CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > SU2

Cp plot in Paraview with SU2 output

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By DLuo
  • 1 Post By asonda

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 13, 2015, 03:31
Default Cp plot in Paraview with SU2 output
  #1
New Member
 
Yan Bochao
Join Date: Aug 2014
Posts: 14
Rep Power: 8
wruudf is on a distinguished road
Hi:
I am trying to plot a coefficient pressure along the airfoil of NACA0012 with SU2 output. In order to do this in Paraview (according to the answers I found in this forum), I need to get the value name of the airfoil and use it in the calculator.
Is there anyone who knows how to figure out where is the value name or any other method that can makes me plot the pressure along the airfoil.
Thanks
wruudf is offline   Reply With Quote

Old   April 14, 2015, 18:36
Default
  #2
hlk
Senior Member
 
Heather Kline
Join Date: Jun 2013
Posts: 309
Rep Power: 10
hlk is on a distinguished road
Quote:
Originally Posted by wruudf View Post
Hi:
I am trying to plot a coefficient pressure along the airfoil of NACA0012 with SU2 output. In order to do this in Paraview (according to the answers I found in this forum), I need to get the value name of the airfoil and use it in the calculator.
Is there anyone who knows how to figure out where is the value name or any other method that can makes me plot the pressure along the airfoil.
Thanks
If you change the output file format to TECPLOT and run SU2_SOL yourconfigfile.cfg, an ascii-format file with the variable names will be output (surface_flow.dat). While this format probably wont be readable by paraview, the variable order will be the same as surface_flow.vtk, so you will be able to find out which variable is the pressure coefficient by reading the first line of this file.

Which specific variables are output varies depending on the solution type.
hlk is offline   Reply With Quote

Old   April 15, 2015, 06:10
Default
  #3
New Member
 
Yan Bochao
Join Date: Aug 2014
Posts: 14
Rep Power: 8
wruudf is on a distinguished road
Quote:
Originally Posted by hlk View Post
If you change the output file format to TECPLOT and run SU2_SOL yourconfigfile.cfg, an ascii-format file with the variable names will be output (surface_flow.dat). While this format probably wont be readable by paraview, the variable order will be the same as surface_flow.vtk, so you will be able to find out which variable is the pressure coefficient by reading the first line of this file.

Which specific variables are output varies depending on the solution type.
Thanks for your reply. I think I didn't make myself clear. The variable I need is the coords of the airfoil. The cp however can be directly read in Paraview.
wruudf is offline   Reply With Quote

Old   April 15, 2015, 15:20
Default
  #4
hlk
Senior Member
 
Heather Kline
Join Date: Jun 2013
Posts: 309
Rep Power: 10
hlk is on a distinguished road
Quote:
Originally Posted by wruudf View Post
Thanks for your reply. I think I didn't make myself clear. The variable I need is the coords of the airfoil. The cp however can be directly read in Paraview.
Are you not able to use the surface_flow output? If you set the desired surface as MARKER_MONITORING in your config file you should have an output file with these values.
hlk is offline   Reply With Quote

Old   April 16, 2015, 10:30
Default
  #5
New Member
 
Yan Bochao
Join Date: Aug 2014
Posts: 14
Rep Power: 8
wruudf is on a distinguished road
Quote:
Originally Posted by hlk View Post
Are you not able to use the surface_flow output? If you set the desired surface as MARKER_MONITORING in your config file you should have an output file with these values.
I can use gedit to open the surface_flow.dat or csv. But there are too many nodes and I don't know how to get the data I need.
I found an answer in Google which said to get the data where u,v,w are equal to 0, but I can find it in the file.
wruudf is offline   Reply With Quote

Old   April 16, 2015, 14:49
Default
  #6
hlk
Senior Member
 
Heather Kline
Join Date: Jun 2013
Posts: 309
Rep Power: 10
hlk is on a distinguished road
Quote:
Originally Posted by wruudf View Post
I can use gedit to open the surface_flow.dat or csv. But there are too many nodes and I don't know how to get the data I need.
I found an answer in Google which said to get the data where u,v,w are equal to 0, but I can find it in the file.
The surface_flow output is the data ONLY on the marker specified as MARKER_MONITORING, so it should already be the data you need. The flow.dat file contains the information for the whole domain. You may find the tutorials and other information at https://github.com/su2code/SU2/wiki useful.

Update: MARKER_PLOTTING is the option to use; marker_monitoring sets the marker on which to calculate integrated values (often these are the same).

Last edited by hlk; April 16, 2015 at 16:15.
hlk is offline   Reply With Quote

Old   May 8, 2015, 16:47
Default
  #7
Member
 
Payam D.
Join Date: Aug 2011
Posts: 87
Blog Entries: 3
Rep Power: 11
pdp.aero is on a distinguished road
Quote:
Originally Posted by wruudf View Post
Hi:
I am trying to plot a coefficient pressure along the airfoil of NACA0012 with SU2 output. In order to do this in Paraview (according to the answers I found in this forum), I need to get the value name of the airfoil and use it in the calculator.
Is there anyone who knows how to figure out where is the value name or any other method that can makes me plot the pressure along the airfoil.
Thanks
Just to follow up to this thread, if you wish to plot Cp distribution over airfoil in your 2D simulation follow these:

1- set Paraview as the post-processor in your config file instead of Tecplot.

2- Open the Paraview, click on open file, select the surface_flow.vtk that contain solution over surface, and press Apply.

