Wind Tunnel Setup
 

Hi All,

I've tried to find a solution for my problems in the tutorials and documentation, but I can't seem to find anything which I can apply to this situation.

I have created our solar car aero-shell in Solidworks, and created a tunnel around it. for these tests the car has no wheels so it is floating 12cm from the bottom of the tunnel. I've attached a picture of my mesh setup to clarify this. I realize the mesh is not as dense as it should be, but these are simply my initial tests.

The domain has been created using a composite of the two 3D regions, the car, and the tunnel. the inlet speed is 25m/s, the outlet is 0 static pressure. The walls are free-slip, the ground is a no-slip wall moving at 25m/s and the car is a no-slip wall. I am using the k-epsilon turbulence model.

I am using local parallel solution with 7 threads. when I try to run the solution the solver stops with the following error:
2 isolated fluid regions were found in domain composite

I figured it simply didn't like the fact that the car was separate from the ground, so I tried using an expert parameter to skip checking for isolated domains. when I did this I was presented with the following error:
Error interpolating results onto the new mesh

I have obtained results by doing the blunt body tutorial, with my geometry cut in half along the plane of symmetry substituted in, so I suspect my problem lies in not setting up the separated car correctly.

any help would be much appreciated. please let me know if you require more information from me.

Firstly a minor point: I would recommend using the SST turbulence model. It has superseded the k-e model for many types of flow and I think this is one flow which would benefit from it.

Secondly a major point: The isolated fluid regions error means you have mesh regions which are not connected. This means you have a meshing error to fix. It is not the floating car, somewhere in your mesh is a region of mesh which is not connected to the rest of the mesh. This is a major problem and you MUST fix it.

Let me guess - have you meshed the region inside the car? If so you have to delete this region as it will not be connected.

Finally, a minor point: Your geometry is symmetric and the flow is likely to be symmetric too. Might as well chop it in half and use a symmetry plane.

Thanks for your quick reply!

I've taken a look through the documentation I have regarding volume mesh generation today. I still can't seem to figure out how to tell CFX-mesh not to mesh inside the car, or how to go about deleting the part of the volume mesh inside the car.

in regards to the symmetrical flow, I know this test is symmetrical, and as I have run the simulation using a plane of symmetry. however, once I figure out how to run the car like this, I will be analyzing versions of the car which includes asymmetrical intake duct placement.

thanks for the tip regarding k-epsilon turbulence, I'm fairly new to CFD and I was using it because a friend of mine said it gave fairly accurate results.

If you have modelled the vehicle as surfaces then you will have isolated mesh regions inside the car. Instead you want to cut the vehicle out of the block, so the vehicle is a void. This is how the blunt body mesh is made.

SST turbulence model will also allow you to use the turbulence transition model. For accurate drag prediction on a body like this you might need it as I suspect the transition points on your vehicle could be a fair way back from the front and therefore the laminar flow region is significant.

Thanks so much for your help! the solver is running now. The solution looks like it's converging, but we'll have to see in a few hours how it does.

I noticed you were from Australia, I don't know if you're interested in solar car racing at all, but this car will actually be racing in the World Solar Challenge from Darwin to Adelaide in October.

The solar car race gets national news coverage here. I am not personally involved with it at all, but I watch it on the news.

Steve -

Are you from Calgary U?

Thanks again for all your help. I've been able to run some simulations. the results are quite different than the simulations we ran last year, however the last results were obtained on a computer running FLUENT. Do you know how the results from CFX and FLUENT might differ. As far as I can tell the domain set up and turbulence models are the same, the mesh sizing is similar in both cases, but CFX is giving me drag numbers which are 14% lower than that which we obtained in FLUENT.

lastly, I've been trying to use the function area_z()@Car to find the cross-sectional area of the car for Cd calculation. The z axis is perpendicular to the front of the car, but when I use this to find the area, I get areas which are on the order of 10^-10 m^2. It works fine for the inlet and outlet, returning 25m^2 for both. Do you know what I might be doing wrong?

@Josh, yes I am from the UofC

Both CFX and Fluent should converge on the correct answer. There is no systematic bias in either code, or one would be more "accurate" than the other and the less "accurate" one would go out of business very quickly.

I suspect the difference you are seeing is in regards to the turbulence model. Did both models use the same turbulence model?