FemapV11复合材料建模分析

IntroductionIn this exercise, you perform a linear stress analysis of a composite laminate fitting. The steps you will perform in this workshop are:∙Import a Femap Neutral File with geometry edits for meshing already applied∙Create two layups for the fitting – one for the normal thickness of the fitting and a second for reinforced areas around themounting holes∙Create properties for the two layups∙Mesh the fitting∙Assign material directions to the mesh∙Apply constraints and loads to the fitting∙Analyze the fitting and review resultsStep 1:Start Femap and Import Parasolid Geometry of the FittingStart Femap∙From either a desktop icon, or from the Windows Start menu, select the icon for Femap v11.Set your Femap preferences for the correct Geometry Scale Factor.The Geometry Scale Factor is number of length units permeter used by Parasolid.∙Select the command, File > Preferences.∙In the Preferences dialog box, select the Geometry/Model tab.∙Under the Geometry Preferences option group, set the Geometry Scale Factor to Millimeters.∙Click OK to apply the changes and close the dialog box.Import a Femap Neutral file with the fitting geometry editing for meshing and with mesh sizing already applied.∙Select the command, File, Import, Femap Neutral.∙In your workshop folder, select the Parasolid file,Fitting.NEU.∙In the Neutral File Read Options dialog box, click OK to read in the fitting.Your Femap model should appear as below.In this model, the green surfaces represent 5 mm offsets from the holes modeled as washers and the orange surfaces represent pads around the holes. These areas will be meshed with a thicker laminate than the rest of the fitting. Mesh sizes have also been preset for this model, with a default mesh size of 5.There are also three (3) additional coordinate systems that will be used to set material orientations. Display of points, coordinate systems and nodes are turned off in the current view.Save the model.∙Click the Save Model icon on the Model toolbar to execute the File > Save command.∙In the File, Save As dialog box, navigate up one folder to select the Exercises folder.∙Enter laminate-fitting as the name of the Femap model file.The .modfem extension for Femap models will beautomatically appended to the name.∙Click Save to complete saving the Femap model file.Step 2:Create two layups for the fitting – one for thenormal thickness of the fitting and a second forreinforced areas around the cutout and themounting holesSave your Femap model.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.You will now select a fabric from a material library provided with this workshop.∙Click the Load button in the Define Material dialog box.∙In the Select From Library dialog box, click the Choose Library button.∙In the Library File dialog box, navigate to your workshop folder and select the libraryComposites_Material_Library.esp, then, click the Openbutton to load the library into your model.∙Select the material, CFS003 Carbon LMT25 Epoxy Fabric in the Select From Library dialog box, then, click OK to load the attributes of this material into the Define Material dialog box.Note that the tensile and compressive properties are very similar for this composite fabric material.∙Click OK to complete creating the material.∙Since this will be the only material used in this model, you should Cancel the command.Note: If you want to load all the materials in a library into a Femap model, use the command, File, Import,Femap Neutral and select the material library. You’llneed to change the file extension to from .neuto .esp.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, create Global Plies that represent the top, bottom and mid-plane of the layups byclicking the Global Ply icon∙In the Global Ply Definition dialog box, click the New button.∙In the New Global Ply dialog box, set the Title to Bottom Global Ply.Select the material you just loaded from the material library and set the Thickness to .25.Click the More button to continue creating two moreglobal plies.∙Set the next Title to Midplane Global Ply.Select the material you just loaded from the material library and set the Thickness to .25.Click the More button to continue creating the final global ply.∙Set the next Title to Top Global Ply.Select the material you just loaded from the material library and set the Thickness to .25.Click the OK button to complete creating global plies.You should now see three global plies.∙In the Global Ply Definition dialog box, click Done.∙In the Layup Editor dialog box, set the Title to Standard Layup.∙Select the Global Ply ID, 1..Bottom Global Ply.Select the Material, 1..CFS003 Carbon LMT25 Epoxy Fabric.Set the Thickness to .25 and the Angle to 0.∙Click the New Ply button.∙For the next ply, set the Global Ply ID to 0..None.Set the Angle to 45.Click the New Ply button.∙Continue creating another ply by setting the Angle to 0.Note how the previous selections for Global Ply ID, Material, Thickness and Angle maintained.