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

[Cory Quammen]

On Fri, Feb 2, 2018 at 4:44 AM, Andrew Parker
 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  wrote:
>>
>> Andrew,
>>
>> Responses inlined below:
>>
>> On Fri, Jan 19, 2018 at 6:27 AM, Andrew Parker via ParaView
>>  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 

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

[Andrew Parker via ParaView]

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.
Thanks,
Andy

On 19 January 2018 at 13:18, Cory Quammen  wrote:

> Andrew,
>
> Responses inlined below:
>
> On Fri, Jan 19, 2018 at 6:27 AM, Andrew Parker via ParaView
>  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 

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

[Andrew Parker]

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  wrote:

> Andrew,
>
> Responses inlined below:
>
> On Fri, Jan 19, 2018 at 6:27 AM, Andrew Parker via ParaView
>  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  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:
> >> 

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

[Cory Quammen]

Andrew,

Responses inlined below:

On Fri, Jan 19, 2018 at 6:27 AM, Andrew Parker via ParaView
 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  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 

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

[Andrew Parker via ParaView]

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.
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.

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.

Using the latest stock version of paraview.

Cheers,
Andy

On 6 June 2014 at 20:30, Scott, W Alan  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 
> *Date: *Thursday, June 5, 2014 8:07 AM
> *To: *minh hien 
> *Cc: *"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 Engineer
> 21 Corporate Drive
> Clifton Park, NY 12065-8662
> Phone: 518-881-4909 <(518)%20881-4909>
>
>
>
> On Thu, Jun 5, 2014 at 9:52 AM, minh hien  wrote:
>
> Hi 

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

[Scott, W Alan]

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.commailto:dave.dema...@kitware.com
Date: Thursday, June 5, 2014 8:07 AM
To: minh hien minh@gmail.commailto:minh@gmail.com
Cc: paraview@paraview.orgmailto:paraview@paraview.org 
paraview@paraview.orgmailto: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.
RD 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.commailto: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.comhttp://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