CFX convergence problem simulating ogive-cylinders at varied angle of attack
 

Hello all,

I am trying to simulate free shear flow past an ogive cylinder shape (length of 3m, dia 0.25m) in ANSYS CFX and am running into a problem as I change the angle of attack. The ogive cylinder is contained within a cylindrical control volume (length 10m, rad. 3m) with the following domains/boundary conditions:

1. The default fluid domain is set to air ideal gas with a static pressure of 25000. The total energy option is selected and viscous work term is included. The CFX documentation recommends these settings for a compressible flow. The turbulence model used is the Shear Stress Transport option
2. A supersonic Inlet at one end of the cylinder is defined with a normal velocity of Mach 2 based on a static temperature of 288.15K. The relative static pressure is 0Pa and the turbulence option is set to medium (5%)
3. A supersonic Outlet is set at the opposite end of the cylinder
4. The outer limit of the control volume is set as a Free slip wall
5. The ogive cylinder surface is defined as a No slip wall

I usually monitor the convergence of Drag, Lift and Pitching moment coefficients by use of expressions as I have wind tunnel data to compare to. This setup has worked for an ogive cylinder angle of attack ranging from 0 to 15 degrees. However when I try to simulate an angle of attack of 30 deg, the run fails within the first couple of iterations with the message:

+--------------------------------------------------------------------+
| ****** Notice ****** |
| The non-dimensional near wall temperature (T+) has been clipped |
| for calculation of Wall Heat Transfer Coefficient. |
| |
| Boundary Condition : OCylinder |
| T+ clip value = 1.0000E-10 |
| |
| If this situation persists and you are using the High Speed Model, |
| consider enabling Mach number based blending between low speed and |
| high speed wall functions. You can do so by specifying a Mach |
| number threshold as follows: |
| |
| EXPERT PARAMETERS: |
| highspeed wf mach threshold = 0.1 # default=0.0 (off) |
| END |
+--------------------------------------------------------------------+

Things I have tried to solve this problem:

1. The expert parameter above does not exist in the sense that I can check a box and alter a value. I have tried (successfully) adding it via command editor but this does not improve the ability of CFX to solve this case
2. I have reduced the timescale factor to as low as 0.01 in the Solver Control box but this has the added effect of slowing convergence and the simulation fails before the coefficients of interest reach their steady state values
3. I have set the maximum Timescale in the Solver Control box to an appropriate temporal scale (10m / 680 m/s = 0.015) but this has not helped

I use ICEM mesh generation and hence have a mesh for each angle of attack. All meshes have the same sized elements placed for shock and wake resolution; and prism layers for capturing the boundary layer. All meshes also pass the ICEM quality checks.

I have reached the limits of my own understanding and am interested to know if anyone else has been able to overcome similar problems or has some ideas as to how I should proceed...

I assume this is a steady state run. Are you hammer starting this solution or using previous solution as a starting point?

Either way, I have found that if I baby step the Timescale Factor (it defaults to 1) up from a very small scale to 1 over some period of iterations, your solution converge easier. This is particularly the case for high mach and angle of attack runs.

As an example I use the following expression for timest:

step(10.5-aitern)*0.001+step(20.5-aitern)*step(aitern-10.5)*.005+step(30.5-aitern)*step(aitern-20.5)*.03+step(40.5-aitern)*step(aitern-30.5)*.08+step(50.5-aitern)*step(aitern-40.5)*.4+step(aitern-50.5)*1

This will step timest up from 0.001 to 1 over 50 iterations (you can adjust as you see fit).

Edit: Sorry, just noticed you have adjusted the timescale factor. In the past, I have found that 0.01 might not be low enough to ease into a stable solution. If you interpolate a "close" previous result, you might be able to get away with a larger timescale factor. Try lowering timescale and easing it up.

Then use timest in the Timescale Factor under the Solver Control Tab.

I hope this helps.

Ed

Try starting the run using local time scale factor, a value of 5.0 should be OK to start. Once the flow is converging switch back to physical time scale.

Also, rather than using Edmund's CEL function you can do this manually with "Edit run in progress". Depends on whether you want to automate it or keep manual control, up to you.

Ed:
Your assumption is correct, the simulation is steady state and I am trying to hammer start it. Thanks for the stepping algorithm. I'll give it a shot anyway seeing as it starts off an order of magnitude lower than I've run it previously

Glenn:
I'll give the local timescale factor a shot as well. At the moment I run several cases via a batch script and use CFX just to create the '.cfx' and '.def' files so an automated CEL function is ideal.

Thanks both for your suggestions, I'll let you know how they work out.

Oh yes, and another thing - for high mach number flows a good initial guess is very useful. Try doing a model at a lower velocity, subsonic if you have to. No need to converge it fully, just enough to get a reasonable flow field for the initial condition for the full speed run.

Alternately you can ramp the inlet speed up using a function like Edmund recommended for the time step size (or manually do it through the edit run in progress)

I have had some success with the stepping algorithms and usually employ them for both timest and the inlet velocity.

Thanks a heap for your help.

Hi,

I dont know how to insert these expression in CFX, can u please help me. I know to write expression to evaluate properties in post processing but dont know where to write in solver.

thank you