Divergence detected in AMG solver and floating point exception in ANSYS Fluent
 

I am trying to quantify the heat exchange of an empty aluminium box in the high atmosphere (25 000 m)

But I keep getting an error message (see image)
I have tried this command in the Fluent console:
/mesh/repair-improve/improve-quality

It happens right away during the calculation
I don't have a dynamic mesh
My skewness seems big, but I don't know how to improve this.
Can you help me, I don't know what is happening.


Any advice or recommendation will be highly appreciated.
Thanks in advance

Have you set your initialization to start from the inlet? what about your reference values? It really shouldn't do that right away. Your bounding box is very small, can I see the inlet values?

Issue
 

There appear to be multiple issues with your case, assuming that the sides in visual are symmetry and rest are walls, i.e., a closed domain.

Firstly, the mesh is not good enough. For this domain, you can generate full hex mesh. Even if it is not full hex, an automatic mesh should be of quite high quality. Check the settings in you Meshing too. Ensure that CFD is enabled under Physics.

If the domain is closed, as I mentioned in the beginning, you have to use ideal gas or incompressible ideal gas or Boussinesq approximation. But you need to share more details of the physics before someone could provide further help. But first, a good quality mesh is needed. Skewness above 0.98 is a problem.

Thanks for yours answers
 

Tait10 "Have you set your initialization to start from the inlet? what about your reference values? It really shouldn't do that right away. Your bounding box is very small, can I see the inlet values? "

The values of the initialization and reference values are attached. The inlet is set as a "Pressure-far-field" There is also a screen attached. The temperature value is 221 K (not visible in the screen).

Vinerm "assuming that the sides in visual are symmetry and rest are walls, i.e., a closed domain."

I should have mentioned that, attached you will see a screen showing the symmetry, the rest of the outside of the mesh is set as a "far-pressure-field"

"Firstly, the mesh is not good enough. For this domain, you can generate full hex mesh"

I am limited by the number of mesh elements with the student version. I can't get my university to give me a proper licence. With this, I am at the max.
For the hex mesh, it does not happen automaticity for the exterior, I am going to force it with mesh sizing on the edge.

"Ensure that CFD is enabled under Physics."

I could not find what you were talking about in Fluent, sorry

"If the domain is closed, as I mentioned in the beginning, you have to use ideal gas or incompressible ideal gas or Boussinesq approximation. But you need to share more details of the physics before someone could provide further help"

Both of my fluid are ideal gas
with a Sutherland model for viscosity. (I am trying to quantify the impact of convection)


Thank you very much for your interest

you can find additional screens

Setup
 

If the box is solid, you do need such a fine mesh in there. Just put a coarse mesh. It is pure diffusion. Even a few cells would give you more or less same results. Far-field boundary condition is not appropriate until and unless you have rather high speed flow around the box. The only important region is a thin layer around the box, the boundary layer. Break the enclosure into multiple boxes and you will end up with full hex. Even student license gives you access to half a million cells; that's at least 5 times more than you need for this case.

Use pressure outlet in place of far-field. Set operating density to 0 and initialize with a pressure that you expect at 25 km height. Reference values are not important for a simulation; only when you want to determine some coefficients, such as, heat transfer coefficient.

Thank you very much for your helps!!

I did forget to set the "Physics Preference" for FLUENT in the mesh

I tried to have a hex mesh, but I was lazy and didn't changed the model to help the mesher. So I tried to use the edge sizing to get hex but it didn't work so I used the feature "hex_Dominant_Method".
But this would forbid me to use the inflation. So I judged that having the inflation was more important. I removed the hex and I upload the mesh like this into FLUENT.
The average quality is 0.6
I did all the modification that you suggested on the FLUENT setup.
The simulation is now running, hopefully it will be good enough.


Thank you very much, you are super helpful!
My roommate saw your message on my screen and apparently you also helped him for his PhD.

Thanks again
Rokual

Good
 

It's good that there was something helpful. Prefer not to use Hex Dominant mesh for CFD. The mesh although looks good yet you do not need boundary layer (inflation) inside the solid. Boundary layer mesh is required because flow has physical boundary layer where gradients are high. Solids do not have velocity gradients, hence, boundary layer mesh is not required inside the solid.

Hello,

Due to a deadline, Just restarted to work on this analysis.

About the mesh, the inflation inside is into the air inside. I have attached some screen with the detail and description of the mesh.
Since last time, I added a heater. It represent a thin Polyimide film heater (I've attached a picture). The heater could deliver up to 8 W, and I am expecting the surface temperature to be around between 150 and 200 °C.
I have also put "inflation" around the heater, but the quality is quite terrible as I don't have high-velocity flow and I am only looking into the convection effects, I was suggested to instead of the "inflation", just make element really small around the boundary. I will deal with this issue later, because the simulation can still run, and I realize that there is a bigger issue with my Set up.

