RFR Gear Simulation Problem
 

I am running a multiphase transient simulation of a rotating gear half-submerged in oil.

The rotating speed accelerates to 100rpm over 1sec, then stays constant for 1sec.

The time step is set at 0.002s which gives an RMS courant no. in the correct region of 2-10 for most of the simulation, until the simulation crashes at 621 timesteps (1.24secs).

Picture below is of Oil Volume Fraction at moment of crash
https://www.cfd-online.com/Forums/me...884-crash.html

The error code is

ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Overflow |
|

This simulation ran with homogeneous fluid models, laminar flow with a mixture model added in the interphase transfer model option.

The domain interface pitch change is set to none, this is assumed to be correct because both sides of the interface match up. I have also added intersection control to the interface.

In Solver control I have also used Multiphase control > Volume Fraction Coupling > Segregated

There is also an opening in the top of the domain with 0[Pa] relative pressure set to entrainment.

If there is an expert out there who could advise on anything I could try to stop the simulation crashing, I would greatly appreciate it!

Link below is a video of a previous simulation but stopped at 600 timesteps.

https://www.youtube.com/watch?v=YfaM...ature=youtu.be

Over flow error is an FAQ: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

In your case I would be very suspicious about your time step size. Try adaptive time stepping, homing in on 3-5 coeff loops per iteration. This is a much more robust approach than Courant number, especially for multiphase flows.

Thanks!
 

@ghorrocks thanks for your reply! I think I already have adaptive timestepping? With a max number of coefficient loops set to 5..

It seems the issue I'm having is related to the break-up of the free-surface. Homogeneous fluid model settings inherently mean shared velocity for both fluids (oil and air).

I would like to make the fluids inhomogeneous, but the simulation crashes after a very small number of timesteps with

ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+---------------------------------

Any advice on improving convergence aside from lowering timestep?

What are your initial conditions ? Starting from rest ? How are you increasing the speed from 0 rpm -> 100 rpm in 1 sec ?

May I ask what is the goal of computing the transient in the first 1 sec ?

Have you tried to run the case steady state case @ 100 rpm ? Running steady cases is a lot easier, and you can infer a lot of information from those results to later model the transient case if really needed.

Regarding your pitch change model, you have not indicated which frame change model you are using. If you have a transient rotor stator frame change model, the code needs to know the pitches on both sides of the interface regardless if the two meshes perfectly match at the start of the run.

@Opaque thanks for your reply!

Yes my initial conditions are starting from rest.

Regarding the Pitch change yes Transient Rotor Stator, so you are saying its best to change the setting from none to specified angle, then set the angle to zero if they are perfectly aligned?

To the best of my knowledge this case will not run in steady state with buoyancy added as the solver cannot add gravity in a rotating frame. (This is from trying to run this case in Steady State, it then crashing, and the solver error messages suggesting to run a transient simulation).

The ramped/accelerating speed is to try and improve convergence, as I have had issues with simulation crashing if the speed is set immediately to 100rpm. The acceleration is a simple IF statement stating if t<1 it is accelerating to 100rpm, and t>1 the speed is 100rpm.

Here are some ideas I would have used:

Run the case in steady state w/o buoyancy and learn from the results

A a better understanding of the pitch change model setting. For the specified angle option, you must enter the pitch of the passage on either side. Say you have a 1/4 wheel on side 1, you enter 90 [deg], and if you have a 1/3 wheel on side 2, you enter 120 [deg]. That is, you enter the pitch angle on either side, not the pitch differences.

Now, you start the calculation with the steady state results with or without buoyancy.

The segregated volume fraction coupling is the default option.
I got much more stable simulations when using the coupled (implicit solving of the volume fraction with the hydrodynamic eq) option.
Will be a bit more comp. time consuming but is worth a try.

Often the coupled VF solver converges quicker than the segregated solver, so simulation time is shorter. But this depends on the exact simulation, some are slower.