Laboratory Demonstration Exercises

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1 Laboratory Demonstration Exercises 3-1

2 Lab Demo 1 - Plus Block Open SolidWorks, click on new document part OK. Right Click on Front Plane, click on Sketch icon (pencil w/ axes). In the sketch toolbar on the top, click on the Rectangle icon. Starting in quadrant 2, Click and Drag a rectangle across the origin ending in quadrant 4. Escape when done. Click on the Dimension icon (right above the sketch icon). Click on the right vertical line, draw the mouse to the right and set the length to 1 inch. Click on the bottom horizontal line, draw the mouse down and set the length to 4.5 inches. Click on the bottom line, click on the origin, drag right and set the distance to.5 inch. Click on the left line, then click on the origin, pull down, set dimension to 2.25 inches. The rectangle is now all black which means that it is fully defined fully dimensioned and locked to the origin. The base feature must always be tied to the origin in some way in order to become fully defined. To create a solid from this sketch click on the feature tab just above the Feature Manager. Select the Extrude Base icon in the upper left. The view will rotate to an isometric view. In the pull down menu change blind to Mid Plane and set the length to 4.0 inches. Pressing Enter will give you a preview of the extrusion. Click on the check mark when it is OK. In the Feature Manager there is now an item called Base-Extrude1. this should already be selected and ready to be edited. Change the part name to Plus-Block Base. Check Point 1. File: Save as LabDemo1 Right click on the top face of the block to select this as the next plane to sketch on and click on the sketch tool icon in the fly out menu. At the top of the work space are quick select icons in the transparent Heads-Up toolbar. Pick the top view. Pick the line tool in the Sketch Tool Bar. Starting about 1/3 of the way in from the right on the upper edge of the 3-2 block, click and draw a line about 1.5 inches long to the left. Now draw a line straight down to the bottom edge, draw a line 1.5 inches to the right along the bottom edge until you are just under the starting point and finally close the figure. Activate the smart dimension tool. Click on the right edge of the block and then click on the right vertical line you just drew. Draw the cursor up and set the dimension to 1.5 inches. The line will turn from blue to black. Do the same from the left edge to the left line. To add to the solid base block click on the Feature tab and select the Extrude Boss icon. Then click on isometric view. Leave the extrusion blind and set the length to 2.0 inches. Press Enter for a preview and reverse the direction if necessary. Click on the check mark when it is OK. In the Feature Manager there is now an item called Base-Extrude2. Change the part name to Plus-Upright. Repeat the above steps but on the bottom. Select the bottom view from the pull down selection at the top of the work space, right click on the bottom face and then click on thesketch icon. With the line tool, draw and dimension the rectangle as above and extrude it down 2 inches. Rename this feature as Plus-Bottom. We now have a solid plus shaped block in isometric view. If you don t have this figure, you may open the check point #2 file retrieved from the server and catch up with the demonstration. Check Point 2. Save File To drill the holes, start by right clicking on the top face of the block followed by a click on the Sketch icon. In the view toolbar, click on top view. Click on the circle drawing tool, click on the origin and drag a circle of about.5 inches in radius. Click on the dimension icon, click on the circle and set its diameter to 1.0 inch. The circle should be black meaning it is completely defined.

