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. |
Assuming you are using a massflow-BC just start with 1/10 or 1/100 of the original value for the first 10 Iterations.
|
Already did that!
But thx |
What are the values for the initial conditions you are using?
|
none
Stationary simulation. Thx |
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, |
Have you tried grid sequencing - expert initialization node in the coupled implicit solver?
|
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
|
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
|
One more thing.
The segregated solver is very sensitive to bad cell quality and orientation. So always check this in a scalar field. |
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. |
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 |
Quote:
Quote:
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. |
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 22:00. |