CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Drag prediction and wall boundary condition (http://www.cfd-online.com/Forums/main/102700-drag-prediction-wall-boundary-condition.html)

 Jeremie84 May 31, 2012 16:14

Drag prediction and wall boundary condition

Hello everyone,
I’m modeling a semi-trailer truck with a drag reducing device on it (trailer skirts). I want to compute the drag coefficient of the underbody and skirts.
I am doing a hybrid mesh with tetra and prism layers. Since I am focusing on the underbody and the skirts, prism layers will be extruded on theses surfaces to solve the boundary layer (and get accurate drag predictions, if possible ;-)). On the other hand, there will be no prism layers on the other parts (side and top of the trailer, the cab, gap between the trailer and the cab) to limit the number of cells.
My question concerns the wall boundary conditions in Fluent. I apply a no-slip condition for the walls with the prism layers. But I’m wondering what the best option is for the other walls with no prism layers:
- A slip condition,
- A no-slip condition even if tetra cells are immediately adjacent to these walls. In this case, the y+ will be excessively high, but should I “worry” about that if I am not computing the drag coefficient on these walls?
Thanks a lot
Jeremie

 FMDenaro May 31, 2012 16:23

Quote:
 Originally Posted by Jeremie84 (Post 364159) Hello everyone, I’m modeling a semi-trailer truck with a drag reducing device on it (trailer skirts). I want to compute the drag coefficient of the underbody and skirts. I am doing a hybrid mesh with tetra and prism layers. Since I am focusing on the underbody and the skirts, prism layers will be extruded on theses surfaces to solve the boundary layer (and get accurate drag predictions, if possible ;-)). On the other hand, there will be no prism layers on the other parts (side and top of the trailer, the cab, gap between the trailer and the cab) to limit the number of cells. My question concerns the wall boundary conditions in Fluent. I apply a no-slip condition for the walls with the prism layers. But I’m wondering what the best option is for the other walls with no prism layers: - A slip condition, - A no-slip condition even if tetra cells are immediately adjacent to these walls. In this case, the y+ will be excessively high, but should I “worry” about that if I am not computing the drag coefficient on these walls? Thanks a lot Jeremie
what are you searching for is a difficult task.. I suppose you will use RANS formulation, and you have to face the first task: understanding how many grid-points you get in the boundary layer...
- In principle you must have at least 3-4 points in the viscous sub-layer region (y+<1) to hope in a resolved boundary layer. However, this is an ideal estimation for flat walls...
- remember that if you decide to use wall-functions (first grid point is outside the viscous sub-layer, y+>1) then you have the risk that the solution in terms of the drag will strongly depend on the wall function rather than on the flow solution.

 Jeremie84 June 1, 2012 09:00

Yes I will use RANS formulation. Ideally, I’d like to capture the viscous sublayer (as you mentioned). But unfortunately that will depend on the cell count (compromise between accuracy and computation time). If the cell count is too high, I will use wall functions (first grid point in the log-law region).
Actually, my question was about the “other” walls: those where I will not compute the drag coefficient. The mesh will be quite coarse adjacent to these walls (tetrahedral cells, not prism layers). And I am wondering if it is relevant to apply a no-slip condition on these walls or if I can neglect the viscous effects and apply a slip condition.
Thanks again
Jeremie

 Far June 1, 2012 09:44

well, it is not easy to tell you without testing it that when to use slip or no slip condition. You should proceed with both methods and check the results.

 Jeremie84 June 1, 2012 10:19

OK, thanks. I will try both.
I assume that in both cases, I will have a lack of accuracy (although I am not looking for accuracy on these particular walls because I am not computing the drag coefficient on these walls): if I choose a slip wall I neglect the viscous effects, and if I choose a no-slip condition I am not sure to correctly capture the boundary layer due to the coarse mesh adjacent to the walls (tetra cells). Am I right? I suppose that it’s a question of choosing the “least worst” option, no?
Thank you very much
Jeremie

 Far June 1, 2012 10:51

In the case of slip condition, you may have the loss of accuracy, but in the other case; i.e. wall function you may have the wrong physics and numerics, which may pollute the whole solution. For example if you are using wall function and Y+ is zero some where then the phsics of wall ceases to be valid. I hope you get my point.

 Jeremie84 June 1, 2012 11:20

Thank you Far,
I understand your point and it is very useful to understand the difference between loss of accuracy and wrong physics. But just to be sure: how y+ can be equal to 0? If I have relatively large tetra cells adjacent to a wall (with a no-slip condition and wall function on), would y+ be extremely high so that the physics of wall ceases to be valid as you mentioned?
Thanks again
Jeremie

 Far June 1, 2012 11:43

check this

first few lines from 2nd paragraph:

Quote:
 The major short-coming of standard wall-functions, being based on the log-law, is that the underlying grid requirement ceases to be valid inevitably in ﬂows with separation, as Y+(1) goes to zero at the separation point and becomes small in regions of separated ﬂow.

 Far June 1, 2012 11:50

few more references

 Jeremie84 June 1, 2012 13:34

I will probably apply a slip condition to the walls where I don't compute the drag force. And try to use the non-equilibrium wall function for the no-slip condition walls where I compute the drag force, and check for potential separation.

Best regards

Jeremie

 Far June 2, 2012 02:49

which code and turbulence model you are using?

 Jeremie84 June 4, 2012 09:27

I am using ANSYS Fluent 12.1
Concerning turbulence, Realizable k-e model seems well suited for automotive external aerodynamics.

Regards,

Jeremie

 Far June 4, 2012 09:31

If possible switch to fluent 14, it has really nice algorithm and you may achieve convergence in 200-400 iterations for any size of problem.

My choice is SST turbulence model.

 Jeremie84 June 4, 2012 09:38

If it was just up to me, I would already use Fluent 14... :-)

 Jeremie84 June 4, 2012 16:15

I was also thinking… Since the pressure drag comprises more than 90% of total trailer drag, a first option could be to consider all the vehicle’s walls as slip walls, and thus neglect the boundary layers and the friction drag.
But in that case, with only slip walls, I wonder if I will be able to capture the main flow characteristics, such as separation, etc. Does the friction (or the absence of friction) have a major impact on the pressure drag?
Thanks again.
Best regards,
Jeremie

 FMDenaro June 4, 2012 16:21

the boudary layer theory states that the pressure in the boundary layer is approximatively independent from the vertical position, that means you have a pressure distribution that can be predicted by the Euler equation. However, things are quite more complex for curved walls...

 All times are GMT -4. The time now is 16:27.