Femap实例-中面建模及多载荷集分析

IntroductionIn this exercise, you will generate a midsurface model of a machined bracket. The steps to complete this exercise are:•Import geometry•Generate and edit midsurfaces•Assign mesh attributes, set mesh sizing and mesh the bracket•Create constraints and loads, including combined load sets•Analyse the bracket using a Multi-set analysis and view the stress results.Step 1:Import geometryImport the Parasolid geometry of the multi-thickness solid model.•Open a new FEMAP model.•Select the File, Import, Geometry command.•Select the Parasolid file ex13-Bracket_inches.x_t from your class Geometry folder.•Click OK to accept the defaults in the Solid Model Read Options dialog box.Change the view orientation to the Trimetric view.•Press the F8key (or use the View, Rotate, Model command) to open the View Rotate dialog box.•Select the Isometric button.•Click OK to close the dialog box.Save the model•Save the model in your class Exercises folder as “ex13-Bracket.modfem”.Step 2:Create midsurfacesExtract the midsurfaces from the solid.•Select the Geometry, Midsurface, Automaticcommand.•Click the Select All button to select all the surfaces on the solid.•In the Mid-Surface Tolerance dialog box, click the Measure Distance icon to enable measuring a 3-Ddistance. Ctrl+D can also be used to measure adistance from the graphics window while in acommand.•When the Locate –Define Location to Measure From dialog box is displayed, select one of the points onthe thickest edge of the sold. Set the Method to OnPoint and select one of the points shown below.•Click OK to confirm the selection of the first point.•Select the “other” point shown below that has not been chosen, then click OK to confirm the selection.•Click OK to accept the calculated distance, .156 in the Mid-Surface Tolerance dialog box. FEMAP willnow extract the mid-surfaces.Display the automatically generated Midsurfaces group.•In the Model Info pane, turn on “highlighting” by clicking the Show When Selected icon.•Expand the Group object in the tree and select1..Midsurfaces in the Model Info pane. This willhighlight the newly created group. Since we are onlyworking with a single part, you can delete the groupand the original solid.•Right-click 1..Midsurfaces and select Delete from the context-sensitive menu.•Expand the Geometry object in the Model Info tree, select 1..ex12-Bracket, and using the context-sensitive menu, Delete the original solid part.•Expand the view if needed with the Ctrl+A hotkey to “Autoscale”Note that the midsurfacing operation has generatedsplit lines in the midsurfaces that will be easily beremoved in the next step.Remove the split lines from the surfaces.•Select the command, Geometry, Solid, Cleanup.•Select All surfaces and click OK.•In the Solid Cleanup dialog box, accept the default option to Remove Redundant Surfaces and click OKto proceed with remove the split lines in the surfaces.Extend the surface representing the bend of the rib.•Switch your view orientation to the Front view.•Note that the bottom edge of bend surface doesnot intersect the surface representing the flange.•Select the command, Geometry, Midsurface, Extend.•Select the bottom edge of the bend surface in the Select Entity dialog box.Complete extending the surface representing the bend of the rib.•In the Surface Extend Options dialog box, leave the option for Extend Shape as Linear.•Using the Extend To –Solid option, select the Solid that represents the flange and click OK.Note that the blend surface now extends to theintersection with the flange.Trim the two surfaces representing the flat sections of the rib.You will use two different Geometry, Midsurfacecommands to do this, the first is to use the Trim with Curve operation and the second is use the Intersect operation.•Select the command, Geometry, Midsurface, Trim with Curve.•Select the flat surface of the rib closest to the back surface (the surface with the four mounting holes) inthe Solid/Surface to Trim dialog box and the clickOK.•In the Entity Select ion –Select Line(s) to Trim With dialog box, select the top edge of the rib and theedge of the blend surface intersecting the flat ribsection and click OK to confirm your selection.•With highlighting enabled in the Model Info pane, select the sheet solid of the rib section you justmodified and note how it has been sliced into threesurfaces.Continue with trimming the two surfaces representing the flat sections of the rib.•Select the command, Geometry, Midsurface, Intersect.•Select the two (2) surfaces that will represent the blend and the end of the rib then click OK togenerate the intersection.Delete the extraneous surfaces.•Select the command Delete, Geometry, Surfaces.•Select the small tab on the longer flat section of the rib and the two surfaces on the flat rib sections thatextend beyond the blend of the rib. Click OK todelete the surfaces.Stitch the surfaces together to create contiguous sheet solids.•Select the command Geometry, Solid, Stitch.•Select all the surfaces and click OK.