CATIA Training Exercises Wireframe and Surface Design Version

CATIA Training Exercises Wireframe and Surface Design Version 5 Release 9 June 2002 EDU-CAT-E-WFS-FX-V 5 R 9 Copyright DASSAULT SYSTEMES 2002 1

Table of Contents 1. Master Exercise: Mobile Phone Creating the wireframe geometry Creating the surfaces Trimming and joining the body surfaces Creating the part body Modifying the geometry 2. Recap Exercise: Button Creating the wireframe geometry Creating the surfaces Creating the solid Modifying the geometry 3. Exercise: Wrench Body Creating the surface of the handle Creating a lofted surface to link the parts Creating the side surface of the head Creating a connecting surface Completing the wrench body Copyright DASSAULT SYSTEMES 2002 p. 3 p. 7 p. 12 p. 15 p. 19 p. 21 p. 23 p. 24 p. 26 p. 28 p. 31 p. 33 p. 37 p. 39 p. 42 p. 44 p. 46 2

Mobile Phone Exercise Mobile Phone: Presentation Mobile Phone (1): Creating wireframe geometry Mobile Phone (2): Creating basic surfaces Mobile Phone (3): Trimming and joining the body surfaces Mobile Phone (4): Creating the part body Mobile Phone (5): Modifying the Geometry Copyright DASSAULT SYSTEMES 2002 3

And now practice in the context of the Mobile phone 1 Enter the Wireframe and Surface Design workbench Create the wireframe geometry Create the surfaces Enter the Part Design workbench 2 Trim and join the body surfaces Create the part body 4 3 5 Modify the geometry Copyright DASSAULT SYSTEMES 2002 4

Exercise Mobile Phone : Presentation 35 min. In this exercise you will see how to create a mobile phone body using the Wireframe and Surface Design and Part Design workbenches: m Creating wireframe elements (Points, splines, combine curves, circles, lines) m Creating surfaces (swept, extruded, revolved surfaces) m Manipulating surfaces (trim, symmetry, join) m Creating solid from surface (Close, fillet, shell) m Modifying the geometry Copyright DASSAULT SYSTEMES 2002 5

Design Intent : Mobile Phone • Creation of guide and center curves by using combine, lines, sketcher, and splines. • Creation of surfaces using Sweep, Extrude and Revolution • Operations on surfaces using Trim and Join • Creation of solid from surfaces using Close, Fillet and Shell • Modification of the geometry by changing parameters of the surface definition Copyright DASSAULT SYSTEMES 2002 6

Exercise Mobile Phone: Creating the wireframe geometry 10 min. Create the guide curves and profiles. Copyright DASSAULT SYSTEMES 2002 7

Do It Yourself (1/4) Part used: Mobile_phone_step 1 -1. CATPart Guide curve 1 Guide curve 2 1 - Create these points : (0, 0, 9), (40, 0, 7. 5), (60, 0, 6), (80, 0, 5. 8) and (90, 0, 5. 8). 2 - Draw a spline passing through these points imposing a tangency condition with the X axis at the two extremities. 3 - Create these points : (0, 17, 0), (20, 0), (40, 19, 0), (60, 18, 0) and (90, 18, 0). 4 - Draw a spline passing through these points imposing a tangency condition with the X axis at the last extremity. 5 - Create a combine curve using the two previous spline curves. Rename it “Guide curve 1” 6 - Create these points : (0, 0, -3), (70, 0, -4) and (90, 0, -4). 7 - Draw a spline passing through these points imposing a tangency condition with the X axis at the last extremity. 8 - Create a combine curve using the last created spline curve and the second spline curve. Rename it “Guide curve 2”. Copyright DASSAULT SYSTEMES 2002 8

Do It Yourself (2/4) 7 - Create this sketch in the YZ plane : Rename it “Profile 1”. 8 - Create this circle centered on the point (70, 0, 0): 9 - Create the circle centered on the point (20, 0, 0): Copyright DASSAULT SYSTEMES 2002 9

Do It Yourself (3/4) 7 - Create a combine curve using the first created spline and the second circle. Rename it “Guide curve 3”. 8 - Create a combine curve using the third created spline and the second circle. Rename it “Guide curve 4”. 9 - Create a combine curve using the first created spline and the first circle. Rename it “Guide curve 5”. 10 - Create a combine curve using the third created spline and the first circle. Rename it “Guide curve 6”. 11 - Create a line starting from the point (0, 0, -300) and X directed (whatever it’s length, it will be used as an axis). Copyright DASSAULT SYSTEMES 2002 10

Do It Yourself (4/4) Create this sketch in the YZ plane and rename it “Profile 2”. Copyright DASSAULT SYSTEMES 2002 11

