[woodwax]

Hello

Iam very new in ANSYS.

Iam trying to simulate aluminium container filled up with water and heated from the bottom of the container. The container have a very thin (0.6mm) walls.

I cannot reach converging solution.
I tried mesh with triangles and with hexa with/without inflation but the result is the same. I dont have any other ideas.

Can anyone who is a pro check the mesh or the setup? And help me with good advices, or modidfy the project. Thank you!

I put here som pics of the residual, mesh and here is the link for the project:
https://files.fm/u/bbv8ng36

[AlexanderZ]

what model settings do you use?
did you try to solve only flow without energy?

best regards

[RaiderDoctor]

I don't think this has anything to do with the model settings, but rather how you are actually setting your problem up. I've made up a list of everything I see that is problematic. If you're a newbie, it's totally okay to feel lost in all this stuff. The world of CFD is really complicated, even for those of us who've worked with it for a few years. I highly recommend running through some tutorials that ANSYS offers and reading everything you can on how the program operates. As always, welcome to the forum!

• No water is present in the simulation
• As this is an axisymmetric case, it would be better suited to run a 2D simulation with the domain split in half
  • This would save time and allow a more accurate solution
  • See attached pictures (First is the cross-section of the case you are running, second is how I recommend you run it - 2D cut in half)
• You are running a transient case, but nothing changes with respect to time
• Furthermore, 20 iterations per time step is not enough to reach a converged solution
  • You can plainly see this by checking the residuals, and seeing that the first time step never converged
  • If a time step does not converge, it is very unlikely that any other step after it will
• You did not set your materials; you mentioned you were looking at water, but the default materials are still set (Tree-Materials)
• This is a big one; you improperly set your fluid domain to the walls of your container
  • When you meshed your geometry, you imported the walls of your container. This is not right, as the walls do not model any fluid flow
  • I’m guessing you want to look at the water inside the container, and how the heat is transferred to it
  • When you create your simulation, keep in mind what parts are your fluid domain, and what parts are your solid domain. It’s possible to import both in Fluent, but just understand that a majority of the calculations will be solved for the fluid
  • Always double-check which material is assigned to which zone (Tree-Cell Zone Conditions)
• In your Boundary Conditions, you rightly set that the walls of the container are made out of aluminum (Note: make sure that these values are correct for aluminum)
  • However, I think you can skip meshing the walls of the container altogether, and just us the Wall Thickness parameter below the Heat Flux option under the Thermal tab
  • According to the manual, “You can, however, in conjunction with any of the thermal conditions, model a thin layer of material on the wall” (For more check out 6.3.15 in the Fluent User’s Guide).
  • By using this feature, you can efficiently model the walls of the container without the need to mesh them, which will save you a lot of headache
• You never set your reference values. These are important, as they are used in calculation of the residuals
• Under Calculation Activities in the Tree, make sure you select how many times you’d like the simulation to save your data
  • This may seem weird, but Fluent will not save your data at each time step/iteration automatically
  • This is good when you have several thousand time steps that take up a lot of data
  • If you don’t set this, your work will not be saved
• I know I already encouraged you to run a steady-state simulation, but this is for future reference; your time step size and number of time steps are not appropriate
• Remember, a large times step will offer good stability but very poor accuracy. A small time step will offer good accuracy, but can cause the simulation to diverge. It’s up to you to decide what step size is appropriate, and if it captures the flow quantities in your simulation well enough
• The number of time steps relate to how long the simulation should last. Think of it this way, if you were running a simulation of flow in a pipe, you’d want to simulate to just after it becomes fully developed. The reason for this is two-fold, after it’s fully developed, it’s no different than a steady-state simulation, and calculating more steps will only increase your storage way more than it needs to be
• The maximum number of iterations per time step should always be overestimated. The only reason this even exists is so Fluent doesn’t spend an eternity trying to calculate a simulation that diverged a long time ago. It’s a fail-safe, and one that you should utilize appropriately. Set a little more than the number of iterations needed to converge, and monitor your solution to make sure it’s working well

[woodwax]

Thanks a lot for this precise, detailed guidance. After a hard work I can get some solution.

Now, I have container filled with water (not full). The bottom of the container is set to 373K, on the mantle I set natural air convection with 4 W/m2 (see pics.)
I compairing laminar flow vs k-epsilon flow.
I suprised how big is the temperature difference between the two modes.

But more surprisingly is the streamlines.
On the laminar flow mode there is a lot of streamlines also I can imagine that the water is flowing like on the picture.
But in case k-epsilon flow there is a very few with strange form of streamlines, I cannot imagine that water is going by this way.

Why are stramlines so strange on k-epsilon flow and why is so few of them?
What is the correct mode for this case? k-epsilon or laminar or something else? I think k-epsilon


This was a steady case with 100 number of iterations. Is this enough?

[RaiderDoctor]

Okay, a few questions here. I'm going to try and answer them out of order that you asked, but in an order that I think is most to least important. Cool?


No one here really knows if 100 iterations is enough for your simulation. The main reason? Because we have no way to judge your convergence. One way to judge convergence is by looking at your residuals; if they are below a set value, then you have a "good" solution. I say "good" because you need to see if your set value is low enough to maintain good accuracy. Next, you need to see if the particular quantities of interest (heat on the bottom plate or on the walls of the cylinder) are also converged. This isn't done by monitoring residuals, but by setting up a Surface Monitor (make sure you set it to each iteration, not time step). I'll leave you to read through the manual on how to do that. Basically, you want to make sure that when your solution is "converged" the surface monitor value isn't changing anymore. If it is, then your solution really isn't finished yet.


Why are you comparing k-epsilon with laminar flow? As fluid motion is derived not from a pressure difference, but a thermal one, this seems really weird to me. Go back and check your Reynold's number to make sure you have a case that is turbulent before using a turbulence model. You can use both models, but it just more computationally expensive to run more calculations.


What made you select k-epsilon? If you're answer is "because it's the most common", go back and read through the different models again. K-epsilon is good with flat plates, but potentially bad with flow separation. This might be all moot, thought, as you may not need a turbulence model at all.


I can say with some certainty that your solution for your turbulence model is wrong. The main reason why I can say this is that your temperature variation is non-existent in the turbulence model, so that's bad. Also, your turbulence model has a max volume that is 4 orders of magnitude lower than your laminar model. Check your solution, and see what's up.

[woodwax]

So, from the laminar model I calculate the Reynolds number: Re = ρ V D/μ = (998 * 0.14834 * 0.445) / 0.001003 = 65682

Where
ρ is the density of water = 998 kg/m3
V is the velocity of the fluid, I choose the maximum velocity from laminar solution = 0.14834 m/s
D is the diameter (of container?) = 0.445 m
μ is Viscosity of the fluid = 0.001003 kg/m*s

That is the correct way for calculating Reynolds number?