SolidWorks Tutorial 2003 ANGLE-13HOLE The ANGLE

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SolidWorks Tutorial 2003ANGLE-13HOLEANGLE-13HOLE PartThe ANGLE-13HOLE part is anL-shaped support bracket. The ANGLE13HOLE part is manufactured from 0.090”[2.3] aluminum.There ANGLE-13HOLE part contains fillets, holes and slot cuts.Simplify the overall design into seven features. Utilize symmetry and LinearPatterns.The open L-Shaped profile is sketched onthe Right plane.Utilize an Extruded Thin feature with theMid Plane option to locate the partsymmetrical to the Right plane.Insert the first Extruded Cut feature for thefirst hole. The first hole is sketch on the topface of the Extruded Thin feature.Courtesy of SDC Publications www.schroff.comPage 1

SolidWorks Tutorial 2003Insert a Linear Pattern to create anarray of 13 holes along the bottomhorizontal edge.Insert a Fillet feature to round the fourcorners.Insert the second Extruded Cut featureon the front face of the Extruded Thinfeature.Courtesy of SDC Publications www.schroff.comPage 2ANGLE-13HOLE

SolidWorks Tutorial 2003Insert a Linear Pattern to create an arrayof 3 holes along the top horizontaledge.Utilize the Sketch Mirror tool tocreate the slot profile.Insert the third Extruded Cutfeature to create the two slots.Courtesy of SDC Publications www.schroff.comPage 3ANGLE-13HOLE

SolidWorks Tutorial 2003Create a New Part.1) Click Newfrom the Standardtoolbar. The Templates tab is thedefault tab. Part is the defaulttemplate from the New SolidWorksDocument dialog box.2)Click OK.3) Set the Dimensioning Standard and Part Units. ClickTools from the Main menu. Click Options.4) Click the Document Properties Tab.5) Select ANSI from the Dimensioning Standard list box.6) Click Units.7) Select Inches[Millimeters] forLinear units.8) Select 3 [2] forDecimal places.9) Click OK to setDocument units.Courtesy of SDC Publications www.schroff.comPage 4ANGLE-13HOLE

SolidWorks Tutorial 200310) Save the Part.Click File, SaveAs.11) Select SW-TUTORIAL for theSave in file folder.12) Enter ANGLE-13HOLE for Filename.13) Enter ANGLEBRACKET-13HOLE forDescription.14) Click the Savebutton.Insert an ExtrudedThin feature sketchedon the Right plane.Select the Sketchplane.15) Click Right fromthe Feature Manager.The Right plane isdisplayed as a vertical linein the Front view. TheRight plane name icon inthe FeatureManager isdisplayed in blue.Courtesy of SDC Publications www.schroff.comPage 5ANGLE-13HOLE

SolidWorks Tutorial 2003ANGLE-13HOLEInsert a new sketch.16) Click Sketchto insert asketch on theRight plane.17) Click Rightfrom theStandards viewtoolbar. TheRight planegreen boundaryis displayed inthe Right view.18) Click Linefrom the SketchTools toolbar.The cursordisplays the Linefeedback symbol.19) Sketch ahorizontal line.Click the Origin. Click a position to the right of the Origin. Thecursor displays the Horizontal feedback symbol.20) Sketch a vertical line. Click a position directly above theright end point. The cursor displays the Line feedbacksymbol.Courtesy of SDC Publications www.schroff.comPage 6

SolidWorks Tutorial 2003ANGLE-13HOLEAdd Relations.21) Click Add RelationsCurrent lineselected.The vertical line, Line2 isdisplayed in the SelectEntities box.22) Click thehorizontal line,Line1.23) Click the Equalbutton.24) Click OKto add an Equalrelation.Add Dimensions.25) Click Dimension.26) Click the horizontal line.27) Click a position below the profile.28) Enter .700 [17.78] in the Modifydialog box.29) Click the Check Mark. Theblack sketch is fully defined.Courtesy of SDC Publications www.schroff.comPage 7

