[NumericCFD]

I am conducting a steady state model of a single blade passage of Francis turbine runner. I have designed a runner using CFTurbo and exported it to turbogrid. I have successfully meshed the geometry.

When I run the model, the residuals decrease consistently for some iterations however, they diverge and the model crashes (see attached photos)

I have setup a solver monitor point that calculates the hydraulic efficiency of the turbine blade. When monitoring this point, the efficiency converges to approximately 88% rather early (many iterations before the residuals diverge). If I prematurely stop the solver when the efficiency has converged, I get nice looking pressure profiles on the blade and decent streamlines. However, if I leave it to iterate until it diverges the solution crashes. (See attached photos). The mid solution pressure profile and streamlines show that the geometry is being accepted by the solver. Looking at the same output when it crashes though is creating confusion as it appears the water is no longer entering the passage (based of the streamlines).

The design software in CFX states that the efficiency for the flow conditions should be around 88%.

Model Schematics
Turbulence model: SST
Advection scheme: Upwind
Turbulence numeric: First order
System dynamics: Rotating at 333 RPM
Inlet conditions: Mass flow rate = 3990 kg/s
Cylindrical components: A = 0, R = 0.262752, T = 0.96486
Outlet conditions: Static average pressure 1: atm
Mesh characteristics: I've tried with different mesh node counts from 200 000 to 1 200 000, but achieve same results. Y+ value is small enough based of literature



Thanks for helping!

[ghorrocks]

See FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

I think the FAQ covers everything you should look at in this case.

An additional comment: When a CFD simulation diverges the results then become very weird. So it is not surprising that your flow field after the divergence has weird pressures, flow velocities and even the flow direction is completely wrong. SO do not pay any attention to a diverged simulation. But looking at the results when the residuals start increasing (but have not gone completely crazy) should give you an idea of where the problem is. Do a run where you add the residuals to the output file and stop the run when the residuals start increasing. Have a look at the residuals in the results file in CFD-Post and it should show you where the problem area is.

[Opaque]

Originally Posted by NumericCFD

I am conducting a steady state model of a single blade passage of Francis turbine runner. I have designed a runner using CFTurbo and exported it to turbogrid. I have successfully meshed the geometry.

When I run the model, the residuals decrease consistently for some iterations however, they diverge and the model crashes (see attached photos)

I have setup a solver monitor point that calculates the hydraulic efficiency of the turbine blade. When monitoring this point, the efficiency converges to approximately 88% rather early (many iterations before the residuals diverge). If I prematurely stop the solver when the efficiency has converged, I get nice looking pressure profiles on the blade and decent streamlines. However, if I leave it to iterate until it diverges the solution crashes. (See attached photos). The mid solution pressure profile and streamlines show that the geometry is being accepted by the solver. Looking at the same output when it crashes though is creating confusion as it appears the water is no longer entering the passage (based of the streamlines).

The design software in CFX states that the efficiency for the flow conditions should be around 88%.

Model Schematics
Turbulence model: SST
Advection scheme: Upwind
Turbulence numeric: First order
System dynamics: Rotating at 333 RPM
Inlet conditions: Mass flow rate = 3990 kg/s
Cylindrical components: A = 0, R = 0.262752, T = 0.96486
Outlet conditions: Static average pressure 1: atm
Mesh characteristics: I've tried with different mesh node counts from 200 000 to 1 200 000, but achieve same results. Y+ value is small enough based of literature



Thanks for helping!

Since your model seems to converge quickly. My advice is:
1 - Add Output Equation Residuals = All to your backup files, and results file.
2 - Set backup files for iterations 20, 40, 60, 80
3 - Post-process those backup files to locate the maximum residual for the continuity equation, P-Mass, and analyze the flow conditions around that area, mesh quality, etc.
4 - Diagnostics from the output file @ iteration 20, and 40. Something seems off? High effort count? OK, vs ok/F ?