3- While in the pipeline, surface_flow.vtk is selected, go to the Filters top menu, Alphabetical, and select Scatter Plot as the filter.

4- In the Properties, set the Attribute Mode to Point Data, and under the X Axis Data toggle the Use Data Array on Point(0).

5- Under in the Line Series, deselect all the variables, then check the Pressure Coefficient.

Good Luck,
PDP
pdp.aero is offline   Reply With Quote

Old   May 22, 2015, 18:34
Default
  #8
Member
 
D L
Join Date: Jun 2012
Posts: 44
Rep Power: 10
DLuo is on a distinguished road
For a 3D wing,
1. Generate slice in the orientation desired
2. TriangleStrips
3. CleantoGrid
4. ExtractSurface
5. ScatterPlot

Then you can follow steps 4 and 5 that pdp.aero wrote
R.Mah likes this.
DLuo is offline   Reply With Quote

Old   June 2, 2016, 10:36
Default
  #9
New Member
 
Join Date: Jun 2012
Posts: 19
Rep Power: 10
asonda is on a distinguished road
Quote:
Originally Posted by pdp.aero View Post
Just to follow up to this thread, if you wish to plot Cp distribution over airfoil in your 2D simulation follow these:

1- set Paraview as the post-processor in your config file instead of Tecplot.

2- Open the Paraview, click on open file, select the surface_flow.vtk that contain solution over surface, and press Apply.

3- While in the pipeline, surface_flow.vtk is selected, go to the Filters top menu, Alphabetical, and select Scatter Plot as the filter.

4- In the Properties, set the Attribute Mode to Point Data, and under the X Axis Data toggle the Use Data Array on Point(0).

5- Under in the Line Series, deselect all the variables, then check the Pressure Coefficient.

Good Luck,
PDP
Hi,

I just ran the Euler Naca0012 testcase on SU2-4.1.2 (Ubuntu), and tried to repeat the steps above on ParaView 4.4.0 64bit.
Unfortunately when I reach step 4, there seems to be no option to get the x-coordinates (i.e. Point(0)) for the x-axis.
The list of possible variables for the x-axis are the residuals and flow properties: P, cp, Mach, T.
This applies to both the "scatter plot" and "plot data" filters.
What am I doing wrong?
Many thanks in advance for any help.

Alberto
EddySouth likes this.
asonda is offline   Reply With Quote

Old   November 5, 2018, 10:32
Default
  #10
New Member
 
Xiaolu Wang
Join Date: Apr 2018
Location: Southampton, UK
Posts: 5
Rep Power: 4
EddySouth is on a distinguished road
Quote:
Originally Posted by asonda View Post
Hi,

I just ran the Euler Naca0012 testcase on SU2-4.1.2 (Ubuntu), and tried to repeat the steps above on ParaView 4.4.0 64bit.
Unfortunately when I reach step 4, there seems to be no option to get the x-coordinates (i.e. Point(0)) for the x-axis.
The list of possible variables for the x-axis are the residuals and flow properties: P, cp, Mach, T.
This applies to both the "scatter plot" and "plot data" filters.
What am I doing wrong?
Many thanks in advance for any help.

Alberto
hello Alberto, I had the same problem with you: can't see the x-coordinates in paraview. However, if you saved the data as csv file, and open with excel, you will find the x-coordinates along with y- and z-. Hope will helpful for you(maybe too late) and other users.
EddySouth is offline   Reply With Quote

Old   November 6, 2018, 04:57
Default
  #11
New Member
 
Nathan Ricks
Join Date: Aug 2015
Posts: 10
Rep Power: 7
nathanricks is on a distinguished road
Quote:
Originally Posted by EddySouth View Post
hello Alberto, I had the same problem with you: can't see the x-coordinates in paraview. However, if you saved the data as csv file, and open with excel, you will find the x-coordinates along with y- and z-. Hope will helpful for you(maybe too late) and other users.
I had this same problem at one stage, if you update your version of paraview the x-coordinate should be findable in the logical location. i.e. I'm using paraview 5.4.0 and it is available, but I remember it wasn't in version 4.something
nathanricks is offline   Reply With Quote

Old   November 6, 2018, 05:47
Default
  #12
New Member
 
Xiaolu Wang
Join Date: Apr 2018
Location: Southampton, UK
Posts: 5
Rep Power: 4
EddySouth is on a distinguished road
Quote:
Originally Posted by nathanricks View Post
I had this same problem at one stage, if you update your version of paraview the x-coordinate should be findable in the logical location. i.e. I'm using paraview 5.4.0 and it is available, but I remember it wasn't in version 4.something
Hello Nathan.

Today I am trying the 5.5.2 version of paraview, yes, the x-coordinate can be seen now exactly. Previously, I used 4.4.0 version, I guess maybe the paraview learned that the 4 versions missed some functions, and recovered them in 5 versions.
Thank you for discussion.

Xiaolu
EddySouth is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM] Paraview plot time average tonyuprm ParaView 3 September 11, 2019 02:44
Plot output parameterís oscillation Pierre1 CFX 1 March 23, 2015 09:25
SU2 2.0.8 cannot output correct Paraview file momo_sjx SU2 2 December 3, 2013 16:25
paraFoam reader for OpenFOAM 1.6 smart OpenFOAM Installation 13 November 16, 2009 21:41
[OpenFOAM] Paraview Cp Plot prapanj ParaView 0 June 11, 2009 05:32


All times are GMT -4. The time now is 06:09.