Catia+Part+Design+Book

CATIA Part Design & Sketcher

CATIA® V5R6

TABLE OF CONTENTS Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Manual Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Log on/off procedures for Windows NT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 To log on . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 To logoff . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 CATIA Version 5 Screen . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6 Part Design Screen . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7 Pull-down Menus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 Edit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10 Insert . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13 Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14 Window . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16 Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 Bottom Toolbar in Part Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Part Design Workbench . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Sketcher Screen . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 Sketcher changes to bottom toolbar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21 Sketcher Workbench . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22 Working with Documents . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24 Creating a new document . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24 Opening an existing document . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25 Saving a document . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Closing a document . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27 Basic Sketcher . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29 Basic Shapes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29 Creating a new part with a new sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30 Saving and closing the part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30 Rectangle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Oriented Rectangle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32 Parallelogram . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 33 Elongated Slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34 Elongated Curved Slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Keyhole . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37 Hexagon . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38 Circle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 Circle through 3 points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Circle with Cartesian coordinates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41 Circle tangent to 3 elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 Arc through 3 points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 Arc through 3 points using limits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Arc . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Spline . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 Connect Curve . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 © Wichita State University

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CATIA® V5R6

Ellipse . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 49 Parabola . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 Hyperbola . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51 Conic . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 52 Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53 Unlimited Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54 Bi-tangent Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Bisect Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 Axis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58 Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59 Point using coordinates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60 Equidistant points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61 Intersection Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63 Projection Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 Profiles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66 Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83 Dimensional Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83 Geometrical Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83 Modifications to profiles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 Corner . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 Chamfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129 Trim and Break . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 132 Hide/Show . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 137 Basic Part Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Basic Shapes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Pad . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140 Pocket . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 148 Multiple Profiles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151 Shaft . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153 Groove . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156 Hole . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 Rib . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 171 Slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 173 Stiffener . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 175 Modifications to Shapes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177 Fillet . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177 Chamfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185 Draft Angle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187 Shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 191 Thickness . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 193 Modifying values . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 195 Interfacing with Sketcher . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 200 Advanced Sketcher . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 205 3-D Elements on Sketch Plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 205 Construction Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 210 Advanced Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 215 Sketch Transformations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 223 Table of Contents, Page ii

©Wichita State University


CATIA® V5R6

Sketch Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233 Advanced Part Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 237 Part Transformations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 237 Patterns . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 242 Modifying Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253 Inserting Bodies and Boolean Operations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 266 Inserting Part Bodies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 266 Boolean operations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 267 Part Design Lofts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271 Part Design Using Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 273 Applying Materials . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 277 Reference Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 279 Offset from plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 279 Parallel through point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 280 Angle/Normal to plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 281 Through three points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 281 Through two lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 282 Through point and line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 283 Through planar curve . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 283 Normal to curve . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284 Equation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284 Tangent to surface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 285 Mean through points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 285 Problems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 287 Problem #1.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 287 Problem #2.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 288 Problem #3.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 289 Problem #4.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 290 Problem #5.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 291 Problem #6.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 292 Problem #7.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 294 Problem #8.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 295 Problem #9.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 296 Problem #10.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 297 Problem #11.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 298 Problem #12.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 299 Problem #13.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 300 Problem #14.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301 Problem #15.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 302 Problem #16.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 303 Problem #17.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 304 Problem #18.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 305 Problem #19.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 306 Problem #20.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307 Problem #21.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 308 Problem #22.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 309 Problem #23.0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 310 © Wichita State University

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CATIA Part Design & Sketcher Problem Problem Problem Problem

#24.0 #25.0 #26.0 #27.0

CATIA® V5R6

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 312 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 313 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 314

