CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Paraview & paraFoam (http://www.cfd-online.com/Forums/openfoam-paraview/)
-   -   Temperature and streamlines simultaneously in paraview for wedge-typed mesh (http://www.cfd-online.com/Forums/openfoam-paraview/125344-temperature-streamlines-simultaneously-paraview-wedge-typed-mesh.html)

babakflame October 23, 2013 11:44

Temperature and streamlines simultaneously in paraview for wedge-typed mesh
 
1 Attachment(s)
Greetings All

I want to get a picture from paraview which has both temperature contour and streamlines. After clicking on stream tracer from filter in paraview, I need to specify points for line source; I do not know how to determine these points for a wedge-typed mesh. would some body plz hint me?
My system of coordinates are completely clear from the attachments; If you tell me where the point should be, I would become very happy.

X domain: 0 - 0.15
y domain: 0 - 0.9
z domain: -0.0065429081 - 0.0065429081

Regards
Bobi

babakflame October 23, 2013 12:35

1 Attachment(s)
Greetings all

I found the point source positions: (according to geometry)

(0 0.45 0) to (0.15 0.45 0)
The result is the following image; however I want a continous temp slice on which streamlines are shown in black lines. would somebody plz hint me how can I get it?
Also in Sources->Ruler; when we use this ruler nothing happens in the pic; how can we have a real ruler that shows distance in any location of the pic?


Any hint?

Regards
Bobi

babakflame October 24, 2013 09:35

2 Attachment(s)
Greeting all

I have posted the best pic I got from paraview and the shape that is my desired.

Would anybody PLZ hint me how can I get the desired pic (left one) from paraview?

Kind Regards
Bobi

Tobi October 24, 2013 11:33

Hi Bobi,

you want the left picture visualized in paraview?
Can you sent me the case (last timestep) without PDF on my email account.
Then I will have a look on it.

Regards Tobi

babakflame October 24, 2013 12:19

Hi Tobi

Yes, What I got as the best is the right picture; however I want sth like the left one i.e continous temperature profile with streamlines in black on it.

I sent the requirements via file2send.

Kind Regards
Bobi

Tobi October 24, 2013 13:42

1 Attachment(s)
Hi Bobi,

is this related to that you want?

Regards Tobi

babakflame October 24, 2013 13:58

Hi Tobi

Yes, Exactly sth like this. Would you PLZ hint me how did you do this in paraview?
I can cut a slice through the mesh and get the temperature distribution on it;but how about black streamlines? What I found in paraview is colour lines (from stream tracer) not these black lines that you put on the image. The advantage of black lines is that it makes stream lines distinctive from the background temperature.

Another important question. Is there any way to put vertical and horizontal rulers around our graph (like tecplot) in paraview?

Kind Regards
Bobi

Tobi October 24, 2013 15:48

Hi,
hmmm ... i dont know if this is possible or how to do that.

In the attachment you find a file you can load with paraview.

1. cut your domain with some clips
2. build a slice through your domain
3. add calculator
4. build new vectorfield "Velocity_xy = i_Hat*U_X+j_Hat*U_Y"
5. streamlines with that source on a line
6. move your slice to temperature values
7. move your streamlines to "solid color"
8. change color to black and maybe print your lines thicker
9. build glyph on streamlines with the velocity field
10. change type to "cone"
11. change settings of cone
12. enjoy.

Regards
Tobi

babakflame October 25, 2013 04:51

Hi Tobi

Many thanks for your instructions.
Also I tried to open the file you had put in the forum with paraview. I put it on its original folder. After running paraview from that folder and loading state (this file), I confronted with this error:

Code:

babak@babak-System:~$ cd OpenFOAM/babak-2.2.x/flameletModel-2.2.x/tutorials/flameletSimpleFoam/HM1Tobi2
babak@babak-System:~/OpenFOAM/babak-2.2.x/flameletModel-2.2.x/tutorials/flameletSimpleFoam/HM1Tobi2$ paraFoam
created temporary 'HM1Tobi2.OpenFOAM'
ERROR: In /home/babak/OpenFOAM/ThirdParty-2.2.x/ParaView-3.12.0/VTK/IO/vtkOpenFOAMReader.cxx, line 4348
vtkOpenFOAMReaderPrivate (0x520e020): Can't open directory /home/shorty/OpenFOAM/shorty-2.2.x/run/case/


ERROR: In /home/babak/OpenFOAM/ThirdParty-2.2.x/ParaView-3.12.0/VTK/Filtering/vtkExecutive.cxx, line 756
vtkPVCompositeDataPipeline (0x5208cf0): Algorithm vtkPOpenFOAMReader(0x5204690) returned failure for request: vtkInformation (0x520d690)
  Debug: Off
  Modified Time: 109401
  Reference Count: 1
  Registered Events: (none)
  Request: REQUEST_INFORMATION
  FORWARD_DIRECTION: 0
  ALGORITHM_AFTER_FORWARD: 1




ERROR: In /home/babak/OpenFOAM/ThirdParty-2.2.x/ParaView-3.12.0/ParaViewCore/ServerImplementation/vtkSIProxyDefinitionManager.cxx, line 543
vtkSIProxyDefinitionManager (0x2ba3520): No proxy that matches: group=misc and proxy=ViewLayout were found.


