I-Beam Analysis

Step through the model build process for a composite I-beam model.

Interface laminates and sublaminates will be demonstrated. You should complete the Composite Analysis tutorial first. The steps required to define a ply-based laminate on complex geometry with T connections include:
  • Ply creation
  • Set ply normals
  • Sublaminate creation
  • Interface laminate creation
  • Template property creation
The analysis model includes:
  • Surface geometry and mesh of I-beam
  • Orthotropic material
  • System collector that contains system used to assign material direction
  • Unit system is PSI
  • The manufacturing process uses complex tooling to manufacture 4 sublaminates (co-cured to form the final part):
    • top cap on Tool 1
    • bottom cap on Tool 4
    • left web on Tool 2
    • right web on Tool 3

Figure 1.

Figure 2.


Prepare the HyperMesh environment for the tutorial.
  1. Open HyperWorks.
  2. In the Solver Interface dialog, set the profile to OptiStruct.
  3. Open the model file, composite_beam.hm.
  4. Open the Composite Browser by clicking the Composite tool in the Model ribbon or View > Browsers > HyperMesh > Composite.

Review Stacking Direction and Element Normals

Review stacking direction and element normals.

  1. Open the composites panel by clicking 2D > composites > element normals.
  2. Toggle from color display to vector display and click display. This will display the current element normals for displayed 2D elements.
    Note: For typical ply-based models with T junctions, cap element normals should point away from the web. Web element normals are arbitrary as long as the direction is consistent. Confirm that the element normals of the cap elements point away from the web and that web element normals point in the direction of global y.

    Figure 3.

Review Material Reference Orientation

Review the assigned material reference orientation.

  1. Open the composites panel by clicking 2D > composites > material orientation.
  2. Select the component on which material orientation will be reviewed by setting the middle top collector to comps and then selecting the ibeam component.
  3. Click review to plot the current material orientation. The material orientation for this part has already been defined as the x direction of the local system with id = 1.

    Figure 4.

Create Plies

Create the plies that make up the composite laminate.

  1. In the Composite Browser, create shapes and plies from the white space context menu using the following steps.
  2. Create the shapes according to the table and image below. Each shape should be the full length of the beam. By Face is a convenient method for selection.
  3. Create the plies according to the table below. Note that after one ply has been created, Duplicate is available from the context menu and can quickly generate the other plies. Only orientation and shape need to be entered.
  4. After all plies are created, auto color by Shift-selecting the plies in the browser, selecting one the Color icons, and clicking Auto color.
    Ply Name Ply ID Material Thickness Orientation Shape
    ply1 1 M40J 0.01 90 Top_cap
    ply2 2 M40J 0.01 0 Top_cap
    ply3 3 M40J 0.01 45 Left_web
    ply4 4 M40J 0.01 -45 Left_web
    ply5 5 M40J 0.01 90 Center_web
    ply6 6 M40J 0.01 45 Right_web
    ply7 7 M40J 0.01 -45 Right_web
    ply8 8 M40J 0.01 0 Bottom_cap
    ply9 9 M40J 0.01 90 Bottom_cap
    Figure 5.

    Figure 6.

Set Ply Normals

Correct ply normals.

In models with T junctions that are modeled using a ply-based method, plies on each side of the web will have opposite stacking directions. On one side, the element stacking direction will be consistent with the cap, and on the other side it will not. See the image below.

Figure 7.
The discontinuity in stacking direction on the left side of the I-beam model will be corrected using ply normals. Ply normals manipulate the direction that an individual ply stacks.
Note: When ply normals are changed, a DRAPE table is created and assigned to the ply.
  1. From the Composite Browser white space context menu, click Orient > Ply Normal.
  2. Toggle the Select ply arrows so that ply3 is active.
  3. Click Apply to plot current ply normals. Note the discontinuity described above.
  4. To correct ply normals, click the Pick elements > Elements collector twice to access the element selection panel.
  5. Select only elements of the web and click proceed.
  6. Click the Reverse radio button under Normals and then click Apply. This will plot corrected ply normals for ply3.
  7. Reset the Display radio button under Normals to prevent any additional changes.
  8. Confirm the web of ply3 has no discontinuity with the caps by repeating Step 2 and Step 3.
  9. Repeat Step 3 through Step 8 for ply4.

