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

question about immersed solid in CFX 12.0

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

Like Tree1Likes
  • 1 Post By stumpy

Reply
 
LinkBack Thread Tools Display Modes
Old   October 18, 2009, 21:21
Question question about immersed solid in CFX 12.0
  #1
New Member
 
Yu Fang
Join Date: Oct 2009
Posts: 8
Rep Power: 7
Anny is on a distinguished road
hi,everybody.My question is about immersed solid in ansys CFX 12.0.who has used it?And who knows its accuracy index?I use it to model a supercharger,but its result is far away with the test data. In my model, the inlet boundary is pressure inlet, it is set 0Pa,outlet boundary is 20kPa,it is same as test data,but the massflow rate of the compution is about half of the teat data.I don't konw why.I am suspicious of the CFX model is not suit for gas,it is only suit for liquid.
Anny is offline   Reply With Quote

Old   October 19, 2009, 05:55
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
I am suspicious of the CFX model is not suit for gas,it is only suit for liquid
Sounds like rubbish to me. What makes you say that?

The immersed solid feature will not work well if the mesh is not fine enough to resolve the motion and any cracks or gaps which are significant. For instance this means if you are trying to model the leakage in a Roots blower type supercharger you need a very fine mesh to have a few elements in the clearance between the rotors.

Are you sure your mesh is adequate?
ghorrocks is offline   Reply With Quote

Old   October 20, 2009, 20:31
Default
  #3
New Member
 
Yu Fang
Join Date: Oct 2009
Posts: 8
Rep Power: 7
Anny is on a distinguished road
I tired a refined mesh in the boundary of the immersed solid, but the result is same as before, not to be better.
Anny is offline   Reply With Quote

Old   October 20, 2009, 21:18
Default
  #4
New Member
 
Yu Fang
Join Date: Oct 2009
Posts: 8
Rep Power: 7
Anny is on a distinguished road
http://www.cfd-online.com/Forums/blo...1&d=1256091221
Here is the mesh picture.
http://www.cfd-online.com/Forums/att...1&d=1256091895
Here is the CCL file.

Last edited by Anny; October 20, 2009 at 22:26.
Anny is offline   Reply With Quote

Old   October 27, 2009, 17:01
Default
  #5
Senior Member
 
Join Date: Apr 2009
Posts: 517
Rep Power: 12
stumpy is on a distinguished road
Immersed Solid does not work with variable density + transient, so in that respect you are correct that it is not suitable for compressible gases in transient runs. Also the default settings can give too much "leakage" through the immersed solid. Under Solver Control try setting the "Momentum Source Scaling Factor" to 50 or 100 and also set the expert parameter "smooth inside ims = t" (required for stability with high Momentum Source Scaling Factors).
shanxuewenjdx likes this.
stumpy is offline   Reply With Quote

Old   November 2, 2009, 03:10
Default
  #6
New Member
 
Yu Fang
Join Date: Oct 2009
Posts: 8
Rep Power: 7
Anny is on a distinguished road
stumpy, Thanks for your reply, it's very useful to me, and I tired to do follow your advice. I trid setting the "Momentum Source Scaling Factor" to 50 or 100, 100 is not appropriate, 50 is OK. But where is the expert parameter "smooth inside ims = t"? I can't find it.
Anny is offline   Reply With Quote

Old   November 3, 2009, 18:42
Default
  #7
Senior Member
 
Join Date: Apr 2009
Posts: 517
Rep Power: 12
stumpy is on a distinguished road
If it's not in the GUI, then you'll have to type it in through the CCL. In the Command Editor you can type:

FLOW: Flow Analysis 1
EXPERT PARAMETERS:
smooth inside ims = t
END
END

I assume your case with the scaling factor set to 100 would have failed without this expert parameter set.
stumpy is offline   Reply With Quote

Old   November 3, 2009, 20:17
Default
  #8
New Member
 
Yu Fang
Join Date: Oct 2009
Posts: 8
Rep Power: 7
Anny is on a distinguished road
你说对了,你太厉害了,料事如神,我好佩服你啊
Anny is offline   Reply With Quote

Old   November 3, 2009, 20:24
Default
  #9
New Member
 
Yu Fang
Join Date: Oct 2009
Posts: 8
Rep Power: 7
Anny is on a distinguished road
English can't express my thanks fully., so I use my mother language Chinese. You are right, when I set to 100, it will tell me there is a error in CFX_solver manager. Thank you very much, you are the saviour to me.
Anny is offline   Reply With Quote

Old   May 25, 2012, 05:57
Default
  #10
New Member
 
belgacem
Join Date: Jan 2012
Posts: 22
Rep Power: 5
belgacem is on a distinguished road
Hi friend
I am also studying immersed boundary method and and try to simulate a block falling in the water. I am using "immersed solid" then rigid body 6DOF and I let it fall freely but it can't stoped in the bottom where the velocity must be zero. I give a density to the block and i let it fall freely under gravity. Noted that the rigid body is defined as an immersed solid. i have specified a stationary coordinate frame that has its origin at the center of mass of the physical rigid body. Another fixed coordinate frame was specified related to the water at rest.
What can I do to stopped the rigid body in the bottom where the potentiel energy must be zero?

thank you!
belgacem is offline   Reply With Quote

Old   April 6, 2013, 21:57
Default
  #11
New Member
 
Join Date: Jul 2012
Posts: 25
Rep Power: 5
yuanmengyuan1989 is on a distinguished road
Quote:
Originally Posted by stumpy View Post
If it's not in the GUI, then you'll have to type it in through the CCL. In the Command Editor you can type:

FLOW: Flow Analysis 1
EXPERT PARAMETERS:
smooth inside ims = t
END
END

I assume your case with the scaling factor set to 100 would have failed without this expert parameter set.

when i did as you said, i occoured an error :
ERROR #001100000 has occurred in subroutine EPORT_OBSOLETE_PRM. Message: The following unused Expert Solver Parameter was found: || SMOOTH INSIDE IMS | The parameter may be incorrectly spelled.
then i do not now how to do. what's up with it? do you konw? thank you!
yuanmengyuan1989 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
On Bug of Fluent 12.0 lzgwhy FLUENT 0 August 26, 2009 06:41
Question about the shock wave in CFX software nucharin Main CFD Forum 1 January 25, 2005 09:26
Conductig Solid question Peter CFX 0 February 18, 2002 12:15
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19
CFX Build 5 question... cfd guy CFX 6 June 19, 2001 22:38


All times are GMT -4. The time now is 19:38.