[Paraview] [EXTERNAL] Re: Make animation from steady state result

Fri Feb 2 10:21:43 EST 2018

On Fri, Feb 2, 2018 at 4:44 AM, Andrew Parker
<andy.john.parker at googlemail.com> wrote:
> Cory,
>
> As a follow up.  Can I ask if it would be possible to do all that is
> suggested on Scott's page:
> https://www.paraview.org/Wiki/Advanced_Tips_and_Tricks#Animating_a_static_vector_field
>
> Along with all of your additional steps below from your last post (be great
> to add these to Scott's page), entirely in pvpython or pvbatch?  I make use
> of the anaconda version from here: https://anaconda.org/conda-forge/paraview
>
> Would it be possible do you think to script all of this? I have not tired it
> yet I should add just checking for show stoppers before I begin.

I don't foresee any showstoppers. To make scripting easier, use the
Python tracing capability within the ParaView GUI. Tools menu -> Start
Trace, then perform the suggested actions. When done, choose Tools ->
Stop Trace, and you will see a dialog with the generated script that
you can use as a starting point.

Thanks,
Cory

> Thanks,
> Andy
>
> On 19 January 2018 at 13:18, Cory Quammen <cory.quammen at kitware.com> wrote:
>>
>> Andrew,
>>
>> Responses inlined below:
>>
>> On Fri, Jan 19, 2018 at 6:27 AM, Andrew Parker via ParaView
>> <paraview at paraview.org> wrote:
>> > Dear all,
>> >
>> > Sorry to post onto an old thread. I have been reading this thread and
>> > the
>> > related write up here:
>> >
>> > https://www.paraview.org/Wiki/Advanced_Tips_and_Tricks#Animating_a_static_vector_field
>> >
>> > This thread (and the tips and tricks post) is really close to what I
>> > want to
>> > do, but I have a few follow-up questions.  I too have a steady-state
>> > solution field. I want to trace particles from the inlet of my domain to
>> > the
>> > exit, following the steady-state velocity field, and report for each
>> > particle the temperature-time history (or any other scalar from my
>> > simulation) that the particle sees.  In additional and crucially, the
>> > time
>> > the particle has within the domain: a residence time.  The residence
>> > time
>> > would be the maximum value or IntegrationTime each particle attains
>> > before
>> > it leaves the domain.
>> >
>> > I see that if I follow the notes I can plot (using Glyphs) the
>> > temperature
>> > as it varies across my domain as the particles are animated down the
>> > streamlines: this is working.  What I do not seem to be able to find
>> > however, is the IntegrationTime.  It appears as point-field data after
>> > the
>> > streamlines are created, but vanishes after the contour filter is
>> > applied.
>> > I guess the contour filter is computing a singular value for all values
>> > of
>> > the IntegrationTime from T=0 to T=N with a specific level of
>> > granularity.
>>
>> By default, the Contour filter does not copy the scalar field used to
>> determine the contour surface since it will always be the same value.
>> You can tell it to copy the scalar field by enabling the Compute
>> Scalars option.
>>
>> > However, I can't seem to extract the specific value of IntegrationTime
>> > (the
>> > contour value) when I stop the simulation at any given point.  Do you
>> > know
>> > how to do that?  The "time" scale in the VCR window always goes from
>> > 0->1
>> > not from 0->(max value of IntegrationTime in seconds).  Can the actual
>> > value
>> > of time be backed out or animated? If so how do I do that, or am I
>> > applying
>> > the Contour filter wrongly: as per the post, I am only using the default
>> > values in the Counter filter panel.
>>
>> Instead of using the Sequence animation mode, use Real Time. Then, set
>> the Start Time to the minimum IntegrationTime value and End Time to
>> the maximum IntegrationTime value. You can see these listed either in
>> the Information tab of the StreamTracer filter in the Pipeline Browser
>> or under the Contour filter's Property tab under the Isosurfaces
>> section (Value Range). To show the current time in the render view,
>> use an Annotate Time source, available in the Sources menu.
>>
>> > Finally, and importantly for me, while the Glyphs move across the screen
>> > following the streamlines, and render via the temperature field, how to
>> > I
>> > actually extract information from this pseudo time series to perform
>> > analysis?  For example, the min and max temperature seen by a particle
>> > as it
>> > moved across the streamline for instance?  I'm actually hoping to plot
>> > offline (as a function of IntegrationTime) the min and max temperature
>> > obtained for each particle: I can then take the min and max of that set
>> > for
>> > the quickest and slowest particles.
>>
>> You can run the Connectivity filter on the StreamTracer output to
>> assign a unique value to each streamline. This unique value will be
>> called RegionId. It starts at 0 and ends at the number of stream lines
>> minus 1. Selecting each stream line can be done with the Threshold
>> filter in ParaView using the RegionId as the threshold array, then you
