# Direction of layers in shell conduction

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

 May 4, 2016, 07:19 Direction of layers in shell conduction #1 New Member   stefania Join Date: Feb 2016 Location: Italy Posts: 20 Rep Power: 8 Does anybody know what are the directions of the layers in shell conduction? I have two fluids divided by a solid. This solid has different materials with different properties. where does the first layer start? Near the fluid 1 or the fluid 2? Thanks a lot!

 May 5, 2016, 17:46 #2 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,112 Rep Power: 60 Does your simulation (i.e. your mesh) have two fluids separated by a solid? If so, then you should solve the heat transfer in the solid directly and not invoke the shell conduction model. The shell conduction model is for modelling the solid wall so that it does not have to be meshed explicitly. To use the shell conduction model, your domain should have two fluids separated by an interface. Actually, it will be a wall and shadow-wall that connects to the two regions. The exception to this is if you want to model thermal contact resistances at interfaces. I don't think the shell conduction model can be used with "different solids with different properties." It is a homogeneous substance with properties defined via the material properties in the materials pane. If you have different solids, then you should mesh the different solids explicitly and declare them as different substances. The first layer is always the layer closest to the surface. If your fluids are connected by an interface, then each fluid will have it's own surface (the wall and then shadow-wall). The wall will belong to one fluid (say fluid-1) and shadow-wall will belong to the other fluid (say fluid-2). The 1st layer of the wall will be closest to the surface of fluid 1. The 1st layer of shadow-wall will be closest to the surface of fluid 2.

May 6, 2016, 11:32
#3
New Member

stefania
Join Date: Feb 2016
Location: Italy
Posts: 20
Rep Power: 8
Quote:
 Originally Posted by LuckyTran Does your simulation (i.e. your mesh) have two fluids separated by a solid? If so, then you should solve the heat transfer in the solid directly and not invoke the shell conduction model. The shell conduction model is for modelling the solid wall so that it does not have to be meshed explicitly. To use the shell conduction model, your domain should have two fluids separated by an interface. Actually, it will be a wall and shadow-wall that connects to the two regions. The exception to this is if you want to model thermal contact resistances at interfaces. I don't think the shell conduction model can be used with "different solids with different properties." It is a homogeneous substance with properties defined via the material properties in the materials pane. If you have different solids, then you should mesh the different solids explicitly and declare them as different substances. The first layer is always the layer closest to the surface. If your fluids are connected by an interface, then each fluid will have it's own surface (the wall and then shadow-wall). The wall will belong to one fluid (say fluid-1) and shadow-wall will belong to the other fluid (say fluid-2). The 1st layer of the wall will be closest to the surface of fluid 1. The 1st layer of shadow-wall will be closest to the surface of fluid 2.
Thank you very much for your reply. I'm still studying the furnace and I would like to insert in my simulation the heat transfer through the walls. I created only the fluid domain for my simulation so I have the wall and shadow-wall. If I enable the shell conduction I can insert the layers of the wall with a specific material I defined in the material panel. I'm not sure what is the direction of the layers. In order to define the wall I chose the wall where the adjacent cell are referred to the furnace and I started from there for the stratification of my wall. I'm not sure that is correct.

The reason why I want to do that is because in the precedent simulation the temperature of my wall cool down immediatly with the contact of the air at ambient temperature. So I want to initialize the solution with a steady state simulation and then start a transient simulation with the opening of the door evaluating also the heat flux for conduction through the walls.

What do you suggest?

Thank you again.

