Hello,

Question 1) : This is Ok. These dimensions should be sufficient so that the boundary conditions on the side faces of your domain are not influencing the pressure field near the investigated model (too much).

Question 2) : SST model is the best possible choice for a (U)RANS model. In particular if you study the effect of a diffusor.

Usually one aims for y+ values in the order of y+~1-2.

The number of inflation layers depend on the targeted y+ value, because at the same time you should aim for a smooth mesh transition between the last prism layer (last counted from the wall surface towards the free open volume) and the adjacent tertahedrons in the volume mesh. The change in volume between the outermost prism layer elements and the next following tetrahedral elements should be in the order of 1-5, not larger. Since the prism layers directly at the surface are very thin (small volume) and we need to resolve the profile of the boundary layer at the wall surfaces with approx. 10-15 prism elements, we usually end up with 15-20 prism layers for such a smooth transition. In regions, where walls are in close proximity (e.g. the road surface and the car floor surface) the things might be more squeezed. Consequently their might be either none tetrahedral elements or they are small as well. In this case a slightly smaller number of prism layers might be sufficient.

Question 3) : Largely depends on what mesher do you use. ANSYS Meshing? Fluent Meshing? ICEM/CFD? ANSA?

The usual way is to enclose the car body in a series of enclosed rectangular boxes. One box placed inside of the next slightly larger box. Usually 2-3 boxes are enough. Each box gets its own meshing parameters, so that the most aggressive meshing parameters are gettign assigned to the innermost box. Then a mesh size transition is planned and takes place to the next following box and so forth. By that you end up with a fine mesh in the car's surrounding without transitioning this fine mesh to the all over outer (virtual) wind-tunnel volume and to the area in front of the car, where essentially there is not so much change in the fluid field of motion.

If ever possible I would recommend to use ANSYS 2019.R3 instead of the old 18.x.

Hopefully this helps.

Rgeards,

Dr. Th. Frank.

Hello,

Question 1) : This is Ok. These dimensions should be sufficient so that the boundary conditions on the side faces of your domain are not influencing the pressure field near the investigated model (too much).

Question 2) : SST model is the best possible choice for a (U)RANS model. In particular if you study the effect of a diffusor.

Usually one aims for y+ values in the order of y+~1-2.

The number of inflation layers depend on the targeted y+ value, because at the same time you should aim for a smooth mesh transition between the last prism layer (last counted from the wall surface towards the free open volume) and the adjacent tertahedrons in the volume mesh. The change in volume between the outermost prism layer elements and the next following tetrahedral elements should be in the order of 1-5, not larger. Since the prism layers directly at the surface are very thin (small volume) and we need to resolve the profile of the boundary layer at the wall surfaces with approx. 10-15 prism elements, we usually end up with 15-20 prism layers for such a smooth transition. In regions, where walls are in close proximity (e.g. the road surface and the car floor surface) the things might be more squeezed. Consequently their might be either none tetrahedral elements or they are small as well. In this case a slightly smaller number of prism layers might be sufficient.

Question 3) : Largely depends on what mesher do you use. ANSYS Meshing? Fluent Meshing? ICEM/CFD? ANSA?

The usual way is to enclose the car body in a series of enclosed rectangular boxes. One box placed inside of the next slightly larger box. Usually 2-3 boxes are enough. Each box gets its own meshing parameters, so that the most aggressive meshing parameters are gettign assigned to the innermost box. Then a mesh size transition is planned and takes place to the next following box and so forth. By that you end up with a fine mesh in the car's surrounding without transitioning this fine mesh to the all over outer (virtual) wind-tunnel volume and to the area in front of the car, where essentially there is not so much change in the fluid field of motion.

If ever possible I would recommend to use ANSYS 2019.R3 instead of the old 18.x.

Hopefully this helps.

Rgeards,

Dr. Th. Frank.

Thomas Frank, Thank you for your answer, this was really helpful.

Hi Abdallah,

I guess the domain size you considered is more than enough. For comparable Re numbers I usually go a bit below (10-15 % less) and did not experience any problem.

As far as the y+ is concerned, I guess it should be related not only to the turbulence model you use, but also to the boundary conditions you impose on the solid wall. So, if you use wall function, y+ around unity is Ok. However, if you use a no-slip condition, probably you should go below unity. BTW have tried the EARSM model?

I guess you use the ANSYS mesher. If so, Thomas is right. You may define volumes (boxes or cylinders) in the areas where yu need the mesh to be refined.

Good luck!

Adrian

Adrian Lungu Thank you for your answer.

I'm applying no slip condition to the model, and slip condition to the floor. The problem I'm still facing is that I'm limitied to 512k cells, and after calculating the first layer height needed to acheive y+(1-2) and applying that setting to the model, floor and the walls, I'm unable to acheive a smooth transition between the last inflation layer and the tetrahedron elements next to it, especially on areas far from the model where the mesh is coarse.

I'm using symmetry but still facing the same problem. Any recommendations?

How about imposing the y+ condition only on the model? I mean no enforcing the y+ condition on walls on which the slip condition is imposed.

Will this have a big effect on the results? And if i did that, should i apply anything additional to the walls instead of the inflation layers?

Appreciate your help.

Adrian Lungu : From my perspective there is absolutely no way to achieve an acceptable accurate solution for a flow around a car model with the limit of the free ANSYS Student version (512k cells). Usually such a simulation requires at least 5-6 Million cells, depending on the surface details of the car model.

Regards,

Dr. Th. Frank.

Adrian Lungu : The y+ condition can be limited to the car surface. Depending on what you like to predict on the road surface as well. But it is not required on the outer "walls". Any kind of boundary layer on outer walls will have no effect on e.g. drag and lift of the car model. Therefore it would be a useless spent effort. Outer "walls" can be set to symmetry instead (if not a scale-resolving turbulence model is used; in this case opening BC's would be the better choice).

Regards,

Dr. Th. Frank.

Hi Abdallah

about domain question, it depends on your 2-D or 3-D simulation, furthermore, if there is no any district around your model to simulate it(same as walls of wind tunnel or flume wall,..) symmetry boundary condition is performed or free slip , you should check flow near your boundary be equal to free stream velocity , so you do not need to increase your domain.

but

in the case of Y+ : for sst-k-w you should set it less than 1, for this matter you have to initial guess and run your simulation , after that check the Y+ in fluent around the surfaces of your solid model and if it is not acceptable, reduce the thickness of your boundary layer.

B.R

Ramin Alipour

Hi

The cases are very simple and having a cursory over present papers you could find a handful of authentic sources in this issue. Check out my papers and introduced references for a quick guide.

Regards,