Menu

Laminate Shell Composite Modeling in Femap

The steps performed in this video are:

  • Import a Femap Neutral File with geometry edits for meshing attributes already applied
  • Create layups for the model
  • Create properties for the layups
  • Mesh the geometry
  • Assign material directions to the mesh
  • Apply loads to the Panel
  • Analyze the Panel and review results

Lets Import the Femap Neutral file.
File-Import-Femap Neutral, Select the neutral file and click open.
In Neutral file Read Options dialog box, click ok.
The Femap model should appear as displayed on the screen.

Lets create a new 2D orthotropic material using a prepeg fabric.
Using the Model Info pane, right-click on the Material object and select new.
 In the Create Material dialog box, click the Type button and select Orthotropic (2D) in the Material Type dialog box.
Click OK to confirm your selection.
Click the Load button in the Define Material dialog box.
Select the material, Carbon Epoxy Fabric in the Select from Library dialog box, then, click ok.
Click OK to complete creating the material.
Create a layup for the standard thickness of the fitting.
Right-click on the Layups object in the Model Info pane and select New.
In the Layup Editor dialog box, set the Title to Standard Layup.
Select the Material, Carbon Epoxy Fabric. Set the Thickness to .5 and the Angle to 0.
Click the New Ply button. For the next ply, Set the Angle to 45. Click the New Ply button.
Continue creating another ply by setting the Angle to 0. To Duplicate plies 2 and 3.
Select Ply 2 in the Layup Editor dialog box. While holding the Shift key, select Ply 3.
Click the Duplicate button.

To create symmetric of the layup, Select ply 1 while holding shift key, select ply 5 click the symmetric button.
Click OK to complete editing the layup.
Right-click on the Properties object in the Model Info pane and select New from the menu.
In the Define Property dialog box, click the Elem/Property Type button.

In the Element / Property Type dialog box, select Laminate,
then, click OK to change the Define Property dialog box
to Laminate Element Type.

Set the Title to Standard Laminate.
Set the Layup to Standard Layup.
Set the BondShr Allow to 75.
Set the Failure Theory to Tsai-Wu, then, click OK to create the laminate property.

Go to mesh –geometry –surface. Click on select all button and click ok. In automesh Dialog box select laminate property created and click ok.
Now the mesh has been created.

Since this model is dealing with orthotropic materials, proper material directions should be assigned, otherwise the material direction is assumed to be aligned with the global X-axis.
Select the command, Modify, Update Elements, Material Orientation.

  • In the Entity Selection dialog box, click Select All, then OK.
  • In the Material Orientation Angle dialog box, select the following:

Set Angle using Coordinate Axis as ‘Y’.
Select as the Csys, 0..Basic Rectangular.
Click OK to assign the material orientation.
Display material angle.

 Open the View Options dialog box by pressing the F6 hot key.
In the View Options dialog box, set the Category to Labels, Entities and Color.
Select as the Options, Element – Material Direction.
Set the Color Mode to Use View Color and set the View Color to black (0).
Check show material direction option.
Click OK to apply the changes.

In the Model Info pane, right-click the Constraints object, and select New.
In the New Constraint Set dialog box, enter the Title as
Constraints and then, click OK to create the constraint set.
Expand the newly created constraint set and right-click the
Constraint Definitions object and select On Curve from the menu.
Select the existing group boundary and click on more button. And click ok.
Set the type to Fixed and click Ok to create the constraint.

In the Model Info pane, right-click the Loads object, and select New.
 In the New Load Set dialog box, enter the 100 N Load and, then, click OK to create the Load set.
Expand the newly created load set and right-click the Load.
Definitions object and select On Surface from the menu.
Select the Pads on the surface then click ok.
In the Create Loads on Surfaces dialog box, set the Title to 100 N Load.
Set the type to Force.
Set the FZ to -100.
Click OK to create the load.

In the Model Info pane, right-click the Analysis object and select New from the menu.

  • In the Analysis Set Manager dialog box, click the New button.
  • In the Analysis Set dialog box, set the Title to Linear Statics.

Set the Analysis Program NX Nastran.
Set the Analysis Type to Static.
Click Ok to create the analysis set.
Click the Analyze button.

Once the analysis has complete, close the NX Nastran Monitor pane.

To Display Von Mises stress contours.
Open the PostProcessing Toolbox.
Set the Contour Style to Contour.
The Output Set should default to the new results
and the Output Vector to 1000033..Lam Ply1 VonMises Stress.
Select output vector 6060..Laminate Max Failure Index and then,
Click ok to update the graphics pane to view the maximum failure index.

Download a Free 45-Day Trial or Buy Femap