# post processing dam break problem

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

 February 16, 2008, 22:55 post processing dam break problem #1 chris wetton Guest   Posts: n/a Hi, im currently working on a problem of solving the dam break problem using the VOF method on CFX. I have managed to generate the models however when post processing my models apear as blocks instead of smooth surfaces. At first I thought this was due to the way i defined the simulations however if i put a plane through the middle at any point in the model the flows are smooth. Any ideas any one. thanks again Chris

 February 17, 2008, 06:12 Re: post processing dam break problem #2 Glenn Horrocks Guest   Posts: n/a Hi, How are you displaying the surface? Usually you use an isosurface set at a volume fraction of 0.5 Glenn Horrocks

 February 17, 2008, 06:23 Re: post processing dam break problem #3 chris wetton Guest   Posts: n/a Hi Glen, yeah I am using an isovolume with a volume fraction of 0.5 but still cant think why the simulation is blocky. Do you think it could be a problem with my settings when creating the model? regards Chris

 February 17, 2008, 11:46 Re: post processing dam break problem #4 andy20 Guest   Posts: n/a Use an *isosurface* not an isovolume. Here's the difference: - The edge of an isovolume is defined by the mesh cell boundaries and is therefore rough even for smooth data. Roughly speaking, a single value is associated with each cell, and so each cell is either completely in or completely out of the isovolume. This makes it look rough. - The surface of an isosurface is defined by interpolating the results from the mesh and solving to find a smooth surface at the required value. This results in a smooth boundary. Try, for example, doing both an isovolume and an isosurface for something like the X or Y coordinates in CFXPost, which of course should be smooth, and you'll se the effect[*] Hope that helps. andy. [*] Unless of course you have a structured mesh where all the cells are aligned to share X or Y coordinate boundaries! In that case try another variable. ;-)

 February 17, 2008, 13:35 Re: post processing dam break problem #5 chris wetton Guest   Posts: n/a Andy, thanks for that. Just a quick question though, Will the isosurface be a 2D surface and not 3D? cheers Chris

 February 17, 2008, 17:17 Re: post processing dam break problem #6 Glenn Horrocks Guest   Posts: n/a Hi, An isosurface, in general is a surface with curvature in 3 dimensions. If you have done a 2D simulation it will have curvature in 2 dimensions and be flat in the 3rd dimension. If you have done a 2D simulation and you want contour lines (the 2D version of isosurfaces), first generate a plane or use a symmetry plane to generate a contour object. Glenn Horrocks

 February 18, 2008, 04:58 Re: post processing dam break problem #7 andy20 Guest   Posts: n/a Chris - Yes it will be the 2D surface that encloses the volume described by the condition that defines it...so it will be 'hollow' - but for visualising a free surface after a dam break I think it's what you want. I think the best thing is for you to just try it and see, rather than me explaining in great detail - it's only a 2 minute job to try it out!! I don't know of any way of getting a smooth isovolume in CFX-Post. I honestly think there isn't one, but if I'm wrong I hope someone more knowledgable will post the details for both of us... Regards, Andy

 February 22, 2008, 07:33 Re: post processing dam break problem #8 Chris Wetton Guest   Posts: n/a Andy/Glen thank you so much for your help. The isosurface looks great and when combined with an isovolume I have managed to get a complete model of the Dam Break Problem. Will owe both of you a pint. Chris

 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 sega OpenFOAM Paraview & paraFoam 4 July 14, 2009 08:41 Charles FLUENT 2 June 2, 2008 03:12 sega OpenFOAM Running, Solving & CFD 3 April 20, 2008 10:03 Abhijit Tilak Main CFD Forum 0 April 26, 2004 11:59 Mehdi BEN ELHADJ Main CFD Forum 4 August 24, 2000 07:39

All times are GMT -4. The time now is 17:41.