Learning Forum

[Mona Gläsle]

Hi,

 

I'm currently working on simulating the joule-thomson effect for cryo cooling with real gas CO2. Unfortunately my simulations don't converge. Here's a short overview of my setup:

 

 

1. Geometry
   My geometry has a very small diameter compared to its length. Fist there is a long upstream pipe, then the gas is throttled through a small orifice into a bigger expansion part followed by a downstream pipe. Here's a sketch:
    

 

1. Mesh
   I used the Watertight Geometry Workflow and a poyhedra mesh for the Mesh generating. My Mesh Quality is:

Mesh Size	786574 Cells, 3878491 Faces, 2542058 Nodes
Cell Quality	Orthogonal Minimum = 0.2, Average = 0.97 Skewness Maximum = 0.8, Average = 0.023 Aspect Ratio Maximum = 13.6, Average = 4.2
Surface Quality	Skewness: Maximum = 0.56, Average 0.002

According to the recommendations the mesh quality should be okay.

2. Physics Setup

Inlet	Pressure-inlet with 3.5 MPa, 293.15K
Outlet	Pressure-outlet with 0.6 MPa
Walls	Thickness of 0.0001m, no heat flux
Material	C02, real-gas-nist model
Model	SST k-omega (2equn), with viscous heating

I limited the temperature to 216.65K so that the gas doesn't desublimate or respectively because the real-gas data from the NIST databank for CO2 is only defined in the temperature range from 216.592 K on.

 

3. Solver
   I've tried different solver settings (pressure-based, density-based, solution-steering) for steady-state. I also tried to reduce the under-relaxation factors and the courant number. I tried hybrid initialization or hybrid +FMG initialization. Especially the energy residual remains constant and doesn't decrease at all. I also tried to start without energy, then enabling energy with first order discretization and moving on to second order. But the simulations never converged. My longest simulation was 2000 Iterations. I often get the warning that the temperature limit is reached at some cells (mostly between 5 and 200 cells).

 

Does someone dealt with the Joule-Thomson effect before or know good settings to reach convergence for a compressible real gas problem? Or am I doing something wrong? Should I simplify my geometry? I would be grateful for any help!

 

I look forward to your answers!

 

Kind regards,

Mona

[SVV]

Hi Mona,

Can you try running the case with first order discretization and reduced URF for energy till the residuals settles down and then switch back to the second order and default or atleast .9 URF. 

With pressure inlet condition, I assume you have specified the initial gauge pressure correctly. You can use pressure based solver, if Mach number is low.

When you say simulation is not converging, how bad is it. I would also recommend monitoring Flus imbalance along with residuals.

 

[NickFL]

What V.V. says is excellent. I would also add in that obtaining a solution in only 2000 iterations might be unrealistic with a poor initial solution. What we need to do is give it something that is closer to the true solution so that it doesn't have to work so hard. This is where using a 2D model can be helpful in finding the solution conditions. It will also allow you to find regions of high gradients so that you can create a higher mesh density in these regions. Also having your cells in the wrong area can cause the solution to oscillate and by using the 1st order discretization will add dissipation pushing the solution towards the solution basin.

Geometrically this is not a complex model, but the physics make the modeling difficult. Typically these are the models that you have to "babysit" during the solution process. That means run a few hunderd iterations, SAVE, see what the solution looks like, decide whether to adjust the relaxation factors or go back to the last saved solution. This kind of iterative process allows us engineers to look busy :)

[Mona Gläsle]

Thank you both for your reply!

@V.V.
1. Would you suggest first order discretization only for energy or for all?
2. How low should I go with the URF for energy or with the CFL number?
3. Mentioning the initial gauge pressure is a very good point. First I thought that the flow won't become supersonic so I just set the initial gauge pressure to 10 MPa. But my not converged results so far are indeed supersonic and there is a shock (Mach number > 1). How do I set the supersonic/initial gauge pressure correctly? I set the operating pressure to 0 Pa.
4. As I assume that the Mach number exceeds 1, is the pressure based solver off the table? I still have the feeling that pressure-based works a bit better in my case.
5. I do monitor mass flow rate at the inlet and outlet. It's the same value at the inlet as at the outlet (negative). Is that what you ment with monitoring flux?

With bad I mean things like that:

density-based:

pressure-based:


@NickFL
I will try to run the calculation for more iterations and "babsit" it. In what diensions do you talk? Is the expected time for such a difficult model more like 20000 iterations? Then I'm gonna babysit for days?
The 2D model might be a good starting point, I'll try that.