CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Can CFX model periodic heat transfer problem

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 18, 2016, 09:48
Default Can CFX model periodic heat transfer problem
  #1
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
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.
Ethan_Sparkle is offline   Reply With Quote

Old   December 18, 2016, 18:03
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   December 18, 2016, 22:55
Default
  #3
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
Hi Horrocks, really thank you for your reply.
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.
Ethan_Sparkle is offline   Reply With Quote

Old   December 18, 2016, 23:04
Default
  #4
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
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
================================================== ====================

+--------------------------------------------------------------------+
| U-Mom |
+--------------------------------------------------------------------+
Boundary : symmetry34 1.7396E-23
Boundary : wall1 -3.6313E-07
Boundary : wall2 -3.6471E-07
Domain Interface : flowinterface (Side 1) 9.5685E-07
Domain Interface : flowinterface (Side 2) -2.2901E-07
-----------
Domain Imbalance : 1.2790E-13

+--------------------------------------------------------------------+
| V-Mom |
+--------------------------------------------------------------------+
Boundary : symmetry1 -4.6013E-07
Boundary : symmetry2 4.8665E-08
Boundary : symmetry34 7.7580E-07
Boundary : wall1 3.8661E-08
Boundary : wall2 -4.0300E-07
Domain Interface : flowinterface (Side 1) -9.2033E-08
Domain Interface : flowinterface (Side 2) 9.2033E-08
-----------
Domain Imbalance : 1.4211E-13

+--------------------------------------------------------------------+
| W-Mom |
+--------------------------------------------------------------------+
Boundary : sym12 -6.8212E-13
Boundary : symmetry34 -3.4704E-26
Boundary : wall1 1.9230E-12
Boundary : wall2 -1.6828E-13
Domain Interface : flowinterface (Side 1) 1.3119E-11
Domain Interface : flowinterface (Side 2) -1.3119E-11
-----------
Domain Imbalance : 1.0726E-12

+--------------------------------------------------------------------+
| P-Mass |
+--------------------------------------------------------------------+
Domain Interface : flowinterface (Side 1) 5.0000E-05
Domain Interface : flowinterface (Side 2) -5.0000E-05
-----------
Domain Imbalance : 0.0000E+00

+--------------------------------------------------------------------+
| H-Energy |
+--------------------------------------------------------------------+
Boundary : wall1 4.6752E-07
Boundary : wall2 2.5518E-07
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 (%) |
+--------------------------------------------------------------------+
| U-Mom | 9.5685E-07 | 0.0000 |
| V-Mom | 9.5685E-07 | 0.0000 |
| W-Mom | 9.5685E-07 | 0.0001 |
| P-Mass | 5.0000E-05 | 0.0000 |
+----------------------+-----------------------+---------------------+
| H-Energy | 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 |
+--------------------------------------------------------------------+
X-Comp. Y-Comp. Z-Comp.

Domain Group: fluid

wall1 2.6798E-07 4.6238E-08 -1.6137E-14
wall2 2.6924E-07 3.1800E-07 -1.3205E-14
----------- ----------- -----------
Domain Group Totals : 5.3722E-07 3.6424E-07 -2.9342E-14


+--------------------------------------------------------------------+
| Viscous Force On Walls |
+--------------------------------------------------------------------+
X-Comp. Y-Comp. Z-Comp.

Domain Group: fluid

wall1 9.5143E-08 -8.4900E-08 -1.9065E-12
wall2 9.5474E-08 8.5001E-08 1.8132E-13
----------- ----------- -----------
Domain Group Totals : 1.9062E-07 1.0117E-10 -1.7252E-12


+--------------------------------------------------------------------+
| Pressure Moment On Walls |
+--------------------------------------------------------------------+
X-Comp. Y-Comp. Z-Comp.

Domain Group: fluid

wall1 -2.3120E-11 1.3400E-10 -2.2199E-09
wall2 -1.5900E-10 1.3462E-10 9.5425E-09
----------- ----------- -----------
Domain Group Totals : -1.8212E-10 2.6861E-10 7.3226E-09


+--------------------------------------------------------------------+
| Viscous Moment On Walls |
+--------------------------------------------------------------------+
X-Comp. Y-Comp. Z-Comp.

Domain Group: fluid

wall1 4.2424E-11 4.7569E-11 -1.1452E-09
wall2 -4.2503E-11 4.7738E-11 1.8926E-09
----------- ----------- -----------
Domain Group Totals : -7.8219E-14 9.5307E-11 7.4737E-10


+--------------------------------------------------------------------+
| Locations of Maximum Residuals |
+--------------------------------------------------------------------+
| Equation | Domain Name | Node Number |
+--------------------------------------------------------------------+
| U-Mom | fluid | 1393 |
| V-Mom | fluid | 1475 |
| W-Mom | fluid | 1003 |
| P-Mass | fluid | 1386 |
+----------------------+-----------------------+---------------------+
| H-Energy | fluid | 2624 |
+----------------------+-----------------------+---------------------+