3 Select the feature tab and click on the Extruded Cut icon. Change Blind to Through All and click OK (check mark). Change the name from Cut-Extrude 1 to Circular Hole. Click on isometric view in the view toolbar to see the hole. Right click on the front face, click on sketch icon and change the view to front. Click on the rectangle drawing tool. Click in Quadrant 2 in the center part of the plus, drag down to Quadrant 4 and click to set the rectangle. Set the dimension of the rectangle to.5 high by 1.0 wide. Draw a centerline diagonally through the rectangle. Esc: click on the line and control click origin. Select midpoint (the whole rectangle becomes black.) As with the circle, do an extruded cut through the body. Change the name from Cut-Extrude 2 to Rectangular Hole. Return to Isometric view. Check Point 3. Save File Right click on the right face, sketch and right view. Draw a horizontal line about 1.5 inches long above the origin, right click, select tangent arc, click on the end of the line just drawn and draw a half circle to the right and then downwards and back to just under the starting point of the arc, right click to line, draw a line of equal length to the one above, right click to tangent arc and draw an arc left - upward right to close the slot sketch. Make the lines 1.5 inches long, the circles.25 inches in radius. Draw a centerline between the two centers. Esc: Click on the line and control click origin. Select midpoint. The slot is completely defined. Select Feature tab then Extruded Cut and do a blind cut 2.75 inches deep. Pick OK. Change the name from Cut- Extrude 3 to Slot. Change to isometric view.check Point 4. Save File Use the arrow keys to rotate the object around and look at the various faces. In the view tool bar select Hidden Lines Removed for the display. File/Save as LabDemo1. (Leave Open) File/Open. Open Landscape titleblock. File/Save As LabDemo1. (Always rename title block as soon as it is opened.) In View Layout tab select Standard 3 View icon. Select LabDemo1 in the property manager, then click on the check mark (OK). 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. 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. Click on the front view to select it and select the Hidden Lines Visible icon. Click on the Model View Icon. With LabDemo1 highlighted click on the blue arrow (next). Pick isometric and place it in the upper right corner of sheet. Pick use sheet scale in property manager and hidden lines removed. In the view menu unselect origins to get rid of the origin marks. Save Drawing. Check Point 5. Save file. In Feature Manager, right click on Sheet1 and Select Edit Sheet Format. (The views will disappear.) Double click on Name: to get a note box. Click after name and add your name. Click OK (check mark) For title type in Plus Block. Drawing #: Scale: 1:2, Units: Inches, and add the date. For material add Steel. Add your lecture section number and lab section number. When all those are entered, Right click on Sheet1 and select Edit Sheet. Save Drawing. Check Point 6 3-3

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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

6 Click on the Model View Icon. With LabDemo2 highlighted click on the blue arrow. Pick isometric and place it in the upper right corner of sheet. If it is too large check use custom scale in the property manager and set the scale to 1:4. Using the view tool bar make each of the three views to show hidden lines and the isometric view not to. Select each view one at a time and then select the view form for each. Right click on the selection border of each view in turn. Pick Tangent Edges and check tangent edges removed. In the view menu unselect origins to get rid of the origin marks. Save Drawing. Check Point 4. Save file. Menu Bar: Tools Options. Document Property Tab / units / one decimal place. Dimensions / Uncheck Add parentheses by default : Annotation Font / Font / Points radio button / 10 pt: Arrows / Length.2, head.1. OK. Most of these are already set as defaults. Click on Layer Manager: New: Make Layer name Dimensions: Color Royal Blue. Click OK: Set layer to None on pull down menu. (If you do not have a Layer Toolbar present, right click on any tool bear and select Layer from the fly out menu.) Select the center mark icon in the lower left. Click on the three circles or semicircles to insert the center lines. Click center mark icon again to deactivate. Save drawing. Check Point 5. On pull down layer menu select dimensions layer. Click in white area to deselect any views no green borders around any view. On the menu bar select Insert Model Items. Set the import from box to entire model and click OK. The model is now dimensioned, but needs some cleanup. Move the.5 cap dimension to the right side. Move dimensions closer to body. In right view right click and hide the 2.0 inch and 1.5 inch dimensions on the bottom. Click on the dimension icon and dimension the two half circles. Click on the 2.0 inch dim in the lower right of the front view. While holding down the shift key, drag it over the right view and release. Now place it to the left of the right view. Click on the 2.0 inch dimension at the top of the front view. Holding the shift key down, drag it over the top view, release and place the dimension. Make sure that all the extensions lines of external dimensions have noticeable breaks with the object lines. If not click on the green square (grip) when the dimension is highlighted and move it to where it should be. Find the R.4 dimension and select it. In the property manager is a box entitled Dimension Text which contains R<DIM>. Place the cursor to the right of that and type TYP. Check Point 6. In the property manager right click on the Sheet Format1 item and select Edit Sheet Format. (The drawing disappears leaving only the title block.) Double click on Tolerance block. Place the cursor after the colon. In the note dialog box under text Format click on the right icon Add Symbol, Modifying Symbols: select plus/minus, click OK and type.1. Click on the check mark (OK) Make the scale 1:2. Double click on Name: to get a note box. Click after name and add your name. Click OK (check mark) For title type in Widget. Drawing # - 73P56. Scale 1:2, Units: Inches, and Add the date. For material add Gold. Add your lecture section number and lab section number. When all those are entered, Right click on Sheet1 and select Edit Sheet. Save Drawing. Check Point 7 You now have a dimensioned engineering drawing. It is coupled to the solid drawing so that if you decide to change the original drawing, this drawing will also be changed. 3-6

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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