Appendix A . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 315 Customize - Start Menu . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 315 Customize - User Workbenches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 316 Customize - Toolbars . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 316 Customize - Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317 Customize - Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317 Appendix B . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319 General - Display - Tree . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319 General - Display - Visualization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 320 General - Parameters - Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 321 General - Parameters - Units . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 322 Mechanical Design - Part Design - General . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 323 Mechanical Design - Part Design - Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324 Mechanical Design - Sketcher . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 325 Appendix C . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 327 Material Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 327 Construction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 327 Fabrics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328 Metal . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 329 Other . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 330 Stone . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 331 Wood . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 332 Applying a material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 333 Properties of a material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 334 Rendering . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 334 Inheritance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 335 Feature Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 335 Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 336 Drafting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 336

Table of Contents, Page iv



CATIA® V5R6

Introduction CATIA Version 5 Part Design and Sketcher Upon completion of this course the student should have a full understanding of the following topics: -

Creating sketches

-

Constraining sketches

-

Modifying sketches

-

Creating parts

-

Modifying parts

-

Performing boolean operations on parts

-

Basic use of surfaces in part design

-

Applying materials to parts

© Wichita State University

Introduction, Page 1


CATIA® V5R6

Manual Format It is important to understand the format of the manual in order to use it most effectively. This manual is designed to be used along with an instructor; however, you will need to do a lot of reading as well, in order to fully understand CATIA Version 5. The exercises in this book will list steps for you to complete, along with explanations that try to inform you what you have just done and what you are getting ready to do. The actual steps are in bold type and the information that follows the steps is for your benefit. Anything that appears in italics refers to a message CATIA provides—this includes information in pull-down menus, pop-up windows and other messages. Bold type is also used to call your attention to key terms you may not yet be familiar with. An example of a step and its explanation is shown below (note: normally the lines will not be there): Select a location to the right of the origin. This specifies the other end point of the line. You will continue specifying locations in order to complete your profile. It should appear similar to the diagram shown below.

As you can see, the desired action blends in with the text except that it appears in bold. The information following the step explains what that step accomplished and where you are going next. It is important for you to read this information to help in your understanding of CATIA Version 5. Also, you will find that the exercises build upon themselves. Later exercises often assume you know how to do certain steps which have been covered in earlier exercises. If you did not quite pick up what you needed to know from an exercise, you will probably wish to review it several times before moving on to the more advanced sections. As you progress through the manual, it expects that you are learning and therefore you are able to do a lot more with fewer steps. Eventually, you are expected to be able to create parts without any steps.




CATIA® V5R6

Part Design & Sketcher CATIA Version 5 uses the Sketcher as its principal method to create profiles. These profiles can be constrained using many different types of constraints. The first objective of the course is to learn to use the Sketcher and constrain your profiles to the desired specifications. If you have used the Dynamic Sketcher from CATIA Version 4, this will look very similar. Otherwise it is a new environment and it can be frustrating at first, especially if you already know CATIA Version 4. However, in time you will find that it is a very powerful method for creating profiles, and is easy to use. The second objective of the course is to use these sketches in part design. The sketches are used to define the two-dimensional cross-sections to be used to design three-dimensional shapes. There are a few different shapes that can be made as well as various operations that can be performed on them. By combining these shapes and operations, you can design a variety of parts. The third objective of the course is to familiarize you with the advanced methods of creating sketches and parts. This includes using construction geometry and projecting threedimensional geometry to the sketch plane. This will include the use of formulas to set up typical values at multiple locations as well as more complex formulas to provide a more dynamic sketch. In terms of part design, you will learn how to use multiple parts and perform boolean operations on them. The fourth objective is to become efficient at modifying your designs. You can modify your design either by changing the parameters of a part operation or by modifying the sketch that was used. In CATIA Version 5 this is fairly simple, and the modification of your design is the real strength of part design. The fifth objective is to introduce the use of wireframe and surfaces in the part design process as well as applying various materials to your design. This is meant only to be an introduction and not a complete course on these subjects. In conclusion: You should be able to design many parts using the Sketcher and the Part Design workbenches of CATIA in an efficient manner. As mentioned before, you may find it frustrating at first but very natural by the end of the course.




