Composite Analysis

Define the stacking direction of plies in the laminate.

1. Open the Material Reference Orientation dialog by right-clicking in the white space of the Composite Browser and selecting Orient > Element Normals from the context menu.
2. Select elements by double-clicking on the elements collector and making a selection using the pop-up.
3. Click display.
   Current element normals for 2D elements are displayed. Notice that the current element normals point out. Elements in the model represent the OML of the part, and the plies stack inward. Therefore, element normals must be flipped to properly represent the stacking direction of the laminate from the tooling surface.
4. Click reverse to flip the direction of the element normals.

   
   
   Figure 2.

   
   
   Figure 3.

Define the material orientation for the part.

1. Open the Composites panel by clicking 2D > composites > material orientation.
2. Select the elements on which material orientation will be set by double-clicking on the elements collector and selecting all elements in the tapered_beam component.
3. Set the material orientation x method to System.
4. Select system id = 1, the local system on the geometry near global (-3,0,40).
   Note: The user profile and orientation method will determine the final solver cards created or manipulated. In this case specifically, in OptiStruct the MCID field of the element cards will be populated by the system id. Internally, OptiStruct will project the system x axis onto the elements to define the material x direction.

   
   
   Figure 4.

   
   
   Figure 5.

Review materials.

1. In the Composite Browser, highlight the material carbon_epoxy.
2. Review the material properties in the Entity Editor.
   Note: These properties are typical of a uni-direction carbon-epoxy product in mmNS consistent units.

   Note: In the OptiStruct user profile, MAT8 cards are used to define orthotropic shell material properties.
3. Repeat Steps 1 and 2 for the material glass_epoxy.

   
   
   Figure 6.

Create the plies that make up the composite laminate.

1. In the Composite Browser, right-click in white space and select Create > Ply from the context menu.
   Uni-directional plies will be created first.
2. For the first layer in the following table, type the Ply Name, Material, Thickness, and Orientation into the tabular fields provided in the Composite Browser.

   Ply Name	Ply ID	Orientation	Thickness	Material	Shape
   uni_1	1	0	0.2	carbon_epoxy	Shape 1
   uni_2	2	90	0.2	carbon_epoxy	Shape 1
   uni_3	3	90	0.2	carbon_epoxy	Shape 2
   uni_4	4	0	0.2	carbon_epoxy	Shape 2

3. To define Shape1 and Shape 2:
   1. In the Composite Browser right-click in white space and select Create Shape from the context menu.
   2. In the Entity Editor, populate the Entity IDs. Select appropriate elements in the tapered_beam component.
   3. Click OK to confirm the selection.
      The new ply appears in the Composite Browser.
   4. Rename the newly created set in the Entity Editor using the appropriate shape name in the table.
   5. Repeat Step 2 though 3d to create the other shape.

      
      
      Figure 7.

4. Shapes can be assigned to one or multiple plies by selecting plies in the Composite Browser and populating the Shape field in the Entity Editor. Assign shapes using the table above.
5. Create woven plies according to the following table by repeating Step 1 through Step 4.
   You will model woven plies using the unidirectional weave type. This method uses a material model with properties at the scale of the warp/weft direction – the material properties are the unidirectional equivalent after dehomogenizing homogenized properties where E1=E2. The unidirectional weave ply type internally uses four unidirectional plies with 0.25 thickness, where the stacking sequence is [θ/θ+90/θ+90/θ].

   Note: If you do not know these properties but wish to use this ply type, you can use the homogenized weave ply type instead. If these plies are then changed to unidirectional weave or are draped, the material will be dehomogenized automatically.

   Ply Name	Ply ID	Orientation	Thickness	Material	Shape
   woven_1	5	45	0.18	glass_epoxy	Shape 1
   woven_2	6	45	0.18	glass_epoxy	Shape 1
   woven_21	7	-45	0.09	glass_epoxy	Shape 1
   woven_22	8	45	0.09	glass_epoxy	Shape 1

6. After all plies have been created, auto color by shift selecting the plies in the Composite Browser, selecting one of the Color icons, and click Auto color.

   
   
   Figure 8.

Create the laminate and stack the plies.

1. In the Composite Browser, right-click in white space and select Create > Laminate from the context menu.
2. In the Entity Editor, confirm that the Card Image for the laminate is set to STACK. This will set the card that defines the laminate in OptiStruct. In other solvers, this will be None.
3. In the Entity Editor, confirm the laminate option is Total. This specifies that the ABD matrix calculated from the laminate will be exact. Other common options include:
   • Smear – this removes the effect of stacking sequence from the ABD matrix
   • Symmetric – this allows only half the plies to be modeled. The other half will be managed automatically such that the full laminate is defined plies.
4. Shift-select the previously created plies and drag them into the laminate.
5. Drag and drop one or more plies within the laminate so that their stacking sequence matches the image below.

   Figure 9.

   Note: Plies can also be automatically created from a spreadsheet import. Created plies can be exported to a spreadsheet. To access this functionality, right-click on a laminate and select Import or Export CSV.

