[dennis722]

Hello, i'm simulating a frontwing with a rotated tire and the results i get are very weird.
I use the surface wrapper and surface remesher, because the part has many errors.
But the pressure and vectors look good.

[fluid23]

Well, first of all it appears that you have some unsteady phenomenon. You should consider using the implicit unsteady solver. The sinusoidal waves in your residual and force curves are a result of this. That will help some.

My next question is whether your wall y+ values are appropriate for your turbulence/wall model. Followed by are the inputs into your force coefficient reports correct (i.e. reference area, density, velocity?).

[dennis722]

thats my setup and the residuals going wild when i choose the implicit unsteady solver, but the drag and lift values stay constant

i don't know what to do

[fluid23]

It looks like you aren't letting each time step converge. Try adding more inner iterations and see if things calm down a bit. You should expect to see a spike in residuals at each new time step after which they will reduce and converge if things are setup properly.

[dennis722]

the residuals looks better after unenable the maximum inner iterations, but the drag an lift results are as low as at the beginning

between 1350-1400 iterations i have tested something this doesn't matter

[fluid23]

Ok... so what about the other issues I mentioned. Wall y+ and force coefficient report inputs?

[dennis722]

the force coefficient report is correct, but i never worked with the wall y+ values

[fluid23]

Are you sure that your reference area is appropriate? Maybe try looking at the forces rather than coefficients to get a sense of whether they are correct. How do you know that they are wrong at present? Do you have feel for what they should be or are you trying to duplicate experimental data or published results?

As for wall y+, that is at the core of everything you are trying to do, especially on drag values. I suggest looking into this more. Based on your turbulence and wall model selections I would target 1-5 or 30-60, but anything between 5-30 will also be ok, just a little less accurate.

[dennis722]

i have uploaded the settings of my plots and the coordinate system of my simulation

i think the Cl and Cd values are too low, because normally frontwings like this doesn't have such low values. I looked at some comparable worth in the internet

[fluid23]

I suspect that your reference area choice is not correct. I don't know a lot about car aerodynamics but I do no a good bit about airplane aerodynamics and I would never choose a wetted surface area as a reference area. You typically want to choose a 'planform' area.

For example, a rectangular aircraft wing would use A= span * chord. Using wetted surface area will make your reference area more than twice what it should be.

That being said, I calculated the actual force from your plot and settings and I am getting around 60 N. That does seem a bit too low. The comparable values you are seeing on the internet, what do those show?

[fluid23]

Oopps... sorry. I see now that you used frontal area. That may be more appropriate assuming it was setup correctly.

[dennis722]

I have changed the reference area and now i have a Cd=0,345 and a Cl=-0,775 which is much more relastic
I think the parts i choosed in the frontal area report were wrong, because i took the regions without the ground, inlet,outlet and symmetry planes as the parts.
Now i have set my directly my assembly as the part for the frontal area


and back to the y+ values where can i chance the value in star ccm+? i only find that i can set it to high or low y+ values in the solver

[fluid23]

Wall y+ isn't a value you choose, it is a product of your mesh. It is a non-dimensional distance that you use to judge whether your near wall cells are sized properly. For sizing of wall y+ for a given flow I would refer you here...

http://www.cfd-online.com/Wiki/Dimen..._wall_distance

Your goal is to get a mesh that results in wall y+ values that are appropriate for the wall model and turbulence model you choose. For k-e with all wall y+ model you will want to have between 1-5 or 30-60 for best accuracy. Independently these ranges are the 'low' and 'high' wall treatments. The all wall y+ model will effectively interpolate between low and high wall models for values that are between 5-30... this will result in some error, but probably not anything that you are worried about give the scope of your effort. So... shoot for 1-60 for wall y+ and you will be fine.

You will have to let the model converge (or at least get very well established) then examine a scalar scene with all wall boundaries as input parts and field function set to wall y+...

This should get you started, there is more to it than that so I strongly encourage you to read and understand what wall y+ is, how it is used and hopefully realize that it can NEVER be ignored.

[dennis722]

Thank you very much for your answers! I will take a closer look to the y+ values and try to understand it