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.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. >
_______________________________________________ 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