Exercise Mobile Phone: Creating the surfaces 10 min. Create swept, extruded and revolved surfaces. Copyright DASSAULT SYSTEMES 2002 12

Do It Yourself (1/2) Part used: Mobile_phone_step 2 -1. CATPart 1 - Create a swept surface using “Guide curve 1” and “Guide curve 2” as guide curves, the sketch “Profile 1”as profile and its two vertex points as anchor points. 2 - Create a circle swept surface using “Guide curve 3” and “Guide curve 4” as guide curve and “Profile 2” as profile and its two vertex points as anchor points. 3 - Create a circle swept surface using “Guide curve 5” and “Guide curve 6” as guide curve and “Profile 2” as profile and its two vertex points as anchor points. Note : switch on the option “Position Profile” for the two previous swept surfaces. P 1 users have to load the next CATIA Part to go on. Copyright DASSAULT SYSTEMES 2002 13

Do It Yourself (2/2) 4 - Extrude the spline 3 using the ZX plane as direction (Length=25 mm). 5 - Create a revolution surface using Spline 1 as profile and Line 1 as axis (Angle 1=0 deg and angle 2=5 deg). Copyright DASSAULT SYSTEMES 2002 14

Exercise Mobile Phone: Trimming and joining the body surfaces 5 min. Trim the surfaces by selecting the surface area you want to keep. Copyright DASSAULT SYSTEMES 2002 15

Do It Yourself (1/3) Part used: Mobile_phone_step 3 -1. CATPart 1 - Trim the first created swept surface with the revolution surface. 2 - Trim the previous trim surface with the extruded surface. Copyright DASSAULT SYSTEMES 2002 16

Do It Yourself (2/3) 3 - Trim the previous trim surface with the first circle swept surface. 4 - Trim the last trim surface with the second circle swept surface. Copyright DASSAULT SYSTEMES 2002 17

Do It Yourself (3/3) 5 - Symmetrize the resulting surface using the XZ plane as reference and join it with the last trim surface. Copyright DASSAULT SYSTEMES 2002 18

Exercise Mobile Phone: Creating the part body 5 min. Close the body surface into a solid, then fillet and shell the solid. Copyright DASSAULT SYSTEMES 2002 19

Do It Yourself Part used: Mobile_phone_step 4 -1. CATPart Access the Part Design workbench and define in work object the “Solid” body. 1 - Close the surface Body surface. 2 - Add variable fillets on the two side top edges (from 4 mm to 2 mm) 3 - Add 1 mm edge fillets on these four edges : Copyright DASSAULT SYSTEMES 2002 20

Exercise Mobile Phone: Modifying the geometry 5 min. Modify the geometry by modifying a construction element. Copyright DASSAULT SYSTEMES 2002 21

Do It Yourself Part used: Mobile_phone_step 5 -1. CATPart You will modify the overall shape of the part by changing the parameters of a construction element. 1 - Display the second spline and its points. 2 - Double-click on Point. 6 to change its Y component value to 16 mm. Copyright DASSAULT SYSTEMES 2002 22

Recap Exercise In this exercise you will see how to create a button body using the Wireframe and Surface Design and Part Design workbenches: 25 min. m Creating the profiles m Extruding the profile m Creating the solid part m Modifying the geometry Copyright DASSAULT SYSTEMES 2002 23

Exercise Button (Step 1) : Creating the wireframe geometry 5 min. In this step you will: m Create the points m Create the profile curves m Create the direction lines Copyright DASSAULT SYSTEMES 2002 24

Do It Yourself Pt 5 Line. 1 Pt 4 Pt 3 Pt 2 Spline. 1 Pt 1 Points, Spline, Line (1 -, 2 -, 3 -) Sketch on XY plane (4 -) Line on YZ plane (5 -) Button_step 1. CATPart Create the wireframe geometry: 1 - Create 5 points : Pt 1(0, 0, 5), Pt 2(0, 10, 9), Pt 3(0, 23, 7), Pt 4(0, 30, 8), Pt 5(-20, 30, 7) 2 - Create a spline passing through Pt 1 to Pt 4 3 - Create a line passing through Pt 4 and Pt 5 4 - Draw a sketch on XY plane with two coincidences and a radius of 20 mm 5 - Draw a vertical line on YZ plane Copyright DASSAULT SYSTEMES 2002 25

Exercise Button (Step 2) : Creating the surfaces 5 min. In this step you will: m Create extruded surfaces Copyright DASSAULT SYSTEMES 2002 26

