CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Addition of body force as function of position in icoFoam solver.

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

Like Tree3Likes
  • 3 Post By SHUBHAM9595

LinkBack Thread Tools Search this Thread Display Modes
Old   July 14, 2020, 05:23
Default Addition of body force as function of position in icoFoam solver.
New Member
Join Date: Jul 2016
Posts: 8
Rep Power: 10
FluidFox is on a distinguished road
Hi All,

I am new to OpenFOAM, but have experience with CFD.
I am moving over from an axisymmetric 2D code of my own to run 3D simulations in OpenFoam.
I have happily followed a number of tutorials and have now set up my own testcases to run.

What I want to do now is add in a body force.
My test case is a cylindrical cavity, and I want to add a force that will drive rotation of the fluid (e_theta direction in polar coordinates)*.

I have followed a few tutorials and have made a copy of icoFoam as my_icoFoam and successfully run wmake and executed. I have read the source code and it mostly makes sense on a high level, but I am having trouble on where to start to implement a force as a function of position.

Based on other entries I need to modify the code to look something like this:

        fvVectorMatrix UEqn
          + fvm::div(phi, U)
          - bodyforce
          - fvm::laplacian(nu, U)
but I am unsure how to define `bodyforce`.

My main question at the moment is how I write a function/variable in the appropriate form to be included in the equation above. From what I have read I can extract cartesian components from the mesh as mesh.C().component(vector::Y), but I am unsure how to use these. Do I need to define an additional field that represents my body force?

My other main question is about defining vectors. Do I have to implement this in cartesian components for OpenFoam, or is it somehow possible to define the body force vectors in cylindrical polar coordinate system.

I have tried to read documentation and other forum posts before asking this, but since I am new to OF I may have missed something or not understood, so apologies if that is the case. Any help or pointing in the direction of a useful tutorial would be much appreciated.Thanks!

*For reference, the simplest force I am looking to implement is a constant times radial distance (k*r) pointing in the direction perpendicular to r and z (clockwise from above).
FluidFox is offline   Reply With Quote

Old   September 4, 2020, 04:18
Join Date: Aug 2017
Posts: 69
Rep Power: 8
SHUBHAM9595 is on a distinguished road
Hey Jack,

1) As you are solving for a volVectorField (U), you first need to initialize your source term. One of the ways to do it is to define it in createFields.H

Info<< "Reading custom source CS\n" << endl;
volVectorField CS
2) You can define your force term (K*R) in UEqn.H as u already mentioned using the mesh coordinates

volScalarField xx = mesh.C().component(vector::X);
volScalarField yy = mesh.C().component(vector::Y);
volScalarField rr  = sqrt((xx*xx)+(yy*yy));
volScalarField CS1 = K1*rr; // here K1 is const
3) Then u need to assign above volScalarField to the previously initialised volVectorField
CS.replace(vector::X, CS1);
CS.replace(vector::Y, CS1);
CS.replace(vector::Z, CS1);
4) Finally, u have to add CS in ur UEqn.H, now as for the present source term "Kr", its independent of the field variable which we are solving (U), thus u can add it as an EXPLICIT source term. Otherwise u have to add it via "fvm::Sp"
fvVectorMatrix UEqn
          + fvm::div(phi, U)
          - (1/rho)*(CS) 
          - fvm::laplacian(nu, U)
Make sure you use the right dimensions while defining the constant K1, otherwise it'll show u an error while solving.
Divyaprakash, mllokloks and Tibo99 like this.
SHUBHAM9595 is offline   Reply With Quote


body force, coordinates, icofoam problem, source code

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
ActuatorDiskExplicitForce in OF2.1. Help be_inspired OpenFOAM Programming & Development 10 September 14, 2018 11:12
Running UDF with Supercomputer roi247 FLUENT 4 October 15, 2015 13:41
Compilation errors in ThirdPartymallochoard feng_w OpenFOAM Installation 1 January 25, 2009 06:59
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50
Droplet Evaporation Christian Main CFD Forum 2 February 27, 2007 06:27

All times are GMT -4. The time now is 02:28.