Hi Everyone,
Thank you very much for building the CFD workbench, it's going to be very useful in many areas. I just begin to use it. I am trying to simulate water flow in a pipe (19mm in diameter) through a strainer (holes at 2.5mm diameter) at the middle like this one. The problem is that I tried different settings, flow rate obtained in Paraview is very large (5m/s) seems not correct or I interpreted the units incorrectly. Pressure residual never drops below 0.1 in all the simulations.
The FreeCAD file is attached. I hope anyone can point out what's wrong on it?
OS: Windows 8.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13541 (Git)
Build type: Release
Branch: releases/FreeCAD-0-17
Hash: 9948ee4f1570df9216862a79705afb367b2c6ffb
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Thank You Very Much,
Eric
Water Flow in a Pipe with Strainer
Moderator: oliveroxtoby
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
-
- Posts: 14
- Joined: Wed Nov 28, 2018 3:57 pm
- Location: Hong Kong / Minneapolis
Water Flow in a Pipe with Strainer
- Attachments
-
- Test v1.0 CFD.FCStd
- (87.2 KiB) Downloaded 89 times
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Water Flow in a Pipe with Strainer
Hi,
welcome to the FreeCAD-forum.
I ran your model with some other mesh-refinement (box-refinement-volume instead of surface)
and a reduced pressure at the inlet. The p-residual still remains above 0,1. In my
opinion the sharp edges at the strainer-holes induces turbulence, the solver cant find a stable solution.
But I am not very familiar with pipe-flows. I will do some additional calculations at the weekend.
BTW1: the pressure of 290 Pa in p-dict is a normalized pressure =p/rho-water. The "real" pressure is
1000 times higher, at 290000 Pa, approx 3 bar. Is that what you mean?
BTW2: the diameter of the pipe is 38 mm, not 19 (?)
Keep on foaming...
Thomas
welcome to the FreeCAD-forum.
I ran your model with some other mesh-refinement (box-refinement-volume instead of surface)
and a reduced pressure at the inlet. The p-residual still remains above 0,1. In my
opinion the sharp edges at the strainer-holes induces turbulence, the solver cant find a stable solution.
But I am not very familiar with pipe-flows. I will do some additional calculations at the weekend.
BTW1: the pressure of 290 Pa in p-dict is a normalized pressure =p/rho-water. The "real" pressure is
1000 times higher, at 290000 Pa, approx 3 bar. Is that what you mean?
BTW2: the diameter of the pipe is 38 mm, not 19 (?)
Keep on foaming...
Thomas
-
- Posts: 14
- Joined: Wed Nov 28, 2018 3:57 pm
- Location: Hong Kong / Minneapolis
Re: Water Flow in a Pipe with Strainer
Thank You Thomas,
I didn't aware that the pressure is normalized. I specified 290 Pa at the inlet as either static or total pressure thinking that it's something like 3cm depth of water. I think I don't understand CFD and the settings very well. How can I simulate 3cm depth of water at the inlet? Should I divide the actual pressure by 1000 as the inlet pressure?
It's my mistake, the diamter of the pipe is 38 mm (1.5 inch), 19 mm is the radius.
Eric
I didn't aware that the pressure is normalized. I specified 290 Pa at the inlet as either static or total pressure thinking that it's something like 3cm depth of water. I think I don't understand CFD and the settings very well. How can I simulate 3cm depth of water at the inlet? Should I divide the actual pressure by 1000 as the inlet pressure?
It's my mistake, the diamter of the pipe is 38 mm (1.5 inch), 19 mm is the radius.
Eric
-
- Posts: 14
- Joined: Wed Nov 28, 2018 3:57 pm
- Location: Hong Kong / Minneapolis
Re: Water Flow in a Pipe with Strainer
Hi,
Thank you Thomas, I found this in a cfd forum. I should read OpenFOAM documents in more detail.
"OpenFOAM uses the rho-normalized pressure p*=p/rho
[p*] = {kg/(m.s**2)} /(kg/m**3) = m**2/s**2 = [0 2 -2 0 0 0 0]
in your BC you just have to divide your real pressure with your density"
I run the simulation again with inlet pressure set to 290 Pa / 1000 kg/m3 and obtained the following result. Although I still not able to get pressure residual down below 0.1. The simulation results are very close to that calculated from formulas.
I will try to fillet the strainer openings' edges and run the simulation again with different settings to see if the residual can drop.
One thing I want to ask, why the model display below in ParaView has some stranger walls inside the pipe? It should only be a simple cylinder with 25 holes at the middle of the pipe.
