heat source way too hot
 

Hello,

I set up a transformer with 500W heat load, and it reaches 200 degree more than ambient
Its 2 domains, one is air with 80L/s flowing trough it. Air temperature rises by 13 or so degrees, so that part works ok. The other domain is the size of 1 1/2 bricks. It has a sub domain with heat flux in W/m^3. Its 460 or so W coming in. The wall to air I set 0.2mm roughness. Mesh it pretty fine. Boundary is conservative heatflux. In testing that transformer would reach something like 30 degrees more than surrounding air, it would not reach 500K? What am I doing wrong?
The air domain could do with a inflation layer, but still, that transformer sits at 500k!

https://iili.io/2c5lKF.gif

https://iili.io/2c73Ug.gif
https://freeimage.host/i/2c5lKF

the mesh doesn't look fine, based on the results
Do you have any inflation layers at the transformer wals.
be sure to resolve the near wall flow, check what your HTC contour looks like

Did you check the energy imbalances? Either during the calculation or at the end in the output file? This should tell you if all energy that you put into the domain is coming out, either through outlet or conducting walls. If not, than it is not converged. Then you need more iterations.
Probably you solid is much slower than your fluid, so better solve energy only. Or increase the timesteps for energy (solid and fluid) significantly.

increased surface area. Also added inflation layer. Converged within 1 W, so nothing to find there either


https://i.ibb.co/rp84mxk/transformer-heatx-3.gif

I detailed the transformer a bit, which increased its surface area a lot, so now its 100 Celsius. That's better. Still a bit ofa worry, the original design does not have such a fast air flow, and its still colder
https://i.ibb.co/720Q1Vv/transformer-heatx-4.gif

* Radiation might be important. You might need to include a radiation model.
* I suspect the biggest problem is because your mesh is completely inadequate (as urosgrivc said). Have you done a mesh sensitivity check? You need to check your mesh is adequate to accurately resolve your flow. If not then you are guessing, and as the results don't look right then your guess is completely wrong.

In your case,
I would put an additional monitor point at the outlet for the energy that is leaving the system.

Heatcapacityofair [J/kgK]*massfow(outlet)[kg/s]* DeltaT(outletT-inletT) = 500W

if this is not equal to the input power(500W) of the transformer during the solve proces, than you have not reached steady-state conditions yet.
This would tell you the energy balance in this system.
You are able to marge time forward faster in the solid domain which is vhat should be used for cases like this,
or huge amout of iterations will be needed to achieve steady state, it might be that you have stoped the simulation too soon if you haven't "sped up the solid domain"

Why do this? The imbalances calculation already does this, and it is more complete (includes all heat sources and sinks, accounts for variable density, specific heat and anything else).

Yes, you need to ensure the imbalances are sufficiently low, but use the built in imbalances calculation, not an approximate version of it.

Yes this is approximately the same thing
I just wanted to explain what to be careful about, as I am afraid that he doesent know where to find default imbalances and what they mean.

(Neglecting any mesh issue) I don't know the size of your geometry, but it looks a bit like a nozzle. So, rather small, not? Are you sure about the 500W? Are you sure the temperature is wrong? I'm not.
Do you model full 3D or a wedge with symmetry/periodice boundaries? Did you correct the heat input for the small portion?

I would agree with Gert-Jan
Are you maybe neglecting the efficiency (~95-98%)
and that a 500W well designed power transformer only needs to dissipate about ~3% of this energy in heat form?

if 500W is 3%, well than we would be talking about 16.7kW power transformer an that would not fit inside 150mm box

-change in mesh size did not change the temperature at all
-quick online calculator showed if I set the temperature of the transformer to 75 Celsius and the box to 25 then for 0.3m2 I have 80 W radiative heat.
-its a line reactor actually, the data sheet says 500W loss for the one I am using, so this would be the heat load
-that dent on the top tight, it helps to push the moving air on to the top surface, increasing heat loss.
-if I incorporate heat loss, this will have to be from the domain boundary steel to air I guess? Not sure if I try a dodgy first, reduce heat load by 80W
-also, if this is in a metal box, some of the heat may be conducted elsewhere. I put some small heat transfer coefficient from the domain wall to ambient, which reduced the temperature a little. I went for 10W/m2*K, still air. So there are lots of surrounding factors. Also, is the supplier cautious, are the 500W measured?

Check if 500W loss is all heat or is it just loss due to the magnetic fields not being coupled 100%.

Is this just the difference between power in and power out? Than you dont hawe the exact number for heat input
What is the total watage of the line reactor? does 500W seem wright?

according to this;
Heat loss for:
150 kVA and smaller : 50 Watts/kVA (aprox. 5%)
150 - 500 kVA : 30 Watts/kVA (aprox. 3%)
500 - 1000 kVA : 25 Watts/kVA (aprox. 2.5%)
1000 - 2500 kVA : 20 Watts/kVA (aprox. 2%)
larger than 2500 kVA : 15 Watts/kVA (aprox. 1.5%)

is your line reactor at least 10kW?

its 120kVA 3 phase.
I assume, all losses are eventually turning into heat?
for radiation, only option is Monte Carlo in CFX.

Well if it's a ~120kW than I am confused with all the previous data and the size...
shouldnt it be like 10X the size of this one, sorry but too little data to help

ok, its 300x240x130mm. 4 bricks
220A, 0.28mH, 480W for typical rectifier it says. Now, that particular one at full load its 30% THD and at 10"% load 55% THD. So not sure if the 480W are aimed at 60"% THD at full load.
Pretty hard tor us to measure though, the losses through it

Incorrect. For heat transfer between surfaces the discrete transfer model is also applicable, and in most cases it is recommended over Monte Carlo as it is much faster and easier to use if your application just has radiation heat transfer between surfaces. The Monte Carlo model is required in complex radiation applications involving absorption and things like that.

There are also simpler models suitable for optically opaque fluids such as fluidised bed burners. They cannot model heat transfer between surfaces.

no I mean in my simulation. The domain for my heat source only offers Monte Carlo. The air domain has more options. But, the heat source would radiate?

I am not an expert on Radiation modelling but I think if you want radiation to pass through a solid domain (ie, it is transparent, like glass) then you need the Monte Carlo method. If the solid is opaque (like a block of metal) then you can use the discrete transfer model in the fluid domains only, and apply radiation boundary conditions on the interfaces to any solid regions as the radiation will not go through the solid domain.

Most heat sources I have seen in your application are opaque, which means the discrete transfer model is the model you should be using (assuming the fluid is optically transparent and you just have heat transfer between surfaces which can see each other).

that helps, reduced the heat. I tried another geometry in the meantime, so better get back to that one

Both the Discrete Transfer model and the monte Carlo models are tunable models, meaning that you need to set them refined enough to be accurate. So you need to do a sensitivity study to make sure you have set them refined enough to be accurate. For the discrete transfer model I think it is the number of rays from a face, and for the Monte Carlo method it is the number of rays to trace.

But I recommend a simple analytical case when first starting with radiation modelling - a square domain with radiation, and model the radiation heat transfer from one side to the other. It is very instructive to see what is involved in getting simple cases with known exact answers like this to be accurate before attempting your more complex model. It will help you understand what you will need to do to make your model accurate.