steam and water pressure vessel simulation

[frugal]

Hello All,

I am new to CFD and I am trying to analyze thermal transfer in a water / steam pressure vessel.

I have set up the model using solids to represent the case, the internal water volume, the internal steam volume and some attached parts.

When I try to solve, I get a "two different fluid materials are touching" error.

However, if I suppress the water and try to run the solver using only the steam, it quits with "The Analysis has stopped because the Solver has exited unexpectedly" which points to an additional and possibly more fundamental problem than the two fluid media.

I understand that multi fluid models are not possible, but as I am not interested in flow, I presume that there must be a work-around to create a boundary between the two fluids (possibly a distributed resistance?) and I am wondering what the best approach is.

CFZ file attached.

Many thanks,

Thomas

[frugal]

Addendum to my previous post.

After looking at further tutorials - especially the "Natural convection around a telecom. module" - I decided to simplify the model and simulation until I could get something to work. All of the tutorials work fine, but I cannot recreate any of them if I start from my own (inventor) model.

I cannot see any difference between the completed and functional tutorial and the recreation attached. All attempts stop with the gnomic "The Analysis has stopped because the Solver has exited unexpectedly". 

Any help would be much appreciated. 

Kind regards,

Thomas

[David.Short.]

Hi @frugal,

For your steam/water simulation just use steam (saturated) as the material and then perform a two phase simulation by enabling quality under advanced physics. Quality 0 corresponds to water and 1 corresponds to 100% vapour, so with that in mind apply appropriate initial and boundary conditions. Take a look at the help documentation on two phase mixtures.

As for your natural convection simulation. It runs with no problems on my machine (I went to 1000 iterations then stopped it).

Please ensure that you are working form your local C drive and the folder is not being automatically backup by something like dropbox.

Hope that helps,

David

[frugal]

Hi David,

Thank you for your reply.

It was indeed an issue with google drive that was preventing the solver from running.

Now that I can now actually do something productive I will try the two phase simulation - I am sure that that is the answer.

Many thanks,

Thomas

[frugal]

Hi David,

I spent some time with the two phase simulation but I can't get meaningful results.

I started with two volumes, one Quality 0 saturated steam for the water, the other for Quality 1 steam for the steam section.

Quality is active in the Advanced Physics tab.

I set the Initial conditions for them both to Temperature 120C.

The exterior surfaces of the vessel have Film Coefficient BCs set to allow transfer to the air.

However, the analysis stops after a few iterations with the "Field Variable Fluctuations are minimal" message and there doesn't seem to be any heat transfer from the steam volume to the case.

I simplified the scenario further to a single volume of saturated steam (Quality 1) and reduced the complexity of the geometry to a bare minimum with a similar result. If I add a Film Coefficient to the exterior surface of the steam, I can get further into the analysis and I start to see heat transfer to the metal case, but the analysis stops after 9 iterations with the same message. I have also tried adding an exterior air volume (which, if I understand correctly, means also removing the Film Coefs. from the exterior of the solid) with different but also dubious results - I get further into the analysis but it stops with the message "Flat lines detected in Convergence Monitor" and the results indicate that the surrounding air is essentially completely saturated with heat at the same temperature as the steam.

Another nudge in the correct direction would be greatly appreciated.

I also noticed that there seems to be an issue with model scale when adding new models to the Design Study.

I am not quite sure under what circumstances it occurs, but the model created in Inventor (in mm) is showing up in CFD at approximately 1/10 of its actual size. Right clicking on the Geometry (mm) in the Design Study Bar brings up the Geometry Tools window, not the units. I found a mention of something similar here - is it possible that this has not been resolved?

Many thanks,

Thomas

[David.Short.]

Hi Thomas,

Please can you attach a [.cfz] file rather than the [.cfdst]. The [.cfz] file is similar to a zip folder and contains all the relevant files for your simulation setup. The [.cfdst] file is a stand alone file that cannot be used without the rest of the design study folder contents.

It sounds like you might need a transient simulation if you want to utilize initial conditions. The steady state solution is essentially an infinite transient solution and thus initial conditions are forgotten.

Either perform a steady state solution with a total heat generation source within the tank or use initial conditions in a transient solution. Using one volume makes much more sense to me.

What exactly is the end goal of the simulation?

Ahh yes you have found an old bug. This has been resolved in CFD2018.

All the best,

David

[frugal]

Hi David,

Thanks for the quick response.

The water in the boiler is kept at a constant temperature with only minor fluctuations when there is load. Thus I thought that considering the water/steam to be always at a fixed temperature using an initial condition would be the simplest approach.

The end goal of the simulation is to analyze the heat transfer from the boiler to the equipment attached to it which has a more complicated geometry.

I want to look at how changes in that geometry and materials affect the distribution of heat.

With respect to the scale issue - I am using the CFD 2018.

Many thanks,

Thomas

[frugal]

---

@David.Short.wrote:

It sounds like you might need a transient simulation if you want to utilize initial conditions. The steady state solution is essentially an infinite transient solution and thus initial conditions are forgotten.

Either perform a steady state solution with a total heat generation source within the tank or use initial conditions in a transient solution.

---

Hi David,

I have spent some more time on this and I am starting to make a little headway.

I misunderstood what was meant by initial conditions - I don't want to analyze the cooling from a starting point.

