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

Centrifugal Pump Cavitation

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 30, 2018, 08:11
Default
  #21
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by Christophe View Post
Also, 24 total seconds, may take a very very long time to solve. Especially when using a proper time step for transient turbo machinery. These settings are probably appropriate for something rotating at 100 rpm.
I have written the following details for my transient simulation:
Total Time=10s
Time steps=0.001 s
Initial time=0 s

Output control
Backup:
Time step=100

Transient Results:
Time step interval=10

Does the Solution for the transient simulation look right so far as seen from the attached pictures?
Attached Images
File Type: png Monitor.png (29.9 KB, 16 views)
File Type: png transient.png (60.0 KB, 17 views)

Last edited by DKY2Y; January 30, 2018 at 15:46.
DKY2Y is offline   Reply With Quote

Old   January 30, 2018, 16:53
Default
  #22
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Please do not PM me with duplicates of posts you have made on the forum. If it is on the forum I will see it.

Is this a steady state or transient simulation?

This does not look converged adequately.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 30, 2018, 16:59
Default
  #23
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Please do not PM me with duplicates of posts you have made on the forum. If it is on the forum I will see it.

Is this a steady state or transient simulation?

This does not look converged adequately.
Yeah it is a transient simulation however the simulation has not converged yet. It has been running for the past 24 hours.

The youtube video which I was watching used a transient simulation of an impeller and volute excluding cavitation. However I used the same values of time steps as the video did.
DKY2Y is offline   Reply With Quote

Old   January 31, 2018, 04:39
Default
  #24
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Before you do any simulation you need to do some basic validation and verification first. The most important bit of this is to determine what mesh, time step and convergence criteria is required for your simulation.

The time step size is simplified by using adaptive time steps, homing in of 3-5 coeff loops per iteration. Then the solver will find its own time step size.

But you should do a sensitivity analysis on mesh size and convergence criteria first, so you know what settings you need for the accuracy you require.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 4, 2018, 13:25
Default
  #25
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Before you do any simulation you need to do some basic validation and verification first. The most important bit of this is to determine what mesh, time step and convergence criteria is required for your simulation.

The time step size is simplified by using adaptive time steps, homing in of 3-5 coeff loops per iteration. Then the solver will find its own time step size.

But you should do a sensitivity analysis on mesh size and convergence criteria first, so you know what settings you need for the accuracy you require.
Thank you, the transient simulation worked. Does the result look alright for now? My project supervisor asked me to increase decrease the time step to enhance the convergence. I will repeat it again to get a better result.

It should be noted that the output normal force is high mainly due to the centrifugal pump which has high volume flow rate and output discharge pressure.
Attached Images
File Type: png results 1.png (33.2 KB, 18 views)
File Type: png results 2.png (31.8 KB, 16 views)
File Type: png results 3.png (31.7 KB, 17 views)
File Type: png results 4.png (24.6 KB, 16 views)
File Type: png results5.png (21.1 KB, 14 views)
DKY2Y is offline   Reply With Quote

Old   February 4, 2018, 16:42
Default
  #26
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I have no idea what you are looking for so cannot say if those results are OK. The main thing you do to check a simulation is OK is:
* validate against a benchmark result or experiment results.
* Do sensitivity analyses of mesh size, convergence criteria and time step size to check they are OK
* Other considerations are listed in the FAQ.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 18:04
Default
  #27
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
I have no idea what you are looking for so cannot say if those results are OK. The main thing you do to check a simulation is OK is:
* validate against a benchmark result or experiment results.
* Do sensitivity analyses of mesh size, convergence criteria and time step size to check they are OK
* Other considerations are listed in the FAQ.
Hi, thank you for assistance. I have a question regarding writing an expression on CFX Pre. This is for NPSHA. The journal article I am using defines NPSHA as :
NPSHA= Pinlet - (Pv/ Density *g)

The vapor pressure is 3170 Pa at 25 degrees. I have written the following expression if you could check if it is correct as I am not too sure if I should input my vapour pressure as Pa or another unit within the expression:
massFlowAve(Total Pressure in Stn Frame )@ R1 Inlet-(3170/(1000*9.81))
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 18:08
Default
  #28
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I would recommend:

areaAve(p)@ R1 Inlet-(3170[Pa]/(areaAve(Density)@ R1 Inlet*g))

You should use static pressure, not total pressure; you should get density from the simulation rather than hard coding it; might as well use the internal variable "g" for gravity; and you should define units for quantities with units.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 18:20
Default
  #29
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
I would recommend:

areaAve(p)@ R1 Inlet-(3170[Pa]/(areaAve(Density)@ R1 Inlet*g))

You should use static pressure, not total pressure; you should get density from the simulation rather than hard coding it; might as well use the internal variable "g" for gravity; and you should define units for quantities with units.
Thank you. Before I start the simulation, I have used the following boundary conditions for the inlet pressure. I used 1.63 Pa static pressure with respect to 0 atm Reference Pressure. Outlet is given by mass flow rate obtained from the journal.

