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

How to simulate thermal stress and heat transfer simultaneously using OF?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 24, 2011, 08:14
Default How to simulate thermal stress and heat transfer simultaneously using OF?
  #1
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
Dear All,

I need help to simulate thermal stress and heat transfer simultaneously using OF.
Any help is welcomed.

Many thanks,

Marco.
masb is offline   Reply With Quote

Old   May 24, 2011, 17:20
Default
  #2
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
Hi Marco,

SolidDisplacementFoam solves for thermal stress and temperature, check out the tutorial.

Philip
bigphil is offline   Reply With Quote

Old   May 25, 2011, 05:21
Default
  #3
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
Hi Philip,

That's great! Thank you for your help.

Regards,

Marco.
masb is offline   Reply With Quote

Old   May 25, 2011, 05:39
Default
  #4
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
Hi Philip,

The tutorial was set to not solve the thermal equation. Could you help me put the thermal equation working?

Regards,

Marco.
masb is offline   Reply With Quote

Old   May 25, 2011, 05:48
Default
  #5
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
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
bigphil is offline   Reply With Quote

Old   May 25, 2011, 07:21
Default Foam fatal io error:
  #6
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
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
masb is offline   Reply With Quote

Old   May 25, 2011, 08:27
Default
  #7
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
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
bigphil is offline   Reply With Quote

Old   May 25, 2011, 08:56
Default Source code directory
  #8
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
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.
masb is offline   Reply With Quote

Old   May 25, 2011, 09:13
Default
  #9
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
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
bigphil is offline   Reply With Quote

Old   May 25, 2011, 09:53
Default It works fine.
  #10
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
Philip,

Thank you. It works but the temperature output is constant. I think I should change the initial and boundary temperature conditions.

Regards,

Marco.
masb is offline   Reply With Quote

Old   May 25, 2011, 09:58
Default
  #11
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
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;
    }
By the way, d2dt2Schemes in system/fvSchemes should be changed to "Euler" if you want to look at transient stresses:
d2dt2Schemes
{
default Euler;
}


Philip
bigphil is offline   Reply With Quote

Old   May 26, 2011, 07:35
Default Thermal stress
  #12
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
Philip,

Thanks a lot! It works fine. Do you have an idea how to show the displacement induced by the thermal expansion?

Regards,

Marco.
masb is offline   Reply With Quote

Old   May 26, 2011, 07:43
Default
  #13
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
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
bigphil is offline   Reply With Quote

Old   May 26, 2011, 07:58
Default Displacement
  #14
Member
 
Marco Bernardes
Join Date: May 2009
Posts: 38
Rep Power: 8
masb is on a distinguished road
Dear Philip,

I will do that.

Thank you again,

Marco.
masb is offline   Reply With Quote

Old   July 14, 2011, 09:13
Default compactNormalStress in solidDisplacementFoam
  #15
Senior Member
 
Hisham's Avatar
 
Hisham El Safti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 247
Blog Entries: 10
Rep Power: 8
Hisham is on a distinguished road
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
Hisham is offline   Reply With Quote

Old   July 14, 2011, 10:35
Default
  #16
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
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
bigphil is offline   Reply With Quote

Old   July 14, 2011, 10:59
Default
  #17
Senior Member
 
Hisham's Avatar
 
Hisham El Safti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 247
Blog Entries: 10
Rep Power: 8
Hisham is on a distinguished road
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
Hisham 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
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 3 June 12, 2013 02:12
Conjugate Transient Heat Transfer Jaap FLUENT 0 May 24, 2008 16:09
'Heat Transfer' Fab Main CFD Forum 3 October 14, 2007 13:39
time averaged heat transfer in oscillating flow Matthieu Ubas Main CFD Forum 2 November 5, 1999 15:20
Info: Short Course On Thermal Design of Electronic Equipment Arnold Free Main CFD Forum 0 August 10, 1999 10:18


All times are GMT -4. The time now is 02:55.