[CFD Post]  Surface and 3D streamlines difference
Starting from the same point I've plotted a surface stream line and a 3D stream line and found them different 
These are the steps I followed  3D Stream line Inserted an arbitary point (Say Point P) in the domain and plotted a 3D streamline starting from this point in the forward and backward directions. Surface stream line  Inserted a XY Plane with the Zlocation as the Zcoordinate of Point P. With such plane as the chosen surface and the Point P itself as the location to start from, I plotted a surface streamline in the forward and backward directions. I found that the 3D stream line and the surface stream line thus generated are not the same. Could some one please clarify upon this. 
Of course they are different. Surface streamlines are constrained to stay on the surface, but 3D streamlines can go where ever they want. So surface streamlines are only influenced by the flow adjacent to the surface, but 3D streamlines are influenced by the entire domain.

Unless the simulation is 2D, often the surface streamlines seem to be "cut" or broken. Hence, even if you want to see streamlines on (or near) a particular plane/surface, it makes sense just to create a line in plane/surface towards inlet side and start a 3D streamlines from there. Since they are 3D, they remain complete and not broken when they wander out of plane, at the same time; revealing the physics near the surface of interest  which is the objective.
OJ 
It is intended to be a 2D simulation , however with CFX it is always a 2.5D

Indeed, it is represented as 2.5D given the limitation of software, but since the intention is 2D, the variations in third direction (third perpendicular axis or theta direction for axisymmetry) should be zero. Incidently, the streamlines on surface are likelier to remain on the surface, unlike actual 3D case, where they wander off the plane in third direction. Hence surface streamlines are usable here.
This of course may not be true in case of swirling axisymmetric case. OJ 
Even though the thickness added in CFX for a 2D planar problem is (should be) of a negligible dimension does it not mean that the flow varies with in such negligible thickness.
Therefore I have the confusion in choosing between 3D and surface stream lines for a 2D simulation result (either from CFX or Fluent). For the 3D and surface stream lines look different. Though Fluent solves the 2D problem by a 2D solver, when I load the .cas , .dat files into CFDPost for post processing then a thickness gets automatically represented in CFDPost so I again have this confusion between 3D or surface stream lines to choose from. 
If you have a 2D simulation you should draw surface streamlines on the symmetry surfaces to avoid problems with the small deviations which pull the streamline off the surface.

Hi Glenn. Thanks for your response but doesn't the flow vary with in the negligible thickness that is extruded out to solve a 2d planar problem in cfx.

The symmetry enforces any gradients in normal direction to it as zero, meaning, it doesn't allow any change in velocities perpendicular to the symmetry plane. This happens at both symmetry surfaces which are very close to each other and hence influence the flow between them to ensure the flow remains parallel to them. Hence, there is (ideally) no deviation in the direction perpendicular to symmetry.
If you observe change it may as well be a numerical artifact and a result of a bad mesh, extreme boundary conditions or number of factors, but it shouldn't be any strong to have any major bearing on the flow. Logically, it doesn't make sense to have a 3D streamline in 2D simulation since if you see it is different than surface streamline, aren't we actually antithesizing our earlier assumption of 2D? :) OJ 
Yes, Saisanthosh you comment does not make sense. If you constrain the streamlines to the symmetry planes then you reduce the integration errors from noise in the third dimension. So 2D models should use surface streamlines on a symmetry plane to reduce this error.

CFD post
Hi mates
I would appreciate if some body can help me to about how I can starting CFD post[/B] in comment lines and export data. Cheers 
1 Attachment(s)
Quote:
The normal velocity component is, as expected, exactly zero. Any idea what causes this and how to fix it? 
Streamlines start from a seed point, or many of them. So these are just the seed points for the streamline.
The easiest way to fix this is to make the streamline integrate backwards and forwards. 
1 Attachment(s)
Quote:
I'm not sure how exactly CFD post calculated the streamlines. But the velocity in top left corner is very low. So maybe there is a maximum integration time or something. I tried to manually change the time limit for the integration. THe attached pitcture shows the streamlines for three differend time limites. Increasing the limit over 100 000 s does not have any effect. However, this would not explain the ending streamlines in the big vortex. 
You are correct in that case, the streamlines ending is because that is where the integration ended. Note that CFX does not calculate streamfunction but integrates over the velocity field so that means numerical accuracy will result in streamlines not closing. And of course streamfunction does not exist for 3D flows anyway.
So you will have to adjust the integration parameters  but note the streamline has to end somewhere, so in recirculations you will never eliminate the streamline ending. 
Ok, thanks for your answer! I would like to get that vortex in the corner closed  or if it's not closing, at least the streamlines shouldn't end right there.
I tried increasing the max. integration time, but I could not see any change when increasing it over 10^5 s. Based on the velocity at this point, I should definately see a difference in streamline length when increasing it from 10^5 to 10^6. The only explanaiting that I can think of is that there is an internal maximum integration time (< 10^6 s) in CFX that stops the integration even though the value given in the max time field is not reached. But in this case, I would expect to obtain an error message when entering high values for max time. I also played with the other parameters... the tolerance and so on...but that didn't help either. Any suggestions on what else I could try to fix this? 
You can move the ending point around by adjusting the parameters as you have done. You might be able to move it to a location where it is not as visible.
But as my previous post said:" Note that CFX does not calculate streamfunction but integrates over the velocity field so that means numerical accuracy will result in streamlines not closing." This means in a recirculation the line has to end somewhere so it is impossible to completely avoid the line ends. 
All times are GMT 4. The time now is 08:07. 