[Hamidzoka]

Dear venkat;
When the CFL falls below 0.1 while the convergence problems still exists, the source of problem is definitely somewhere else. So, reducing the CFL to 0.0000001 does not help at all!
Following suggestions come to my mind regarding your case:

- Try total pressure at inlet boundary instead of velocity. it is a more stable condition at inlet.
- Check if your boundary conditions are consistent and physically meaningful. moving walls, direction of rotation, amount of pressure, etc.
- Change the output pressure condition from radial equilibrium to averaged one. radial equilibrium condition sometimes induces instabilities within the flow field.
- Make sure that you have set a proper initial velocity field in the axial direction so that the fluid can find an initial stream from inlet to outlet.
- Check the mass flow and make sure that it is physical.
- Check that if your have properly defined rotor/stator interface.
- Check that if you have correctly defined moving and stationary parts.

In general, early divergence in CFD simulations is caused by a mistake in setting boundary conditions, initial conditions or wrong geometry arrangements.
I hope it helps.

Regrads

[StretchyAlien]

A bit late on the reply here, but my experience with the viscosity clipping is that it tends to be an issue with your initial solution. Here's why I think that:

The documentation states that the viscosity clipping occurs to prevent the solution from blowing up when mu and mu_turb are very different. This happens most frequently when there is a velocity spike in the flow field. That being said, it isnt a bad thing if the solver prints this message out, so long as it stops printing before you use the solution (it is artificially changing the solution when this message is printing). If you can initialize the flow field to something closer to what you expect the final answer to look like you can sometimes avoid this issue altogether.

Have you tried running an initialization case with easier BCs? With the rotor at 0 rpm?

If you ever did solve the issue, let us know what you did.

[supafly]

Hi, I have similar problem with clipping Mu/Mt and convergency. My case is high pressure centrifugal compressor with IGV (row 1), impeller (row 2) diffuser (row 3) and straighter (row 4) vanes.
Could somebody tell me, may such mesh quality be the reason of numerical unstability?



So it's very strange that i have good convergence at low pressure at outlet, pretty convergence at high pressure at outlet, but between them calculation is blew up. there is no mass flow or pressure ratio pikes during calculation, it's just message

! DENSITY NEGATIVE IN DOMAIN 10
! PRESSURE NEGATIVE IN DOMAIN 10 1 1 1
! DENSITY NEGATIVE IN DOMAIN 22
! PRESSURE NEGATIVE IN DOMAIN 22 1 1 1

and so on at some iterration, then solution crushed.

maybe some changes in expert parameters needed?
I change just
MVRELF 0.9-> 0.45 (rel/f for meshes with high Aspect ratios/Skew angles)
RQSTDY 1->0 rel/f for mixing plane int/
MUCLIP 5000->50000 (as recommended in manual)


BC's are total pressure/temp at inlet, static pressure at outlet