9 other: 50 mm. Click on arc: click on near upright edge of L: 22.5 mm. Extrude cut: Through All: Rename Slot. Check Point 4: Save Part. Select wide top surface: Sketch: Top view: Circle Tool: Draw circle near lower right corner. Smart Dimension: Make hole 12.5 mm from right edge, 10 mm from bottom edge, diameter 6.5 mm. Extrude Cut: Up To Next: OK. Rename Small Right Hole. Select Small Right Hole in Feature Manager. Linear Pattern. Select Right Edge: Distance 10 mm: Number of Instances 9. OK Rename Small Hole Array. Check Point 5: Save Part. Isometric View: Fillet Tool: Radius 10: Select four right vertical edges top and bottom of right notch. Check strawberry field to make sure it contains four edges. OK Rename Right Rounds. Check Point 6: Save Part The part is complete and ready to bring into a drawing. Open a new Landscape Title Block. Save As: LabDemo3. Tools: Options: Document Properties: Units: MMGS radio button: Number of decimals 1: OK. Standard 3 View: LabDemo3: OK: Click on Front View: Hidden Lines Visible. If Tangent Edge box appears, select Removed. Right click on sheet not on a view: Properties: Scale 1:2: OK. Adjust views so that there is plenty of room about each for dimensions. View: Origins to turn off origins. Model View: LabDemo3: Next (Blue Arrow) Isometric View: click in drawing to set view: Hidden Lines Removed: Custom Scale 1:4. Click on drawing sheet to deselect all views. To add center marks to the slot arcs, pick the center mark icon in the annotation tool bar. In the property manager uncheck use document defaults and extension line boxes. Make the size mark 2 mm. In the drawing click on each arc to add the center marks without and extension lines. Layer Properties: New Layer: Name Dimensions: Color Royal Blue (fourth row fifth column): OK: OK. With no view selected: Insert: Model Items: In Source/Destination window select entire model: OK. Check Point 7: Save Drawing Zoom in on front view. Select 35 mm dimensions and shorten lower extension line. Move the 25 mm dim down to slot. Bring 20 mm dimensions over to step. Move 17.5 to right of L upright, 75 mm closer to body, 15 mm closer and outside extension lines and 30 mm closer to body. Place 20 mm leader so that it is clear of other dimensions. Scroll up to top view. Shorten extension lines for 50 and 22.5 mm dimensions, if necessary. Move top dimensions closer to body. Add a 2X before the R10 for the slot. Move 15 mm to step. Shift Drag 100 mm to right view. In lower right corner move dimensions around so they are not cramped and are clear of their extension lines. Add a 9X before the φ6.5 dimension. Click on 10 mm dimensions between holes. In Property Manager, place cursor to left of <DIM> in the Dimension Text Box and type in 8X. Pull φ10 leader off body. Click on φ35, place cursor after <DIM> in Dimensions Text box and type INSCRIBED click on depth symbol and type 10. Pull dimension below view. With Smart Dimension, dimension edge of hexagon. Finally click on R10, place the cursor before <DIM> and type 2X. View: Origins to turn origins back on. Select Center Line too in Sketch Tool Bar. Place cursor over origin for a few seconds 3-9

