|
[Sponsors] |
May 30, 2017, 02:52 |
Periodic heat transfer-CFX
|
#1 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
Hi.
I want to model periodic heat transfer problem in a circular channel with uniform wall temperature, say 330 [K]. IN CFX, I am able to achieve the periodic flow using either a source term in the momentum equation/ by specifying mass-flow rate. However, when I want to model heat transfer using source term I get weird results. Can anybody put some light on the source term for the energy equation. It appears to me that this setting does not solve the periodic temperature but a full flow (includes similar setting like uniform temperature at inlet. |
|
May 30, 2017, 03:19 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
Please post your CCL.
|
|
May 30, 2017, 03:33 |
|
#3 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
LIBRARY:
CEL: EXPRESSIONS: Tbulk = massFlowAve(T)@Domain Interface 1 Side 1 END END MATERIAL: Air at 25 C Material Description = Air at 25 C and 1 atm (dry) Material Group = Air Data, Constant Property Gases Option = Pure Substance Thermodynamic State = Gas PROPERTIES: Option = General Material EQUATION OF STATE: Density = 1.185 [kg m^-3] Molar Mass = 28.96 [kg kmol^-1] Option = Value END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1] Specific Heat Type = Constant Pressure END REFERENCE STATE: Option = Specified Point Reference Pressure = 1 [atm] Reference Specific Enthalpy = 0. [J/kg] Reference Specific Entropy = 0. [J/kg/K] Reference Temperature = 25 [C] END DYNAMIC VISCOSITY: Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1] Option = Value END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 2.61E-02 [W m^-1 K^-1] END ABSORPTION COEFFICIENT: Absorption Coefficient = 0.01 [m^-1] Option = Value END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^-1] END REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^-1] END THERMAL EXPANSIVITY: Option = Value Thermal Expansivity = 0.003356 [K^-1] END END END END FLOW: Flow Analysis 1 SOLUTION UNITS: Angle Units = [rad] Length Units = [m] Mass Units = [kg] Solid Angle Units = [sr] Temperature Units = [K] Time Units = [s] END ANALYSIS TYPE: Option = Steady State EXTERNAL SOLVER COUPLING: Option = None END END DOMAIN: Domain 1 Coord Frame = Coord 0 Domain Type = Fluid Location = FLUID BOUNDARY: Domain Interface 1 Side 1 Boundary Type = INTERFACE Location = INLET BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Conservative Interface Flux END MASS AND MOMENTUM: Option = Conservative Interface Flux END END BOUNDARY SOURCE: SOURCES: EQUATION SOURCE: energy Flux = -200 [W m^-2] Option = Flux END END END END BOUNDARY: Domain Interface 1 Side 2 Boundary Type = INTERFACE Location = OUTLET BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Conservative Interface Flux END MASS AND MOMENTUM: Option = Conservative Interface Flux END END END BOUNDARY: wall Boundary Type = WALL Location = WALL BOUNDARY CONDITIONS: HEAT TRANSFER: Fixed Temperature = 330 [K] Option = Fixed Temperature END MASS AND MOMENTUM: Option = No Slip Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Option = Non Buoyant END DOMAIN MOTION: Option = Stationary END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END FLUID DEFINITION: Fluid 1 Material = Air at 25 C Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Option = Thermal Energy END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = Laminar END END SUBDOMAIN: Subdomain 1 Coord Frame = Coord 0 Location = FLUID END END DOMAIN INTERFACE: Domain Interface 1 Boundary List1 = Domain Interface 1 Side 1 Boundary List2 = Domain Interface 1 Side 2 Interface Type = Fluid Fluid INTERFACE MODELS: Option = Translational Periodicity MASS AND MOMENTUM: Option = Conservative Interface Flux MOMENTUM INTERFACE MODEL: Mass Flow Rate = 2.97e-05 [kg s^-1] Option = Mass Flow Rate END END END MESH CONNECTION: Option = GGI END END OUTPUT CONTROL: MONITOR OBJECTS: MONITOR BALANCES: Option = Full END MONITOR FORCES: Option = Full END MONITOR PARTICLES: Option = Full END MONITOR POINT: Monitor Point 1 Coord Frame = Coord 0 Expression Value = Tbulk Option = Expression END MONITOR RESIDUALS: Option = Full END MONITOR TOTALS: Option = Full END END RESULTS: File Compression Level = Default Option = Standard END END SOLVER CONTROL: ADVECTION SCHEME: Option = High Resolution END CONVERGENCE CONTROL: Length Scale Option = Conservative Maximum Number of Iterations = 300 Minimum Number of Iterations = 1 Timescale Control = Auto Timescale Timescale Factor = 1.0 END CONVERGENCE CRITERIA: Residual Target = 0.000001 Residual Type = RMS END |
|
May 30, 2017, 05:33 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
Are you sure it has converged? I would add the imbalances to your convergence criteria. In this sort of simulation I would expect the velocity field to converge much faster than the temperature field. Try running it for longer, including imbalances as a convergence criteria.
What initial condition did you use? |
|
May 30, 2017, 05:44 |
|
#5 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
yes, the solutions are converged with criterion, 1e-06.
The problem is the temperature profiles as you can see in third figure. this is not typical of a periodic flow which i must get. Thanks. no initial conditions. solving steady-state. |
|
May 30, 2017, 05:57 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
Yes, I suspected your simulation is converged to the criteria you defined. I am saying your criteria is not appropriate and you should include imbalances as part of your convergence criteria.
|
|
May 30, 2017, 06:18 |
|
#7 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
yes, your observation is very correct. How can I use Imbalance as convergence criterion ?
