Hello StarCD users,

Recently I have encountered not a problem but some surprise when I calculated a the drag coef of a new car. The mesh was tetmesh,flat body,high reynolds number. I run with 3.10A. The thing is that my drag coeff is really high >.35 , I tried prisms,RNG etc and the drag is always the same y+ is not hte problem.

I tried my big model with underhood and real underbody. My drag had to be higher,and it was, but really high > .45. My coeffs are have been never so high , I reconfigured my model several times and the result is always the same, could be the version a problem?.

I post Forces/cellarea, and they are allways below 10*average value (summ command). They seem normal.

Did someone encounter the same problem?

Thank you.

Best Regards,

Yuri

(1). It is interesting. (2). Are you saying that the drag prediction used to be low, now it is getting higher. (3). Is that because your solution is not mesh independent? Or perhaps you are getting more accurate solution? (numerically)

My solution is mesh independent,not only nearly size independent(certain range) but "prism" independent too.

I don´t think is a more accurate solution even numerically because the overprediction is too high. I had heard about overprediction of stagnation preassures with Navier Stokes codes, but it is far too high.

Could be a problem with the version of the code,the turbulence model? Could be a problem inherent to the geometry. The global behavior of the fluid is really good and it seems that there is no iportant feature in it that could cause this overprediction clearly.

Getting a more accurate solution (numerically) with this model would mean that no matter how good is my mesh or the build up of the model,I would only be able to get "relative" results do you have some experience with drag prediction and Navier Stokes codes?.

Thank you

Jordi

(1). Drag prediction is not easy. (2). Try a 2-D car shape first, so that you can easily increase the mesh size in 2-D calculation. (3). Or you could do some validation cases like the flow over a flat plate. Then you will see the mesh size required to get the accurate solution. (4). Once you have satisfactory results, you can model the 3-D flow in a similar fashion. (5). My experience with the commercial codes tells me that skin friction and drag is still not easy to predict, in general. The turbulence modeling is one of the major factor in addition to the mesh size. What is your 3-D mesh size?

Hi Yuri,

I think (hope) it is a problem with the code. I use the acoef command to calculate the torque in pumps and normally the calculations are matching the lab. results very good. When I changed to 3.100A (HP-UX) the results was suddenly way off (approx. four times measured value). The Y+ values are more or less at the same level in all the cases, so it should be ok. I have only received but not tried the new version (3.15), so let us hope that the problem is solved.

Best regards Kenneth R Jensen Alfa Laval LKM

Hi Kenneth,

Fisrt off all,thank you for your interest. Have you tried the same mesh, with the two versions?. For me it would be very difficult to try the 3.105 now.

Do you have any experience with other types of codes?

If the problem is the version, I think we would have to be aware of this problem.

Do you use "sweep" type meshes? Hexa, prisms with tetra?

Thank you,

Yuri,

Where do you calculate the drag? In Star or in Prostar? If you do it in Prostar, then you can also do it in star using the posdat.f subroutine. There is a nice example how to do this on the adapco-online page.

Using V3100A is not a very good idea, since it was a bit buggy. V3100B is confirmed to run quite well. Now version 315 is out but not many people already tried it. Someone told me that it is much more stable on tet meshes.

Hi Joern,

I am using 3.100B now, I will try to get an old case and run it on 3.100B. When I have results I will tell all of you. I have an additional trouble in the calculation, I use slithly porous medium with prisms though. Calculations that run "well" on 3.100B can fail easily on 3.100A.

Best Regards,

Yuri.

You might have to use switch 149 if you use porous cells (this procedure might be standard in v315 but I'm not sure).

Hello Yuri,

Have you tried contacting user support. The reason I ask is that there are so many things that can go wrong the first time, some quite trivial .. it is encouraging that you are getting the same "bad" coefficients with various meshes/turbulence models. To me, that sounds like a post processing or setup problem. For instance,

- when you sum the forces, you need to be careful to include all the walls, even "interior" ones under the hood. If the vector sum of the area is not zero, even a constant pressure field will produce a drag.

- the value you use for normalizing should match what is used in the experiment.

- Your physical domain must match the experiment. For example, how much clearance do you have between the top of the car and the top of the domain. Is the ground moving? What are the inlet turbulence values.

.. etc;

Good luck!

Hi Yuri,

>>Have you tried the same mesh, with the two versions?. The geometry are the same type but different in size. The cell sizes (tetra) are approx. the same.

>>Do you have any experience with other types of codes? No. I tried some other codes in order to find the best one for our purpose, but I don't think you can call it experience.

>>Do you use "sweep" type meshes? Hexa, prisms with tetra? I use tetras and sometimes in combination with prisms, depending of the problem.

Kenneth,