November 23, 2018 at 2:11 pmJosé MantovaniSubscriber
Hello guys! I try to make a simulation of classical Turbulent Channel Flow.
I'm basing my simulation on the work of Moser and Kim (1999) and I want to simulate for Rethau values equal to 180, 300, and 590. I found, as it seems, a PowerPoint presentation from Stanford University with comments and data on how to model this type in the images below. In the image have the boundary conditions used, material parameters, initial conditions, solver setup, etc..
So I use same initial conditions, same geometry dimensions, a similar grid and k-epsilon with enhanced wall treatment. And I get the results in the image below.
As We can see in the first image (that I get in the internet) the TKE Contour looks like a channel flow in a downstream region, but my TKE Contour looks like a upstream region (as if the flow were coming out of a tank and flowing into the channel). By this (and other divergences, like the values of TKE), I have some questions:
- How Can I input the initial conditions: inlet and outlet conditions as a Periodic Boundary Conditions?
- What do I need to change to make my simulation look like the first image?
- The variable y + by default already has in FLUENT, how can I insert the variable u +? (I ask this because I found several formulas on the internet).
- How can I compute the value of uthau and Rethau to ensure if I have the values I want?
I decided to test this in a simple 2D simulation to understand this issue of periodic boundaries and how to model a zero pressure gradient in order to heal my doubts and be able to perform this 3D simulation using LES.
I am immensely grateful for those who read and help me, I hope this helps other users in the community.
November 23, 2018 at 3:57 pmRobAnsys Employee
For periodics build a model and set the upstream & downstream surfaces as type interface in Meshing (ideally with different names) and make sure the mesh is about the same. In Fluent look at teh Mesh Interfaces and Periodic.
Periodic settings are in the Boundary Conditions section, look in the options below the list of boundaries. Not sure about LES and periodics as you may have eddies larger than the domain length - test with RANS to see how it works and then experiment.
Assuming the u+ value has a formula you can use a Custom Field Function. Use x or y coordinate as the wall distance function, remember to correct for the model position!
November 23, 2018 at 4:29 pmJosé MantovaniSubscriber
Thanks to reply rwoolhou, I will try and soon I share here.
When I load the geometry in Meshing and I mesh using Edge Sizing, after that I click on the lines and I set the horizontal as wall and vertical as inlet and outlet. How did you say this process of naming the boundaries changes? Should I interface? Sorry, I did not understand correctly. I need first define the line as interface in Ansys Meshing? How make this? I see this image below in Google, but I don't find in FLUENT.
November 23, 2018 at 5:26 pmRobAnsys Employee
In ANSYS Meshing set the named selection as interface, and Fluent will pick that up. The panel may be slightly different in Fluent, but you can find the interfaces in the list on the left side of the Fluent window.
November 23, 2018 at 5:50 pmJosé MantovaniSubscriber
Thanks one more time rwoolhou. I do and now its work. But, now I need set u+ formula, can you help me? Look in image below the results for u velocity and tke contours and a xy plot of u+ vs y+ and how I define the u+.
I am doing something wrong, the graph does not appear at all with what I found on the internet ... In the file it does not indicate the values of k and epsilon or turb intensity ...
November 23, 2018 at 8:37 pmDrAmineAnsys EmployeeUplus is the ratio of the bulk velocity to wall stress velocity or the use of the equation from Fluent to get ustar.
April 24, 2020 at 11:10 amIRobinSubscriber
I know this is an older post but I would like to achieve the same result as José mentioned. I followed all steps pointed out by rwoolhou, but my solution does not converge no matter what I try. I used the exact same values as given in the PowerPoint of the Stanford University (density, viscosity, length width, etc...) I have attached some pictures of the settings I used:
And for the periodic boundary condition I use:
When I monitor the maximum velocity value at one of the periodic boundaries, it shows an increasing trend no matter how long I iterate. The residuals are not showing anything better:
Although the residuals start to behave a bit after longer iterations, it is not seen back in the velocity control point (keeps increasing). I also tried to lower the pressure drop (to values of -0.008 Pa/m), specify a mass flow, but the velocity keeps on increasing every simulation no matter how long it iterates... Such an 'easy' problem should not take that many iterations, or does anyone have an idea of what I am doing wrong?
April 24, 2020 at 2:57 pmRobAnsys Employee
Why are you using a negative pressure drop over the section?
May 13, 2020 at 2:11 pmIRobinSubscriber
I used both positive and negative values, but the result did not change. The reason why it is negative is that I expect a negative pressure drop (flow from left to right). But to come back to the simulation, I seem to be unable to get a converging and mesh independent solution. After 100 000 iterations, one of my meshes finally converged. But when I refine further, this iteration number went up even further. Note that I also used a first guess of the velocity field, otherwise it would take even longer.... It just seems strange that such a trivial problem takes so many iterations before it converges.
May 13, 2020 at 3:30 pmRobAnsys Employee
The value is the "drop" so with a negative I'm not sure what the maths will try and do: possibly a pressure rise!
If you put a velocity bc at one end and pressure at the other does it work? I'm not too worried about the accuracy, this is to check the mesh.
May 13, 2020 at 4:14 pmIRobinSubscriber
When using a velocity inlet (u_x = 1.0 m/s) and a pressure outlet (p=0), I get an (almost) instantly converged solution (monitored values do not change after 30 iterations). I have attached the velocity and turbulent kinetic energy below:
These results are identical (almost to the last digit) to what José Mantovani illustrated at the top/beginning of this post. He then solved it by using the periodic boundary conditions... But this seems to fail when I try it. Ones again, if I simply change the inlet/outlet BC to interface's and enable the (translational) 'periodic boundary' for both via the interface menu + set a pressure drop of 0.1. I get an infinitely increasing velocity..
May 13, 2020 at 6:18 pmKalyan GoparajuAnsys Employee
When you run long enough, due to the specification of translational periodic boundary condition with a pressure drop, the flow will actually attain what is called a fully developed state. It could happen that the residuals might converge to a value of 1e-3, but the velocity can still keep increasing. This is an indication that the problem hasn't yet attained an equilibrium state.For such problems, don't just base the convergence on residuals alone. Instead, run the simulation for as long as the monitors to reach a plateau. For this, I would recommend either turning off the residuals or further lowering the threshold to say 1e-5 or 1e-6.
May 14, 2020 at 9:38 amIRobinSubscriber
Thank you for your reply. I indeed lowered the residuals such that they don't stop/influence the simulation. As I mentioned, I did also monitor points of interest (like the maximum velocity, average mass flux) and noticed that these have a hard time obtaining a plateau. For example, for a mesh with roughly ~10000 elements, it took well over 120 000 iterations before I noticed a plateau. Then again, it still required additional computation to verify whether this was indeed a plateau. I have run multiple simulations of different kinds with ANSYS Fluent in the past year and never encountered one which took this many iterations while being such an 'easy' problem. Hence I wanted to make sure I did not do anything wrong.
May 14, 2020 at 1:34 pmKalyan GoparajuAnsys Employee
Though your setup is correct, I agree with you, 120,000 iterations sounds too much for this problem. Are you using a coupled solver? Did you turn on pseudo-transient? Can you perhaps try increasing the time scale factor to 3 or 5 and see it if helps achieve a faster convergence?
- 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
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- The solver failed with a non-zero exit code of : 2
- Exporting Data Results
- error in cfd post