August 17, 2022 at 8:52 amnguy3394Subscriber
For heating up a water column to 100C, I am not getting any velocity vector indicating that heat transfer buoyancy is occuring in the water. Hot water is not rising, and I don't think that is correct. How do you make sure that this phenomenon happens?
August 17, 2022 at 8:52 am
August 17, 2022 at 8:54 am
August 17, 2022 at 12:24 pmRobAnsys Employee
What is the water density?
August 17, 2022 at 3:07 pmnguy3394Subscriber
998.2kg/m3. Cell zone condition is assigned to water-liquid. Operating density is also 998kg/m3
August 17, 2022 at 3:30 pmRobAnsys Employee
OK, and why would warm water at 998.2kg/m3 rise above cooler water at 998.2 kg/m3?
August 17, 2022 at 3:42 pm
August 17, 2022 at 3:51 pmRobAnsys Employee
But if the density is constant, why would it move?
August 17, 2022 at 4:19 pmnguy3394Subscriber
then I believe I have not setup the water_liquid correctly. Does Ansys already have the water density-temperature function, or do I have to define it myself via the piecewise-polynomial profile?
August 18, 2022 at 9:27 amRobAnsys Employee
You will need to define it. Assuming the water volume isn't sealed then one of the polynomial functions is appropriate. Otherwise you'll need Bousinesq, or change a few facets to a pressure outlet to allow the volume to adjust.
August 19, 2022 at 8:29 am
August 19, 2022 at 2:51 pmRobAnsys Employee
Plot the vertical velocity component and then run another 200 iterations. And/or add a point monitor for velocity. Buoyant flows tends to be inherently transient so you've probably picked up that.
August 19, 2022 at 3:14 pm
August 22, 2022 at 4:09 pmRobAnsys Employee
Maybe. Have a think about what the boundaries and flow mean, and what's going on. Here, the plume "ought" to go up the middle, but as it's a confined space Coanda Effect comes into play, as the plume goes left/right the pressure field changes (look at your results). Eventually, the plume sticks or, in this case flicks back to the other side. Cycle repeats.
Can you trust the steady result? That depends on what you need to know. Should you run transient, again that depends on what you need to know.
You do need to run more than 300 iterations though. Compare the results at 2500, 3000, 3500 and 4000 iterations.
August 23, 2022 at 6:06 amnguy3394Subscriber
Thank you for your explanation. For steady state, it usually stops at 500 iterations for 1e-5 residuals. From what you say, it is possible for the steady state's plume to be in the middle or to the side of the column? I have ran the calculation again several time; the plume switches from the center to the side from time to time, but the velocity as well as the temperature magnitude remain the same. It is an interesting phenomenon.
And then, do we have a way to verify if the velocity magnitude is resonable? 3.3mm/s for the maximum speed in the 4mm tall column maybe accurate for me, but I can't be sure.
August 23, 2022 at 2:53 pmRobAnsys Employee
I suspect there are some buoyant flow equations that'll let you calculate the theoretical speeds, I've not looked but try Google.
Yes, it is possible to have several correct steady solutions based on "stuff". The "pitchfork bifurcation" is likely the phenomena you're seeing here: it's caused some confusion for several clients over the years too. Where you do have several steady solutions you often see a poor convergence but sensible results as the solver drifts between the many (potentially infinite) possible answers.
August 24, 2022 at 6:35 am
August 24, 2022 at 6:27 pm
August 25, 2022 at 1:49 pmRobAnsys Employee
You need to compute from whatever makes most sense for your model.
The time step size is how quickly Fluent jumps through time. If the step size is too large you'll miss flow features, too small and the model will take a long time to solve each second. The number of steps is then how many updates you want Fluent to do. Re the time step, plot a sine curve with 2, 5, 10 and 50 points per cycle.
August 27, 2022 at 9:57 pm
August 27, 2022 at 10:13 pmnguy3394Subscriber
I just want to make sure that I can use these settings instead of having to actually sketch the solid wall around the water column, and then assign the material properties.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- Floating point exception
- The solver failed with a non-zero exit code of : 2
- How to model free convection warming of liquid in a plastic bag