[cfd_begin]

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.

[ghorrocks]

Please post your CCL.

[cfd_begin]

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

[ghorrocks]

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?

[cfd_begin]

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.

[ghorrocks]

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.

[cfd_begin]

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 |
+----------------------+-----------------------+---------------------+

[ghorrocks]

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.

[cfd_begin]

I also tried by setting conservation target as : 0.001. But no change observed.

[cfd_begin]

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.

[ghorrocks]

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.

[cfd_begin]

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

[ghorrocks]

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?

[Opaque]

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.

[ghorrocks]

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.

[Opaque]

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"

[cfd_begin]

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.

[cfd_begin]

I think there is some problem occurring near the two domain interfaces that is making results bad.

[cfd_begin]

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.

[techtuner]

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