[Christoph.Ha]

Hello,

i try to simulate a conjugated heat transfer problem inside a machine housing. So i have a fluid (r134a) floating on the inner side of the machine, which i want to simulate in the first step (without energy on this step).

• Inlet is velocity Inlet with 20000 Pa and 15 m/s
• Outlet is pressure outlet is pressure outlet (0 Pa gauge)
• Model is k omega (SST)
• Hybrid initialization
• Mesh should be fine eneugh, Skewness max. 0.94 (average arround 0.18)

I tried several things (URF, different Models, Time step size, smaller inlet velocity, ...) and also read the FAQ, but weren´t able to solve my problem.

Console shows following:

reversed flow in 10972 faces on pressure-outlet 10.
58 1.4592e+04 2.0549e-01 1.9756e-01 2.7431e-01 3.4938e-01 4.4964e-01 0:44:55 32

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 12510 cells

reversed flow in 11267 faces on pressure-outlet 10.
59 1.5151e+04 1.6443e-01 1.8216e-01 2.1520e-01 2.8820e-01 4.3027e-01 0:42:40 31

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 11978 cells

reversed flow in 11686 faces on pressure-outlet 10.
60 2.6691e+05 1.0398e+00 5.2143e-01 3.0286e-01 8.5261e+00 1.5065e+02 0:41:20 30
# Divergence detected in AMG for omega: protective actions enabled!
# Divergence detected in AMG for omega, temporarily solve with BCGSTAB!

Divergence detected in AMG solver: omega
reversed flow in 10488 faces on pressure-outlet 10.

Divergence detected in AMG solver: omega
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: omega
Error at host: floating point exception

Error at Node 0: floating point exception

Error at Node 1: floating point exception

Error at Node 2: floating point exception

Error at Node 3: floating point exception

Error at Node 4: floating point exception

Error at Node 5: floating point exception

Error at Node 6: floating point exception

Error at Node 7: floating point exception

Error: floating point exception
Error Object: #f

Calculation complete.

Do you guys have any idea?
Thanks in advance!

Christoph

[Christoph.Ha]

No one with an idea?

Regards,
Christoph

[MKuhn]

Hello Christoph,

how did you implement the thermodynamical properties of R134a? Do you have the right properties? Under atmospheric pressure and room temperature, it should be liquid. And 15 m/s are quite high for liquid flow.

Moritz

[litzj]

do you check your y+ value near the wall? it should be near 1 or 30

using k-e might be an option

[Christoph.Ha]

Hello MKuhn,

the pressure is 2.73 bar and the temperature is 5°C, so it should be a gas. My Density is 20.7 kg/m³ and the viscosity is 1.103e-05 kg/ms.

@litzj: That is one big problem for me. Since the geometry is quite complexe, it is not easy to create reasonable inflation layer. In addition to that, with 15m/s the Layer needs to be very thin (in the area of some µm), which leads to incredible big mesh sizes. But what i thought so far is, that it should still converge? And which y+ values do you recomand using k-e?
I uploaded an image of the fluid domain including the mesh. The inlet is on the right side, outlet is a larger (pulled apart) area on the bottom. The housing connects on the top end of the fluid domain.

Thank you so far!
Christoph

[MKuhn]

Originally Posted by Christoph.Ha

the pressure is 2.73 bar and the temperature is 5°C, so it should be a gas. My Density is 20.7 kg/m³ and the viscosity is 1.103e-05 kg/ms.

Do you use these values a constant or temperature dependent values in the material dialog box? Is 2.73 bar your operating pressure as you can set it by operating conditions?

Try to check if this problem related to R134a and run your model just with air instead of the refrigerant.

[Christoph.Ha]

At the moment at constant, since i don´t enabled energy yet.
2,73 is my pressure on the inlet, operating pressure is on default. Specified Operating Density is Enabled.

Trying it with air is a good hint. I´m running it at the moment, but it doesn´t seem to converge either ..

