Fluids

Fluids

Topics related to Fluent, CFX, Turbogrid and more.

Non-Convex Cells in ANSYS Forte

    • Usman
      Subscriber

      Dear Team,

      I hope this message finds you well. I created a 1/7th sector mesh of a diesel engine using automatic mesh generator in FORTE (Please see following figure).

      However, while running simulations it gives the following errors:

      Could you please provide any suggestions on how to avoid this error? Your suggestions will be highly appreciated.

      Many thanks!

    • losinyao181031
      Subscriber

      I am working on this too, and I met the same problem, 

      sent message to me, i can try to help 

      losinyao181031@gmail.com

    • jcooper
      Ansys Employee

      Hi:

       

      COnvex cells are when the mesh folds on itself during motion.  This can happen when elements are too small for compression.

      The appearance of your mesh suggests that the control point 3 and maybe 5 may be placed incorrectly, or that there are not enough nodes between 2 and 3.  I would check all the mesh settings and try to obtain an appearance similar to the template image below.

       

       

    • Usman
      Subscriber

      Could you please recommend a value for the central points? The sector angle is 360/7 degrees. The bore and stroke sizes are 11.5cm and 12.5cm. Also, can I import a sector mesh from Solidworks? As, it is easy to create a geometry there. I would mesh it in the forte. I tried importing STL files from Solidworks, but this does not allow me to do name selections. I tried to provide name selection in Forte but I could not find any option to do so. 

      Your suggestions will be highly appreciated. 

      Many thanks!

    • jcooper
      Ansys Employee

      Control point 3 should be placed just above the bulge, where the bowl profile starts  (sorry, I can't  recommend a value, as I am unfamiliar with the geometry, but the node bunching looks wrong, like everything is pulled upwards.)  It could be that your bowl profile includes part of the vertical section above the bowl.

      For alternate imports, you could try importing surfaces from a Fluent tet mesh file.  

      Named Selections cannot be imported directly from STL files modified in SpaceClaim into Forte. This information is only stored in SpaceClaim's .scdoc files, which are not currently supported by Forte. 

      To retain Named Selections in Forte, one send the SpaceClaim geometry to ANSYS Meshing, mesh with tets and then export the resulting mesh as a Fluent .msh file. This can then be imported into Forte, which will remesh the interior

       

       

       

       

    • Usman
      Subscriber

      Dear,

      Thank you for your reply. I do not know how to estimate central point values. Is there any tutorial on it?

      I imported the .msh file into Forte. It worked fine at the beginning; however, at the time of injection, simulations stopped (the Error was "Time step driven too small"). Also, sometimes, simulations do not stop; however, the nozzle does not inject fuel, although I have set up fuel injection properly.

    • jcooper
      Ansys Employee

       

       

       

      Control points are specified as fractional length along the bowl profile.  This can be hard to estimate visually, as the bowl profile is not straight. The bowl profile extends all the way from almost the outer radius of the geometry to the inner radius, or 0.0:

      Looking at your mesh above, it looks like control point 5 should be set at 0.8 rather than 0.9.  You can try moving control point 3 to 0.36-0.4 and Control Point 2 to 0.3.  Your mesh should end up looking like the template above with no sudden bunching of nodes or change in cell size.  You want a nice, uniform element distribution so that the mesh can compress without folding them.  If elements are too small because of poor bunching, there is a risk of premature folding during mesh motion. ie: mesh folds before remesh can correct the problem.  This can also lead to small timesteps.

      This may not be the cause of the spray issue, however.  If spray is not entering the domain when it should, it is possible that the Start point of the injection is set wrong.  Make sure that the Timing is set to Crank Angle ans that the Start of the injection is set relative to ATDC with correct duration and mass.  

      The timestep problem can also be due to overly tight controls on Chemistry convergence.  You can reduce your absolute tolerance for Chemistry solver to 1.0e-08 if problems persist:

       

       

       

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