Cooling problem

[tibich72]

Hi,

I've inherited a system that uses Elmer to simulate cooling electronic components. Basically, we model the components in 3D, then immerse them in a box of air and specify an air flow. I'm not an expert on FEM and/or thermal analysis and now I have to modify the system a bit for a new problem.

Here's how the boundary conditions of the air box are modeled now:

Code: Select all

Boundary Condition 1
  Target Boundaries(1) = 5
  Name = "Airbox Boundary 1"
  Normal-Tangential Velocity = True
  Wall Law = True
  Boundary Layer Thickness = 0.00387252995529114
  Surface Roughness = 9
End

Boundary Condition 2
  Target Boundaries(1) = 3
  Name = "Airbox Boundary 2"
  Normal-Tangential Velocity = True
  Wall Law = True
  Boundary Layer Thickness = 0.00387252995529114
  Surface Roughness = 9
  Temperature = 40
End

Boundary Condition 3
  Target Boundaries(1) = 2
  Name = "Airbox Boundary 3"
  Normal-Tangential Velocity = True
  Wall Law = True
  Boundary Layer Thickness = 0.00387252995529114
  Surface Roughness = 9
  Temperature = 40
End

Boundary Condition 4
  Target Boundaries(1) = 6
  Name = "Airbox Boundary 4"
  Normal-Tangential Velocity = True
  Velocity 1 = 3.1
  Temperature = 40
End

Boundary Condition 5
  Target Boundaries(1) = 4
  Name = "Airbox Boundary 5"
  Normal-Tangential Velocity = True
  Wall Law = True
  Boundary Layer Thickness = 0.00387252995529114
  Surface Roughness = 9
  Temperature = 40
End

Boundary Condition 6
  Target Boundaries(1) = 1
  Name = "Airbox Boundary 6"
  Normal-Tangential Velocity = True
  Temperature = 40
End

Basically, this (I hope) says that the air enters through face 6 (boundary condition 4) and exits through face 1 (boundary condition 6). My first question: does setting WallLaw to true and setting the "Boundary Layer Thickness" mean that indeed the air is not allowed to flow through that boundary?

With these boundary conditions, the max temperature for the component of interest is 69C. Now, if I remove the line "Normal-Tangential Velocity = True" from the boundary conditions the max temperature shoots up to 171C. I could not find a detailed explanation for "Normal-Tangential Velocity" (in fact, the Elmer Solver manual and Elmer Models Manual give contradictory syntaxes for this command -- maybe this could be fixed in the future). What is the use of "Normal-Tangential Velocity"?

I've also noticed other posts regarding air flow and they seemed to model things differently (see, for example, viewtopic.php?f=3&t=1382&start=0&hilit=air+speed), but they were using a keyword "Noslip wall BC" that was not mentioned anywhere in the documentation. Where can I find more info about this keyword?

Any help with these walls and boundary conditions is appreciated.
Tibi

[Juha]

Hi,

Welcome aboard, i'll try to give some answers to your questions.

Yes, you probably have got the in- and outflow boundary conditions correct, other BCs seem to describe walls.

When using the wall laws (approximation of the tangential velocity some distance away from the
real wall) "Boundary Layer Thickness" is the distance from the physical wall where this tangential
velocity approximation is computed.

The "Normal-Tangential Velocity = True" setting gives you the possibility to give the boundary conditions
for velocities in terms of normal and tangential components instead of the components in coordinate axis
directions.

Looking at the wall BCs, I'm afraid your wall boundary conditions are missing the "no flow through the
wall" condition "Velocity 1 = 0", i.e. normal velocity should be set to zero. You should not give the
tangential components however, as these are computed automatically using the law of the wall.

The "Noslip Wall BC=True" setting can be used if you are not using wall laws, but instead have a boundary'
layer mesh dense enough to capture the physics near the walls. This sets all the turbulent flow related
variables to their wall values. The basic K-Epsilon model is not so well suited to this type of direct boundary
layer modelling though, other models such as the SST K-Omega, for example, should be more accurate.

Regards, Juha

[tibich72]

Juha, thank you very much for your reply. I've updated the model with the correct speeds, but I still have some issues with air speed.

Just as a clarification. When I set the air speed to a value (say 13.6 in my case), how does Elmer know whether the flow is from the outside towards the inside of the model or the other way around. Is there a sign that needs to be specified (e.g. -13.6 is from inside to outside, and 13.6 the other way around)?

I've also plotted the velocity for air for the model and it seems a bit strange to me (see attached photos):

velocity.jpg

3D view of air speed

(38.96 KiB) Not downloaded yet

velocity slice.jpg

Slice normal on Z axis, through the center of the model

(60.42 KiB) Not downloaded yet

These are taken from Paraview. As you can see, the speed on the left side of the box is not constant (13.6) but instead it has a distribution. I thought that setting the velocity of the boundary condition means that the speed is constant all over the face -- is this not the case?

