CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Superheated steam phase change to sub-cooled water (

andyross33 July 15, 2013 18:33

Superheated steam phase change to sub-cooled water
Hello forum,
I am having difficulty employing multi-phase within CFX. We are attempting to simulate the phase change through a steam-liquid water heat exchanger where superheated steam (@ 220F,1 atm) enters the inlet, snakes through a series of tubes, and exits as sub-cooled water. External water flow is passing over these tubes and the aim is to absorb as much of the latent heat energy from the superheated steam as possible.
Initially, I set up the geometry of this latent heat exchanger and ran into convergence issues. Working through the forum, tutorials, Ansys tech rep, etc. I wasn't having any luck gaining convergence at which point I simplified the model to one length of tube. With that, I have reached convergence; however, I do not understand the results.
I have specified mass fraction of 1 and 0 for the vapor and liquid, respectively, at the inlet and oppositely for outlet (using an Opening BC for each). I have placed a -1000 W/m^2 heat flux on one side of the fluid domain to ensure heat is leaving the system.
I've run the simulation for 4,000 iterations and watched the mass/energy imbalances settle very close to zero. The temperature and pressure values show that the water is indeed in the sub-cooled domain but the mass fractions do not reflect that. The mass fraction of the vapor is 1 throughout the domain and of course 0 for the liquid whereas I of course expect to see it vary.
Can anyone point me in the right direction?

andyross33 July 16, 2013 14:18

2 Attachment(s)
This is a simple geometry I am considering but maybe the attached image would be helpful. The inlet is at the bottom left with outlet at the other end. The highlighted wall is where the heat flux was placed. There is a symmetry wall on the other side of this.

I've also included the OUT file (zipped) of the last run.

I am really at a loss with this guys, any and all help is appreciated.

ghorrocks July 16, 2013 19:06

Any multiphase model with phase change is going to be challenging. Sorry to not be very helpful, but this is too complex a model for me to help much.

andyross33 July 16, 2013 19:29

GHORROCKS, I am new to phase change modelling and so I'm naive to the complexities involved although I am starting to grasp it. What I am having trouble with is the lack of clear documentation in what I think should be a fairly straightforward type of simulation. There are no complex geometries (straight pipe), sub-sonic flow and boundary conditions are well defined. Your forum posts on this (and other) topics have helped me immensely and so I do not question your knowledge. I just find it hard to believe I can't get this relatively simple - if I dare use that word - simulation to provide meaningful results. I am chasing this with Ansys as well so I will update when I have an answer.

I suspect that my problem lies in my model settings although I find that with all the various options, I have gotten lost in which material definitions I should be using (homogeneous binary mixture or variable composition mixture - the mass fractions are changing over the domain after all) and domain settings (do I use continuous fluid & dispersed fluid, or droplets).

Perhaps I should start with defining to you exactly what I want to learn from the model which is how much heat energy transfer will occur from the tube flow to the external water flow. In fact, I don't really care about the levels of mass fractions other than I wanted to keep an eye on the outlet because if we do not have sub-cooled water there than that means we are leaving some readily available heat energy on the table.

Do you have any suggestions on how to proceed with this? I know I am lacking on details but I really have just grown confused and need some step by step hand holding. For example, to start, how would I set up the material definitions? I have defined so far:

H2Og = pure substance, IAPWS, gas (with table generated for mat'l props)
H2Ol = pure substance, IAPWS, liquid (with table generated for mat'l props)
H2Ogl = homo. bin. mixture (with table generated for saturation props)

Does this look right?


ghorrocks July 16, 2013 19:36

The HBM approach is certainly one approach I would try. Just a thought - if you model it with IAPWS vapour at the inlet as a single phase material will that work? Not sure of that.

Do not underestimate the difficulty in phase change modelling. It is a complex area and will require careful model development to get working.

