On Fri, Feb 2, 2018 at 4:44 AM, Andrew Parker <andy.john.par...@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.quam...@kitware.com> wrote: >> >> Andrew, >> >> Responses inlined below: >> >> On Fri, Jan 19, 2018 at 6:27 AM, Andrew Parker via ParaView >> <paraview@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 <wasc...@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-boun...@paraview.org] On Behalf Of >> >> Moreland, Kenneth >> >> Sent: Friday, June 06, 2014 11:43 AM >> >> To: David E DeMarle; minh hien >> >> Cc: paraview@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.dema...@kitware.com> >> >> Date: Thursday, June 5, 2014 8:07 AM >> >> To: minh hien <minh....@gmail.com> >> >> Cc: "paraview@paraview.org" <paraview@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....@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. _______________________________________________ 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