HM-4460: Composite

In this step, you will load the ANSYS user profile in HyperMesh.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, set the user profile to Ansys.

In this step, you will load the model file in HyperMesh

1. From the menu bar, click File > Import > Geometry.
2. In the Import tab, set File type to CATIA.
3. Click .
4. In the Select CATIA file dialog, open the pillar_w_ncf.CATPart file.
5. Click Import.
   Note: You will import the Ply and Composite data later in this tutorial.
   HyperMesh imports geometry data only.

   
   
   Figure 1.

6. In the Model Browser, review the model contents.

   
   
   Figure 2.

In this step, you will mesh all of the model surfaces simultaneously while specifying element sizes and element types.

1. Open the Automesh panel by completing one of the following options:
   • From the menu bar, click Mesh > Create > 2D AutoMesh.
   • From the main menu, open the 2D page and click automesh.
   • Press F12.
2. Open the size and bias subpanel.
3. Set the entity selector to surfs.
4. Click surfs > displayed.
5. In the element size= field, enter 5.
6. Set mesh type to mixed.
7. Set the mesh mode to interactive.
8. Set the elements to surf comp/elements to current comp toggle to elems to current comp.

   
   
   Figure 3.

9. Click mesh.
   Note: You should now be in the density subpanel of the meshing module. There is node seeding and a number on each surface edge. The number indicates the number of elements that were created along the edge.
   The meshing module opens.

   
   
   Figure 4.

10. Click return.
    The mesh is accepted.

    
    
    Figure 5.

11. From the menu bar, click File > Save As > Model.
12. In the Save Model As dialog, navigate to your working directory and save the HyperMesh database with the name pillar_w_ncf_FINAL.hm.

In this step, you will load the ply information from FiberSim in HyperMesh.

1. From the menu bar, click File > Import > Geometry.
2. In the Import tab, set File type to FiberSim.
3. Click .
4. In the Select FiberSim file dialog, open the pillar.h5 file.
5. Click Import.
   HyperMesh imports and populates the database with laminate data (ply book and ply stacking data), composite material information, each ply data (triangular elements spanning a single ply), and a coordinate system.
6. In the Model Browser, review the model's contents.

   
   
   Figure 6.

7. Click on the Visualization toolbar.
   Elements and feature lines become transparent.
8. In the panel area, click comps.
9. Select the Geometry and auto1 components.
10. Click select.
11. Use the transparency slider, as seen in Figure 7, to review the system collector imported by the FiberSim model.

    
    
    Figure 7.

12. Click return.
13. On the Visualization toolbar, click to shade the elements and mesh lines.
14. On the Visualization toolbar, click to shade the geometry and surface edges.

    
    
    Figure 8.

15. In the Model Browser, turn off the display of geometry for all of the components.

    
    
    Figure 9.

In this step, you will review and edit element normals in a model in HyperMesh.

1. From the menu bar, click Mesh > Check > Elements > Normals.
   Note: Element normals need to be changed to match the Z direction (red color).
   The Normals panel opens.
2. Set the first switch to elems as seen in Figure 10.

   
   
   Figure 10.

3. Click elems > displayed.
4. Set the vector display/color display toggle to color display.
5. Click display.
   Note: The red side of the elements is the positive normal direction Z, while the blue side is the negative normal direction.
   HyperMesh displays, on each side of the part, the element normals using the colors red and blue.

   
   
   Figure 11.

6. Set orientation to elem.
7. Select one element that has the right direction.
   This element will be used as the model for the other elements.
8. Click adjust.
   All of the elements are set in the same normal direction.
9. Optional: If the blue color is in the Z direction, click elems > displayed and then click reverse.
   All of the elements are set in the right normal direction (red).

   
   
   Figure 12.

10. Click return to exit the panel.

In this step, you will realize the ply geometry shape.

1. In the Model Browser, right-click on the Plies folder and select Realize from the context menu.
2. In the Ply Realization dialog, click Component.
3. In the panel area, click comps as seen in Figure 13.

