October 28, 2020 at 7:54 amjfonkenSubscriber
I experience a problem with my pressure-outlet boundary conditions when executing FSI with Ansys Fluent and Ansys Mechanical APDL. I'm modeling an abdominal aortic aneurysm including the aorto-illiac bifurcation. At both outlets (called LCI and RCI), I'm applying a pressure-outlet boundary condition. After each time step, the boundary pressure for the next time step is calculated using a Windkessel model and a 'define_execute_at_end' UDF. At each iteration, I'm using a 'define_profile' UDF to couple the calculated pressure to the right boundary. One pressure is calculated for the entire outlet (since the pressure is based on the flow through the surface).
When I use these UDFs and monitor the pressure in a Fluent-only (rigid mesh) model, the pressures behave as expected. The pressure for all iterations within one timestep is the same and corresponds to the results visualized in CFDpost (see figure below). The pressure is constant along the entire outlet, with only small differences at the borders.October 28, 2020 at 12:56 pmDrAmineAnsys EmployeeA thought: Within a coupling iteration Mechanical and Fluent will exchange the information. Fluent will not only run say 5 iteration per time steps but 5 iterations for the time step per coupling iteration. DEFINE_PROFILE is executed may times at time step even before the time steps starts. I would rather use a DEFINE_ADJUST which gets executed every iteration and to check whether at the end of the time step the pressure prescribed corresponds to the pressure received and reported in Fluent. It might be possible too that one would require more iteration per time steps so that things stabilizes.
October 29, 2020 at 8:27 amjfonkenSubscriberHi Amine Thanks for your suggestion! I started to use the DEFINE_ADJUST function to output the current pressure at each face at the LCI and RCI outlet boundaries, such that I could compare the current and prescribed pressures. I would expect that the current pressure corresponds to the prescribed pressure, since the DEFINE_PROFILE is executed before DEFINE_ADJUST. However, this is not the case for my model, as also seen in the figure in my first post.
If I understand you correctly, you suggest that I use DEFINE_ADJUST to adjust the pressure at the boundary faces instead of using DEFINE_PROFILE?
October 29, 2020 at 12:46 pmJeroenFeherAnsys EmployeeHi there. I'd like to chime in on this as well. The define profile is (almost always) required to prescribe your pressure. I think what was suggested by DrAmine is to define a variable which you update, either using your define_execute_at_end or your define_adjust. Then that variable is used in your define_profile. From what I understood, you are already doing this , but using a define_execute_at_end but it will allow you exact control on what's being prescribed.
However, this brings me to point 2, namely the results from those figures. Let's start with the second figure. I can see you have backflow on 100% of your outlet surface in this case. What is the backflow specification you have there? The equations used for generic windkessel models provide you with a static pressure and prescribing total pressure during backflow is incorrect.
You mentioned you have outlets which are free to move in radial direction. When your vessel expands or contracts, you will have fluid movement at the wall, in radial direction, but not necessarily at the center of your vessel. In fact if the vessel is perfectly symetrical there is no radial velocity at the exact center. So basically a pressure gradient should exist in radial direction or you would have no radial velocity and no movement of the wall. However, I'm not sure what magnitude that gradient should be.
October 29, 2020 at 1:58 pmDrAmineAnsys EmployeeHello: yesis correct. Reversal flow might spoil the strategy. I did not say that the ADJUST will be used to setup the pressure at the boundary but to get the right pressure which should be then applied via the DEFINE_PROFILE.
So back to the reversal flow: bear in mind that if back-flow occurs the pressure you are prescribing will be (in general) interpreted as stagnation pressure (total pressure).
October 29, 2020 at 3:01 pmjfonkenSubscriberThat worked Jeroen, thanks!!
Viewing 5 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
- The solver failed with a non-zero exit code of : 2
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.