Surface path (oilflow) in paraview
 

Any way to have an oilflow in paraview?

Something quite like this:

http://www.cradle-cfd.com/product/po...ilflow_car.jpg

Thanks!

Ciao Lore.

have a look at this link. you should be able to adapt the methodology to your surface.

http://paraview.org/Wiki/ParaView/Custom_Filters

Thank you Vieri;
my only concern is that what you linked is related to a section of the field i.e. a region where the velocity is not zero… In my case the surface of the body has the non slip condition, so velocity=0… Do you think I could manage to have the oilflow anyway? I tried with no luck but maybe I did something wrong…

I eventually find a way thank to the paraview mailing list.

First of all you need to evaluate the velocity gradient at the walls of the surface shear stress by running wallGradU or wallShearStress in openFoam. Then, in paraview:
tools-->manage plugins-->surface LIC-->load selected, choose surface LIC as visualization type, then among the display options of your geometry choose what you evaluated above as the vector.

Hello Lore,

Thanks for your post and explanation. It's very clear for me but somehow the oilflow doesn't show up. Maybe it has to do with the paraview version that I have (v3.12) but upgrading to v13.4 doesn't work for me either.

I guess that you processed your data with foamToVTK -latestTime, opened ParaFoam and loaded the patch.vtk for which you're interested?

Thanks for the answer!

Ralph

I think it should work either with VTK or with the built in reader. Have you selected everything as depicted in the picture I uploaded (as indicated by the yellow arrows)?

Yep. There's only one problem. After opening paraFoam from the case by calling " paraFoam", loading data only for the surface under consideration (for which wallGradU was performed) and loading LIC from the plugins... the LIC option isn't available as visualization type.

So my question is: which patches do you load? Could you maybe send me your case of the cylinder (because my case is currently several GBs...). Thanks! ralph at marinecfd (dot) com

I just tried and I can confirm it works both with VTK and with paraFoam. With the latter sometimes you don't get anything in the vectors drop down menu, that's a bug of paraview, simply select something else in you pipeline tree (even the firs entry, the one called builtin in my picture above) then select your patch back again and you should be able to see it working.

Also, usually I don't use paraFoam directly but I create a .foam file and then open that one in paraview.

I'll send you my case via email to you right away!

Somehow the trick doesn't work on my Linux machine. Also an installation of Paraview on a windows machine doesn't yield the desired effect. There's no error but nothings shows up, even after some support by Lovecraft22. Anyone some clues how to solve this?

I've got Ubuntu 10.04 on the computer where I tried ParaView 3.12 (no special graphics card, 4 processors, 8GB memory), on my windows machine (less capable in every way compared to the Linux machine) I tried version 3.14.

Hi,

As Sail was saying the method explained here works:
http://paraview.org/Wiki/ParaView/Custom_Filters

To make it work, you only need to select wallShearStress or WallGradU for the SurfaceVectors filter instead of U which is null on the surface.

After that you can apply the MaskPoints filter and use the StreamTracerWithCustomSource filter on the SurfaceVectors.

Using this method I obtain more satisfying results than with the LIC method.

Regards,
Thibault

HI Ralph

Did you find the solution? I have the exactly the same question with you!

Thanks!

Best regards,
Ye

Greetings to all!

@Ye: Are you referring to this question?
Can you show which patches you've selected? Or in other words: did you select only the surface patches or did you choose the internal mesh only?

Best regards,
Bruno