November 15, 2018 at 10:26 amJamessmp23Subscriber
I want to understand about the simulation convergence for steady state and share topology, combine component with non-share topology.
First, which one is converged ? (for these simulations I set the iteration number = 2000)
1. all the residual graph is stable
2. the continuity graph is stable
3. the continuity graph is not stable but can run the CFD-post
4. the simulation is converged before the setup iteration (at the TUI command appears the calculation is converged at 800, the setup iteration number is 2000 )
Second, Here are air velocity contours of my simulations with 1) share topology 2)none share topology 3)none share topology with merge component
The question is why the air flow got stuck only at the inlet or only at the riser ? does it happened because of the topology, merge component or the simulation is not converged yet ?
2) air contours of non-share topology
3) air contours of non-share topology with combine component
Thank you all,
November 15, 2018 at 1:43 pmRobAnsys Employee
Not entirely sure where to start, so if I miss something let us know.
Share topology is a geometry operation and means the meshing tool considers the volumes to be connected. There should be some videos etc covering this.
If you don't use share topology then Fluent will create mesh interfaces to allow flow to pass between volumes: looking at the results this hasn't happened.
Residuals are a function of the error, and need to be very low. However, just because a result is numerically converged it doesn't mean it's correct: if I don't have flow through the domain the solver may converge but is the answer physically correct (in the above this may be your error).
I can read any Fluent data into CFD Post - this just means the data is valid and not that it's converged!
November 15, 2018 at 2:09 pmKeyur KanadeAnsys Employee
Yes, as Rob pointed out share topology is geometry operation. It will decide if you are going to get conformal or non conformal mesh.
In your case please use share topology so that you will get conformal mesh.
If you can combine all bodies in one body then it is better.
For convergence, please see help manual.
November 18, 2018 at 7:32 amJamessmp23Subscriber
Thank you for replying, For now I'm simulating the combine component method with more greater iterations(from 2000 up to 6000 or 8000).
For the share topology I tried to simulated it again even the same duplication, at the TUI it said "floating point exception" and in the upper sentences has a "Experiencing convergence difficulties - temporarily relaxing and trying again"
(Mesh check was normal and wasn't has any error)
Then I tried to adjust the relaxation by used the Flexible cycle on multigrid (control>advanced>multigrid), used the second order instead of third order.
all these methods did not work for me in this case. Any suggestion ?
November 18, 2018 at 2:29 pmKarthik RAdministrator
Convergence issues can be because of multiple reasons. There could be a problem with your model set-up, boundary condtions, initializations, or mesh. In oreder for us to understand and help you in an efficient manner, please share some more details about your problem? Specifically, what are you trying to model, how are you trying to do this, what are your boundary conditions, and what is your end goal.
November 19, 2018 at 12:48 amJamessmp23Subscriber
i'm trying to see the basic circulation flow pattern of airlift-bioreactor from the reference paper, I need to set the all parts of the reactor as share topology except the draft tube to see the gas holdup, gas and water velocity at the riser and downcomer.
For this steady state simulation, I used the euler-euler multiphase, k-epsilon realizable.
On material I set the primary phase as water and secondary phase as air with 0.005 m diameter.
I set the cell zone : draft tube as solid (stationary wall) and other parts are fluid, at boundary condition I only set the air inlet = 0.075 m/s.
I used couple scheme, Least square cell based, third order MUSCL, Quick,third order MUSCL,third order MUSCL.
At control I set the flow courant number = 40. For the initialization I used Hybrid initialization and patch the air volume fraction as 0.2 at all parts except the draft tube section.
Do I set anything wrong or any suggestion for better fluent setup ?
November 19, 2018 at 1:09 amJamessmp23Subscriber
After I redraw the geometry and name selection, I thought I knew the reason why the flow did not flow through the sparger section,
Because of my stupid and not carefully I set the intersection face between the sparger and the bottom of the reactor as wall.
I will simulate it again, still any suggestion for better fluent setup are welcome.
Thank you for all support,
November 19, 2018 at 11:41 amRobAnsys Employee
You may need to switch to the transient solver as multiphase problems are inherently time dependent. I'd also drop back to 2nd order for most things, and 1st order for turbulence.
You will need to ensure everything connects up in the meshing tool: you will need share topology on all parts.
November 27, 2018 at 4:47 amJamessmp23Subscriber
Sorry for late reply, I was busy with other works.
I used the steady state solver for the latest simulation but the liquid flow doesn't circulate in the reactor,
I had done previous reference reactor, they do have the liquid circulation which have the same setup but different geometry.
Any suggestion ? now I will try to do it in transient solver.
Question : Do in the end(steady state),the steady state solver and transient solver have the same results ?
November 27, 2018 at 5:48 amseeta guntiAnsys Employee
If the flow has inherent unsteady ness in the flow filed, steady and transient will give different results. Steady flow will give the flow field at particular instant. The same flow filed may not exists for all times. So they won't give the same results.
But the flow does not have any unsteadiness in the flow field but you ran the case as unsteady, then both cases will give the same flow filed.
- You must be logged in to reply to this topic.
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.