[s.m]

Hi
i am simulating the flow over an airfoil, i done my simulation with openFoam, and now i wanna plot the velocity profile over a line that is approximately perpendicular to the surface of airfoil, at trailing edge.

what should i do?
P.S. i use paraview for postprocessing the results.
Thank you very much.

[Artur]

Hi,

In paraview you could use the "plot over line" filter. Optionally, you can use the OF sampling utilities. There's quite a lot of info in this link and the tutorials it mentions:

http://www.openfoam.org/docs/user/sample.php

Cheers,

A

[s.m]

hi dear all
i am simulating the flow on an 3 element airfoil, now i want to plot the velocity profile at the different stations on the airfoil, as like as the pictures in the attachment, could you please give me some suggestion how i can plot this figure?

[s.m]

Dear Foamers, i need a help!
i want to plot the contour of turbulent intensity on my airfoil, somthing like the picture in the attachment, i don't know how can i do it, can any body guide me?
Thaknk you very much.

[s.m]

Originally Posted by Artur

Hi,

In paraview you could use the "plot over line" filter. Optionally, you can use the OF sampling utilities. There's quite a lot of info in this link and the tutorials it mentions:

http://www.openfoam.org/docs/user/sample.php

Cheers,

A

Dear artur how can i set the plot over a line in paraview?
first of all i load the VTK of my file, then i select the plot over line in direction of y axis then i hit apply, i doesn't show my any thing in it's figure,
Sorry, can you guide me more

[Artur]

Hi,

You got it right, not sure what your problem is to be fair. Here's a step-by-step of how I do it:

1. load your case to apraview using paraFoam
2. add the plotOverLine filter, in Display tab of the object inspector mark the thing you want to plot (my example is for pressure)
3. hit apply and a figure should appear on the right hand side showing a plot in the line coordinate system

Your problem might be that either you didn't load the data to paraview but just the mesh or you have nothing selected in the display tab I think.

If you want to plot the axial components of velocity and not just its magnitude you may use the Calculator filter first, select the result to be the U_X scalar and then apply the plot over line to it - without doing this you would only be able to plot the magnitude of U.

Let me know if that helps.

A

P.S. depending on what you want to plot, you might also look at the OpenFOAM probe utilities which allow you to sample over a surface. You can then easily read the data into Python, Matlab or whatever and make nice plots there. If you want to plot the Cp over your foil that's probably the better way to do it.

[wyldckat]

Greetings to all!

@Saeideh: Sorry for taking so long to answer to your questions, but my to-do list here on the forum is getting bigger than the time I have available

I moved a couple of posts you had made on other threads into this one, because they are all related, one way or another. So, in order:

Originally Posted by s.m

i am simulating the flow on an 3 element airfoil, now i want to plot the velocity profile at the different stations on the airfoil, as like as the pictures in the attachment, could you please give me some suggestion how i can plot this figure?

The PDF file you're referring seems to be this one: http://www.iitk.ac.in/reach/2010/ses...10_for_web.pdf
This is a pretty tricky thing to do in ParaView. Let's see:

1. You need to do something similar to what I described in this post: http://www.cfd-online.com/Forums/ope...tml#post468732 post #12
   The difference from that post is that you need the "n/c" which seems to stand for "normal by chord".
2. In the first image attached, is a circle pretending to be an airfoil:
   1. I applied the "Slice" filter to the original case file from OpenFOAM.
   2. Then I applied the filter "Plot Over Line" to it. The position of the 2 points was done with the help of the big "Y axis" button on the lower left corner of the image to set the line aligned, then with the help of the mouse (+ the Shift key) to move the two extremities of the line.
      Note: you might have to manually calculate the positions of these two points, since you need them to be located exactly in the right place.
3. Once the filter "Plot Over Line" is applied, in the second image is shown the settings used on the left, for the plot on the right. I don't have yet the "n/c" entry, but I do have "arc-length", which is the distance between the first line point to the sample point.
4. Apply the "Calculator" filter to the "PlotOverLine1" entry, as shown in the 3rd image, with the calculation:
   

   arc_length/0.5

   And the "Result Name Array" named "n/c".
5. In the 4th image is shown that you now have to apply the filter "Plot Data" to the "Calculator1" entry. And is shown how the filter is configured.
6. For configuring the labels for the plot axis, check this post: http://www.cfd-online.com/Forums/par...tml#post455158 post #2

Note: The use of the "Slice" filter was merely for making it easier to see where the line was placed. You can right-click on the entry "PlotOverLine1" and choose "Change Input..." and choose the ".OpenFOAM" file or VTK file as your input.

Then it's just a matter of doing the same for all other stations.

Originally Posted by s.m

i want to plot the contour of turbulent intensity on my airfoil, somthing like the picture in the attachment, i don't know how can i do it, can any body guide me?

First use the filter "Slice" and then apply the "Contour" filter to the item "Slice1"... Make sure to configure the correct field to be represented in the "Slice1" and the correct field and contour values for "Contour1".


Mmm... I was planning on taking care of another reply here, but it's best to answer where you had asked it, namely here: http://www.cfd-online.com/Forums/ope...tml#post468745 post #15

Best regards,
Bruno