Learning Forum

[nguy3394]

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?

[nguy3394]

[nguy3394]

[Rob]

What is the water density? 

[nguy3394]

998.2kg/m3. Cell zone condition is assigned to water-liquid. Operating density is also 998kg/m3

[Rob]

OK, and why would warm water at 998.2kg/m3 rise above cooler water at 998.2 kg/m3?

 

[nguy3394]

 

because of gravity, cool water (more dense) falls down while warm water (less dense) rises to the top. When I open the velocity vector, I am expecting a pattern quite similiar to what I drawn. 

 

 

[Rob]

But if the density is constant, why would it move? 

https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v221/en/flu_ug/flu_ug_sec_density.html

[nguy3394]

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? 

[Rob]

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. 

[nguy3394]

 

Now I have obtained the velocity and temperature, but the velocity is not symmetric for a steady-state case. The residual graph looks fine, why is this the case?

[Rob]

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. 

[nguy3394]

 

I tried it and the results are the same. However, when I stop the calculation when the residual graph is stabilized, the velocity is symmetric. What does this mean for steady-state? Can I trust this result?

[Rob]

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. 

[nguy3394]

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. 

[Rob]

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. 

[nguy3394]

Next I'm trying to get the animation going for transient case, but the storage directory is greyed out and animation playback option does not work after a calculation. Also, for the initialization, where should I compute from? All-region, wall, or heat source?

[nguy3394]

The video did not happen because I did not specify number of time step, its working now. Then, does this time step size correspond to actual time in real life? If number of time step is 500, and time step size is 0.2s, does it mean the whole process take 100s in real time?

 

[Rob]

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. 

[nguy3394]

Thank you. Now I have switched the column model to 2D axisymmetric instead of 3D, it seems faster and easier to control. For the wall boundary condition, if the water column is inside a 5mm acrylic wall at 20C room temperature, this setting is correct is that right?

 

 

[nguy3394]

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.