# how to extract x,y and z direction components of force

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

 December 19, 2012, 08:45 how to extract x,y and z direction components of force #1 New Member   Join Date: Nov 2012 Location: Germany Posts: 7 Rep Power: 7 Hi all, Im currently working on a student research project and i'm computing wave loads on an offshore structure. The simulation is working fine, but i'm stuck at extracting force components. My intention is to extract the force components. Force in X, Y, and Z direction at specific coordinates. For example at the point [1,2,3] i want to extract a force in form of [200N,300N,500N]. I already tried Force report, but this gives me only the accumulated force for the whole structure. My second try was to use a XYZInternalTable, but i only receive the pressure at specific coordinates given by star ccm+ without knowing the reference surface to calculate the force from pressure. Currently i'm stuck at trying user defined field functions. Maybe any suggestions?

 December 19, 2012, 12:02 update #2 New Member   Join Date: Nov 2012 Location: Germany Posts: 7 Rep Power: 7 Well, i found a part solution: Now i'm able to extract components for Forces caused by wall shear stress. For example: Force components [i j k]: [0.0 0.0 0.025] corresponding Position: [x y z] [-29.73 -18.75 -64.5] Im using a XYZInternalTable with the following user defined function as scalar field function: Code: `\$\$Area * \$\$WallShearStress.mag()` Now the next problem occured. I cant use the same code syntax for pressure related forces, because pressure function is of scalar type. My first idea was that i could use the scalar pressure value just as the magnitude of a potential pressure vector. Star reacts with an an error : "Pressure is not a type of array". Now i'm confused how to continue to get the values i'm looking for Last edited by dke; December 19, 2012 at 13:35. Reason: Code corrected

 December 19, 2012, 12:43 #3 New Member   Join Date: Nov 2012 Location: Germany Posts: 7 Rep Power: 7 Yay simple syntax mistake. \$Pressure instead of \$\$Pressure works So field function for Pressure induced Force: Code: `\$\$Area * \$Pressure` Last edited by dke; December 19, 2012 at 13:35. Reason: Code corrected

 December 19, 2012, 15:30 #4 Super Moderator   Ryne Whitehill Join Date: Aug 2009 Posts: 313 Rep Power: 12 Don't bother making field functions, a force report is the right way to do this. In the force report, there is a "direction" component. You can set up 3 reports, one for X, one for Y, one for Z. edit: I misunderstood your problem, my apologies! Ignore the above Last edited by rwryne; December 19, 2012 at 16:02.

 December 19, 2012, 15:51 #5 Senior Member   Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 229 Rep Power: 12 The report doesn't help you for displaying the distribution of the force on a surface within a scalar plot. It just gives you a final number. For a scalar plot of the y-component you have to create a scalar field function like this: Code: `\$Pressure * \$\$Area_Normal[1]` where \$Area_Normal is a vector FV: Code: `\$\$Area/\$\$Area.mag()`

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post be_inspired OpenFOAM Programming & Development 8 July 3, 2014 10:54 renyun0511 OpenFOAM Running, Solving & CFD 2 November 1, 2011 23:09 colopolo CFX 13 October 4, 2011 22:03 renyun0511 OpenFOAM Running, Solving & CFD 0 April 8, 2011 07:15 ScottN FLUENT 0 September 21, 2010 09:18

All times are GMT -4. The time now is 08:36.