Thermoelectric Cooler Simulation

[dousti]

Hello,

I would like to simulate a thermoelectric cooler (TEC) module inside Simulation CFD. However, I don't know how to determine the metal contact properties. More precisely, there is no place for specifying the thermal and electrical resistances of the metal contacts.

In the material of type "Thermoelectric Comp.", how does the Seebeck coefficient is defined? Is the summation of the Seebeck coefficient of the n-type and p-type pellets or is it the summation of them? Similarly, how are the thermal and electrical conductivities are defined?

Thanks.

[dousti]

No one has ever used the thermoelectric module?!

[Jon.Wilde]

Hi,

Does this link from the Wiki help at all?

[dousti]

Thanks for your response. I have already checked these two wiki pages (i.e., this and this)

I started with a very simple CAD:

- A PCB (10 cm x 10 cm x 0.15cm)

- A chip (2.5 cm x 2.5 cm x 0.1 cm)

- A TEC (2.5cm x 2.5cm x 0.4 cm)

- A Heatsink (2.5 cm x 2.5 cm x 2cm)

As shown in the attached files, the material properties are selected from the default library.The TEC size is set as the size of Sample 1 described in this.

An air volume is added sorrounding this objects with a size of 27cm x 25 cm x 16cm.

The boundary conditions are set as follows:

- Temperature of surfaces of air volume is set to 25C.

- Chip generates 3 W

The TEC module is configured to keep the cold side temperature (the one facing the IC chip) at 25C. As CFD Results 1 in the attachments shows, the maximum temperature goes as high as 127C!

On the other hand, if the cold side of TEC is reveresed, i.e., the cold side faces the heat sink, the max temperature will be about 35C. (See CFD Results 2 in the attachments)

Changing the material type of TEC to aluminium, give even better results. The max temperature reaches only 29C!! (See CFD Results 3 in the attachments)

I am pretty sure something is wrong in my setup but unfortunately, I could not pinpoint the source of error.

[Jon.Wilde]

I suggest that the issue is likely the Boundary Conditions on the external air domain.

Try with just Pressure on the top and bottom and a Temp (Ambient) on the bottom also. We call this the 'chimney approach' and it should work a little better.

[dousti]

Thanks for your response. The result got even worse! The temperature went up to 151C! Please take a look at the result (CFD Result 4 in the attachment).

I attached my CAD and CFD design (TestTEC.zip). You can try seeing the result by opening "Assembly1_1_support_support.cfz" with Simulation CFD.

PS. If I change the Air condition from variable to fixed, the result becomes much worse. I am also suspicious to the boundary conditions but I cannot find what is wrong about it.

[Jon.Wilde]

A few proposed changes:

1. Run for more than 100 iterations - use 500 and CFD should stop at a converged solution
2. You cannot use Auto Forced convection with natural convection as the flow and thermal solutions are connected
3. Utilise the Mixing Length turbulence model for natural convection on this scale (Solve -> Physics -> Turbulence)
4. Set gravity in the correct direction (which is -ve z). I used 0,0,-1 'earth'
5. I would use a CTM from a datasheet rather than ours if you can? I think that might actually be the issue here

[apolo_vanderberg]

To answer your question initally the Link Jon provided does outline how the coefficients are defined:

Seebeck Coefficient, a, units of V/K:

a = 0.000210902 + 3.4426e-07(Tav - 23) - 9.904e-10(Tav - 23)²

Electrical Resistivity, r, units of Ohm-m:

r = 1.08497e-05 + 5.35e-08(Tav - 23) + 6.28e-11(Tav - 23)²

Conductivity, k, units of W/m-K:

k = 1.65901 - 0.00332(Tav - 23) + 4.13e-5(Tav - 23)²

Now as far as your given model, with Aluminum you are essentially conducting in to the air and as such i would expect that a block of highly conductive material will do better than a TEC which generates extra heat to be able to pump energy between cold/hot sides.

I would also follow Jons recommendations to set up a proper natural convection analysis, either enlarge the air domain and leave the temperature conditions on it, or setup an appropriate inlet/outlet

Looking at the screen shots I can see you have ~100k elements, I would be cautious on the mesh quality between the fins such that we are capturing the air flow between them as well as ensuring we have 2 elements across the heated chip. Feel free to watch the SimTV videos on Basic Meshing if you are unfamiliar with how to refine the mesh

Lastly, I would expect most Natural convections models to inherently be slight over-predictions in the thermal profile as by default we are not taking in to account radiation which will contribute to the heat sinks ability to dissipate heat.

I would get the model running stable without radiation before considering turning this on.

[dousti]

Thanks Jon for your response.

I applied your suggestions 1 to 4. The situation (see the attachment CFD Results 5) becomes even worse. The temperature peaked to ~840C.

Regarding suggestion #5, initially I started with my own TEC model values. After I couldn't get proper results, I started using sample models provided by Autodesk. I really would expect Simulation CFD to come with a working sample project for TECs.

[dousti]

Thanks apolo.vanderberg for your response.

I already read these equations which are taken from CRC Handbook of Thermoelectrics. However, it's not clear to me how Simulation CFD models the contact resistance and thermal conductances.

Well, it might be the case that Aluminium perform better due to not having the Joule heating side effect. However, I mainly performed that simulation to show that the simulation setup works pretty well with natural convection (at least produces reasonable results), whereas adding TEC to the model results in unreasonably high temperature on the heat sink (~130C for the initial setup and ~900C for the tuned natural convection parameters per Jon's comments).

I increased the exterior air size from 27cm x 25 cm x 16cm  to 45 cm x 57 cmx 55 cm. The result has again become worse. (see the attachment CFD Result 6).

I watched this video. Initially, I used the automatic meshing feature provided by Simulation CFD. This time, I used a finer mesh for the heatsink (a 30% increase). Not much of a difference was observed. I still have pretty high temperature (see the attachment CFD Results 7). You can also see the meshing in the attachment Meshing.

In all of the above experiments, the radiation was off. I also think that (as I stated above) the problem rooted in TEC, since without it, the simulation results in reasonable values.

[apolo_vanderberg]

Can you attach your support sharefile so i can take a step through your setup

Thanks

[dousti]

Thanks apolo.vanderberg for your quick response.

According to this, I assume that by support sharefile you want my cfz file. I attached it.

[dousti]

Any updates?

[apolo_vanderberg]

The issue here is that you have a situation where a TEC is not beneficial.

First running your model with a bit more mesh to ensure we are capturing everything, there are a couple areas of interest.

FIrst the TEC is showing a warning (Max Current reached) so to maintain the constraints imposed we are requiring more current than this TEC allows for.

To show this I took these settings and ran a different variation where the TEC is assigned as a Solid material, and then supprsesed for meshing. On the "Cold" side of the TEC, I assigned T=25C, on the "Hot" side I assigned the 38W Total Heat Flux, that is being reported taht would be dumped in to the sink.

This produces very similar temperatures showing that the Heat Sink in question cannot dissipate 38W and thus the temperatures with the TEC are probable and what should be expected.

Looking at the Wall Heat Flux for this model we are not using effectively the fins that you have. The bulk of the heat loss is around the perimiter with very little entraining in to the central part of the fin. I might suggest opening the fin spacing (perhaps remove 1 fin and expand the gap) to get better use of the fins there.