[Paraview] particle tracking on top of unsteady flow solution

Tue May 20 15:35:43 EDT 2014

OK try this. Apply a Programmable Filter to the csv file. Turn on advanced
properties on that panel and use the following scripts:

Script:

oi = self.GetOutputInformation(0)
ut = oi.Get(vtk.vtkStreamingDemandDrivenPipeline.UPDATE_TIME_STEP())
t = inputs[0].RowData['t']
output.RowData.append(numpy.transpose(inputs[0].RowData['x'][t==ut]), 'x')
output.RowData.append(numpy.transpose(inputs[0].RowData['y'][t==ut]), 'y')
output.RowData.append(numpy.transpose(inputs[0].RowData['z'][t==ut]), 'z')

RequestInformation script:

oi = self.GetOutputInformation(0)

oi.Remove(vtk.vtkStreamingDemandDrivenPipeline().TIME_STEPS())

oi.Append(vtk.vtkStreamingDemandDrivenPipeline().TIME_STEPS(), 0)

oi.Append(vtk.vtkStreamingDemandDrivenPipeline().TIME_STEPS(), 1)

oi.Remove(vtk.vtkStreamingDemandDrivenPipeline().TIME_RANGE())

oi.Append(vtk.vtkStreamingDemandDrivenPipeline().TIME_RANGE(), 0)

oi.Append(vtk.vtkStreamingDemandDrivenPipeline().TIME_RANGE(), 1)

The csv file looks like:

x,y,z,t

0, 0, 0, 0

1, 0, 0, 0

2, 0, 0, 0

1, 0, 0, 1

2, 0, 0, 1

3, 0, 0, 1

If the column names are different, you can adjust the Script code.

After this filter, you can apply Table to Points and Glyph usual way. The
heart of this is the inputs[0].RowData['x'][t==ut] bit. This selects
elements from an array that fit a certain criteria. In this case t == ut
where t is the time column value and ut is the time value requested from
the filter by ParaView's animation engine. If you are running into an
issue, make sure that the values in the csv file match exactly the values
in the simulation file. If there are round off errors, you may have to
implement a more complicated logic in the file to round the ut value to one
that is closest in the table.

Best,

-berk

On Mon, May 19, 2014 at 5:41 AM, Tom-Robin Teschner <
tomrobin.teschner at yahoo.de> wrote:

> Hi Berk,
>
> I think option two would be best as I don't use vtu (at least for my
> animations) + for the sake of animation I can reduce the csv file to
> contain only 1 particle per location so the csv file would be indeed small.
> If you could send me the python file I would be very thankful, could you
> also let me know how to put it into paraview as i have never used the
> python shell before (in paraview).
>
> Thanks,
> Tom
>
>    Berk Geveci <berk.geveci at kitware.com> schrieb am 19:21 Freitag, 16.Mai
> 2014:
>
>
> Since you want to sync the two, you can't live without the time
> information, unless the simulation time values are simply an integer
> sequence of 0, 1, 2, 3 etc. The time value is what ParaView uses to sync
> sources. So unless you have this particular case, we need to do something
> to fix the issue. There are two ways I thought of:
>
> 1. Using a pvd file pointing to vtu files
> 2. Doing Python magic to extract particles from a single csv file
>
> 2 is very doable and fun under two conditions:
> a. the number of particles and the number of time steps are relatively
> small (otherwise the csv file will be too big)
> b. you add the time value as another column.
>
> If these hold, I can send you a script that does this. Otherwise, I can
> send you an example file collection of pvd/vtu files.
>
> -berk
>
>
> On Thu, May 15, 2014 at 5:48 PM, Tom-Robin Teschner <
> tomrobin.teschner at yahoo.de> wrote:
>
> thanks berk,
>
> thanks for the reply. i can live without the time information, but would
> paraview automatically map the csv file to the flow solution that i would
> load before?
> the problem is that i have one cgns file containing all flow solutions so
> i wonder if paraview would know which csv file to use.
> i'll probably give it a try in the next days when i have some time, but
> thanks again for your reply.
>
>  cheers,
> tom
>    Berk Geveci <berk.geveci at kitware.com> schrieb am 15:59 Dienstag,
> 13.Mai 2014:
>  Hi Tom-Robin,
>
> ParaView does not support having a time series of particles within a
> single csv file. You can have a file series of csv files as described here:
>
> http://www.paraview.org/Wiki/ParaView/Users_Guide/Loading_Data
>
> Unfortunately, you will not be able to specify a time value in this case.
> ParaView will pick 0, 1, 2 etc.
>
> To be able to specify time values, you will have to use a  format such as
> pvd or Xdmf. Of course, I just noticed that we have absolutely no
> documentation on the PVD format :-) We'll fix that. Here is some info:
>
> http://www.cacr.caltech.edu/~slombey/asci/vtk/
>
> Xdmf is better documentation.
>
> Both of these formats support ASCII content. Xdmf supports having all of
> the data in one file although if you have thousands of time steps, the file
> may get somewhat bulky.
>
> -berk
>
>
> On Thu, May 8, 2014 at 10:59 AM, Tom-Robin Teschner <
> tomrobin.teschner at yahoo.de> wrote:
>
> Hi,
>
> I am doing particle tracking at the moment and I am visualise my results
> with paraview. I have a 3D Navier Stokes solver from which I get a CGNS
> file with the flow solution (for example velocity and vorticity in x, y and
> z) and I also get csv file where I store position of particles, which i
> track inside my code.
> Now I want to bring them both together, i.e. have an animation of the
> flowfield (let's say of the x velocity) and on top I want to display the
> particles at each timestep (so how they move along the flow). the csv file
> looks something like this (shorten for visualisation):
>
> "X" , "Y" , "Z"
> 0.0068 , 0.52500 , 0.005
> 0.0593 , 0.52510 , 0.005
> 0.1171 , 0.52542 , 0.005
>
> I have loaded the particles into paraview and then used tabletopoints from
> the filters but then I get all the particles displayed, instead of getting
> one particle per timestep. I have tried to use a fourth column for time but
> I was unable to map that to my animation.
>
> Does anyone have an idea how to solve this?
>
> Kind regards,
>  Tom-Robin Teschner
>
> _______________________________________________
> Powered by www.kitware.com
>
> Visit other Kitware open-source projects at
> http://www.kitware.com/opensource/opensource.html
>
> Please keep messages on-topic and check the ParaView Wiki at:
> http://paraview.org/Wiki/ParaView
>
> Follow this link to subscribe/unsubscribe:
> http://www.paraview.org/mailman/listinfo/paraview
>
>
>
>
>
>
>
>
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://www.paraview.org/pipermail/paraview/attachments/20140520/c64860ea/attachment-0001.html>