Fluids

Fluids

Adaptive time step

    • michutorres
      Subscriber
      Hi all,nI made a fixed time step to get the convergence with time step =0.01 and 25 iterations per step. Then someone recommend me to use adaptive time step to let the software decide. How can I do this? It is inviable to continue with ime step =0.01 and 25 iterations per step as I need to simulate 30 minutes (1800 seconds) of real life.nThank youn
    • Karthik R
      Administrator
      Hi, nIn the run calculation, change the Time Advancement type from Fixed to Adaptive. This should enable Adaptive time step. The default is CFL-Based. If you wish to read more into this, please use this Users Guide link below.nKarthikn
    • michutorres
      Subscriber
      ok, but before clicking on calculate, which parameters should I put in Courant Number, Initial Time Step and max iterations?nn
    • ai0013
      Subscriber
      It depends on your flow characteristics. nTypically an accurate solution requires a CFL = 1 (For explicit treatment). This will assure that your flow doesn't travel more than one cell per time step. However in implicit treatment, people often can raise this number to 5-20 (or even higher) at the expense of loss in accuracy. If you can afford running this condition, it will be optimal, nIf you do LES you should decrease this number to 0.5 (or even lower)nn
    • michutorres
      Subscriber
      Where can I set the CFL=1? Is this the Courant Number?.
    • DrAmine
      Ansys Employee
      That is the Global Courant Number calculated in the interfacial cells. For implicit runs you can try have it lower than 5-20.n
    • michutorres
      Subscriber
      Ok Thank you.nHow can I interpret the following adaptive step method?nFluent will start doing 5 iterations per time beginning with 0.1 seconds time step and then automatically Fluent will adapt these two parameters to make a quicker and accurate simulation?nn
    • DrAmine
      Ansys Employee
      It will adapt it based on the adatipve method used and whether you are running multiphase or not.nFor single phase we have at least two way: truncation error based and CFL based. For the user friendly CFL based, Fluent will try to update the time steps based on your settings to increase the time step size or reduce it so that CFL criterion is matched as much as possible.nnYour description is correct. n
    • michutorres
      Subscriber
      I didn't enable multiphase model. nI enabled solidification&melting, viscous laminar and energy on.nI have a single phase. I am using CFL.nSomeone from this forum told me that firstly I need to get the convergence with fixed step and then turn to adaptive step. But then I don't know if between this change I should initilize and set the adaptive step as in the fixed method or I should continue with the calculation without initilizing another time.nn
    • DrAmine
      Ansys Employee
      You can restart with clean initialization and use that adaptive time stepping. I usually do not use it for single phase runs but that is a personal preference. It is not bad.n
    • michutorres
      Subscriber
      I am running the simulation and I think now it's ok and in few hours I could have the simulation finished.nnNow the temperatures of the internal faces of the deposit are increasing correctly. But the problem now is that the temperature of a point in the adhesive is not increasing correctly. I checked the properties of my adhesive and are ok. Maybe there is a problem with the interface between the deposit and the adhesive, or maybe it's a problem with the physics of Fluent... What do you think?n
    • DrAmine
      Ansys Employee
      You can check the heat balance at that interface if it is physical + double checking material properties + check your mesh quality and consider convergence every time step. I am sure that Fluent can handle this kind of problems in very accurate way.n
    • michutorres
      Subscriber
      ok. How can I check the heat balance at that interface? That has to be checked at the end of the simulation or I can print to console like residuals?nBy the way, I won't be capable to interpret if the heat balance in that itnerface is correct or not.n
    • DrAmine
      Ansys Employee
      As flux report or as Report definition.n
    • michutorres
      Subscriber
      My heat flux is 79000 W/m2. Now that I am going to check the heat balance at the interface between the deposit and adhesive making a report definition, which should be the heat interface value?n
    • Karthik R
      Administrator
      Hi,nWhat means is - please check if you are conserving your total heat. Check if the energy is conserved. If it is not, then your solution is not correct and you will need to properly converge your model.nKarthikn
    • michutorres
      Subscriber
      Hi,nnow I am going to refine my mesh as someone told me that mesh quality skewness should be under 0.8 and orthogonality mesh quality should be higher than at least 0.15.nI clicked on Metrics Display and I can only see a graphic like below. Where can I check the exact value to see if my skewness is under 0.8 and orthogonality over 0.15?nn
    • DrAmine
      Ansys Employee
      You can limit the graph and then click on the pivot / pillar to highlight the cells. However I recommend doing that in Fluent and rely on Fluent metrics.n
    • michutorres
      Subscriber
      How can I do this in Fluent? Where is the option Fluent metrics?n
    • Karthik R
      Administrator
      Hi,nYou won't get a histogram plot like this in Fluent (not unless you are using Fluent Meshing). If you are working with Ansys Meshing, it is better you do this there. In Fluent, you will only be able to print the values of your mesh quality or plot a contour of your mesh metric. Look under Contour -> Mesh -> Orthogonal Quality and see if this helps.nKarthikn
    • DrAmine
      Ansys Employee
      In Fluent you rely on iso-surface or cell registers to show the cell with certain quality range. No histogram like in Ansys Meshing.n
Viewing 20 reply threads
  • You must be logged in to reply to this topic.