Fluids

Fluids

Face ID xxxxxx out of declared range

    • mashimaro_star
      Subscriber

      This is recently happened. When I reopen a Fluent case (which I can open using tecplot without any problem), Fluent gives me error:


      "Face ID 3790811 out of declared range (1<=id<=3681795)".


      I use double precision and 32 processors to calculate the case.  The mesh was generated using Fluent Meshing.


       


      Is there any specific way to solve this problem? 

    • Keyur Kanade
      Ansys Employee

      Hi, 


      Can you open that file in Fluent Meshing?


      Once open in Fluent Meshing, can you please check the mesh using Mesh --> Check. 


      Also check the quality of the mesh. 


      If everything is ok they you can switch Fluent Meshing to Fluent mode by GUI or TUI option. 


      Regards,


      Keyur

    • mashimaro_star
      Subscriber

      Hi Keyur,


      Thank you for the prompt reply. Yes I can open it in Fluen Meshing. The problem is that I can read the mesh using Fluent, perform computation, then save dat and cas. However, if I close the case and want to reopen the case using Fluent, it returns the error I mentioned in the original post. 


      The "check" and "check the quality" reports are as follows. Could you please see if there is anything I can do? I do not want to read the mesh every time and then read the journal file to recover the case setup... Thank you very much. 


      Domain extents.


      x-coordinate: min = -7.617500e-02, max = 7.110600e-02.


      y-coordinate: min = -2.358700e-02, max = 4.558700e-02.


      z-coordinate: min = -1.885470e-01, max = 1.561000e-03.


      Volume statistics.


      minimum volume: 1.747063e-13.


      maximum volume: 2.587584e-10.


      total volume: 4.123249e-05.


      Face area statistics.


      minimum face area: 2.478286e-09.


      maximum face area: 8.736383e-07.


      average face area: 1.365562e-07.


      Checking number of nodes per edge.


      Checking number of nodes per face.


      Checking number of nodes per cell.


      Checking number of faces/neighbors per cell.


      Checking cell faces/neighbors.


      Checking isolated cells.


      Checking face handedness.


      Checking periodic face pairs.


      Checking face children.


      Checking face zone boundary conditions.


      Checking for invalid node coordinates.


      Checking poly cells.


       


      Done.


       


      Minimum Orthogonal Quality = 3.00263e-01


      (To improve Orthogonal quality , use "Inverse Orthogonal Quality",


      where Inverse Orthogonal Quality = 1 - Orthogonal Quality)


       


       


      Maximum Aspect Ratio = 1.62759e+01

    • Rob
      Ansys Employee

      How did you transfer the mesh from Fluent Meshing to Fluent?  The mesh check there looks to have passed, but I suspect the cell ID's will be different to you'll not be able read the existing data back onto the mesh. 


      Can you open the old case in serial on a machine? Also does the error stop you working, or can you continue? 

    • mashimaro_star
      Subscriber

      Thank you very much for your suggestions. Serial mode can open the old case file. 


      For the parallel mode, even I use the same number of processors after and before the simulation, it returns the error. The error stop me from working...


      Is there anyway that I can solve this problem? Thank you very much. 

    • Rob
      Ansys Employee

      Excellent news. 


      OK, open in serial then read in the data & save both with a new name. Partition to 32 nodes manually and resave both (new name again). Re-try in parallel. 


      I've seen it before and the above usually fixes it: it's actually possible sometimes to read into serial, save and then read into parallel but the extra step eliminates other problems. Using a different name is an additional safety step: I don't trust computers not to eat my work!  

    • mashimaro_star
      Subscriber

      Thank you very much! Problem solved! 

Viewing 6 reply threads
  • You must be logged in to reply to this topic.