[mikandri]

Hello everyone,
I'm trying to simulate a model of an axial flow pump.
I'm having problems with meshing, I can't change the geometry and CFX is not converging. Also the number of nodes allowed is limited at 512k because of the student Suite.
I'm a novice in CFD and any tips are appreciated.

I attached pictures of the geometry, issues with meshing and solver.
Previously I created a simulation of the same blade geometry, but with just a long cylinder at the center with no closing ogive like the one in the attachment, successfully. It had similar bad face angles too but every other metric ok at the outlet and it converged successfully. I've tried lots and lots of combinations in "mesh data" in turbogrid and don't really know what to try anymore
After a certain number of iterations (about 330) i get the warning "wall added at outlet"
The previous geometry used to converge with many less iterations than that and no such warning.

Any help would be appreciated.
Thanks!

[Opaque]

May I ask:
1 - What approach are you using for solver control: AutoTimescale, or Physical Timescale
2 - How does the computed/used timescale compare to the scales reported by the solver? see Global Scales section
3 - How much linear solver effort is reported in the output file when solving the momentum/continuity equations? It is the standalone number in the last row to the right of the diagnostics. Say more than 5, and less than 15?

Because it seems to be converging w/o issues, just slowly, I would try to increase the used timescale. Say Timescale Factor of 2 and see if the slope of the residual plot goes down faster (it is currently too flat -> slow)

[mikandri]

Originally Posted by Opaque

May I ask:
1 - What approach are you using for solver control: AutoTimescale, or Physical Timescale
2 - How does the computed/used timescale compare to the scales reported by the solver? see Global Scales section
3 - How much linear solver effort is reported in the output file when solving the momentum/continuity equations? It is the standalone number in the last row to the right of the diagnostics. Say more than 5, and less than 15?

Because it seems to be converging w/o issues, just slowly, I would try to increase the used timescale. Say Timescale Factor of 2 and see if the slope of the residual plot goes down faster (it is currently too flat -> slow)

Thanks for the reply!
Also I didn't point out that this is a steady state simulation.

1. Auto Timescale (was set by default, I don't really know the difference)
2. Timescale factor is set at 1.0 in solver control. I can't find the scales reported by the solver...
3. If I'm looking at the correct values in the last iteration of the solver I see:
-to the right of P-mass in the "Linear Solution" column 12.9
-K-TurbKE 5.7
-E-Diss.K 12.3

Since I think the issue could be with the mesh (that I'm not able to improve) here are the mesh statistics found in the out file:
(Fluid 1 is the first part with the ogive, Fluid2 the part with the blades and Fluid3 all the rest after the blades)

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| Fluid 1 | 20.7 ok | 2 OK | 75 OK |
| Fluid2 | 9.9 ! | 3 OK | 189 ok |
| Fluid3 | 12.0 ! | 3 OK | 2105 ! |
| Global | 9.9 ! | 3 OK | 2105 ! |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| Fluid 1 | 0 22 78 | 0 0 100 | 0 0 100 |
| Fluid2 | 3 26 71 | 0 0 100 | 0 <1 100 |
| Fluid3 | 21 46 33 | 0 0 100 | 1 2 97 |
| Global | 9 33 58 | 0 0 100 | <1 1 99 |
+----------------------+---------------+--------------+--------------+

Also, yes I guess it just converges slowly (I'll try to change timescale factor) but still after some time i get the warning
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 14.3% of the faces, 0.9% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: Outlet. |
| The fluid name is: Fluid 1. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
which doesn't make much sense since no fluid should be able to enter from the outlet with this kind of pump!

[Opaque]

Mesh quality looks good enough to me.

May I ask why you are using K-E instead of SST? Would you get the same problem with SST?

Careful interpreting the artificial walls at the outlet. It is not that fluid is coming in, it means a recirculation zone is being formed (which means flow is trying to come in) and the outlet boundary condition does not support such a situation. Imagine such a zone really exists; then, cutting the domain at that specific location will have a reverse flow for an outlet.

You can extend/shorten the domain depending on what makes more sense. However, for less than 1% of the area being covered, I would not worry that much at the moment since the solution is not fully converged yet. If you look at the partially converged solution in the post-processor, you may be able to identify which areas of the outlet surface are being blocked. Usually around the edges.

Summary: try running a larger time step, check the influence of using SST instead of K-E. Let us see what that leads to.

[mikandri]

Originally Posted by Opaque

Mesh quality looks good enough to me.

May I ask why you are using K-E instead of SST? Would you get the same problem with SST?

Careful interpreting the artificial walls at the outlet. It is not that fluid is coming in, it means a recirculation zone is being formed (which means flow is trying to come in) and the outlet boundary condition does not support such a situation. Imagine such a zone really exists; then, cutting the domain at that specific location will have a reverse flow for an outlet.

You can extend/shorten the domain depending on what makes more sense. However, for less than 1% of the area being covered, I would not worry that much at the moment since the solution is not fully converged yet. If you look at the partially converged solution in the post-processor, you may be able to identify which areas of the outlet surface are being blocked. Usually around the edges.

Summary: try running a larger time step, check the influence of using SST instead of K-E. Let us see what that leads to.

Thanks for the tips.
The covered area gets up to 10% when converged so non-negligible and the solution doesn't really look like what I'd expect it to.
I'll try to use SST and timescale factor 2

[mikandri]

Originally Posted by Opaque

Mesh quality looks good enough to me.

May I ask why you are using K-E instead of SST? Would you get the same problem with SST?

Careful interpreting the artificial walls at the outlet. It is not that fluid is coming in, it means a recirculation zone is being formed (which means flow is trying to come in) and the outlet boundary condition does not support such a situation. Imagine such a zone really exists; then, cutting the domain at that specific location will have a reverse flow for an outlet.

You can extend/shorten the domain depending on what makes more sense. However, for less than 1% of the area being covered, I would not worry that much at the moment since the solution is not fully converged yet. If you look at the partially converged solution in the post-processor, you may be able to identify which areas of the outlet surface are being blocked. Usually around the edges.

Summary: try running a larger time step, check the influence of using SST instead of K-E. Let us see what that leads to.

UPDATE:
With SST I still get 10% of the area covered by wall. With Timefactor 2.0 it takes about half the iterations to converge so that's really good.
The results still don't look good and I don't really know what else to try

[AtoHM]

Now go on with Opaque's hint to move the outlet closer/further away. You need to get the boundary out of the recirculation zone.


Although I am not convinced that the mesh quality is good enough. Max Edge Length of 3e6. How it that even possible?

[mikandri]

Originally Posted by AtoHM

Now go on with Opaque's hint to move the outlet closer/further away. You need to get the boundary out of the recirculation zone.


Although I am not convinced that the mesh quality is good enough. Max Edge Length of 3e6. How it that even possible?

Thanks for the reply.
Tomorrow I'll try moving the outlet.
This is the geometry file http://www.mediafire.com/file/oqw8m9vnfm0ihh5/file
I really don't know how to make the mesh better and yeah Max Edge Length of 3e6 seems ridiculous