CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Post-Processing

wall pressure

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 7, 2012, 12:28
Default wall pressure
  #1
Senior Member
 
Daniel Witte
Join Date: Nov 2011
Posts: 127
Rep Power: 5
danny123 is on a distinguished road
Hello,

I have a relatively simple problem, but I could not figure out an easy solution by googling and the like. I have calculated my CFD using MRFSimpleFoam as solver. Now I need to extract some tangible results from this calculation.
This is a rotating domain, so the shaft torque of the rotor is one value that can be easily measured. There is a function called wallShearStress plotting the shear stress on any patch, e.g. the interface to the rotor. The wall shear stress is the force acting in parallel to the surface on which it applies (according to what I recall from hydrodynamic books). There is an orthogonal force on that surface, which is the pressure. Even though this pressure is supposely small in my case, I would like to quantify it.
Is the pressure force part of the wallShearStress or is there a tool like wallShearStress to retrieve the pressure? Obviously, I could take the pressure in the cell close to that wall, but this requires a lot of data shuffling. A simple tool applying to the patches only would be easier.

Regards,
Daniel
danny123 is offline   Reply With Quote

Old   March 7, 2012, 13:50
Default
  #2
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8
sail is on a distinguished road
Hi Daniel.

Usinng the forcelib while performing your calculations will give you forces and moments (so torque as well) referenced to the 3axis.

Forces and moments are outputted as viscous, pressure and total.

I'm not shure if it might comes handy but doing one more iteration could be simpler than trying to integrate your pressure. Iirc there isn't an utility that does that out of the box.
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Old   March 8, 2012, 06:12
Default forcelib.so
  #3
Senior Member
 
Daniel Witte
Join Date: Nov 2011
Posts: 127
Rep Power: 5
danny123 is on a distinguished road
Hi Vieri,

Thanks for the quick reply. What I understand from some posts is that I would need to change the controlDict file and include some lines such as:

forces
{
type forces;
functionObjectLibs ("libforces.so");
Linux
patches (rotor);
rhoInf 1.0; // meaning that you need to multiply result with your assumed density in kg/m3 in order to get N m
CofR (0 0 0.108); //Origin for moment calculations
}

Then I have to re-run the case and get the file containing the torque on the axis. This is correct? I assume that OpenFoam will set the torque level to 0 at (0 0 0) and add up the torque along the rotation axis until position CofR. This is correct too? Where to put this change to the controlDict file, at the end after "runTimeModifiable yes;"? The result will the forces fx, fy, fz, Mx, My, Mz whereas Mz is my shaft drive torque, the others shaft bending torque. This is correct too? Do I need to alter OpenFoam source code and recompile it or is libforces.so part of the 2.0.1 package?

Thanks for your help. Regards,

Daniel
danny123 is offline   Reply With Quote

Old   March 9, 2012, 10:07
Default
  #4
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8
sail is on a distinguished road
Quote:
Originally Posted by danny123 View Post
Hi Vieri,

Thanks for the quick reply. What I understand from some posts is that I would need to change the controlDict file and include some lines such as:

forces
{
type forces;
functionObjectLibs ("libforces.so");
Linux
patches (rotor);
rhoInf 1.0; // meaning that you need to multiply result with your assumed density in kg/m3 in order to get N m
CofR (0 0 0.108); //Origin for moment calculations
}

Then I have to re-run the case and get the file containing the torque on the axis. This is correct? I assume that OpenFoam will set the torque level to 0 at (0 0 0) and add up the torque along the rotation axis until position CofR. This is correct too? Where to put this change to the controlDict file, at the end after "runTimeModifiable yes;"? The result will the forces fx, fy, fz, Mx, My, Mz whereas Mz is my shaft drive torque, the others shaft bending torque. This is correct too? Do I need to alter OpenFoam source code and recompile it or is libforces.so part of the 2.0.1 package?

Thanks for your help. Regards,

Daniel
Hi Daniel

You i think your observations are correct. The forces come up out of the box with your version of OF, you won't need to recompile anything.

Actually, you won't need to rerun the case, just add the lines to the controlDict and run few more iterations, that should suffice.

Also, i'm not shure about the position of the COM and the z axis as the torque, but possibly is due to your geometry. Are you simulationg a vertical axis turbine? If so it is correct.

The moments are calculted integrating the viscous and pressure forces multiplied by the distance from the center.

Good luck.
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Old   May 28, 2013, 15:50
Default
  #5
s.q
New Member
 
Join Date: May 2013
Posts: 22
Rep Power: 4
s.q is on a distinguished road
Quote:
Originally Posted by sail View Post
Hi Daniel

You i think your observations are correct. The forces come up out of the box with your version of OF, you won't need to recompile anything.

Actually, you won't need to rerun the case, just add the lines to the controlDict and run few more iterations, that should suffice.

Also, i'm not shure about the position of the COM and the z axis as the torque, but possibly is due to your geometry. Are you simulationg a vertical axis turbine? If so it is correct.

The moments are calculted integrating the viscous and pressure forces multiplied by the distance from the center.

Good luck.


hi vieri
i had simulated a wind turbine using fluent and now i want to calculate the output power of turbine using torque.

would you plz guide me how calculate the torque using integrals as you mentioned in this forum.
i used the report forces-moments... but its amounts are 10 times bigger than real amounts.
s.q is offline   Reply With Quote

Old   May 30, 2013, 02:43
Default
  #6
Senior Member
 
Daniel Witte
Join Date: Nov 2011
Posts: 127
Rep Power: 5
danny123 is on a distinguished road
Hello s.q.,

This thread is about OpenFOAM software. For Fluent, you should file your request in the Fluent forum.

Regards,

Daniel
danny123 is offline   Reply With Quote

Old   December 3, 2013, 08:45
Default wallpressure
  #7
Member
 
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 3
Tobias Adam is on a distinguished road
I guess Daniel doesn´t need this info any more, but it might be useful for someone else.
The pressure on the wall can be calulated by adding this to the functions of the controldict:

Code:
wallPressure
{
type surfaces;
functionObjectLibs ("libsampling.so");
surfaceFormat raw; // vtk;
outputControl outputTime;
interpolationScheme cellPoint;

fields ( 
p
);
surfaces
(
airfoil_airfoil
{
type patch;
patches ("airfoil.*");
interpolate true;
triangulate false;
}

this post for the visualisation of the pressure may help too: plot cp on airfoils

regards
Tobi
Tobias Adam is offline   Reply With Quote

Reply

Tags
wall pressure force

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Non equilibrium wall function : pressure acquisition problem MafioTia OpenFOAM 1 October 10, 2010 04:45
Wall pressure distribution Karthik FLUENT 0 August 18, 2004 06:53
New topic on same subject - Flow around race car Tudor Miron CFX 15 April 2, 2004 06:18
pressure gradient term in low speed flow Atit Koonsrisuk Main CFD Forum 2 January 10, 2002 11:52


All times are GMT -4. The time now is 05:51.