## Fluids

Topics relate to Fluent, CFX, Turbogrid and more

#### Energy Equation Divergence ansys divergence

Subscriber

Hello

During the simulation the error appears to me

For pressure–velocity coupling, a segregated solver was used with the SIMPLE algorithm. The second-order upwind scheme was used to discretize the convective terms in the governing equations.

The residuals were set to 10−4 for continuity, 10−5 for momentum, and 10−6 for energy equations.

The number of iterations per time step was set to 20.

The time step size 0.001

number of time steps 5000

mesh: 500 000 element

This is the geometry (heat sink TPMS) (Fluid: air, Solid: aluminum)

• Rob
Forum Moderator

What's the mesh quality like?

Subscriber

Hellom

This is the Report quality:

Mesh Quality:

Minimum Orthogonal Quality =  3.24228e-07 cell 86742 on zone 6 (ID: 1279410 on partition: 2) at location ( 1.00402e-02  7.34195e-03  3.86050e-03)
(To improve Orthogonal quality , use "Inverse Orthogonal Quality" in Fluent Meshing,
where Inverse Orthogonal Quality = 1 - Orthogonal Quality)
Warning: minimum Orthogonal Quality below 0.01.

Maximum Aspect Ratio =  1.34494e+03 cell 296109 on zone 6 (ID: 1115234 on partition: 2) at location ( 5.03466e-02  1.06909e-03 -8.35610e-03)

Fluent can try to improve the mesh quality via the TUI command
/mesh/repair-improve/improve-quality
Domain Extents:
x-coordinate: min (m) = -9.000000e-02, max (m) = 1.500000e-01
y-coordinate: min (m) = -1.000664e-02, max (m) = 1.000000e-02
z-coordinate: min (m) = -1.000000e-02, max (m) = 1.050000e-02
Volume statistics:
minimum volume (m3): 8.992539e-16
maximum volume (m3): 6.769667e-10
total volume (m3): 9.907077e-05
Face area statistics:
minimum face area (m2): 7.985135e-11
maximum face area (m2): 1.673634e-06
Checking mesh.....................................
Done.

Subscriber

I reduced the mesh to 10 million elements, but the problem persists until now

• Rob
Forum Moderator

Yes, it's the mesh. Min ortho quality of 0.05 is considered to be poor quality, you're somewhat below that. Similarly aspect ratio has some leeway for inflation, but 1,300 is very high.

Looking at the second image, check the walls bounding the flow that cut the structure don't have narrow gaps or crevices which then cause the skew cells.

Subscriber

I reduced the meshing from half a million to 10 million elements to reduce the effect of meshing
I also checked that the geometry does not have any gaps or crevices.
But no change, the problem still exists

Could the problem be somewhere other than the mesh or the geometry?

• Rob
Forum Moderator

And what did that do to the cell quality?

Subscriber

The problem has been solved. You were right. There was a problem with the mesh.

Subscriber

I have another problem with the results
When I create pathlines for the air, it appears that it passes through the structure without being considered, as shown in Image 1

Also, there is no change in air temperature as shown in pictures 2

No turbulence appears.

I used the SST K w for viscous

• Rob
Forum Moderator

That means you've managed to mesh both zones but not split the solid from the fluid: that may explain the improvement in cell quality.

Subscriber

Sorry, I didn't understand how to split the solid from the fluid?

I am working with a solid separated from the fluid, like the picture below

• Rob
Forum Moderator

Try subtract. Unless you really want to see the solid heat up you don't need it in the CFD model.

Subscriber

I need to see the heating of the solid with the velocity of the fluid and show the turbulence

• Rob
Forum Moderator

OK, so you'll need to subtract and retain the solid and then share topology. The terms etc are covered in the tutorials, and I advise having a look at the various conjugate heat transfer tutorials/videos on the Ansys system.