A wall has been placed
 

Hello Everybody,

I have a problem with a simulation in CFX. The Problem is:

The geometry is as simple as that: a board with an ellipse at the beginning. In the middle of the board i have a hot aluminium plate. Three Free Slip walls, one Symmetry plane, Inlet, Outlet, 10e6 nodes, structured mesh

I have already done a simulation with the following boundarys:

- SST
- Inlet: 10 (m/s), Tu = 0.1 ; l=10mm, 300K
- Outlet: 0 Pa
- Ansys V11

and it worked fine.

Now I have the same case just with a little change, there is a wire behind the ellipse to increase turbulence.

But now it isnt working at all, I get the message:
- " A wall has been placed at portion(s) of an OUTLET..."
- The maximum Mach number is about 10
- The Residuals drop to 1e-100
- The Result File is completely empty

I have already changed a lot of parameters but nothing helped.

Any Ideas, Solutions, deja vus? Any more informations?

Thanks a lot

Camoesas

What is your reference pressure? If your outlet is 0 Pa then you will need a finite reference pressure or you will have problems.

The error message suggests the wire is causing convergence problems. A wire in high Ma flows is going to have shocks and rarefactions and all sorts of complex stuff happening so will be a lot harder to converge than high Ma flow over a flat plate.

You will probably need to start with small time steps and increase them as the simulation proceeds. Also make sure your mesh quality is good.

have you used "outlet" or "opening" boundary conditions?

HI,

My reference Pressure is 101325 Pa. The Flow velocity should be 10 m/s, thus far far away from supersonic.
For the Outlet I use outlet and not Opening

Regards

Then why are you running a compressible flow solver? You have to be using a compressible solver as it was talking about Mach numbers. Go back to an incompressible solver and I bet it converges just fine.

Hey Glenn,

thats interesting, but after a lot of searching and aimless clicking in Ansys I still don't know where to choose compressible / incompressible solver!

I can't remember ever seen such a menu :confused:


Could you please lift the fog! Thanks

Hello!
I'm simulating a centrifugal compressor and i have the same problem (a wall has been placed at portion of an outlet boudary condition...)
I tried by setting a static pressure as outlet boundary condition but the situation persist.
I just want to know if your problem has been solve, and how? it could help me.
Thankyou

Unfortunately everybody in the world calls them incompressible and compressible solvers, but CFX is different. In CFX to activate the compressible solver you have to have a compressible fluid model chosen (such as ideal gas) and select the total energy equation option for heat transfer. If you select an incompressible material (eg constant density gas) or "thermal energy" heat transfer model you will be using the incompressible solver.

This occours at higher PR, when for example separations reach the outlet face (in my experience). You should switch to opening.

A better approach is to move the outlet boundary downstream so there is no reverse flow. Reverse flow at the outlet (whether it is an outlet or an opening) is harder to converge than one with no reverse flow.

Hello Everybody,

Thank you for trying to help me.

Now me Simulation is just running fine! It was the mesh indeed. I got a new one and now everything s fine!