•Click OK to accept the default Gap Tolerance.•Note how there are now three sheet solidsrepresenting the back face, web, and rib of thebracket.Intersect the surfaces to imprint the surfaces at the intersection of the three main features of the bracket.•Select the command Geometry, Midsurfaces, Intersect.•Select all the surfaces and click OK.•Again, using the Model Info pane, click the three sheet solids under the Geometry tree and note howthe surfaces have been imprinted using theintersection operation.Create Offset Curves around the six holes on thebracket.•If not displayed, active the Curves on Surfaces toolbar.•Click the Curve Washer icon on the Curves on Surfaces toolbar.•In the Define Washer or Offset Curves dialog box,set the Mode to Washer , enable the option for Save Split Lines and set the Offset to .125. Click OK to accept the settings.•Select one of the arcs on each of the six holes on thebracket and click OK .•Cancel out of the Curve Washer command.•After completing the Curve Washer operation, your model should appear as follows (shown with multiple windows to more clearly display the washers).Step 3:Assign mesh attributes, set mesh sizing and mesh the bracketAssign the mesh attributes (property) to themidsurfaces.•Select the Geometry, Midsurface, Assign Mesh Attributes command.•Press Select All the surfaces and click OK.•The Define Material –ISOTROPIC dialog box will open, prompting you for a material. Click the Loadbutton to open up the default material library.•In the Select from Library dialog box, select one of the Stainless Steel materials and click OK.•Click OK.•In the dialog box, click Yes to consolidate the properties by thickness.•Note that there are now two (2) properties that reflect the two different wall thicknesses of the part.Set the mesh size for the mid-surfaces.•Using the Select toolbar, set the Selector Entity to Surface and Selector Mode to Select Multiple .•Select all the surfaces by holding down the Shift keyto create a box picking region around the entire model.•In the graphics pane, right-click your mouse andselect Mesh Size from the context-sensitive menu.•In the Automatic Mesh Sizing dialog box, set the Element Size to .2 set the Max Angle Tolerance to15. Disable the Max Elem on Small Feature optionthen click OK to set the mesh size.Set the mesh size for the curves around the holes•Before meshing, turn on the mesh size indicators using the F6hotkey to open the View Options dialog box.•In the View Options dialog box, set the Category to Labels ,Entities and Color, enable the Draw Entityoption and set Show As to 3..Symbols and Count.Click Apply to update the display and once theoptions are displayed as below, you can close thedialog box by clicking either the OK or Cancelbutton.Set mesh sizes for the holes.•Using the Select toolbar, set the Selector Entity to Curve and leave the Selector Mode as SelectMultiple.•Select the curves surrounding the holes on the bracket to include the hole and the washer’s arcs,but not the split lines.•In the Model Info pane, expand the Selection List object .•Right-click the Curves object and select Mesh Size from the context-sensitive menu.•In the Mesh Size Along Curve dialog box, set the Number of Elements to 6 then click OK to set themesh size.Mesh the model.•In the Model Info pane, right –click the Surfaces object then select Mesh from the context-sensitivemenu.•Click OK in the Automesh Surfaces dialog box to mesh the model using the “Mesh Attributes”assigned to the surfaces in an earlier step.With mesh size symbols turned off and elementthickness display turned off, your model shouldappear similar to the following.Step 4:Create constraints and loads, including aCombined load setCreate the constraints on the back wall of the part.•In the Model Info pane, create a Constrain Set. Use a descriptive name for the title of the constraint set.•Expand the new constraint set and right-clickConstraint Definitions and select On Surface from the context-sensitive menu.•Select the eight (8) surfaces which represent the washers around the holes on the back wall of the bracket.•In the Create Constraints on Geometry dialog box,set the constraint to Pinned then click OK to create the constraints.•Again, right-click Constraint Definitions and select On Surface from the context-sensitive menu.Continue with creating the constraints on the back wall of the bracket.•Select the two (2) remaining surfaces on the back wall of the bracket and click OK.•In the Create Constraints on Geometry dialog box, set the constraint to Surface and choose Slidingalong Surface (Symmetry)then click OK to create the constraints.Create the loads on the holes on the left end of the bracket. To do this, you will create a Rigid elementconnecting the washers of the holes on the front of the bracket to a node at the center of the holes.•Select the command, Model, Element.•In the Define Plate Element dialog box, click the Type button an d select the Rigid element under theOther type.