This tutorial takes you through the process of developing a ply lay-up definition for a composite structure using a PCOMPG card, and shows the advantages of post-processing the results with global ply numbers. The traditional definition method, using PCOMP, is introduced first here to ultimately show the practical advantages of using PCOMPG for the given scenario. The model for this tutorial is shown below. Since the structure, loads, and boundary conditions are symmetrical about the x-axis, only one half of the structure is modeled with suitable boundary conditions applied to enforce half symmetry.

Torsion frame

The following exercises are included:

 

Retrieve the HyperMesh Database File

---

Step 1:  Launch HyperMesh, set the OptiStruct User Profile and retrieve the file

Step 2:  Review the model setup in HyperMesh

The structural model has been already set up and can be solved without any further modifications. Review the model setup before submitting the job.

The model is set up for linear static analysis. As mentioned earlier, only half of the structure is modeled; and to impose the half symmetry boundary conditions, all the nodes on the symmetry plane are constrained in dof1, dof5, and dof6.

All of the components are modeled with the PCOMP property which lists the plies (stacking sequence) from the bottom surface upwards, with respect to the element’s normal direction, as shown in the image below.

Ply stacking sequence with respect to element normal

Components in this model that have names starting with the word "Flange" represent junctions in which different components are connected together. While reviewing, closely watch the flange area formed by the Skin and Rib components (highlighted in the following figure). Review the ply lay-up of the Skin_inner, Rib, Flange1_Rib_Skin, and Flange2_Rib_Skin components (laminate layout is shown in the bottom portion of the following figure). Note that few plies are common for the Skin_inner, Flange1_Rib_Skin, Flange2_Rib_Skin, and Skin_outer components, but appear in different stacking sequence in each component. For example, the 4th ply in Skin_inner is the 3rd ply in Flange2_Rib_Skin and the 2nd ply in Skin_outer components.

Ply stacking for the Skin_inner, Rib, Skin_outer, Flange1_Rib_Skin, and Flange2_Rib_Skin components

This opens the HyperLaminate (GUI) in which the ply lay-up information can be defined, reviewed and edited. Material properties and design variables can also be created and edited here.

Details of the laminate appear in the GUI.

Observe that the first 5 layers are the same as Skin_inner lay-ups and that the last two lay-ups are the same as the 3rd and 4th lay-up of Rib, as shown in the last figure. You can verify how other flanges are modeled.

Step 3:  Submit the Job

The name and location of the frame_PCOMP.fem file displays in the input file: field.

If the analysis is successful, no error messages are reported to the shell. The analysis is complete when the message Process completed successfully appears in the shell.

The default files written to the directory are:

The frame_PCOMP.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

Step 4:  View the results/Post-processing

Stress distribution on the top face of the frame

The stress value does not vary gradually in the top face region, but suddenly decreases to a lower value across the Flange2_Rib_Skin component. Looking at the table of laminate properties of Flange1_Rib_Skin again, observe that the 3rd ply property of the Flange2_Rib_Skin component is of a matrix material and the third plies in the components adjacent to it (Flange1_Rib_Skin and Skin_outer) are of a carbon fiber material. The sudden changes in the stress values occur because we are looking at stress on two different materials. This example shows that, for the results to be meaningful during post-processing of the PCOMP results, you have to correlate the ply results to their corresponding ply property.

This highlights that, during the post-processing of PCOMP components, plotting results based on just the ply number is not sufficient. You have to keep track of ply properties (material, thickness, orientation, failure index, etc.) on your own during post-processing with this method. In cases that use large and complex models, it becomes tedious to track the individual ply properties during post-processing.

This drawback to using PCOMP can be avoided with the use of the PCOMPG card for property definition. Using the PCOMPG card, you can assign a global ply number for each ply and post-process the results based on global ply number. The following steps explain the procedure to redefine the model with PCOMPG property.

Step 5:  Redefine the model setup in HyperMesh

Laminate information with global ply number

Now you create new PCOMPG components with global ply numbers defined as shown in the above figure. As discussed earlier, the 4th ply in Skin_inner is the 3rd ply in Flange2_Rib_Skin and the 2nd ply in Skin_outer components. Therefore, all of these plies will be defined with the same global ply ID 4. Similarly, all other plies are to be defined, as shown in the above figure.

Referring to the figure showing laminate information with global ply number above, you will create the Flange1_Rib_Skin_GPLY component.

The new component Flange1_Rib_Skin_GPLY was created. Its first 5 plies are the same as Skin_inner_GPLY and its last 2 plies are the 3rd and 4th plies of the Rib component.

To reduce the number of steps in this tutorial, the ply lay-up information of other components is already defined with PCOMPG property and appropriate laminate information in the updated_PCOMPG_properties.fem file you saved to your working directory from the optistruct.zip file. This file is imported into HyperMesh to update (overwrite) the properties instead of manually updating them.

The updated_PCOMPG_properties.fem file is saved in OptiStruct input file format. Open this in any text editor to review how the components are defined with PCOMPG properties. A section of the file is shown below.

Components defined with PCOMPG

This option overwrites the old PCOMP properties with PCOMPG properties defined in the updated_PCOMPG_properties.fem file.

Step 6:  Review the imported properties in HyperLaminate

All of the components now appear under PCOMPG. The components created earlier (Skin_inner_GPLY, Rib_GPLY, and Flange1_Rib_Skin_GPLY) are still present. There is no element associated with these components. Review the PCOMPG components to view the laminate definitions.

Step 7:  Submit the Job

The name and location of the frame_PCOMPG.fem file displays in the input file: field.

If the job is successful, new results files can be seen in the directory where the model file was written. The frame_PCOMPG.out file is a good place to look for error messages that will help to debug the input deck, if any errors are present.

The default files written to the directory are:

Step 8:  View the results/Post-processing

A message window may appear with information about the successful loading of the model and result files into HyperView.

Post-processing the results based on global ply number eliminates the need to track the ply number and corresponding ply properties on the components. The results are displayed based on the global ply number, irrespective of the ply order, so you can chose any one global ply number and view results across the whole component. If a particular ply is not present in any given region, no result is displayed.

See Also:

OptiStruct Tutorials