Fluids

Fluids

Fluid-structure interaction problem: sudden jump in pressure & flow

    • jfonken
      Subscriber

      Hi all,

      For my PhD project, I'm working on fluid-structure interaction (FSI) models of abdominal aortic aneurysms (AAA) using Ansys Mechanical APDL, Fluent and System Coupling (version 2020R1). I've been able to simulate quite a few FSI models, but I'm facing problems with a subset of models. The flow and pressure at the inlet and outlet of the model are written to a text file. If I plot the flow for a successful model, I get something that looks like this:

      Flow - successful model

    • YasserSelima
      Subscriber
      Numerically, there are many reasons that could cause this jump in the pressure. The most common one I know is not deeply converged solution. I would suggest repeating the same simulation, using tighter convergence criteria and increasing the maximum number of iterations per time step. Then you can see if the jump disappears or notn
    • Stephen Orlando
      Ansys Employee
      Hi Judith,nLooks like you're getting good results so far! What are the setup differences between the successful and unsuccessful runs? I'm not really familiar with the windkessel model, but if that's driving the boundary conditions, maybe that's the source of the problem. I think you'll just have to take a very close look at the convergence and results near the anomaly to find the source of the problem.nSteven
    • jfonken
      Subscriber
      Hi Yasser and Steve,nThanks for your input and suggestions! Sorry for my delayed replay, my model needed some time to run with tighter convergence criteria. Unfortunately, this didn't solve the problem. There aren't any (major) setup differences between the successful and unsuccessful runs. However, the mesh is different and therefore, the Windkessel parameters are different. The parameters are calculated in a same way and the mesh is created in a similar way as well. In my study, I run 2 FSI models for each patient. In one model, the pre-stress that's present in the geometry is estimated. In the other model, the pre-stress estimation is omitted. For the same patient, the model with pre-stress estimation runs fine (pressure and flow plots shown below). However, the model without pre-stress shows the sudden jump in flow, as shown above. In this model, the systolic pressure in the first cardiac cycle is fairly high and the diastolic pressure in the first cardiac cycle is fairly low, since a periodic solution hasn't been reached yet, due to high displacements at the start of the FSI simulation. I tried lowering the stiffness of the wall, but this hasn't solved my problem either. I'm now thinking about trying the following:nRun the simulation with a stiffer wallnRun the simulation with a higher Windkessel compliance, such that the pressure is decreasednHopefully, one of these simulations works well, such that I at least know what is causing this problem. Ofcourse, I'm also going to have another look at the convergence and results near the anomaly. I didn't find anything weird so far, but maybe a fresh look will make things clear nIf you have any further suggestions, I'm more than happy to hear!nBest regards,nJudithnModel with pre-stress estimation - Pressure nModel with pre-stress estimation - Flownn
    • jfonken
      Subscriber
      Hi Yasser and Steve,nThanks for your input and suggestions! Sorry for my delayed replay, my model needed some time to run with tighter convergence criteria. Unfortunately, this didn't solve the problem. There aren't any (major) setup differences between the successful and unsuccessful runs. However, the mesh is different and therefore, the Windkessel parameters are different. The parameters are calculated in a same way and the mesh is created in a similar way as well. In my study, I run 2 FSI models for each patient. In one model, the pre-stress that's present in the geometry is estimated. In the other model, the pre-stress estimation is omitted. For the same patient, the model with pre-stress estimation runs fine (pressure and flow plots shown below). However, the model without pre-stress shows the sudden jump in flow, as shown above. In this model, the systolic pressure in the first cardiac cycle is fairly high and the diastolic pressure in the first cardiac cycle is fairly low, since a periodic solution hasn't been reached yet, due to high displacements at the start of the FSI simulation. I tried lowering the stiffness of the wall, but this hasn't solved my problem either. I'm now thinking about trying the following:nRun the simulation with a stiffer wallnRun the simulation with a higher Windkessel compliance, such that the pulse pressure is decreasednHopefully, one of these simulations works well, such that I at least know what is causing this problem. Ofcourse, I'm also going to have another look at the convergence and results near the anomaly. I didn't find anything weird so far, but maybe a fresh look will make things clear nIf you have any further suggestions, I'm more than happy to hear!nBest regards,nJudithnModel with pre-stress estimation - PressurenModel with pre-stress estimation - Flownn
    • YasserSelima
      Subscriber
      Can you try to stop the simulation before this peak, and go through it by an order of magnitude smaller time step?n
    • jfonken
      Subscriber

      Can you try to stop the simulation before this peak, and go through it by an order of magnitude smaller time step?https://forum.ansys.com/discussion/comment/109973#Comment_109973

      Yes, I'll try that as well!n
    • jfonken
      Subscriber
      When further looking into the Fluent output, I noticed that the mesh is remeshed in the first iteration of the timestep in which the sudden jump in flow occurs. The output looks like:nThe part indicated in red is a part that I haven't seen before. Taking a closer look at my remeshing parameters, I saw that I didn't enable regional remeshing. I think this causes the cell skew after remeshing to be higher than the maximum cell skew specified (0.8, see below). nI also saw that there's an option to adjust the maximum skewness for the smoothing algorithm. The same part of my journal with the regional remeshing and the maximum skewness for the smoothing algorithm now looks like:nI think this may resolve my problem in this simulation, but I'm curious about your ideas!nBest regards,nJudithn
    • YasserSelima
      Subscriber
      If you have dynamic mesh, re-meshing is a normal procedure when the mesh meets the criteria of remeshing. Partitioning is re-dividing the cells on the nodes. This happens when the number of cells changes dramatically in one or more partition after remeshing. nHow can this affect the solution ? I don't actually know ... but this supports using smaller time step during this period.nMost Probably can read something from this log file.n
    • jfonken
      Subscriber
      The simulation with the new remeshing parameters executed successfully, so I've found the source and solution of my problem! Thank you all for your suggestions!n
    • Stephen Orlando
      Ansys Employee
      Good to hear! One other note. I noticed in one of the videos that the domain doesn't move very much. If the displacements are small relative to size of the domain, then remeshing shouldn't be needed, only smoothing.n
    • jfonken
      Subscriber

      Good to hear! One other note. I noticed in one of the videos that the domain doesn't move very much. If the displacements are small relative to size of the domain, then remeshing shouldn't be needed, only smoothing.https://forum.ansys.com/discussion/comment/110594#Comment_110594

      It's indeed true that the displacements in the video are quite small. However, I only made a video of the last cardiac cycle. In the first cardiac cycle, the highest mesh displacements are found. I think these displacements caused the mesh to become too skewed, which explains the crash of the simulation in a later stage. n
Viewing 11 reply threads
  • You must be logged in to reply to this topic.