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

heat transfer, multiple regions, chtMultiRegionFoam?

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

Like Tree1Likes
  • 1 Post By Ohlzen-Wendy

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 24, 2015, 04:04
Question heat transfer, multiple regions, chtMultiRegionFoam?
  #1
New Member
 
Join Date: Jun 2015
Posts: 12
Rep Power: 7
Ohlzen-Wendy is on a distinguished road
Hi everybody,

I am searching for a solution for a calclation of the Scenario showing in the attachment.
we have following Situation:
a small Region produces heat and the heat is transfered into a fluid in a chamber (air without any velocity). a other part of the heat is transfered through different solid materials (e.g. aluminum and steel) into a cooling element. the cooling element is positioned in a Kind of pipe where air is flowing with a given Temperature and Speed.

I think this should be possible to solve with the solver chtMultiRegionFoam but I have several Problems:

The geometry is far more complex then shown. I want to use the program ANSA for creating the mesh of the Case. But how can I create a case with several regions like I Need for chtMultiRegionFoam?
- create every part on its own and merge them afterwards?

If I create the mesh in one case, how can I create the regians afterwards?

Is chtMultiRegionFoam the correct solver for my Problem. I think so but I am not sure.

Has anyone had a similar Problem before? I would be glad if I could get some help.


Best wishes

Andreas
Attached Images
File Type: jpg skizze.jpg (19.4 KB, 279 views)
Kummi likes this.
Ohlzen-Wendy is offline   Reply With Quote

Old   June 24, 2015, 04:17
Default
  #2
Senior Member
 
Laurent DASTUGUE
Join Date: May 2014
Location: Chartres, France
Posts: 119
Rep Power: 8
laurentD is on a distinguished road
Hi Andreas,

i often work with the 'chtMutiRegionFoam' utility, but i don't use ANSA for the mesh.
Otherwise, i think the method is the same.
First i do a complete mesh with my meshing tool. Then for all materials i add boundaries (skins) and labels. OpenFOAM is able to read these labels.
Secondly i transfer the mesh files to OpenFOAM separately.
For example in a model with fluid and solid, i transfer the fluid files, i build the directory related to this fluid (constant/fluid/polymesh, system/fluid, 0/fluid) and after that, i do the same with the solid mesh.
I hope this can help you, it is not simple to explain.

Have a good day,
Laurent
laurentD is offline   Reply With Quote

Old   June 24, 2015, 04:32
Default
  #3
New Member
 
Join Date: Jun 2015
Posts: 12
Rep Power: 7
Ohlzen-Wendy is on a distinguished road
Hi Laurent,

so I create a mesh in e.g. ANSA. Export the mesh, boundaries etc. of each submesh seperately and copy them manualy with the case structure as shown in the attachment?

do I have to run some other utilities like setSet etc. afterwards?
maybe you can upload something like the allrun script You usaly use?

best wishes and thank you so far

Andreas
Attached Images
File Type: jpg OF_Structure.jpg (20.3 KB, 138 views)
Ohlzen-Wendy is offline   Reply With Quote

Old   June 24, 2015, 05:16
Default
  #4
Senior Member
 
Laurent DASTUGUE
Join Date: May 2014
Location: Chartres, France
Posts: 119
Rep Power: 8
laurentD is on a distinguished road
My allrun is useless because i use another mesh utility so i have to use others tools to convert the mesh to OpenFOAM.
But i have read looked for informations related to ANSA and it seems that ANSA can directly provide the polymesh directory.
So if you have the polymesh directory for each 'materials' (like in your tree) it should work.
To verify each part of the mesh, move the polymesh of a material uner constant/ and do the checkMesh command from the work directory (the root one). After this verification think to move again the polymesh directory to put it on the right place.
Laurent
laurentD is offline   Reply With Quote

Old   July 1, 2015, 02:46
Default
  #5
New Member
 
Join Date: Jun 2015
Posts: 12
Rep Power: 7
Ohlzen-Wendy is on a distinguished road
hi everybody,

had some other Projects to work on but spent the last day on openFOAM.
So far I managed to Export the whole mesh from ansa and using the "splitMeshRegions -cellZones -overwrite" command to create my regions for fluids and solids.
I modified also the regions setting and solvers. But I still have some questions.

what Kind of BCs do I have to use on the patches between the regions. if it is a fluid to a wall i use the common wall BCs to pressure and velocity etc. but if i have a patch between 2 solids?
splitMeshRegions also created patches for "both sides" ("wall1_to_wall2" and "wall2_to_wall1"). do I have to use the some bcs on each side?

baffles:
What are they for? I want to have a constant heat flux (W/m³ or total W) from one solid. how can I include this? I Need the baffles for this or?