•Click the RBE2tab.•Click the New Node at Center button. Femap will then create the Independent node at the center ofthe selected Dependent nodes.•Click the Nodes button.•In the Entity Selection dialog box, change Methods^to on Curve and select the two curves making up one of the two holes on the web then Click OK to confirm your selection.•Create a second rigid element on the other hole byrepeating the previous two steps (New Node atCenter and selecting nodes on the two curves on the edge of the other hole).Create loads on the center nodes of the rigid “spider”elements in the holes.•Zoom in on the end of the bracket where you just created the rigid “spiders”.•From the Model Info tree, right-click the Loads object select New .•Enter a Title for the new Load Set as Front Web Hole Loading and click OK .•Expand the Load Set just created, right-click Load Definitions and select Nodal from the menu.•Select the node at the center of the front hole rigid element on the web then click OK .•In the Create Loads on Nodes dialog box, enter adescriptive name for the load, set the Load Type to Force , and set the Load value to FZ = 1.•Create a second load set and load at the node at the center of the read hole on the web by repeating steps b) through f) for the other hole. Set the Title for the second load set to Rear Web Hole Loading and click OK .Create a combined load set that will take the two previous load sets and by setting a scale factor, willcreate a combined load of 100 lbs in the negative Zdirection.•Select the command Model, Load, Combine.•In the Combine Load Data dialog box, set the Title to Combined 100 lb Web Hole Load.•In the From list, select both of the load sets you just created.•With both load sets selected, set the Scale Factor to -50.•Click the Add Combination button.•After the previous step, the Combinations section of the dialog box should appear as shown to the right.•Click OK to create the combined load set.•In the Model Info pane, right-click the combined load set you created and select Activate from the menu. Create a Nastran combined load set that will take the two previous load sets and by setting a scale factor, will create a combined load of 50 lbs in the positive Zdirection for the front hole and 50 lbs in the negative Z direction for the rear hole.•In the Model Info pane, right-click the Loads object and select New from the menu.•In the New Load Set dialog box, set the Title to a descriptive name similar to below.•For the Set Type, select Nastran LOAD Combination then click OK.•Select Reference Sets after right-clicking the newly created load set in the Model Info pane.•In the Referenced Loads Sets for Nastran LOAD dialog box, click the first load set under the Available Sets list field.•With the first load set selected, set the value For Referenced Set to 50then click the Add Referenced Set button.•With the second load set selected, set the value For Referenced Set to -50 then click the Add Referenced Set button. The Referenced Sets list field shouldappear as below.•Click OK to update the load set.Display the element thickness.•From the View toolbar, select the View Style pull down icon and select the Thickness/Cross Sectionicon to toggle on the display of the elementthickness.Step 5:Analyze the bracket and display stress resultsModify the Femap preference for Output Set Titles .•Select the command File, Preferences .•Select the Interfaces tab.•Under the Nastran Solver Write Options group, setthe Output Set Title option to 2..Nastran SUBTITLE .•Click OK to apply the changes to Femap’s preferences.Create an MultiSet Analysis Set and run the analysis.•Create an new analysis set for NX Nastran Linear Statics by right-clicking the Analysis object in theModel Info pane and select New.•Set the Title of the analysis set to MultiSet Linear Statics.•Expand the newly created analysis set to display Boundary Conditions.•Select Boundary Conditions then click Edit.Continue with creating the new analysis set for linear statics.•Set both the Constraints and Loads to None.•Click the MultiSet button.•In the Entity Selection –Select Constraint Set(s) to Generate Cases dialog box, click Select All thenOK.•In the Entity Selection –Select Load Set(s) to Generate Cases dialog box, click the Select fromList button.•In the Select One or More Load Sets(s) dialog box, select the two combined load sets, then clickOK.•Click OK to add the two load sets to the analysisset. The analysis set should now show two subcases as part of the analysis set.•Click the Analyze button in the Analysis Set Manager dialog box to start the analysis.•Close the NX Nastran Analysis Monitor when theanalysis completes and the results sets have been read into Femap.Review the results.•Activate the first results set by right-clicking on it in the Model Info pane.•Using the PostProcessing Toolbox, create a deformed contour plot of the Plate TopMajorPrin(cipal)Stress.•Set the Type to Elemental•Enable the option for Double-Sided Planar.•Save your model and exit Femap.。