What's more disturbing, though, are the small specks in the middle of the slice view. Those are the fins of a heatsink, and they seem to have a velocity different than zero. Here's how the material properties for aluminum (for the heatsink) and air are defined:

Code: Select all

Material 1
  Name = "Aluminum"
  Heat Capacity = 921
  Density = 2700
  Heat Conductivity = 200
End

Material 8
  Name = "Air"
  Heat Capacity = 1005
  Density = 1.1141
  Heat Conductivity = 0.0271
  Compressibility Model = Incompressible
  Viscosity = 1.7014E-05
  Heat Expansion Coefficient = 0.0
  Specific Heat Ratio = 1.4
  Reference Temperature = 25
  KE Cmu = .09
  KE C1 = 1.44
  KE C2 = 1.92
  KE SigmaK = 1
  KE SigmaE = 1.3
  KE Clip = 1.0e-6
  Viscosity Model = KE
  Heat Conductivity Model = KE
End

Do I have to specify anything extra for the definition of aluminum to say that it's a solid and does not flow? Or is it normal the way results are computed?

Thanks,
Tibi

[Juha]

Hi,

you don't exactly give flow speed on the boundary, but the velocity components either in x,y & z-directions,
or in normal- & tangential directions depending on the "Normal-Tangential Velocity" setting. For the
Normal direction + is outwards - inwards.

The different boundaries share nodes, between nodes the velocities shown are interpolations of the nodal
values. Ignoring the tangential slip wall law, you have zero velocities on the walls ,13.6 units in the inflow boundary,
near the walls you have something inbetween. Constant value on a boundary is btw. unphysical and there
is a conflict on the edges of the different boundaries (not that i think it's a big deal here).

Do you have boundary conditions between the air and the aluminum? These should have wall boundary
conditions as well. Even then the tangential velocities are nonzero on the walls due to the wall law, and the
comment on color interpolation might apply here as well.

You, by the way, seem to have very coarse mesh...

Regards, Juha

[tibich72]

Hi Juha,

thanks again for the information. However, I'm wondering whether it's always the case that a '+' is outwards->inwards. I'm attaching two images from Paraview showing the velocity vectors on a slice through the middle of the model.

vel_vect_plus.jpg

Normal speed positive

(183.43 KiB) Not downloaded yet

vel_vect_minus.jpg

Normal speed negative

(152.01 KiB) Not downloaded yet

As you can see, in the first image, when the normal speed on the inbound face is positive, the vectors seem to go from inside to outside. When the speed is negative, they seem to do the right thing and go inside (plus the shape of the heat trail and distribution seem to be in line with what's expected). Do you think it has anything to do with the way geometry is defined (e.g. face orientation or something like that)? I'm using my own CAD software to write a BREP file that's meshed by Gmsh, maybe there's something there that needs to be in a certain way.

Thank you for explaining the interpolation of values for elements. I agree that the mesh should be much finer, but currently Gmsh crashes when trying to produce fine local meshes when using STEP/BREP models -- that's something that I need to address by probably using some other mesher.

Thank you also for the tip regarding boundary conditions between air and aluminum (and air and everything else, for that matter). I'll adapt the system to generate those boundary conditions.

Cheers,
Tibi

[Juha]

HI,

the rule which i tried to formulate yesterday (;-) is that the + is to the direction of the outward pointing
normal, this seems also be your observation! This obviosly only applies if the "Normal-Tangetial Velocity=True",
otherwise you give velocity component values in the coordinate vector basis.

regards, Juha

[tibich72]

Juha, thanks for the clarification. I understood your previous post to imply outwards -> inwards for plus. Having '+' in the direction of outward pointing normal makes sense.

Cheers,
Tibi

[tibich72]

There still seems to be something strange (if not wrong) with my model. I've added boundary conditions to each face between air and solids in my model, and now everything is much hotter than before (by about 70C). Moreover, if you look at this slice through the middle of the model (and through the heatsink), it seems that the air is simply going around the heatsink and not through it (which I assume is the cause of the overheating).

velocity_int_zero_normal.jpg

Velocity vectors with zero normal on internal faces

(280.91 KiB) Not downloaded yet

I've managed to get a finer mesh out of Gmsh and looked at the elements through that slice -- it seems that there are a few elements between the fins of the heatsink:

velocity_int_zero_normal.jpg

Velocity vectors with zero normal on internal faces

(280.91 KiB) Not downloaded yet

I'm not sure why this behavior would happen. I'm also attaching the .sif file used in simulation, maybe there's something wrong there. Any suggestion is greatly appreciated.

I have another question related to the +/- sign of the normal. What happens if the model needs to set a non-zero normal velocity as a boundary condition for some internal face -- what's outwards and inwards in that case?

Thanks,
Tibi

[Juha]

Hi,

what are the heatsinks in your .sif file? Anyway, you now have free tangential slip at the solid/air
interfaces, i think you should (at least in principle) apply the wall law to those.

The +/- rule:

The boundary condition setting "Normal Target Body=n" forces the normal to point in direction
of body n (n must be one of the bodies attached to the boundary). Lower numbered body
seems to get picked by default.

-Juha

[tibich72]

Hi Juha,

the heatsink is body #2, name "HS_1", with this def:

Code: Select all

Body 2
  Name = "HS_1"
  Equation = 1
  Material = 1
  Target Bodies(1) = 2
End

Thanks for the clarification regarding the +/- rule. I'll have to re-run the system with all the boundaries between fluids and solids having a wall def too, and will see how it goes. I'll post the results.

Thanks,
Tibi