[Rajaero]

Hello Guys,
I am working on transient multi-phase simulation of Oil inject twin screw compressor (rotors clearance 0.036 mm) by Twin-mesh and CFX. I am getting "overflow" error at 35th and 40th time step.

The following possible changes already made to solve "overflow" error:
1. Tried with k epsilon and SST turbulence model.
2. Different mesh size (max element size 1 mm and 0.8 mm and 2 mm)
3. Different inlet and outlet condition (pressure inlet and mass flow inlet, opening and static pressure outlet)
4. Homogeneous and in-homogeneous with and without free surface model and interface transfer
5. Coupled and segregated multi-phase coupling method
6. Tried with different relaxation parameter and memory allocation factor (expert parameter)
7. run in first order and high resolution
8. Tried with small time step

Note:
I tried all the above changes but still,
I got over flow exactly at 35th time step with first order (advection, transient, turbulence) scheme.
I got overflow exactly at 40th time step with high resolution (advection and turbulence) scheme and second order (transient) scheme.

please someone help me with this "overflow" problem. I truly appreciated your help in advance. I have attached a image of overflow error for your reference.

Thanks...

[Gert-Jan]

You are trying to solve a very difficult problem. I hope you have a lot of experience with CFD.
But lets start here: are you able to run single phase, with only oil.

[Rajaero]

Thanks Gert-Jan
I tried to run the case with single phase (air) (assumed as dry screw compressor) . It worked fine. I solved up to 180 time step (half cycle) with first order ( transient, turbulence, advection) scheme.

But when I use multi-phase its not working. I tried many time with different method.
Thanks...

[Gert-Jan]

Why not use second order transient?


Probably it is in the multiphase but it will be difficult to find the real error. Just a matter of trial and error. I would start as simple as possible and then increase complexity step by step. (You already succesfully passed the first with air.)

- Do you run homogeneous or inhomogeneous?
- Did you try with a very small amount of oil?

[ghorrocks]

Gert-Jan is on the right track - start simple, add the complexity one step at a time.

The only thing I will add is that outputting a backup file a few iterations before it crashes can be useful. You might be able to see what effect is causing it to diverge, or see some non-physical effect occurring.

[Rajaero]

Thanks Gert-jan,
I also tried with second order transient for single phase and multiphase.
Now i am running with homogeneous free surface model.
I also tried with different amount of oil (20 L/min, 45 L/min, 60 L/min). do you want me to use very small amount of oil?
I tried without (heat transfer, buoyancy effect, interface transfer) in order to simplify the problem. But, i did not succeed.
Thanks...

[Rajaero]

Thanks Glenn,
I will follow your suggestions and let you know. if you have any other suggestions please tell me.

Thanks...

[urosgrivc]

Have you tried really small timestep?
What is your courant number and these timestep settings
how many iterations do you need to converge a step?

[Gert-Jan]

First question: is the oil only meant for lubricant, or is the twin screw used as multiphase pump with significant amounts of oil?

- First skip buoyancy, Unless your twin screw rotates with 1 rpm, it won't be of influence

- The amount of oil doesn't say anything to me, since I don't know the dimensions. I would start with a small amopunt (0.01% volume flow), and then double it with each calculation

- You should define min and max volume (or mass?) fractions in your domain. Usually I take 1e-5 for gas and liquid.

- In fact you should run Total Energy since compressibility plays and important role, but a better start could be using Thermal Energy

[Rajaero]

Thanks Urosgrivc,
Actually i am using following expression method for time step size,
TMangleStepR1 1[degree]
TMrotationalSpeedR1 3000[rev/min]
TMtimestep TMangleStepR1/abs(TMrotationalSpeedR1)
TMNumberOfTimestepsperRun 90

I tried to reduce the angle step (1 deg, 0.5 deg, etc..) for time step control
I did not control Courant number for this simulation.
min Coef loop = 3
max coef loop = 5

Thanks...

[Rajaero]

Thanks Gert-Jan,
is the oil only meant for lubricant, or is the twin screw used as multiphase pump with significant amounts of oil?
1.Oil is used to cool the air temperature during compression process
2. It act as a lubricant and hydraulic seal between screw element

Thanks for your advises. I will follow and let you know if it worked.

[Gert-Jan]

You run transient. So, you must be sure that you reach convergence within a time step. Are you sure the max of 5 coefficient loops is sufficient?
I would recommend to plot the residuals inside each time step as well, not only the end value (=default). Look for Monitor Coeff. Loop Convergence in the CFX-help (paragraph 22.1.5.1.1)

[urosgrivc]

It also depends what your conditions are for convergence,
For a complex simulation 0,0001 simply is not good enough.
And I would count a two-faze transient simulation with surface tension a very complex simulation

if you would let say decrease the value to 0.00001 than the timestep would get far smaller to obtain 2 to 5 coefficient loops for convergence in one timestep this would also automatically decrease the Courant number

Transient simulations are just always more complex and computationally expensive than we imagine at the beginning.
But almost any problem can be solved of course and that is the most interesting part of it

Fluent has several advantages ower cfx regarding screw compressor simulation, the main one being overlapping mesh possibility

[ghorrocks]

You are modelling a screw compressor and if this is a multiphase simulation you won't be able to use immersed solids, so you have to use moving mesh and/or keyframe remeshing to model the motion. This is quite tricky to get working as well.

[Rajaero]

Thanks gert-Jan, Urosgrivic, Glenn
I would like to thank for your suggestions.
I will run my case with coeff loop 10 and small time step size.
Unfortunately Twin-mesh (mesh generation tool for rotors) cannot be compile with Fluent. SCORG can compile with FLUENT and CFX but in my company we only have Twinmesh.
Current problem:
I am using following multi-configuration method for my simulation,
Config 1 - (0 to 90 deg)
config 2 - (90 - 180 deg)
Config 3 - (180-270 deg)
Config 4 - (270-360 deg)
each configuration- no of time step 90
total no of time step - 360 (for 1 complete cycle)
I need to run up to 7 cycle (360 * 7=2520 time step needed) to get periodic steady state.
Questions:
1. My first configuration run finished successfully (90 time step). But, simulation stops at 91 time step and give overflow error. Please tell me some suggestion on this?

[Rajaero]

Hello Guys,
I will follow your suggestions about Time step size and Max coefficient loop. I will let you know if it worked.
Problem with Computation time:
I am using 19 cores (IBM local parallel) for this simulation. Based on my time step (0.0003s - approximate time step size) control i need 4 days to complete 1 cycle.
if i reduce the time step size to 0.00001s, i am worrying about my computation time.
is there any-other way without reducing time step size? Just curious?

Thanks....

[ghorrocks]

How are you modelling the screw motion?

If you need a small time step and you want a faster run time then buy a faster computer. If there was an alternative we would have suggested it.

[Rajaero]

Hello Glenn,
Twin-mesh will create a dynamic structural mesh for screw rotors. In cfx we need to read the twin-mesh grids by "Mesh read" and "Junction box routine". I will use expression method to define a direction of motion, RPM for male and female rotors, step angle.
I will let you know if i solved the over flow problem.
Thanks...

[ghorrocks]

Sounds like you are using keyframe remeshing. This is good, it is the only method which will work in your case.

[Gert-Jan]

https://www.twinmesh.com/