Introduction to SolidWorks for Technology. No1: Childs Toy
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1 Introduction to SolidWorks for Technology No1: Childs Toy
2 Table of Contents Table of Contents... 1 Introduction... 2 Part Modelling: Cab... 3 Part Modelling: Base... 6 Part Modelling: Wheel Assembly: Base and Cab Assembly: Wheel Assembly using the Toolbox Completing the Assembly Creating Drawings and Worksheets PhotoView Introduction to Solidworks for Technology Page 1
3 Introduction This exercise is an introduction to SolidWorks for Technology. The exercise looks at a technology project from all areas of SolidWorks; part modelling, assembly, drawings and photoview Learning Intentions At the end of this workshop you should be able to: 1. Create new Parts using basic sketching and feature commands 2. Create a new Assembly, mating two components and adding appearances and scenes 4. Complete Drawings of an assembly including a worksheet for students 3. Create and save photorealistic images using Photoview 360 Prerequisite Knowledge None Saving Your Work Create Folder called Childs Toy. Save all files into this folder Introduction to Solidworks for Technology Page 2
4 Part Modelling: Cab Open a new part. Save Part as Cab. Create a new sketch on the Top Plane Select the Rectangle command and draw a rectangle with one corner co-incident to the origin.. Hold down the left mosue button to drag out rectangle, release when its an approximate size. Accept the sketch to complete. Introduction to Solidworks for Technology Page 3
5 Select Smart Dimension and apply the dimensions below to the rectangle. Hover over line, it will highlight in orange. Left-click on line drag out dimension line and left-click again to open the dimension window. The rectangle now turns black as it is Fully Defined sketch. Select the Features Tab and select Extruded Boss/Base The Sketch will move to an isometric view. Add 85mm dimension. Accept the extrude.. Introduction to Solidworks for Technology Page 4
6 Select the Chamfer command. It is located under the Fillet Icon. Apply a 55mm chamfer to the top edge as shown. The Full preview button will allow you to see the resulting feature. Click OK. Save your work. Apply an appearance to the Cab. Select the Appearance tab on the right. Browse for Organic, Wood, Pine. Select Polished Pine and drag and drop onto the Cab. A pop-up window will appear. Select the part icon to apply the appearance at part level. Save you work. The Cab part is now complete Introduction to Solidworks for Technology Page 5
7 Part Modelling: Base Base shape Open new Part. Save as Base. Create a sketch on the Top Plane. Draw a Corner Rectangle and dimension as shown. Select Extrude Boss/base and extrude 15mm with a blind end condition. Accept the extrude Rename the feature as Base shape (press Fn+F2) Introduction to Solidworks for Technology Page 6
8 Wheel Notches Create a new sketch on the top surface by leftclicking on the surface and selecting the sketch icon from the pop-up toolbar. Select a normal-to view by pressing the space bar and selecting Normal To Sketch two rectangles on the edge of the base as shown. The 1 st corner should have a coincident relationship with the edge of the base, as shown by the cursor having a yellow coincident relation highlighted when sketching Introduction to Solidworks for Technology Page 7
9 Add an Equal relation to the horizontal lines (hold Ctrl key and select lines). The pop-up toolbar will allow you to add relations. Repeat the add relation for the vertical lines. The equal relations can now be seen on the lines as shown Smart Dimension black). the sketch as shown. The sketch is now full defined (sketch is now Select Extruded Cut from the features tab and change the direction to Through All Rename feature as Wheel notch (ctrl+ F2). Click OK Save your work. Introduction to Solidworks for Technology Page 8
10 Tapped Holes for Wheels Create a new Sketch on the vertical surface of the notch as shown. Draw a Centreline diagonally across the surface. Add a point to the midpoint of the centreline. Repeat this for the other notch Exit the sketch In the features tab, select Hole Wizard. The following specification is added: Type: Straight Tap Standard: ISO Hole Specification; M5 x 0.8 End Condition: Blind, depth 25mm, thread 20mm Then select Positions and select 3D Sketch Introduction to Solidworks for Technology Page 9
