CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   BL generation around a wheel issues (

me3840 February 2, 2011 20:00

BL generation around a wheel issues
I'm trying to generate a BL around a spinning wheel (on a car), but I can't seem to get it to work. I'm using ANSA for a surface mesher, while I use Tgrid and ANSA as a volume mesher (neither has been able to generate a BL).

The issue is the ground - the prisms won't generate near the ground, with the wheel slightly above the ground or slightly below it, or they will just generate straight through the ground, and the volume mesh will fail.

Does anyone have any advice on avoiding this? Is there a way I can generate the layer taking into account the ground? Can I do a simulation that gets rid of the control volume? I don't know much else outside the realm of finite volume modeling.

I also have ICEM at my disposal, but I'm new to it, so I don't know much about it.

vangelis February 7, 2011 08:05

Hi there,

I suppose you have a very narrow angle there between the
tyre and the road.
Have you checked that the mesh of the tyre and the road are topologically connected?
Can you attach a snapshot of the area?


me3840 February 17, 2011 19:08

Sorry for the slow response. I got a new version of ANSA which will generate prisms while taking into account proximity to opposing zones. I can generate prisms now, but there will be excluded zones. Is it feasible to just generate solid prisms all the way to the ground? The wheel is mounted inside of a fairing, and a flat plate is parallel to the ground, leaving not much distance from the ground to the bottom of the fairing. I tried making a curve on the ground and setting ANSA to generate prisms over it, too, but it would not connect the two layers.

Yes, the wheel and ground are topo connected.

vangelis February 18, 2011 04:07

In this case I would say that a picture is worth a thousand words, so if you can post one it would make things easier.
By the way which ANSA version are you using now?

me3840 February 18, 2011 11:48

Whoops, sorry, forgot to add them last time.

I'm using ANSA 13.1.1.

When I do the layer generation, ANSA excludes areas and then I tetra mesh around that. I've gotten a couple to mesh, but the solutions diverge in FLUENT with the wheel stationary and spinning.

Edit: the second image is surface mesh only, while the first has the layers.

vangelis February 21, 2011 03:28

That makes things more clear.

It seems that you have a very narrow angle there
and it also seems that you are trying to generate
a relatively high boundary layer mesh with respect
to the surface mesh size.
Are you generating layers in Absolute height mode
or aspect?
What is the total bl height with respect to the shell
mesh size?
You need to check that the total height of the layers
can fit in that tight space.

Here are some suggestions that may help:

Increase the Smooth Vectors Max Angle to say 85 deg
Reduce the proximity check factor to 0.1
Activate the Allow Squeeze
De-activate Exclude and collapse.
Increase also the adjust angle to sides to 85deg.

If this does not work, then you probably need
to change the geometry a bit in that manner:

Let me know how it goes

P.S. when you use ANSA for CFD work make sure you select
the CFD option from the startup launcher.
This ensures that all default settings of the software are
tuned for CFD.
This ensures that

me3840 February 24, 2011 22:28

Yeah, I extruded a sheet around the tire to the ground and that worked. I'll try those settings in ANSA on another model - I got it to mesh in Tgrid. I'd rather use ANSA, though. I am using the CFD option.

What's the difference between absolute and aspect height mode? I was using absolute.

The results are rather invalid after running through Fluent, though - the pressure near the wheel is a lot higher than the rest of the car, and the streamlines in that area don't make it apparent anything's spinning. I'm going to try again with a kklw simulation (I used a ke before); I hear ke doesn't do too great with separated flows.

vangelis February 25, 2011 06:14

Absolute mode means that the value you specify
as first layer height is an absolute distance, say 0.5mm

whereas aspect mode you specify a factor, say 0.2,
and ANSA will generate as first height a value equal
to this factor multiplied by the local average length of
the surface mesh.

All times are GMT -4. The time now is 05:24.