CFX diffuser simulation
 

Dear All,

I'm a new user of CFX and would greatly appreciate any comments on my set-up. I've been trying to do steady state simulation of one passage/segment of a radial diffuser on a multistage centrifugal pump, without heat transfer. It's a complicated strongly 3D shape, with a diffuser section capturing water ~ 28 m/s from a centrifugal impeller, diffusing it over a short roughly tangential passage, then turning it through 180 degrees, and directing back into the eye (centre) of the next impeller stage. I have tried various approaches with little success re convergence. I'm about to try again to get a good solution, but any comments would be very welcome!

Mesh: I currently have several meshes approx 100K elements. Y+=80. Max aspect ratio is 335, which CFX does not flag up (despite help manual advising <100). Orthogonality is 11 max - it flags this up in the .out file, and likewise with expansion factor - almost 1900. I'm using CFX mesh (also beginner here) but struggling to figure out how to control the mesh internally - there are very acute angles in the model where surfaces converge. I use inflation but it's collapsing in these regions which I think is causing a lot of the convergence problem.

Boundary conditions: Inlet was set to opening as advised by error message (due to backflow requiring artificial wall), with static pressure 0 & entrainment direction. Outlet set to outlet and mass flow rate.

Turbulence: Using KE with scalable WF to try and obtain any sort of converged solution, hope to use KO SST as separation seems certain, given the geometry.

Solution: No convergence. Residuals osc. sharply (numerical instability?) Max can be two orders of magnitude greater than RMS (localised grid quality?). Reducing the timestep hugely (1e-5) removed the oscillations.

Plan: 1)Further hair pulling with CFX mesh- improve mesh quality until the min ortho angle & expansion factor aren't flagged up.

2)Set boundary conditions to: inlet= inlet & mass flow, outlet = outlet & static pressure = 0 (switch to opening if required then back to inlet/outlet later in solution)

3)Run steady state, reduce timestep, switch to opening BC if necessary, hopefully reach some convergence

4)run transient initialised with the steady state solution.

Any comments on my logic/understanding would be greatly appreciated, as would tips for controlling orthogonality angle and expansion factor.

Thanks!

Ianto

Re: CFX diffuser simulation
 

Some thoughts:

Ideally you would want to shoot for y+ = 1 for SST. The CFX mesher is able to estimate the first cell height of your inflation if you have some knowledge of the flowfield, e.g. Reynold's Number. If not, a first cell height ~ .001" should yield y+ ~1-10 depending on your local grid size. Expansion factor for the inflated boundary should 1.2-1.4. The aspect ratio of the last cell of the prism layer to the first cell of the tet layer should be 0.5-2 to limit numerical diffusion (denoted by oscillating residuals).

Even though the manual says aspect ratios should be < 100, experience tells me you'll probably be fine so long as you keep it < 500.

If you're having trouble getting a region to inflate try increasing the minimum internal angle to, say, 10 or 15 degrees.

You can probably set your inlet back to the inlet boundary condition. If you have inflation abutting your inlet it's very common to have CFX backflow within the first few layers. Check the error message. If it's saying you're only backflowing ~2% of the faces or something < 1% of the total inlet area then you're within the inflated boundary. Velocity magnitudes in the tangential direction within the viscous sublayer should be very very low, near zero, which is why CFX tends to backflow in that region.

How do you determine your timestep? I usually use 1/3 of the calculated advection time, which for the geometries I typically run can be on the order of 1e-3s. Depending on your grid quality and flowfield 1e-5s may not be unreasonable to start and you can always increase it as the flowfield stablizes.

Hope this was useful.

John

Re: CFX diffuser simulation
 

Hi John, yes thanks - very useful!

I did have Y+ of 1 (I started with the KO model), but raised it to 80 when I went to K-Epsilon, hoping to improve the aspect ratio problems and convergence with the more "robust" (I read "less accurate" for separated flow) KE model. I'll change it back if I ever get a converged solution with KE. Re is ~ 3M. Expansion factor is 1.3.

Regards the aspect ratio of the last cell of the prism layer to the first cell of the tet layer, I don't know what this is or how to extract/calculate it as the cell size varies throughout the domain depending on local geometry, any suggestions?

I've now output the residuals and refined the mesh in the Max resid areas using controls, changed the inlet to "inlet mass flow" outlet to "outlet zero static pressure", reduced timestep to 3E-05 (advection time is 9E-03) and trying another run. SO far it isn't looking any more likely to settle down than before.

When I run it in solver I still get alerts:

Minimum Orthogonality Angle [degrees] = 9.5 ! Maximum Aspect Ratio=335.6 ok Maximum Mesh Expansion Factor=674.6!

Which despite having (i think) tweaked all aspects of the mesh, are exactly the same figures as before. Does this make sense?

I'm going to stop it again and plot the residual locations as they aren't going anywhere, just oscillating so sharply they make a continuous thick band across the screen. Any other suggestions would be very much appreciated.

Thanks again for your input!

Ianto.

Re: CFX diffuser simulation
 

Try increasing the timestep to 3e-3s. Also, CFX uses a geometric expansion to calculate the prism layers. If you know the approximate size of the background mesh, you can estimate the size of the last layer of the prisms and compare. Also, what advection scheme are you using?

Re: CFX diffuser simulation
 

Hi,

Whats the numerical scheme your using? If you have problems with convergence use the upwind with K-e turb model. Then use that info to restart a more accurate simulation. With this kind of BC you wouldnt be simulating reality (i.e impeller flow effects are not considered) but its a good start. You could also try to use TP at inlet and massflow at outlet.The most realistic way is to simulate the impeller and diffuser together.

Re: CFX diffuser simulation
 

Thanks guys, under pressure just now, reply properly later today, using high advection scheme - so upwind first.... okay..., thanks again!

Re: CFX diffuser simulation
 

Hi John/Sans,

I switched to upwind, timescale 3.0E-03 and the residuals plummeted immediately - they're now down below 1.0E-06 - thanks guys!

Could anyone advise which order to refine my simulation - ideally, I want high resolution, transient simulation with KO SST turbluence model, so - is there a best order for switching on each of these settings? Perhaps transient followed by KO-SST then high resolution advection scheme?

Thanks again.

Ianto

Re: CFX diffuser simulation
 

Hi, Answers to your questions are available in the manual under "Robustness and Accuracy". Read the sections "Advice on Flow Modeling" and "Best Practices Guide for Numerical Accuracy". Also search this forum for similar queries on convergence and accuracy.

Re: CFX diffuser simulation
 

Great, thanks!