Controlling beam profile display for postprocessing

Beam rendering is available in the Visualization module for undeformed, deformed, and contour plots only. For deformed plots Abaqus/CAE scales the displacement components of the deformation based on the deformed field output variable but does not scale the twisting of the beam profile using the rotational components of the deformation when you change the deformation scale factor.

You can view a realistic display of the beam profile for results data by selecting ViewODB Display Options in the Visualization module.

See Also
Producing a contour plot of linear beam section stresses
Controlling beam profile display

Context:

The rendering of beam profiles requires the presence of beam orientation data in the output database. Beam normals are written to the output database automatically for all the steps that include field output. For analyses that include geometric nonlinearity, you can display beam profiles during postprocessing only if nodal output is requested in the model. For more information, see Using a Beam Section Integrated during the Analysis to Define the Section Behavior.

Abaqus/CAE does not render the tapering of beam profiles along their length. If your model includes tapered beam sections, Abaqus/CAE renders these beams using the beam's starting profile along its entire length. For more information about tapered beams, see Creating beam sections.

Beam elements that have BRADIUS values are rendered using circular beam profiles with the radius coming from the BRADIUS field in the output database.

Displaying beam profiles is useful for checking that the correct profile has been assigned to a particular region and that the assigned beam orientation results in the expected orientation of the profile. For example, Figure 1 shows the box beam profiles displayed on the light-service crane described in Example: cargo crane.

Figure 1. The cargo crane example with beam profiles displayed.

Note:

If your results include quadratic beam elements, Abaqus/CAE does not consider the midside nodes in those elements when the beam profiles are rendered.

If you assign a general beam section to a wire, Abaqus/CAE displays the beam profile as an ellipse with a cross-sectional area and moments of inertia (I11 and I22) that match the values you specified. If you assign a truss section to a wire, Abaqus/CAE displays the truss profile as a circle with a cross-sectional area that matches the value you specified.

Abaqus/CAE renders beam profiles according to the current settings for color coding and translucency. When these settings change, the color and translucency of the beam profiles change as well. When beam profiles are displayed, Abaqus/CAE disables scaling and shrinking of the model.

  1. Locate the Render beam profiles option.

    From the main menu bar, select ViewODB Display Options. In the dialog box that appears, click the General tab.

  2. From the bottom of the dialog box, toggle on Render beam profiles to display beam profiles.
  3. If desired, apply a Scale factor to the beam profiles to increase or decrease their size. The default value is 1.
  4. Click OK to implement your changes and to close the dialog box.

    Abaqus/CAE displays the profile of the beam section with the appropriate dimensions and in the correct orientation. By default, your changes are saved for the duration of the session. If you want to retain the changes you applied for subsequent sessions, save them to a file. For more information, see Saving customizations for use in subsequent sessions.