Learning Forum

[raushan79]

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 information

 

 

I 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 setting

 

Initialization

 

 

Run Calculation

 

I am sincerely looking for a solution to solve this issue.

[Rob]

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. 

[raushan79]

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.

[raushan79]

Sir,

I am looking for your reply.

 

[Rob]

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. 

[raushan79]

Dear Sir,

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.

[Rob]

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). 

[raushan79]

Dear Sir,

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. 

 

[Rob]

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. 

[raushan79]

Dear Sir,

Thank you very much for your support.

Could you please explain the drawback of CFF in a bit more detail?

 

[Rob]

No. 

[raushan79]

Thank you for your support.