to get the skewness down on the BL enough to generate any layers past 6 or 7 or so. The surface mesh has a skewness below 0.6 - is there some sort of routine I can use to reduce the boundary skewness?

[vangelis]

Hi there,

If you have a surface mesh with skewness<0.6
you can improve it further in ANSA by using the
function SHELL MESH>RESHAPE [Advanced].

Ensure that you start ANSA in CFD mode so that
the quality criteria and settings are tuned for CFD.

By default in Quality criteria ANSA has Fluent skewness 0.5.

If you go to HIDDEN mode you will see how many elements violate skewness.

if you use Reshape Advanced ANSA will fix them.

You should be able to grow layers then in ANSA also.

Let me know if there is a problem.

Vangelis

[me3840]

What's the difference between the RESHAPE and RECONSTRUCT algorithms? Usually I've used reconstruct, and most of the time it gets me close to all below .5, but I have to move gridpoints manually a few micrometers to get it down to <.5. RESHAPE seems to almost do my manual movement automatically.

[vangelis]

Reconstruct improves the quality of the mesh
but still the algorithm is constrained by the boundaries
of the Macros (the Perimeters) or the feature lines if we are talking about plain FE-mod mesh.

Reshape of the other hand is more advanced as
it performes automatic JOIN of Perimeters (or feature lines for FE-mod) and reconstruct in order to get the best possible result.

Both function work based on the quality criteria
you specify.

Vangelis

[Centurion2011]

http://www.cfd-online.com/Forums/flu...nvergence.html