CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   STAR-CCM+ (https://www.cfd-online.com/Forums/star-ccm/)
-   -   Wake length behind a circular cylinder (https://www.cfd-online.com/Forums/star-ccm/124579-wake-length-behind-circular-cylinder.html)

Corleone84 October 8, 2013 13:04
Wake length behind a circular cylinder
 
1 Attachment(s)
Hello guys.
I'd like to calculate the Wake length behind a circular cylinder for Reynolds number 40 (2D Geometry,laminar, steady) in Star ccm +. My Drag coefficient is 1.1864 . How can i calculate the Wake length in Star ccm? I know,the Length of the Wake is, Lw is defined as the streamwise distance between the confluence point (wake stagnation point) and the rear stagnation point of the cylinder.
Thanks!

triple_r October 8, 2013 15:41
Won't plotting u_x on the center-line behind the cylinder and looking for a sign change work?

bestniaz December 29, 2015 05:02
Quote:
Originally Posted by triple_r (Post 455800)
Won't plotting u_x on the center-line behind the cylinder and looking for a sign change work?
I calculated the re circulation length successfully,,, thanks

But how to calculate the other parameters as mention the figure, Sc, Bw etc.. plz

triple_r December 29, 2015 10:37
1 Attachment(s)
The easiest way that I can think of is using: Line Integrated Convolution.

To use this, create a vector scene for velocity, select the vector display and change its display mode from glyph to Line Integrated Convolution.

You should see a very nice plot of a bunch of mini streamlines. You can control the display by changing the options under line integrated convolution if you expand the vector plot. Increase the "number Steps" to get longer streamlines, and have a large (for example 0.7) blending factor so you can actually see the lines. Then you should be able to just see a plot like the one in the first post, and you can use the ruler (distance report) tool to measure distances.

In the attached figure I've used the symmetry to just solve for half of the domain, and the line is not exactly vertical, but in the output window star reports all three components of the distance:

Code:
Distance Report
  Distance = 0.16684 (m)
  Coordinate System : Laboratory
  Node Point p1 : [ 0.71210 0.16622 0.0000 ]
  Node Point p2 : [ 0.72646 0.0000 0.0000 ]
  Components
    d(X) = 0.014365 (m)
    d(Y) = -0.16622 (m)
    d(Z) = 0.0000 (m)
so the distance s, for example, is going to be 2 x 0.166 = 0.332.

I hope this helps.

bestniaz December 29, 2015 23:21
Quote:
Originally Posted by triple_r (Post 578955)
The easiest way that I can think of is using: Line Integrated Convolution.

To use this, create a vector scene for velocity, select the vector display and change its display mode from glyph to Line Integrated Convolution.

You should see a very nice plot of a bunch of mini streamlines. You can control the display by changing the options under line integrated convolution if you expand the vector plot. Increase the "number Steps" to get longer streamlines, and have a large (for example 0.7) blending factor so you can actually see the lines. Then you should be able to just see a plot like the one in the first post, and you can use the ruler (distance report) tool to measure distances.

In the attached figure I've used the symmetry to just solve for half of the domain, and the line is not exactly vertical, but in the output window star reports all three components of the distance:

Code:
Distance Report
  Distance = 0.16684 (m)
  Coordinate System : Laboratory
  Node Point p1 : [ 0.71210 0.16622 0.0000 ]
  Node Point p2 : [ 0.72646 0.0000 0.0000 ]
  Components
    d(X) = 0.014365 (m)
    d(Y) = -0.16622 (m)
    d(Z) = 0.0000 (m)
so the distance s, for example, is going to be 2 x 0.166 = 0.332.

I hope this helps.
Thanks dear for your response...
But I am using the Fluent and in fluent I could not find anything related to "glyph to Line Integrated Convolution."....

triple_r December 30, 2015 10:15
Sorry, saw this in StarCCM+ forum, so thought you are using that. I don't have access to FLUENT, so can't help a lot, but FLUENT should have a tool to generate streamlines. Usually they ask for a starting point/line/plane for the streamlines. instead of using the inlet for the starting seed, create a line/plane that cuts through the recirculation zone and you should get what you wanted. You'll need to change the number of seed points to get the edge of the recirculation zone though.

Another way is to plot the normal-to-plane component of vorticity and try to find the zeroeth contour (for edge) and maximum (for the "eye"), but because of walls, I don't know if you are going to get a detailed enough picture from this.

Good luck.

bestniaz December 31, 2015 01:10
Quote:
Originally Posted by triple_r (Post 579075)
Sorry, saw this in StarCCM+ forum, so thought you are using that. I don't have access to FLUENT, so can't help a lot, but FLUENT should have a tool to generate streamlines. Usually they ask for a starting point/line/plane for the streamlines. instead of using the inlet for the starting seed, create a line/plane that cuts through the recirculation zone and you should get what you wanted. You'll need to change the number of seed points to get the edge of the recirculation zone though.

Another way is to plot the normal-to-plane component of vorticity and try to find the zeroeth contour (for edge) and maximum (for the "eye"), but because of walls, I don't know if you are going to get a detailed enough picture from this.

Good luck.
Thank you so much,,,,
I did it successfully... Once again thanks.
Best Regards
Niaz


All times are GMT -4. The time now is 04:21.