how to explain the temperature gap on solid-fluid interface

vicder · November 1, 2016, 01:59

Hi guys,

Recently , Because of my research , I need to use heat transfer simulation and I have a question.

My simulation is about iron block heating , so I create two domains that the material of one is steel , the other is air in CFX.The heat transfer model is thermal energy.The analysis type is steady.

About the boundary condition , I put temperature 1000C on bottom of the air domain and Heat transfer Coef. 2W.m^-2K^-1 on top of steel domain.

Besides , the interface between two domains is assumed to be solid-fluid interface and heat transfer option is Conservative Interface Flux , interface model is none.

Based on the setting as above , the result as my attachment shows that there is a temperature gap across interface. In my opinion , it should be changing gradually across interface , not a gap of temperature across interface. How do I understand it?

This phenomenon is related to Thermal Contact Conductance?Or is this the other way to explain this?

Thank you!

ypBvPyT.jpg

uutBawB.jpg

ghorrocks · November 1, 2016, 17:57

I assume the bottom block is the steel and the top block is air.

If so, why did you specify a heat transfer coefficient on top of the steel? This will mean it does not use an interface between the steel and air. You should remove the heat transfer coefficient and let CFX calculate the heat transfer at the interface.

Also - are you sure your simulation is converged? Note that residuals are not a good measure of convergence for CHT simulations like this. Imbalances is a better measure of convergence.

vicder · November 2, 2016, 04:42

Thank you for reply!

I have checked my model and make sure that the bottom block is the air and the top block is the steel. About the Imbalances measure , I will try it.

However, I mesh two blocks again with smaller mesh size and there is a temperature gap across interface too. Attachment is about the new graph and temperature data along the yellow line.

In my new result , is it reasonable?
Is it related to thermal contact conductance?

14895574_1322742927804211_1337246887_o.jpg
14886316_1322742897804214_632992499_n.jpg

ghorrocks · November 2, 2016, 05:07

Have you modelled thermal contact resistance? If you have not put a model in for it then no, it is not thermal contact resistance.

Please attach an image of your mesh, label the bodies. Also attach your output file.

Opaque · November 2, 2016, 08:47

Your current solution does not seem converged for a steady state heat transfer between 2 distinct materials.

You are trying to understand your model, and verify if it is correct. Here is some basic steps

Set top boundary condition to same temperature at the bottom.
Is the solution isothermal ? No? Review setup and convergence level

Set thermal conductivity to the same value on both materials, and top boundary at a fixed temperature
Is the solution a linear profile across both materials ? No? Review setup and convergence level.

Keep material properties as you intend to run the simulation, keep top boundary at fixed temperature
Is the solution a linear profile within each block, but different slopes each ? No ? Review setup, and convergence level

If the above is satisfied, and you still see a small temperature gap on step 3, review CFX discretization theory, difference between conservative values and hybrid values.

Hope the above helps,

vicder · November 2, 2016, 09:14

Thanks for reply.

To ghorrocks,

Indeed , I haven't modelled thermal conduct resistance. Follow your suggestion , I redo my simulation with imbalance criteria and the result is as the same as my first simulation almost.

The attachment contains that mesh of my model , new result of temperature distribution , the temperature data chart along yellow line and output file in txt format.

To Opaque,

Thanks for your suggestion, I'll try it in my free time.

Mesh.JPG
Graph.JPG
Temperature Data.JPG
OutputFile.txt

ghorrocks · November 2, 2016, 18:10

Your output file is strange and appears to have some fundamental problems.

- You have an inlet boundary on the air domain which is actually a wall at 1000C. Are you sure this is what you intended?
- Despite very high temperatures you have not activated a buoyancy model. And there are no inlets or outlets so this means there is nothing to drive the flow. So the air is stationary. Are you sure this is what you intended?
- Your steel domain has a convective boundary to 25C and other walls which are adiabatic.
- Also your domain inbalances are miles off indicating this is not converged.

Opaque · November 2, 2016, 20:19

You have a setup with no flow; therefore, use the laminar flow model and you will get the correct solution.

You are using a RANS model for a no flow condition, and the turbulence wall function does not reproduce the laminar boundary layer behavior. You are seeing the heat transfer wall function behavior at the walls

Hope the above helps,

vicder · November 3, 2016, 05:59

Based on suggestions of ghorrocks and Opaque , the result of simulation is more reasonable and my problem has been solved.

Thanks for your information.