Create Sublaminates

Create the sublaminates, which represent the stacks up plies on each unique tool used to manufacture the part.

  1. In the Composite Browser, right-click in white space and select Create > Laminate from the context menu Repeat this action so that there are five laminates created in total.
  2. Shift-select four laminates (IDs 2-5) and drag them into the laminate with id = 1. Notice that the parent laminate becomes an Interface Laminate and children become Sublaminates.
  3. Edit the names of the laminates and drag the plies from the unstacked plies folder into the sublaminates so that they match the image below.
    Figure 8.

Create the Interface

Define the interface, which specifies how the sublaminates are joined.

The interface laminate contains a list of sublaminates. It also contains a list of interfaces that specify how sublaminates connect (interface) with each other. Each interface definition contains two inputs: interface ply1 and interface ply2. These are either the top most or bottom most ply of each sublaminate that interface. The order they are entered is the order the sublaminates are stacked, in the direction of the element normal. See the figure below for the correct interfaces for the I-beam.

Figure 9.
  1. In the Composite Browser, right-click on the interface_laminate laminate and select Interfaces.
  2. Create the 5 interfaces in the Interface definition table at the bottom of the dialog. Use the image above as a reference.
  3. Define Interface ply1 and Interface ply2 for each interface using the values in the dialog below.
  4. Click OK to define the interfaces.

    Figure 10.

Create Ply-Based Properties

Create ply-based template properties.

Typically, only one ply-based property is required per part. However, for cases where portions of a part require different property attributes (offset is most common), multiple properties are required. For the I-beam model, the elements that make up the web are at the midplane of the laminate, and the elements that make up the caps are at the tube tooling surfaces.

  1. In the Composite Browser, right-click on white space and select Create > Property from the context menu.
  2. Confirm the Card Image is set to PCOMPP.
  3. Set Name to caps.
  4. Set Z0 to 0.0. This defines the offset such that plies begin stacking from the location in space of the elements.
  5. Assign the elements of the caps by right-clicking on the property in the Model Browser and selecting Assign from the context menu.

    Figure 11.
  6. Repeat Step 1 through Step 5 for the web property. Set the name to web. Leave Z0 as blank. This will place the midplane of the laminate at the elements in the web.

    Figure 12.

    Figure 13.

Optional: Ply Direction Visualization

Plot vectors that represent the ply1 direction on each element.

  1. Select a ply, and from the ply entity context menu, select the Ply 1 Direction option.
  2. Select a ply in the browser. This will plot the ply 1 direction (fiber direction) at each element.
  3. Click the Ply 1 Direction option again to deactivate it.

    Figure 14.

Optional: Composite Layers Visualization

Visualize the thickness and ply layers of the laminate. This is used to confirm that all plies are in the expected order. If the interfaces were defined incorrectly, there will be discontinuities where portions of a ply jump to an unexpected location in the full stack.

  1. In HyperWorks, open the Element and Handle Visualization dialog at the bottom of the graphics area.
  2. Active 3D and Ply layers.
  3. From the menu bar, select File > Preferences.
  4. In the Graphics area, type 5 in the ply visualization thickness factor input. This will increase the displayed thickness of each ply layer for the purposes of visualization.
    Figure 15.
  5. In HyperMesh Desktop, set Element Representation to 2D Detailed Element Representation. This will visualize the total thickness on each element.
  6. Set the Composite Layers control to Composite Layers. This will display the individual layers within each element thickness.
  7. Color elements by ply color and change the Element Color Mode to By Prop.
  8. From the menu bar, select Preferences > Graphics and type 5 in the ply visualization thickness factor input. This will increase the displayed thickness of each ply layer for the purposes of visualization.

    Figure 16.