Do It Yourself Sketch. 2 Line. 1 Spline. 1 Sketch. 1 Surface Extrude. 1 (1 -) Surface Extrude. 2 ( 2 -) Button_step 2 -3. CATPart Create the basic surfaces: 1 - Create the first extruded surface : select profile Sketch. 1 and direction Sketch. 2 2 - Create the second extruded surface : select profile Spline. 1 and direction Line. 1 Copyright DASSAULT SYSTEMES 2002 27

Exercise Button (Step 3): Creating the solid 10 min. In this step you will: m Create a pad using the existing surfaces as limits m Add fillets on edges m Shell the part Copyright DASSAULT SYSTEMES 2002 28

Do It Yourself (1/2) Sketch. 3 on XY plane (1 -) Sketch. 4 YZ plane (2 -) Button_step 4. CATPart 1 - Create a sketch (rectangular contour) on the XY plane 2 - Create a sketch (trapezoidal contour) on the YZ plane Copyright DASSAULT SYSTEMES 2002 29

Do It Yourself (2/2) Pad up to surface (3 -) Split of pad (4 -) Pad up to surface (5 -) Fillets (6 -) Shell (7 -) 3 - Create a pad on Sketch. 3, up to the Extrude. 2 surface 4 - Split Pad. 1 with Extrude. 1 as splitting surface 5 - Create a pad on Sketch. 4 up to the Extrude. 1 surface 6 - Make 1. 5 mm fillets on the 6 horizontal and vertical edges 7 - Shell the bottom faces with 1 mm (5 faces) Copyright DASSAULT SYSTEMES 2002 30

Exercise Button (Step 4): Modifying the geometry 5 min. In this step you will: m Modify the geometry by moving the definition points of the spline and changing parameters in the Sketcher Copyright DASSAULT SYSTEMES 2002 31

Do It Yourself Pt 3 Point on spline (1 -) Sketch. 1 (2 -) Button_step 5. CATPart 1 - Double click on Pt 3 and change the Z value to 5 mm to modify the shape of the spline 2 - Open Sketch. 1 to change the radius value to 25 mm Copyright DASSAULT SYSTEMES 2002 32

Wrench Body Exercise Wrench Body: Presentation Wrench Body (1): Creating the Surface of the Handle Wrench Body (2): Creating a Lofted Surface to Link the Parts Wrench Body (3): Creating the Side Surface of the Head Wrench Body (4): Creating a Connecting Surface Wrench Body (5): Completing the Wrench Body Copyright DASSAULT SYSTEMES 2002 33

Exercise Wrench body : Presentation 35 min. In this exercise you will learn how to create a wrench body using the Wireframe and Surface Design and Part Design workbenches : m Creating wireframe elements (point, line, spline) m Creating surfaces (revolution, loft, sweep) m Manipulating surfaces (symmetry, join) m Creating solid from surface (close, extrude) Copyright DASSAULT SYSTEMES 2002 34

Design Intent : Wrench Body • Creation of guide, section and spine curves using spline, sketcher, project and split • Creation of revolution, loft and sweep surfaces • Creation of solid from surfaces using close and thick Copyright DASSAULT SYSTEMES 2002 35

And now practice in the context of the Wrench Body 1 Enter the Wireframe and Surface Design workbench Create a connecting surface 4 Create the side surface of the head Enter the Part Design workbench 5 Create the surface of the handle Create a lofted surface to link the parts 2 3 Complete the wrench body Copyright DASSAULT SYSTEMES 2002 36

Exercise Wrench body : Creating the Surface of the Handle 10 min. Create the surface of the handle by revolving a spline defined in 3 D. Copyright DASSAULT SYSTEMES 2002 37

Do It Yourself Part used: Wrench_body_step 1. CATPart Vertex 2 Vertex 1 C B A Spline 1 Points, Spline (1 -, 2 -, 3 -) Revolving surface (4 -) 1 - In the WIREFRAME Open Body create three points : (115, 7, 0), (122, 6, 0) and (127, 5, 0). Rename them Point A, Point B and Point C. 2 - Create a spline selecting Vertex 1 then points A to C and finally Vertex 2. 3 - Impose horizontal tangency at the end points of the spline. 4 - In the SURFACES Open Body create a surface, revolving the spline 360 degrees around the horizontal line of the sketch. (360 -degree revolution is needed for the downstream close operation to create a solid in Part Design). Copyright DASSAULT SYSTEMES 2002 38

Exercise Wrench body : Creating a Lofted Surface to Link the Parts 10 min. Create a lofted surface to associate the head with the link. Copyright DASSAULT SYSTEMES 2002 39

