[treviusss]

Welcome,

I've been trying to calculate a steady flow around Ahmed body in 2D. The vehicle is in refinement zone in which I'm changing element size to perform a mesh independence test. Also I'm changing element size in rest of the domain and first layer height (which has 5 layers). Right now I have done 5 meshes :
12 000, 24 000, 58 000, 89 000 and 128 000 elements. The last one I wanted to do has 262 000 elements to make a final mesh to choose from but I can't solve the problem because it can't reach convergence no matter what I do.

I'm using Realizable k-epsilon model with Non Equilibrium Wall Function. Velocity in Inlet is 40m/s with 1% Turbulent Intensity and 10 Turbulent Viscosity Ratio. Outlet has 5% Turbulent Intensity.

Pressure-Velocity Coupling is SIMPLE.
For the first 100 Iterations I'm using First Order Upwind in Momentum, k and epsilon and then I'm chaning to Second Order Upwind.
Pressure is in Standard all the time (don't know if I'm doing it right)

I'm initializing the flow field with zero velocity and turbulent values from inlet (as written in 4.3 in http://www.southampton.ac.uk/~nwb/le...ice_Ver1_2.pdf)

After about 1k or 2k iterations residuals starts to oscillate. I have tried to lower Under Relaxation Factors according to this site: https://www.sharcnet.ca/Software/Flu...g/node1022.htm

"If unstable or divergent behavior is observed, however, you need to reduce the under-relaxation factors for pressure, momentum, , and from their default values to about 0.2, 0.5, 0.5, and 0.5"

But still I couldn't reach convergence of this problem.

Is there anything I can do to reach convergence without changing mesh?

Thanks for answers in advance

[Abdelwahed]

Did you add BL mesh i mean inflation, because such turbulance model needs very small values of Y+ which define the the size of the first layer to catch the BL for better convergence. I observed that you didnt mention BL mesh.

[treviusss]

Yes, I did. Inflation layer consists of 5 layers and I was changing first layer height to reach appropriate y+ value as stated in this article http://www.southampton.ac.uk/~nwb/le...ice_Ver1_2.pdf

Check for y+-values (30-300)

When I used First Layer Height of 1mm I got those results (shown in one of the attachments):

Average of Facet Values
Wall Yplus
-------------------------------- --------------------
back 16.187474
bottom 67.326585
nose 91.813777
slope 22.933844
top 67.43571
---------------- --------------------
Net 63.210509

(maybe a little too low in some zones)

And when I used First Layer Height of 2mm I got these :

Average of Facet Values
Wall Yplus
-------------------------------- --------------------
back 39.315677
bottom 102.8682
nose 175.95522
slope 45.114512
top 124.41201
---------------- --------------------
Net 111.33648

I attach how my mesh looks, in this photo the mesh is that one which I can't solve. First Layer Height is 1mm, Elements near vehicle are 2mms and around the rest domain 5mm.

Also I tried to solve another time but right now after 100 iterations I changed to Second Order Upwind and changed straight away to Under Relaxations Factor to 0.2 Pressure, 0.5 for Momentum, k and epsilon. This time the case still can't converge.

Results are in attachments : Residuals and how velocity magnitue looks when I stop calculating. It looks to me like it can't solve the turbulent flows that are in the wake of the vehicle.

The last photo is how velocity magnitude looks in the case that I solved with a little bigger elements in refinements (3mm) and domain (7mm)

Thanks for any more answers or ideas in advance

[Abdelwahed]

I ve seen your mesh and it seems very dense and such mesh is useless because it takes a lot of memory and time and will ever give a good result. First you need to specify the computation domain dimenstions , as in leterature put the inlet at 1.5 L (L is Ahmed body length) and put the outlet at 3L and the upper surface at 0.5 L and set it as symmetry. Try to simple the Ahmed body countours with about 250 or 300 simples make sure to be dense at nose and at the rear to catch turbulence effecte. After for a velocity of 30 m/s i found that the first layer need to be at 0.012 mm to get an y+ about 1. Set the inflation at 11 layer at least with a ratio of growing about 1.15.
After try to mesh the domain with reasonable element size and growing ratio of 1.2. Try to get a smooth and progressive growing mesh.
I advice to increase turbulence to 9.99 % because for small velocities it effects computation.
Try to add BL mesh at the wall under the Ahmed body i means at the gap under Ahmed body.
Wich it is usefull.

[treviusss]

I know that this mesh that I want to solve is dense but I wanted to calculate it only to compare results to other meshes.

My domain is 2L in Height, 2L in front of the Ahmed body and 6L behind it.
I don't understand what you meant by saying "try to simple Ahmed body countours". I made this geometry in DesignModeler and I think its simply as it is. Some straight lines and arcs, 25 degree slant. Also it is 1/3 size of normal Ahmed body.

Why did you say I need y+ to be 1? I've read many articles and papers and everybody stated that for external automotive calculation while using k-epsilon model you should consider y+ to be from 30 to 300 and with 5 layers.

To be honest I have no idea how to make a good growing mesh towards my body. I tried using Edge Sizing with bias but it didn't work out as I wanted, only edges went progressive while the rest of the elements in face are still the same, if you can give me some tips how to do it I'd be really glad.

About that turbulence in inlet I based it on this video :
https://www.youtube.com/watch?v=iQWzoomxjc8&t=372s
and the paper that he posted in description
https://drive.google.com/file/d/0B9w...BOZzFaVXc/edit

I'll try to add inflation layer to "road" but as I said in the title of this topic I wanted to find out any methods to converge this case without changing mesh.