11 Select the two points the sketch for the position of the Hole Click OK and save Mirror the Features Select Mirror from the features tab. Open the design tree (press the + symbol beside ) and select the Front Plane as Mirror Face and the wheel notch and Tapped Hole as the Features to Mirror. Click OK Introduction to Solidworks for Technology Page 10
12 Full Round Fillet Select the Fillet feature. Select the Full Round Fillet option and select a face to enter into each of the boxes below, working left-to-right or vice versa. Click OK Add a blue high gloss plastic appearance to the part and save. The Base part is now complete Introduction to Solidworks for Technology Page 11
13 Part Modelling: Wheel Open a new part and save as Wheel. Create a sketch on the Front Plane. Using the circle command draw a circle with its centre on the origin. Smart Dimension the circle as 45mm. Extrude the circle 14mm Click OK Select the Hole wizard feature and edit the specification Hole type: Counterbore Standard: ISO Type: Pan Head Cross Recess Size: M5 End Condition: Through all Introduction to Solidworks for Technology Page 12
14 Select Positions and 3D Sketch and hover over the circle face until centre-point appears. Click on the centre to add the hole. Click OK Select the Fillet command and add a 4mm Constant Size Fillet to the front edge and click OK. Save your work Add a Red high gloss plastic appearance to the wheel The Wheel part is now complete. Introduction to Solidworks for Technology Page 13
15 Assembly: Base and Cab Create a new assembly or within the Base part select Make Assembly from Part/Assembly Insert the base part and select OK. Save as Childs Toy Assembly Select Insert Components and (Browse if not shown) click the Cab part. Use the rotate on insert tool to rotate about Y axis into the correct orientation. Click OK Introduction to Solidworks for Technology Page 14
16 Rotate the view (hold down middle mouse button) and select the bottom of the cab, on the pop-up toolbar select Mate. Select the top surface of the Base and add the coincident mate Add another coincident mate to the back of the cab and the end of the wheel notch Introduction to Solidworks for Technology Page 15
17 In the Advanced Mates tab select Width mate. In the Width made select the two sides of the cab for the width and the two sides of the base for the tab. Click OK when complete Save your work. The first part of the assembly is complete Introduction to Solidworks for Technology Page 16
18 Assembly: Wheel Assembly using the Toolbox Open a new assembly or within the wheel part select Make Assembly from Part/Assembly. This assembly will be used as a sub-assembly for the Toy. Select OK in the new assembly file. Save as Wheel Assembly Introduction to Solidworks for Technology Page 17
19 Using the Toolbox. Select the Design Library tab and then the Toolbox icon. (If it is not added select Add Toolbox). Browse for ISO. Then browse for Bolts and Screws, Slotted Head Screws and select Slotted Pan Head Drag and drop screw onto screen Configure the component to the following specification Size: M5 Length: 30mm Thread Display: Schematic Click OK, then click X to accept only 1 screw Introduction to Solidworks for Technology Page 18
20 Mating the Wheel Parts Select the mate command and select the cylindrical surface of the screw head and the hole to add as a concentric mate (automatic). You may need to flip direction. Click OK to accept mate. Also select Lock Rotation Add a second coincident mate, selecting the back of the screw head and the inner surface of the counterbore. Accept mate and Select OK. Save your work. Introduction to Solidworks for Technology Page 19
21 Go to the toolbox and browse for Plain Washer, Regular Flat Washer..Drag and drop in a washer. Configure to a M5 washer. Accept and press X. Mate the cylindrical washer surface to the cylindrical surface of the wheel. Select Lock Rotation and add this mate. Mate the flat surface of the washer to the back of the wheel. Click OK to exit the mate command Save your work The Wheel Assembly is now complete Introduction to Solidworks for Technology Page 20
22 Completing the Assembly Insert Wheel Assembly Open the Child s Toy Assembly and select Insert Components. Select the Wheel Assembly to insert. Press the Keep Visible pin down to allow you to insert the assembly multiple times. Use the rotate on insert toll to rotate 2 wheel assemblies about the Y axis Introduction to Solidworks for Technology Page 21