Also - Why not do this with a 1D model? Writing a model which can track the phase change of the fluid as it goes along in a 1D sense may well be easier and more accurate than doing it in full 3D. Do you need the 3D model for some reason?

andyross33 July 16, 2013 20:03

Eventually we would like to add buoyancy to the model to track particulate dropping out of solution and view how these flow between the heat exchanger tubes. There may be cause for concern with regards to fouling the tube surfaces and it would be helpful to see if these particles do indeed drop to the tank bottom or congregate somewhere else. I suppose I could create a 2D model to start as the old rule of thumb of starting simple definitely applies here in spades. However, I was thinking by reducing my geometry to a straight pipe that I had already simplified things substantially.

I have currently set the inlet to have a vol fraction of 1 for H2Og and 0 for H2Ol. Can you clarify what you mean by your suggestion? As I understand it, I have defined it as a single phase at the inlet by doing it this way.

RicochetJ July 17, 2013 05:36

In my opinion you so need to do this in stages!

First of all you're right in trying to get this to work using one length of tube.

1. Perform an energy and mass balance on the heat exchanger involving the one length of tube. This is not a CFD problem. It's a pen and paper problem. From this you need to calculate the temperatures and heat fluxes. Good heat transfer text books should show you how to do this. Before diving into CFD make sure that you have done this.

2. Forget phase change for the time being. Ignore it. Set up a CFD simulation using pure substances (water single phase in the tube, and single phase outside of the tube). Run the simulation. Are the temperatures around the ball park that you expect it to be? Do the temperatures and heat fluxes agree with your energy and mass balance in point 1?

3. Layer on models that you need. So run a simulation with buoyancy. Then again but with buoyancy turbulence production and dissipation switched on. How do they change the result? Keep adding "layers" until you get to a point where the last thing you need to do is switch on the phase change models.

Make sure you use the previous simulation as the initial guess for the next simulation. Also don't expect phase change to be steady state.

I think you'll need to use IAPWS IF97 water properties, even for the simulations in point 2.

You can't dive in to complex simulations in the way that you're doing.

andyross33 July 17, 2013 18:15


Good tips. I have done the hand calcs to refer against and I agree, this should be done as a matter of course on any simulation wherever possible. I am currently in the process of verifying my latest results.

I do like the idea of running a water based simulation, especially to get initial values before turning on phase change. I often wonder how best to initialise. For example, with snaked tubes the velocity vectors are constantly changing and so a single initial guess may be close for one tube but not the next when it reverses direction. Using a more stable, single phase solution as the initial input to the multiphase may help with convergence.


With the Ansys tech help, I made some progress on the model and am now seeing liquid mass fractions form. Not sure yet if the results make sense but at least it is getting closer to reality. Where I had gone wrong was in the materials, I had not imported the IAPWS material definitions correctly. The other major contributor was in my selection of continuous vs dispersed morphology. Because the inlet is pure vapor, then vapor should be set as the continuous and the liquid as the dispersed - I had it the other way around, although I did see the way I had it as a suggestion in another forum post.

Lastly, the Ansys tech rep suggested not using material names with numerics in them (I had H2Og for example) as this may cause issues in the CEL expressions.

andyross33 July 17, 2013 18:18

One other point, the Ansys folks suggested including the Wall Condensation model as otherwise the formation of liquid phase may not occur as readily due to the lack of wall effects. Anyone have experience with this, and perhaps some general tips, as it is a new feature I have not yet tried?

ghorrocks July 17, 2013 18:32

I have not used the wall condensation model seriously - as you can see your "simple" model is not simple at all. Remember that geometric simplicity is much easier to deal with than physics complexity!

As for the comment about continuous versus disperse: This is problem dependent. If you have pure vapour condensing then vapour = continuous and liquid = disperse makes sense. If you have pure liquid which is boiling then liquid = continuous and vapour = disperse makes sense. So I agree in your case vapour=continuous and liquid=disperse seems appropriate.

andyross33 July 17, 2013 18:42

That makes sense. However, I may eventually have both boiling followed by condensing. That is, liquid water enters, boils as it passes by the outside of the heat exchanger and then, since this is a recirculating system, condenses again as it passes through the inside tubes of the heat exchanger. In this case, would you select the water to be continuous since it is at that state at the inlet?

All times are GMT -4. The time now is 21:20.