# Laboratory Demonstration Exercises

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1 Laboratory Demonstration Exercises 3-1

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5 Lab Demo 2 3 View Drawings and Dimensions If your computer is already logged on, take the time to do a Restart. This cleans the area and protects your memory devices. From the server (network neighborhood MELAB02 ME 152) copy the landscape title block drawing and th elabdemo2 folder over to the ThawSpace drive. Open SolidWorks, new, part. Right Plane, sketch, right view. If the grid is showing, right click in work area and deselect display grid. Starting to the left of origin on same level, draw an approximate 1.5 x 4 inch vertical rectangle. Esc click on bottom line and control click the origin. Make a midpoint relation. This ties the part to the origin. Dimension bottom 1.5 in and height 4 inch. Extrude Base, midplane, 5 inch. OK. Type f to fit drawing on screen. Rename Block Right click on front face, sketch, front view. Circle draw a 1.5 in radius circle on face. Dimension diameter 3 inch, center 2 inch from bottom and 2 inch from left side. Cut through all. Rename Hole. Check Point 1. File: Save as LabDemo2 Click on top face, sketch, top view. Line draw vertical line from one side to another about 1/3 of the way from the left edge. Right click, center-point arc, click on mid point of line, move mouse down, click on bottom, then drag to left and up around to the top of the line to get half circle. Dimension line 2 inch from left side. If the circle had its center at the line s midpoint it will be fully defined. Extrude-Boss; blind, 2 inch. Go to isometric view to make sure in right direction. OK. Rename Cap. Click on front face, sketch, front view. Line. Draw from upper right corner to base of cap, up 1.5 inch and back to start. Dimension the top of the triangle.5 inch below the top of the cap. Extrude-Boss, Change blind to up to vertex. Go to isometric view and click on vertex where cap intersects the block on the far side. OK. Rename Triangle. Check Point 2. Save file. Click on Top plane: insert reference geometry - plane. Set distance to 2 inch. A new plane should be seen above original plane. OK. Click on new plane, sketch, top view. Rectangle. Draw a 1 x 2 inch rectangle down and away from the lower right corner. Dimension width 1 inch height 2 inch. Center line, draw CL horizontally from origin. Feature Tab: Cut/Revolve. Set angle to 180. Go to isometric to check if it is the bottom arc. OK. Rename Curve-Cut. View: Plane to shut off the plane display. Select Fillet icon. Set radius to.4 in. Show hidden lines. Pick three square edges. One of the corner lines will be a hidden line. Rename Rounds. OK. Change display back to shaded with edges. Check Point 3. Save file. File/Save as LabDemo2. (Leave Open) File/Open. Open Landscape titleblock. File/Save As LabDemo2. (Always rename title block as soon as it is opened.) In left toolbar select Standard 3 View icon. Select LabDemo2 in the property manager, then click on the check mark. A 3 view drawing is shown on the title block. Right Click in white area of drawing and select Properties. Set default scale to 1:2 if it is not already set as such. View: Origins to shut off the origin display in the drawing. Click on top view. With mouse on edge of green border click and drag closer to front view. Bring right view closer to front view. Click on front view and move all three to the center of the paper. Note that the top and right views are linked to the front view so they move with it. The top view only moves up or down and the right view only moves right-left. 3-5

