[FarzinD]

Hello everyone,
I'm trying to simulate pipe sudden expansion with ANSYS CFX. The flow is upward and expected to be symmetric. So I did one case with whole pipe expansion geometry, and another with half pipe and symmetry plane.
The flow models are exactly the same. In both there is particle motion, one-way coupled with fluid flow.
The results should be similar, but there is a considerable difference.
Here are the fluid velocity contours; half-pipe expansion [with reflection] on the left and whole-pipe on the right.
PIPE_EXPANSION_ANSYS_CFX_1.jpg
The whole pipe result seems to be more accurate and realistic.
Why this difference exists? Thanks for sharing your thoughts.

[Thomas MADELEINE]

the whole pipe is more realistic sounds quite encouraging to me since the symmetry BC are just an simplification of your real geometry.
But you shouldn't have big difference between the two if there is a real symmetry.

To my point of view, I will not use a symmetry in a pipe but a rotational interface. A symmetry will forbid the rotational movement inside a pipe and so can be not accurate at all (in other hand it can avoid a divergence effect on this phenomena).

Plot the rotational velocity in your whole pipe, if there is some this is the difference between your two cases.

[FarzinD]

Originally Posted by Thomas MADELEINE

the whole pipe is more realistic sounds quite encouraging to me since the symmetry BC are just an simplification of your real geometry.
But you shouldn't have big difference between the two if there is a real symmetry.

To my point of view, I will not use a symmetry in a pipe but a rotational interface. A symmetry will forbid the rotational movement inside a pipe and so can be not accurate at all (in other hand it can avoid a divergence effect on this phenomena).

Plot the rotational velocity in your whole pipe, if there is some this is the difference between your two cases.

Thank you Thomas,
As far as I know, from CFX documents, in cases like this where there is symmetrical geometry and flow, symmetry BC should give the same result as whole pipe.

About rotational geometry, it should be a 2-D simulation, right? then I should find a way to deal with CFX 3-D based solver.
Here are the velocity vectors in expansion plane (pipe cross section, top view) :
PIPE_EXPANSION_ANSYS_CFX_2.jpg
The arrows are all upward, pointing out of the plane. So there is no rotational velocity.

[Thomas MADELEINE]

when you have a symmetry it should be approximately the same results. the difference is that symmetry forbid any massflow through the surface and reality the average massflow is null (you can have vortex and other stuff like this)

you can have an periodic interface with the angle you want (it is better when you simulate less than 180°) common thing are:
quasi-2D (1°)
a sixth (60°)
one quarter (90°)
it is possible with 180° but you have to create two interfaces: one at 0° the other at 180° (not sure to be clear one this one sorry).

If you simulate particle I will avoid quasi-2D but I am not an expert on this.

anyway if you don't have any vorticity in your pipe, it should be something else...
Sadly, I don't know anything in particle tracking, so I can't help much on this one...

[FarzinD]

Originally Posted by Thomas MADELEINE

when you have a symmetry it should be approximately the same results. the difference is that symmetry forbid any massflow through the surface and reality the average massflow is null (you can have vortex and other stuff like this)

you can have an periodic interface with the angle you want (it is better when you simulate less than 180°) common thing are:
quasi-2D (1°)
a sixth (60°)
one quarter (90°)
it is possible with 180° but you have to create two interfaces: one at 0° the other at 180° (not sure to be clear one this one sorry).

If you simulate particle I will avoid quasi-2D but I am not an expert on this.

anyway if you don't have any vorticity in your pipe, it should be something else...
Sadly, I don't know anything in particle tracking, so I can't help much on this one...

I don't think changing the geometry is a good idea for me. Because I use a specific grid (Structured, O-Grid type, and the purpose is to do grid dependence study) and I don't think I can handle it for an angular slice of pipes.
Here is the meshing discussion in ANSYS ICEM CFD sub-forum.
http://www.cfd-online.com/Forums/ans...expansion.html

[Thomas MADELEINE]

I think this (in picture) is the best way to have some fine mesh at a portion of a pizza... it is quite simple to do on ICEM with the O-grid option and select two edge (If I remember correctly).