23 Click OK command to finish the insert Mating the Wheels to the Base To add mates between the screw and the base, hide the wheel; press the TAB key down and hover cursor over wheel. Mates to add: Concentric: cylindrical surface of screw and Tapped hole Lock rotation Coincident Back of washer with notch surface Show the wheel again by holding down SHIFT + TAB on keyboard and hover over where wheel is. Repeat this for each wheel assembly Save your work. The Assembly is now complete Introduction to Solidworks for Technology Page 22
24 Creating an Exploded View Select Exploded View. Click on Cab and select Y (vertical) arrow to move the Cab. Pull the Cab upwards. When in place click anywhere away from assembly. Note this is now Explode Step 1 Select the Wheel to move next. Move along the X axis. Note how the whole wheel assembly moves Introduction to Solidworks for Technology Page 23
25 Repeat for the two far wheel assemblies To explode the wheel assembly for the last wheel, tick Select the subassembly parts. This will allow you to explode the screw, washer and wheel individually Click OK To return to the assembled view, right click on the top of the design tree and select Collapse Introduction to Solidworks for Technology Page 24
26 To explode again right click on top of design tree and select Explode To edit an exploded view, click on the ConfigurationManager tab and select the ExplView1, then select Edit Feature Childs Toy Assembly.avi Introduction to Solidworks for Technology Page 25
27 Creating Drawings and Worksheets Adding Views Create a drawing from the Child s Toys Assembly Select an A3L sheet template (e.g. DCG A3L) In the View Palette, drag and drop the elevation by selecting Front view. Drag and drop the Top view for plan and Left view for end elevation. Notice how the views will auto project from elevation when dragged nearby. Change to a colour view by clicking on the view and selecting Shaded With Edges Introduction to Solidworks for Technology Page 26
28 Create the isometric View Click on the elevation and select Projected view from View Layout tab. Project out to the top lef. Hold the CTRL button down to move the isometric into the correct position. To change scale from1:2, click on view and change. Use custom scale to 1:1 Introduction to Solidworks for Technology Page 27
29 Dimension Drawing Select Model Items from Annotation tab. Select Selected Component as the Source and click on the Base in Plan. The Import items into all view is un-ticked.. Note: These dimensions are Driving dimensions imported from the parts Right click on any dimension you don t want and Hide Adjust the dimension to appear as neat as possible on the Plan Introduction to Solidworks for Technology Page 28
30 You can also add driven dimensions by clicking on Smart dimension and add dimensions manually Note: these dimensions are Driven dimensions; non-imported from parts Use the Note command to add Text Your Solution Drawing is now complete. Save your work Introduction to Solidworks for Technology Page 29
31 Detailed sheet Select Add Sheet. To add an extra view, (isometric from the front: 1. Open the assembly (use R-Key for recent documents) 2. Select the required view using the view selector cube 3. Press the SPACEBAR and click New View 4. Name the view and select OK 5. Save the file 6. Open the drawing and in the view palette refresh the views 7. Drag and drop the new view into the drawing Click on the view and select Show in exploded state To explode Add a detail view of the wheel Adjust the circle centre, radius and position of view as required Introduction to Solidworks for Technology Page 30
32 Creating worksheets Open the Base part. Open Save As. In the Design Tree select the features as shown and Delete. Select Save a copy and open. Save as Base Outline Introduction to Solidworks for Technology Page 31
33 In the copied part, delete the features as shown. Save the part Open the drawing (R-key) Add another sheet and add the orthographic views as before In the View Pallete browse for the Base outline part. Drag in the current isometric view Introduction to Solidworks for Technology Page 32
34 Add appropriate notes to the worksheet and save Introduction to Solidworks for Technology Page 33
35 PhotoView 360 PhotoView 360 is fully integrated into SolidWorks To add in render toolbar see Open the Childs Toy Assembly. Select the render tools tab and Render Region. Adjust the region to around the assembly Introduction to Solidworks for Technology Page 34
36 Select Final Render and allow PhotoView 360 to create the Rendered image. Save Image as Childs Toy1 Exit PhotoView 360 and open the exploded view of the assembly. Render the image as above and save as Childs Toy2 Introduction to Solidworks for Technology Page 35
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