Currently i´m thinking of those reversed flow´s. They appear and dissapear during the iterations. I googled it but it shouldn´t lead to big problems. But since my continuity diverges the most, would it be usefull to extend the outlet region?

[MKuhn]

Now it looks that you have a pressure inlet. That doesn't match with your first post, where you wrote that you have a velocity inlet. As you set the gauge pressure at the outlet to 0, you will have a pressure drop along your channel of 2,37 bar, this is quite a lot and will not match with the 15 m/s and could be the reason that the solution will not converge.
Set the operating pressure (Define -> operating conditions ..) to 2,37 bar, choose velocity inlet with 15 m/s and leave the value for Supersonic/Initial Gauge Pressure to "0", because you have not supersonic flow.

Moritz

[AlexanderZ]

Regarding y+

For k-e model with Enchanced Wall treatment it is recommended to have y+ between 70 to 300

Best regards

[Christoph.Ha]

Sorry for the late reply guys.
So i tested what Moritz suggested (gauge pressure inlet / outlet to 0 and operating pressure to 2.73) with SST transient and k-w (sst).
It still won´t converge (see picture from k-w (sst) below).

Y+ between 70 and 300 sounds doable, i´m going to check this case.

Furthermore i have a question about the turbulence specification method on the inlet and outlet. I use "intensity and length scale", with values of 20% (highly tubulent) and 0,005m. Does this sound reasonable to you guys?

Thanks in advance,
Christoph

[MKuhn]

These are the results with air or R134a? Do you use velocity inlet now?
Do you the "check mesh" command in Fluent? All right?
Use the functions under report to find out where high velocities or pressures occur, this could indicate bad mesh.

[Christoph.Ha]

Those are results with r134a. I tested air before and it looked pretty similar. Yes, i´m using the velocity inlet now.

Mesh check says following:

Domain Extents:
x-coordinate: min (m) = -6.149421e-02, max (m) = 6.151522e-02
y-coordinate: min (m) = -7.349509e-02, max (m) = 1.059904e-01
z-coordinate: min (m) = -2.534911e-02, max (m) = 4.388730e-02
Volume statistics:
minimum volume (m3): 4.318037e-18
maximum volume (m3): 5.955609e-08
total volume (m3): 4.982530e-04
Face area statistics:
minimum face area (m2): 3.088456e-12
maximum face area (m2): 3.007505e-05
Checking mesh.........................
Done.

Do you mean Results -> Reports -> Discrete Phase / Projected Areas?
I´m not very familiar with these functions, there shows nothing up like velocitie or pressure. Could you give me a short explanation for that?

Thank you very much,
Christoph

[MKuhn]

You can check the maximum velocity via:
Reports -> Volume Integrals than Report Type "Maximum", Field Variable "Velocity Magnitude" and your Cell Zone, should be only one Cell Zone.

Another way. Go to Adapt -> Iso-Value than Iso-Values of "Velocity Magnitude" than "Compute". With "Mark" you can store the cells within a certain Velocity range. Afterwards you can display these cells Adapt -> Manage..

Also check Reports -> Fluxes than Mass Flow Rate and calculated the differenz between your Inlet and Outlet, shoud be near zero.

[Christoph.Ha]

Maximum Velocity shows following:

Max
Velocity Magnitude (m/s)
-------------------------------- --------------------
fff_fluid -1e+20
---------------- --------------------
Net -1e+20

The Adapt -> Iso-Values of shows 0 for Min and Max, domain is the right one.


Mass Flow Rate shows following:

Mass Flow Rate (kg/s)
-------------------------------- --------------------
outlet 1.#QNAN
inlet 0.00041686927
---------------- --------------------
Net 1.#QNAN

What does #QNAN mean?