CATIA® V5R6

Log on/off procedures for Windows NT To log on: The monitor screen should have a gray box displayed with Press Ctrl + Alt + Delete to log on.

Hold down the Ctrl and Alt keys and press Delete. Select the User name box. This will allow you to type in your user name in the space provided. Type in your user name (do not press Enter). This is the user name that was provided to you at the beginning of class. Select the Password box. This will allow you to type in your password in the space provided. Type in your user password (do not press Enter). This is the password that was provided to you at the beginning of class. Select the Domain box. This allows you to choose which domain you wish to log into. Select CADLAB. The domain CADLAB is the proper domain for your user.

The Logon Information box should look similar to the one above except with your user name and your password.




CATIA® V5R6

Select OK. When you select OK with your mouse, you are telling the computer that the information that is in the Logon Information box is correct and you are ready to log in. If for some reason it can not log you in, you need to verify that you typed in the correct information. Once you are logged into the system then you should see a CATIA icon on your screen. Double-click on the CATIA icon.

This will run CATIA.

To logoff: Select the pull-down menu File.

Select Exit. This will exit you from CATIA; you will still need to log off the system. Hold down the Ctrl and Alt keys and press Delete. The Windows NT Security box should appear.

Select Logoff... A new box will appear, allowing you to cancel the logoff in case you ever happen to select that option by mistake. (This isn’t terribly likely to happen.) Select OK. This will log you off the system.




CATIA® V5R6

CATIA Version 5 Screen

This is how CATIA Version 5 looks when you first run it. There are various areas of the screen which need to be pointed out. A

This is your specification tree. Currently it has an entity referred to as a product. You will be working with parts in this class so this will change to be a part and as you perform different actions the tree will reflect those actions.

B

The pull-down menus are used for a variety of different tasks. These will be discussed in detail later in the book.

C

The Welcome to CATIA V5 window allows you to change to different workbenches that are available. In this class, you will primarily be using the Part Design workbench.

D

The bottom row of icons, or toolbar, contains various icons that will allow different actions to be performed. These will be discussed in detail later in the book.

E

The current workbench is the Product Structure workbench. The current workbench can be switched to a different one by using the appropriate icon on the workbench.

The workbenches and the toolbar are customizable. However, this book will assume that they are in their original location. If you change the positions of the icons, you will be responsible for knowing where you put them. Introduction, Page 6



CATIA® V5R6

Part Design Screen

This is how the Part Design screen normally looks when you first start a new part. Notice that the pull-down menus remain the same. However the workbench on the side changes to the Part Design workbench and the bottom row of icons has some additional icons. A

The xy plane, yz plane and zx plane are represented in the specification tree for every part that you create. These are the standard planes that CATIA uses.

B

Notice the definition for your first partbody is also located in the specification tree when you begin a new part.

C

These are the actual planes that are represented in the specification tree. You will normally use these to help design your part.

D

This is the 3D compass and it has three separate parts. The letters X, Y and Z represent the axes. The Z axis is the default orientation. It has a free rotation handle, a compass manipulation handle and a privileged plane. The point close to the Z axis is the free rotation handle. The red square is the compass manipulation handle. The XY plane is the privileged plane which is located at the base of the compass. This has various options throughout CATIA, however in this class you will primarily be using it as another method of rotating your part around.

E

This axis represents the true rotation of the part. The compass, by contrast, can be attached to actual objects.




CATIA® V5R6

Pull-down Menus

File

New

Creates a new analysis, drawing, part or product

New from

Creates a new document based on an existing one

Open

Opens an existing document

Close

Closes the current document

Save

Saves the current document with the same name

Save As

Saves the current document with a name you specify

Save All

Saves all documents that are currently opened

Save All As

Saves all documents that are currently opened with a name you specify

Print

Prints the current document

Desk

Allows you to view the relationships between documents

Send To

Allows you to send CATIA data to an e-mail or another directory

Exit

Exits CATIA

The other documents listed there are the most recent documents that were opened. This allows you to open them again quickly.




