[harshavardhanps383]

Good evening,

I designed square cylinder and splitted square cylinder into two parts.
When I draw static pressure on corner line, I getting small peak at the intersection( as shown in figure). I want to know why this peak at the intersection?

thanks in advance

[andy_]

What is a square cylinder? How was it split? What equations are you solving? What boundary conditions are imposed? What does the grid look like. I think you may need to provide some more information like this if the issue to be understood.

[harshavardhanps383]

Sorry sir,
I designed square cylinder with length 7m(splitted at 2m from inlet).

I am simulationg flow through square cylinder in fluent(with fine mesh) with boundary conditions zero gauge total pressure at inlet mass flow rate (7.99kg/sec) at outlet and Navier Stokes governing equations are used.
After simulation I plotted static pressure on corner line I got above figure.
But I want know why this peak at 2m from inlet( Where I splitted square cylinder into two parts).

Thanks in advance

[sbaffini]

Is this like a pipe buth with a square cross setion, so that the flow is inside the square cylinder? Or is the flow outside of the square cylinder like in external aerodynamics?

In both cases, what is a corner line?

With A LOT of extrapolation, I guess you are referring to the first case, a flow trough a pipe with a square cross section and that by corner line you refer to one of the 4 streamwise lines passing trough one of the vertices of the square cross section.

Now, if that is the case, this means you are plotting the pressure on the wall, in one of the corners, along the streamwise direction. And I am pretty sure you are using the node values to do it.

If that is the case, the reason you see that jump, while impossible to know for certain, is almost surely due to the fact that node values on boundaries are most probably built by first constructing boundary values on cell faces and then interpolating from there. The problem here is that, if you split up the boundary, the interpolation stencil there is "broken" by design, it's just one sided (the cost of rebuilding it correctly in all the cases is unreasonable, given the postprocessing nature of the interpolation).

My general suggestion is to never use interpolations in postprocessing, at least not if you don't know what you're doing and not willing to accept dirty results in certain cases. For Fluent, in almost every case, this means not using node values in post processing.

In your very specific case (again, if that is what you're doing), the location of the line where you are plotting the pressure is plagued by additional considerations. What if you had split up the cylinder in 4 faces? What face Fluent should have used to plot your pressure? At convergence, hopefully, this doesn't make any difference, but in general? Not using node values should work for you as well. But in case it doesn't, I suggest using a line passing trough the corner cell center (so, not exactly on the wall), again without node values.

[FMDenaro]

Originally Posted by harshavardhanps383

Sorry sir,
I designed square cylinder with length 7m(splitted at 2m from inlet).

I am simulationg flow through square cylinder in fluent(with fine mesh) with boundary conditions zero gauge total pressure at inlet mass flow rate (7.99kg/sec) at outlet and Navier Stokes governing equations are used.
After simulation I plotted static pressure on corner line I got above figure.
But I want know why this peak at 2m from inlet( Where I splitted square cylinder into two parts).

Thanks in advance

The static pressure is associated to the normal unit vector, therefore this is is a singular point. I have no idea if your software simply change the value going to a closest node on the other wall or not. Maybe there is an interpolation issue. However, you can never describe a real corner on a finite grid.