Find answers, ask questions, and connect with our <br>community around the world.

Home Forums ANSYS Fluent Beginners to Advanced level Lesson 11 Flow over cylinder

  • Lesson 11 Flow over cylinder

    Posted by Raghu Karthik on November 18, 2023 at 1:26 pm

    Hi ,
    I am trying flow over cylinder with fluent with fluent meshing. Given problem : water flows over 1m dia. cylinder at 50 m/s. Meshing consists of 2 zones one is the larger enclosure for setting up the flow domain and the other surrounded closer to cylinder for local sizing (i used 0.05 m, 0.1 m, 0.2 m); Mesh : polyhedra; Solver : SIMPLE solver with PRESTO! for pressure (Second order is not working for any mesh size). Minimum orthogonal quality in all cases is more than 0.4. and average is more than 0.98. The residuals are always diverging for the case of 0.05 and correspondingly TVR (turbulent viscosity ratio) is crossing the limit 1.0e5 for far too many cells in the entire downstream behind the cylinder. Next for 0.1 the residuals are converging but they look like a ball bouncing on a staircase and correspondingly the TVR crosses 1.0e5 for just behind the cylinder but not as worse as that of case 0.05 local sizing. At last, for 0.2 the residuals are converging in a straight forward way but the obvious concern would be the sizing 0.2 would not naturally describe the geometry to an appropriate resolution! but it converges. Also i tried adding and decreasing the number of boundary layers it did not effect the convergence. I tried a lot to understand but now i need help.

    The attached images are for reference (case 0.1 local sizing for cylinder region).

    Rahul replied 4 months, 4 weeks ago 2 Members · 3 Replies
  • 3 Replies
  • Rahul

    Member
    November 18, 2023 at 7:09 pm

    Hi Raghu,
    1. It seems you are modelling with a very high Reynolds number of 4.9e7. Please try the case with a lower Re of around 5000 first with an appropriate turbulence model like SST kw and run the case.
    2. Also, the way in which the body of influence(BOI) for the mesh is taken needs to be changed. Generally mesh refinement is done for a longer distance on the downstream side. You should consider taking the BOI as a cuboid as marked in the attached figure and check the case.
    3. Also, please make sure you have selected the domain size such that there is at least 10 times the diameter on the downstream side of the cylinder.
    Best regards
    Rahul
    Flowthermolab support

  • Raghu Karthik

    Member
    November 20, 2023 at 11:41 am

    Hi,

    Further doubts:

    I tried all, but i think i didn’t use proper inflation layers. The first cell thickness is around 0.015 mm for a y+ of 5 and the body is 1 m, I am afraid its too small to mesh. With the improper inflation layers that I have used until now (the one that doesn’t resolve boundary layer) I made an animation of Turbulent viscosity ratio which seems to start at a point closer downstream to top and bottom most points of the cylinder and slowly move into the bulk and increases gradually over iterations until it crosses the limit 1.0e5 . I am also thinking that if the viscous region near wall is not resolved and the first cell is too far away from the wall which leads to overprediction of velocity gradients near the wall and hence an over prediction of wall shear stress which implies over predicted wall yplus value (from y+ formula). Likewise due to high velocity gradient we can assume over predicted velocity near wall which implies over predicted turbulent kinetic energy and hence turbulent viscosity ratio. and this effects the flow downstream and ansys is throwing a warning message turbulent viscosity ratio exceeded the limit 1e5. But somehow this is not a problem with 0.2m sized mesh it converged way beyond 1e-6 in all residual parameters. So should i consider using very small inflation layers (in that case how do i deal with aspect ratio : it leads to too many cells to bring down aspect ratio of these cells.) (or) Since the velocity is 50 m/s i will straight way implement slip condition at cylinder to study character of pressure drag alone.
    A reference would also be of extra help!!!

    Thank you,

    karthik

    • Rahul

      Member
      November 20, 2023 at 12:29 pm

      Hi Karthik,
      Coarser meshes will normally give results with lower residuals but will not be able to capture the flow physics accurately. Please check the range of wall y+ obtained in Fluent after the simulation in the results panel for the 1st cell height you are using.
      I think you are running a 3D model for this case. Then it will be difficult to resolve the domain properly as you are using Ansys Student version and have a mesh size limit. Also, drastically increasing the mesh size will only increase the required computational power.
      I suggest you to try doing a 2D simulation for the same. In that case, you can use a finer mesh and try to obtain the desired wall Y+. The 1st wall thickness for the diameter and velocity you have mentioned seems to be actually lower than the value you mentioned. That is why I suggested to try with a lower Re, so that you can use a mesh with a bigger 1st cell height (For example for Re=5000, you need a first cell height of only 10mm approx. to get wall y+ <5).
      Also, there are lot of reference papers related to flow past a cylinder, both CFD and experimental, which can be obtained by a simple Google search for the Reynolds number and conditions of your choice. Please take a look to get an understanding of the domain sizes, boundary conditions and computational models used.
      Also please use the mesh refinement as I mentioned in the previous post for better results instead of a circular one, since downstream flow physics can only be captured only with a finer mesh in that region.
      Best regards
      Rahul

Log in to reply.

error: Content is protected !!