Compressor Simulation in Star CCM+

chili023 · February 24, 2011, 07:51

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, 11:15

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, 16:46

Quote:

Originally Posted by Amelie

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

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, 03:22

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.

February 24, 2011, 07:51	Compressor Simulation in Star CCM+	#1
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	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.

August 3, 2011, 11:15	how we can export an	#12
layth New Member layth Join Date: Apr 2011 Posts: 10 Rep Power: 15	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[Commercial meshers] Using starToFoam	clo	OpenFOAM Meshing & Mesh Conversion	33	September 26, 2012 05:04
[Other] StarToFoam error	Kart	OpenFOAM Meshing & Mesh Conversion	1	February 4, 2010 05:38
A genearl question on STAR CCM	nstar	STAR-CCM+	5	June 24, 2009 10:39
error in star ccm	maurizio	Siemens	3	October 16, 2007 06:17
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues	michele	OpenFOAM Meshing & Mesh Conversion	2	July 15, 2005 05:15

February 24, 2011, 12:06		#2
JBeilke Senior Member Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 533 Rep Power: 20	Assuming you are using a massflow-BC just start with 1/10 or 1/100 of the original value for the first 10 Iterations.

February 24, 2011, 12:36		#3
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	Already did that! But thx

February 24, 2011, 14:12		#4
Vinicius Member Vinicius Girardi Join Date: Mar 2009 Location: Sao Paulo, Brazil Posts: 80 Rep Power: 17	What are the values for the initial conditions you are using?

February 28, 2011, 10:30		#5
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	none Stationary simulation. Thx

February 28, 2011, 10:40		#6
Vinicius Member Vinicius Girardi Join Date: Mar 2009 Location: Sao Paulo, Brazil Posts: 80 Rep Power: 17	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,

March 3, 2011, 14:20		#7
Amelie New Member Join Date: Dec 2010 Posts: 1 Rep Power: 0	Have you tried grid sequencing - expert initialization node in the coupled implicit solver?

March 4, 2011, 12:10		#8
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	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

March 7, 2011, 11:50		#9
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	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

March 8, 2011, 12:30		#10
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	One more thing. The segregated solver is very sensitive to bad cell quality and orientation. So always check this in a scalar field.

March 11, 2011, 07:15		#11
chili023 New Member AB Join Date: Jun 2010 Posts: 21 Rep Power: 16	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.

August 11, 2011, 03:22		#14
ping Senior Member Ping Join Date: Mar 2009 Posts: 556 Rep Power: 20	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.