February 14, 2023 at 12:11 pmMohammed AliSubscriber
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
February 14, 2023 at 1:14 pmC NAnsys Employee
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
February 14, 2023 at 2:34 pmMohammed AliSubscriber
Hi, thanks for the reply.
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.
February 14, 2023 at 3:05 pmRobForum 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.
February 14, 2023 at 3:09 pmMohammed AliSubscriber
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
February 14, 2023 at 3:20 pmRobForum 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.
February 14, 2023 at 3:23 pmMohammed AliSubscriber
after initialising, the pressure reported in the whole domain is 1.01 kg/m^3
February 14, 2023 at 3:27 pmMohammed AliSubscriber
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?
February 14, 2023 at 4:50 pmRobForum 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.
February 14, 2023 at 4:51 pmMohammed AliSubscriber
February 14, 2023 at 4:56 pmMohammed AliSubscriber
fyi, my model is:
- 2d horizontal cylindar with a diameter of 0.3m
- domain is: 2.4m height by 1.5m width
February 15, 2023 at 10:30 amRobForum Moderator
Is 1.095 kg/m3 EXACTLY what Fluent returned?
February 15, 2023 at 10:59 amMohammed AliSubscriber
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.
February 15, 2023 at 11:07 amRobForum 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 126.96.36.199 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.
February 15, 2023 at 11:15 amMohammed AliSubscriber
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!!
February 15, 2023 at 11:18 amRobForum 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.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- Suppress Fluent to open with GUI while performing in journal file
- error: Received signal SIGSEGV
- Using GPU in FLUENT
© 2023 Copyright ANSYS, Inc. All rights reserved.