================================================== ====================
| False Transient Information |
+--------------------------------------------------------------------+
| Equation | Type | Elapsed Pseudo-Time |
+--------------------------------------------------------------------+
| U-Mom | Auto Timescale | 2.64824E+02 |
| V-Mom | Auto Timescale | 2.64824E+02 |
| W-Mom | Auto Timescale | 2.64824E+02 |
+----------------------+-----------------------+---------------------+
| H-Energy | Auto Timescale | 2.64824E+02 |
+----------------------+-----------------------+---------------------+

+--------------------------------------------------------------------+
| Average Scale Information |
+--------------------------------------------------------------------+

Domain Name : fluid
Global Length = 6.8511E-03
Minimum Extent = 1.0000E-03
Maximum Extent = 4.0000E-02
Density = 9.9700E+02
Dynamic Viscosity = 8.8990E-04
Velocity = 7.0714E-03
Advection Time = 9.6885E-01
Reynolds Number = 5.4277E+01
Thermal Conductivity = 6.0690E-01
Specific Heat Capacity at Constant Pressure = 4.1817E+03
Prandtl Number = 6.1316E+00
Temperature Range = 1.5259E-04

+--------------------------------------------------------------------+
| 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 | 8.90E-04 | 8.90E-04 |
| Thermal Conductivity | 6.07E-01 | 6.07E-01 |
| Static Entropy | 1.23E+03 | 1.23E+03 |
| Velocity u | -1.58E-03 | 1.29E-02 |
| Velocity v | -8.31E-03 | 8.32E-03 |
| Velocity w | -1.61E-05 | 1.20E-05 |
| Pressure | -5.27E-02 | 1.18E-01 |
| 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 1.00E-03 0.0 %
Search Calculations 9.99E-04 0.0 %
File Reading 4.00E-03 0.0 %
File Writing 4.70E-02 0.1 %
Miscellaneous 3.26E+00 4.4 %
--------
Total 7.34E+01

+--------------------------------------------------------------------+
| Job Information at End of Run |
+--------------------------------------------------------------------+

Host computer: ZC-PC (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.
Ethan_Sparkle is offline   Reply With Quote

Old   December 18, 2016, 23:58
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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*(T-300[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
ghorrocks is offline   Reply With Quote

Old   December 19, 2016, 04:46
Default
  #6
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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*(T-300[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
Hi Horrocks, thanks for your so quick reply. I have read the linked discussion and the momentum source section from the CFX help files. But still don't understand why a total source term -C*(T-300[K])is able to pull the inlet temperature to 300K. Could you please explain this a bit further? What does this mean when this source term is added to the energy equation? Many thanks.

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.
Ethan_Sparkle is offline   Reply With Quote

Old   December 19, 2016, 05:11
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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 n-th 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:
While the outlet source case result seems similar but still not right.
Yes, I agree. The Fluent result does not look right. If I have misunderstood the fluent result please explain it to me.
ghorrocks is offline   Reply With Quote

Old   December 19, 2016, 07:19
Default
  #8
Senior Member
 
Join Date: Feb 2011
Posts: 491
Rep Power: 13
Antanas is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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 n-th 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.



Yes, I agree. The Fluent result does not look right. If I have misunderstood the fluent result please explain it to me.
Maybe the problem is in that in Fluent you specify temperature in the bulk of fluid (i.e. upstream), but not on inlet periodic face, unlike you trying to do in CFX.
Antanas is offline   Reply With Quote

Old   December 19, 2016, 07:28
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   December 19, 2016, 07:33
Default
  #10
Senior Member
 
Join Date: Feb 2011
Posts: 491
Rep Power: 13
Antanas is on a distinguished road
Try to refer to section 13.4 (13.4.2) of Fluent Users's Guide.
Antanas is offline   Reply With Quote

Old   December 19, 2016, 09:33
Default
  #11
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
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.
Ethan_Sparkle is offline   Reply With Quote

Old   December 19, 2016, 16:58
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   December 19, 2016, 17:00
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The source term gets the temperature difference from 300K and applies heat (or cooling) to get the temperature back to 300K.
ghorrocks is offline   Reply With Quote

Old   December 19, 2016, 20:52
Default
  #14
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
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 near-wall 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.
Ethan_Sparkle is offline   Reply With Quote

Old   December 19, 2016, 21:58
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
It looks like they have converted the scaled temperature back to real temperature for the post processing using eqn 14-21 from your post. That is why it is not periodic.
ghorrocks is offline   Reply With Quote

Old   December 19, 2016, 22:05
Default
  #16
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
Yeah I guess so, I'll try the additional variable to see whether it can achieve the same goal Thanks Horrocks
Ethan_Sparkle is offline   Reply With Quote

Old   December 20, 2016, 12:46
Default
  #17
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 921
Rep Power: 18
evcelica is on a distinguished road
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.
evcelica is offline   Reply With Quote

Old   December 20, 2016, 17:28
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   December 20, 2016, 23:53
Default
  #19
Member
 
Join Date: Dec 2016
Posts: 31
Rep Power: 5
Ethan_Sparkle is on a distinguished road
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 14-22 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?
Ethan_Sparkle is offline   Reply With Quote

Old   December 21, 2016, 00:40
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,047
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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(T-300[K]).
ghorrocks is offline   Reply With Quote

Reply

Tags
heat transfer, periodic boundary

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Radiation in semi-transparent media with surface-to-surface 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


All times are GMT -4. The time now is 21:07.