5.8. Solid Model Loads

You can define loads directly on the solid model at any time before you actually initiate the solution. Thus, solid model loads may be defined before or after finite element meshing. (Details of how to define solid model loads are discussed in Loading in the Basic Analysis Guide.) The remainder of this section describes other functions related to solid model loads.

5.8.1. Transferring Solid Model Loads

Solid model loads will be transferred to the finite element model automatically when you begin the solution calculations (when you issue a SOLVE command (Main Menu> Solution> Solve> Current LS)), or you may transfer them "manually" using the following methods:

  • To transfer solid model loads and boundary conditions to the finite element model:

    Command(s): SBCTRAN
    GUI: Main Menu> Preprocessor> Loads> Define Loads> Operate> Transfer to FE> All Solid Lds
    Main Menu> Solution> Define Loads> Operate> Transfer to FE> All Solid Lds

  • To transfer solid model body force loads to the finite element model:

    Command(s): BFTRAN
    GUI: Main Menu> Preprocessor> Loads> Define Loads> Operate> Transfer to FE> Body Loads
    Main Menu> Solution> Define Loads> Operate> Transfer to FE> Body Loads

  • To transfer solid model DOF constraints to the finite element model:

    Command(s): DTRAN
    GUI: Main Menu> Preprocessor> Loads> Define Loads> Operate> Transfer to FE> Constraints
    Main Menu> Solution> Define Loads> Operate> Transfer to FE> Constraints

  • To transfer solid model forces to the finite element model:

    Command(s): FTRAN
    GUI: Main Menu> Preprocessor> Loads> Define Loads> Operate> Transfer to FE> Forces
    Main Menu> Solution> Define Loads> Operate> Transfer to FE> Forces

  • To transfer solid model surface loads to the finite element model:

    Command(s): SFTRAN
    GUI: Main Menu> Preprocessor> Loads> Define Loads> Operate> Transfer to FE> Surface Loads
    Main Menu> Solution> Define Loads> Operate> Transfer to FE> Surface Loads

5.8.2. Displaying Load Symbols

Solid model loads may be displayed at any time after you have turned on the appropriate load symbols:

  • To show boundary condition symbols on displays, use the /PBC command. This command includes an option to display boundary condition values, as well as symbols. (Turning off /VSCALE scaling before issuing the /PBC command may help.)

  • To show body force loads as contours on displays, use the /PBF command.

  • To show surface load symbols on model displays, use the /PSF command.

All of these commands can be accessed in the GUI by picking Utility Menu> PlotCtrls> Symbols.

5.8.3. Turning Off Large Symbols for Node and Keypoint Locations

Large symbols for node and keypoint locations are displayed by default (/PSYMB,DOT,1).

  • To display smaller symbols for node and keypoint locations, use one of the following methods:

    Command(s): /PSYMB,DOT,0
    GUI: Utility Menu> PlotCtrls> Symbols

5.8.4. Selecting a Format for the Graphical Display of Numbers

You can indicate the field length and the number of digits that are displayed for the numbers appearing on a model.

  • To specify a format for the display of numbers, use the following command:

    Command(s):

    /GFORMAT

5.8.5. Listing Solid Model Loads

You can list all solid model loads or you can list separate types of solid model loads using the following methods:

  • To list all solid model loads:

    Command(s): SBCLIST
    GUI: Utility Menu> List> Loads> Solid Model Loads

  • To list the body force loads at keypoints:

    Command(s): BFKLIST
    GUI: Utility Menu> List> Loads> Body> On All Keypoints
    Utility Menu> List> Loads> Body> On Picked KPs

  • To list the DOF constraints at keypoints:

    Command(s): DKLIST
    GUI: Utility Menu> List> Loads> DOF Constraints> On All Keypoints
    Utility Menu> List> Loads> DOF Constraints> On Picked KPs

  • To list the DOF constraints on a line:

    Command(s): DLLIST
    GUI: Utility Menu> List> Loads> DOF Constraints> On All Lines
    Utility Menu> List> Loads> DOF Constraints> On Picked Lines

  • To list the DOF constraints on an area:

    Command(s): DALIST
    GUI: Utility Menu> List> Loads> DOF Constraints> On All Areas
    Utility Menu> List> Loads> DOF Constraints> On Picked Areas

  • To list the forces at keypoints:

    Command(s): FKLIST
    GUI: Utility Menu> List> Loads> Forces> On All Keypoints
    Utility Menu> List> Loads> Forces> On Picked KPs

  • To list the surface loads on lines:

    Command(s): SFLLIST
    GUI: Utility Menu> List> Loads> Surface Loads> On All Lines
    Utility Menu> List> Loads> Surface Loads> On Picked Lines

  • To list the surface loads on areas:

    Command(s): SFALIST
    GUI: Utility Menu> List> Loads> Surface Loads> On All Areas
    Utility Menu> List> Loads> Surface Loads> On Picked Areas


Release 18.2 - © ANSYS, Inc. All rights reserved.