Learning Forum

[zain.qazi]

Hello. 

I am simulating a Nitrogen High Aspect Ratio Cooling Channel using the Eulerian Model with RPI boiling Model. The model was set up gradually, starting with a simple flow field, then with the energy equation on in single phase and then finally turning on the Eulerian model with RPI boiling model. Prompts for "Lookup exceeded lower temp range.." show up once the results from the single phase are loaded in the Multiphase setup. The look up continues to fail until the solution diverges after the first few iterations. 

Boundary Conditions: mass flow inlet 0.00425 (liquid), pressure outlet 21.4 bar, constant temp outer wall 463 K. 

Physical Properties: RGP Tables from CFX.

This is a validation of an experiment and numerical case.

What is the reason for these prompts simply due to turning on the Multiphase RPI model and how to approach it?

 

[Rob]

I assume you have two tables? Ie one for the liquid and a second for the vapour? Which solver are you using?

[zain.qazi]

The tables were created through CFX and read in Fluent for the calculation. CFX creates two different tables for the rgp file, one for liq and one for vapour, which I assign to my two nitrogen materials (liq and vap) in Fluent accordingly. 

[Rob]

OK, good. If you switch from single to multiphase which phase does Fluent think is filling the domain? 

[zain.qazi]

Switching to multiphase and generating a simple contour of the vol fraction shows 100% liq nitrogen in the domain. The temperature contours do not show the same results anymore either. The outlet liq temp shows 3e-4 K which is non realistic. 

[Rob]

Yes, which phase is liquid? Ie primary or secondary? Switching from single to multiphase isn't always simple. 

[zain.qazi]

The primary phase is the liquid phase

[Rob]

I suspect it's the way energy is handled when you include the multiphase model, check the velocity field too. There are ways around this using MDMs and interpolation files to patch the correct values back into the solver. 

[zain.qazi]

Found in the User Guide that using a single phase solution as the starting point for a Eulerian is not the way to go (p 3166). Will attempt setting up a Mixture Model Case first and using that as the initial solution. 

[Rob]

Run 10-20 time steps/iterations then see what happens. That way you're not waiting too long if it doesn't work. 

[zain.qazi]

A case was run using the Eulerian model with the Volume Fraction Equation deselected to get an initial solution. The URFs were kept to 0.3 with a first order discretization. Somewhy, after around 500 iterations, the pressure starts to peak and the simulation experiences convergence difficulties and crashes with a Floating Point Exception. Any insights on this peaking pressure?

The mesh is a uniform hexahedral with a y+ greater than 30 as recommended for boiling. For a 1.9x0.25x188mm channel there are approximately 500,000 elements, already refined after previous versions. 

[Rob]

Look carefully at the flow as the divergence approaches. Whilst some of the boiling models are allegedly steady state the resulting multiphase flow usually isn't.

Also, whilst the mesh has y+>30 how does the aspect ratio look? It's a failing in most of the text books: everyone is told about cell aspect ratio, but then doesn't realise that inflated meshes always have a high aspect ratio. That's OK if the solution doesn't change along the cell; this never happens in multiphase..... 

[zain.qazi]

According to the monitors, residuals for k and epsilon seem a bit high but have a reducing trend. The temperature monitors seem to behaving as they should with a rising fluid temp and solid wall temp. The behaviour of massflux report is not exactly at zero but in the order of e-4 and consequently at this point the continuity residual is still a bit high too. The solution is initialized with a 24 bar pressure in the domain as the outlet BC is 21.4 bar to avoid previously faced Reverse Flow problems. Just after the simulation starts facing convergence difficulties the pressure starts to peak. On observing the contours, small circular regions of high pressure (~30 bar) can be seen near the lower heated wall. 

About the mesh, no inflation layers are used. The aspect ratio is still a bit high though as this mesh was made using a reference paper. I have tried with a mesh with lesser Facial Aspect Ratio and have incurred the same problem. The axial node distribution has been studied in many previous researches and has shown to have no significant effect on the results so a suitable number of nodes have been used (530) to keep computation time in check. Here's a picture of the mesh:

[Rob]

Not just the monitors - what is the flow doing? 

[zain.qazi]

The velocity is increasing at a reducing rate from 5 to 40 m/s between the inlet and outlet. High pressure is seen at the inlet around 30 bar and drops to 21 bar at the outlet. The temperature stays more or less constant in the core region. Near the wall it rises to 140 K but is around 80 K in the flow away from the wall. Should increase when the simulation progresses. 

 

[Rob]

Any unexplainable jumps in value? If you have flow at that speed I'd want higher mesh resolution in the fluid zone. And a lower aspect ratio. 

[zain.qazi]

Update: The pressure peaks were probably due to the way I chose to initialize the solution by patching it at 24 bar and having a 21.4 bar outlet BC. I initialized with the outlet and reduced the wall temperature (150 K) as a starting point and the simulation runs very well with Global Time Step at Default URFs.

But this wall temperature needs to be ramped up to 463 K. and going to 190 K already shows fluctuating (within a specific range) monitors for e.g the pressure in the picture below. I am wondering if this could be a problem of the flavour of RPI that I am using which right now is the standard one. Any insights on this would be very helpful. 

Also, any tips on whether to use Psuedo Time Stepping (Global Time Step) is a good way to proceed or not or maybe playing around with Flow Courant number could be helpful here.

 

Thanks

[zain.qazi]

[Rob]

You want to keep the Courant Number fairly low, so for PBCS I'd try 20-50 and see if that helps. The problem may be down to a sudden phase change in a cell, hence looking at contours etc to understand what's going on.