I know a lot of questions but somehow I have not found any satisfying Information.

best wishes


Andy
Ohlzen-Wendy is offline   Reply With Quote

Old   July 1, 2015, 07:37
Default
  #6
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 17
zfaraday will become famous soon enough
Hello!

Quick answer.

As for the coupling between regions for temperature, take a look at these BC's:
Regarding the volumetric heeat generation, take a look at this thread:
how-i-can-introduce-my-power-heat-w-chtmultiregionfoam.html

Hope it helps.

Best regards,

Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   July 2, 2015, 10:38
Default
  #7
New Member
 
Join Date: Jun 2015
Posts: 12
Rep Power: 7
Ohlzen-Wendy is on a distinguished road
Hi everybody,

I make some progress regarding my calculation. therefore I set up a small test case. (
This one is running but I still have some questions I am not totally sure about.

If i introduce a heat transfer with a fixed power or flux on a patch between a fluid and a solid or a solid and a other solid - do i have to set the bc on both patches?

while chtMultiRegionFoam is running after some time the time step is decreased to something like 1e-13s. is there a way to track the maximum magnitude speed of the whole domain while the simulation is running?

best wishes

Andy
Ohlzen-Wendy is offline   Reply With Quote

Old   July 2, 2015, 11:57
Default Boundary Conditions
  #8
New Member
 
Bruce Clarke
Join Date: Jul 2015
Posts: 3
Rep Power: 7
BClarke352 is on a distinguished road
Hi,

I'm also having trouble with some boundary conditions - I have a pipe with fluid in that has a velocity of 1 metre per second, inside a steel block. I've set the fluid and solid regions using topoSet but I'm having trouble with my temperature, velocity and pressure fields. For some reason, velocity and pressure aren't restricted to the fluid region. Does anyone know why this might be happening? Should there be something that I change in changeDictionaryDict to prevent this from happening. Also, I'm trying to make one of the faces of the steel block hotter so it causes the pipe to heat unevenly. However, it doesn't appear to be having any effect despite paraFoam clearly showing me one face that is hotter than the rest.

Any help anyone can give me would be much appreciated!
BClarke352 is offline   Reply With Quote

Old   July 2, 2015, 13:06
Default
  #9
Member
 
VA
Join Date: Mar 2015
Location: ON, Canada
Posts: 30
Rep Power: 7
vabishek is on a distinguished road
Quote:
Originally Posted by BClarke352 View Post
Hi,

I'm also having trouble with some boundary conditions - I have a pipe with fluid in that has a velocity of 1 metre per second, inside a steel block. I've set the fluid and solid regions using topoSet but I'm having trouble with my temperature, velocity and pressure fields. For some reason, velocity and pressure aren't restricted to the fluid region. Does anyone know why this might be happening? Should there be something that I change in changeDictionaryDict to prevent this from happening. Also, I'm trying to make one of the faces of the steel block hotter so it causes the pipe to heat unevenly. However, it doesn't appear to be having any effect despite paraFoam clearly showing me one face that is hotter than the rest.

Any help anyone can give me would be much appreciated!
Hello Bruce,

It is hard to say what could be going wrong in your case without taking a look at the case files. It would make it a lot easier if you could attach a test case.

Based on the info you have provided, I think the issue might be with the "regionProperties" file in the constant/ directory. If the regions are not specified correctly in that file, it could lead to a situation where the fluid equations are solved in the solid region and vice versa. Check that file to make sure everything is correct.

