Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Thermal contact conductance(TCC) 4
- Thread starter feavnik
- Start date
-
3
- #2
Stringmaker
Mechanical
Vinay, what questions did you have specifically? I've used 174's on many occasions in a thermal surface-to-surface contact analysis. Here is a little section below that I thought may be helpful from the documentation:
"The conductive heat transfer between two contacting surfaces is defined by
q = TCC X (Tt -Tc)
where:
q: is the heat flux per area.
TCC: is the thermal contact conductance coefficient, having units of HEAT/(TIME * TEMPERATURE) for force-based node-to-surface contact, or units of HEAT/(TIME * TEMPERATURE * AREA) for the traction-based model.
Tt and Tc: are the temperatures of the contact points on the target and contact surfaces.
The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option. TCC has units of heat/(time x area x temp). If contact occurs, a small value of TCC yields a measure amount of imperfect contact and a temperature discontinuity across the interface. For large values of TCC, the resulting temperature discontinuity tends to vanish and perfect thermal contact is approached. When not in contact, however, it is assumed that no heat is transferred across the interface. To model contact conduction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options."
-Brian
"The conductive heat transfer between two contacting surfaces is defined by
q = TCC X (Tt -Tc)
where:
q: is the heat flux per area.
TCC: is the thermal contact conductance coefficient, having units of HEAT/(TIME * TEMPERATURE) for force-based node-to-surface contact, or units of HEAT/(TIME * TEMPERATURE * AREA) for the traction-based model.
Tt and Tc: are the temperatures of the contact points on the target and contact surfaces.
The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option. TCC has units of heat/(time x area x temp). If contact occurs, a small value of TCC yields a measure amount of imperfect contact and a temperature discontinuity across the interface. For large values of TCC, the resulting temperature discontinuity tends to vanish and perfect thermal contact is approached. When not in contact, however, it is assumed that no heat is transferred across the interface. To model contact conduction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options."
-Brian
- Thread starter
- #3
Hi Brian,
Thanks for replying. I know the value of q, how do I find the difference in contact/target temperatures (Tt -Tc).
Can you please elabotrate a bit on "The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option."
Again, here I need to find Tt and Tc.
Thanks,
Vinay
Thanks for replying. I know the value of q, how do I find the difference in contact/target temperatures (Tt -Tc).
Can you please elabotrate a bit on "The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option."
Again, here I need to find Tt and Tc.
Thanks,
Vinay
Stringmaker
Mechanical
Vinay,
Tt and Tc are not something you typically know in most cases. Apply loads and bc's as one normally would in a thermal analysis, specify the appropriate elements and contact regions,value for TCC, etc and let Ansys do it's thing. Note that TCC is input as real constant 14 (see below script). The documentation is just telling you that it can be specified other ways as well. Here's an example of what your input should look like:
ET,100,TARGE170 !Target Element Type Defined
ET,101,CONTA174 !Contact Element Type Defined
KEYOPT,101,1,2 !DOF set to temperature
KEYOPT,101,5,3 !Adjust Gaps/Penetration
KEYOPT,101,9,1 !Exclude Initial Penetration/Gap
KEYOPT,101,11,1 !Include shell thickness (if shell model, excluded for solids)
KEYOPT,101,12,0 !Standard contact specified
!
FKN =.1 !normal stiffness factor
FTOL = .2 !penetration tolerance
ICON = .2 !initial closure factor
CNOF = 1e-6 !offset value assigned to contact surface
TCC = 500/144/3600 !contact conductance value (perfect conduction)
!
!R1, R2, FKN, FTOLN, ICONT, PINB !Real 1-6
!PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT !Real 7-12
!COHE, TCC, FHTG, SBCT,RDVF, FWGT !Real 13-18
!
C*** Contact to Target Specification
!
R,1000,,,FKN,FTOL,ICON,,
RMORE,,,,0,,,
RMORE,,TCC,,,,,
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,100 !Specify Target Elements
ESEL $NSEL !Select Elements of Target Surface
ESURF !Mesh target surface
!
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,101 !Specify Contact Elements
ESEL $NSEL !Select Elements of Target Surface
ESURF !Mesh contact surface
!
Edit this to suit your application...this is just a general format of what a contact macro would look like.
Good luck,
-Brian
Tt and Tc are not something you typically know in most cases. Apply loads and bc's as one normally would in a thermal analysis, specify the appropriate elements and contact regions,value for TCC, etc and let Ansys do it's thing. Note that TCC is input as real constant 14 (see below script). The documentation is just telling you that it can be specified other ways as well. Here's an example of what your input should look like:
ET,100,TARGE170 !Target Element Type Defined
ET,101,CONTA174 !Contact Element Type Defined
KEYOPT,101,1,2 !DOF set to temperature
KEYOPT,101,5,3 !Adjust Gaps/Penetration
KEYOPT,101,9,1 !Exclude Initial Penetration/Gap
KEYOPT,101,11,1 !Include shell thickness (if shell model, excluded for solids)
KEYOPT,101,12,0 !Standard contact specified
!