I had a quick look on the ICEM topic,the simple extrusion of your block to mesh the sudden expansion of your pipe is the best idea for me.
so you have three extrusion:
1 for the first part of your pipe in length direction
2 for the second part of you pipe in length direction
3 in radial direction to fill the expansion

you cut the block on the length direction and extrude a new one to fill the sudden expansion. you can at the end create a boundary layer easily with a final O-Grid option on the face that are on the wall...

it is about time I didn't use ICEM so I hope it will work...

then in CFX (to fill the forum section ^^) you can have the periodic interface. you should have also a faster run since you have less elements in your mesh.

[ghorrocks]

I am suspicious that the simulations Farzin shows are not fully converged or have some other form of numerical inaccuracy. This would mean the results are rubbish and comparisons between two rubbish simulations are also rubbish.

Farzin: What checks have you done to ensure your simulation is properly converged, the mesh is adequate, your particles are correct and all the other normal checks which should be done in a CFD simulation?

[QCFD]

Since the bulk velocity on one of your cases appears higher than the other, I suspect there is more of a difference between the models than just symmetric vs. full pipe.

Is there heat transfer in this problem (is the fluid heating up and expanding)

What are you using for inlet and outlet BCs (pressure, mass flow, ...)

Also, I would definitely check your mass imbalance for both cases in solver manager

[FarzinD]

Originally Posted by Thomas MADELEINE

I think this (in picture) is the best way to have some fine mesh at a portion of a pizza... it is quite simple to do on ICEM with the O-grid option and select two edge (If I remember correctly).

I had a quick look on the ICEM topic,the simple extrusion of your block to mesh the sudden expansion of your pipe is the best idea for me.
so you have three extrusion:
1 for the first part of your pipe in length direction
2 for the second part of you pipe in length direction
3 in radial direction to fill the expansion

you cut the block on the length direction and extrude a new one to fill the sudden expansion. you can at the end create a boundary layer easily with a final O-Grid option on the face that are on the wall...

it is about time I didn't use ICEM so I hope it will work...

then in CFX (to fill the forum section ^^) you can have the periodic interface. you should have also a faster run since you have less elements in your mesh.

Thank you, maybe I should try that later.
But I think with this type of geometry (half-pipe), I should get a reasonable, similar result. The reason is that this simulation is like what someone else (Sekti Nugroho, 2001) did in his thesis. The models I used here for elementary study are different, however they implemented some desired models.
And this is what they get for this flow conditions:
Nugroho-Fonti-Velocity.jpg
Clearly their result is much similar to the whole pipe simulation, than the half-pipe.

[FarzinD]

Originally Posted by ghorrocks

I am suspicious that the simulations Farzin shows are not fully converged or have some other form of numerical inaccuracy. This would mean the results are rubbish and comparisons between two rubbish simulations are also rubbish.

Farzin: What checks have you done to ensure your simulation is properly converged, the mesh is adequate, your particles are correct and all the other normal checks which should be done in a CFD simulation?

The convergence criteria used for these two simulation are the same (CFX-pre defaults). though I add particle tracking controls, I don't think even turning the particle tracking off make the results more alike at all.
One thing that I noticed when solver was running is that the half-pipe took more iterations to converge than the whole pipe (25 against 19).
PIPE_EXPANSION_ANSYS_CFX_3.jpg
Another weird thing with the half-pipe case was that after many struggles that I made a desired mesh with a good quality (http://www.cfd-online.com/Forums/ans...expansion.html) I saw in the CFD-post, that the plane (for visualization, though it was not needed) I locate in the position that symmetry wall should be, does not exactly lie on it.
PIPE_EXPANSION_ANSYS_CFX_4.jpg

[FarzinD]

Originally Posted by QCFD

Since the bulk velocity on one of your cases appears higher than the other, I suspect there is more of a difference between the models than just symmetric vs. full pipe.

Is there heat transfer in this problem (is the fluid heating up and expanding)

What are you using for inlet and outlet BCs (pressure, mass flow, ...)

Also, I would definitely check your mass imbalance for both cases in solver manager

The models are exactly the same, because for the whole-pipe simulation (which I tried later) I just copied the half-pipe cfx-pre case, and removed the symmetry wall boundary, and as for as I remember nothing else I did.
There is no heat transfer and I set it's option to none.
I'll check the mass balance soon and tell if it is as it should or not.

[flotus1]

Please run much more iterations on both cases. Ideally, run until the residuals level out. A converged solution is always one thing less to worry about when dealing with strange results.

[ghorrocks]

The convergence criteria used for these two simulation are the same (CFX-pre defaults)

So you have not checked this. It is pointless comparing simulations which are potentially inaccurate. You need to check the simulation is accurate before you can draw any conclusion from it.