CATIA® V5R6

Edit

Undo

Undoes the last option. You can undo multiple options in a row.

Repeat

Redoes the last undo option. You can redo multiple options in a row.

Update

Updates your document with changes

Cut

Cuts the selected objects from the document

Copy

Copies the selected objects

Paste

Pastes the previously cut or copied objects in the document

Paste Special

Gives additional options to the paste

Delete

Deletes selected objects

Search

Searches your document for certain objects

Selection Sets

Adds or deletes objects from a selection set or creates one

Define Selection Set Takes preselected geometry and stores it in a selection set Links

Edits document links

Properties

Displays and edits graphic properties

Scan or Define in Work Object


Defines the current work object and allows you to scan through the part



CATIA® V5R6

View

Toolbars

Allows you to view or hide toolbars. You can also customize a toolbar.

Geometry

Toggles between seeing and not seeing geometric elements, also known as geometry

Specification

Toggles between seeing and not seeing the specification tree




CATIA® V5R6

Compass

Toggles between seeing and not seeing the compass

Reset Compass

Resets the compass to its original location if moved

Tree Expansion

Allows you to expand or collapse the levels in your specification tree.

Specifications Overview

Gives an overview window of the specification tree allowing you to zoom in on areas of the tree

Geometry Overview

Gives an overview window of the geometry in your document, allowing you to zoom in on an area of the geometry

Fit All In

Zooms the display so as to make all the geometry fit on the screen

Zoom Area

Zooms in on an area that you specify

Zoom In Out

Zooms in or out on your part by using the left mouse button to drag up or down

Pan

Drags the display of your part around with the left mouse button

Rotate

Rotates the display of your part around with the left mouse button

Modify

Named Views

This allows you to look at your geometry in a variety of ways. You can Zoom In or Zoom Out. You can specify a plane and look normal to the plane with the Normal View. You can simulate what it looks like as you turn your head right or left using Turn Head. It will also let you Fly Through or Walk Through your design. The Accelerate and Decelerate options control how fast you fly or walk. The Previous view and Next view options allow you to page through the different views that you have defined with the other options. The Look At option allows you to specify the direction you want to look at your part. Retrieves different views and it allows you to add new views for retrieval at a later time.




CATIA® V5R6

Render Style

The different render styles control how the parts will be displayed. You can customize your own type of render style using the Customize View option. You can also view your part either in Perspective or in Parallel. In parallel mode, the part is shown with every dimension exactly to scale; in perspective mode, the area of your part that is closer to the screen appears larger than the area that is farther away. This only affects your part visually, not geometrically.

Navigation Mode

Switches between Examine, Walk and Fly modes.

Lighting

Varies ambient lighting effects

Depth Effect

Clips geometry between clipping planes

Ground

Visually inserts a plane at ground level

Magnifier

Creates a zoomed in view of your part in a separate window

Hide/Show

Hides or shows geometry. The Swap visible space option will toggle between the hidden side and the show side.

Full Screen

Shows your geometry using the full screen, with no menus or toolbars. To turn off full screen mode, use the right mouse button.




CATIA® V5R6

Insert

Object

Inserts an object such as a spreadsheet or a word processing document

Body

Inserts a new body in to your part

Annotations

Inserts annotations in to your part, same as Part Design options

Constraints

Inserts constraints, same as the Sketcher options

Sketcher

Runs the Sketcher, same as the Sketcher icon in Part Design

Axis System

Defines a new axis system

Sketch-Based Features

Inserts various Sketcher features, same as the Sketcher options

Dress-Up Features

Inserts fillets, chamfers, etc., same as the Part Design options

Surface-Based Features

Inserts various features using surfaces, same as the Part Design options

Transformation Features

Inserts various transformation features, same as the Part Design options

Boolean Operations

Inserts boolean operations between part bodies

Advanced Replication Tools Allows you to create and store features




CATIA® V5R6

Tools

Formula

Allows you to apply formulas to your part

Image

Capture allows you to capture images off of the screen into various formats such as TIFF, JPEG, PNG or BMP. The Album option is where the captured images go by default. This option will allow you to access them. The Video option allows you to record what you are doing and replay it.

