Femap轴承载荷_BearingLoad

IntroductionIn this exercise, you will create and compare the results of a load applied to the edge of a hole using two different types of load distributions. In this exercise, you will complete the following steps:∙Open an existing model file∙Create a Cylindrical Coordinate System for the hole on the plate∙Apply a 100 lb. load on a curve∙Using a Data Surface apply a 100 lb. bearing load on a curve in a separate load set∙Expand the bearing load and set the load vectors to scale by magnitude∙Set up and run a Multi-Set analysis∙View and compare the results from the two analysesStep 1:Open an existing model fileIn this step you will open an existing model file and save it in your Exercises folder.Start Femap.∙Select the File, Import, Femap Neutral command.∙In the Read Model from Femap Neutral dialog box, select the file, ex7-Bearing Load - inches.NEU fromyour class files Geometry folder.∙Click the Open button.∙Your model should appear as follows:Save the file in your exercises folder.∙With the File, Save As command, save the model as ex5-bearing.mod in your training class exercisesfolder.Step 2:Create a cylindrical coordinate system for the large hole on the plate.Create a coordinate system for the large hole.Zoom in around the large hole on the right side of the plate.∙Click the Zoom icon on the View toolbar.∙Click and drag your mouse so that the right side of the plate will be displayed in your graphics window.Create a new cylindrical coordinate system.∙In the Model Info pane, right-click the Coordinate Systems object and select New from the context-sensitive menu.∙In the Define Coordinate System dialog box, enter: ID = 101Title = HoleMethod to XY LocateType to CylindricalClick OK to continue with creating the newcoordinate system.∙In the Locate – Define Coordinate System Origin dialog box, click the Methods button and selectCenter from the menu.∙Select the right edge of the large hole (Curve ID = 101) and click OK to confirm your selection.∙In the Center – Define Location on CSys X-Axis dialog box, click the Method button again and select Locate from the menu.∙Since the default “snap mode” for Femap is set to screen, right-click your mouse in the graphicswindow and select Snap to Point from the pop-upmenu.Select the start point on the bottom of the arc as the locator for the vector defining the X-axis of thecoordinate system and click OK.∙The third point locates a point on the positive X-Y plane of the new coordinate system. Click theMethods button again in the Locate – DefineLocation in CSys X-Y Plane and click Midpoint. ∙Select the right edge of the large hole (ID = 101) and click OK to create the cylindrical coordinate system.∙Click Cancel or use the Esc key to exit the command after the coordinate system is created.Step 3:Create a 100 pound load on a curve.Before creating loads, you must create a Load Set for the load(s).Create the load set.∙In the Model Info pane, expand the Model object.∙Right-click Loads and select New from the menu.This is same action as selecting the Model, Load,Create/Manage Set command.∙In the New Load Set dialog box, enter the name as Curve Load.∙Click OK to create the load set.Create the load.∙Expand the Loads object, then the Curve Load set in the Model Info pane.∙Right-click Load Definitions and select On Curve from the menu.This is the same action as selecting the Model, Load, On Curve command.Select the right side of the large hole (Curve ID = 101) and click OK to confirm your selection.Remember that you can use the Preview Selectedicon in the Select dialog box to confirm that youselected the correct entity or entities beforeconfirming your selection with the OK button.In the Create Loads on Curves dialog box, set the Title to 100 lb. in +X and the following:Set the load type as Force.Set the Coord Sys to 1..Basic Cylindrical.Enter 100 in the FX field. You can optionallydeselect the FY and FZ checkboxes.Click OK to create the load.Step 4:Create a 100 lb. bearing load on a curve using a Data Surface.In this step, you will create a new load set, an Equation Data Surface and use that data surface to create a distributed bearing load on the same curve that you used in the previous step. You will also use the Tools, Check, Sum Forces command to list the value of the load and adjust the load to achieve a 100 lb total load on the curve.Create a new load set.