[Y27]

Hi, thanks for taking the time to read my post!

As far as I am aware, CHT is used for regions of differing nature such as solid-fluid and solid-porous. However, I am attempting to simulate heat transfer across multiple solid-solid interfaces (Conduction) before finally encountering a liquid interface at the centre. This is done in a concentric fashion. I have made a small 2D diagram shown in the file below to help demonstrate this.

Regions-Boundaries.jpg

I want to apply a constant heat flux of 0.1 W/m^2 at the first solid-solid boundary, which then conducts thermal energy through the consecutive solid layers according to their material properties, until it reaches the liquid.

I can use the CHT with segregated flow and energy solvers to set up the simulation but this seems wrong as I want the source of heat flux to be at a solid-solid boundary, not at the fluid-solid boundary (Correct me if i am wrong and this is sufficient).

I then made a very simple model consisting of one solid cylinder imprinted on an another solid cylinder and used the finite element solid energy model to test if I could set the heat flux across the solid-solid interface. The physics model allowed me to set the heat flux at the boundaries - but not at the interface as there was no option to define the the thermal specification at all. However, i monitored the heat flux at the boundary using the field function "Boundary heat flux" and the value was very large compared to the values I inputted (specifying negative for heat flux leaving the boundary and positive for incoming). I lowered the temperature difference between solid parts which reduced the heat flux (still no where near the value specified). I would like the heat flux to be independent, is this possible using finite element solid energy?

Using CHT, I can easily solve this at the interface with the following equation which makes both temperature and heat flux independent variables, providing an input value for the contact resistance to be defined.

heat flux eqn.jpg

However, with Fe solid energy the energy equation differs from this.

I feel like I am missing something relatively simple. I am more than happy to re-read the guide if anyone can point in me in the right direction i would be very grateful!

If I missed something please let me know and I will be happy to post it, thanks!

[ping]

i have no experience with the star FE solver but know you can certainly do what you have described with the FV solver and can use either the contact or mapped interface at your solid-solid contacts and within these interfaces add energy heat flux or source values - see this help page:
Pre-Processing > Defining the Regions Layout > Interfaces Overview > Contact Interface - looks like where you got the equation from?
to speed up solid solving ensure you set the energy under relaxation factor to .99999 with the seg.solver.

[Y27]

Originally Posted by ping

i have no experience with the star FE solver but know you can certainly do what you have described with the FV solver and can use either the contact or mapped interface at your solid-solid contacts and within these interfaces add energy heat flux or source values - see this help page:
Pre-Processing > Defining the Regions Layout > Interfaces Overview > Contact Interface - looks like where you got the equation from?
to speed up solid solving ensure you set the energy under relaxation factor to .99999 with the seg.solver.

Thanks for your reply, using the FV solver is definitely the way forward. Where I am confused now is how to set up the physics at the boundaries and interfaces.

I want to specify a constant heat flux of 0.1 W/m^2 at the ID of the outer solid - which then supplies all of the thermal energy for heating the other solid parts and also the fluid. I created a report to show the heat flux at the outer solids ID wall was correct. However, the issue I am facing is how to correctly define the thermal specification at the boundary and/or interface.

For example;

At the fluid-solid interface, a contact resistance is required - but I do not know the temperature of the solid after initialisation because it changes with time. Should the value of the contact resistance be based on initial temperature conditions, will it update the value within the solvers during the simulation - even with the prescribed "constant" setting? Do I need to define some kind of function which calculates (temp.1 - temp.2) and the heat flux - and apply that at the contact resistance?

Also,

For the initial heat flux of 0.1 W/m^2 at the outer solid ID - when I set it at the interface I get values on either side ([1], [0]) which add up to the specified values (0.15 and -0.05), however, I want Boundary [1] to yield a value of 0.1, not 0.15. I also tried to define the heat flux using the "Boundary heat flux" field function at the interface where the value was defined at the region boundary for the outer solid ID wall - which was set to a heat flux of 0.1 W/m^2. This made both sides of the interface have a constant value 0.1 W/m^2. Is this a case of me misinterpreting the data or is there something fundamental I am missing?

