CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

TurbDyMFoam for dummies

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 29, 2008, 05:50
Default Hi everybody and happy 2009 I
  #1
Member
 
antonio segalini
Join Date: Mar 2009
Posts: 75
Rep Power: 8
antonio_ing is on a distinguished road
Hi everybody and happy 2009
I have started today working with a darrieus VAWT geometry. I did a first simulation without any rotation with simpleFoam but now I have to add the rotation of the profiles. Since the vortices will interact in a unsteady way, i guess that the best solver should be turbDyMFoam, but i have no experience with this solver (or equivalently icoDyMFoam).
Can anyone give me some details?

thanks in advance
antonio_ing is offline   Reply With Quote

Old   January 7, 2009, 04:01
Default can anyone give me some help?
  #2
Member
 
antonio segalini
Join Date: Mar 2009
Posts: 75
Rep Power: 8
antonio_ing is on a distinguished road
can anyone give me some help?
antonio_ing is offline   Reply With Quote

Old   March 22, 2010, 19:04
Default Help on turbDyMFoam
  #3
New Member
 
Mauro Parodi
Join Date: Mar 2010
Location: Torino
Posts: 4
Rep Power: 7
mparodi is on a distinguished road
Hi Antonio,

did you manage to get some basic material on turbDyMFoam?

I am also trying to set up a case, but without success.

Mauro.
mparodi is offline   Reply With Quote

Old   April 30, 2010, 09:29
Default
  #4
Member
 
Nick Gardiner
Join Date: Apr 2009
Location: Chichester, UK
Posts: 93
Rep Power: 8
NickG is on a distinguished road
Hi

This is what I do starting from separate inner and outer meshses:

-> mergeMeshes /home/nick/OpenFOAM/nick-1.5-dev/Turbine/2degGgi/ 600mm2degTunnel /home/nick/OpenFOAM/nick-1.5-dev/Turbine/2degGgi/ 600mm2degRotor
[That has 4 arguments: master root ; master case; slave root; slave case]

To set up case from combined mesh in new folder:

copy to new case folder from tutorials/IcoDyMFoam/mixerGgi: 0, constant, system

replace /constant/polymesh with mergeMeshes polymesh (inside the folder named from the value of your timestep in mergeMeshes controlDict)

change type for inside and outside sliding interface to ggi and paste underneath startFace:

shadowPatch outsideSlider;
zone insideZone;
bridgeOverlap false;

for insideSlider and:

shadowPatch insideSlider;
zone outsideZone;
bridgeOverlap false;

for outsideSlider. Your sliding faces maybe named differently so replace insideSlider and outsideSlider accordingly. e.g. mine read:

InterT
{
type ggi;
nFaces 180;
startFace 7782;
shadowPatch InterR;
zone outsideZone;
bridgeOverlap off; //relates to consistency of mesh size across interface: can be true, false, on, off
}
InterR
{
type ggi;
nFaces 180;
startFace 15482;
shadowPatch InterT;
zone insideZone;
bridgeOverlap off;
}

change names of slider moving and static arguments in dynamicMeshDict to correspond to your interface boundary names (e.g. from insideSlider to InterR for my case)
change rpm and coordinateSystem if necessary.

write k, epsilon, etc. depending upon turbulence model. Use example from turbFoam as an example for interface patches: type ggi; e.g. from my k file:

InterT
{
type ggi;
value uniform 25; // you don't need to include this line
}

[if you want to run in parallel: add to decomposeParDict: globalFaceZones ( insideZone outsideZone );]

write "setBatch" file: faceSet insideZone new patchToFace InterR
faceSet outsideZone new patchToFace InterT
quit
place in case folder

-> setSet -batch setBatch

-> setsToZones -noFlipMap

-> turbDyMFoam

Hopefully it runs!
NickG is offline   Reply With Quote

Old   May 3, 2010, 15:13
Default Working!
  #5
New Member
 
Mauro Parodi
Join Date: Mar 2010
Location: Torino
Posts: 4
Rep Power: 7
mparodi is on a distinguished road
Hi Nick,

I really appreciate your help .

The model looks to be running now!

Many Thanks,

Mauro.
mparodi is offline   Reply With Quote

Old   September 24, 2010, 07:10
Default
  #6
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 155
Rep Power: 6
lordvon is on a distinguished road
You did not have to replace the fvsolution or fvscheme files under /system/ in the icoDyMFoam tutroial?
lordvon is offline   Reply With Quote

Old   September 24, 2010, 08:16
Default
  #7
Member
 
Nick Gardiner
Join Date: Apr 2009
Location: Chichester, UK
Posts: 93
Rep Power: 8
NickG is on a distinguished road
If you're using turbDyMFoam but starting from IcoDyMFoam then you need equations for the turbulence. Check fvsolution or fvschemes in turbFoam tutorial for examples
NickG 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
TurbDyMFoam Application jdkummer OpenFOAM Installation 2 November 24, 2011 09:14
Time Step problem with turbDyMFoam yuhai OpenFOAM Running, Solving & CFD 1 March 3, 2009 06:42
TurbDyMFoam Unknown dynamicFvMesh type mixerFvMesh david OpenFOAM Running, Solving & CFD 11 February 16, 2009 17:30
ExtrudeMesh for Dummies wolle1982 OpenFOAM Mesh Utilities 2 October 28, 2008 11:35
SnappyHexMesh vs turbDyMFoam young OpenFOAM Running, Solving & CFD 0 October 16, 2008 10:21


All times are GMT -4. The time now is 11:29.