
[Sponsors] 
December 18, 2016, 09:48 
Can CFX model periodic heat transfer problem

#1 
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
Hi everyone, I come across this issue recently and have read many threads here already, still no clue.
Is it possible to model the periodic heat transfer problem in CFX? In fluent Help, there is a turtorial about modeling periodic heat transfer problem. But I cannot achieve it using CFX. I can successfully get the flow field, but not the temperature field. In summery, there are two problem. First, when I define the mass flow rate in the periodic interface, there's nowhere I can define the temperature of the flow. Second, When I using a certain temperature condition, it seems the fluid temperature will all reach that wall temperature after several iteration. Anyone can help with that? Thank you so much. 

December 18, 2016, 18:03 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
I know of no limitation in the periodic boundary in CFX for temperature modelling. I suspect some other issue is causing the problem.
Can you show an image of what you are modelling and an example output file. 

December 18, 2016, 22:55 

#3  
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
Quote:
The example is from the fluent help tutorial, this is a 2D case. To compare the results, I modeled both in 3D using fluent and CFX. In fluent, I can define the flow bulk temperature as 300K when specifying the mass flow rate, as shown After iteration, I got the following results for velocity and temperature field. However, when using CFX, first I don't know where I can specify the upstream bulk temperature for the flow, because there is no place for me to input this information in the interface dialog box. Still, I finish the iteration using thermal energy model, and the flow converged pretty quickly while the heat transfer is not that good. Finally I got a similar velocity with that from fluent but a completely different temperature field results like this Really confused about that. 

December 18, 2016, 23:04 

#4 
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
CFD Solver finished: Mon Dec 19 10:32:20 2016
CFD Solver wall clock seconds: 7.1925E+01 ================================================== ==================== Termination and Interrupt Condition Summary ================================================== ==================== CFD Solver: Run duration reached (Maximum number of outer iterations) ================================================== ==================== Boundary Flow and Total Source Term Summary ================================================== ==================== ++  UMom  ++ Boundary : symmetry34 1.7396E23 Boundary : wall1 3.6313E07 Boundary : wall2 3.6471E07 Domain Interface : flowinterface (Side 1) 9.5685E07 Domain Interface : flowinterface (Side 2) 2.2901E07  Domain Imbalance : 1.2790E13 ++  VMom  ++ Boundary : symmetry1 4.6013E07 Boundary : symmetry2 4.8665E08 Boundary : symmetry34 7.7580E07 Boundary : wall1 3.8661E08 Boundary : wall2 4.0300E07 Domain Interface : flowinterface (Side 1) 9.2033E08 Domain Interface : flowinterface (Side 2) 9.2033E08  Domain Imbalance : 1.4211E13 ++  WMom  ++ Boundary : sym12 6.8212E13 Boundary : symmetry34 3.4704E26 Boundary : wall1 1.9230E12 Boundary : wall2 1.6828E13 Domain Interface : flowinterface (Side 1) 1.3119E11 Domain Interface : flowinterface (Side 2) 1.3119E11  Domain Imbalance : 1.0726E12 ++  PMass  ++ Domain Interface : flowinterface (Side 1) 5.0000E05 Domain Interface : flowinterface (Side 2) 5.0000E05  Domain Imbalance : 0.0000E+00 ++  HEnergy  ++ Boundary : wall1 4.6752E07 Boundary : wall2 2.5518E07 Domain Interface : flowinterface (Side 1) 2.1295E+01 Domain Interface : flowinterface (Side 2) 2.1295E+01  Domain Imbalance : 0.0000E+00 ++  Normalised Imbalance Summary  ++  Equation  Maximum Flow  Imbalance (%)  ++  UMom  9.5685E07  0.0000   VMom  9.5685E07  0.0000   WMom  9.5685E07  0.0001   PMass  5.0000E05  0.0000  ++++  HEnergy  2.1295E+01  0.0000  ++++ ================================================== ==================== Wall Force and Moment Summary ================================================== ==================== Notes: 1. Pressure integrals exclude the reference pressure. To include it, set the expert parameter 'include pref in forces = t'. ++  Pressure Force On Walls  ++ XComp. YComp. ZComp. Domain Group: fluid wall1 2.6798E07 4.6238E08 1.6137E14 wall2 2.6924E07 3.1800E07 1.3205E14    Domain Group Totals : 5.3722E07 3.6424E07 2.9342E14 ++  Viscous Force On Walls  ++ XComp. YComp. ZComp. Domain Group: fluid wall1 9.5143E08 8.4900E08 1.9065E12 wall2 9.5474E08 8.5001E08 1.8132E13    Domain Group Totals : 1.9062E07 1.0117E10 1.7252E12 ++  Pressure Moment On Walls  ++ XComp. YComp. ZComp. Domain Group: fluid wall1 2.3120E11 1.3400E10 2.2199E09 wall2 1.5900E10 1.3462E10 9.5425E09    Domain Group Totals : 1.8212E10 2.6861E10 7.3226E09 ++  Viscous Moment On Walls  ++ XComp. YComp. ZComp. Domain Group: fluid wall1 4.2424E11 4.7569E11 1.1452E09 wall2 4.2503E11 4.7738E11 1.8926E09    Domain Group Totals : 7.8219E14 9.5307E11 7.4737E10 ++  Locations of Maximum Residuals  ++  Equation  Domain Name  Node Number  ++  UMom  fluid  1393   VMom  fluid  1475   WMom  fluid  1003   PMass  fluid  1386  ++++  HEnergy  fluid  2624  ++++ ================================================== ====================  False Transient Information  ++  Equation  Type  Elapsed PseudoTime  ++  UMom  Auto Timescale  2.64824E+02   VMom  Auto Timescale  2.64824E+02   WMom  Auto Timescale  2.64824E+02  ++++  HEnergy  Auto Timescale  2.64824E+02  ++++ ++  Average Scale Information  ++ Domain Name : fluid Global Length = 6.8511E03 Minimum Extent = 1.0000E03 Maximum Extent = 4.0000E02 Density = 9.9700E+02 Dynamic Viscosity = 8.8990E04 Velocity = 7.0714E03 Advection Time = 9.6885E01 Reynolds Number = 5.4277E+01 Thermal Conductivity = 6.0690E01 Specific Heat Capacity at Constant Pressure = 4.1817E+03 Prandtl Number = 6.1316E+00 Temperature Range = 1.5259E04 ++  Variable Range Information  ++ Domain Name : fluid ++  Variable Name  min  max  ++  Density  9.97E+02  9.97E+02   Specific Heat Capacity at Constant Pressure 4.18E+03  4.18E+03   Dynamic Viscosity  8.90E04  8.90E04   Thermal Conductivity  6.07E01  6.07E01   Static Entropy  1.23E+03  1.23E+03   Velocity u  1.58E03  1.29E02   Velocity v  8.31E03  8.32E03   Velocity w  1.61E05  1.20E05   Pressure  5.27E02  1.18E01   Temperature  4.00E+02  4.00E+02   Static Enthalpy  4.26E+05  4.26E+05  ++ ++  CPU Requirements of Numerical Solution  ++ Subsystem Name Discretization Linear Solution (secs. %total) (secs. %total)  Momentum and Mass 3.76E+01 51.2 % 5.60E+00 7.6 % Heat Transfer 1.34E+01 18.3 % 2.35E+00 3.2 %     Subsystem Summary 5.10E+01 69.5 % 7.95E+00 10.8 % Variable Updates 1.11E+01 15.1 % GGI Intersection 1.00E03 0.0 % Search Calculations 9.99E04 0.0 % File Reading 4.00E03 0.0 % File Writing 4.70E02 0.1 % Miscellaneous 3.26E+00 4.4 %  Total 7.34E+01 ++  Job Information at End of Run  ++ Host computer: ZCPC (PID:6112) Job finished: Mon Dec 19 10:32:20 2016 Total wall clock time: 7.336E+01 seconds or: ( 0: 0: 1: 13.364 ) ( Days: Hours: Minutes: Seconds ) End of solution stage. ++  The results from this run of the ANSYS CFX Solver have been   written to E:/Workbench files/Tutorial_Periodic   Flow_pending/dp0_CFX_2_Solution_8/Fluid Flow CFX_001.res  ++ ++  For CFX runs launched from Workbench, the final locations of   directories and files generated may differ from those shown.  ++ This run of the ANSYS CFX Solver has finished. Not sure whether this will help or not. 

