[FarzinD]

Originally Posted by Thomas MADELEINE

It is a one way coupling and the particles don't affect your flow, right ?
your problem seems to be based one the fluid and not the particle, right ?

Have you tried to run your calculation without the particle part ? only a steady state run of your fluid ? you should expect to get the same problem normally (if I understood correctly)

Yes, the particles do not affect the flow and the results without them should be the same. Actually, I was planned to do that simplification though haven't done that yet.

[FarzinD]

Latest modification I've done ended with these results:
-Decreasing timescale factor to 0.3: increasing velocity of the monitor point (expansion), for both half-pipe and whole-pipe.
-doubling the number of nodes [in axial direction]: increasing increasing velocity of the monitor point (just tried on half-pipe).

After doing all of the above modifications the velocity of the interested point (expansion) in half-pipe (which increased from 7.2 to 7.8 m/s) is less than the whole-pipe's velocity (9.5 m/s).

[ghorrocks]

If this is a steady state simulation then the time step size (or time scale factor) is not important. Just the residuals and imbalances it gets to. Time step size is important for transient simulations only.

If changing your mesh size as you describe changes the result by that much it shows that you are a long way from a mesh insensitive simulation (which means the results of your simulation are not dependant on your mesh). You will have to do considerable mesh refinement to reach mesh insensitivity.

[flotus1]

Please dont get this the wrong way, but to me it just seems like this is leading nowhere.

Why dont you take one step back and really think about what you are trying to model and which boundary conditions you used.
The results for the full model and a half model have to be perfectly identical, especially for a simple setup like a pipe expansion.
Period.

As long as the results dont match exactly, there is no point in tweaking any solver setting or changing the grid spacing.
There must be something wrong with the setup.
It might be a good idea to draw a sketch with the exact boundary conditions you used for both models (including a coordinate system) and upload it here.

[ghorrocks]

No offence taken, I value constructive comments. But I think this thread is slowly heading in the right direction.

The results for the full model and a half model have to be perfectly identical, especially for a simple setup like a pipe expansion.

Yes I agree - when the two simulations you are comparing are solved with good numerical accuracy. If the simulations are solved with poor accuracy then the results can be almost random, and they will not be even close to identical. And that appears to be what is occurring here.

Farzin reported that tighter convergence got the results to get closer to each other - so this suggests to me that numerical accuracy is an issue here.

I do agree with your final point - it would be good to show the exact setup to check there is no fundamental error in the setup. Note that I am not saying there is no fundamental setup problem, I am saying there is a numerical accuracy problem and there might be a fundamental setup problem.

[flotus1]

So we both agree that there is some fundamental error here

Let me modify my initial statement from "it just seems like this is leading nowhere." to "maybe we are searching in the wrong place."

[FarzinD]

I doubt that the mesh refinement can solve the problem. Because the velocities' changes are in the order of 0.1 but the difference between the cases are in the order of the 1.
Though I recently found that mesh refinement has a different effect on two cases and doubling the number of nodes for whole-pipe caused the monitor point's velocity decrease from 9.47 to 9.2m/s. (The half-pip which have about half amount of mesh elements, velocity at this point equals to 7.8m/s.)
This is the conditions of the flow for both cases I'm trying to simulate:
PIPE_EXPANSION_ANSYS_CFX_8.jpg
And this is the CFX-pre ccl files of two cases:
PipeExpansion_CCLs.zip

[flotus1]

Still not quite the complete description of boundary conditions I expected but...
Are you really using a velocity boundary condition for inlet and outlet?

[FarzinD]

Originally Posted by flotus1

Still not quite the complete description of boundary conditions I expected but...
Are you really using a velocity boundary condition for inlet and outlet?

Yes, I'm using velocity components for both inlet and outlet.
Actually in the previous work of others (Nugroho, 2001) which I'm intending to do, the mass flow rate is given. I assumed the fluid is incompressible and calculated these velocities, which are nearly the same as velocities computed in that study.
The table of parameters used in that study has come below:
Nugroho-Fonti-Table.jpg

[flotus1]

With two velocity boundary conditions, the problem is ill-posed.
Use a pressure boundary condition at the outlet instead.

[FarzinD]

After choosing discharge-to-atmosphere as outlet boundary condition, with the coarse grid I used at first, velocity at the expansion plane for both cases is nearly the same (5.3712 against 5.3713 m/s).
However, there is much more modifications to do to reach an accurate result and the outlet condition of the study mentioned before is unclear to me, the problem that initiated this discussion is solved.
Thank you Alex, Glenn and Thomas. I learned much during these tries and errors.