[Melikmemmed]

Hi everyone,

I am doing simulation in ANSYS CFX to find aerodynamic drag force on a heavy duty truck. When I gave inflation layer during meshing I get around 15.6 percent less drag than one without the inflation. Which result is more reliable?
My another question is how maximum skewness affect the result. Should I try to decrease maximum skewness or average skewness is more important than the maximum skewness?
Many thanks

According to the ANSYS CFX solver guide in order to turbulence model work properly minimum number of nodes placed in boundary layer normal to the wall should be at least 10. I calculated the boundary layer thickness according to the formula given in the CFX solver guide and get 0.0456 m. So I tried to place enough nodes inside boundary layer to get better result. I suspect my result because it does not converge, keeps fluctuating when I gave inflation layer.

Dimensions of truck: length:15035mm; width:2480mm; height:4024mm
Dimensions of air domain: length:165600mm; width:27280mm; height:22100mm
Dimensions of body of influence: length:45800mm; width:7440mm; height:11050mm
Setup: Inlet: normal speed:28m/sec; Outlet: Average static pressure > relative pressure: 0; Road: no slip wall > wall velocity: u=0, v=0, w= -28 m/sec; Truck: no slip wall; Wall tunnel: free slip wall
Turbulence model: shear stress transport; wall function: Automatic
Turbulence numerics: High resolution

1. With inflation layer
Body sizing > Body of influence: 0.2m
Inflation (all around the truck except tires) > First layer thickness > 0.000016m (calculated it giving y+=1) > maximum layer: 28 > growth rate:1.4
Mesh details: Quality: max skewness: 0.99967; average skewness: 0.24289
RMS U-Mom, RMS V- Mom, RMS W-Mom fluctuate before reaching 1e-4
Drag force: -2016.71 [N]; Lift force: -291.094 [N]

2. Without inflation layer
Body sizing > Body of influence: 0.2m
Mesh details: Quality: max skewness: 0.83334; average skewness: 0.21862
RMS values do not fluctuate and reaches 1e-4
Drag force: -2389.53 [N]; Lift force: -610.763 [N]

I would greatly appreciate any feedback
Thanks in advance

[karachun]

You should perform mesh convergence study. Reduce both mesh size and first cell height.

No one can give you the exact number of inflation layers or mesh size. Values in guides are values you can start with.

When you have 3-4 cases with different level of mesh refinement then you can decide if you need additional mesh refinement or change in results is small enough and your mesh is converged.

Moreover you should check that your domain size (because your problem is external flow) is large enough so it doesn't affect result forces. You study this convergence in the same way - perform multiple calculations and gradually increase domain size.

Here is a userful link about mesh convergence study methodology.

https://www.grc.nasa.gov/www/wind/va.../spatconv.html

[Melikmemmed]

Thank you for your response. I appreciate your time.

I was not asking the number of inflation layers or mesh size. Sorry for any confusion in the question. Actually when I give inflation layer, number of nodes increases around 46 percent. Without inflation layer the result converges RMS 1e-5. But when I gave inflation layer it does not even reach 1e-4, although mesh is more refined.

I want to know is it obligatory to use inflation layers around the vehicle? What is the common practice? Is the result can be accepted if RMS values do not reach 1e-4 ?

Besides that adding inflation layer increases maximum skewness over 90 percent. Is it important to keep maximum skewness under 90 percent?
Kind regards

[karachun]

Originally Posted by Melikmemmed

I want to know is it obligatory to use inflation layers around the vehicle? What is the common practice? Is the result can be accepted if RMS values do not reach 1e-4 ?

If your object has large frictional resistance then yes, you need inflation.
If you have problems with mesh quality then you should repair geometry. Simplify it, remove some small parts to help mesher create good mesh.

[urosgrivc]

Inflation layers make results near the wall finer and resolve the boundary layer better.

If you have large elements in the near-wall region then the velocity gradient near the wall needs to be modeled and thus approximated.
If you have fine inflation layers near the wall then this velocity gradient is in most cases closer to the real one, but this adds some computational cost.

Because drag on the vehicle is caused by pressure differences and viscous drag forces (frictional resistance). You will be able to observe that pressure differences (front faces relative to the back faces) will cause the largest part of the drag force.
Plot your FORCE vectors in cfx post in the direction of the travel and observe where the most drag is coming from. This ˝pressure difference drag˝ will also be resolved relatively well by larger mesh elements.
Then the second part is viscous forces: Because your fluid is air it has relatively low viscosity and this is why this part is small to the total drag.
(if you would be modeling a submerged body in a liquid like water or honey this part would be much higher and the difference between inflation or no inflation layers probably a bit larger)
With inflation layers, you are able to resolve this part much better.
You can observe these forces if you plot vectors in the tangential direction on the wals these will always point in the direction of the local flow on the wals.

Be sure to plot vectors of velocity right near the walls on a previously made plane and observe how the velocity behaves near the walls you should be able to observe and understand near-wall velocity profile better.

Be sure to read this... and google is an almost infinite source of knowledge:https://www.computationalfluiddynami...hing-in-ansys/
and this video nicely explains where drag comes from: https://www.youtube.com/watch?v=GMmN...icientEngineer

Also, think a little bit about the models K-omega K-epsilon and SST and try different ones to get a filling for what happens if you change them.
for your case, SST might show some benefits as you have a combination of near-wall flow and a large surrounding volume.
This model will automatically process the near-wall region differently than the air away from the wall.

Simulations with a few large elements will almost always converge better than the simulation with a large number of small elements,
because convergence only means that the simulation is stable and all the energies add up
It will not mean that the results of drag are more precise or accurate.
For this, a mesh independence study must be done.
A simulation with finer elements will always produce more accurate results compared to a real scenario but this can be very computationally expensive -> search DNS.
This is exactly why turbulence models are used. But you still need to figure out how fine is fine enough.

[Melikmemmed]

Thanks a lot for detailed explanation. I read the article you shared before and I read it again, thanks. As you stated, since SST is accepted as best practice, I used SST for variations of this simulation. My problem is when I gave inflation layers, drag force decreases instead of increasing. As inflation layer solves the viscous layer better, I expected with addition of viscous forces, the result would be greater. Adding inflation layers also increase maximum skewness near to 1. I am not sure, maybe that is the reason why the solution ( RMS values) fluctuates around 1.0e-4. I will update the post if I can get better result.

I am attaching comparison of the results for different mesh sizes for further clarification of my problem.

Base truck 3 coarse mesh 2.1.jpg
Base truck 3 coarse mesh 2.jpg
Base truck 3 coarse mesh.jpg
comparison.jpg

Comparison2.jpg

[ghorrocks]

You are doing a steady state simulation with a RANS turbulence model (SST). This is a fundamental flaw as the flow around the truck is not steady state (it has large scale transient aerodynamic instabilities) and RANS is not applicable (need a LES approach).

You will probably need to use the DES or SAS turbulence models. These are not simple models to use and require careful validation.

But before you do any of this you should look at the "Ahmed Test Body", which is a simple car-like body which has been used extensively for vehicle aerodynamics simulation and wind tunnel results. You should develop an approach which works using the extensively validated Ahmed Test Body before trying your own geometry.

Finally - vehicle aerodynamics is not a simple field for beginners. The simple CFD approaches will not give you good results, you need to be more sophisticated than that.