This FAQ discusses some of the things you need to consider: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

The most important thing in this case appears to be the convergence criteria. Try a tighter convergence criteria and see if it makes a difference.

[Lance]

Originally Posted by FarzinD

The models are exactly the same, because for the whole-pipe simulation (which I tried later) I just copied the half-pipe cfx-pre case, and removed the symmetry wall boundary, and as for as I remember nothing else I did.

Did you use massflow as boundary condition at the inlet? Changing the inlet size (half vs full domain) without changing the mass flow rate will give you different velocities.

[FarzinD]

Originally Posted by Lance

Did you use massflow as boundary condition at the inlet? Changing the inlet size (half vs full domain) without changing the mass flow rate will give you different velocities.

No, it's velocity components.

Originally Posted by ghorrocks

So you have not checked this. It is pointless comparing simulations which are potentially inaccurate. You need to check the simulation is accurate before you can draw any conclusion from it.

This FAQ discusses some of the things you need to consider: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

The most important thing in this case appears to be the convergence criteria. Try a tighter convergence criteria and see if it makes a difference.

Your suspicion was right. I'd forgotten how important the convergence criteria really is.
After modifying the criteria the velocity contours are much similar, but the values are slightly different. Half-pipe has a maximum of ~7m/s at expansion area and whole-pipe's maximum is ~9m/s.
The whole-pipe seem to be converged after about 40 iterations and the half-pipe after about 60, but in less time.
Results of two cases but after 80 iterations:
PIPE_EXPANSION_ANSYS_CFX_5.jpg
The question is that the whole-pipe results are really more reliable?

[ghorrocks]

No, do not jump to conclusions (ie comparing one simulation to another) when you still have no idea if your simulation is accurate or not.

Keep tightening the convergence criteria until the result does not change within a tolerance you are happy to live with.

Then check your mesh - do another mesh with half the element edge length (ie approx 8x the number of nodes) and compare it to this simulation. Keep refining your mesh until the answer is accurate within a tolerance you are happy to live with.

Then check any other tunable parameter in your model - it could be the number of particle tracks or anything.

Note that all of these checks are internal, so just checking if the simulation is giving accurate answers to the simulation you asked. Only once you have some confidence of the accuracy of the simulations with and without the symmetry plane - then you compare the results between the simulations.

[Thomas MADELEINE]

for a convergence criteria, creating a monitor point of your velocity and plot it during the run looks like a good idea to me, since that the variable you are interested in.
you will know if the velocity is converged or not

[ghorrocks]

That sounds like a really good idea in this case.

[FarzinD]

Originally Posted by ghorrocks

No, do not jump to conclusions (ie comparing one simulation to another) when you still have no idea if your simulation is accurate or not.

Keep tightening the convergence criteria until the result does not change within a tolerance you are happy to live with.

Then check your mesh - do another mesh with half the element edge length (ie approx 8x the number of nodes) and compare it to this simulation. Keep refining your mesh until the answer is accurate within a tolerance you are happy to live with.

Then check any other tunable parameter in your model - it could be the number of particle tracks or anything.

Note that all of these checks are internal, so just checking if the simulation is giving accurate answers to the simulation you asked. Only once you have some confidence of the accuracy of the simulations with and without the symmetry plane - then you compare the results between the simulations.

Originally Posted by Thomas MADELEINE

for a convergence criteria, creating a monitor point of your velocity and plot it during the run looks like a good idea to me, since that the variable you are interested in.
you will know if the velocity is converged or not

This is the graph of the monitor point for velocity at expansion plane. It seem that it is converged after 40 iterations. (Half-pipe simulation)
PIPE_EXPANSION_ANSYS_CFX_6.jpg
About the mesh, I think it is sufficient, because it has more radial nodes than the study mentioned above (Nugroho, 2001). But number of nodes on the axial curves maybe needed to be modified.
In addition I chose the number of nodes on each curve( Or edge, in ICEM CFD language) so that the number of the element in half-pipe grid is almost half the whole-pipe's.
PIPE_EXPANSION_ANSYS_CFX_7.jpg

One thing that I found is that I entered mass rate for particles in half-pipe case equal to whole-pipe, which is incorrect. But after correction, the results for fluid are the same as before; because as I said the fluid and particles are related with one-way coupling, so the particle inputs and motion cannot affect the characteristics of fluid's flow.

[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)