November 1, 2016, 01:59	how to explain the temperature gap on solid-fluid interface	#1
vicder New Member Join Date: Nov 2016 Posts: 7 Rep Power: 10	Hi guys, Recently , Because of my research , I need to use heat transfer simulation and I have a question. My simulation is about iron block heating , so I create two domains that the material of one is steel , the other is air in CFX.The heat transfer model is thermal energy.The analysis type is steady. About the boundary condition , I put temperature 1000C on bottom of the air domain and Heat transfer Coef. 2W.m^-2K^-1 on top of steel domain. Besides , the interface between two domains is assumed to be solid-fluid interface and heat transfer option is Conservative Interface Flux , interface model is none. Based on the setting as above , the result as my attachment shows that there is a temperature gap across interface. In my opinion , it should be changing gradually across interface , not a gap of temperature across interface. How do I understand it? This phenomenon is related to Thermal Contact Conductance?Or is this the other way to explain this? Thank you! ypBvPyT.jpg uutBawB.jpg Last edited by vicder; November 1, 2016 at 03:18. Reason: Additional details

November 2, 2016, 08:47		#5
Opaque Senior Member Join Date: Jun 2009 Posts: 1,880 Rep Power: 33	Your current solution does not seem converged for a steady state heat transfer between 2 distinct materials. You are trying to understand your model, and verify if it is correct. Here is some basic steps Set top boundary condition to same temperature at the bottom. Is the solution isothermal ? No? Review setup and convergence level Set thermal conductivity to the same value on both materials, and top boundary at a fixed temperature Is the solution a linear profile across both materials ? No? Review setup and convergence level. Keep material properties as you intend to run the simulation, keep top boundary at fixed temperature Is the solution a linear profile within each block, but different slopes each ? No ? Review setup, and convergence level If the above is satisfied, and you still see a small temperature gap on step 3, review CFX discretization theory, difference between conservative values and hybrid values. Hope the above helps,

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
sliding mesh problem in CFX	Saima	CFX	46	September 11, 2021 08:38
Centrifugal fan	j0hnny	CFX	13	October 1, 2019 14:55
Closed Domain Buoyancy Flow Problem	Madhatter92	CFX	6	June 20, 2016 22:05
Radiation interface	hinca	CFX	15	January 26, 2014 18:11
Water subcooled boiling	Attesz	CFX	7	January 5, 2013 04:32

November 1, 2016, 17:57		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	I assume the bottom block is the steel and the top block is air. If so, why did you specify a heat transfer coefficient on top of the steel? This will mean it does not use an interface between the steel and air. You should remove the heat transfer coefficient and let CFX calculate the heat transfer at the interface. Also - are you sure your simulation is converged? Note that residuals are not a good measure of convergence for CHT simulations like this. Imbalances is a better measure of convergence.

November 2, 2016, 04:42		#3
vicder New Member Join Date: Nov 2016 Posts: 7 Rep Power: 10	Thank you for reply! I have checked my model and make sure that the bottom block is the air and the top block is the steel. About the Imbalances measure , I will try it. However, I mesh two blocks again with smaller mesh size and there is a temperature gap across interface too. Attachment is about the new graph and temperature data along the yellow line. In my new result , is it reasonable? Is it related to thermal contact conductance? 14895574_1322742927804211_1337246887_o.jpg 14886316_1322742897804214_632992499_n.jpg

November 2, 2016, 05:07		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	Have you modelled thermal contact resistance? If you have not put a model in for it then no, it is not thermal contact resistance. Please attach an image of your mesh, label the bodies. Also attach your output file.

November 2, 2016, 09:14		#6
vicder New Member Join Date: Nov 2016 Posts: 7 Rep Power: 10	Thanks for reply. To ghorrocks, Indeed , I haven't modelled thermal conduct resistance. Follow your suggestion , I redo my simulation with imbalance criteria and the result is as the same as my first simulation almost. The attachment contains that mesh of my model , new result of temperature distribution , the temperature data chart along yellow line and output file in txt format. To Opaque, Thanks for your suggestion, I'll try it in my free time. Mesh.JPG Graph.JPG Temperature Data.JPG OutputFile.txt

November 2, 2016, 18:10		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	Your output file is strange and appears to have some fundamental problems. - You have an inlet boundary on the air domain which is actually a wall at 1000C. Are you sure this is what you intended? - Despite very high temperatures you have not activated a buoyancy model. And there are no inlets or outlets so this means there is nothing to drive the flow. So the air is stationary. Are you sure this is what you intended? - Your steel domain has a convective boundary to 25C and other walls which are adiabatic. - Also your domain inbalances are miles off indicating this is not converged.

November 2, 2016, 20:19		#8
Opaque Senior Member Join Date: Jun 2009 Posts: 1,880 Rep Power: 33	You have a setup with no flow; therefore, use the laminar flow model and you will get the correct solution. You are using a RANS model for a no flow condition, and the turbulence wall function does not reproduce the laminar boundary layer behavior. You are seeing the heat transfer wall function behavior at the walls Hope the above helps,

November 3, 2016, 05:59		#9
vicder New Member Join Date: Nov 2016 Posts: 7 Rep Power: 10	Based on suggestions of ghorrocks and Opaque , the result of simulation is more reasonable and my problem has been solved. Thanks for your information.