FKN =.1 !normal stiffness factor
FTOL = .2 !penetration tolerance
ICON = .2 !initial closure factor
CNOF = 1e-6 !offset value assigned to contact surface
TCC = 500/144/3600 !contact conductance value (perfect conduction)
!
!R1, R2, FKN, FTOLN, ICONT, PINB !Real 1-6
!PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT !Real 7-12
!COHE, TCC, FHTG, SBCT,RDVF, FWGT !Real 13-18
!
C*** Contact to Target Specification
!
R,1000,,,FKN,FTOL,ICON,,
RMORE,,,,0,,,
RMORE,,TCC,,,,,
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,100 !Specify Target Elements
ESEL $NSEL !Select Elements of Target Surface
ESURF !Mesh target surface
!
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,101 !Specify Contact Elements
ESEL $NSEL !Select Elements of Target Surface
ESURF !Mesh contact surface
!
Edit this to suit your application...this is just a general format of what a contact macro would look like.
Good luck,
-Brian
Stringmaker
Mechanical
Disregard my first post. Sorry this is a more correct version:
Vinay,
Tt and Tc are not something you typically know in most cases. Apply loads and bc's as one normally would in a thermal analysis, specify the appropriate elements and contact regions,value for TCC, etc and let Ansys do it's thing. Note that TCC is input as real constant 14 (see below script). The documentation is just telling you that it can be specified other ways as well. Here's an example of what your input should look like:
ET,100,TARGE170 !Target Element Type Defined
ET,101,CONTA174 !Contact Element Type Defined
KEYOPT,101,1,2 !DOF set to temperature
KEYOPT,101,5,3 !Adjust Gaps/Penetration
KEYOPT,101,9,1 !Exclude Initial Penetration/Gap
KEYOPT,101,11,1 !Include shell thickness (if shell model, excluded for solids)
KEYOPT,101,12,0 !Standard contact specified
!
FKN =.1 !normal stiffness factor
FTOL = .2 !penetration tolerance
ICON = .2 !initial closure factor
CNOF = 1e-6 !offset value assigned to contact surface
TCC = 500/144/3600 !contact conductance value (perfect conduction)
!
!R1, R2, FKN, FTOLN, ICONT, PINB !Real 1-6
!PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT !Real 7-12
!COHE, TCC, FHTG, SBCT,RDVF, FWGT !Real 13-18
!
C*** Mesh Target Surface
!
R,1000,,,FKN,FTOL,ICON,,
RMORE,,,,0,,,
RMORE,,TCC,,,,,
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,100 !Specify Target Elements
ESEL $NSEL !Select elements and nodes of target surface
ESURF !Mesh target surface
!
C*** Mesh Contact Surface
!
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,101 !Specify Contact Elements
ESEL $NSEL !Select elements and nodes of contact surface
ESURF !Mesh contact surface
!
Edit this to suit your application...this is just a general format of what a contact macro would look like.
Good luck,
-Brian
Vinay,
Tt and Tc are not something you typically know in most cases. Apply loads and bc's as one normally would in a thermal analysis, specify the appropriate elements and contact regions,value for TCC, etc and let Ansys do it's thing. Note that TCC is input as real constant 14 (see below script). The documentation is just telling you that it can be specified other ways as well. Here's an example of what your input should look like:
ET,100,TARGE170 !Target Element Type Defined
ET,101,CONTA174 !Contact Element Type Defined
KEYOPT,101,1,2 !DOF set to temperature
KEYOPT,101,5,3 !Adjust Gaps/Penetration
KEYOPT,101,9,1 !Exclude Initial Penetration/Gap
KEYOPT,101,11,1 !Include shell thickness (if shell model, excluded for solids)
KEYOPT,101,12,0 !Standard contact specified
!
FKN =.1 !normal stiffness factor
FTOL = .2 !penetration tolerance
ICON = .2 !initial closure factor
CNOF = 1e-6 !offset value assigned to contact surface
TCC = 500/144/3600 !contact conductance value (perfect conduction)
!
!R1, R2, FKN, FTOLN, ICONT, PINB !Real 1-6
!PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT !Real 7-12
!COHE, TCC, FHTG, SBCT,RDVF, FWGT !Real 13-18
!
C*** Mesh Target Surface
!
R,1000,,,FKN,FTOL,ICON,,
RMORE,,,,0,,,
RMORE,,TCC,,,,,
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,100 !Specify Target Elements
ESEL $NSEL !Select elements and nodes of target surface
ESURF !Mesh target surface
!
