CFD in Discovery Refine is not converging, high velocities

[todd.moser]

I've got a model of a suspension where I'm forcing oil through an orifice to assess damping performance. All of the oil applied to the inlet must go through the orifice. As I increase my flow rates I'm getting very high velocities through the orifice (around 300 M/s). There is also a huge prssure drop across the orifice that would probably cause cavitation. I'm using  polyhedra mesh and I've refined the mesh at the orifice. I'm currently using engineering convergence (I tried the others, too) and Turbulent K-omega SST

I'm monitoring the mass flow through the orifice which should match the inlet mass flow but it doesn't. Does anyone have suggestion on a settings change that might help? Am I beyond the capability of Discovery?

[jcooper]

Hi Todd:

Flows with constrictions should generally be solvable in Discovery. Multiphase problems may present more difficulty, however, and it is possible that breaking out of the Discovery framework will be necessary to fine-tune the mesh and phase setup. Fluent is generally recommended over Discovery because of the extended control you will have over both. 

All high speed cases face startup problems with the solution.  Flows through constrictions often require a special type of initialization that set up the pressure and velocity fields (hybrid initialization).  Is the flow upstream of the orifice completely supersonic?  If yes, this will end the communication between the inlet and flow downstream of the supersonic region and the solution will diverge. This will happen even in Fluent.  (The reason for this is that the pressure wave that communicates downstream information back to the inlet can no longer propagate upstream.)

Even in a standard CFD solver, you may have to try approaching the target flow rate very gradually to avoid velocity overshoots as the solution converges.  Note that the same mesh may not be good enough for all the flow rates. As flow rates increase, the refinement at the orifice will have to get more rigorous. Body of influence refinement gives the best control. It is therefore possible that the meshes that are coming from the Discovery process are not refined enough for this simulation. You will also have to reduce the solution timestep significantly - this will scale inversely with the maximum velocity. 

The setup of the multiphase fluid is also important.  How is the suspension set up?  What is the carrier fluid?  Are there any compressible phases?  If the interfacial area is described using an effective diameter, reducing this diameter will make the solution more sensitive and increasing it (to a point) will make the solution more robust.  Fluent may give more control over the modelling in this respect. Modelling a compressible phase as incompressible may result in an insoluble problem because the fluid density is unable to respond to the pressure changes.  The result will be that velocity is supersonic when it should be subsonic.

I hope this helps.

Regards