In order to fulfil the criteria I would need to configure all other interfaces so that they become passive to the heat flux supplied in the outer boundary. I have attempted many ways of doing this and have managed to get some good results but also some bad which appear to break the 2nd law of thermodynamics. What are the recommended settings for this type of heat transfer - do I need to define the heat flux at every boundary and/or interface or just where the source of heat is occurring? I can't find one tutorial or help guide that explains this comprehensively and concisely - I have been trying to piece together the many bits of information on interfaces , boundaries and regions etc., but I have no way to verify if the results I am getting are based on sound physics or not.

Apologies for the long reply - any push in the right direction is much appreciated, thank you!

If you need me to update or include any other data/plots in this post I'll be happy to do so.

[ping]

Originally Posted by Y27

At the fluid-solid interface, a contact resistance is required - but I do not know the temperature of the solid after initialisation because it changes with time. Should the value of the contact resistance be based on initial temperature conditions, will it update the value within the solvers during the simulation - even with the prescribed "constant" setting? Do I need to define some kind of function which calculates (temp.1 - temp.2) and the heat flux - and apply that at the contact resistance?

are you sure you need a contact resistance or are you just misinterpreting the help? I suggest you ignore this setting, but if you need it then the temps are taken from the cells adjacent. you dont need heat flux there since you said the only input was at the inner wall of the outer solid.

Originally Posted by Y27

For the initial heat flux of 0.1 W/m^2 at the outer solid ID - when I set it at the interface I get values on either side ([1], [0]) which add up to the specified values (0.15 and -0.05), however, I want Boundary [1] to yield a value of 0.1, not 0.15. I also tried to define the heat flux using the "Boundary heat flux" field function at the interface where the value was defined at the region boundary for the outer solid ID wall - which was set to a heat flux of 0.1 W/m^2. This made both sides of the interface have a constant value 0.1 W/m^2. Is this a case of me misinterpreting the data or is there something fundamental I am missing?

this sounds wrong and you are overcomplicating such simple concepts and menus - heat flux is heat flux and it will flow into both adjacent solids - nothing to do with boundary sides.

boundary heat flux is a system field function that is calculated and reported with and cant be set and should be used to measure what is happening at other boundaries and interfaces.

Originally Posted by Y27

In order to fulfil the criteria I would need to configure all other interfaces so that they become passive to the heat flux supplied in the outer boundary. I have attempted many ways of doing this and have managed to get some good results but also some bad which appear to break the 2nd law of thermodynamics.

contact interfaces with solids are simple and the only thing that can go wrong is that the interface is poor ie your part prep., imprinting and meshing has let you down but this will not affect the 2nd law, but simply not transfer as much heat ie creates some resistance. so check your interfaces carefully and if having trouble getting conformal meshing then change them to mapped contact interfaces. your 2nd law problem is probably a lack of convergence - set up some temperature monitor points in the middle of each of your solids and in the fluid and at the fluid outlet and plot these till they converge. and remember to set the energy solver under relaxation factor to 0.999999 to speed convergence.

Originally Posted by Y27

What are the recommended settings for this type of heat transfer - do I need to define the heat flux at every boundary and/or interface or just where the source of heat is occurring?

no - as I said it is dead simple doing these types of cases - you only put heat in or out where you want it added or subtracted and no other settings are required on a simple contact interface.

Originally Posted by Y27

I can't find one tutorial or help guide that explains this comprehensively and concisely - I have been trying to piece together the many bits of information on interfaces , boundaries and regions etc., but I have no way to verify if the results I am getting are based on sound physics or not.

for some the cad and part prep. work required see this one but also ensure you are imprinting all your surfaces: Tutorials > Mesh > Meshing: Multi-Part Heat Exchanger

the first few in this large group will help on the thermal side: Tutorials > Heat Transfer and Radiation

[Y27]

Hi,

Thanks for going to all the trouble to reply. I really appreciate it!