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8 Lab Demo 3 - Alignment Jig Open a new part. View: Origins. Tools: Options: Document Properties: Units: Select MMGS: # Decimals 1: OK. Front Plane: Sketch. Line: Starting at origin draw line up 35 mm, left 30 mm, down 75 mm, right 175 mm, up to level with origin close sketch. Smart dimension: total height 75 mm, length 175 mm, width of L 30 mm height above origin 35 mm. Extrude boss/base 100 mm, mid plane: OK. Rename feature to L Base. Front Face: Sketch: Front View. Rectangle Tool: Starting on right edge about 1/4 way down, draw down & to left about the same distance above the bottom. Smart Dimension: Make width 25 mm, top of rectangle 10 mm from top corner, bottom edge, 10 mm above bottom corner. Isometric View: Extrude Cut: Through All: OK: Rename Right Notch. Check Point 1: Save as: LabDemo3. Front Face: Sketch: Front View. Circle Tool: Draw circle in arm of L. Smart Dimension: Click on Left Edge, click on circle: 15 mm, click on top edge: click on circle: 17.5 mm: click on circle: move cursor to get leader line: set dimensions: diameter 20 mm. Isometric View: Extrude Cut: Through All: OK: Rename Left Hole. Select right face upright of L: Sketch: Right View. Rectangle Tool: Starting on top edge, 1/4 way from left edge, draw rectangle down & to the right. Smart Dimension: Set vertical edges 20 mm from each outside edge and height of rectangle 17.5 mm. Isometric View: Extrude Cut: Through All: OK. Rename Left Notch. Check Point 2: Save file. Select wide top surface: Sketch: Top View: Rectangle Tool: Draw rectangle centered on top edge and another one centered on bottom edge. Escape: Click on left vertical edge of one rectangle, control click, make them collinear and equal: Make right edges collinear. Smart Dimension: Make left edge of rectangle 50 mm from intersection of surface and L vertical: Width 40 mm, and depth into surface 15 mm. Isometric view: Extrude Cut: Blind: 20 mm down. OK Rename Steps. Select wide top surface: Sketch: Top view: Center Line Tool: Draw line from center of one step edge to center of other step edge. Tools: Sketch Entities: Polygon: Six sides. Set center of hexagon at center of center line just drawn. Drag to right and set hexagon. Smart Dimension: Diameter of inscribed circle 35 mm. Escape: Click on center of hexagon: click on right vertex of hexagon: Horizontal. Extrude Cut: Blind: 10 mm. OK. Rename Hexagon. Check Point 3: Save Part. Select bottom of hexagon: Sketch: Top View: Center Line. Draw a diagonal line from one vertex to opposite vertex. Circle Tool: Set center of circle at center of center line: draw circle. Smart Dimension: diameter 10 mm. Extrude Cut: Through All: OK. Rename Through Hole. Select wide top surface: Sketch: Top View: Line Tool: Draw vertical line on surface between origin and hex hole: Right click: Tangent Arc: Draw half circle to right at top of line: Right Click: Line: Draw vertical line down to even with start point: Right Click: Tangent Arc: Close figure. Center Line: Draw center line between centers of arcs. Escape: Center Line: Draw center line from origin to center of line just drawn. Escape: Select line just drawn: Horizontal. Smart Dimension: Arc radius 10 mm. Click on one arc: click on 3-8

10 and move cursor without clicking to the left clear of the body to get a dashed blue line. This indicated that the center line is aligned with the origin. Click and drag a line completely across the top view. Escape. Select the note icon in the Annotations Tool Bar (the big blue A.) Click above the center line to set note. In the Property Manager select the Add Symbol Icon. Select center line marking and click OK. Place q marking near center line. View: Origins to turn origins back off. In right view, move the 17.5 into slot and move both 20 mm dimensions closer to body to clean it up. Set the 100 mm width below the view. To complete the title block, right click on Sheet1 in the Feature Manager and select Edit Sheet Format. The drawing will disappear. Double click on Name: without moving mouse, place the cursor the right and type in your name. The title is Alignment Jig, Drawing # is 25486, Tolerance ±0.1, Next Assembly is 35492, Units are Millimeters, Scale is 1:2, add today s date. For material add Cast Stainless Steel. Since this does not fit in box, highlight the entire lie and reduce font size to 10 pt. Add your section numbers at the top of the sheet. Finally right click in the middle of the sheet and select Edit Sheet. Save sheet. 3-10

