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

Boundary condition for tap nozzle water flow

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 23, 2020, 02:19
Smile Boundary condition for tap nozzle water flow
  #1
New Member
 
Malay
Join Date: Aug 2020
Posts: 3
Rep Power: 5
malay1995 is on a distinguished road
Hi Everyone,

I am try to conduct various simulations of tap nozzle design. According to the different designs of nozzle the velocity of the water flowing out of the nozzle should increase and simultaneously the pressure should decrease according to the bernoullis equation.

I know the flow rate of regular resident house is around 0.1kg/s and the pressure at inlet side of nozzle is 3,00,000 Pascals. In my case I used mass flow rate of 0.1kg/s on inlet and kept pressure outlet on the outlet. All the remaining value of pressure are default.

I ran six different designs with similar mesh and boundary conditions. However after the completion of fluent analysis, I checked the inlet pressure and velocity using surface integrals from results and I noticed that the inlet pressure is different in all of the six case and the velocity is similar in all case which is fine.

My main concern is why it is showing different inlet pressure while the boundary conditions are same?

Also please let me know if I am using incorrect boundary conditions. In these study I know the flow rate and I am interested in Velocity and pressure on the outlet side. Experiments show the velocity increases and pressure decreases on outlet side and the flow rate remains constant.

Please find attached images of two of the cases in which it shows different pressure on inlet side while boundary conditions and mesh is same just the design is different.
CASE-01.png

CASE-02.png
Some one please help me out. I am ready to provide any other information if needed.

Thanks & Regards,

Malay
malay1995 is offline   Reply With Quote

Old   August 25, 2020, 11:56
Default
  #2
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
You have zero static pressure at the outlet in each case and constant mass flow. But different designs have different resistance. If resistance is high then you need larger pressure rise to achieve desired mass flow.
There are three parameters that define the flow - velocity (volume flow/area) and two pressures at inlet and outlet. You define two of them on two BC and the third variable is obtained during solution.

Q_{v}=\mu S \sqrt{\frac{2 (P_{in}-P_{out})}{\rho}}


Different designs have different discharge coefficient \mu and therefore each design must have different inlet pressure to satisfy this equation.


Design with low inlet pressure gives you lower resistance.


You can set Total Pressure at inlet and Static Pressure at outlet. This setup will give you different velocity and therefore volume and mass flow rates.

Last edited by karachun; August 25, 2020 at 14:43.
karachun is offline   Reply With Quote

Old   August 27, 2020, 02:22
Default
  #3
New Member
 
Malay
Join Date: Aug 2020
Posts: 3
Rep Power: 5
malay1995 is on a distinguished road
Hi

Thanks for your reply.

I have set the mass flow rate as inlet which is 0.1kg/s and rest all values are default.
In my case I know the mass flow rate and inlet pressure.
I am interested to find the changes in velocity and pressure in various designs as you can see.
I want to know how can i define inlet pressure as 3,00,000 Pascals and mass flow rate as 0.1kg/s.
I do not know how much will be the outlet pressure but it should drop and velocity should increase.
Please tell me the exact boundary conditions to be used with certain values.
Thanks
malay1995 is offline   Reply With Quote

Old   August 27, 2020, 02:38
Default
  #4
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
This BC is nonsense.
You can not set both mass flow and total pressure at inlet and set nothing at outlet.You should set mass flow at inlet and zero static pressure at outlet. Pressure at inlet will be calculated by solver.
If you model incompressible fluid then fluid properties do not depend on pressure level and therefore you don't need to specify operational pressure of 300 000 Pa.
karachun is offline   Reply With Quote

Old   August 27, 2020, 02:45
Default
  #5
New Member
 
Malay
Join Date: Aug 2020
Posts: 3
Rep Power: 5
malay1995 is on a distinguished road
Yes I am aware of this situation
May I know which boundary conditions are best in my case.
I want to simulate the following case:
Inlet:
Known Parameters,
Mass Flow Rate 0.1Kg/s
Pressure 3,00,000 Pascals

Outlet:
Known Parameters,
Mass Flow Rate 0.1Kg/s
Parameters to be found by ANSYS ,
Velocity
Pressure

Please tell me which boundary conditions should I use on inlet and outlet for the above specific case. I am more than happy to clear answer any questions about the case.

Thanks & Regards
malay1995 is offline   Reply With Quote

Old   August 27, 2020, 03:01
Default
  #6
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
I've already mentioned them in my previous post. Mass flow rate at inlet and zero static pressure at outlet. When you make a report you should mention somewhere "300 000 Pa must be added to pressure value". You can set Operating pressure to 300 000 Pa but this will not affect incompressible flow.

Or you may set Total pressure at inlet to 300 000 Pa at inlet and mass flow at outlet (or use velocity outlet and recalculate velocity that correspond to mass flow rate of 0.1 kg/s).

Second variant is less numerically accurate and you may also need to enable double precision.
karachun is offline   Reply With Quote

Reply

Tags
boundary condition, flunet, water flow

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
Question about adaptive timestepping Guille1811 CFX 25 November 12, 2017 17:38
Boundary condition of velocity and pressure at interface for air water pipe flow jignesh_thaker2007 OpenFOAM Running, Solving & CFD 7 June 19, 2014 10:12
Boundary condition of velocity and pressure at interface for air water pipe flow jignesh_thaker2007 OpenFOAM Running, Solving & CFD 0 June 10, 2014 16:42
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05


All times are GMT -4. The time now is 16:28.