July 19, 2023 at 11:52 amSakunSubscriber
I am simulating a single compressor blade in fluent 2021 R1. I have obtained a converged solution (attached cL results) and now i am proceeding with LES simulations. I have followed the procedure to simulate LES based simulation, as suggested in ansys user guide and i am using bounded central differencing scheme for both transient scheme (according to the ansys user manual suggestions) and all the flow variables as well but according to the attached cD result attachment, simulation become really unsteady.
Please can i have some recommandations to solve this issue,
July 19, 2023 at 2:36 pmFederico Alzamora PrevitaliSubscriber
LES will be inherently unsteady, and will oscillate slightly around a given value. If you look at Cl from iteration 100k (I assume this is when you started LES), you should see something similar.
You can sample this data and compute the RMS value of Cd to get a time-averaged value.
July 20, 2023 at 8:07 amSakunSubscriber
Thank you very much for the reply,
Yes you are correct i have started this simulation at 100k th iteration. In this simulation i have validate this against a exp data (isentropic mach number VS chord, attached picture) so honestly i am using cD and cL values to check the convergence. I need to have a reasonable steady condtition in LES to get the data to validate against experiment data.
July 20, 2023 at 8:14 amNickFLSubscriber
You say that you have a converged solution–this is likely for a steady RANS solve. Remember the A in RANS stands for averaged. This averaging is done in time to make the problem easier to solve. The downside it, it removes the fluctuations in the flow field and only gives us a time-averaged value. For many problems this is sufficient to provide an engineering representation of the flow field.
An LES on the other hand is a transient simulation that will allow these fluctuations in the flow field to develop. This is could be why you are seeing the unsteadiness in these coefficients. (It could also be diverging. Are the residuals behaving well?) If you were to save all the flow fields from your LES and then average them, it would (to some reasonable approximation) match the steady RANS simulation from above.
July 26, 2023 at 9:59 amSakunSubscriber
Appreciate for the reply and well explanation.
LES simulation ran without diverging and i have set up the simulation for 2000 timesteps with 60 max iteration per time step and delta T is 1e-06. i have attached a pictures of residuals and cL results with LES settings as well.
For my case, flow through time is 0.001148s but in the simultion happened only for 0.002s but the results are not suitable for the validation. So does it mean i have to run at least 1s or there is something wrong with my case set up ?
Thank you very much for your time,
July 26, 2023 at 12:49 pmNickFLSubscriber
How do you figure 1s of simulated time before you start sampling? Even in the most extreme cases I have heard about 3x the residence time. Basically, this time is just removed to eliminate the possibility that the steady-state initial condition pollutes the LES results. It is the numerical equivalent of not starting our measurements in the lab until we reach a steady state.
Just an FYI, I would recommend you switch the plots to be flow time rather than iteration. Every timestep you have x number of iterations, and it doesn't make sense to plot those that are not part of the solution.
And a last point, I don't see a real change between in the conitinuty residual with iteration 12 remaining and 0. You could easily lower your max number of iterations per timestep (by at least 12) to reduce the wall clock time.
July 27, 2023 at 11:33 amSakunSubscriber
Thank you very much for your kind reply,
So basically what you have mentioned in the 1st paragraph is, that 0.002 flow time in the LES simulation is to lower the influence of my initial condition values and make the simulation environment settle for LES (correct me if i am wrong). Just had a thought of running more of flow through time till 1s, since flow has not developed (attached velocity contour).
Sure, I will change the plots to flow time, thank you very much for the recommendation.
About the max number iterations per time step, I put 60 because i wanted to have a continuity residual of 1e-05 or 1e-06.
Thanks for your time,
July 30, 2023 at 6:17 amNickFLSubscriber
What is the goal of the simulation? Are you interested on this blade or the downstream one? If it is this one, you might be able to start collecting data. Waiting until 1 second seems like a bit too long. I don't think you want to wait 10 years for your solution. If it is a downstream part you are interested in, then maybe a bit longer. A good way to visualize the shed eddies is the vorticity. Look and see if these are dissipating at roughly the same spot. This can be an indication of start-up effects being removed from the simulation. Better would be to use a couple of monitor points on surfaces or at points you are interested in.
If you can reduced your iterations from 60 to 45 you would be saving 25% of your wall clock time, and a reduction to 30 would save you 50%. If you want a more accurate solution, it would probably be better to increase the number of cells and have less iterations. If you look at the quantities of interest from iteration 45 -> 30 -> 15, I would imagine there is little change.
July 31, 2023 at 10:02 amSakunSubscriber
Thank you very much again for the well explained reply,
Aim of this simulation is to validate the blade profile using advanced turbulence modal(attached picture), either DDES or LES. Yes, you’re absolutely correct about the timing and with my current resources, it will take many weeks to reach 1 second. The reason i have mentioned about simulating the case up to 1 second is that because in most of the research papers that related to turbomachinery, they have carried on the simulation between 1s and 5s for accuracy purposes. To assign monitor points on the surface, can i set up that in fluent before starting the simulation or do i have to do it in CFD-Post ?
I have been followed your recommendations and setup max iterations per time step as 30, so hopefully I’ll be able to simulate more timesteps.
July 31, 2023 at 11:32 amNickFLSubscriber
Use the monitor points to send it to the tui or even to an external file. Under solution in the tree, there is Report Definitions. Here you can create monitor points for surface, volume, flux, forces, etc. Review the documnentaiton for more details.
July 31, 2023 at 1:25 pmSakunSubscriber
Noted and highly appreciate for your guidence and time.
August 2, 2023 at 11:08 amSakunSubscriber
Sorry to bother you again,
Will you be able to help me on this following question as well ? highly appreciate if you can.
- 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.