# How to represent a fan on a simulation?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 5, 2018, 10:36 How to represent a fan on a simulation? #1 New Member     Igor Leonardo Join Date: Jul 2016 Location: Brazil - SP - SJC Posts: 20 Rep Power: 9 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. denbjornen likes this.

February 5, 2018, 10:45
Continued
#2
New Member

Igor Leonardo
Join Date: Jul 2016
Location: Brazil - SP - SJC
Posts: 20
Rep Power: 9
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
 1.png (17.2 KB, 428 views) 2.png (16.3 KB, 421 views) 3.png (103.3 KB, 414 views) 4.png (63.5 KB, 389 views) 5.jpg (19.9 KB, 300 views)

February 5, 2018, 14:36
Fan curve
#3
New Member

Igor Leonardo
Join Date: Jul 2016
Location: Brazil - SP - SJC
Posts: 20
Rep Power: 9
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
{
}
}```

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
 1.png (8.6 KB, 380 views) 2.jpg (21.6 KB, 346 views) 3.png (92.5 KB, 413 views)

 October 9, 2020, 09:56 #4 New Member   parth Join Date: Feb 2020 Posts: 23 Rep Power: 5 Hi Igor, thank you for the explaination. I had a doubt, how to incorporate the fan RPM and diameter for similar problem? raj kumar saini likes this.

 June 21, 2022, 20:55 fanPressure in openFOAM 8 #5 New Member   Jeferson Souza Join Date: Jan 2012 Location: Brazil Posts: 19 Rep Power: 13 I'm trying to use the fanPressure boundary condition with openFOAM 8 (of8). I solved this problem in of7 without any problem, however when I try to solve the same problem in of8 (or of9) it simply does not work. Both pressure and velocity are set to zero at the inlet boundary. I corrected the boundary condition for the new syntax. I got no errors, however I got no solution either. Does anyone knows what is different in of8? Thanks.

 Tags curve, fan, openfoam, rotation, simplefoam

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post eric0722 FloEFD, FloWorks & FloTHERM 3 January 2, 2021 03:36 chaudhry_hashim STAR-CCM+ 0 June 27, 2014 09:59 soonic OpenFOAM Running, Solving & CFD 0 July 7, 2013 20:16 Serazio FLUENT 0 February 7, 2011 14:27 j.gerber FloEFD, FloWorks & FloTHERM 0 September 7, 2009 09:37

All times are GMT -4. The time now is 18:00.

 Contact Us - CFD Online - Privacy Statement - Top