SolidWorks Tutorial 2003ANGLE-13HOLEExtrude the sketch.30) Click ExtrudedBoss/Basefrom the Featurestoolbar.31) Select Mid Planefor Direction1 EndCondition.32) Enter 7.000[177.80] forDepth. The ThinFeature box isdisplayed.33) Click the ReverseDirection Arrowbutton for OneDirection.Material thicknessis created abovethe Origin.34) Enter .090 [2.3]for Thickness.35) Check Auto-fillet corners.36) Enter .090 [2.3] for Fillet Radius.37) Click OKto insert an Extrude-Thin feature.38) Fit the model to the Graphics window. Press the f key.39) The Extrude-Thin1 feature is displayed.Courtesy of SDC Publications www.schroff.comPage 8

SolidWorks Tutorial 2003ANGLE-13HOLEModify featuredimensions.40) Double-clickExtrude-Thin1in the Graphicswindow.41) Double-click7.000 [177.80]dimension.42) Enter 6.500[165.10] in theModify dialogbox.43) Click theCheck Mark.44) Click Rebuildfrom theMain toolbar toupdate thefeaturedimensions.Insert a new sketch for theExtruded Cut.45) Select the sketchplane. Click the topface of the ExtrudeThin1. The cursordisplays the Facefeedbacksymbol.46) Click Sketch.47) Click Topfromthe Standards viewtoolbar.Courtesy of SDC Publications www.schroff.comPage 9

SolidWorks Tutorial 200348) Click Circlefrom theSketch Toolstoolbar.49) Sketch acircle on theleft side of theOrigin.Add dimensions.Create a horizontaldimension.50) Click the Origin.51) Click the centerpoint of the circle.52) Click a positionbelow thehorizontal profileline.53) Enter 3.000[76.20].54) Create a vertical dimension.Click the bottomhorizontal line.55) Click the center point.56) Click a position to the leftof the profile.57) Enter .250 [6.35].58) Create a diameterdimension. No number59) Click the diameter of thecircle.60) Click a position above theprofile.61) Enter .190 [4.83].Courtesy of SDC Publications www.schroff.comPage 10ANGLE-13HOLE

SolidWorks Tutorial 2003ANGLE-13HOLEInsert an Extruded Cut.62) ClickExtruded Cutfrom theFeaturestoolbar.63) SelectThrough Allfor Direction1End Condition.64) Click OKto insert the Extruded-Cut feature.Create a Linear Pattern.65) Click Linear Patternfrom theFeatures toolbar. The Cut-Extrude1is displayed in the Features to Patternbox.66) Select the bottom horizontal edgeof the Extrude Thin1 feature forDirection1. Edge 1 is displayed inthe Pattern Direction box.67) Enter 0.5 [12.70] for Spacing.68) Enter 13 for Number of Instances.69) The Direction arrow points to theright. Click theReverseDirectionbutton ifrequired.70) Click OKtoinsert a LinearPattern.Courtesy of SDC Publications www.schroff.comPage 11

SolidWorks Tutorial 200371) ClickIsometric.72) Save theANGLE13HOLEpart. ClickSave.Insert Fillet feature.73) Click Zoom to Area. Select the rightside of the ExtrudeThin feature.74) Click Filletfromthe Features toolbar.75) Enter .250 [6.35] forFillet Radius.76) Select the two smalledges. Edge 1 andEdge 2 are displayed in Fillet box.77) Click OKtocreate the Fillet.Combine Fillets of thesame size.Edit the Fillet featureand add two left edges.Courtesy of SDC Publications www.schroff.comPage 12ANGLE-13HOLE

SolidWorks Tutorial 2003Edit the Fillet feature.78) Click Zoom to Area. Selectthe left side of the Extrude Thinfeature.79) Right-click Fillet1 in theFeatureManager.80) Click Edit Definition.81) Select the two left small edges.Edge 3 and Edge 4 aredisplayed in the Fillet box.82) Click OKtoupdate the Fillet.Display theIsometric view.83) ClickIsometric.84) Save theANGLE13HOLE part.Click Save.Courtesy of SDC Publications www.schroff.comPage 13ANGLE-13HOLE