I hope that helps!
vabishek is offline   Reply With Quote

Old   July 3, 2015, 00:54
Default
  #10
New Member
 
Join Date: Jun 2015
Posts: 12
Rep Power: 7
Ohlzen-Wendy is on a distinguished road
Quote:
Originally Posted by Ohlzen-Wendy View Post
Hi everybody,

I make some progress regarding my calculation. therefore I set up a small test case. (
This one is running but I still have some questions I am not totally sure about.

If i introduce a heat transfer with a fixed power or flux on a patch between a fluid and a solid or a solid and a other solid - do i have to set the bc on both patches?

while chtMultiRegionFoam is running after some time the time step is decreased to something like 1e-13s. is there a way to track the maximum magnitude speed of the whole domain while the simulation is running?

best wishes

Andy
The case files for the OF-Case you find here:
https://drive.google.com/file/d/0B_I...ew?usp=sharing
Ohlzen-Wendy is offline   Reply With Quote

Old   June 12, 2018, 15:15
Default high energy residuals in cht multi region simple foam
  #11
New Member
 
elham usefi
Join Date: Apr 2016
Location: tabriz,iran
Posts: 13
Rep Power: 6
elham usefi is on a distinguished road
Hi everybody. I am simulating a heat transfer problem with the modified chtMultiRegionSimpleFoam solver in which the fluid region is incompressible with force convection (modified) and the solid region is the same as original chtMRSF. When I simulate the fluid region alone with a fixed value or fixed gradient B.C. for temperature with buoyant bousinesqBoussinesqSimpleFoam I get sensible results with all the residuals under e-8. And the same goes for solid region only. But when I solve fluid and solid together with my modified solver and a “turbulent temperature coupled baffle mixed” B.C for temperature in the solid-fluid interface, energy residuals for fluid and solid cannot decrease less than e-4 and e-3, but still the results look sensible! I have tried different schemes and solvers and iteration numbers, but no progress. I guess the thing is with “turbulent temperature coupled baffle mixed” B.C but I can’t understand it well!
Another thing that I’ve found out is that when I increase the solid conductivity or decrease the fluid conductivity, the energy residuals for fluid decreases to e-6! but nothing happens for energy residuals for solid region! On the other hand, when I use an unsteady version of my solver, energy residuals decrease to e-5! Then the problem should be with laplacian term in fluid energy equation but I have tried every scheme! And I need to use the transient solver.
elham usefi is offline   Reply With Quote

Old   July 2, 2018, 09:13
Default
  #12
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 17
vangelis is on a distinguished road
Hi there
Just to mention that the latest ANSA v18.1.x supports the output of CHT openfoam cases. The user must create different Material and assign it to the corresponding volume properties. In this way ANSA will now how to output mesh for each fluid or solid zone.

Then the user should also set mappedwall boundary conditions on the surfaces between the different materials
vangelis is offline   Reply With Quote

Old   July 3, 2020, 00:15
Default
  #13
New Member
 
Fluid Tool Engineering
Join Date: Jul 2019
Location: Ho Chi Minh City
Posts: 10
Rep Power: 3
Fluid Tool is on a distinguished road
Quote:
Originally Posted by zfaraday View Post
Hello!

Quick answer.

As for the coupling between regions for temperature, take a look at these BC's:
Regarding the volumetric heeat generation, take a look at this thread:
how-i-can-introduce-my-power-heat-w-chtmultiregionfoam.html

Hope it helps.

Best regards,

Alex
Hi Alex,

It was old topic but I want ask problem at heat flux on baffle between fluid and solid. I want to set heat flux on this face but it will not couple 2 volumes. is there way to set heat flux on coupling between regions?

Thanks
Fluid Tool is offline   Reply With Quote

Reply

Tags
ansa, chtmultiregionfoam, cooling, multiphase, thermal

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
Radiation interface hinca CFX 15 January 26, 2014 17:11
Heat Transfer mechanisms tafaugl CFX 1 November 7, 2012 18:46
chtMultiRegionFoam: heat transfer coefficient between solids brent OpenFOAM Running, Solving & CFD 0 November 1, 2012 08:22
Multiregion Heat Transfer + natural convection (water) with chtMultiRegionFoam fattychickenrun OpenFOAM 5 October 31, 2011 16:53
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 15:55


All times are GMT -4. The time now is 04:04.