However, I also do not want to use a total heat generation source as the temperature in the boiler is constant. Instead I have switched to setting boundary conditions on the surface of the steam volume inside the boiler:

Temperature 120C

Quality 1

Film Coef - 5w/m2/K at reference temperature 120C

The last BC was causing problems before as I had the units wrong (mm2 instead of m2). I believe that this was causing the air temperature around the boiler to saturate at 120C.

Ideally, I would like a static as opposed to a transient solution as I am interested in the equilibrium state that the system attains (I have empirical results that show this happens).

At the start of the simulation, the internal volume of the steam is shown to be at room temperature. Should I be suppressing the volume of steam after the surface BCs are set or also applying an initial condition?

Many thanks,

Thomas

[David.Short.]

Hi Thomas,

I think you are missing one fundamental point, that surface boundary conditions should not be applied internally. If you want to apply a temperature BC you should suppress the boiler internal volume and apply the BC to it (essentially making it an external boundary condition).

The only BC that we recommend applying internally are the heat generation volumetric BCs.

What do you hope to gain from including Quality in the simulation? If you already known that the volume of steam inside the boiler produces a constant temperature then why not just model that with a BC (temperature on suppressed volume)? Including phase change will just add complexity. If you wanted to model accurately the temperature distribution in the boiler then maybe it would be necessary to include Quality (you would then also need to accurately model the heating source).

All the best,

David

[frugal]

Hi David,

Thanks for the response.

I have run some more trials with the temperature BC applied to the surfaces of the suppressed steam volume and with the quality removed.

I initially assumed that the water and steam in the boiler would distribute heat to the casing differently - however, that is an unnecessary subtlety at this point.

With a transient solution, I am beginning to see more plausible results for the heat loss to the air. But I still don't see any conduction of heat to the solid material of the case. The image below shows a transient solution after 4000 seconds, The plane is cut transversely through the boiler and attached parts. I would expect to see a significant difference between the temperature of the air and the metal. Instead the metal appears to be essentially "transparent".

 

[David.Short.]

Good morning (German morning) @frugal,

I think that your mesh is insufficient to model the conduction correctly. Try to have at the very least 3 elements through the thickness of the steel around the suppressed steam volume. A manual or uniform mesh might work well for this however it will dramatically increase the element count. Alternatively model the thickness with a few layers in CAD then CFD will automatically put one element through the thickness of each layer.

Does that make sense?

Rerun the model with a finer mesh and let me know how it goes. Also before rerunning please consider using dimensions for your external volume as stated here. This will help improve accuracy of natural convection results.

All the best,

David

[frugal]

Good morning David,

From the time of your posts I figured that you had to be either an insanely early riser or in Europe :).

I did as you suggested - running the same simulation on a cad-created multilayered version of the boiler to increase the node count through the wall and increasing the proportions of the external air volume as per the link. I also spent some time reading up on meshing - a fine example of Rumsfeldian unknown unknowns i.e. things that I didn't know I didn't know. Looking more closely it would seem that I still have a ways to go in order to get a good mesh.

On the other hand, the results from the simulations are still confusing to me.

Below are two images of static solutions from two slightly different scenarios: the first has a film coefficient BC applied to all of the exterior surfaces while the second is exactly the same minus the Film Coeffs. Apart from the highly unlikely temperatures of the surrounding air volume (in both), I looked at some points on the part attached to the boiler. Without the FCs the temperatures at these points are very close to 120C which, although the model is grossly simplified, doesn't match the empirical findings. With the FCs, the readings on the points drop to around 104C, which seems far more plausible.

However, from what I read here, John Wilde said:  "Film coefficients can only be used on the external surfaces of a model - usually to simulate heat lost from a solid to the air. You could also model the air and then you would not need a film coefficient - they are useful to speed things up if you choose not to model/mesh the air though"

Obviously my next step will be to work on improving the mesh, but my question is whether or not I should be using the exterior Film Coeffs at all?

Many thanks,

Thomas

 

[David.Short.]

Hi Thomas,

If you don't apply film coefficients you will be simulating a perfectly insulated box. This is likely not realistic so I would use film coefficients to model what ever is exterior to you external volume.

Please send your .cfz file. The boiler volume looks very strange in those screenshots so I would like to take a look.

Thanks,

David

[frugal]

Hi David,

I was wondering about that. File attached.

Many thanks,

Thomas

[David.Short. · Accepted solution]

Hi Thomas,

Some changes are needed in your setup. For example if you want to include natural convection effects in the fluid you must have flow enabled in solve. Also you need a lot more mesh. 

Remember the solver only sees the mesh (not the geometry) therefore the mesh must represent the physical geometry accurately.

I have attached a .cfz with a setup for both a steady state simulation and also a transient simulation.

Results are shown below. SS on the left and Transient after 83 seconds on the right.

This is a solid view of the boiler attachment after 83 seconds.

To get faster results you might be able to increase the time step size to 0.5 seconds.

Let me know if you don't understand something in the setups.

All the best,

David

[frugal]

Hi David,

Your settings seem to work well for this simplified version.

I had tried adding slip/symmetry to the walls of the exterior air volume before, but I got "hall of mirrors" errors.

Not quite sure why this didn't work.

My only remaining question I guess is about the mesh settings you applied.

Everything is obvious except for the Uniform setting, which doesn't show if any Size Adjustment was made.

I am sure that I can figure this out empirically/fooling around.

Many thanks for walking me through this.

Best,

Thomas