Composite Analysis

Define the stacking direction of plies in the laminate.

1. Open HyperMesh.
2. In the User Profiles dialog, set the profile to OptiStruct.
3. Open the model file, composite_hat.hm.
4. Open the Composites panel by clicking 2D > composites > element normals.
5. Toggle from color display to vector display and click display.
   Current element normals for 2D elements display. 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.
6. Back in the Composites panel, 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 component on which material orientation will be set by setting the panel middle top collector to comps and selecting the tapered_beam component.
3. Set the material orientation method from the panel middle bottom collector to by system id.
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.

   Note: The composites panel can be used to project vectors or systems which define a material orientation. To set a material orientation which follows a curve, the Aerospace Material Orientation tool can be used from the Engineering Solutions Aerospace user profile. Access this tool by clicking Aerospace > Composites > Material Orientation.

   
   
   Figure 4.

   
   
   Figure 5.

Review materials.

1. In the Model Browser, highlight the material carbon_epoxy.
2. Review the material properties in the Entity Editor.
   Note: All panels must be closed for the Entity Editor to display.

   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.

   In the upcoming three steps, ply-based modeling data will be used. Ply-based models are organized such that the modeling entities used are analogous to the manufactured parts. Data for ply-based models includes:

   • Plies – one unique ply per physical ply in the part should be defined. Plies define material and thickness, orientation and shape.
   • Laminate – one laminate per physical part. The laminate defines the list of plies which make up the composite part.
   • Template property – defines the data which traditional solver properties usually contain. Example attributes are offset and non structural mass. OptiStruct supports ply-based modeling entities, the specific ply-based property card is a PCOMPP. For other solvers, the template property takes the card image of the typical composite zone property and defines all solver property data other than layers.

Create the plies that make up the composite laminate.

1. In the Model 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.

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

3. To define Shape1 and Shape 2:
   1. Click the element collector twice to open the element selection panel.
   2. Select appropriate elements in the tapered_beam component.
   3. Click Create.
      The new ply appears in the Model Browser.
   4. Rename the newly created set in the Entity Editor using the appropriate shape name in the table.
   5. Repeat Step 2 and 3 to create the remaining plies from the table above. For shapes that already exist, change the Shape to Set, click twice on the set collector to open the set selection panel, and select the appropriate set.

      
      
      Figure 7.

4. Create woven plies according to the following table by repeating Step 2 and Step 3. You will model woven plies as two uni-directional plies with half thickness. This is done so that the plies can be draped in a later step.

   Ply Name	Ply ID	Material	Thickness	Orientation	Shape
   woven_11	5	glass_epoxy	0.09	45	Shape 1
   woven_12	6	glass_epoxy	0.09	-45	Shape 1
   woven_21	7	glass_epoxy	0.09	-45	Shape 1
   woven_22	8	glass_epoxy	0.09	45	Shape 1

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

   
   
   Figure 8.

Create the laminate by stacking plies.

1. In the Model Browser, right-click in white space and select Create > Laminate from the context menu.
2. Fill the table with the 8 plies previously created. To populate a row choose one of the following methods:
   • Click white space in the Name column, then click the drop-down arrow to the right of the column. Select the ply.
   • Double-click white space in the ID column, then type the ID of the ply.
3. Confirm that Card image is set to STACK. This will set the card that defines the laminate in OptiStruct.
4. 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.

   
   
   Figure 9.

   Note: Plies can be automatically created from a spreadsheet import. Created plies can also be exported to a spreadsheet. To access this functionality, right-click in the grey area immediately to the left of the Name column and select Import from excel or Export to excel.
5. Click Create to create the laminate.

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

1. In the Model Browser, right-click in the white space and select Create > Property from the context menu.
2. In the Entity Editor, set Card Image to PCOMPP. For other solvers, the card image will be the typical zone-based composite property.
3. 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 tapered_ beam component by highlighting tapered_beam component in the Model Browser, double-clicking in the Property field in the Entity Editor and selecting the PCOMPP property.

   
   
   Figure 10.

   Note: No other information about the composite property layers needs to be set, regardless of solver. All other information about the section is held in the ply and laminate entities.

Plot vectors that represent the x,y,z directions on each element.

1. From the menu bar, select Tools > Orientation Review.
2. Select the Material system tab.
3. Under Display options, confirm that Visibility X, Y, and Z are selected.
4. Click the elements collector twice to open the elements selection panel and select all elements.
5. Click Apply to plot the material orientation on each element.

   
   
   Figure 11.

Plot vectors that represent the ply 1 and 2 directions on each element.

1. From the menu bar, select Tools > Orientation Review.
2. Select the Ply directions tab.
3. Click Apply.
   This will plot the ply 1, 2 directions for the current ply in the list.
4. To scroll through plies, click the << or >> icons under Select ply.

   
   
   Figure 12.

Plot the boundaries of each ply.

1. At the top of the Model Browser, select the drop-down arrow next to the Selector icon and choose the Ply icon (default is Component).
2. Click on Selector to activate it. This will link selections in the Model 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. 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. Change Element Color Mode to By Prop. This will color each layer by the color of the ply.
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 14.

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 onset theory specified on the PCOMPP property FT field.

   
   
   Figure 15.

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 Model Browser, right-click the Plies 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 smaller numbers by selecting them within the Plies folder.

   Note: Kinematic draping is the preferred solution for OptiStruct and Nastran profiles. For other profiles, use the Drape Estimator tool.
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 16.

Generate zone-based 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 17.

   
   
   Figure 18.