Gas-Liquid heat exchanger analysis setup - temperature reaching absolute zero?

[jonathan.reed5BJXK]

I have a model of a heat exchanger (I cannot post the model/ cfd file as it is for work) and am trying to run a thermal analysis.

I have a counter-flow heat exchanger configuration with Air @ 26 kg/min, 370degC at the gas inlet port; 0.1 BarG at the gas outlet port; water @ 20 L/min, 20degC at the liquid inlet port; 0 BarG at the liquid outlet port.

The problem is that this results in the gas outlet temperature somehow reaching -273degC - so my BC's/ setup must be wrong. This happens for both steady-state and transient analyses, but steady-state should be sufficient for my purposes.

The Air is variable and compressible; I'm using ADV 5 modified Petrov-Galerkin;  Heat transfer is on; the heat exchanger body material is stainless steel; radiation is off.

What am I doing wrong here?

Thanks in advance!

[karol.suchon]

Hello Jonathan, 
There will be hard to notice what is wrong with the settings without the file. 
If you cannot share the model via the forum, please create a support case, I will try to help you.
BR
Karol

[jonathan.reed5BJXK]

What file do you need? 

The .cfdst file isn't supported on here.

I will upload the file as I need a solution to this problem, I have tried a few different approaches and none seem to work.

Thanks for your help with this by the way.

[karol.suchon]

The Cfdst file is only a linker between the results and geometry, you could pack the entire folder and zip it later. 
You could also send me the link via PM, and we will continue the conversation on the forum( maybe the thread will be useful for someone in the future) but I will not put any screenshots which show the entire geometry.

BR
Karol

[karol.suchon]

Hello Jonathan,
I have some conclusions, but I need to test some parameters. Overall in the simulation, you have a compressible flow, and the decompression generates the issue with absolute zero temperature, I will try to find the proper settings.

[jonathan.reed5BJXK]

Thanks for looking into this for me. 

I assumed I had some incorrect setup parameters as even with decompression of flow, the temperature would not reach absolute zero.

[karol.suchon · Accepted solution]

To be honest, I will turn off the compressible flow, we have a high temperature of the air, so even with a very high velocity we should not reach the Mach number above 0.25 Mach, so the compressible effect could be negated. Without it, we get rather reasonable results. You should also turn off the auto-forced convection, it will work fine for the water body, but the air density will change and have an influence on the velocity field. So the methodology to divide the simulation into the pure flow and next to pure heat transfer will give improper results.

Try to run the simulation without these two effects and let me know if you get any issues with the results.
BR
Karol

[karol.suchon]

One additional thing, could you edit the model for extrusion on the fluid inlet, if we apply the temperature BC on the surface which has the common edge with the solid body, we also apply the BC to that edge, which could give us improper temperature results. If we apply 20 C of water does not mean that the solid body on the inlet also has that temperature.

[jonathan.reed5BJXK]

I've attempted a steady-state analysis using the settings amendments you suggested and it seems to be providing reasonable results, so I think you have solved it - thank you!

I will attempt a transient analysis for a given time period and compare the results.

[karol.suchon]

I strongly do not recommend using transient simulation 😞
Even if we have a Mach number which should not generate compressibility, the velocity inside is still huge so we need to apply extremely small time steps to keep Courant number below 1. So the simulation will take a huge amount of time or will diverge at some point. 
BTW are you sure about the mass flow rate for the inlet, it rather not too common to have 100 m/s on the inlet 🙂 Check if the mass flow rate is not compressed before the HX 🙂
BR
Karol

[jonathan.reed5BJXK]

Okay I will stick to the stead-state analyses then! 😅

The mass flow rate is an assumption as there is no accurate means of finding the exact figure at that point in the line (I could estimate it based on pipe geometry and resultant pressure drop, and conductive/ convective heat transfer from the pipework itself, but this probably wouldn't result in a particular reliable result).

The temperature and density are varying from the point of know mass flow rate to the inlet of the Heat Exchanger, but in this scenario there is a compressor after the HE with a set flow based on an ideal inlet temperature, so the mass flow rate at the inlet of the HE gives a worst-case scenario.

...or at least that's how I am justifying the CFD setup/ results in my head!

[karol.suchon]

Ok, so we need to stay with the current conditions 🙂