ERROR: In /home/babak/OpenFOAM/ThirdParty-2.2.x/ParaView-3.12.0/ParaViewCore/ServerManager/vtkSMDeserializer.cxx, line 62
vtkSMStateLoader (0x31ec9d0): Could not create a proxy of group: misc type: ViewLayout


Segmentation fault (core dumped)

It seems that the file wants sth from your computer.
Also if the data can be used by others, I would be glad if you delete the file,cause I have downloaded it.

Regards
Bobi

Tobi October 25, 2013 05:25

Hi Bobi,

well it seems that PV Need my Folder:
Code:

Can't open directory /home/shorty/OpenFOAM/shorty-2.2.x/run/case/
Well this file is only a paraview state file that should Show you the steps I wrote befor.

Regards
Tobi

babakflame October 26, 2013 04:54

Hi Tobi

From your instructions I learned new things in paraview:) :D
Many thanks.
Just two short questions:
1- Your streamlines have orientation, but mine didn't get. would you plz allude to the place where we put orientation on our streamlines?
2- what is the role of glyph?
with slice - calculator and stream tracer consecutively, I got sth like your image. The same pic achieved by glyph, though.

Kind Regards
Bobi

Tobi October 26, 2013 05:06

Hi Bobi,

my streamlines have no orientation. On the streamlines I used the filter "glyphs" to get the orientation shown as small triangls :) that s all. In that filter you have to use the befor calculated velocity field (source).
Then you will have 3D glyps with orientation. Then change 3D Glyphs to the settings you want to have. Additionally change the parameters so that your solution is good for you.

Regards Tobi

babakflame October 26, 2013 08:32

1 Attachment(s)
Hi Tobi

I took a look into paraview tutorial too. I got what is going on with Glyph filter.
I tried a lot to got a nice pic, however it seems that glyph settings is not that much simple.:(

I took a snapshot from my paraview that shows my glyph settings.
I would be very glad if you put a snapshot like mine that shows your glyph settings.

I don't know where is the problem because pointers about the bluff body are very big, but in the bluff-body wake they are small.

Regards
Bobi

Tobi October 26, 2013 09:33

Hi,

you are not doing that:

1. cut your domain with some clips

- cut the domain into the interessting domain

2. go down the properties menue and set scaling to "off"
3. set a good scale factor your self
4. decrease the number of glyphs

Have fun,
Regards Tobi

babakflame October 27, 2013 05:46

2 Attachment(s)
Hi Tobi

Many thanks for your helps. Finally I got a nice pic. Although the density of streamlines around the vortices center are high but generally the quality is acceptable.

@ Bruno
Hi buddy

Would PLZ take a look at my pic and the desired one?

I need to put a coordinate system with the origin at the leftmost point in the inner jet exit. (sth like the desired pic). Does paraview support this capability?

Kind Regards
Bobi

wyldckat October 27, 2013 05:53

Greetings to all!

@Bobi: If the results are in 3D, then the only thing I know of is the Cube Axes: http://www.paraview.org/Wiki/ParaVie...tion#Cube_Axes

Best regards,
Bruno

babakflame October 28, 2013 02:14

Hi Bruno

Many thanks for your help. Wedge-typed mesh is kind of 3-D.
I am going to take a look into the link.

Regards
Bobi

babakflame October 28, 2013 09:00

Hi Bruno
Just a simple problem.
Where is this filter i.e. cube axes? I can't find it.

Regards
Bobi

wyldckat October 28, 2013 17:59

Hi Bobi,

http://www.paraview.org/Wiki/ParaVie...tion#Cube_Axes
Quote:

Finally, in the Display section of the Properties tab of any object shown in a 3D view, you can toggle the display of a Cube Axes Display.
Problem is that said "Display" section actually depends on the ParaView version. Either way, more visual information is provided here: http://paraview.org/Wiki/ParaView/Di...a#Annotation_2

Best regards,
Bruno

babakflame October 29, 2013 14:32

Dear Bruno

Many thanks for your kind hints. I am using paraview 3.12 with O.F. 2.2.x.
It seems that I should upgrade my paraview version to 3.14. would you PLZ hint me how can I do this without affecting my O.F. settings?
I mean without leaving O.F. 2.2.x.

Regards
Bobi


All times are GMT -4. The time now is 10:38.