[Smeet]

I am simulating a journal bearing fluid element and want a xy plot on curve length on the surface marked in the picture [attached below] . Since it is a closed curved surface, fluent cannot plot along curve length. Is there any way to plot along curve length for such a surface?

I found a old thread where someone suggested to make an iso surface and then clip it to form a curved line, which I was not able to figure out. Can someone explain me that too? I made an iso surface at a constant distance from the axis, and now it is suggested to clip this surface to form a curve line on which I can plot, but clipping this even to the thinnest margin will form a sliver of surface, not a line. Am I selecting the right options in the clipping menu [attached below]??

[Rick]

Did you try the export option in CFD-Post?

[Smeet]

I didnt get you, how does the export option work in cfd post??

[Rick]

Create a polyline by boundary intersection method. If the points on this polyline are in the order you want, then you can plot the variable on this polyline in CFD-Post. However, if they are not, then export the required variable values for this polyline and do post-processing on the generated file.

[Smeet]

Thank you very much Rick!!
I got the curve length plot I was looking for.
I wish you a good day ahead!

[Smeet]

For anyone looking for the procedure to make xy plot on curve length on a closed surface:

1. Open CFD post and make a plane (from locations option) normal to your curve (z-axis is the normal in my case here)
2. Open the polyline option and select boundary intersection method, in 'boundary list' select the surface of your interest (on which you want to plot your variable); in 'intersect with' select that plane.
3.Click Apply and this creates the polyline.
4. Now open the chart option and in data series tab select polyline for location, in x axis tab select 'curve length of polyline x' and in y axis tab select the variable of your interest. Click apply and there is your plot. You can also export it to Excel or any spreadsheet software for further post processing.

Hopefully this is the plot you were looking for.

[saumi]

Hello Guys, I am fairly new to Ansys Fluent. I have worked with OPENFOAM in the past.

I am running a simple 2D case of an Elbow (See attached Image). My fluid is air at the moment. I want to plot my pressure and velocity variables against a spline/curve passing through the center fluid following the geometry of the elbow (Check the second image).

Can please anyone explain to me how I can achieve this in Ansys Fluent 2024 R2?
Thank you!