CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

How to represent a fan on a simulation?

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

Like Tree5Likes
  • 5 Post By igor.leo93

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 5, 2018, 10:36
Default How to represent a fan on a simulation?
  #1
New Member
 
igor.leo93's Avatar
 
Igor Leonardo
Join Date: Jul 2016
Location: Brazil - SP - SJC
Posts: 20
Rep Power: 6
igor.leo93 is on a distinguished road
Hello everyone,
I have some questions concerning representation of a fan on a simulation. Basically:


1- How do I apply the fan curve on a simulation (Boundary conditions)?


I would like to see the flow rate change to a value equivalent to the operating point regarding the system resistance curve and the fan curve.


2- Is it possible to apply a rotating flow at inlet?

I know the RPM curve as a function of either velocity or pressure, I would like to add a tangential velocity vector on the inlet for example.


See my case bellow for more information please:


Basically, I took a random fan and it’s curves from the Internet, then, I modeled a 3D geometry of a tube with an obstruction. In a manner that I could drawn the system resistance curve and the fan curve and see the operating point. So I simulated it with simpleFOAM and the results matched my calculations. Now I would like to add the fan effects on the simulation, and see the flow rate drop as a function of the system resistance until the pressure provided by the fan is equal to the total head loss.


I will show here some information, but the full case is attached with an excel containing all the information.
igor.leo93 is offline   Reply With Quote

Old   February 5, 2018, 10:45
Default Continued
  #2
New Member
 
igor.leo93's Avatar
 
Igor Leonardo
Join Date: Jul 2016
Location: Brazil - SP - SJC
Posts: 20
Rep Power: 6
igor.leo93 is on a distinguished road
For Details, see attached images 1 2 3 and 4.

So, considering this fan, the operating point would be at 0.76 m³/min with a inserted pressure difference of 109 Pa, while the system resistance is 105.25 Pa, so I applied this flow rate on the inlet and the calculations were confirmed, some plots: See attached image 5

Now all I want to do is change the boundary conditions in a way that this fan is represented, and operating point would be obtained via simulation, and insert the “rotation” due to the fan would be nice too if possible.

I hope someone more experienced with fan analysis can give me some tips, I found some information on the forum about how to do this but couldn’t understand it very well, I am only used to do very simple simulations with simpleFoam.

Any help is appreciated.

Thanks.

Igor
Attached Images
File Type: png 1.png (17.2 KB, 178 views)
File Type: png 2.png (16.3 KB, 170 views)
File Type: png 3.png (103.3 KB, 160 views)
File Type: png 4.png (63.5 KB, 154 views)
File Type: jpg 5.jpg (19.9 KB, 128 views)
igor.leo93 is offline   Reply With Quote

Old   February 5, 2018, 14:36
Default Fan curve
  #3
New Member
 
igor.leo93's Avatar
 
Igor Leonardo
Join Date: Jul 2016
Location: Brazil - SP - SJC
Posts: 20
Rep Power: 6
igor.leo93 is on a distinguished road
Ok just an update, i've managed to find out how to insert the fan curve. It's pretty simple actually.

I will post here the changes in case anyone else needs.

The changes are basically to the p and U files.

For U:

Code:
boundaryField
{
    inlet
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           uniform (0 0 0);
    }
    walls
    {
        type            noSlip;
    }
}
and for p:

Code:
boundaryField
{
    inlet
    {
       type            fanPressure;
       file        "./constant/fanCurve";
       outOfBounds     clamp;
       direction       in;              // in | out
       p0              uniform 0;
       value           uniform 0;
    }
    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }
    walls
    {
        type            zeroGradient;
    }
}

Notice how on the inlet it is now associated with a file named "fanCurve". Which means that now we need to create a file inside our constant folder named "fanCurve". The file must look like something like this:


Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       IOobject;
    location    "constant";
    object      fanCurve;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
8
(
(0.00000    124.48)
(0.01267    90.46)
(0.01533    74.69)
(0.01950    63.90)
(0.02300    59.34)
(0.02983    56.43)
(0.03533    47.30)
(0.04550    0.00)
)
It is important to notice:

1- The first line contain the amounts of points to be considered.
2- The first column must be in the units of m³/s and the second one either kinematic pressure or Pa (Depends on the solver you are using, in my case it's kinematic, because i'm using simpleFoam).

This is it, the solution converged to the same results as i had calculated, as can be seen on the attached pictures.
Attached Images
File Type: png 1.png (8.6 KB, 181 views)
File Type: jpg 2.jpg (21.6 KB, 162 views)
File Type: png 3.png (92.5 KB, 195 views)
igor.leo93 is offline   Reply With Quote

Old   October 9, 2020, 09:56
Default
  #4
New Member
 
parth
Join Date: Feb 2020
Posts: 7
Rep Power: 2
parthigcar is on a distinguished road
Hi Igor, thank you for the explaination. I had a doubt, how to incorporate the fan RPM and diameter for similar problem?
parthigcar is offline   Reply With Quote

Reply

Tags
curve, fan, openfoam, rotation, simplefoam

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
How to build current blower fan model in Flotherm eric0722 FloEFD, FloWorks & FloTHERM 2 November 24, 2020 10:20
Fan simulation with inlet and outlet duct chaudhry_hashim STAR-CCM+ 0 June 27, 2014 09:59
fan driven flow, Fan BC validation (getting lost) soonic OpenFOAM Running, Solving & CFD 0 July 7, 2013 20:16
Question) fan simulation & B.C Serazio FLUENT 0 February 7, 2011 14:27
FloEFD Heat Sink Simulation feature, but with no fan? j.gerber FloEFD, FloWorks & FloTHERM 0 September 7, 2009 09:37


All times are GMT -4. The time now is 01:35.