I talked to a Professor regarding this topic and he recommended me to start with a laminar calculation to get a proper initialization. In addition i should try to lower my inlet velocity in the beginning, so i did a run with 3 m/s inlet velocity, air as fluid and laminar.
I even made the outlet a lot longer (arround 5*d) to get rid of the backflow.
The continuity does still diverge quite strong

[MKuhn]

The values show, that is something wrong with your set up or mesh.
Maximum Velocity should show reasonable values in the range of your inlet velocity. The mass flow at the in- and outlout should be equal. 1.#QAN is a floating point exception error.

For troubleshooting, according to your residuals, stop the simulation after 10 iteration (so before the error occurs) and retrieve the values for velocites and mass flow again. Also check the velocities and in- and outlet via Reports -> Surface Integrals than your in and outlet BC and choose velocity magnitude after 10 iterations.

[AlexanderZ]

Inlet is velocity Inlet with 20000 Pa and 15 m/s
Outlet is pressure outlet is pressure outlet (0 Pa gauge)


Did you set operating pressure? I guess it should be 0 for your BC
Try to use much smaller velocity at the begging, You may initialize your case with small velocity value, for example V-yaxis = 0.01m/s

Best regards

[Christoph.Ha]

Hello,

Velocity shows:

Max
Velocity Magnitude (m/s)
-------------------------------- --------------------
fff_fluid 88251.539
---------------- --------------------
Net 88251.539

Mass Flow Rate shows:

Mass Flow Rate (kg/s)
-------------------------------- --------------------
inlet 0.00083373836
outlet -0.00093480007
---------------- --------------------
Net -0.00010106171

So i guess Mass Flow Rate seems tob e okay and the Problem is linked somehow with way to high velocitys.

Inlet Velocity (Min and Max) shows 3 m/s, which is the value i set as inlet BC.
Outlet Velocity (Min / Max) shows: 0.006173 m/s / 0.875 m/s

The picture below shows the cells with a velocity higher than 100m/s (red marked). Afterwards I used the “Adapt” function to refine the mesh within this areas:

Grid size ( original / adapted / change)
cells ( 20655141 / 22018958 / 1363817)
faces ( 42564325 / 46436483 / 3872158)
nodes ( 4220342 / 4633091 / 412749)

Now I’m going to do a run with the optimized Mesh.
Question is, why those areas are that critical, compared to other “sharp” edges right at the inlet area?


Edit: Second picture shows the run with the "Adapted" mesh. I did the changes after iteration 17.

[Christoph.Ha]

Originally Posted by AlexanderZ

Inlet is velocity Inlet with 20000 Pa and 15 m/s
Outlet is pressure outlet is pressure outlet (0 Pa gauge)


Did you set operating pressure? I guess it should be 0 for your BC
Try to use much smaller velocity at the begging, You may initialize your case with small velocity value, for example V-yaxis = 0.01m/s

Best regards

Operating Pressure is set to 101325 at the moment (i wanted to make sure that the 2,73 bar aren´t the problem).
Inlet and Outlet Pressure (gauge) is 0. I will try now a run with Inlet Velocity set to 0.01 m/s, thanks for the advice!

[Christoph.Ha]

Hello,

i have some news. Today i tested an setup without the solid wall, so just the fluid domain. That converged very well and max. Velocitys are <10m/s (with an inlet Velocity of 5m/s). So i think there must be something wrong with the interface.
During initialization i get following info: "Info: Interface zones overlap for mesh interface contact_region.
This could adversely affect your solution."
After some research i found out, that the walls of both domains have some issus with the contact definition. But i´m not aware of how i could solve that issue, does anybody of you guys can tell me how to fix it?

Thanks in advance,
Christoph

EDIT: Mesh -> Contacts -> Contact Region shows Contact: 686 Faces, Target: 687 Faces. Scoping Method is Geometry Selection.

[MKuhn]

Do you need realy the solid mesh? You can also define on your outer boundaries a certain wall thickness for a solid material in conjunction with "shell conduction".