SolidWorks Tutorial 2003ANGLE-13HOLEInsert a new sketch for the secondExtruded Cut.85) Select the sketch plane. Clickthe front face of the ExtrudeThin1. The cursor displays thefeedback symbol.Face86) Click Sketch.87) Click Frontfrom theStandards view toolbar.88) Click Hidden Lines Visiblefrom the View toolbar todisplay the Linear Pattern1feature. Do not align the centerpoint of the circle with thecenter point of the LinearPatter1 holes. The center pointis position is controlled withdimensions.89) Click Circlefrom theSketch Toolstoolbar.90) Sketch acircle on theleft side of theOriginbetween twoLinearPattern1holes.Linear Pattern1 HolesCourtesy of SDC Publications www.schroff.comPage 14

SolidWorks Tutorial 2003Add dimensions.91) Create a horizontaldimension. Click theOrigin.92) Click the center point ofthe circle.93) Click a position belowthe horizontal profileline.94) Enter 3.000[76.20].95) Create a verticaldimension. Click thetop horizontal line.96) Click the center point.97) Click a position to theleft of the profile.98) Enter .250 [6.35].99) Create a diameterdimension. Click thediameter of the circle.100)Click a position above the profile.101)Enter .190 [4.83].Insert an Extruded Cut.102)Click Extrudedfrom theCutFeatures toolbar.103)Select ThroughAll for Direction1End Condition.104)Click OKtoinsert the ExtrudedCut feature.Courtesy of SDC Publications www.schroff.comPage 15ANGLE-13HOLE

SolidWorks Tutorial 2003ANGLE-13HOLECreate the secondLinear Pattern.105)Click Topfrom theStandards viewtoolbar.106)Click LinearfromPatternthe Featurestoolbar. The CutExtrude2 isdisplayed in theFeatures toPattern box.107)Select the tophorizontal edgeof the ExtrudeThin1 feature forDirection1.Edge 1 isdisplayed in thePattern Directionbox.108)Enter 3.000[76.20] forSpacing.109)Enter 3 for Number of Instances.110)The Direction arrow points to theright. Click the Reverse Directionbutton if required.111)Click OKto create the LinearPattern.112)Click Isometric.113)Save the ANGLE-13HOLE part.Click Save.Courtesy of SDC Publications www.schroff.comPage 16

SolidWorks Tutorial 2003ANGLE-13HOLEInsert a new sketch for the thirdExtruded Cut.114)Select the sketch plane. Clickthe front face of Extrude Thin1.115)Click Sketch.116)Click Frontfrom theStandards view toolbar.117)Sketch a verticalcenterline. ClickCenterlinefromthe Sketch Toolstoolbar.118)Click the Origin.119)Click a verticalposition above the tophorizontal line.120)Click Sketch Mirrorfrom the SketchTools toolbar.Two sets of parallel linesare displayed on thecenterline.The centerline is a line of symmetry.Courtesy of SDC Publications www.schroff.comPage 17

SolidWorks Tutorial 2003ANGLE-13HOLE121)ClickRectanglefrom the SketchTools toolbar.Sketch sideMirror side122)Do not alignthe rectanglefirst point andsecond point tothe centerpoints ofLpattern1.Click the firstpoint of therectangle to theleft of theOrigin.FirstpointSecondpoint123)Click thesecond pointof the rectanglediagonally fromthe first point, tothe left of theOrigin. Asecond sketchis created onthe Mirror sideof the centerline.124)Trim the vertical lines. Clickfrom theSketch TrimSketch Tools toolbar.Trim Vertical Lines125)Click the two vertical lines ofthe left rectangle.126)Click the twovertical line ofthe rightrectangle.Courtesy of SDC Publications www.schroff.comPage 18

SolidWorks Tutorial 2003ANGLE-13HOLE127)Sketch the right arc on the left side of the centerline. Click Tangent ArcTools toolbar.from the Sketch128)Drag the mouse pointer along the top horizontal line tothe right. A dotted horizontal line is displayed.129)Click the top right endpoint. Drag the mouse pointerto the right and downward. Click the bottom rightendpoint. The cursor displays the Coincident to pointfeedback symbolat each endpoint.130)Sketch the left arc on the left side of the centerline.Drag the mouse pointer along the top horizontal lineto the left. A dotted horizontal line is displayed.131)Click the top left endpoint. Drag the mouse pointerto the right and downward. Click the bottom leftendpoint. The cursor displays the Coincident topoint feedback symbolat each endpoint.Courtesy of SDC Publications www.schroff.comPage 19

