[JuanRincon]

Hi, as the title suggest i have been simulating a centrifugal pump impeller but the simulation does not converge.
I did read some threats where this comunity suggest:


Changing the boundary conditions:

well, right now my inlet is static pressure, with a zero gradient turbulence model, and the outlet is mass flow. I believe those are strong conditions to secure convergence. how ever i try to change them by using the data from an old simulation that already converge, to use mass flow as inlet and averaged static pressure as outlet, the turbulence model choosen is medium (5%)


refining the mesh:
inicially I was using a patch conforming without inflation layer, then I switch it to a patch conforming with 5 inflation layers (smooth transition, growth rate 1.2, transition ratio 0.7). In the last simulation I change it again to a patch independent with 8 inflation layers ( smooth transition, growth rate 1.2, transition ratio 0.2 due to very thight channels).

changing the turbulence model.
initially i was using the SST model, then i switch it to K-e model, in which the imbalances were better, so i think i'm going to stick with it.

As a convergence parameter i'm using RMS with a value of 3e-5, checking imbalances and monitoring pressure velocity and head, and torque, the variables that I need.

also, before this simulation I run the same geomeotry varing the mass flow with a parametric study, for that i did used the inicial conditions (patch conforming without inflation layer, SST turbulence model, RMS 5e-5), I did get results, and they where coeherent, but i needed the results fot post procesing.
Can i use the information obtained as an initial value? if so, how?

I would like to share the geometry but i can't due to confidenciality issues.
If you guys got an idea or need more information please ask me.

thank you very much.

[ghorrocks]

You should be choosing boundary conditions, turbulence models and mesh size according to match the physical system you are modelling (with mesh size determined by a sensitivity study), not what converges better.

Tips on getting convergence are here: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[Jiricbeng]

I think the main issue is the static pressure at the inlet. Switch the static pressure to total pressure at the inlet. It should work. I have very bad experience with static pressure at the inlet and mass flow at the outlet combination.

Btw I guess you assume the pump sucks the liquid from a tank in which you know the pressure. Since the liquid in the tank has low velocity, setting total pressure is even more physical.

[JuanRincon]

Originally Posted by ghorrocks

You should be choosing boundary conditions, turbulence models and mesh size according to match the physical system you are modelling (with mesh size determined by a sensitivity study), not what converges better.

Tips on getting convergence are here: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Hi, thanks for the answer. I didn't really like what i was doing, and I wanted to stay with the inicial boundary conditions.the problem is i've been simulating for just 1 year, and i have learn a lot but i still need to learn a whole lot to so probably I was wrong with the setup, that and the threats where I read change the mesh size or the turbulence model, or the boundary conditions.

Originally Posted by Jiricbeng

I think the main issue is the static pressure at the inlet. Switch the static pressure to total pressure at the inlet. It should work. I have very bad experience with static pressure at the inlet and mass flow at the outlet combination.

Btw I guess you assume the pump sucks the liquid from a tank in which you know the pressure. Since the liquid in the tank has low velocity, setting total pressure is even more physical.

you are totally right Sr, i didn't realise that, i'm going to try it.

thank you.

[kishan_042]

I was also doing a Simulation of Pump.

Model: SST-kw
Total Pressure Inlet
Mass Flow Outlet
Meshing with: Curvature (Fine)
Scheme: Coupled

But Still, I am getting 15% Higher Head than Experiment, and Efficiency around 20% Lower than the Actual, please suggest the right method of doing this.

Thank you in anticipation.

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[Gert-Jan]

When setup correctly (mesh, BC's, numerics) my experience with (mixed flow) pumps is that CFX is quite accurate. As long as you base your calculation on time averaged results and do second order timestepping (=default). Use Total Pressure difference for efficiency calculation.

Mostly, I trust my CFX calculations more than experiments performed by others........ ;-)

[kishan_042]

When I use pressure difference, ie. Total Pressure Inlet & Static Pressure Outlet I get floating point error while doing Initialization (Scaler-0 remains 0, Scalar-1 Doesn't reach a limit of 1x10-6).

is there any specific reason I am getting this error?

[Gert-Jan]

I don't know what you are doing. Guess you are now performing a calculation where with pressure on both inlet and outlet. That is a bad idea. Go back to your previous setup with massflow at the outlet.

I only mentioned that if you calculated the efficiency (outside CFX), you should base that on total pressure difference between inlet and outlet. Not static pressure..