∙Click the New Ply button.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.Note how the two plies have been copied at the top of thelayup. Also note how the value of the Total Thickness hasbeen updated.∙Click OK to create the layup and to exit the Layup Editor dialog box.∙Click Cancel to end creating layups.In this step, you will display the Laminate Equivalent Properties using the Entity Info pane.∙Open the Entity Info pane by either clicking the Entity Info icon on the Panes toolbar, or by selecting the command,Tools, Entity Info.Edit the layup.∙Right-click on the Standard Layup object in the Model Info pane and select Edit from the menu.Note how the Laminate Equivalent Properties are nowdisplayed in the Entity Info pane including:∙Total Thickness∙In-Plane Properties∙Bending/Flexural Properties∙A, B, D, A-Inverse, B-Inverse and D-Inverse matrices∙In the Layup Editor dialog box, using the Shift key, select plies 4 and 5, and click the Duplicate button.Again, note how the Entity Info window’s display of theLaminate Equivalent Properties have been updated.∙Since we want a symmetric layup, using the Shift key, select plies 2 through 6, then click the Symmetric button.Note that you now have a total of 12 plies and a totalthickness equal to 3.∙Select Ply 12.Note that until only a single ply is selected, the New Plybutton is inactive. However, you will need to deselect the ply in order to create a new ply on top of the layup;otherwise the new ply will be created below the selected ply.While holding the Ctrl key, select Ply 12.∙Set the Global Ply ID to 3..Top Global Ply. Set the Angle to0 and then, click the New Ply button.Update the Global Ply for the middle plies.∙Select Ply 7.∙Set the Global Ply ID to 2..Midplane Global Ply.∙Click OK to complete the creation of the layup. Save your Femap model.Copy the first layup.∙Right-click on the newly created layup in the Model Info pane and select Copy from the menu.Modify the copied layup to represent the reinforced areas around the holes.∙Right-click the copied layup in the Model Info pane and select Edit from the menu.∙In the Layup Editor dialog box, change the Title to Hole Reinforcement Layup.∙While the Ctrl key, select plies 5, 6, 8 and 9.∙Click the Duplicate button.Note that the duplicated plies are now at the top of thelayup.Select plies 14 and 15, then click the Move Down button seven (7) times to move these two plies below the middle ply.They should now be plies 7 and 8.Repeat the previous steps for plies 16 and 17 so that they are just above the middle ply.Select plies 16 and 17, then click the Move Down button two(2) times to move these two plies below the top ply.The layup should now look like the following.∙Click OK to complete editing the layup.Step 3:Create properties for the two layupsRight-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 toLaminate Element Type.Set the Title to Standard Thickness Laminate.Set the Layup to Standard LayupSet the BondShr Allow to 25.Set the Failure Theory to Tsai-Wu, then, click OK to create the laminate property.If Femap’s User Interface preference are set to the default of AutoRepeat Create Commands you will still be in the mode of creating a property. If not, you will need to again openthe Define Property dialog box by right-clicking on theProperty object in the Model Info pane and selecting New.∙In the Define Property dialog box, set the Title to Reinforced Area Laminate.Set the Layup to Hole Reinforcement Laminate.Set the BondShr Allow to 25.Set the Failure Theory to Tsai-Wu, then, click OK to create the laminate property.∙Cancel the property creation command.Set the mesh attributes for the model.∙Select the command, Mesh, Mesh Control, Attributes on Surface.∙In the Entity Selection dialog box, click Select All, then the OK button.∙In the Surface Mesh Attributes dialog box, Set the Property to 1..Standard Thickness Laminate.Select Offset as Surface to Top Face.With the option for Mapped Meshing Options turned On,select the option for Map Subdivisions.Click OK to set the surface attributes.Save your Femap model.Step 4:Mesh the fittingTurn off display of surfaces.∙On the Entity Display toolbox, click the View Surfaces Toggle icon.Mesh the part.∙Select the command, Mesh, Geometry, Surfaces.∙In the Entity Selection dialog box, click the Select All button, then, the OK button.∙In the Automesh Surfaces dialog box, set the Property toe Meshing Attributes.Click OK to mesh the fitting.Turn on display of element thickness.∙On the View toolbar, select the View Style menu icon and select Thickness/Cross Section from the menu.You model should now appear similar to below.Update the property of the elements around the holes to use the Hole Reinforcement Laminate property.∙Select the command, Modify, Update Elements, Property ID.∙In the Entity Selection – Select Elements to Update Property dialog box, set the Method to on Surface.