12 Click in empty part of drawing to deselect everything. Annotation Tab: Model Items: set Source to Entire Model: OK to get dimension in section view. Tools Options Document Properties Dimension Uncheck Add parentheses by default. Units three decimals. OK. In section view right click on lower.25 diameter: Display Options: Display as Radius. Clean up other dimensions and extension lines. Dimension the hole center circle in top view. Right click on dimension: Display as Diameter. In Dimensions Text box type in B.C. before the dimension. (B.C. stands for bore center.) Annotations Tab: Hole Callout. Click on the counter bore hole at ten o clock in the top view. In Property Manager delete Thru All modifier <hw thru> at the end of the first line. Set cursor to start of dimension. Type in 12X, if it is not present. Place call out. Check Point 4 Click on layer manager: new layer: name it GDT: color green: OK. Using the mouse wheel zoom to enlarge the front section view. Escape: Click on bottom line between O ring groove and the counterbore. Annotations Tab: Datum Feature: Label A: Click in drawing to set datum identifier. OK. Click on top between counterbore and hole: Geometrical Tolerance Icon: Symbol: Parallelism: Tolerance1:.005: Primary A: On second line setsymbol to flatness, Tolerance 1 to.004: Set GDT box. OK Select the left vertical line on the big inner circle: Geometrical Tolerance icon: Symbol: circularity: tolerance 1:.002: Set GDT box. OK. Change layer back to None. To add center lines to the holes in the section view, Annotations Tab: Center Line. Click first on one side of a sectioned hole, then the other side. Repeat with all parts of the sectioned holes. Escape: Set layer back to GDT layer. When putting in a perpendicular GDT, one may not select the centerline to attach the leader. Click on the horizontal line at the top of the hole close to the center line to select it. Geometrical Tolerance Icon: Symbol: Perpendicularity: Tolerance1:.003: Primary A: Set GDT box. OK. Move the SECTION AA Note back to near the sections view where it does not interfere with any of the dimensions. Right click on Sheet Format1: Edit Sheet: Double click on Drawing #: add 5974 : OK: Repeat to fill in other title block entries: right click Sheet1: Edit Sheet to get drawing back: Save drawing. Check Point 5 3 : 12

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15 labdemo5, OK, Front View. Set Front view in drawing, move cursor up and set top view. Esc. Select front view: make hidden lines visible. Right click in drawing: properties: scale: 1:4. View: Origins. Activate front view: center line: tickle origin, pull mouse down to get dashed blue guide line: draw a center line vertically through body center from one side of purple box to the other. View Layout Tab: Click on section view: set right view section and adjust directions as necessary. (Note: The sectioning is done with the None layer selected.) Origins Off. Hidden lines removed for section view. Model View: LabDemo5: Next (blue arrow):isometric view: click in drawing to set view: hidden lines removed. Click on auxiliary view: click on top angled face in right sectioned view: drag up to open area and place auxiliary view. Remove Hidden Lines. Create a new layer dimensions, color blue. Deselect all views: Annotation Tab: Model Items/ Set Import From to Entire Model, In dimension box select Hole Wizard Locations and Hole Callout. OK: Zoom in on auxiliary view. Tools Options Document Properties Dimensions: Uncheck Add parentheses by default : Annotation Fonts: Dimensions: Font: Points: 10: OK: Arrows : 0.2 : OK Click on 1.25 dimension: In Property manager place cursor before <DIM> and select the square symbol o from the list below. Move dimensions around so that they are clear and placed off the body. Shift drag the 1.00 dimension to Right View and the 3.00 dimension to Front View. Select 3.81 dimension: In dimension property manager select Leader Tab: Make first arc condition Max: OK Select right view: Move 30 from part. Set all dimensions off body in an orderly fashion and adjust extension lines as necessary. Check Point 6. Save If Hole Wizard Locations and Hole Callout buttons were not turned on when the dimensions were brought in you will have to do it manually now. Click on the hole call-out icon. Click on one of the clearance holes in the auxiliary view and set the leader. With the Smart Dimension tool, locate the lower left hole with dimensions. Add center marks without extension lines to the ears and arc. Click on 3.00 dim: tolerance in property manager: pull down to Symmetric:.005: change number of decimals to.123 in both boxes: OK: Click on 5.00 dim: tolerance in property manager: pull down to Bilateral:.008 upper:.002 lower: change decimals to.123 : OK: Click on R.81: tolerance in property manager: pull down to limits: +.003: -.003: change decimals to.123 : OK. Note that the nominal figure and tolerance figures both must have the same number of decimals. Click on the Note Icon (A): Place it on a blank part of the page. Type in All Fillets and Rounds are : click on R.25 dimension, UOS : Esc : Right click on R.25 and hide it. The dimension in the note is now linked to the fillet dimension. Right click Sheet1: Edit sheet format: Add to title block: Title: Transition Base: Drawing #: T57821: Tolerance: ±.01 (Add Symbol Modifying Symbol plus/minus): Next Assy: T You may add the rest of the information to complete the title block. Right click SheetFormat1: Edit Sheet to get drawing back. 3 : 15

