CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Centrifugal pump impeller simulation doesn't converge

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 29, 2019, 15:24
Default Centrifugal pump impeller simulation doesn't converge
  #1
New Member
 
Juan Felipe Rincón Franco
Join Date: Aug 2018
Posts: 12
Rep Power: 7
JuanRincon is on a distinguished road
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.

Last edited by JuanRincon; April 29, 2019 at 15:40. Reason: adding information about boundary conditions.
JuanRincon is offline   Reply With Quote

Old   April 29, 2019, 19:04
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 30, 2019, 05:23
Default
  #3
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 209
Rep Power: 13
Jiricbeng is on a distinguished road
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.
Jiricbeng is offline   Reply With Quote

Old   April 30, 2019, 09:40
Default
  #4
New Member
 
Juan Felipe Rincón Franco
Join Date: Aug 2018
Posts: 12
Rep Power: 7
JuanRincon is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.

Quote:
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.
JuanRincon is offline   Reply With Quote

Old   June 24, 2019, 08:21
Default
  #5
New Member
 
Kishan Patel
Join Date: Mar 2019
Posts: 2
Rep Power: 0
kishan_042 is on a distinguished road
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.
kishan_042 is offline   Reply With Quote

Old   June 24, 2019, 08:55
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 25, 2019, 03:55
Default
  #7
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,818
Rep Power: 27
Gert-Jan will become famous soon enough
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........ ;-)
Gert-Jan is offline   Reply With Quote

Old   June 25, 2019, 06:52
Default
  #8
New Member
 
Kishan Patel
Join Date: Mar 2019
Posts: 2
Rep Power: 0
kishan_042 is on a distinguished road
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?
kishan_042 is offline   Reply With Quote

Old   June 25, 2019, 06:59
Default
  #9
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,818
Rep Power: 27
Gert-Jan will become famous soon enough
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..
kishan_042 likes this.
Gert-Jan is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Out File does not show Imbalance in % Mmaragann CFX 5 January 20, 2017 11:20
Want Impeller Driven Fluid Flow: What Inlet and Outlet BC to use for Centrifugal Pump Zev Xavier FLUENT 3 May 9, 2016 07:42
Differing Pitch Centrifugal Pump Simulation Problem [OpenFoam] k.vimalakanthan OpenFOAM 2 July 16, 2015 08:31
Centrifugal Pump simulation b.eshghi Main CFD Forum 8 November 13, 2010 03:06
Centrifugal Pump and Turbulence Model Michiel CFX 12 January 25, 2010 04:20


All times are GMT -4. The time now is 01:31.