C*** Mesh Contact Surface
!
ESEL,NONE $NSEL,NONE !Unselect all nodes & elements
TYPE,101 !Specify Contact Elements
ESEL $NSEL !Select elements and nodes of contact surface
ESURF !Mesh contact surface
!
Edit this to suit your application...this is just a general format of what a contact macro would look like.
Good luck,
-Brian
- Thread starter
- #6
Franky3000
Mechanical
Hi Brian:
do have that macro of TCC in GUI format, I mean how to do the commnads from the menu, not from the command line ?
how you can change the KEYOPT ?
thanks
Frank
do have that macro of TCC in GUI format, I mean how to do the commnads from the menu, not from the command line ?
how you can change the KEYOPT ?
thanks
Frank
Stringmaker
Mechanical
Frank,
Using the contact wizard is by far the easiest way to make contact via GUI. As for changing element keyopts that can be done in GUI mode under Preprocessor -> Element Type -> Add/Edit/Delete -> Options.
Good luck,
-Brian
Using the contact wizard is by far the easiest way to make contact via GUI. As for changing element keyopts that can be done in GUI mode under Preprocessor -> Element Type -> Add/Edit/Delete -> Options.
Good luck,
-Brian
Franky3000
Mechanical
Hi Brain:
Thanks so much for your valuable reply and advice.
Another question, please:
I have two 2D surfaces that have a common line and I need to study the heat transfer from one surface to the other through their common line, so how should I mesh these surfaces and their common line in a way that ANSYS will consider the thermal contact conductance ?
Thanks
Frank
Thanks so much for your valuable reply and advice.
Another question, please:
I have two 2D surfaces that have a common line and I need to study the heat transfer from one surface to the other through their common line, so how should I mesh these surfaces and their common line in a way that ANSYS will consider the thermal contact conductance ?
Thanks
Frank
Stringmaker
Mechanical
Frank,
Thermal shell elements are the best choice for something like that. Check out SHELL 131 and SHELL 132 and determine which one suits your needs best.
-Brian
Thermal shell elements are the best choice for something like that. Check out SHELL 131 and SHELL 132 and determine which one suits your needs best.
-Brian
Franky3000
Mechanical
Hi Brain:
Thanks again for your valuable help and replies.
Now I am able to model the interface conductance at the interface between two areas and I can play with the value of thermal contact conductance to get different results, so now, I am wondering if I do NOT define the contact pair at the interface, and let the ANSYS solves the model, what is the default of ANSYS in dealing with the interface ? does it consider it as a perfect contact (very high value of thermal conductance) or perfect thermal resistance (very low value of thermal conductance) ?
Thanks
Frank
Thanks again for your valuable help and replies.
Now I am able to model the interface conductance at the interface between two areas and I can play with the value of thermal contact conductance to get different results, so now, I am wondering if I do NOT define the contact pair at the interface, and let the ANSYS solves the model, what is the default of ANSYS in dealing with the interface ? does it consider it as a perfect contact (very high value of thermal conductance) or perfect thermal resistance (very low value of thermal conductance) ?
Thanks
Frank
Stringmaker
Mechanical
If you have a continuous mesh why would you need to consider any sort of contact there? If your mesh is not continuous then of course you'll need contact to bridge the gap.
Franky3000
Mechanical
Hi Brain:
Are you saying if we have a nice continuous meshing at the interface of two areas, we do not need to define a contact pair ? ...well so what is the importance of having such function of creating a contact pair ?
I agree with you that if the mesh is not continuous at the interface, you will have an artificial gap and it will hurt the solution.
Are you saying if we have a nice continuous meshing at the interface of two areas, we do not need to define a contact pair ? ...well so what is the importance of having such function of creating a contact pair ?
I agree with you that if the mesh is not continuous at the interface, you will have an artificial gap and it will hurt the solution.
Franky3000
Mechanical
hi guys:
what should i do when I get a error message saying "unconstrained model" when trying to solve thermal analysis steady state case ?
thanks
what should i do when I get a error message saying "unconstrained model" when trying to solve thermal analysis steady state case ?
thanks
Franky3000
Mechanical
hi all:
is there a way to undo or cancel the command of "Merge" ?
Thanks
Frank
is there a way to undo or cancel the command of "Merge" ?
Thanks
Frank
-
1
- #16
Franky3000
Mechanical
hi,
Thanks so much "cbrn"....it works...wow..you saved my day !
best regards
Frank
Thanks so much "cbrn"....it works...wow..you saved my day !
best regards
Frank
- Status
Similar threads
- Question
- Locked
- Question
- Locked
- Question