Hi,

I am simulating air flow over a 3-D wedge shaped body. The flow direction is from the negative x direction to positive x-direction. Could someone help me out with the B.C's. The flow is incompressible, I have created a cubical flow domain and assign velocity inlet condition to one of the faces with the turbulence intensity and hydraulic diamter turbulence parameters, Could someone tell me what should be the B.C on the other 5 faces on the cube. Can I use a pressure outlet condition (0 gauge pressure) in rest of the faces of the cube with intensity and viscosity ratio turbulence parameters (if I can then what would be a good value, the inlet vel is about 40m/sec).

Rahul

Assign velocity-inlets to the remainder of the faces except the outlet. I found that this used to work for me.

It all depends on what you're trying to solve!

What Mach number are you simulating?

If it's in the low subsonic region (below Mach .2 or maybe .3) then you're in the incompressible regime, and you can use velocity inlets on the forward face and the 4 side faces. Then use a pressure outlet on the rear face. If you're in the compressible flow regime, then you should be running the model with the ideal gas law. In this case DO NOT USE THE VELOCITY INLET!!! Read the user manual on BCs. Using a velocity inlet and a pressure outlet does not limit the maximum dynamic pressure for compressible cases, so you are risking getting completely useless results. In the compressible regime, I recommend using a pressure BCs. You can either use pressure inlets on the 5 faces and a pressure outlet on the last, or you can use pressure far field on all 6 faces. Be careful when using pressure far field though, your BC has to be far enough away from the model so that the body effects do not extend to the BC. With the pressure inlet / pressure outlet combo, the BCs can be a little closer, but not much.

Hope this helps, and good luck, Jason

Hello Jason,

The flow in my case is in the low subsonic region, and is incompressible. Thank you for your suggestion. As in my problem I need to find the pressure distribution on the wedge based on directional load, i.e the flow comming in from the - x direction and going to the +x direction. Would you suggest that for the cube that I have created can I use velocity inlet at the forward face of the cube and use a +x, velocity inlet on the other 4 faces and a pressure outlet in the end face. This would probably be a better approximation to create a situation where the flow is directionally in the +x direction. I would like to know how would this approximation work. Also would you suggest that I use the turbulence intensity and viscosity ratio, turbulence parameters with the velocity inlet and pressure inlet conditions? If so what would be a good approximations. I currently use an intensity of 0.2% and viscosity ratio of 10. Though my solution seems to converge (I have been monitoring forces on the wedge which seem converged), but still have the message turbulent viscosity ratio limited to a ratio of 10000 in 60000 cells. Please suggest.

Rahul

The TVR warning is usually related to your near-body mesh, not your boundary conditions. You can see where the problem is by going to Plot->Contours. Turn on Filled, turn off Node Values, turn off Auto Range, and turn on Draw Grid. For the range, use something like 50000 to 100000. Plot it on 'default-interior', and make sure that Clip to Range turned on when you turned off Auto Range. The causes of this warning have been discussed a lot on this forum, so I recommend searching for information. Typically, it's that your mesh isn't refined enough where it needs to be.

For incompressible flow, using the 5 velocity inlets all with a +X velocity, and the pressure outlet is a decent choice. Turbulence intensity and viscosity ratio depend on your problem. Again, search the forum for some advice on this.

Hope this helps, and good luck, Jason