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

Fri Jan 19 08:36:55 EST 2018

Thank you very much for these comments.  I'll give them a go and follow up
if need be.
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.
>
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <https://paraview.org/pipermail/paraview/attachments/20180119/a513e1e3/attachment.html>