|
[Sponsors] |
[stressAnalysis] How to simulate thermal stress and heat transfer simultaneously using OF? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 24, 2011, 09:14 |
How to simulate thermal stress and heat transfer simultaneously using OF?
|
#1 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Dear All,
I need help to simulate thermal stress and heat transfer simultaneously using OF. Any help is welcomed. Many thanks, Marco. |
|
May 24, 2011, 18:20 |
|
#2 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Hi Marco,
SolidDisplacementFoam solves for thermal stress and temperature, check out the tutorial. Philip |
|
May 25, 2011, 06:21 |
|
#3 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Hi Philip,
That's great! Thank you for your help. Regards, Marco. |
|
May 25, 2011, 06:39 |
|
#4 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Hi Philip,
The tutorial was set to not solve the thermal equation. Could you help me put the thermal equation working? Regards, Marco. |
|
May 25, 2011, 06:48 |
|
#5 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Marco,
In the tutorial "constant/thermalProperties" file, change "thermalStress no;" to "thermalStress yes;". The solver will now solve the energy equation (for temperature) after solving the momentum equation (for displacement). Hope it helps, Philip |
|
May 25, 2011, 08:21 |
Foam fatal io error:
|
#6 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Dear Philip,
Then I get the following error message: Regards, Marco. --> FOAM FATAL IO ERROR: cannot open file file: /home/marco/OpenFOAM/marco-1.7.1/run/tutorials/stressAnalysis/solidDisplacementFoam/system/controlDict at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 61. FOAM exiting |
|
May 25, 2011, 09:27 |
|
#7 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Marco,
You seem to be running the solidDisplacementFoam solver inside the solver source code directory, you must run the solidDisplacementFoam solver in the tutorial case directory (i.e. inside plateHole). The user guide shows one how to run this plateHole tutorial (http://www.openfoam.com/docs/user/pl...hp#x6-370002.2), the only difference is that you will have to turn on the thermalStress option in thermalProperties. Philip |
|
May 25, 2011, 09:56 |
Source code directory
|
#8 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Philip,
Sorry to bother you but I ran it in the source code directory. I tried both options. Using "thermalProperties no;" it works fine. Using "thermalProperties yes;" I get the mentioned message. Regards, Marco. |
|
May 25, 2011, 10:13 |
|
#9 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Marco,
What version of OpenFOAM are you using? I just tried solidDisplacementFoam and plateHole in OpenFOAM-1.6-ext and it works fine when I turn on "thermalStress" in "constant/thermalProperties". Just to recap, did you try the following: copy the tutorial to your home directory - $ cp -r $FOAM_SOLVERS/stressAnalysis/solidDisplacementFoam/plateHole $FOAM_RUN/ change into the plateHole directory - $ cd $FOAM_RUN/plateHole edit "constant/thermalProperties" and turn "thermalStress" to yes. then run the solver in the plateHole directory - $ solidDisplacementFoam If you might get an error about a ddtScheme not being defined, then put this in the "system/fvSchemes" file: ddtSchemes { default Euler; } Also you will have to increase the number of correctors in the "system/fvSolution" file to something like 1000: stressAnalysis { compactNormalStress yes; nCorrectors 1000; D 1e-06; } Philip |
|
May 25, 2011, 10:53 |
It works fine.
|
#10 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Philip,
Thank you. It works but the temperature output is constant. I think I should change the initial and boundary temperature conditions. Regards, Marco. |
|
May 25, 2011, 10:58 |
|
#11 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Marco,
Yes the tutorial case is not set-up for showing off the temperature solving capabilities, you could change one of the boundary conditions in "0/T" to see a non-uniform temperature, something like: Code:
right { type fixedValue; value uniform 500; } d2dt2Schemes { default Euler; } Philip |
|
May 26, 2011, 08:35 |
Thermal stress
|
#12 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Philip,
Thanks a lot! It works fine. Do you have an idea how to show the displacement induced by the thermal expansion? Regards, Marco. |
|
May 26, 2011, 08:43 |
|
#13 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Marco,
The displacement field D is a combination of the displacements due to the traction/displacement boundary conditions and also the displacement due to thermal expansion. To view just thermally induced displacements you would have to set your D boundary conditions to something like all of them as traction-free excepts for one or two as symmetry plane or something like that. Also I would recommend you validate this solver against some sort of analytical solution, because I am not sure how often it is used. Philip |
|
May 26, 2011, 08:58 |
Displacement
|
#14 |
Member
Marco Bernardes
Join Date: May 2009
Posts: 59
Rep Power: 17 |
Dear Philip,
I will do that. Thank you again, Marco. |
|
July 14, 2011, 10:13 |
compactNormalStress in solidDisplacementFoam
|
#15 |
Senior Member
Hisham Elsafti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 257
Blog Entries: 10
Rep Power: 17 |
Dear Philip,
Thanks a lot for the info. Regarding the solidDisplacementFoam solver, there is a switch called "compactNormalStress", which controls the way the "divSigmaExp" vector field is calculated. I would like to know what does this switch represent in physical terms? This switch is set to 'yes' in the solver plate with hole example. I would like to know also if there are any plasticity implementations available for that solver. Thanks a lot for any help! Hisham |
|
July 14, 2011, 11:35 |
|
#16 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Hi Hisham,
divSigmaExp seems to be the portion of div(sigma) which is treated explicitly. I am not too familiar with this solver (I use stress solvers based on newStressedFoam in OpenFOAM extend). I am not quite sure what difference the compactNormalStress makes, it seems to just be a slightly different way of calculating the explicit portion of the divergence of sigma. When it is set to yes it seems to be doing the same as newStressedFoam. I would recommend you run a few test cases with it on and off to see how it might effect the results. As regards plasticity, here in UCD (http://adhesion.ucd.ie/openfoam) solid stress plasticity solvers and material models have been developed, but as yet they have not been released into OpenFOAM extend (I imagine they will be included at some stage). These solvers are based around the newStressedFoam solver. You could contact Prof. Ivankovic at UCD asking nicely to have access to them, or maybe some sort of collaboration. Hope it helps, Philip |
|
July 14, 2011, 11:59 |
|
#17 |
Senior Member
Hisham Elsafti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 257
Blog Entries: 10
Rep Power: 17 |
Hi Philip
Thanks a million for your quick and efficient response I will explore the OF extended project (read about it a while ago and seemed to have forgotten about it) I will review Prof. Ivankovic publications then I'll contact him with less ignorance Thanks again Hisham |
|
July 20, 2015, 13:48 |
How to simulate thermal stress and heat transfer simultaneously using OF?
|
#18 |
New Member
Join Date: Feb 2015
Posts: 4
Rep Power: 11 |
Hi,
What if in this case I would like to add water cooling at one side of the plate and heat flux at the other side? I would like to simulate stresses inside the solid plate in this case. Thank you. |
|
July 20, 2015, 23:24 |
|
#19 | |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 |
Quote:
Philip |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Natural convection in a closed domain STILL NEEDING help! | Yr0gErG | FLUENT | 4 | December 2, 2019 01:04 |
Thermal stress analysis with heat flux boundary condition | cvasse | OpenFOAM Running, Solving & CFD | 0 | March 20, 2018 10:46 |
2—way FSI with heat transfer | ronggehejiumeizuiguo | Main CFD Forum | 0 | June 7, 2015 02:36 |
Question about heat transfer coefficient setting for CFX | Anna Tian | CFX | 1 | June 16, 2013 07:28 |
Info: Short Course On Thermal Design of Electronic Equipment | Arnold Free | Main CFD Forum | 0 | August 10, 1999 11:18 |