December 18, 2016, 23:58 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
You are right, you cannot do temperature control in translation periodic boundaries.
No matter, with a source term you can do anything . Put a source term on the upstream periodic face (under the "Sources" tab) and make it pull the temperature back to 300K. Set a total source term to C*(T300[K]) and a source term coefficient of C. Define the CEL expression C as a large number, maybe 1000000. Some discussion about doing similar things with source terms: Simulation of Axial Fan Flow using A Momentum Source Subdomain 

December 19, 2016, 04:46 

#6  
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
Quote:
I also have tried this in CFX either at the inlet face boundary source or outlet face boundary source, While the outlet source case result seems similiar but still not right. 

December 19, 2016, 05:11 

#7  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
The outlet case is giving the results I expect. I am not sure why the inlet case did not converge  are you using a total energy model or just thermal energy?
I don't know what the fluent temperature results mean. I don't understand what they are showing. It does not appear to be the temperature of the first row, or the temperature of the nth row (which is just everything at 400K, as the CFX result showed). So what is it? Source terms are terms added to the equation which can be used to modify things by adding or removing energy/momentum or whatever the conservation equation is conserving. In this case it adds or removes an amount of energy required to return the air to 300K. So the air comes out at 300K. Quote:


December 19, 2016, 07:19 

#8  
Senior Member
Join Date: Feb 2011
Posts: 491
Rep Power: 13 
Quote:


December 19, 2016, 07:28 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
The help for fluent states that t_bulk "sets the inlet bulk temperature for periodic heat transfer calculations"  that does not expand my knowledge very much.
I don't understand what Fluent has done such that some of the inlet boundary is not at 300K. And I can't see what the difference between the bulk temp and the inlet temp is when you have only got the inlet to define it at. If the flow is compressible it could be the total temperature  but the Fluent document says this approach is not valid for compressible flows, and the velocities in this example are low so that does not seem applicable. 