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17 LabDemo6A - Shells, Linear Patterns, Hole Wizard, Draft Open a new part file in SolidWorks. View: Origin. Activate a sketch on the front plane. In the rectangle pull down select Center Rectangle. Start on the origin and draw in a rectangle. (The center rectangle makes sure that the origin is at the center of the rectangle.) Dimension the rectangle 4 wide x 1.5 high. Esc. Make the centerline and the origin have a midpoint relation. Extrude backwards 8 in. OK. Rename to Case. Click in drawing and type f to fit on screen. Fillet: radius.5: select left, right and back top edges. OK. Rename to Top Edges. Pick hidden lines visible: fillet: radius.25: select two back vertical edges. OK: Shaded view. Rename to Back Edges. Note: the fillets and rounds must be done before the shell command. Hit up arrow 5 times. Shell: wall thickness.1, select front and bottom faces. OK. This makes body a thin shell. Rename Hollow. Check Point 1. Save as CaseTop. Bottom view: right click bottom: sketch. Draw a circle near the lower left corner: Dimension circle.4 diameter,.85 from both outer edges. Extrude-boss - blind, 1.3 in with 2 of draft OK. Make sure it extrudes into shell opening. Rename feature to Peg. Top view: select top face by clicking in upper left corner right over peg: Hole Wizard: Countersink: Standard- ANSI inch: Oval Head: Size - #8: End condition - through all. Position Tab: Dimension:.85 from both (top and left) outer edge. Finish. Check Point 2. Save In Feature Manager control-click both Peg and CSK... : select Linear Pattern: Click top edge for direction: distance 2.30 in: number 2: Click left edge for 2nd direction: distance 6.30 and number 2 Check pattern reversing directions if necessary. OK. Rename Peg & Hole Array Right click right face: Sketch: Right view: Draw circle centered at top edge: Dimensions: diameter.1, 1.50 from left end. Extruded Cut: through all: OK: Isometric view. Rename feature to Groove. In feature manager select Groove: Linear Pattern: click bottom edge for direction: distance.25: number 3: click bottom edge again for direction 2: distance 2.25: number 3: OK: Rename Triple Groove. Check Point 3. Save. Note that the linear pattern may be used to replicate the pattern twice in the same direction. To use a feature mirror, pick a mirror plane. Select Front Plane, then pick Mirror in Feature Manager. Expand feature in upper left corner of drawing area. Select each feature of the part. OK. The whole feature should be mirrored. However, hitting the up arrow about 6 times reveals that the Shell feature will not mirror, something to watch out for. Check Point 4. 3 : 17