I obtained the value for the inlet pressure by working it out from the NPSHa formula since one of the NPSH values given in the journal article was 1.31 m. Is this a good way for obtaining the inlet pressure boundary condition in order to get 1.31 m NPSH?
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 18:26
Default
  #30
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The inlet at 1.63Pa with a reference pressure of 0 atm does like an extreme vacuum to me. Does this pump operate in a vacuum environment?

Most of the time you want to set the inlet pressure to 0 [Pa] and you use the reference pressure to set the pressure level.

But I cannot answer your last question without further information: Is this a incompressible or compressible simulation? Are you modelling cavitation?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 18:39
Default
  #31
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The inlet at 1.63Pa with a reference pressure of 0 atm does like an extreme vacuum to me. Does this pump operate in a vacuum environment?

Most of the time you want to set the inlet pressure to 0 [Pa] and you use the reference pressure to set the pressure level.

But I cannot answer your last question without further information: Is this a incompressible or compressible simulation? Are you modelling cavitation?
The experimental setup of the pump is shown in the attached picture which indicates that it works in a vacuum environment.

I am modelling cavitation and I am assuming that it is a homogenous model.
Attached Images
File Type: png setup.png (148.3 KB, 14 views)
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 18:47
Default
  #32
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
For your model where the pressure is very close to absolute zero anyway then using a zero reference pressure is OK.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 19:17
Default
  #33
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
For your model where the pressure is very close to absolute zero anyway then using a zero reference pressure is OK.
Oh sorry my fault, the actual equation for the NPSH is:

NPSHA= (Pinlet - Pv)/ Density *g)

So I wrote it down the way you showed me:

(areaAve(p)@ R1 Inlet-3170[Pa])/((areaAve(Density)@ R1 Inlet*g))

Hence from calculations and from the change in formula the inlet pressure changed to 1602.1 kg/m3. Does it sound sensible to use this for my boundary condition since it increased?
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 19:45
Default
  #34
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
kg/m3 is the units for density. Please check your units.

And if you meant 1602 Pa then your pressure is less than the vapour pressure of your liquid. Is this what you intended? Does the fluid enter your domain already as a vapour?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 19:53
Default
  #35
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
kg/m3 is the units for density. Please check your units.

And if you meant 1602 Pa then your pressure is less than the vapour pressure of your liquid. Is this what you intended? Does the fluid enter your domain already as a vapour?
Sorry, I meant 16021 Pa. I set up my inlet conditions as the following:
Volume fraction: Water=1 And Vapor 0. The picture shows the cavitation effect for NPSH of 1.31 m from the journal article.
Attached Images
File Type: jpg pic2.jpg (29.1 KB, 20 views)
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 20:00
Default
  #36
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
That is sounding more realistic.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 21:19
Default
  #37
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
That is sounding more realistic.
Something does not seem right with the convergence since the NPSH monitor point is going negative at this point. It must stay steady at a value close to 1.31 m.
Attached Images
File Type: png pic2.png (15.6 KB, 11 views)
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 21:21
Default
  #38
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
What does the convergence looks like? Is it still converged?

What does the flow field look like? Have a look in CFD-Post.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 22, 2018, 21:36
Default
  #39
New Member
 
Joseph M
Join Date: Nov 2017
Posts: 24
Rep Power: 8
DKY2Y is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
What does the convergence looks like? Is it still converged?

What does the flow field look like? Have a look in CFD-Post.
It has converged however the solution looks wrong as shown in the attached pictures.

I think the boundary conditions are incorrect.
Attached Images
File Type: png pic2.png (14.6 KB, 12 views)
File Type: png pic3.png (9.4 KB, 12 views)
File Type: png pic4.png (25.9 KB, 12 views)
DKY2Y is offline   Reply With Quote

Old   February 22, 2018, 21:41
Default
  #40
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Have you read the best practices guide for cavitation modelling in the CFX documentation? That gives a lot of background in how to make cavitation models work properly.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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
Centrifugal Pump Cavitation Simulation in Fluent joshghoun FLUENT 0 September 16, 2014 09:49
CFD simulation of centrifugal pump cavitation billy7590 Fluent Multiphase 0 March 22, 2014 08:28
CFD simulation of centrifugal pump cavitation billy7590 Main CFD Forum 0 March 22, 2014 02:27
Centrifugal Pump Cavitation problem or not. ismael.s CFX 13 February 27, 2012 08:00
cavitation impeller centrifugal pump mino2006 CFX 2 September 19, 2007 12:16


All times are GMT -4. The time now is 05:58.