Create the ply-based property, which specifies solver property card-specific attributes.

1. In the Composite Browser, right-click in the white space and select Create > Property from the context menu.
2. In the Entity Editor, confirm that Card Image is set to PCOMPP. For other solvers, the card image will be the typical zone-based composite property.
3. In the Entity Editor, set Z0 to 0.0.
   This defines the offset such that plies begin stacking from the location in space of the elements.
4. Assign PCOMPP to the elements of the tapered_ beam component. Right-click on the property and select Assign from the context menu. Select the elements of the tapered_beam and click Proceed.

   
   
   Figure 10.

   Note: No other information about the composite property layers needs to be set, regardless of solver. All layer information is defined on the play and laminate entities.

Plot vectors that represent the x,y,z reference orientation of each element.

1. Select a laminate, and from the laminate entity context menu, select the Material Reference option.
2. Select the laminate or a ply in the Composite Browser. This will plot the x,y,z reference orientations on each element contained in the ply or laminate.
3. Select the Material Reference option again to deactivate it.

   
   
   Figure 11.

Plot vectors that represent the ply 1 directions on each element.

1. Select a ply, and from the ply entity context menu, select the Ply 1 Directionoption.
2. Select other plies in the Composite Browser. This will plot the ply 1 direction (fiber direction) at each element.
   Note: For the unidirectional weave ply type, both the warp and weft fiber directions will be plotted.
3. Select the Ply 1 Direction option again to deactivate it.

   
   
   Figure 12.

Plot the boundaries of each ply.

1. At the top of the Composite Browser, select the drop-down arrow next to the Selector icon and choose the Ply icon (on by default).
2. Click on Selector to activate it. This will link selections in the browser to display in the graphics area.
3. Expand the Plies folder and left-click on one or more plies. Notice the boundaries appear highlighted in the graphics area.

   
   
   Figure 13.

Visualize the thickness and ply layers of the laminate.

1. In HyperWorks:
   1. Open the Element and Handle Visualization dialog at the bottom of the graphics area.
   2. Activate 3D and Ply Layers.
   3. From the menu bar, select Preferences > Graphics and type 5 in the ply visualization thickness factor input. This will temporarily increase the displayed thickness of each ply layer for the purposes of visualization.

      Figure 14.

2. In HyperMesh Desktop:
   1. Set Element Representation to 2D Detailed Element Representation. This will visualize the total thickness on each element.
   2. Set Composite Layers control to Composite Layers. This will display the individual layers within each element thickness.
   3. Color elements by ply color and change the Element Color Mode to By Prop.
   4. From the menu bar, select Preferences > Graphics and type 5 in the ply visualization thickness factor input. This will temporarily increase the displayed thickness of each ply layer for the purposes of visualization.

      
      
      Figure 15.

Request typical composite results from OptiStruct.

1. In the Model Browser, right-click in white space and select Create > Output from the context menu.
   This creates a GLOBAL_OUTPUT_REQUEST card if one is not already present in the model.
2. In the Model Browser, select GLOBAL_OUTPUT_REQUEST to open the card in the Entity Editor.
3. Request ply level strains by checking CSTRAIN. Set the following options:
   • EXTRA = MECH – this will request mechanical strains, which cause stress
   • NDIV = 2 – this will output results at the top and bottom of each ply
   • OPTION = YES – this will request the output
4. Request ply level stresses by checking CSTRESS. Set the following options:
   • NDIV = 2 – this will output results at the top and bottom of each ply
   • OPTION = YES – this will request the output
5. Request the first ply failure/onset by checking CFAILURE. Set the following options:
   • NDIV = 2 – this will output results at the top and bottom of each ply
   • OPTION = YES – this will request the output
   This will print first ply onset results using the allowables defined on the MAT8 material card for each ply and the first ply failure theory specified on the PCOMPP property FT field.

   
   
   Figure 16.

Perform a draping simulation to account for local orientation changes in each ply due to placing material on a tool with compound curvature.

1. In the Composite Browser, right-click the laminate1 folder and select Drape > Kinematic Drape from the context menu.
   This opens the Kinematic Draping tool and performs a draping simulation on all plies.

   Note: Plies can also be draped individually or in small numbers by Shift-selecting them directly.
2. Double-click the Node collector to select the Seed point.
3. Select Node 4173. This is the location where the ply first touches the tool during manufacturing.
4. Confirm the Method is set to Quadrants.
5. Click Apply to drape the plies.
6. Repeat the Ply Direction Visualization exercise to visualize the draping results. Before clicking Apply, check the Drape fiber orientation.
   Note: Draping simulation generates a DRAPE table for each ply draped. The table contains thickness and orientation corrections for each element.

   
   
   Figure 17.

Generate zone-based solver properties from the ply-based model.

1. In the Model Browser, right-click the Laminate folder and select Realize from the context menu.
2. Uncheck the Include drape option and click Realize. Notice the new properties generated and assigned to the model.

   
   
   Figure 18.

   
   
   Figure 19.