For my model, I want to study the temperature of a volume of air at 1 bar trapped into a thin aluminium box in the high atmosphere environment (250 Pa and -50 °C). Inside the box, there will be some heaters to influence the temperature. For now, I've place only one.

I want the trapped air inside the aluminium box to be at 1 bar (initially, if the volume is at 20 °C for example).
I don't think that I understand the "Operating Conditions...". I thought that this would set the pressure at 1 bar... but it obviously didn't and all the fluids, outside and inside are at 250 Pa. (it is visible a picture attached)
250 Pa is the value of the outlet pressure condition of the air outside.
I understand that setting a pressure for the volume of air inside would be weird...
But, would it be possible to set, for example, the number of mol of air? In my case, it would be 0.02 mol. And then inside the restricted volume of the box and with the ideal gas law, Fluent could deduce the pressure and temperature with the heater?

Besides the outlet pressure boundary condition, all the boundary are walls with identical settings. It is visible in the screens attached.

I hope that this make sense
I am really grateful for you help
Thanks in advance,
Rokual


PS:
When I set a "hybrid initialization" after a few iterations (6-10) I get a new floating point exception error. I don't have this issue with a "standard initialization"... I really don't understand this either.

the other screens

Setup
 

The mesh quality inside the box is not good. You can make it coarser and it will work better than having a fine but skewed mesh. Inside the aluminum box, you need at least four cells across the thickness. You only have one and that is not good; minimum four are required. I'd suggest not to mesh the aluminum box since it is very thin and you can rather use thin wall boundary. That way you will not have to mesh the aluminum box.

As far as physical setup is concerned, since you have a closed domain, you need to model air using ideal gas. You cannot specify moles in the box but you can specify pressure and temperature; in fact, that's what Fluent does when you do initialization. Whatever pressure and temperature you use for initialization will be used to determine the density, hence, mass of air in the box. Do NOT use hybrid initialization; it does not apply to your case.

Thank you very much for the info.

I'll update the model and post the results :)

gettting some results
 

Hello,

I have corrected the mesh as Vinerm suggested. The mesh is coarser, but the quality is higher. The heater and the aluminium box are not modelled solid anymore. They are just named surface, and the thickness is set directly in ANSYS in the wall condition.
About the initialisation, I understood that I needed to use the “patch” option to set the right condition for each zone.
About boundary conditions, Initially, I had pressure outlets on the sides like Vinerm , on the bottom and the top. But, the air was falling on the box. And, the velocity was blowing the convection heat effect that I was expected on the top of the box.
By replacing the side of the boundary with “pressure inlet” with the option “prevent reverse flow rate” seemed to work. The inlet would act as a wall and hold the air to prevent it from falling while allowing the pressure drop induced by the convection sucking air on the side of the model.


This time, on the outside, I have set atmospheric condition because the convection effect would be more visible than with a thin atmosphere. I think that I got a promising result. On top of the box, we can see a column of hot air and inside a convection cell. I am quite happy with the look of the convection cells.
The effect is less visible when outside it is a thin atmosphere. I am considering making the “outside air” element larger on the sides and higher.
I think this is promising.
Next step, I will implement the radiation effect.


Thanks again Vinerm for your suggestions 😊
Any comment on the current set up will be welcomed

The results with the new set up :)

External Boundary Condition
 

The condition on the outermost boundary depends on whether it is open space or closed. If it is open space then pressure inlet or outlet are same. You can use whichever works. If it is closed, then those have to be wall. Gravity is a must for natural convection or else there cannot be a natural convection. The rest looks good.

Trying to add a fan in the model
 

Hello,

I update my model with a "Surface to surface" radiation model, a cylinder of plastic and a fan.

I still have some issues with the model (see last picture). But I am really concerned by the fan.

In real life, it will be a small computer fan from adafruit: https://www.adafruit.com/product/3368

But I have no idea how to implement the fan in the model. I don't have the fan yet, so I can't test it. I randomly defined the fan with a pressure drop of 0.15 Pa, and I got an airflow of around 1.5 m/s.
I don't know if this is a lot or not.
Does someone know how I should implement this little fan?

Thanks in advance
Rokual

Convergence
 

The case is not converged yet. For a converged case, each wall and shadow pair must have equal flux and total heat transfer rate, which is not the case for your simulation; observe the wall_heater_circular boundary and its shadow. If the case is transient, then you have to simulate until the case reaches a statistically steady regime and then look at averaged heat transfer rates. Averaging has to be done over integral flow cycles else it will appear as if there is not conservation.

Fan modeling requires fan data.