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

11 Lab Demo 4 Securing Flange Open new part file. Tools Options Document Properties Units 3 decimal places. View: Origin to turn on origin. OK. Right click on Front Plane: Sketch. Type z 3 times to zoom out. Draw vertical center line through origin. Line: Draw horizontal line starting about 3 inches to left of origin, 3 inches long. Right click: Tangent Arc: Draw half circle about.5 radius. Right Click: Line: 2 inches horizontal. Down.5, 1 inch right, close figure. Esc: Click on origin, Control click on bottom horizontal line: coincident to set the feature to the origin. Click Dimension Icon: click center line, click right edge of figure, drag down and to the right of the CL to create a diameter dimension: 6 inches. Click center line: click second vertical line: drag up and to right of CL: 8 inches. Click center line: click arc: drag up and to the right of CL: 12 inches. Click on arc: drag out:.5 inch radius. Click right vertical line: drag right:.5 inches. Feature Tab: Click revolved boss/base icon: 360 : OK. Type f to fit on screen. Rename to Circular Base. Check Point 1 Top view: Click top face at about the 9 o clock position: Feature Tab: Hole Wizard Icon: Type Specification: Counterbore: Standard: ANSI Inch: Type: Socket Head Cap Screw: Size: 1/2 inch: Fit Normal: Check custom Sizing to check size: thru diam.5312 diam of CB.8125 depth See chapter 2 section on using Hole Wizard. Positions Tab: Sketch Tab: Add/Delete Relations pull down: Add relations: click on origin, click on hole center: horizontal. Smart Dimension: click origin: click center of circle: set distance to 5 inches. OK: OK. Isometric view to observe. In Feature Managfer select CBORE for Feature Tab: Linear Pattern Pull down: circular Pattern. Menu Bar: View Temporary Axes: Click central axis: check equal spacing to get angle 360 : Number of instances 12: Features to pattern: CBORE for : OK: Menu Bar: View- Temporary Axes (to turn off.) Rename to CBore Pattern. Check Point 2 To add groove for O-ring: Right Click Front Plane: Sketch: Front View: Centerline: click on origin, draw vertical line. Circle Icon: draw circle on bottom edge: Dimension: click on center line: click on center of circle: Drag back past center, 7 inches: Click on circle:.25 diameter. Escape: Click on origin: control click on center of circle. Horizontal relationship. Feature Tab: Revolved Cut. OK. Hit up arrow two or three times to view cut. Rename to O Ring Groove. Save part as Flange. Check Point 3 New: Portrait Drawing template with Title block. Save as: Flange. View Layout Tab: Model View: select part Flange, check the blue arrow and click top view: Click in upper third of drawing sheet to set view: Esc. Right Click in empty part of sheet: Properties: Set Sheet Scale 1:4: OK. Make hidden lines visible. Click on Layer Properties: New: Make Layer name Dimensions: Color Royal Blue. Click OK: Set layer to None on pull down menu. Make sure that you are in the None layer before doing a section cut. Click on centerline tool ins Sketch Tab: Line Pull Down. Hover over the CB hole at 9 O clock to activate and move to left of view, but do not click and draw during this move. There should be a blue dashed line with the cursor. Place the cursor over the left purple side of the enclosing box, click and drag to the right side of purple box, passing through center. View Layout Tab: Section View: place cursor below top view and click to set section view. If the section arrows are not facing up, select Flip Direction in the property manager. OK. Set layer to Dimensions. Select section view: turn off hidden lines. Move the note SECTION AA away from the front view. 3 : 11

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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14 LabDemo 5 Auxiliary Views Open new part, inches for units. View: Origin to turn on origin. Right Click: Right Plane: Sketch: Rectangle: Starting horizontally to right of origin draw a rectangle about 5 inch long, 1.5 inch high down and to the left. Esc: Click on top horizontal line, control click on origin: select relation midpoint. Dimensions: Length 5, Height The base should be completely defined. Feature Tab: Extrude Base: Midplane: 3 inch. OK. (Keep origin on the plane of symmetry.) Rename feature Support Base. Right click on right face: Sketch. Right View. Line: Starting about 1/3 of way from left edge on top line, draw a horizontal line 1.25 inches right, up 2.3, down and to the left at about a 30º angle to over the start point. Close figure. Esc: Center line: draw a horizontal line to the left from the upper vertex. Dimensions: Click on centerline and angled line 30º: Click on bottom right of base and top of vertex 3.79 inches: make width of center post 1.25 inches. Click on the left edge of base and the left edge of post: enter the dimension (5 1.25) /2: (Let SolidWorks do the math) OK. Isometric View: Extrude Boss: Up to vertex: click on far edge of base: OK. Rename to Post. Check Point 1. Save as LabDemo5 Right click on angled face of center post, sketch, normal to: Line: Starting about an inch below the left angled face edge, draw a vertical line upward about an inch past the angled face: right click: Tangent arc: draw a half circle up and right to about the right edge: line: draw a line downward until even with the starting point: close figure. Esc. Click on right line, control click on right edge of angled face: make collinear. Dimension: from top edge of angled face on bottom to vertex of line and arc 1 inch. From arc to bottom 3.81 inch. Isometric view: Blind extrude up 1 inch. OK. Rename to Angled Cap. Check Point 2. Save Right click on top angled surface: sketch: normal to: Centerline: draw vertical centerline through origin: esc: select right edge: convert entities: line: from bottom right corner draw out about.38 in: right click: tangent arc: draw half circle.81 radius: right click: line; straight back to base line. Trim Trim to closest: trim off excess lines to left of loop; select sketch mirror. Select lines just drawn to mirror. Click in mirror about and then select the center line. Dimension: from one arc to other arc (center to center) 3.75 inch: radius of arc.81 inch. Extrude boss: isometric view: up to vertex: pick bottom corner: OK. Rename feature Ears. Check Point 3. Save Right click on top angled surface: sketch: normal to: Draw a diamond about the center of top semi-cylinder. Make opposite sides parallel, and an adjacent pair perpendicular and equal. Dimension one side 1.25 inch; Draw diagonal horizontal centerline inside diamond. Esc: Click on center line: make horizontal or vertical. Click on circular edge: convert entities: Make center of arc at midpoint of centerline: click on arc: check for construction box. Feature Tab: Extruded cut: isometric view: up to next: OK. Rename feature Diamond. Click on top angled surface: Normal to: Click about 1/2 inch in from bottom right edge of face. Hole Wizard. Pick hole icon: change Type to screw clearances: pick size as 3/8 inch and make depth.75 inch. Positions. Select smart dimensions and locate the hole.5 inch from edge and.81 inch from bottom(right) to center with ear. Finish. Isometric View. Check Point 4 Select Clearance hole in feature manager. Linear Pattern: Select the bottom edge of the angled face to select direction: Make distance 1 inch and number of instances 3: select a vertical line for second direction, length 1.5, number of instances 2: check preview to make sure directions are correct, if not reverse directions. OK. Rename to Set of Holes. Fillet: click on top end edges of base, inside top face edges and the insides of the ears. Switch to hidden line view to select all the lines:.25 inch: OK: Rename feature Rounds. The part is done: Check Point 5: Save it as labdemo5. Open landscape drawing template. Save as: LabDemo5. Click on Model View: select 3 : 14

