[wruudf]

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

[hlk]

Originally Posted by wruudf

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.

[wruudf]

Originally Posted by hlk

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.

[hlk]

Originally Posted by wruudf

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.

[wruudf]

Originally Posted by hlk

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.

[hlk]

Originally Posted by wruudf

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).

[pdp.aero]

Originally Posted by wruudf

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

[DLuo]

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

[asonda]

Originally Posted by pdp.aero

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]

Originally Posted by asonda

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.

[nathanricks]

Originally Posted by EddySouth

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

[EddySouth]

Originally Posted by nathanricks

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