18 Lab Demo 6B Loft Open a new part- ANSI inches. View: Origin. Right click Top Plane: Sketch: Top View. In the rectangle pull down select Center Rectangle. Start on the origin and draw in a rectangle. (The center rectangle makes sure that the origin is at the center of the rectangle.) Esc. Make the vertical and horizontal lines equal. Make one side 5 inches. Extrude-Base 9 inches up. OK : f to fit on screen. Rename Bottle Body. Right click on top of solid: sketch: top view. With top face still selected select convert entities: Click on purple arrow in upper right corner to accept sketch. There will be a free sketch in the feature manager not in a feature. Check Point 1. Save as bottle. Click on top surface: Reference Geometry - Plane: 3 inches up. OK: Right click on plane in Feature Manager: Sketch: Top view: Circle: Draw a circle 2 inches in diameter centered on origin. Dimension 2 inches. Click on purple arrow in upper right corner to accept sketch. There will be a second free sketch in the feature manager not in a feature. View Planes (Turn off plane) Isometric View. Loft: Expand Feature tree in upper left corner of drawing area: Select sketch 2 and sketch 3; OK. The two sketches should be connected. Rename Transition. Check Point 2. Note that the free sketches have now been absorbed in the loft feature in the Feature Manager. Right click on top surface: Sketch: With the top surface still selected click on, Convert Entities to select all four arcs of the circle. Extrude-Boss 1.5 inch up. OK. Rename Bottle Neck Set display style to hidden lines visible and press the right cursor key once to see all the edges. Fillet: select the four bottom and four side edges. Check the strawberry field box to make sure all the selections say edge and not face or loop. Set radius to.5 inch: OK: Rename Sides & Bottoms: Fillet: Select four top edges, four edges on loft: radius.3. Rename Loft Edges. Select circle at top of loft: radius.2 inch: OK: Rename Neck Edges: Reset display style to Shaded with edges: Click on top surface: Shell:.2 thick: OK: Rename Insides. Bottle is done. Check Point 3 To see inside the bottle, select Section View in view toolbar: click OK: A section view will appear. Click on Section View to return to full view. Check Point 4. Open a landscape title block: Save as bottle. Model View: Select bottle: Next (blue arrow): Isometric view: click in center of drawing: hidden lines removed. Esc. Notice that most of the edges of the bottle are not visible. This is because of the rounding of these edges. To make them visible select the view (get a green border around it): Right click on the border: under View (Drawing 1) select tangent edges: in the fly out menu pick Tangent Edges with font. The edges will now be delineated with phantom lines. You should only use tangent edges in an isometric view, never in the standard three views and use it only with tangent edges with font. 3 : 18

19 Lab Demo 6A Case Lab Demo 6 B - Bottle 3 : 19

20 LabDemo7 Assemblies On Desktop: Open the server drive and drag the LabDemo7 files to your ThawSpace Drive. Open parts Cover, CircuitBoard, and Bottom. Create a new assembly file. The Insert Components box will automatically open. Click on the push pin to keep the box open. Turn on the origin if it is not already on. Click on Bottom in the selection box, move the cursor to the assembly area, place it over the origin and click to set the bottom. The first part brought in will be fixed to the oirgin. In the following order, bring in the cover and then the circuit board then click OK to close the Add Component box. If there is an (f) before either Cover of Circuit board right click on the part and select float. If there is a (-) in front of then don t do anything. Right click on Cover in the feature manager and select Hide Components icon to get it out of the way. View: Origin (turn off.) Assembly Tab: click on mate (paper clip icon): Select the inside faces of the upper left hole on circuit board and the upper left hole on bottom. You will know when you have the inside face when you see the red cylinder outline rather than just a circle. Zoom in on features using the scroll wheel on the mouse to isolate the parts of interest. Choose concentric. OK. Zoom in on upper left corner: select top face of hole extrusion on Bottom and the bottom face of CircuitBoard. Hold the scroll wheel on the mouse down and move the mouse to rotate the assembly so that you can select the proper faces. Make a coincident mate. OK. Select the right face of the circuit board and the right face of the bottom. Make sure you select planar faces. Ignore the error message and pick a parallel mate. OK: OK. The circuit board is mated to the bottom case. Save as Case. Check Point 1 Right Click on Cover: Select Show Components icon. Click on mate (paper clip icon): Select upper left hole on circuit board and upper left hole on cover, choose concentric. OK. Mate: Zoom in on upper left corner: select top face of CircuitBoard and the bottom face of hole extrusion on Cover. Use the cursor keys to get the proper faces. Make this a distance mate of 0 inches. If you cannot activate the distance mate make sure that you have selected two faces and not edges. OK. Select isometric view. Expand the Feature tree in the upper left corner of the work space: Expand Bottom and pick the right plane: Expand Cover and pick its right plane. Make these coincident. OK. The circuit board is mated to the top case. The same steps that mated the circuit board to the base could have been used here also. Other mates were used for demonstration purposes. Save assembly. Check Point 2 Open file Screw#8. Zoom in on bottom of screw. Select edge on top of chamfer. Insert Annotations Cosmetic Thread. Blind: 1.00 inch: Thread callout: #8-32 UNC 2A x 2 : OK : right Click on Annotations near the top of the Feature Manager: Details Shaded Cosmetic Threads to get a view that appears like threads. (This is not necessary as simplified threads will show up in the front view. Save file: Ctrl-Tab to assembly. Insert Components: click on push pin. Bring 4 screws into assembly. Close window. View - temporary axes. Mate: select an axis for hole and an axis for a screw: preview: OK repeat for remaining three screws. Select top face of cover and top edge of screw: Set to coincident: OK; repeat for other three screws. To fully mate the screws set the right plane of each screw parallel to the bottom s right plane. Again ignore the error message about the default. It will 3 : 20

