CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Compressor Simulation in Star CCM+ (http://www.cfd-online.com/Forums/star-ccm/85383-compressor-simulation-star-ccm.html)

chili023 February 24, 2011 07:51

Compressor Simulation in Star CCM+
 
He guys.
First of all I am a native ANSYS CFX 12 User, and just switched to Star CCM+.
For now I like the way Starccm+ meshes the geometry way easier, an stable.
However
I set up a simple simulation of a centrifugal compressor.
Here the specs
steady
ideal Gas
K-Epsilon Turbulence
K-Epsilon two layer
segregated flow
Two Layer All y+ Wall Treatment
My mesh has a good quality and two prism layers with a 1.5 groth.
However
Ansys was able to calculate the simulations at any rpm and massflow i wanted.
Star CCM+ cannot even calculate it without rotation. I always get a point overflow. I read a lot about getting simulations in CCm to convergence but I do not see the need for a ramp in a steady state simulation.
I do CFD for 5 years but i never saw a program so difficult to get started.
Please tell me what am I doing wrong.

JBeilke February 24, 2011 12:06

Assuming you are using a massflow-BC just start with 1/10 or 1/100 of the original value for the first 10 Iterations.

chili023 February 24, 2011 12:36

Already did that!
But thx

Vinicius February 24, 2011 14:12

What are the values for the initial conditions you are using?

chili023 February 28, 2011 10:30

none
Stationary simulation.

Thx

Vinicius February 28, 2011 10:40

But in the initial conditions node, those values are used to make a initial guess of the solution.
There you can choose better values for your case and the solution might converge with them...

Also, check out your mesh quality and sizes... you can take a look at this guideline:

http://www.cfd-online.com/Wiki/Best_...omachinery_CFD

Regards,

Amelie March 3, 2011 14:20

Have you tried grid sequencing - expert initialization node in the coupled implicit solver?

chili023 March 4, 2011 12:10

coupled flow. hmmm you mean just to get it started, don't u?I would prefer to use segregated for my simulation.I will try that.Thx

chili023 March 7, 2011 11:50

The simulation started with coupled flow. So thx Amelie However I discovered something interesting. I did add a inlet and outlet run. Just by doing this I was able to start the simulation with segregated Flow. The segregated solves seames to be quite sensible to ununiform outflow vectors.So THX to everyone

chili023 March 8, 2011 12:30

One more thing.
The segregated solver is very sensitive to bad cell quality and orientation. So always check this in a scalar field.

chili023 March 11, 2011 07:15

Another thing.

I was able to get convergence with no initial conditions and no ramp by using a mass flow outlet and a pressure inlet.

Looks like this bc are very robust.

layth August 3, 2011 10:15

how we can export an
 
hello

i have problem with turbo wizard star ccm+ we need to import the external file .but can not create .esgt format .

could any one help me thanks

regards

abdul099 August 7, 2011 15:46

Quote:

Originally Posted by Amelie (Post 297828)
Have you tried grid sequencing - expert initialization node in the coupled implicit solver?

Grid sequencing is mainly designed for external aero simulations. You might get a lot of problems when using it for small enclosed volumes.

Quote:

Originally Posted by chili023 (Post 296700)
I do not see the need for a ramp in a steady state simulation. I do CFD for 5 years but i never saw a program so difficult to get started.

Should I translate it to my language?
I want to fly. But it doesn't work, as I try to fly with a car. I don't see the need for using an airplane for a flight below flight level 100. I'm flying planes since 5 years, but I never saw a car so difficult to get airborne...

Translated back to your language: Don't try to copy what you did with CFX to another program and expect the same result. Try to understand what's wrong:
The segregated solver struggles to get a solution when initializing with zero velocity and no boundary condition prescribes any flow direction. That's why using pressure - pressure BC usually doesn't work, but velocity -pressure or mass flow - pressure (which implies a flow direction normal to the boundary surface) does work. When pressure - pressure BC are essentially needed, it's best to start with let's say velocity - pressure and switch to pressure - pressure after some iterations / time steps when an initial flow field is established.

ping August 11, 2011 02:22

also I note you are using ideal gas - always harder to get going in steady solver cases, but much more stable if you ramp the under-relaxation factors for pressure and velocity - say start at 1/10th normal values and ramp for 100 iterations. This might solve all your issues!
Also don't waste your time and computer resources with tet volume cells - polys are 5+ times faster for same accuracy.


All times are GMT -4. The time now is 13:48.