# Wake length behind a circular cylinder

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

October 8, 2013, 13:04
Wake length behind a circular cylinder
#1
New Member

Elham
Join Date: Jun 2013
Location: Germany
Posts: 8
Rep Power: 5
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!
Attached Images
 The effects of axis ratio on laminar fluid flow around-5.jpg (90.0 KB, 42 views)

 October 8, 2013, 15:41 #2 Senior Member   Reza Join Date: Mar 2009 Location: Appleton, WI Posts: 115 Rep Power: 9 Won't plotting u_x on the center-line behind the cylinder and looking for a sign change work? bestniaz likes this.

December 29, 2015, 06:02
#3
Member

N B Khan
Join Date: Jan 2014
Posts: 36
Rep Power: 4
Quote:
 Originally Posted by triple_r 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

December 29, 2015, 11:37
#4
Senior Member

Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 115
Rep Power: 9
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.
Attached Images
 recirc.jpg (48.2 KB, 14 views)

December 30, 2015, 00:21
#5
Member

N B Khan
Join Date: Jan 2014
Posts: 36
Rep Power: 4
Quote:
 Originally Posted by triple_r 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.
But I am using the Fluent and in fluent I could not find anything related to "glyph to Line Integrated Convolution."....

 December 30, 2015, 11:15 #6 Senior Member   Reza Join Date: Mar 2009 Location: Appleton, WI Posts: 115 Rep Power: 9 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 likes this.

December 31, 2015, 02:10
#7
Member

N B Khan
Join Date: Jan 2014
Posts: 36
Rep Power: 4
Quote:
 Originally Posted by triple_r 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post goodegg Main CFD Forum 12 January 22, 2013 12:47 Heini Main CFD Forum 0 October 13, 2011 06:30 Tarak OpenFOAM Running, Solving & CFD 2 August 31, 2011 11:27 teguhtf FLUENT 0 April 23, 2011 00:14 Chengwang Lei Main CFD Forum 2 April 24, 1999 03:42

All times are GMT -4. The time now is 22:50.