Simulation Result
Inlet Flow Velocity: 0.17 m/s
Peak Flow Velocity at Strainer Opening: 0.83 m/s
Outlet Opening Velocity: 0.53 m/s
Volume Flow Rate: 0.00019 m3 / s
Calculated from formulas
Outlet velocity when draining a tank or container: v = Cv * (2 g H )^0.5
v = outlet velocity (m/s)
Cv = velocity coefficient (water 0.97)
g = acceleration of gravity (9.81 m/s2)
H = height (m)
v = 0.97 * (2 * 9.81 * 0.03)^0.5 = 0.74 m/s
which is very close to the velocity simulation result at the strainer opening.
Liquid volume flow rate when draining a tank or container: V = N * Cd * A * (2 g H)^0.5
V = volume flow (m3/s)
N = number of apertures
A = area of aperture - flow outlet (m2)
Cd = discharge coefficient = Cc * Cv
Cc = contraction coefficient (sharp edge aperture 0.62, well rounded aperture 0.97)
V = 25 * 0.62 * 0.97 * 0.00001256 * (2 * 9.81 * 0.03)^0.5 = 0.00014 m3 / s
which is very close to the volume flow rate obtained in ParaView from the simulation result.
Note: Correction, the strainner hole diameter is 4 mm each, not 2.5 mm as mentioned in the first post.
Thank you Thomas, I found this in a cfd forum. I should read OpenFOAM documents in more detail.
"OpenFOAM uses the rho-normalized pressure p*=p/rho
[p*] = {kg/(m.s**2)} /(kg/m**3) = m**2/s**2 = [0 2 -2 0 0 0 0]
in your BC you just have to divide your real pressure with your density"
I run the simulation again with inlet pressure set to 290 Pa / 1000 kg/m3 and obtained the following result. Although I still not able to get pressure residual down below 0.1. The simulation results are very close to that calculated from formulas.
I will try to fillet the strainer openings' edges and run the simulation again with different settings to see if the residual can drop.
One thing I want to ask, why the model display below in ParaView has some stranger walls inside the pipe? It should only be a simple cylinder with 25 holes at the middle of the pipe.
Simulation Result
Inlet Flow Velocity: 0.17 m/s
Peak Flow Velocity at Strainer Opening: 0.83 m/s
Outlet Opening Velocity: 0.53 m/s
Volume Flow Rate: 0.00019 m3 / s
Calculated from formulas
Outlet velocity when draining a tank or container: v = Cv * (2 g H )^0.5
v = outlet velocity (m/s)
Cv = velocity coefficient (water 0.97)
g = acceleration of gravity (9.81 m/s2)
H = height (m)
v = 0.97 * (2 * 9.81 * 0.03)^0.5 = 0.74 m/s
which is very close to the velocity simulation result at the strainer opening.
Liquid volume flow rate when draining a tank or container: V = N * Cd * A * (2 g H)^0.5
V = volume flow (m3/s)
N = number of apertures
A = area of aperture - flow outlet (m2)
Cd = discharge coefficient = Cc * Cv
Cc = contraction coefficient (sharp edge aperture 0.62, well rounded aperture 0.97)
V = 25 * 0.62 * 0.97 * 0.00001256 * (2 * 9.81 * 0.03)^0.5 = 0.00014 m3 / s
which is very close to the volume flow rate obtained in ParaView from the simulation result.
Note: Correction, the strainner hole diameter is 4 mm each, not 2.5 mm as mentioned in the first post.
- Attachments
-
- Pipe Flow with Strainer.PNG (285.35 KiB) Viewed 1996 times
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Water Flow in a Pipe with Strainer
Sometimes paraview shows the computing domains after running a multi-cpu simulation.poontitming wrote: ↑Fri Nov 30, 2018 3:14 am One thing I want to ask, why the model display below in ParaView has some stranger walls inside the pipe? It should only be a simple cylinder with 25 holes at the middle of the pipe.
You can export the body as stl-file from FC and load it in paraview as background
(when loading in paraview, the stl is scaled up by a factor of 1000, use "Filter/Transform"
for downscaling).
I ran on 2 cpu and get a good view.
Re: Water Flow in a Pipe with Strainer
I find the "Merge Blocks" filter usually works for combining the processor domains, but it leaves a few lines when I try it with this example.thschrader wrote: ↑Fri Nov 30, 2018 1:14 pmSometimes paraview shows the computing domains after running a multi-cpu simulation.poontitming wrote: ↑Fri Nov 30, 2018 3:14 am One thing I want to ask, why the model display below in ParaView has some stranger walls inside the pipe? It should only be a simple cylinder with 25 holes at the middle of the pipe.
You can export the body as stl-file from FC and load it in paraview as background
(when loading in paraview, the stl is scaled up by a factor of 1000, use "Filter/Transform"
for downscaling).