|
[Sponsors] |
April 7, 2020, 07:15 |
|
#21 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
Pls find the necessary pics of velocity an total pressure in stationary frame.
Inlet BC : 2.4 bar total pressure in stationary frame Outlet BC : Mass flow After simulation: Inlet Total Pressure :67.86 bar Outlet Total Pressure : 9.51 bar Last edited by ruchit@15847; April 7, 2020 at 10:06. |
|
April 7, 2020, 07:24 |
|
#22 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
I asked velocity in stationary frame. Not Velocity. So please plot the Velocity in Stationary frame. And not as vectors but as contours. Also, add small black vectors (on top of it) of velocity in stationay frame (1000 vectors, equally spaced, projected tangential)
Also calculate the total pressure drops in stationary frame. And remove the blue background. Blue vectors on a blue background is a very bad idea. Don't you think? |
|
April 7, 2020, 07:45 |
|
#23 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
Pls find the updated pic of velocity in stationary frame.
I am not getting which total pressure drop u r asking. Last edited by ruchit@15847; April 7, 2020 at 10:06. |
|
April 7, 2020, 08:00 |
|
#24 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
You mentioned:
After simulation: Inlet Total Pressure :67.86 bar Outlet Total Pressure : 9.51 bar If you want to evaluate pressure drop, then you need to evaluate the values in stationary frame. |
|
April 7, 2020, 08:01 |
|
#25 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
Yes..This values are evaluated in stationary frame.
|
|
April 7, 2020, 08:03 |
|
#26 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
Regarding your first velocity vector plot, what do you think of the direction of the vectors?
|
|
April 7, 2020, 08:14 |
|
#27 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
R u asking why the direction of vector is towards inward ??
Let me know u I am rotating domain in -40000 RPM (i.e. direction of rotation is negative Z direction). Stationary coordinate system is such that positive Z is coming out of the plane for all pics I have uploaded. Are u thinking that the sense of rotation of domain is wrong? |
|
April 7, 2020, 08:21 |
|
#28 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
I don't know how everything is orientated since your axis is invisible. Neither do I know if your origin is in the center. Please check.
Anyway, the rotation direction is wrong. Don't you think, based on the vectors you plot? |
|
April 7, 2020, 08:45 |
|
#29 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
Ok. I will check the direction of rotation. But, Is it necessary that the axis about which the pump is rotating should pass through the origin of the pump? Like I have shown in attached fig.
Last edited by ruchit@15847; April 7, 2020 at 10:06. |
|
April 7, 2020, 09:58 |
|
#30 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
No, it is not necessary to rotate around the origin. You can rotate around any axis you like. As long as it is in the middle of your rotor. Better check this!
Nevertheless, the rotor should push the fluid towards the outlet (since you say it is a pump....). So if you look to your geometry, then the rotation direction is clear, isn't it? You could argue about the rotor itself. Isn't it inverted? |
|
April 7, 2020, 10:30 |
|
#31 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
Yes. I cheeked. The rotational axis and central(middle) axis of the pump was not matching. Now I corrected and running the simulation. I will let u update.
But one more question : Since I am running at such a high RPM of 40000, should I increase the RPM in simulation gradually or should I run the simulation directly at 40000 RPM ? |
|
April 7, 2020, 11:08 |
|
#32 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
That depends. It could be that CFX survives a start from scratch. If not, then ramp it in 3 steps. Should be enough.
BTW, why do you remove the pictures? |
|
April 7, 2020, 15:07 |
|
#33 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
Now, I matched the rotational axis of pump with central axis which also solved the direction issue of vectors in Impeller blades which u can see in attached figure.
Inlet BC : 2.4 bar (Total Pressure in Stationary Frame) Outlet BC : 4.89 kg/s After Simulation: Total Pressure in Stationary Frame at Inlet: 2.4 bar (Now it is coming) Total Pressure in Stationary Frame at Outlet: -13 bar Total Pressure in Stationary Frame at Interface between Impeller and Volute = 44.081 bar which is less than Total pressure in Stationary Frame at Outlet. I don't know why it is reducing ? Direction of Rotation : -40000 RPM (Direction of axis of rotation in negative Z direction) Pls find the attached figure of Contour of Total Pressure an Velocity (both in Stationary Frame). In Figure, Positive Z axis is coming out of the Plane. I had to delete the pics due to confidential. Last edited by ruchit@15847; April 8, 2020 at 06:19. |
|
April 7, 2020, 16:32 |
|
#34 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
As mentioned before, your impeller needs to be inverted. It looks like you have chosen a turbine geometry and use it as a pump. This can't work at all.
|
|
April 7, 2020, 16:50 |
|
#35 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
My impeller is inverted means sense of rotation of impeller is wrong. Right??
I am also running one more simulation with opposite rotation as compared to previous one. Still Simulation is running but here I am getting Good result. I will update once it will finish. |
|
April 7, 2020, 16:55 |
|
#36 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,908
Rep Power: 28 |
Impeller geometry is not a pump but a turbine. You can't pump with it.
Rotation direction is right. |
|
April 7, 2020, 17:20 |
|
#37 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
How r u judging my impeller geometry is not pump but turbine? Are u judging based on the higher inlet pressure than outlet pressure?? May be I am missing somewhere else in setup in simulation ??
|
|
April 8, 2020, 00:57 |
|
#38 |
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 8 |
I did two simulation with same Geometry with same case setup except direction of rotation of rotor.
For both simulation, I gave following BC : Inlet BC : 2.4 bar (Total Pressure in Stationary Frame) Outlet BC : 4.89 kg/s Simulation 1: With -40000 RPM (axis in negative Z direction) Total Pressure in Stationary Frame at Inlet: 2.4 bar Total Pressure in Stationary Frame at Outlet: -13 bar Simulation 2: With 40000 RPM (axis in positive Z direction) Total Pressure in Stationary Frame at Inlet: 4.1 bar Total Pressure in Stationary Frame at Outlet: 165 bar |
|
April 24, 2022, 15:14 |
need help
|
#39 |
Member
Vivek MJ
Join Date: Oct 2020
Location: India
Posts: 53
Rep Power: 6 |
Hi, my question is related to the post. i doing centrifugal pump simulation in 2.5D using steady frozen rotor approach in fluent. I would like to know how to calculate the meridional velociity?
what do i need to do to calculate the discharge coefficient, hydraulic efficiency and other parameters? please help me |
|
April 24, 2022, 21:19 |
|
#40 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,850
Rep Power: 144 |
What do you mean 2.5D? I use 2.5D to mean where the flow domain is 2 dimensional, but you are modelling 3 velocity directions - so you are including out of plane velocities. This is usually done with a periodic boundary.
I cannot see how you can model a centrifugal pump in 2.5D, as I understand it. Also - this is the CFX forum, for questions about Fluent try the fluent forum. But your question seems to be more about post processing anyway.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
Tags |
centrifugal pump |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
CFX High speed wall function-ERROR | Fabiio87 | CFX | 5 | April 29, 2021 13:53 |
Power calculation in centrifugal pump - CFD Post | Hazem_9 | ANSYS | 1 | May 11, 2017 15:22 |
Strange high velocity in centrifugal pump simulation | huangxianbei | OpenFOAM Running, Solving & CFD | 26 | August 15, 2014 03:27 |
Autoblade centrifugal pump template | mahdi balali | Fidelity CFD | 3 | February 18, 2014 09:56 |
how to solve the diverage of high speed centrifugal compressor, CFD code is STAR CCM | layth | STAR-CCM+ | 3 | May 21, 2012 06:48 |