SolidWorks Tutorial 2003ANGLE-13HOLEThe two sketchedarcs aredisplayed on theMirror side.132)DeactivateSketch arcMirror arcSketch Mirror.Click SketchMirror.Add Relations.133)Zoom in on thecenterline.134)Press the Shift z key,approximately 3 times.135)Click Add Relation.136)Select the topendpoint of thecenterline.137)Select the circle.138)Click Concentric fromthe Add Relations box.The endpoint of the centerline ispositioned in the center of the circle.Note: Right-click Clear Selectionsto remove selected entities from theAdd Relations box.Courtesy of SDC Publications www.schroff.comPage 20

SolidWorks Tutorial 2003139)Click Add RelationANGLE-13HOLE.140)Select the circle.141)Select the left arc.142)Click Equal from the Add Relations box.The arc radius is equal to the circle radius.143)Select the top endpoint ofthe centerline.144)Select the left center pointof the left arc.145)Click Horizontal from theAdd Relations box.146)Click OKto add aHorizontal relation.The right arc is horizontally aligned to the left arc due to symmetry from theSketch Mirror tool.Dimension the slots.147)Click Dimension.148)Dimension the leftslot. Click the leftcenter point ofthe left arc. Clickthe right centerpoint of the rightarc.149)Click a positionabove the tophorizontal line.Courtesy of SDC Publications www.schroff.comPage 21

SolidWorks Tutorial 2003ANGLE-13HOLE150)Enter 2.0 [50.80] in the Modify dialog box.151)Click the Check Mark.152)Dimension thedistance betweenthe two slots. Clickthe right arc of theleft slot.153)Click the left arc ofthe right slot.154)Click a positionabove the tophorizontal line.155)Enter 1.000 [25.40]in the Modify dialogbox.156)Click the CheckMark. The black sketch is fully defined.Insert an Extruded Cut.157)Click Extrudedfrom theCutFeatures toolbar.158)Select ThroughAll for Direction1End Condition.159)Click OKtocreate theExtruded-Cutfeature.160)Click Isometric.161)Save theANGLE-13HOLEpart. Click Save. The ANGLE13HOLE iscomplete.Courtesy of SDC Publications www.schroff.comPage 22

SolidWorks Tutorial 2003ANGLE-13HOLENote: The dimension between the two slots is over-defined if the arc center pointsare aligned to the center points of Lpattern1.Review the ANGLE-13HOLE Part.The ANGLE-13HOLE utilized an open L-Shaped profile sketched on the Rightplane. The Extruded Thin feature with the Mid Plane option located the partsymmetrical to the Right plane.The first Extruded Cut feature created the first hole sketched on the top face of theExtruded Thin feature.The first Linear Pattern created an array of 13 holes along the bottom horizontaledge.The Fillet feature rounded the four corners.The second Extruded Cut feature created on the second hole sketched on the frontface of the Extruded Thin feature.The second Linear Pattern created an array of 3 holes along the top horizontaledge.The third Extruded Cut feature created two slot cuts sketched with the SketchMirror.Courtesy of SDC Publications www.schroff.comPage 23

SolidWorks Tutorial 2003ANGLE-13HOLEExerciseCreate the ANGLE BRACKET Part. The Base Extrude feature is sketched withan L-Shaped profile on the Right Plane. The ANGLE BRACKET Part ismachined from 0.060 [1.5mm] Stainless Steel flat stock. The default units areinches.Courtesy of SDC Publications www.schroff.comPage 24

SolidWorks Tutorial 2003 ANGLE-13HOLE ANGLE-13HOLE Part The ANGLE-13HOLE part is an L-shaped support bracket. The ANGLE- . Courtesy of SDC Publications www.schroff.com Page 1 . SolidWo

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