CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Compressor Simulation in Star CCM+

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 24, 2011, 07:51
Default Compressor Simulation in Star CCM+
  #1
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
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.
chili023 is offline   Reply With Quote

Old   February 24, 2011, 12:06
Default
  #2
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 185
Rep Power: 9
JBeilke is on a distinguished road
Assuming you are using a massflow-BC just start with 1/10 or 1/100 of the original value for the first 10 Iterations.
JBeilke is offline   Reply With Quote

Old   February 24, 2011, 12:36
Default
  #3
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
Already did that!
But thx
chili023 is offline   Reply With Quote

Old   February 24, 2011, 14:12
Default
  #4
Member
 
Vinicius Girardi
Join Date: Mar 2009
Location: Sao Paulo, Brazil
Posts: 80
Rep Power: 8
Vinicius is on a distinguished road
What are the values for the initial conditions you are using?
Vinicius is offline   Reply With Quote

Old   February 28, 2011, 10:30
Default
  #5
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
none
Stationary simulation.

Thx
chili023 is offline   Reply With Quote

Old   February 28, 2011, 10:40
Default
  #6
Member
 
Vinicius Girardi
Join Date: Mar 2009
Location: Sao Paulo, Brazil
Posts: 80
Rep Power: 8
Vinicius is on a distinguished road
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,
Vinicius is offline   Reply With Quote

Old   March 3, 2011, 14:20
Default
  #7
New Member
 
Join Date: Dec 2010
Posts: 1
Rep Power: 0
Amelie is on a distinguished road
Have you tried grid sequencing - expert initialization node in the coupled implicit solver?
Amelie is offline   Reply With Quote

Old   March 4, 2011, 12:10
Default
  #8
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
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 is offline   Reply With Quote

Old   March 7, 2011, 11:50
Default
  #9
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
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 is offline   Reply With Quote

Old   March 8, 2011, 12:30
Default
  #10
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
One more thing.
The segregated solver is very sensitive to bad cell quality and orientation. So always check this in a scalar field.
chili023 is offline   Reply With Quote

Old   March 11, 2011, 07:15
Default
  #11
New Member
 
AB
Join Date: Jun 2010
Posts: 21
Rep Power: 7
chili023 is on a distinguished road
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.
chili023 is offline   Reply With Quote

Old   August 3, 2011, 10:15
Default how we can export an
  #12
New Member
 
layth
Join Date: Apr 2011
Posts: 10
Rep Power: 6
layth is on a distinguished road
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
layth is offline   Reply With Quote

Old   August 7, 2011, 15:46
Default
  #13
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Quote:
Originally Posted by Amelie View Post
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 View Post
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.
abdul099 is offline   Reply With Quote

Old   August 11, 2011, 02:22
Default
  #14
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 223
Rep Power: 9
ping is on a distinguished road
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.
ping is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Using starToFoam clo OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 33 September 26, 2012 04:04
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 09:39
error in star ccm maurizio CD-adapco 3 October 16, 2007 05:17
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 07:46.