>> can see the min/max of your temperature and IntegrationTime variables
>> in the Information tab. Iterating over all stream lines and saving the
>> min/max of the different scalar fields is possible using ParaView's
>> Python scripting capabilities. However, you may find it faster to
>> export the data to a tool with which you are more familiar.
>>
>> To do that, I would suggest saving the Connectivity filter output to a
>> .csv file. The CSV file will contain all the scalar fields in
>> different columns, including the aforementioned RegionId field. Simply
>> filter on the RegionId field using your favorite software/plotting
>> tool to find the min and max temperature and max IntegrationTime of
>> the particle along the stream line.
>>
>> HTH,
>> Cory
>>
>>
>> > Using the latest stock version of paraview.
>> >
>> > Cheers,
>> > Andy
>> >
>> > On 6 June 2014 at 20:30, Scott, W Alan <wascott at sandia.gov> wrote:
>> >>
>> >> Ken and Jean, excellent idea!  I liked it so much that I wrote it up in
>> >> the SNL ParaView tutorials, tips and tricks page.  It is located here:
>> >> http://www.paraview.org/Wiki/Advanced_Tips_and_Tricks
>> >>
>> >>
>> >>
>> >> Alan
>> >>
>> >>
>> >>
>> >> From: ParaView [mailto:paraview-bounces at paraview.org] On Behalf Of
>> >> Moreland, Kenneth
>> >> Sent: Friday, June 06, 2014 11:43 AM
>> >> To: David E DeMarle; minh hien
>> >> Cc: paraview at paraview.org
>> >>
>> >>
>> >> Subject: [EXTERNAL] Re: [Paraview] Make animation from steady state
>> >> result
>> >>
>> >>
>> >>
>> >> Here's a more expanded list of steps outlining the solution David gave
>> >> in
>> >> case you are not very familiar with the contour filter and animation
>> >> controls in ParaView.
>> >>
>> >>
>> >>
>> >> 1. Create the streamlines as you normally would.
>> >>
>> >>
>> >>
>> >> 2. Add a Contour filter to the streamline (third toolbar, second button
>> >> from the left).
>> >>
>> >> 2.a. Change the Contour By property to IntegrationTime.
>> >>
>> >> 2.b. Press Apply.
>> >>
>> >> This little trick will create a point on each streamline at a
>> >> particular
>> >> time in the particle advection simulation that created the streamlines.
>> >>
>> >>
>> >>
>> >> 3. Open the Animation View (View -> Animation View)
>> >>
>> >> 3.a. On the bottom row, select the contour filter in the first chooser
>> >> box
>> >> and Isosurfaces in the second chooser box. Then hit the blue plus
>> >> button at
>> >> the left.
>> >>
>> >> 3.b. Make sure Mode is set to Sequence and change No. Frames to 100.
>> >>
>> >> 3.c. Hit the play button in the VCR controls (green triangle in the top
>> >> toolbar). You will see the dots animate over the streamlines.
>> >>
>> >> 3.d. You can adjust the speed of the animation by changing the No.
>> >> Frames.
>> >>
>> >>
>> >>
>> >> 4. If you want to see glyphs instead of dots, just add the glyph filter
>> >> to
>> >> the output of the contour filter.
>> >>
>> >>
>> >>
>> >> BTW, props to Jean Favre for originally posting this solution to the
>> >> ParaView mailing list (http://markmail.org/message/ms57z7jjubh2pzjg).
>> >>
>> >>
>> >>
>> >> -Ken
>> >>
>> >>
>> >>
>> >> From: David E DeMarle <dave.demarle at kitware.com>
>> >> Date: Thursday, June 5, 2014 8:07 AM
>> >> To: minh hien <minh.cfd at gmail.com>
>> >> Cc: "paraview at paraview.org" <paraview at paraview.org>
>> >> Subject: [EXTERNAL] Re: [Paraview] Make animation from steady state
>> >> result
>> >>
>> >>
>> >>
>> >> Make an isocontour of the streamlines' integrationTime variable.
>> >>
>> >> Then in animation view, make a track for the isocontour value.
>> >>
>> >>
>> >> David E DeMarle
>> >> Kitware, Inc.
>> >> R&D Engineer
>> >> 21 Corporate Drive
>> >> Clifton Park, NY 12065-8662
>> >> Phone: 518-881-4909
>> >>
>> >>
>> >>
>> >> On Thu, Jun 5, 2014 at 9:52 AM, minh hien <minh.cfd at gmail.com> wrote:
>> >>
>> >> Hi all,
>> >>
>> >>
>> >>
>> >> I got steady state solution for my problem. After plotting streamlines
>> >> at
>> >> steady state, I would like to make animation showing moving of spheres
>> >> (resulted from Glyph filter) on the streamlines, the spheres' velocity
>> >> should be defined by the flow velocity. How can I make this?
>> >>
>> >> Any suggestion would be very much appreciated.
>> >>
>> >>
>> >>
>> >> Thank you in advance.
>> >>
>> >>
>> >>
>> >> Minh
>> >>
>> >>
>> >> _______________________________________________
>> >> 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
>> >>
>> >>
>> >>
>> >>
>> >> _______________________________________________
>> >> 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
>> >>
>> >
>> >
>> > _______________________________________________
>> > 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
>> >
>> > Search the list archives at: http://markmail.org/search/?q=ParaView
>> >
>> > Follow this link to subscribe/unsubscribe:
>> > https://paraview.org/mailman/listinfo/paraview
>> >
>>
>>
>>
>> --
>> Cory Quammen
>> Staff R&D Engineer
>> Kitware, Inc.
>
>

-- 
Cory Quammen
Staff R&D Engineer
Kitware, Inc.