Modify the Section Parameters

Define the section parameters for use with Simulation Composite Analysis.

When a *User Material definition is used, Abaqus cannot compute certain section parameters because the elastic constants necessary to compute these section parameters are not available. You must define these parameters for an analysis to run successfully.

Simulation Composite Analysis comes with the command line program xStiff that reads an Abaqus input file and automatically computes and inserts extraneous stiffness parameters required by reduced integration elements utilizing Simulation Composite Analysis materials. This auxiliary program significantly improves the speed and accuracy of the model building process.

  1. Locate the section definition by searching for *SolidSection.
  2. The section definition will look like this: 
    *SOLIDSECTION, ELSET=PLATE_LAYUP-1, COMPOSITE, ORIENTATION=ORI-1, STACKDIRECTION=3, LAYUP=PLATE_LAYUP
1., 1, EXAMPLEMATERIAL, 45., PLY-1
1., 1, EXAMPLEMATERIAL, 0., PLY-2
1., 1, EXAMPLEMATERIAL, -45., PLY-3
1., 1, EXAMPLEMATERIAL, 90., PLY-4
1., 1, EXAMPLEMATERIAL, 45., PLY-5
1., 1, EXAMPLEMATERIAL, 0., PLY-6
1., 1, EXAMPLEMATERIAL, -45., PLY-7
1., 1, EXAMPLEMATERIAL, 90., PLY-8
1., 1, EXAMPLEMATERIAL, 45., PLY-9
1., 1, EXAMPLEMATERIAL, 0., PLY-10
1., 1, EXAMPLEMATERIAL, -45., PLY-11
1., 1, EXAMPLEMATERIAL, 90., PLY-12
1., 1, EXAMPLEMATERIAL, 90., PLY-13
1., 1, EXAMPLEMATERIAL, -45., PLY-14
1., 1, EXAMPLEMATERIAL, 0., PLY-15
1., 1, EXAMPLEMATERIAL, 45., PLY-16
1., 1, EXAMPLEMATERIAL, 90., PLY-17
1., 1, EXAMPLEMATERIAL, -45., PLY-18
1., 1, EXAMPLEMATERIAL, 0., PLY-19
1., 1, EXAMPLEMATERIAL, 45., PLY-20
1., 1, EXAMPLEMATERIAL, 90., PLY-21
1., 1, EXAMPLEMATERIAL, -45., PLY-22
1., 1, EXAMPLEMATERIAL, 0., PLY-23
1., 1, EXAMPLEMATERIAL, 45., PLY-24
  3. Replace all instances of ExampleMaterial with the name of the Simulation Composite Analysis material created in the previous section.
  4. Save the input file.
  5. Open the Simulation Composite Analysis 2015 Command Shell and change the directory to the location where ASCA_Tutorial_2_Abaqus.inp is saved. 
    >>cd <directory containing input file>
  6. Issue the following command: 
    >>xstf /i ASCA_Tutorial_2_Abaqus
  7. The xStiff utility will copy the input file, calculate and insert all necessary extraneous stiffness parameters, and save the file as ASCA_Tutorial_2_Abaqus_xs.inp.
  8. Open the modified input file and locate the section definition. Verify that the *HourglassStiffness keyword was added to the end of the section definition.
Parent topic: Tutorial 2 - Modify an Abaqus Input File for use with Simulation Composite Analysis