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

16 3 : 16

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

21 disappear when you select parallel. View: Temporary axes (turn off). Save assembly. Check Point 3 Menu: Insert: Exploded View...: With components box (large box in the settings box) highlighted click on the cover and circuit board. Click on the direction box, then click on the up arrow in the assembly. Finally make the distance 2 inches and pick Apply and then Done. Select component box, click on the cover, then make the direction up and the distance 2 inches: Apply: Done. Finally add the four screws to components, direction up, distance 7.5 inches. Apply Done. OK: Isometric view. Save Assembly: Check Point 4. Open: Landscape Title Block Drawing: Save as Case: Model View: Click on Case: Blue Arrow: Isometric View: click in Blank area of drawing to set view: Set Sheet Scale: 1:2: OK: Position Drawing. View: Origins to turn off the origins and select Hidden Lines Removed in Display Styles. Due to the rounded edges the parts look somewhat washed out. To help in visualizing the part we need to add tangent edges. Select the isometric view and right click in the border. In the fly-out menu place the cursor over tangent edges and select Tangent Edges with Font from the selections which appear. The font adds the tangent edges as phantom lines to help depict the curved edges. Tools: Options: Document Properties: Balloons: Check Use bent leaders: Annotation Fonts: Tables: Font size to 8 points: OK; Annotations Tab: Balloon icon in Toolbar: Click on edge of Bottom, click a second time away from part to set the balloon. Repeat for the CircuitBoard, Cover and Screw. OK: Position Balloons. Click on Exploded View to select it (green border): Tables: Bill of Material: Take default parameters making sure the Attach To Anchor Point box is unchecked: OK: Click on the column separator between Item No. and Part Number and drag it to the left to make the column narrower. Repeat with all the other column separators. The BOM should be as small as possible so that it does not dominate the drawing. Save drawing. Check Point 5 Ctrl-Tab to the Bottom part: Click on Configuration Manager Tab (third icon on top of Feature Manager): Right click on Default: Properties: On bottom of dialogue box select User Specified Name: for part number enter 152-BX23: OK. Custom Property Tab: Under property colum select description. Add Bottom under Value / Text. OK: OK Save: Repeat for Cover (152- BX24, Case Cover), CircuitBoard (152- CB74, Circuit Board) and Screw#8 (#8-32 UNC 2A x 2, Oval Head Screw). Return to drawing: Click on Rebuild to get new values in table. Drag column headers to allow entries to fit. Click on table and select the upper left corner of the border to move the table and position BOM to a corner of the title block frame. Drag from upper left to lower right to select the entire table. In the fly to select center justified to make the table uniform. Click in drawing. Save drawing. Check Point 6 At this point you would fill out title block with the necessary information. Tolerance, materials, and next assembly are left blank for top assembly drawing. Note: While in the Assembly, in order to collapse an exploded view, right click in the graphics area and select collapse. To reexplode, select menu: insert: exploded view: OK. 3 : 21

22 3 : 22

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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