Do It Yourself (1/2) Link end face Part used: Wrench_body_step 2. CATPart Head bottom face Sketch. 3 Offset plane Plane and Sketch. 3 (1 -, 2 -) Sketch. 4 (3 -) Middle points (4 -) 1 - In the WIREFRAME Open Body create a plane with a 7. 2 mm distance from the end face of the link. 2 - On the created plane create an arc of a circle (radius =7. 2). Define three coincidences, two between the end points of the arc and the H-axis of the Sketcher and one between the center point of the arc and the V-axis of the Sketcher. 3 - On the bottom face of the head, create an arc passing through the two vertices of the face (radius =24). Define four coincidences, two between the arc and the vertices of the bottom face and two between the end points of the arc and the H-axis of the Sketcher. 4 - Create the middle points of Sketch. 3, Sketch. 4 and of the edge curve of the link end face. Copyright DASSAULT SYSTEMES 2002 40

Do It Yourself (2/2) Line. 1 Spline. 2 S 1 G 1 Spine S 3 G 2 S 2 G 3 Spline. 4 Spline. 3 Splines and line (5 -, 6 -) Lofted surface (7 -) Symmetry and join (8 -, 9 -) 5 - Create three splines, two passing through the two sets of end points of the three arcs and one passing through the set of middle points created on the three arcs. The three arcs are Sketch. 3, Sketch. 4 and the edge curve of the link end face. Impose an horizontal tangency to each spline on the link end. 6 - Create a line normal to the end face to the link (length=20) from Point. 1. 7 - In the SURFACES Open Body create a lofted surface by selecting three sections (Sketch. 4, Sketch. 3 and the edge curve of the link end face), three guide curves P 1 users should create three (Spline. 2, Spline. 3 and Spline. 4) and a spine (Line. 1). sections loft in two times. 8 - Apply a symmetry to the lofted surface with respect to the XY plane. 9 - Join the lofted surface and the symmetry. Copyright DASSAULT SYSTEMES 2002 41

Exercise Wrench body : Creating the Side Surface of the Head 10 min. Create the side surface of the head by a sweeping a profile. The profile and guide curves are created from the existing curves by projection and re-limited. Copyright DASSAULT SYSTEMES 2002 42

Do It Yourself Part used: Wrench_body_step 3. CATPart Side face of the head Extracted edges Split of Sketch. 4 Side surface 1 - In the WIREFRAME Open Body extract with tangency continuity the upper and lower edges of the head. . 2 - Split sketch. 4 with the side face of the head. 3 - In the SURFACES Open Body define the side surface: create a sweep with a profile (Split. 1=sketch. 4 split) and two guide curves (Extract. 1 and Extract. 2). Copyright DASSAULT SYSTEMES 2002 43

Exercise Wrench body : Creating a Connecting Surface 10 min. Create a connect surface at a junction by sketching the profile and revolving it. Copyright DASSAULT SYSTEMES 2002 44

Do It Yourself Part used: Wrench_body_step 4. CATPart Sketch. 5 (1 -) Surface of revolution (2 -) 1 - In the WIREFRAME Open Body sketch the fillet profile on XY plane. - activate the option Construction elements. - create lines on the bottom and top horizontal edges and on the vertical edge of the link by intersecting the 3 D elements. - define two coincidences between the profile and the bottom horizontal edge and between the profile and the vertical edge, two horizontal tangencies at the ends of the profile and two radius constraints (18 mm and 5 mm). 2 - In the SURFACES Open Body create the surface by revolving Sketch. 5 around the horizontal axis of Sketch. 1 (360 deg). Copyright DASSAULT SYSTEMES 2002 45

Exercise Wrench body : Completing the Wrench Body 5 min. Create solids by extruding and closing the surfaces. Remove the exceeding solid by pocketing. Copyright DASSAULT SYSTEMES 2002 46

Do It Yourself (1/2) Part used: Wrench_body_step 5. CATPart Join. 1 Revolute. 1 1 Revolute. 2 Part. Body Initial Part Sweep. 1 Thick / Mirror / Close (2 -, 3 -, 4 -) 1 - Exit the Wireframe and Surface Design workbench and enter the Part Design workbench. 2 - Thick the surface Sweep. 1 by 1. 5 mm inwards. 3 - Mirror the Part. Body. 4 - Close the surfaces Revolute. 1, Revolute. 2 and Join. 1. Copyright DASSAULT SYSTEMES 2002 47

Do It Yourself (2/2) Sketch. 6 (5 -) Pocket (6 -) 5 - Sketch two rectangular contours on the XY plane and build four coincidences, two between the contours and the V-axis of the Sketcher and two between the contours and the corresponding horizontal edge of the head. 6 - Remove the exceeding solid by pocketing (depth=20 mm, Mirrored extent). Copyright DASSAULT SYSTEMES 2002 48