[MStudent]

Hi,

I am a master student, for my final year I am making a thesis about the design of a heat exchanger...

A counterflow double pipe heat exchanger was chosen for it's simplicity.
Through the inner pipe flows a gas starting at 600°C (873K) going to about 50°C (323K), this is a laminar flow according to previous calculations..
Water flow through the annulus starting at a temperature of 6°C (279K), again according to previous calculations this is a turbulent flow with a Reynolds number of approx. 80 000.

I need to do an analysis of this heat exchanger not only using CFD software (I'm using Ansys workbench 15 -> Fluent) but also be able to write out the theory of it...

I had originally chosen to use the k-e model, but after reading the "Turbulence" posts on the Leap Australia CFD blog I am wondering if the SST k-w model would be better.
http://www.computationalfluiddynamic...nce-modelling/

If possible please give me some input on this, as well as more information about the model you end up suggesting.

Any further information concerning this problem is always welcome.


Thanks in advance,

MStudent

[edoan]

split your domain into two regions no turbulence model for the laminar region, depending on your mesh choose a low re or a wall function turbulence model for a case like this any of the two equation models will likely give almost identical results.

[MStudent]

I have met with the professor who is "in charge" of this project and she told me that because of the high Reynolds number of the water flow it would be better to use the SST model...

As for your suggestion, I have no idea how to split the split the region in Fluent so that the laminar part is separate.
I'm using 'standard' unstructured mesh, but I have used inflation in order to refine the near wall region.

https://drive.google.com/file/d/0B15...ew?usp=sharing

https://drive.google.com/file/d/0B15...ew?usp=sharing


So, once more any information is welcome...

-MStudent

[edoan]

ok k-w sst is a fine choice, it is capeable of adapting between low re and wall functions depending on the y+ value, make sure your y+ is either around 1 (to use the low re) or around 30 (for the wall functions) try not to have the mesh in between the two, larger then 30 is also fine up to 200 ish. What are you using for mesher/solver? maybe i can walk you through splitting the domain so you can have the turbulent section and laminar section...btw sorry i cant open up those google drive sharing at work.

[edoan]

i re-read your comment and see that you are using fluent. I also woke up and realized the fact that you can specify two fluids means you already have two domains, in your cell zone zone tab you can specify "laminar zone" for the gas section. Now as long as you have a good mesh and proper boundary conditions you should be able to come up with a successful simulation!

[MStudent]

Thanks for all you help so far, sorry for replying late... I like to stay offline to be more productive.

I did a first run today using the new (SST k-w) model, I took screenshots of everything I did/modified so it's easier for someone to tell where I went wrong or what I should have done differently..

https://drive.google.com/folderview?...28&usp=sharing

http://s12.photobucket.com/user/MStu...nergy/library/


It's 21 Pics, so I don't just want to upload them here. If there are problems opening this please give me a method that is easier to view. The answers for your previous posts are probably in there as well (solver and such).


It seems like there are still quite a few problems;

• As you can see from the screenshot, I set the gas flow to laminar (at least I think I did). Do I still need to enable the "Low Re corrections" in the model tab?

• Did I do the monitors of the values correctly? The gas_outlet temperature is the most important for the function of this heat exchanger it should be steady around 50°C (or below). From the looks of things, the value doesn't even converge into a steady number...

• For the models, do I need to turn radiation on? It was not considered in the design of the heat exchanger... If so, how do I set it? Discrete Ordinance, etc...

Some more general questions:

• How do I determine the y+ value in Fluent, how do I set it, etc...
• For the grid independence test, do I just change the mesh from Course -> Medium -> Fine or is there another way to do this?

Thanks so far for being patient and helping me with this, this is my first time using the software (and first time doing something in this field) and I'm trying to figure it all out by myself...


Also thanks in advance for any other help you can give me,


MStudent


*Edit: added a photobucket link for the screenshots

[edoan]

Ok I cant open these shared folders at work if i remember i will look on my personal computer later. Let me try to answer some of your questions.

If you have properly set the gas flow to laminar then any turbulence properties you do specify will be ignored so the low re corrections will have no effect.

If your steady state simulation is not converging to a steady result there could be a number of things causing this, mesh, BC's, models.... too hard to say anything in particular.

I don't think radiation will be relevant you can consult some papers to confirm.

For Y+ values you can plot them or show contours in the results tab. Y+ and a number of other turbulence properties are under the turbulence selection in the drop down. Y+ only has a meaning next to the wall so i suggest making a plot of the values along the wall. Remember if you want to use the low Re you need Y+ ~= 1 and for the wall functions you can have 30-200ish. The Y+ isn't "set" you make a mesh and depending on the flow it is calculated.

The procedure of a grid independence test is this: pick a coarse mesh size run a simulation and find a value of importance, for you this can be your gas outlet temp. now reduce the mesh size so that your element count roughly doubles. compare your new value with the old value. When these two values change less then say, 2% you can say that your solution is mesh independent to within 2%. You can pick 5% or 1% whatever.