 May 6, 2016, 12:41 #4 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,112 Rep Power: 60 The shell conduction model is a steady-state model. So there will be some inaccuracies because of this, in a transient simulation. It is a model. You can only specify 1 material per wall. So the maximum number of materials you can model using the shell conduction approach is 2 (1 for wall, and 1 for wall-shadow). The number of layers does not change this limitation. Just because you specify 200 layers does not mean you can have 200 different materials, it is still 1. Note that there is a shell conduction model option for both the wall and the wall-shadow. The 1st layer is nearest the wall that the shell is attached to. The 2nd layer is farther away from the 1st layer but still belongs to wall. It is nice and logical, why are you so confused by this? So here is an explicit example. If wall has 2 shells and wall-shadow has 3 shells then it looks something like this: fluid-1|wall|wall-shell 1|wall-shell 2| shadow-shell 3| shadow-shell 2| shadow-shell 1| wall-shadow|fluid-2 Also note that the shell conduction model uses virtual nodes (a virtual mesh) so that there is no real physical location of these cells. You can specify arbitrarily large thickness for the shell conduction model. chek321 likes this.

 May 9, 2016, 05:07 #5 New Member   stefania Join Date: Feb 2016 Location: Italy Posts: 20 Rep Power: 8 Thanks for your reply. I'm confused because if I select coupled for the wall and wall shadow, even if I select the layer starting from the wall for example, when I open wall shadow I have the same layers, so my question is, what is the real direction that fluent assigns to my wall? I didn't physically create the wall, is just virtual. I used the shell conduction in order to initialize my simulation. If I have a furnace at 1500 K I don't know how to impose the temperature gradient inside of my walls. For this reason I thought to initialize the solution with a steady state analyses and then start with a transient simulation. Should I create the real geometry of the walls to perform this simulation? Do you have any suggest for the evaluation of the radiating heat flux through the door? I tried with some simulation but they don't convince me at all. Thanks.

 May 9, 2016, 09:37 #6 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,112 Rep Power: 60 You should check out in the User's Guide: Shell Conduction Considerations (13.2.5 in v17 manual). For a two-sided wall, which is a little different than a normal wall. The 1st layer is closest to the wall. The n-th layer is closest to the shadow-wall. This is a very round-about way to impose initial conditions. But whatever. A simple custom field function would have allowed you to specify a linear temperature profile.

July 2, 2018, 06:51
#7
Member

Vignesh Lakshmanan
Join Date: Nov 2016
Posts: 79
Rep Power: 8
Quote:
 Originally Posted by LuckyTran The shell conduction model is a steady-state model. So there will be some inaccuracies because of this, in a transient simulation. It is a model. You can only specify 1 material per wall. So the maximum number of materials you can model using the shell conduction approach is 2 (1 for wall, and 1 for wall-shadow). The number of layers does not change this limitation. Just because you specify 200 layers does not mean you can have 200 different materials, it is still 1. Note that there is a shell conduction model option for both the wall and the wall-shadow. The 1st layer is nearest the wall that the shell is attached to. The 2nd layer is farther away from the 1st layer but still belongs to wall. It is nice and logical, why are you so confused by this? So here is an explicit example. If wall has 2 shells and wall-shadow has 3 shells then it looks something like this: fluid-1|wall|wall-shell 1|wall-shell 2| shadow-shell 3| shadow-shell 2| shadow-shell 1| wall-shadow|fluid-2 Also note that the shell conduction model uses virtual nodes (a virtual mesh) so that there is no real physical location of these cells. You can specify arbitrarily large thickness for the shell conduction model.
Dear Lucky Tran,

First of all, sorry for restarting the thread.

I am trying to design a heat sink for electronic components of an air conditioner outdoor unit.

Attached is the picture of the heat sink (computational geometry) with components (Heat sink is highlighted in color). The heat sink base is 3.5 mm thick , whereas the fins are 1.5 mm thick. I have no problems in modelling the fins with 1.5 mm thickness and have expected results.
The problem starts when I want to model triangular shaped fins (approximately triangle shape). In the picture, the thickness of the fins vary from 1.5 mm at top to 0.75 mm below. I am not able to mesh it satisfactorily. So I am thinking of modelling shell conduction. Now as per your explanation, if I model shell conduction, say 2 layers for both wall and shadow, do my shells look like this (Air is the only fluid)?

Is my understanding correct?

Thanks and Regards
Vignesh
Attached Images
 Picture1.png (35.4 KB, 53 views)

 July 2, 2018, 15:22 #8 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,112 Rep Power: 60 Yes that is the correct interpretation. But I don't think the layers will help with your triangular fin because it's a thin wall assumption (you can't change the cross-sectional area of the layers).

