Fluids

Fluids

Problem with convergence in ANSYS Fluent

    • riteshnw
      Subscriber
      Hello everyone.nI am doing a simulation on a real scale cuboidal building with small extrusion at the entrance (canopy) and it is inclined at 3 degrees. I performed the simulation in Ansys fluent and the simulation is not reaching at the convergence.nThe minimum element quality is 0.64, minimum orthogonal quality of mesh is 0.71 and max skewness is 0.55. I used the proximity size function and cutcell as assembly meshing and mesh seems to be good and there are about 3.76 million elements and 4.05 million nodes.nI am using standard k-epsilon turbulence model with inlet velocity as 12 m/s and outlet as pressure outlet. nI am using pressure-velocity coupling as SIMPLE and all the parameters of spatial discretization as first order upwind to initialize the solution. The URFs are default and I tried changing them to 0.2 for pressure and 0.5 for other parameters. I set the residuals at 1*10^-4 and initialize the solution from inlet and then started the steady state simulation.nI tried changing the URFs, orders of the simulations, initialization properties. But, I do not understand the problem why the simulation is not getting converged. The minimum residual value it reaches for continuity is 4.75*10^-2 and after that it changes the value around this value and residual plot stays stable.nCan anyone please help me?n
    • Karthik R
      Administrator
      Hello,nDid you create any monitors in your simulation (perhaps, the average velocity at the outlet or at any plane inside your computational domain)? How do they look like? Also, what is your overall mass balance?nSimulations in such large rooms are seldom steady. Because of the nature of the flow, it is possible that the flow is transient and that is why you are seeing this issue. nAlso, one suggestion - can you switch the solver to 'Coupled Pseudo-Transient' and try running your simulation? nWhat is the flow Reynolds number at the inlet?nKarthikn
    • riteshnw
      Subscriber
      Dear Karthik,nThank you for your response.nNo. I have not created any other monitors except the monitors for residual. Do you think I should use them? What can be the significance of using them?nI did not understand why can it be possible to have a transient behavior.nSince my building is fixed and only the air is moving around the building, it can be possible that flow remains steady.nI want to do the simulation outside the building and I have large domain (635.4 m X 425.62 m X247.5 m)nI did not understand the reason behind using coupled pseudo-transient solver. Why I am asking this because if I am using Coupled solver, then I have to enter courant number value which includes the time-step and it is for transient simulation.nCan you please elaborate that?n
    • Karthik R
      Administrator
      Hi, nDepending on the air flow, there might be recirculating regions and separation bubbles inside the room. This was why I was thinking it may be a transient problem.nHaving said that, you should most definitely use monitors to see how the overall flow behavior is. Also, do check the mass balance. nRegarding the Coupled solver, you are not solving a transient problem. The Courant number and pseudo-transient is just a different under-relaxation. This is the default setting in the recent Fluent releases for pressure-based solvers and I just wanted to see if it benefits your simulation.nKarthikn
    • riteshnw
      Subscriber
      Hi Karthik,nThank you.nI will try the simulation using the monitors plot for mass imbalance, average pressure and average velocity and I will let you know the results.nI hope it will work.nnRiteshn
    • Karthik R
      Administrator
      Sure thing !!n
    • riteshnw
      Subscriber
      Dear Karthik,nI performed the si,ulation. I started the simulation with first order upwind and when the residuals and other monitor parameters were stable, I continued with second order upwind and after that I reduced the URFs.nThe mass flow rate and mass imbalance seemed constant throughout the simulation bu there were some up and down variations in avg. pressure and avg. velocity.nPlease find the images in attachment and let me know if they can be considered as good solution.nThank you in advance.nnRiteshnn
    • Karthik R
      Administrator
      Hello,nI'm not able to download any attachments from your post. Could you please insert them directly into your post? You can use the upload image option at the bottom.nWhat near wall model are you using? And what is your y+ value?nAlso, what is the final goal of your simulation?nKarthikn
    • riteshnw
      Subscriber
      Hi Karthik,nI used standard k-epsilon turbulence model. I did not considered the y+ value for my simulation.nMy goal is to see the air displacement behavior around the building with and without the surrounding buildings and then to proceed further.nn
    • Rob
      Ansys Employee
      For urban models monitor velocity on a number of points in the area(s) of interest to look for how (un)stable they are. Plotting a contour of velocity every 10-20 iterations is also recommended to see how the air flow behaves. nThe residuals plot looks about normal for urban flows: they never converge like in the text books! n
    • Karthik R
      Administrator
      Hi,nHave a look at this simulation example. It is very similar to the problem you are attempting to solve.nKarthikn
    • riteshnw
      Subscriber
      Dear Rob and Karthik,nThank you for your responses.nI will proceed further as you have suggested.nnRiteshn
    • DrAmine
      Ansys Employee
      Good luck.nnGlobal scaled residuals might sometimes be irritating.
    • DrAmine
      Ansys Employee
      And do your urban simulation a favor and use a new version
    • riteshnw
      Subscriber
      Yesn
Viewing 14 reply threads
  • You must be logged in to reply to this topic.