∙Select the surfaces around the hole including the washers and pads.In the Select Property to Update dialog box, select 2..Hole Reinforcement Laminate and then, click OK.The mesh should be updated as shown below withelement thickness display enabled.Note that the offsets of the elements are maintained as the original mesh attribute was set to offset from the top surface.Note: In this case, it may be easier to view the mesh by assigning different colors to the two laminateproperties and displaying elements by property coloras shown below.With Femap v10.31, there is now an option to assignrandom colors to properties in the Color Palettedialog box.Step 5:Assign material directions to the meshSince this model is dealing with orthotropic materials,proper material directions should be assigned, otherwisethe material direction is assumed to be aligned with theglobal X-axis.In this fitting, the unidirectional fabric follows the contourof the part.Assign a material angle to the mesh.∙Select the command, Modify, Update Elements, Material Angle.∙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 AxisXSelect as the Csys, 0..Basic Rectangular.Click OK to assign the material angle.Display material angle.∙Open the View Options dialog box by pressing the F6 hotkey.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 ViewColor to black (0).Check the box for Show Material Direction.Click OK to apply the changes.and zoom in around the front, right corner.Modify the material angle around the bend and the right end of the fitting. You will use an API script to assign the materialangles.∙If not already activated, activate the Custom Tools toolbar.∙Select the API script by selecting Custom Tools, Element Update, Orient Material Angle Tangent to Curve.∙Select the inner radius on the fitting.∙In the Entity Selection dialog box, set the selection Method to on Surface.Select the three (3) surfaces around the bend as shown below, then, click OK.∙Repeat the command, Custom Tools, Element Update, Orient Material Angle Tangent to Curve.You can use the Ctrl+y hotkey as an alternative to selecting the command.∙Select the straight edge on the bottom front right edge of the fitting.In the Entity Selection dialog box, set the selection Method to on Surface.Select the surfaces on the right hand end of the fitting as shown below, then, click OK to confirm your selection.Zoom in around the hole on the front, right side of the fitting to see how the material angle has been updated.Save your Femap model.Step 6:Apply constrains and loads to the modelCreate a constraint set for the holes.∙In the Model Info pane, right-click the Constraints object, and select New.∙In the New Constraint Set dialog box, enter the Title as Pinned Mount Holes and then, click OK to create theconstraint set.Create a pinned constraint on the washers.∙Expand the newly created constraint set and right-click the Constraint Definitions object and select On Surface from the menu.In the Entity Selection dialog box, set the Method to color and select one of the washer surfaces.Click the Preview button before clicking OK.In the Create Constraints on Geometry dialog box, set the Title to Pinned Mount Holes.Set the type to Pinned – No Translation.Click OK to create the constraint.Create a constraint normal to the pads.∙Repeat the previous command by pressing the Ctrl+y hotky.∙In the Entity Selection dialog box, set the Method to color and select one of the pad surfaces.Click the Preview button before clicking OK.In the Create Constraints on Geometry dialog box, set the Title to Mount Normal Constraints.Set the type to Surface – Allow Sliding only along Surface (Symmetry).Click OK to create the constraint.Create loads on the fitting.In the Model Info pane, right-click the Loads object, and select New.In the New Load Set dialog box, enter the 500 N Total Load and, then, click OK to create the constraint set.Create a force load on the fitting.∙Expand the newly created load set and right-click the Load Definitions object and select On Surface from the menu.∙Select the bend radius surface, then, click OK.∙In the Create Loads on Surfaces dialog box, set the Title to 500 N Bearing Load.Set the type to Bearing Force.Set the Magnitude to 500.Set the Load Angle to 15.Enable the option for Normal To Surface.Click OK to create the load.Save your Femap model.Step 7:Analyze the fitting and review resultsCreate an analysis set for linear statics.∙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 Bearing Load Linear StaticsSet the Analysis Program to 36..NX Nastran.Set the Analysis Type to 1..StaticClick OK to create the analysis set.∙Click the Analyze button.∙Once the analysis has complete, close the NX Nastran Analysis Monitor paneSave your Femap model.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 m Ply1 VonMises StressYour graphics display should be similar to below.。