TAGGED: -adaptive-mesh, dynamic-mesh, meshing, transient, vof
February 17, 2023 at 1:55 pmraushan79Subscriber
Hello,I am running a 3-D transient multiphase flow simulation for droplet coalescence over the hydrophobic substrate using the VOF model in the fluent 2020R2. To decrease the computational load, I am using volume fraction gradient-based mesh adaptation and adaptive time step advancement tool to model the coalescence. The following issues have been found while running the simulation.Case _1. When I am starting transient simulation at the zeroth time step and run it continuously up to any time step, the gradient-based mesh adaptation works uniformly.For example, if I am running a transient simulation from zero to 330-time step (as shown in the attachment A_Uniform Mesh_ time 330). The mesh adaption works smoothly throughout the domain.Case _2. When I restart the transient simulation at some time step after importing the case and data file and running it for further time steps then the mesh is adapting non-uniformly in the flow domain.For example, if I am running a transient simulation from the 176-time step to the 330-time step (as shown in attachment B_ Non-uniform Mesh_ time 330). The mesh adaptation is non-smooth in the flow domain.I am looking for a solution for Case _2. Because currently, I am working on a problem, where it is required to restart the simulation at any time step and to simulate it for further time steps.Here I am attaching all the details used to model the droplet coalescence.I have defined a volume fraction gradient over the flow domain. As shown in the figure
Then I am defining maximum refinement level-2 for dynamic adaptive mesh refinement based on gradient_0.These are set for Multiphase model informationI defined Phase 1 as Air and Phase 2 as water. CSF model was chosen for surface tension force. The contact angle was 90 degrees.Solution Method settingInitializationRun CalculationI am sincerely looking for a solution to solve this issue.
February 17, 2023 at 4:14 pmRobAnsys Employee
The adaption data isn't saved in the older .cas.gz format, use .cas.h5 and see how that goes. I'm sure I've seen someone raise this before, so there may be more details on here somewhere.
February 18, 2023 at 6:46 amraushan79Subscriber
Sir, I saved checked this after saving the data in .h5 format, but it is not working correctly and facing the same issue.
Thank you for your reply.
February 19, 2023 at 3:56 pmraushan79Subscriber
I am looking for your reply.
February 20, 2023 at 11:24 amRobAnsys Employee
Please check your calender, what day was 18th?
PUMA adaption ought to be default and be picked up by the HDF format; I've not seen any issues when testing here. Please try in 2023R1 and see if it's working in the current release.
February 22, 2023 at 6:40 amraushan79Subscriber
Thank you for your reply.
I have checked the case with Fluent 2023R1 after saving the case and data file in .cas.h5 and .dat.h5 format respectively. But, I am facing a similar issue after running the case at some non-zero time step.
I am sure I am doing a very small error while setting up the case. Please let me know you need any detail to solve this problem.
February 22, 2023 at 9:50 amRobAnsys Employee
Is that the result having fun from scratch, saved as HDF5 and then reopened, or having read the Legacy format in and then resaved? Please post a contour of the refinement levels (in Mesh I think).
February 23, 2023 at 7:49 amraushan79Subscriber
Thank you for your reply. I am using the following steps
Step 1- I launched the fluent through the workbench2020R1. I saved the case and data files in the Legacy format. Then I launched a new workbench2020R1 and imported the case and data files in the .cas.gz and .dat.gz formats and rerun the simulation and again saved the files in the Legacy format. In this case, mesh adaptation is non-uniform while restarting the simulation at the non-zero time step.
Step 2- I launched the fluent through the workbench2020R1. I saved the case and data files in the Legacy format. Then I launched Fluent standalone 2023R1 and imported the case and data files in the .cas.gz and .dat.gz formats and rerun the simulation and here saved the files in the CFF format (.cas.h5 and .dat.h5). Then again I launched a new Fluent standalone 2023R1 and imported the .cas.h5 and .dat.h5 files at non-zero time step and run the simulation. Then again I am getting a non-uniform mesh adaptation.
Step 3- I launched the fluent through the workbench2020R1. I saved the case and data files generated at 0 th time step in the Legacy format as there is no option of saving it into CFF format under Fluent 2020R1 launched through Workbench. Then I launched Fluent standalone 2023R1 and imported the case and data files in the .cas.gz and .dat.gz formats and saved the case and data file in the CFF format (.cas.h5 and .dat.h5) for the 0th time step. Then again I launched a new Fluent standalone 2023R1 and imported the .cas.h5 and .dat.h5 files at the zeroth time step and run the simulation saved files in CFF format. Then I stopped the simulation and restarted it after importing the case and data files in .dat.h5 format at a non-zero time step in the Fluent standalone 2023R1. Now, I am getting the correct mesh adaptation after restarting the simulation. 😀😀
Sir, Please let me know if there is some other way of doing the same simulation correctly.
your support is much appreciated and thank you for your time.
February 23, 2023 at 9:53 amRobAnsys Employee
Launch Fluent in standalone. Set up the model. Save case & data in CFF (HDF format). Run model & save in CFF. It's entirely down to the legacy format not retaining adaption register data: the format predates adaption. CFF (HDF) has been developed to retain more information as well as work more efficiently in parallel. The only drawback of CFF is it can be marginally less reliable: most likely due to the parallel data passing.
February 23, 2023 at 10:54 amraushan79Subscriber
Thank you very much for your support.
Could you please explain the drawback of CFF in a bit more detail?
February 23, 2023 at 2:55 pmRobAnsys Employee
February 24, 2023 at 7:48 amraushan79Subscriber
Thank you for your support.
- 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.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.