July 31, 2023 at 2:45 pmSakunSubscriber
I have some doubts regarding time step calculations and i am using CFL = (u * Δt/Δx) formular. I use CFL number as 1 , for u i am using 383.9 m/s but Δx is what confusing me. According to some resources Δx represent the meaning of ,characteristic length, x direction cell length, minimum grid size, and cell length. So I don’t know what definition to choose in this case.
My Δx, Δy, and Δz mesh sizes around my blade (wall) are below,
∆Y 1.66E-06m (Y+ = 1)
∆X 1.99E-04m (X+ = 120)
∆Z 4.98E-05m (Z+ = 30)
So, what value should i use for my time-step calculations ?
Also, i have seen some people are using cube root method as well, can someone explain this method as well, and are there any other methods that ANSYS has recommended to calculate time-step ?
Highly appreciate for the guidance.
July 31, 2023 at 8:14 pmFederico Alzamora PrevitaliSubscriber
Numerically having a CFL value of 1 means that the flow will propagate by one cell length (delta x) at any given time step. The most conservative approach is then to take your maximum velocity and minimum cell length in setting your delta t. This ensures that the flow never goes beyond one cell, at any given time step, which is good practice if you have infinite resources but may be over restrictive. Hence, in practice it may not be practical to have CFL <= 1 everywhere.
Hence, you should aim for CFL = 1 in the regions of interest for your purpose, and decide on the mesh size and time step to resolve the relevant physics (space and time scales) of your flow.
August 1, 2023 at 9:50 amSakunSubscriber
Thank you very much for your explanation and reply,
Make sense, at the moment i am using CFL= 1 for my simulation specially in my area of interest (blade).
But my confusion is, what does it mean by mesh size ?(also, similarly going as minimum mesh size, cell length and characteristic cell length).
Which mesh size out of from Δx, Δy, and Δz (according to my post)should i use for mesh size to calculate Δt ?
August 1, 2023 at 12:51 pmFederico Alzamora PrevitaliSubscriber
You can start with the least conservative approach and choose the largest cell size that you have listed (your delta x). Once you have established your time step, run your simulation until you have somewhat of an established flow. You can then plot the Convective Courant number on a relevant surface (you can define a plane for this) and see if this meets your requirements. Based on this, you can then decide if you need to reduce your time step or not.
Another question, you mentioned that the region of interest is surrounding blades. Are these blades moving with a Dynamic Mesh?
August 1, 2023 at 1:15 pmSakunSubscriber
Thank you very much again for your quick reply,
When I choose ∆X = 1.99E-04m (X+ = 120), my ∆t is 5.183641E-07. So i will perform simulation and see if I can get CFL <= 1 around my blade profile.
No, it is a single compressor blade (0.7 Mach) with periodic boundary conditions and i am trying to validate isentropic mach number vs chord against the experimental data (attached pictures).
August 2, 2023 at 12:08 pmNickFLSubscriber
Now you understand why I was encouraging you to not have so many iterations per timestep ;) 😉
The truth is there is no real solution here. The CFL condition, in theory, provides an “easy” way to select a time step. But reality is not that easy. We have a fine grid near the wall and if we use this small y dimension, the time step is tiny. We can have large aspect ratio elements, as the elements can be stretched in the flow direction and we can try and use that dimension. But as the velocity increases, the time step limit shrinks. Then your mesh isn’t always aligned with the flow field, so trying to figure out the velocity vector in terms of your mesh orientation just adds complexity. (I will say, based upon the velocity picture on the other thread, it seems you created a very good mesh–well done)
Somewhere on the internet there is a Best Practices for LES by Florian Mentor (ANSYS Germany). I do not think it is on the ANSYS site (it may be in the Customer Portal somewhere), but if poke around on the internet I am sure you will find it. I would recommend reading that. It will explain the difference between LES and the DDES that the previous study used and how they navigated this roadblock by not doing a full LES. Ideally, we would love to have a CFL under 1, but in practice is just isn’t realistic for real-world problems.
Sorry I do not have better advice.
August 3, 2023 at 10:33 amSakunSubscriber
Much appreciated for the reply,
Yeah you’re absolutely correct, I had to experience that just to teach myself a lesson 😪
Yes I do i have both “Best Practices for LES by Florian Mentor” and “Quick guide to setting up LES version 1.4” presentation slides as well and i am going through it now.
Thank you very much again for all the best advises and guidance you have given to me🎉, I have learned a lot about reality of LES with respect to the available resources I have.
- 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?
- Heat transfer coefficient
- 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
- Suppress Fluent to open with GUI while performing in journal file
- Mesh Interfaces in ANSYS FLUENT
- Time Step Size and Courant Number
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.