CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > FloEFD, FloWorks & FloTHERM

Heat Source deactivating Heat Conduction on solids

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 17, 2017, 23:37
Default Heat Source deactivating Heat Conduction on solids
  #1
New Member
 
RJ Carbs
Join Date: May 2017
Posts: 6
Rep Power: 6
rjcarbs is on a distinguished road
I am working on a CFD cooling analysis of a Dome structure. I want to input the heat load using surface heat source feature hence "Heat Conduction on Solids" should be activated. When activated, it will result in a unrealistic outcome, "Solid is Melting" when I run the simulation. It wont work on this set-up. This is an internal analysis.
The solid structure is supposed to be just a dummy solid because I am not concerned on the heat transfer of the walls. The heat load on human and solar load is already calculated, and will be input directly. Is there any workaround on this?
rjcarbs is offline   Reply With Quote

Old   May 18, 2017, 21:32
Default
  #2
New Member
 
RJ Carbs
Join Date: May 2017
Posts: 6
Rep Power: 6
rjcarbs is on a distinguished road
Heat Source can be added even if Heat Conduction in Solids Deactivated, please ignore my initial question.
Another question though, for large structure such as a dome, what is your recommended number of cells to get an accurate and acceptable result.
Also, in human heat load, should I include both the sensible and latent heat of a person or just the sensible heat.
Hope somebody can help.
Thank you.
rjcarbs is offline   Reply With Quote

Old   May 18, 2017, 21:41
Default
  #3
New Member
 
RJ Carbs
Join Date: May 2017
Posts: 6
Rep Power: 6
rjcarbs is on a distinguished road
One more question, Can I make the solids bodies Coarse mesh cause by the default setting, it is refined and so accounts to a large number of mesh but it is not a major concern on the calculation.
rjcarbs is offline   Reply With Quote

Old   May 31, 2017, 05:01
Default
  #4
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 617
Rep Power: 21
Boris_M will become famous soon enough
Oh, just found your post.

There is no suggested cell count as it depends on the model itself and it's dimensions as well as the physics that need to be resolved.

You should consider all heat sources (positive and negative) in the simulation as they will influence the Results. Of course if the majority is 1kW sources, then a tiny source of 0.5W barely plays a role if you want to simplify things.

Yes, it seems you are using the automatic settings and sometimes it can happen that due to a boundary condition the settings behind the automatic settings get very fine. Especially if a boundary condition is applied to a small element like a body or surface.
If you switch to manual mesh settings you can directly see what the settings behind the automatic ones have been. Often the tolerance or small feature refinements get ramped up to a high level and can be reduced again.
The meshing is quite simple, if you switch on the basic mesh you can see the cell level 0 and the other settings will refine the mesh by splitting the cells in 4 cells in the 2D plot (in 8 in the 3rd dimension) per level refinement. So if your fluid cell is for example 10mm and you have level 2 selected for the fluid cells, then you will get 2.5mm cells (4 cells per direction, 64 cells in total). I think that should give you an idea of how the meshing roughly works.

Hope this helps,
Boris
Boris_M is offline   Reply With Quote

Old   June 6, 2017, 02:07
Default
  #5
New Member
 
RJ Carbs
Join Date: May 2017
Posts: 6
Rep Power: 6
rjcarbs is on a distinguished road
Thanks Boris for your reply.

I am done with the CFD but it I want to verify its accuracy.
I noticed in the result that there is no stratification of heat. The temperature is uniform throughout from the ground up to the roof level. The only noticeable temperature difference is in the supply outlet. Please see pictures.
Attached Images
File Type: jpg Solver is Finished.jpg (102.4 KB, 12 views)
File Type: png meshing.png (176.1 KB, 13 views)
File Type: jpg boundary condition.jpg (123.3 KB, 12 views)
File Type: jpg model3.jpg (65.5 KB, 10 views)
File Type: png temperature profile 1.5m.png (128.9 KB, 9 views)
rjcarbs is offline   Reply With Quote

Old   June 6, 2017, 02:26
Default
  #6
New Member
 
RJ Carbs
Join Date: May 2017
Posts: 6
Rep Power: 6
rjcarbs is on a distinguished road
Attached image is the temperature profile at cross section. Also, from initial temperature of 28.5 there is only a decrease of 2C down to 26.5C.
Attached Images
File Type: png temperature profile cross section.png (81.9 KB, 11 views)
rjcarbs is offline   Reply With Quote

Old   June 29, 2017, 04:37
Default
  #7
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 617
Rep Power: 21
Boris_M will become famous soon enough
It is hard to tell from what you wrote on how much heat in total is introduced to the model, also do you have heat transfer conditions to the exterior or solar radiation etc.
There are many things to look at if the expected temperatures are not reached to even see if the setup is correct. The model seems quite huge and I cannot tell how much heat is dissipated as well as where. In general it might also be the problem that the solver has finished because all the goals you have defined are converged in the terms that the values are not chaning enough in the interval it is checking for convergence. You face the problem here that in such a huge volume the heat takes very long to heat everything up and temperatures therefore change very slowly and this is within the convergence criteria. Meaning if the criteria is 5C within the interval it checks (that would be 1/2 travel = 165 Iterations) if it is converged and the temperature increases by 4.5 C in that time, it is smaller than the convergence criteria and therefore the solver is happy with the change and accepts it as converged even though there is a constant linear increase of the temperature but just too small to be outside of the criteria.
You should in such cases either deactivate the convergence and simply let it calculate or define more specific goals to the fluid temperature. I mean imagine how long it would take for the room to heat up by 10C with a lighter burning in one corner of the room. You would say after an hour that there is no change and it will never reach the 10C but the change is just very little and takes maybe 3 days.

Hope this helps,
Boris
Boris_M is offline   Reply With Quote

Old   June 30, 2017, 01:34
Default
  #8
New Member
 
RJ Carbs
Join Date: May 2017
Posts: 6
Rep Power: 6
rjcarbs is on a distinguished road
Thanks Boris,

Your suggestions helped a lot. About the set-up, this is an internal study and radiation is off. The solar radiation is a calculated value and is added as a heat source. The next time I will be running such calculation, I will deactivate convergence criteria and expect better results.

Thanks,
RJ
rjcarbs 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
[swak4Foam] funkyDoCalc with OF2.3 massflow NiFl OpenFOAM Community Contributions 14 November 25, 2020 03:30
Error - Solar absorber - Solar Thermal Radiation MichaelK CFX 12 September 1, 2016 05:15
[foam-extend.org] problem when installing foam-extend-1.6 Thomas pan OpenFOAM Installation 7 September 9, 2015 21:53
centOS 5.6 : paraFoam not working yossi OpenFOAM Installation 2 October 9, 2013 01:41
[swak4Foam] build problem swak4Foam OF 2.2.0 mcathela OpenFOAM Community Contributions 14 April 23, 2013 13:59


All times are GMT -4. The time now is 12:46.