   
   
   Figure 13.

4. Select the listed components as seen in Figure 14.

   
   
   Figure 14.

5. Click select.
6. Click proceed.
7. Set Projection options to FiberSim drape map by proximity method.
8. Set Search Criterion to Element centroid.

   
   
   Figure 15.

9. Click Realize.
   This process takes each FiberSim Ply data and finds the FE elements which are bounded by the ply boundaries, and transfers the ply directions, draping data, and ply orientation into FE elements. This process also converts geometry plies into FE plies. At the end of realization, HyperMesh creates sets containing FE elements for each ply.

   
   
   Figure 16.

In this step, you will add an element typer.

1. In the Model Browser, right-click and select Create > Sensor from the context menu.
   HyperMesh creates and opens a sensor (Et Type) in the Entity Editor.
2. In the Entity Editor, enter a name and ID, and select a color.
3. By default, Element Type is set to SHELL181.

   SHELL181

   Suitable for analyzing thin to moderately-thick shell structures. It is a 4-node element with six degrees of freedom at each node: translations in the x, y, and z directions, and rotations about the x, y, and z-axes. (If the membrane option is used, the element has translational degrees of freedom only). The degenerate triangular option should only be used as filler elements in mesh generation.

   Well-suited for linear, large rotation, and/or large strain nonlinear applications. Change in shell thickness is accounted for in a nonlinear analysis. In the element domain, both full and reduced integration schemes are supported. SHELL181 accounts for follower (load stiffness) effects of distributed pressures.

   May be used for layered applications for modeling laminated composite shells or sandwich construction. The accuracy in modeling composite shells is governed by the first order shear deformation theory.

4. To simulate the element stiffness, set the stress stiffening option, extra displacement shapes, extra stress output, pressure loading, mass matrix, stress stiffness matrix, define the element coordinate system and specify the data storage using the respective keyopts, click Create/Edit.
5. Optional: If necessary, click View > Browsers > HyperMesh > Solver from the menu bar to open the Solver Browser.
6. In the Solver Browser, review the new element type.

   
   
   Figure 17.

In this step, you will update the componenet with the element type.

1. In the Component folder of the Model Browser, select Geometry.
   The Entity Editor opens and displays the component's corresponding data.
2. In the Entity Editor, set card image to HM_COMP.
3. For Type, click Unspecified > Sensor.
4. In the Select Sensor dialog, select sensor1 and click OK.

In this step you will verify FE plies thickness and orientation in HyperMesh.

1. On the Visualization toolbar, set the element color mode to (visualize elements by property).
2. On the Visualization toolbar, set the layer representation mode to (Composite Layers with Fiber Direction).
3. In the Model Browser, Hide and Show each Ply.

   
   
   Figure 18.

   
   
   Figure 19.

4. On the Visualization toolbar, set the element representation mode to (2D Detailed Element Representation).

   
   
   Figure 20.

In this step, you will laminate realize the ply based model.

1. In the Model Browser, right-click on the Laminate folder and select Realize from the context menu.
2. In the Laminate Realize dialog, accept the default settings and click Realize.

   
   
   Figure 21.

   HyperMesh creates a property for each stack, and assigns it to a component.
3. On the Visualization toolbar, set the element color mode to .

   
   
   Figure 22.

   
   
   Figure 23.

4. In the Sections folder of the Model Browser, locate the shell sections.
5. Click on a section.
   The corresponding details for the section display in the Entity Editor.
6. In the Entity Editor, under PLIES, next to Data: TK, click .
7. In the PLIES dialog, review the number of plies, thickness, orientation, and material data.
8. Click Close.

In this step, you will export the deck to ANSYS *.cdb format.

1. Click File > Export > Solver Deck from the menu bar.
   The Export tab opens.
2. Set File type to Ansys.
   If you are in the ANSYS user profile, HyperMesh automatically sets the File type to Ansys and loads ANSYS as the default Template.
3. In the File field, navigate to your working directory and save the file as pillar_w_ncf-FINALhm.cdb.
4. Click Export.