Originally Posted by ping

are you sure you need a contact resistance or are you just misinterpreting the help? I suggest you ignore this setting, but if you need it then the temps are taken from the cells adjacent. you dont need heat flux there since you said the only input was at the inner wall of the outer solid.

If i set the interface thermal spec. to Conjugate Heat Transfer, a node for contact resistance appears underneath.

Attachment 79618


If it is set to "Specified Temperature", the contact resistance option goes away and a Static temperature node appears.


Attachment 79619


Are you suggesting I leave the contact resistance as the default value of 0, or should I switch to specified temperature and enter the initial temperature from the physics continuum? They are the only options available to me.

Originally Posted by ping

this sounds wrong and you are overcomplicating such simple concepts and menus - heat flux is heat flux and it will flow into both adjacent solids - nothing to do with boundary sides.

boundary heat flux is a system field function that is calculated and reported with and cant be set and should be used to measure what is happening at other boundaries and interfaces.

Yes, this makes sense now. Thank you!

Originally Posted by ping

contact interfaces with solids are simple and the only thing that can go wrong is that the interface is poor ie your part prep., imprinting and meshing has let you down but this will not affect the 2nd law, but simply not transfer as much heat ie creates some resistance. so check your interfaces carefully and if having trouble getting conformal meshing then change them to mapped contact interfaces. your 2nd law problem is probably a lack of convergence - set up some temperature monitor points in the middle of each of your solids and in the fluid and at the fluid outlet and plot these till they converge. and remember to set the energy solver under relaxation factor to 0.999999 to speed convergence.

I believe the problem was stemming from the contact resistance at the fluid-solid interface. Without entering a value for this contact resistance I end up with a heat flux that is larger than the input heat flux value at the outer solid ID. Oh, and my apologies - I meant 1st law, not that it matters as I am clearly configuring my set up incorrectly is what the issue is.

Originally Posted by ping

no - as I said it is dead simple doing these types of cases - you only put heat in or out where you want it added or subtracted and no other settings are required on a simple contact interface.

So what setting do i choose at the region boundaries thermal specification? If i leave them as the default "adiabatic" this implies no energy transfer occurs. Whereas, all other settings require some scalar value input - which i do not want to do as I want the solvers to do work them out for me. I have tried setting them as heat flux on the solid boundaries (requires scalar input - when I want it to be solved for), Attachment 79621

and convection for the fluid wall (requires ambient temp. and heat trans. coeff.). As you said this is a simple case, and I have definitely made a meal out of it. Attachment 79620

Originally Posted by ping

for some the cad and part prep. work required see this one but also ensure you are imprinting all your surfaces: Tutorials > Mesh > Meshing: Multi-Part Heat Exchanger

the first few in this large group will help on the thermal side: Tutorials > Heat Transfer and Radiation.

Thank you, the tutorial for multi-timescale CHT was particularly useful, although, in the tutorial, all boundaries are assigned the "convection" condition - and the required parameters (ambient temp. and heat trans. coeff.) are already known.


Apologies if I have given killed your soul with my questions.

[ping]

you have said you want just simple conjugate heat transfer across the interface with no contact resistance so leave this as zero and then the temperature setting is not presented to you.

for your last question about adiabatic, the attachment is said to be invalid so i cant see. but for each boundary you need to decide what the settings should be and if adiabatic is not representative of what you need (eg it is not well insulated) on say an external boundary then decide of something different and in most cases convection is probably a good choice. then you just need to guesstimate a heat transfer coef. and an external air temperature for example.

[Y27]

Hi, apologies for the late reply - I have been very preoccupied. I did however manage to find what I was looking for in another post which I have shared below in case anyone else has the same problem. The member who posted is "Abdul099".

Thank you for your responses Ping, they now make perfect sense to me, I apologise that I was unable to phrase my questions in a manner which clearly stated what i wanted to understand. Your time was and is much appreciated!!

Thermal specification for CHT.