## Fluids

Topics relate to Fluent, CFX, Turbogrid and more

#### NATURAL CONVECTION HEAT TRANSFER USING INCOMPRESSIBLE IDEAL GAS OR IDEAL GAS.

• Mohammed Ali
Subscriber

Hi, I am trying to model natural convection in an external domain around a 2D cylinder. all my boundary conditions are pressure outlets with gauge pressure set to 0. My cylinder wall temp is 350k and ambient air temp is 294k.

With bousinessq, i am getting accurate flow patterns and heat transfer coefficients. However, when i change the density model to incompressible ideal gas or ideal gas (and i am setting all the parameters and operating conditions correctly), the flow is occuring downwards (with gravity) instead of against gravity.

This seems to be a major problem with no solution anywhere. Any help would be appreciated

• C N
Ansys Employee

Hello,

When you change the model to incompressible ideal gas , I recommend you set in the operating conditions to activate the gravity acceleration and give negative direction in z axis -9.81m/s . This way the flow may occur against the gravity . Morever the ideal incompressible gas is used for weak compressible gas with temperature dependency and ideal gas accounts for both pressure and temperature effects. Hope this solves your problem

Thanks

• Mohammed Ali
Subscriber

My simulation works for boussinesq. I have gravity already set. However, as soon as i switch to ideal gas, the flow of air goes downwards with gravity. Is there any recommendation for simulation natural convection with ideal gas assumption - I could use boussinesq, however, when I want to deal with high temperatures, too many errors will be introduced.

• Rob
Forum Moderator

Initialise the model at "outside" conditions. Find the domain density and put that EXACT value into the operating density. Your error is down to the way Fluent accounts (or rather doesn't) for hydrostatic pressure on the external boundary.

• Mohammed Ali
Subscriber

so when I use the ideal gas model, would my inputs be:

• operating pressure: 101325
• operating density: 1.095 (density of air that i want to use)
• while my boundary conditions are all pressure outlets with a gauge pressure of 0

• Rob
Forum Moderator

If the GAUGE pressure is zero what is the pressure? If you initialise the domain, what is the density that Fluent reports? Compute a contour having initialised from the pressure boundaries, turn off node values.

• Mohammed Ali
Subscriber

after initialising, the pressure reported in the whole domain is 1.01 kg/m^3

• Mohammed Ali
Subscriber

however, I just checked and it was initialoising the domain temperature as my cylinder wall surface temp instead of an ambien temp. so my whole domain was at 350k while it should be at 294k. is that what causes the unrealisitc flow do you think?

• Rob
Forum Moderator

What did you set the operating density as? Use all of the decimal places in the operating conditions panel, so, 1.181234 kg/m3 or whatever Fluent returns.

• Mohammed Ali
Subscriber

1.095kg/m3

• Mohammed Ali
Subscriber

fyi, my model is:

• 2d horizontal cylindar with a diameter of 0.3m
• domain is: 2.4m height by 1.5m width
• Rob
Forum Moderator

Is 1.095 kg/m3 EXACTLY what Fluent returned?

• Mohammed Ali
Subscriber

So I think i have found a solution. First i set up the model with incompressible ideal gas and have all boundary conditions as pressure outlets. Then I initialised with ambient air temperature so make fluent calculate the average fluid density. I then input this average density back into the operating density and run the simulation using this. However, I am not sure why this gives me the correct solution.

• Rob
Forum Moderator

That is the solution, hence my first post in the thread.   Look at https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v231/en/flu_ug/flu_ug_bcs_sec_operating.html  specifically 7.3.1.5  You're setting rho-rho0 to be zero, so lose the gravity term for the exterior boundaries, otherwise you need to set a pressure gradient on the exterior boundary to account for (rho-rho0)gh and that gets messy.

• Mohammed Ali
Subscriber

ah ok - i cant access the url since i am using ansys with my company and cant get access to the customer number. however, that explanation has cleared things up. cheers!!

• Rob
Forum Moderator

Click on Help in the software & it’ll add a token to the browser to then let you use the link. If you are using commercial software you may be eligible for full support - check with the licence holder (your colleague) for details.