∙In the Model Info pane, expand the Model object.∙Right-click Loads and select New from the menu.∙In the New Load Set dialog box, enter the name as Bearing Load.∙Click OK to create the load set.Create an Equation Data Surface. The first step is to open the Data Surface pane.∙Select the Tools, Data Surface Editor command.∙Undock the Data Surface Editor pane and expand it so that you can clearly see the contents of the newdata surface that you will create.∙In the Data Surface Editor pane, click the Create Load Data Surface icon and select Equation DataSurface.In the Define Equation dialog box, enter the Title as Sinusoidal Load Distribution and the following:CSys for Data: 101..HoleEquation: abs(sin(!y))Click OK to create the data surface.Create the bearing load.∙Expand the Loads object, then the Bearing Load set in the Model Info pane.∙Right-click Load Definitions and select On Curve from the menu.∙Select the same curve you did when you created the previous 100 lb. load.In the Entity Selection dialog box, click the Previousbutton to reselect the curve on the large hole andclick OK to complete the selection.∙In the Create Loads on Curves dialog box, set the Title to 100 lb Bearing Load and the following:Set the load type as Force Per Node.For the Direction, select the Components button.Under the Load section, uncheck FY and FZ, and set the Value of FX = 1.0.Set the Method to Data Surface and for the DataSurface for FX, select 1..Sinusoidal Load Distribution.∙Click OK to create the load.Note: The load applied to each node on the curve will be the value of the FX times the value ofthe Data Surface equation at each node. Thenext step will sum all the values of theindividual forces on each node and then youwill adjust the value of FX to achieve a totalload of 100 lbs. on the curve.Determine the total value of the load.∙Select the Tools, Check, Sum Forces command.∙In the Locate – Enter Location to Sum Forces About dialog box, click OK to use the default location of0,0,0.∙In the Sum Forces dialog box, use the default Coord Sys of 0..Basic Rectangular.∙Click OK to confirm your selection.∙In the Messages pane, the load listing shows a radial load (Fx direction) of 15.2571 in the cylindricalcoordinate system (CSys 1):∙Select the value of FX in the Messages pane(15.2571) and either use the right-mouse to openthe context-sensitive menu and Copy the value oruse the Ctrl+c hotkey to copy the value.Adjust the value of the load so that the total value of the load is 100 lbs.∙In the Model Info pane, expand the Load Definitions object under the Bearing Load load set.∙Right-click 100 lb Bearing Load to select the Edit Load operation from the context-sensitive menu.∙In the Editing Load Definition dialog box, change the value of FX to 100/15.2571. You can use the Ctrl+vkey to paste the value of 15.2571 from theMessages pane.∙Click OK to complete editing the load.Run the sum forces command again to confirm that the total load is 100 lb.∙Select the command, Tools, Check, Sum Forces.∙Click OK to compute sum of the applied loads.Note that the total force applied to the hole is now99.9997 lbs. You can adjust the load further if youwant to achieve a 100 lb load exactly.Step 5:Expand the load to see the actual loads on each nodeSince the load has been applied to the curve, the load on each node is not visible until the load is expanded. This occurs automatically when you create an Analysis Set and export an analysis file or run the analysis. In this step, you will manually expand the load set to see the individual loads on the nodes.Expand the load.∙Select the Model, Load, Expand command.∙Click OK to continue.Note: If you want to permanently convert the loads from "Geometry-based" to "Nodal andElemental based" loads, you can choose theConvert To Node/Elem option in the ExpandGeometric Loads dialog box.When you choose this option, the Femapdialog box appears with a prompt topermanently convert loads. In the FEMAPdialog box, click Yes to expand the load.This option should only be used once yourloading conditions have been finalized andeven then is not a required step to export theloads properly for analysis.Turn off the display of the elements and scale the loads by magnitude.∙In the Entity Display toolbar, click the ViewElements Toggle icons to turn the elements off inthe display.Change the display of loads using the View Options dialog box.