March 29, 2022 at 6:31 pmRoyaSubscriber
I am modeling a stirred bioreactor and am using MRF for modeling the impeller rotation. When I plot the air volume fraction contour, there is a discontinuity almost at the interface of the two regions and it looks like this;March 30, 2022 at 12:06 pmKarthik RAdministratorHello:
What are your rotating and stationary zones in this simulation? Can you please share some screenshots highlighting how you set up this problem?
March 30, 2022 at 12:24 pmRoyaSubscriberDear Karthik
Thank you so much for your answer. The domain is a tank with an impeller rotating at 250 rpm. There is a sparger at the bottom that injects single-size bubbles into the domain. The rotational region holds the impeller blades and the rest of the tank is stationary region. I use MRF(Frame motion) technique for setting up this problem. You can see the rotational region in picture below;
As you can see, the rotational MRF region's interface is exactly at the same place that the discontinuity in the contour takes place.
Kind regards Roya
March 30, 2022 at 12:35 pmKarthik RAdministratorHello Could you refine the mesh further, especially across the interface between your stationary and rotating regions? I suspect this is an artifact of either convergence or mesh.
March 30, 2022 at 1:31 pmRoyaSubscriberDear Karthik
I just noticed that as I try to change my simulation from MRF to sliding mesh and I use the command-line;
I receive a face-handedness error and my interfaces change to walls instead of remaining interfaces. It seems that although I have defined the interfaces as internals, they are somehow considered as walls. I can refine the mesh at those interfaces, but I don't think this problem has much to do with mesh refinement. As you can see i the first contours I attached in my question, the flow seems to crash a wall around the interface and it is not passing through the interface.
March 30, 2022 at 2:00 pmRoyaSubscriberDear Karthik When I want to change from mrf-to-sliding-mesh using the command line I mentioned earlier, should I first use this command line /define-mesh-interfaces/one-to-one-pairing? No, and then use the matching option in the mesh-interfaces section to run the sliding mesh successfully?
I used to change my simulation directly from MRF to SM, but in someone who works in the CFD field suggested me to first use the one-to-one-pairing-option and after that change from mrf to sliding mesh and activate the matching option.
What is your suggestion? I one-to-one-pairing necessary before changing from MRF to sliding mesh?
Kind regards Roya
March 30, 2022 at 2:14 pmRobAnsys EmployeeLooking at the mesh I'm surprised you need the matching option. Are the walls you're mentioning wall-12 or the like? If so they're part of the interface model and shouldn't do anything in your model.
March 30, 2022 at 2:27 pmRoyaSubscriberDear Rob The thing is that if I use the command line "mesh/modify-zones/mrf-to-sliding-mesh", then I have no problem regarding face-handedness. But if I use the steps that I have been said I need to use them, which are as followed; "A)Using one-to-one-pairing? No=>mrf-to-sliding-mesh=>activate matching option for interfaces", then I receive the face-handed warning every time-step.
So, do I need to use the one-to-one-pairing option? Or can I just change from MRF to SM directly?
Also, the discontinuity in the air volume fraction exists in both MRF and SM. Why is this happening?
These two seem two separate questions but they can still have something to do with each other! Since, if the solution is considering a wall a the interface, then the reason for why this discontinuity is happening becomes clear. But on the other hand, when I check the boundary condition of the interface in the MRF simulation, they are defined as internals and not walls! Which means there should be something wrong with mesh?
March 30, 2022 at 3:05 pmRobAnsys EmployeeThe left handed faces suggests the interior isn't splitting correctly, but I can't diagnose that easily. An old approach was to turn the interior into a wall, slit the wall & wall:shadow pair, turn those into interface zones and then create the nonconformal. With 2021 we brought in the "easier" interface set up, but that doesn't always work as it also hides a few other functions, check the user guide on Interfaces for a TUI command to turn it off.
The discontinuity could be mesh related, and I do wonder why the cell size is so small at the top of the mrf zone. Equally, convergence may be an issue, have you altered any of the UR, Courant number/time scale values?
March 30, 2022 at 3:30 pmRoyaSubscriberDear Rob Should I use one-to-one pairing and matching option every time I want to change my simulation from MRF to SM? Or should I do it only if there is a problem at the interface?
Also, you have asked: "and I do wonder why the cell size is so small at the top of the mrf zone", I just set the size at the top surface of mrf region smaller as it is close to the gas/liquid interface at the top pf the reactor. Do you think that might cause a problem?
Also, as for your last question, I haven't altered the URFs and also, as for this simulation which is MRF, I am running the case Pseudo-transient so I am not sure if Courant number is still valid?
The mass conservation seems to be acceptable in this case. Also, the residuals look like this by the end of the MRF simulation;
Kind regards Roya
March 30, 2022 at 4:05 pmRobAnsys EmployeeThe size isn't a problem but I'd probably have not included the free surface in the geometry & used a register to patch the liquid. The aim of simulation is to avoid messing another step of the model up by doing something earlier in the process: there's a reason we plan simulation runs.
Pseudo transient has a time scale factor, default is one.
The last sliding mesh case I ran I had to use matching but I used the TUI command to turn off the one-to-one pairing https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v221/en/flu_ug/flu_ug_sec_grid_nonconform.html
March 30, 2022 at 4:34 pmRoyaSubscriberDear Rob I am not modeling the interface through mesh. That volume in the middle that you see is a volume that I put there to actually get a better prediction of the vortexes at the top interface. I use adapt/patch to model the free surface at the top. But the top of my rotational region is close to the free surface, so I used a smaller grid size at that interface as well as defining a body of influence around the liquid/air free surface for capturing the top surface more accurately.
Also, as I was using the direct method of mrf-to-sliding mesh (without one to one pairing), I noticed that as I change my model from MRF to SM, some new walls are formed at the interface of rotational-stationary region. These walls do not appear in the list of the boundaries, but they appear in the list of the zones in the contour and mesh windows.
And if I plot these walls, they appear exactly to be at the interface of rotational-stationary region. Is this logical or is that a mistake? How can I fix this?
March 30, 2022 at 5:56 pmRoyaSubscriberEdit:
The walls I mentioned in the comment above only exist in the list. They can't be plotted. The picture given above is actually the interfaces, and not the newly created walls.
March 31, 2022 at 2:23 pmRobAnsys EmployeeThose walls are normal. In your case they shouldn't do anything, they're for cases where the interface surface pair don't fully overlap. Do you see that any other fields have a discontinuity at the interface surface?
Viewing 13 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- Floating point exception
- The solver failed with a non-zero exit code of : 2
- How to model free convection warming of liquid in a plastic bag
Top Rated Tags