Appropriate turbulent model
 

Hi, I am simulating a converging-diverging nozzle, with a compressible flow, and Re=50,000 - 75,000. It suffers an adverse pressure gradient. It is told to me that a K-E high reynold no. model wont work for this type of flow. What is the appropriate turbulent model? K-W can be a choice, but is not offered by Star-CD? Do reply, thanks in advance Ashish

Re: Appropriate turbulent model
 

The k-w model is available (in v3.15 onwards, albeit a beta feature). You just have to turn on the appropriate switches and constants. You can find the instructions in the Supplementary Notes but for your convenience:

1. Select the low Reynolds number k-e model in the Turbulence Models panel. 2. Write the geometry file using command GEOM or an equivalent GUI operation. 3. Select the high Reynolds number k-e model in the Turbulence Models panel. 4. Set Constant 88 to 3 using command RCON 88 3. 5. Write the problem file using command PROB or an equivalent GUI operation. Ignore any warnings about file parm.new. This file can be deleted. 6. For a STAR-HPC analysis, the geometry decomposition process will create .bshl files in each sub-domain subdirectory. These files may be deleted.

The above steps actually activate the _high_-Reynolds form of the 'standard' k-w model although you have chosen the low-Reynolds k-e model options in GUIde.

Re: Appropriate turbulent model
 

try to use the qubic - k-eps modell. it should work fine as well. from my experience you should use the two -layer version.

regards, thomas