∙With the F6 hotkey, open the View Options dialog box.∙In the View Options dialog box, set the Category to Labels, Entities and Color.For Options, select Load Vectors.For Vector Length, select 1..Scale by Magnitude.Click Apply (not OK) to update your display.Change the Options to Load Vectors.Set the Label Mode to Load Value.Click OK to apply the changes and to close the View Options dialog box.Your model should appear as follows:Step 6:Set up and run a MultiSet Linear Statics simulation.In this step, you will set up and run a MultiSet analysis with the Analysis Set Manager.Create a new analysis set.∙In the Model Info pane, right-click the Analyses object and select Manage from the menu.∙In the Analysis Set Manager dialog box, click the New button.∙In the Analysis Set dialog box, set the Title to Load Type Comparison.Leave the Analysis Program as 36..NX Nastran andthe Analysis Type as 1..Static.Click OK to create the new analysis set.Edit the analysis set to set up a multi-set simulation.∙In the Analysis Set Manager dialog box, expand the Master Requests and Conditions, and the BoundaryConditions and Output Requests subtrees.∙Select Boundary Conditions and click the Edit button.∙In the Boundary Conditions dialog box, set both the Primary Sets Constraints and Loads to 0..None.Click OK to apply the changes.∙Click the MultiSet button in the Analysis Set Manager dialog box.∙In the Entity Selection – Select Constraint Set(s) to Generate Cases dialog box, click Select All andthen OK.∙In the Entity Selection – Select Load Set(s) to Generate Cases dialog box, click Select All andthen OK.∙Note that in the Analysis Set Manager dialog box, there are now two sub cases, one for thecombination of the Fixed Holes and Curve Load sets and and second for the combination of the FixedHoles and Bearing Load sets.∙Click the Done button to close the dialog box.Before you analyze the model, you will set your Femap preferences so that the title of the results is the title of the NX Nastran subcase.∙Select the File, Preferences command.∙Select the Interfaces tab in the Preferences dialog box.∙Under the Nastran Solver Options group, set the Output Set Titles to 2..Nastran Subtitle.Click OK to apply the changes and to close thedialog box.Run the NX Nastran simulations.∙On the Model toolbar, click the Analyze Model icon.This is the same action as clicking the Analyzebutton in the Analysis Set Manager dialog box.∙After the previous step, the NX Nastran Analysis Monitor pane is opened and the log file for the NXNastran simulation is displayed.∙Once the analysis is completed and both results sets are loaded into your Femap model, you canclose the Analysis Monitor pane.∙Expand the Results object in the Model Info pane.Note how you have two results sets, one for eachsub case with the title the same as the sub casename.∙Right-click the result set 1..FIXED HOLES – CURVE LOAD and select Activate from the context-sensitive menu.Note: Femap automatically activates the last result set loaded into the model.Step 7:Compare the results of the two simulations.In this step you will toggle between the two output sets to see the subtle differences between the results due to the difference in the load distributions.Display a deformed contour of the Von Mises stresses.∙In the Femap graphics window, right-click your mouse to display the context sensitive menu andselect Post Data.∙In the Select PostProcessing Data dialog box, set the options as below and click OK.On the Post toolbar, click the Select a Deformed View and the Select a Countour View icons.Since the deformed shape is highly distorted, you will change the deformed display from displaying themaximum deformation as a percent of the viewwindow size to a scaled view of the actualdeformation.∙On the Post toolbar, click the Post Options icon and select Actual Deformation from the menu.∙Again, click the Post Options icon on the Post toolbar and select Scale Deformation.∙Set the value of the Actual scale to 1000.Your view should now appear as follows:Note that the maximum deformation is .00039.Switch to the FIXED HOLES – BEARING LOAD output set.∙Click the Switch to Post Data to Next Output Seticon on the Post toolbar.∙Note that the stresses are higher at the midpoint of the right edge of the hole and that the maximumdeformation is now .00044.Save your model and exit Femap. You will use this model in a future workshop.。