Macro

Records, edits and runs macros

Parent/Children

Shows the relationships between components of the part

Customize

Customizes the toolbars, more information in Appendix A




CATIA® V5R6

Visualization Filters Allows you to create and apply filters

Options

Customizes settings, more information in Appendix B

Conferencing

Tools available for conferencing a CATIA session




CATIA® V5R6

Window

New Window

Creates a new window

Tile Horizontally

Tiles your windows horizontally so they do not overlap

Tile Vertically

Tiles your windows vertically so they do not overlap

Cascade

Cascades your windows so they overlap but you can still see the top and left side of each window

The other windows listed are the windows that are currently opened. You can switch windows by selecting from the list.




CATIA® V5R6

Help

CATIA V5 Help

Gets contextual help

CATIA User Companion

Activates the user companion if available

Contents, Index and Search Allows you to search the online help What’s This?

Allows you to select an option to get information about it

User Galaxy

Goes to Dassault Systèmes user galaxy

About CATIA V5

Displays copyright information




CATIA® V5R6

Bottom Toolbar in Part Design

Creates a new part

Positions view normal to a plane

Open an existing part

Changes view

Saves the current part

Changes render style

Prints the current part

Hides/shows elements

Cuts the selected objects

Swaps visible space

Copies the selected objects

Applies material to a part

Pastes what’s been copied or cut

Measures between two items

Undoes the last action

Measures an item

Redoes the last undo

Measures inertial properties

Gets help on a selected item

Updates a part

Generates a formula

Creates an axis system

Generates a table

Tolerancing

Knowledge inspector

Creates a datum

Goes to fly mode

Opens a catalog

Fits all of the geometry in window

Change current body

Pans the display window

Performs a draft analysis

Rotates the geometry

Performs a curvature analysis

Zooms in Zooms out




CATIA® V5R6

Part Design Workbench Changes workbenches

Shells out a side

Selects geometry

Adds thickness to a side

Goes to Sketcher

Creates thread notation

Creates a pad

Adds thickness to a surface

Creates a pocket

Splits an object

Creates a shaft

Closes a surface

Creates a groove

Sews a surface into a part

Creates a hole

Translates an object

Creates a rib

Rotates an object

Creates a slot

Symmetries an object

Creates a stiffener

Mirrors an object

Creates a loft

Generates a rectangular grid

Removes a loft

Generates a circular grid

Fillets with a constant radius

Generates a user-defined grid

Fillets with a variable radius

Scales an object

Fillets between faces

Creates constraints by dialog

Fillets using a tri-tangent

Creates a constraint

Chamfers a corner

Creates text with a leader

Creates a draft angle

Creates a flag note

Draft reflect




CATIA® V5R6

Sketcher Screen

This is how the Sketcher screen normally looks when you first start a new sketch. Notice that the pull-down menus remain the same. However, the workbench on the side changes to the Sketcher workbench, and the toolbar at the bottom has some changes. Also notice the grid that appears when you are in Sketcher. This grid can be turned on and off using the pull-down menu Tools/Options. This grid will be discussed in more detail later in this book.