Shall I put a more tight convergence criterion for energy ? I put table also: Normalised Imbalance Summary | +--------------------------------------------------------------------+ | Equation | Maximum Flow | Imbalance (%) | +--------------------------------------------------------------------+ | U-Mom | 5.5203E-06 | 0.0136 | | V-Mom | 5.5203E-06 | 0.0000 | | W-Mom | 5.5203E-06 | 0.0002 | | P-Mass | 2.9697E-05 | 0.0000 | +----------------------+-----------------------+---------------------+ | H-Energy | 9.4050E-01 | -0.1532 | +----------------------+-----------------------+---------------------+ |
|
May 30, 2017, 06:45 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
Those imbalances look OK so I suspect imbalances might not be the problem. Regardless, I would run it for a few more iterations anyway to see if the temperature field changes or not.
|
|
May 30, 2017, 06:54 |
|
#9 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
I also tried by setting conservation target as : 0.001. But no change observed.
|
|
May 30, 2017, 06:57 |
|
#10 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
I m worried about the source term. is it ok to specify like that or do i need to work on some expression. from previous threads, i see we need to remove heat using source term.
|
|
May 30, 2017, 07:33 |
|
#11 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
Yes, if you want this flow to be periodic you will need to balance the heat so there is no net heat.
You are correct - the source term appears to be doing strange things. It appears to be taking a lot of heat out of the region close to the wall but adding heat in the middle. It does not appear to be doing an even -200 W/m^2 as you requested. Try putting in a source term subdomain instead of a source term on the periodic boundary. |
|
May 30, 2017, 07:41 |
|
#12 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
yes, I have done that. Please,find the attached result.
SUBDOMAIN: Subdomain 1 Coord Frame = Coord 0 Location = FLUID SOURCES: EQUATION SOURCE: energy Option = Source Source = -40000 [W m^-3] END END END END |
|
May 30, 2017, 08:01 |
|
#13 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
I assume you defined the subdomain as the entire domain. If that is the case then this result is as expected.
So it appears you have found something weird in the energy source term when applied to periodic interfaces. It does some weird distribution of the energy, it does not appear to be even. I see you are using ANSYS V17. Does V18.1 (the current version) show this? |
|
May 30, 2017, 08:59 |
|
#14 |
Senior Member
Join Date: Jun 2009
Posts: 1,852
Rep Power: 33 |
May I ask what do you mean by "periodic heat transfer"?
What quantity do you expect to be periodic? I may need to see the mathematical model (equations and boundary conditions) to understand the concept and match it to what ANSYS CFX can do. |
|
May 30, 2017, 18:49 |
|
#15 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
I am assuming (AKS has never really stated what he is doing, most of my comments are based on assumptions), that the intention is that the heat added by the walls at constant temperature will be taken away by a heat sink of constant magnitude across the flow profile. That is why the temperature profile shown in post #1 is unexpected.
My opinion on this is something funny is going on with the source term option in the periodic boundary condition. The simulation appears to be properly converged. It might be a bug in the implementation of the source term. Note this is on V17, so it is not the current version. When he applies the heat sink as a subdomain it behaves as expected. |
|
May 30, 2017, 22:22 |
|
#16 |
Senior Member
Join Date: Jun 2009
Posts: 1,852
Rep Power: 33 |
I think there is a misunderstanding of how the boundary sources work, and what a domain interface is.
For the generalized grid interface approach, the flux is conserved at the interface. As far as I can see the source is applied on a side, not at the interface. Subtle difference, but a difference after all. For the 1:1 approach the value on the control volume vertex on either side of the interface is unique; therefore, no jump allowed. Without the mathematical formulation of the problem at hand, I do not see how a source can solve the problem for "periodic heat transfer boundary condition" |
|
May 31, 2017, 01:43 |
|
#17 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
I state my problem:
I am simulating the laminar flow in a circular tube to study the periodic flow and heat transfer. I want my model to predict the temperature contours and Nusselt number for this problem Nu (constant temperature) = 3.68 Nu (constant heat flux) = 4.64 I also attach the temperature plots I expect at from inlet to outlet for both situations. Thanks Ghorrocks and Opaque. |
|
May 31, 2017, 02:11 |
|
#18 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
I think there is some problem occurring near the two domain interfaces that is making results bad.
|
|
May 31, 2017, 02:23 |
|
#19 |
New Member
AKS
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
Dear Opaque,
For the specified mass flow rate option available in cfx to model periodic flow with a pressure drop, the option for mesh connection is only-GGI. To counter this, one thing i will do is i will not use this option of flow rate but model the pressure drop using source term in the momentum equation. In this way I will be able to get 1:1 thing which you stated. |
|
May 31, 2017, 02:49 |
|
#20 |
New Member
Dmitry
Join Date: Feb 2013
Posts: 29
Rep Power: 13 |
Cfd_begin, I would recommend you Fluent for your task. There it is no need in additional source terms to model heat transfer in periodic case.
Sent from my M040 using CFD Online Forum mobile app |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
CFX Multiphase - Fluid-fluid heat transfer | nasir | CFX | 3 | June 15, 2014 18:44 |
CFX Multiphase - Fluid-fluid heat transfer | nasir | CFX | 0 | June 14, 2014 06:21 |
Water subcooled boiling | Attesz | CFX | 7 | January 5, 2013 03:32 |
CFX wall heat transfer coefficient | mactech001 | CFX | 1 | January 5, 2010 21:33 |
CFX doesn't continue calculation... | mactech001 | CFX | 6 | November 15, 2009 21:25 |