CFD rudder test

Discussion in 'Software' started by nico, Jun 9, 2003.

  1. nico
    Joined: Jan 2003
    Posts: 190
    Likes: 6, Points: 0, Legacy Rep: 52
    Location: SF

    nico Senior Member


    I am currently testing a rudder in a demo cfd package. I am new to CFD and very much still experimenting. I have some problems and questions:

    *what are the minimum cells number and maximum cells sizes for meaningfull results

    *what should be the computionnal domain

    * i have some problems with the forces output: the second one "viscous" looks fine but the first one called "pressure forces" gives big results too big almost 4 * viscous forces for 0° of attack what does pressure forces means here?

    *about the viscous models to be used?

    *and finally what should be the boundary conditions: i have looked at many tutorials and several ideas are seen:
    *Velocity inlet all around the model except at the back with an Outflow
    *Velocity inlet all around the model except at the back with an Pressure Oulet
    *Velocity inlet + Walls +an Outflow
    *Velocity inlet + Symetry +an Outflow (only for 0° attck)

    Thank u
  2. Dim
    Joined: May 2003
    Posts: 315
    Likes: 3, Points: 0, Legacy Rep: 114
    Location: somewhere

    Dim Senior Member

    CFD rudder test.

    Hi, Nico.

    I have transmitted your problem to the address
    The Russian team "Tesis" has developed the powerful program "Flowvision". They the experts in area CFD.
    Probably we soon shall meet their remarkable collective.
    They the participants of the project SeaLaunch:

  3. Dim
    Joined: May 2003
    Posts: 315
    Likes: 3, Points: 0, Legacy Rep: 114
    Location: somewhere

    Dim Senior Member


    I not seems could to you help. I do not like long to wait. My message to "Òesis" can has got in spam?
    Dim.:confused: :(
  4. Tim B
    Joined: Jan 2003
    Posts: 1,438
    Likes: 58, Points: 0, Legacy Rep: 841
    Location: Southern England

    Tim B Senior Member

    I don't know what method the software uses, nor what grid it works on. If I can download the demo, then I can take a good shot at answering your questions.

    In respect to the walls:

    If you specify a wall as an inlet, then it must have a velocity. What you are really looking for on most rudders is a large domain, at least 5 chord widths 'upwind' and 'downwind' of the quarter chord, and at least 3 above and below (assuming the rudder to be on it's side here) with the root of the rudder on a wall, and the tip of the rudder about 1/2 the rudder span from the opposite wall. Start, for now with a rectangular domain (length 10, width 1.5 * Span, depth 6) with your rudder flat (ie. like a wing) in the middle, on one wall. The 'upwind' wall should be an inlet, the downwind wall an outlet (with equal flow to the input, if not free to calculate pressure and flow).The wall adjacent to the root of the rudder acts as an 'endplate' (in aerodynanmic terms) or the hull (in boating terms), and so should be a standard wall with no slip. The three remaining walls should be free-slip walls (these do not restrict the flow). This should give fairly sensible results.

    Could you post a web address to download the software from?


    Tim B.

  5. tspeer
    Joined: Feb 2002
    Posts: 2,082
    Likes: 132, Points: 63, Legacy Rep: 1673
    Location: Port Gamble, Washington, USA

    tspeer Senior Member

    Is this 2D or 3D?

    If 2D, is your interest the code and the rudder is just a sample case, or is your interest the rudder? If your interest is the rudder section and not the code, I'd look into XFOIL as a way to get reliable data.

    I think you'd need to use the outflow BC, since you don't know the downstream pressure all across the wake.

    As for grid density, you're probably looking at 100 cells in each direction - say 300 x 100 cells in a C-grid to handle the section and a dozen chord lengths in all directions around it. At a bare minimum, you'll need 10 cells in the normal direction in the boundary layer. You need to run several grid densities, then plot the results vs 1/n. The intercept at 1/n=0 is your extrapolation of what the result would be if you had an infinite number of grid points.

    Here are some conclusions from:

    Rumsey, Christopher L., "Parametric Study of Grid Size, Time Step, and Turbulence Modelingon Navier-Stokes Computations Over Airfoils," AGARD Conference Proceedings No. 437 Validation of Computational Fluid Dynamics, May 1988.

    "The numerical study for the steady NACA 0012 airfoil case indicates the following:

    1. Lift is computed within 1 percent and drag to within 3 percent of its extrapolated value on an infinite mesh using tird-order spatial differencing on a 265x101 grid with an outer boundary extent of 15c.

    2. FVS and FDS yield identical results in the limit of infinite mesh size, but FDS is more accurate on a given mesh size."
Forum posts represent the experience, opinion, and view of individual users. Boat Design Net does not necessarily endorse nor share the view of each individual post.
When making potentially dangerous or financial decisions, always employ and consult appropriate professionals. Your circumstances or experience may be different.