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

closed tank and dynamic mesh

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 1, 2013, 14:27
Default closed tank and dynamic mesh
  #1
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

I worked with rhoPimpleDyMFoam some times in non closed cases but now I have a closed volumina. Therefor I got "pcorr" step to 1000 iterations every time.

To check if this occure with closed volume cases I changed the tutorial case in the rhoPimpleDyMFoam so that there is no inlet and outlet anymore.

Its the same result. pcorr blows up:
Code:
solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 0.0152941 transformation: ((0 0 0) (0.981781 (0 0 0.190014)))
AMI: Creating addressing and weights between 10944 source faces and 10944 target faces
AMI: Patch source weights min/max/average = 0.945398, 1.00512, 0.999941
AMI: Patch target weights min/max/average = 0.951965, 1.00398, 0.999942
GAMG:  Solving for pcorr, Initial residual = 0.999999, Final residual = 20.8413, No Iterations 1000
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
Is there any solution?
Regards
Tobi


PS: @admin - if its possible the title can be changed into "closed volume and dynamic mesh"
Tobi is offline   Reply With Quote

Old   December 2, 2013, 07:30
Default
  #2
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

I tested my case yesterday again with a few outer faces used to be an atmosphere.

Therefor p is totalPressure and U is an pressureInletOutletVelocity. With this Addition the Simulation is running stable and fast.

pcorr is normal with a few iterations 5 - 20.


But I am still interested why pcorr blows up in closed volume cases.
Maybe I should have a look at the equations
Tobi is offline   Reply With Quote

Old   December 8, 2013, 04:25
Default
  #3
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,900
Rep Power: 37
ngj will become famous soon enoughngj will become famous soon enough
Hi Tobias,

It sounds to me, as if the compressibility of the fluid is not taken into consideration by the solver/pcorr loop. You probably changed the total volume of the box, and then pcorr has a problem in putting the excess volume somewhere.

A suggestion for checking this could be as follows:

1. Set up a simple cavity test.
2a. Move the left and right boundaries with the same velocity.
2b. Move the left and right boundaries with different velocities.

Case 2a should be successful, because the total volume remains constant, and 2b should fail.

Good luck,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   December 6, 2016, 10:11
Default
  #4
New Member
 
Join Date: Dec 2013
Posts: 11
Rep Power: 12
Ricky-11 is on a distinguished road
Hey Tobi.

I'm also dealing with a closed domain with moving boundaries. Although my model doesn't blow up, the iterations in the pcorr step are always a lot slowing down terribly the simulations.

In your (or others opinion), should a reduced level of convergence for pcorr deteriorate the accuracy of results or can we live with it?

Thanks,

R
Ricky-11 is offline   Reply With Quote

Old   December 10, 2016, 20:38
Default
  #5
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
I cannot give you any advice but you can check out - or set - the keyword that calculates the pressure correction for closed volumes. You have to add the keyword in the fvSolution file (not sure, check out the sources yourself).

Sent from my HTC One mini using CFD Online Forum mobile app
__________________
Keep foaming,
Tobias Holzmann

Last edited by Tobi; December 26, 2016 at 06:25.
Tobi is offline   Reply With Quote

Old   December 16, 2016, 16:51
Default
  #6
otm
New Member
 
Join Date: Jun 2009
Posts: 22
Rep Power: 16
otm is on a distinguished road
Hi,
Have you set a pRef and pRefpoint somewhere in your domain? I can't see that it should be necessary with a compressible solver though.


Sent from my iPhone using CFD Online Forum mobile app
otm is offline   Reply With Quote

Old   March 27, 2018, 04:26
Default
  #7
New Member
 
MichG
Join Date: Nov 2017
Posts: 6
Rep Power: 8
MichG is on a distinguished road
Hello Tobias,

I also want to simulate a closed volume stirred tank using the solver rhoPimpleDyMFoam. Im simulating an incompressible fluid, but need the compressible version of the solver for the heat transfer simulation. As you described, the simulation runs only with one patch defined as inletOutlet. My problem is now, because its an inlet, I get a flow in and out of the domain, but I want the domain to be closed.

I defined my BC as follow:
U
Code:
    oben
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
p
Code:
    oben
    {
        type            totalPressure;
        p0              $internalField;
        U               U;
        phi             phi;
        rho             rho;
        psi             none;
        gamma           1;
        value           $internalField;
    }
Do you know how to define the patch, that I dont get a mass flow in and out of the domain with still getting a stable simulation?

Kind regards
Michael
MichG is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Dynamic Mesh (Wave Generation in a Tank) mu ke FLUENT 2 September 16, 2015 03:35
Wave tank dynamic mesh Doro FLUENT 0 October 27, 2011 05:39
dynamic mesh Streamboy FLUENT 1 June 21, 2011 18:03
dynamic mesh interDyMFoam parallel run and processor boundaries lukasfischer OpenFOAM Running, Solving & CFD 0 August 12, 2009 07:36
dynamic mesh and udf problem boboroo FLUENT 1 January 20, 2008 22:26


All times are GMT -4. The time now is 05:38.