CATIA® V5R6

Sketcher changes to bottom toolbar When you go to the Sketcher, most of the icons in the bottom toolbar remain. A few new ones also appear: Cuts part by sketch plane. This is helpful when you need to use an edge of the crosssection to define a constraint. Toggles between snapping to a point of the grid or not snapping. In the Sketcher there is a grid defined in the default settings. This grid can be modified using the pull-down menus. If this icon is highlighted then when you sketch, your selections will snap to a point on the grid. If you do not have this icon selected then you can select anywhere in the sketch to define a point for your sketch. Toggles between creating standard geometry and construction geometry. When sketching, there are times when you just want to create some geometry to use for the construction of other geometry—you do not want it to be an actual part of your sketch in Part Design. If this icon is highlighted, the geometry you create will just be construction geometry, and will not be part of your sketch in Part Design. If you do not have this icon selected, you will be creating standard geometry that will be used in Part Design. Toggles between automatically generating geometric constraints or not. If it is highlighted, CATIA will automatically generate geometric constraints as you sketch your profile. If it is not highlighted, geometric constraints will not automatically appear. Toggles between automatically generating dimension constraints or not. If it is highlighted, CATIA will automatically generate dimension constraints as you sketch your profile. If it is not highlighted, dimensional constraints will not automatically appear.




CATIA® V5R6

Sketcher Workbench Changes workbenches

Creates a spline

Selects geometry

Creates a connect curve

Exits Sketcher

Creates an ellipse

Creates constraints by dialog

Creates a parabola

Creates a constraint

Creates a hyperbola

Creates constraints automatically

Creates a conic

Animates constraints

Creates a line

Creates a user-defined profile

Creates an unlimited line

Creates a rectangle

Creates a bitangent line

Creates an oriented rectangle

Creates a bisect line

Creates a parallelogram

Creates an axis

Creates an elongated slot

Creates a point

Creates an elongated curved slot

Creates a point using coordinates

Creates a keyhole

Creates equidistant points

Creates a hexagon

Creates an intersection point

Creates a circle

Creates a projected point

Creates a circle through 3 points

Creates rounded corners

Creates a circle using coordinates

Chamfers elements

Creates a circle tangent to 3 elements

Trims elements

Creates an arc through 3 points Creates an arc through 3 points using limits

Breaks elements Quick trim Closes elements

Creates an arc Introduction, Page 22



CATIA® V5R6

Symmetries elements Translates elements Rotates elements Scales elements Offsets elements Projects 3D geometry onto the sketch plane Intersects 3D geometry with the sketch plane Projects canonical edges onto the sketch plane




CATIA® V5R6

Working with Documents It is important for you to understand how to work with the documents and especially how to save them in order to be productive using CATIA Version 5. Creating a new document This allows you to start a new document. For this class you will normally start a Part document. This does not close any documents that are already opened, it only creates a new window with the document. Select the new icon in the bottom toolbar. This allows you to create a new document. The document that will be created depends on the selection you make, either an analysis, drawing, part, product or other. You see that there are many different types of documents that you can create in CATIA. Select Part.

Select OK. This will create a new part.




CATIA® V5R6

Opening an existing document This allows you to open a document that has been previously saved. This does not close any documents that are already opened, it only opens a new window with the document. Select the open icon in the bottom toolbar. This allows you to open an existing document. A File Selection window should appear.

This allows you to specify the folder that you want to look in and then specify the file or document that you want to open. Find the document that you want to open and select it. You can either open a document by selecting it and then selecting Open or you can just double-click on the file and it will automatically open. This step assumes that you just selected the file not double-clicked on it. The name of the document should appear in the File name box. Select Open. This should open the document.




CATIA® V5R6

Saving a document This allows you to save a document that you currently have opened. Select the save icon in the bottom toolbar. This will allow you to save the document with the current name. If this is the first time you saved this document then it will automatically open a Save As window allowing you to specify a name for the document. Otherwise it will just save the document with the same name it already has. If you want to save a document with a different name, you have to use the Save As option in the pull-down menu File. Select the pull-down menu File.

Select Save As. A Save As window should appear. You will need to specify which folder you want to save the document into and the name of the document.

Choose the correct folder and then enter the file name in the File name box. Select the Save button. Alternatively, you may press Enter. The document should save with the new name. Introduction, Page 26



CATIA® V5R6

Closing a document This allows you to close a document that is currently open with or without saving. If the document has not been saved, CATIA will ask you whether or not you want to save it. Select the pull-down menu File.