July 3, 2018, 01:26
#9
Member

Vignesh Lakshmanan
Join Date: Nov 2016
Posts: 79
Rep Power: 8
Quote:
 Originally Posted by LuckyTran Yes that is the correct interpretation. But I don't think the layers will help with your triangular fin because it's a thin wall assumption (you can't change the cross-sectional area of the layers).

The pic was just for interpretation purpose. I will be modelling the fins as surface bodies. So (according to the picture) both the wall and wall-shadow will be having shadow walls. I can give thickness as required to closely resemble a solid (with thickness 1.5) fin right.

But ya, you are right !!!! The cross-sectional area cant be changed. I have to model some other way

With Regards
Vignesh

July 25, 2018, 03:02
#10
Member

Vignesh Lakshmanan
Join Date: Nov 2016
Posts: 79
Rep Power: 8
Quote:
 Originally Posted by ViLaks Dear Lucky Tran, First of all, sorry for restarting the thread. I am trying to design a heat sink for electronic components of an air conditioner outdoor unit. Attached is the picture of the heat sink (computational geometry) with components (Heat sink is highlighted in color). The heat sink base is 3.5 mm thick , whereas the fins are 1.5 mm thick. I have no problems in modelling the fins with 1.5 mm thickness and have expected results. The problem starts when I want to model triangular shaped fins (approximately triangle shape). In the picture, the thickness of the fins vary from 1.5 mm at top to 0.75 mm below. I am not able to mesh it satisfactorily. So I am thinking of modelling shell conduction. Now as per your explanation, if I model shell conduction, say 2 layers for both wall and shadow, do my shells look like this (Air is the only fluid)? air|wall|wall-shell1|wall-shell2|shadow-shell2|shadow-shell1|shadow|air? Is my understanding correct? Thanks and Regards Vignesh
Dear Lucky Tran,

In case I use refrigerant cooling , I model a pipe in which refrigerant flows. The pipe is inserted into a plate which is in contact with the components to be cooled. So a fluid zone whose walls are solid (pipe) is inside a solid zone (Base). How to get shadow zones in this case. I need to model conduction. I have a rectangular plate with thickness, inside which a pipe is passing. I have subtracted the pipe from the plate. But Im not getting shadow zones in fluent.

Thanks
Vignesh

 September 28, 2018, 08:01 #11 New Member   Join Date: Dec 2015 Posts: 1 Rep Power: 0 hi, I am modeling a cylinder (d=16m) with a wall thickness (t=0.005m) and insulation(solid2). could you please let me know if shell conduction works for internal walls(in my case cylinder wall) between fluid and solid2? fluid\wall\shell 1\shell 2\wall shadow\solid2 Regards RK

October 3, 2018, 04:19
#12
Member

Vignesh Lakshmanan
Join Date: Nov 2016
Posts: 79
Rep Power: 8
Quote:
 Originally Posted by rouzbehk hi, I am modeling a cylinder (d=16m) with a wall thickness (t=0.005m) and insulation(solid2). could you please let me know if shell conduction works for internal walls(in my case cylinder wall) between fluid and solid2? fluid\wall\shell 1\shell 2\wall shadow\solid2 Regards RK
Hi,

Could you upload a pic? I guess (from what I understand), shell conduction should work.

 July 1, 2021, 16:27 #13 New Member   Mouna Join Date: Jun 2021 Posts: 12 Rep Power: 3 for my case, i i have an interface between a fluid circulating in an inner pipe and a phase change material circulating in outer pipe (it will be transformed from liquid to solid phase during the simulation by cooling it with the fluid of the inner pipe), can i ignore the thickness of the pipe to reduce meshing and put a shell conduction or it is just used for fluid/solid domain and when the phase change material goes to solid it wouldn't work). Or can i just add a wall thickness without meshing or i should mesh it explicitly. thank you

 Tags layers, shell conduction