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23 Copy the folder LabDemo8 to the ThawSpace drive from the server. Open the four files (FourBar1, FourBar2, FourBar3 and FourBar4) in SolidWorks. Open a new assembly. Click on insert component icon and press the push pin. Click on each of the four parts in the order FourBar1, 4, 3, 2 setting each in the assembly. The first part brought into the assembly is fixed, so make sure that was FourBar1 and that the part snapped to the origin when it was brought in.. Close the property manager. Go to isometric view. Zoom in on short bar and base end. Go to hidden lines visible. Shut off the origins: view origins. Mate: Click on Face of hole in end of short rod and Face of hole in base. Make sure you have the face and not the edge. The highlight looks like a cylinder rather than a circle. Concentric: OK: Click on front face of base and back face of short bar (Rotate the parts around using the mouse wheel - hold it down and move mouse until the back side is visible.) Coincident: OK Zoom in on the other end of the base and one end of the long bar. Repeat the mating as was done for the short rod. Close Mate (OK a second time.). F to fit in window. Grab a part with the mouse an note its motion. Both bars should be able to rotate about the pivots on the base. Set them up at an angle. OK. Check Point 1 Mate: Click on Face of hole in open end of short rod and Face of hole in medium rod. Make sure you have the face and not the edge. The highlight looks like a cylinder rather than a circle. Concentric: OK: Click on front face of the short rod and the back face of medium bar (Rotate the parts around using the mouse wheel - hold it down and move mouse until the back side is visible.) Coincident: OK Click on Face of hole in Lab Demo 8-4 Bar Linkage Moving Assembly 3 : 23 open end of long rod and Face of hole in median rod. Make sure you have the face and not the edge. The highlight looks like a cylinder rather than a circle. Concentric: OK: OK to close Mate. Isometric view. Check Point 2 Shaded View: Move Component: click and hold down mouse button on short (red) rod. Move it in a circle and watch how the mechanism moves. This is a four bar linkage which will be analyzed in depth in Dynamics and Intermediate Dynamics. Pins could be added to make the system more realistic, but the motion would not be affected. Before bringing the assembly into a drawing make sure the order of parts in the feature manager is how you want them in the BOM. Drag the icons up and down until they are in the order FourBar2 (Crank), FourBar3 (Rocker Arm, FourBar4 (Connecter) and FourBar1 (Base). Drag the components in the Feature Manager into the correct order. Now bring the assembly into a Landscape drawing as an isometric view. Leave the scale at 1:4. Options : Document Properties : Balloons select bent leaders. (This is selected as a default on lab computers, but not in the Student Version.) Annotations Tab: Balloons. Select an edge each of the four parts and set the balloons. Select the four bar drawing. Table : Bill of Material. OK. Click in work area to set BOM. Check Point 3. Control-Tab to the FourBar1. Click on Configuration Manager Tab (third icon from left on top of Feature Manager): Right click on Default: Properties: On bottom of dialogue box select User Specified Name: for part number enter NB74562: Custom Property Tab: Under property column select

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