December 19, 2016, 07:33 

#10 
Senior Member
Join Date: Feb 2011
Posts: 491
Rep Power: 13 
Try to refer to section 13.4 (13.4.2) of Fluent Users's Guide.


December 19, 2016, 09:33 

#11 
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
It took me ages to upload some pictures about this from the fluent help, bad network.
The case is incompressive, so I just use the thermal energy. From the fluent result, I guess the temperature result is the "first row" result, which I am not sure about that. I got some screenshot here explaining how fluent deal with this problem. It seems the fluent result is reasonable. Still, Horrocks, thanks for your explaination about the source. I can understand why add the source, but still can not understand how can this be achieved by adding this source term to the energy equation. How do this manage to pull the collant output temperature to 300K? Confused. 

December 19, 2016, 16:58 

#12 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
I see what Fluent is doing now. It is not modelling temperature but models a scaled temperature. Thanks for clarifying that.
The CFX model you did before is the first row result. CFX has no built in equivalent of the scaled temperature but I think you will be able to model it by defining scaled temperature as a user variable and applying the conditions specified in the Fluent manual. 

December 19, 2016, 17:00 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
The source term gets the temperature difference from 300K and applies heat (or cooling) to get the temperature back to 300K.


December 19, 2016, 20:52 

#14 
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
But the last page about the postprocessing of the temperature results says the result is actual temperature; if it is the scaled one, it should be periodic in the flow direction, but it's not.
Also the fluent tutorial explains the temperature field this way "The contours in Figure 4.5 reveal the temperature increase in the fluid due to heat transfer from the tubes. The hotter fluid is confined to the nearwall and wake regions, while a narrow stream of cooler fluid is convected through the tube bank." It can be seen from the first page of my last post. 

December 19, 2016, 21:58 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
It looks like they have converted the scaled temperature back to real temperature for the post processing using eqn 1421 from your post. That is why it is not periodic.


December 19, 2016, 22:05 

#16 
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
Yeah I guess so, I'll try the additional variable to see whether it can achieve the same goal Thanks Horrocks


December 20, 2016, 12:46 

#17 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 921
Rep Power: 18 
Going along with what Glenn suggested, making the inlet 300K. I believe you want the energy source term to be uniform at the interface, meaning cool all the fluid by the same amount, don't make it the same temperature.
Say you set this to take 100 Watts out @ the interface uniformly, then your fluid temperature will converge on where you would have 100W of heat transfer. You can monitor this, and change it on the fly in the solve manager until your bulk temperature is 300K, or whatever you want it to be. You could also find a nice curve for bulk temperature vs heat transfer. Maybe you already knew that, it was a pretty long/detailed post with a lot of good ideas floating around. 

December 20, 2016, 17:28 

#18 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
Good idea Erik. If you make the source term an even 100W (or whatever the amount should be) you should get results equivalent to the Fluent one.


December 20, 2016, 23:53 

#19 
Member
Join Date: Dec 2016
Posts: 31
Rep Power: 5 
Hi Erik, it seems you proposed a promising way to do this, I get what you mean, but I do not quite understand how to achieve that. Could you please explain it in detail? or any reference thread. I find it difficult to look for the related post without understand it.
How can I specify the fluid is cooled by the same amount? yeah, the inlet temperature profile (not the uniform 300K) should be something associated with the velocity profile, with its bulk temperature is 300K. How can I get that inlet temperature profile? In the fluent results, everypoint temperature value in the outlet is the corresponding point temperature value in the inlet plus the same delta T. Horrocks, I don't manage to achieve this using the additional variables. You can see the eqution 1422 in former post picture, I guess I need to find the T profile of the inlet, while knowing the velocity profile and bulk temperature. Kind of impossible to do this with out using fortran to do some iteration work. Any convenient idea? 

December 21, 2016, 00:40 

#20 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123 
Erik's idea is much simpler so I suggest you do that. Put a source term on the inlet or outlet boundary face set to a flux of 100[W] or whatever heat loss is appropriate (although you might need need to convert that to W/m^2 or similar to get the units right), and zero source term coefficient. This will replace the previous suggestion of a total source term set to C(T300[K]).


Tags 
heat transfer, periodic boundary 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Radiation in semitransparent media with surfacetosurface model?  mpeppels  CFX  11  August 22, 2019 08:30 
Error  Solar absorber  Solar Thermal Radiation  MichaelK  CFX  12  September 1, 2016 06:15 
dieselFoam problem!! trying to introduce a new heat transfer model  vivek070176  OpenFOAM Programming & Development  10  December 24, 2014 00:48 
Radiation interface  hinca  CFX  15  January 26, 2014 18:11 
Error finding variable "THERMX"  sunilpatil  CFX  8  April 26, 2013 08:00 