Select Close. If the document has already been saved and has not been modified, CATIA will close the current document. If the document has been modified and not saved, CATIA will open the Close window.

If you want to save the changes then press Yes. If the document has previously been saved, it will be saved again under the same name; otherwise, the Save As window will appear. If you do not want to save the changes, press No. To return to the document rather than closing it, select the Cancel button.




CATIA® V5R6

This page is intentionally left blank.




CATIA® V5R6

Basic Sketcher This section will cover the basic use of the Sketcher to create profiles for the Part Design package. This section will consist of four parts: basic shapes, profiles, constraints and modifications to profiles. It is assumed that you have the default icons selected in the bottom toolbar. This includes the snap-to-grid icon, the geometrical constraint icon and the dimensional constraint icon. These and the other options in the bottom toolbar will be discussed in more detail later in the manual. The pictures in this manual are shown without a grid; this is to make them easier to see. When you are sketching, though, you will have a grid by default. If you want to turn the grid off, you can use the pull-down menus. Basic Shapes This part will discuss the various shapes that can be created in the Sketcher using the icons on the Sketcher workbench. The purpose of this group of exercises is to introduce how to use those icons and generate the basic shapes. The usefulness of these shapes depend on the profile you are trying to create. Therefore you should just concentrate on what each icon allows you do and the corresponding shape it creates. Later in the class you will learn how to put everything together to generate your parts. The following exercises assume that you are in a new sketch. The first page shows you the necessary steps to begin a new model and start a new sketch on a particular plane. After that if you need help you will have to refer back to that page. Note: It may not be necessary to do all of the following exercises step by step. If you feel comfortable with the material then you can create all of the basic shapes on one sketch. If you struggle or would like more information then you can consult the individual exercise for that shape.


Basic Shapes, Page 29


CATIA® V5R6

Creating a new part with a new sketch Select the new icon in the bottom toolbar. This creates a new document. There are many types of documents possible, so next you will choose which type you want. Select Part.

Select OK. This will create a new part. Select the Sketcher icon. This will activate the Sketcher, but first CATIA needs to know which plane you wish to use for your sketch. Select the yz plane. You can either select the yz plane symbol in the center of your screen or you can select the yz plane name in the specification tree. By selecting this plane you are telling the computer that you want to sketch a profile in that plane. CATIA will rotate the window around so that you are looking straight down on (that is, normal to) the plane to perform your sketch. Note: Remember to refer back to this page if you have trouble creating a new part with a new sketch. Saving and closing the part Select the pull-down menu File. This will give you the option to use Save As. Select the Save As option from the pull-down menu. This will open up the Save As window. You will need to specify your directory in the Save in box and key in the file name in the File name box. Select Save. This will save the document as a CATPart with the name you specified in the directory you specified. You will now want to close the window because you are finished with this exercise: Select the pull-down menu File. This will give you the option to Close. Select Close option from the pull-down menu. This closes the window and you are now ready to proceed to the next exercise.




CATIA® V5R6

Rectangle This will cover the steps necessary to build a rectangle using the rectangle icon. This is useful any time you need a box shape. All you have to do is specify two opposite corners of the rectangle and Sketcher will generate it for you. Select the rectangle icon. Notice this icon has a down arrow on it. If you select the icon at the location of the arrow the various sub-option icons will appear. For now you just want the regular rectangle. Once you select the icon it should highlight. Select the origin point of the sketch plane. This will specify one of the corners of your rectangle. Select somewhere up and out to the right. This defines the other corner of the rectangle and the rectangle should appear similar to the one below.

Notice how the horizontal and vertical constraints automatically appeared on the rectangle. If you wish, you can save your document: call it rectangle with your initials.




CATIA® V5R6

Oriented Rectangle This will cover the steps necessary to build an oriented rectangle using the oriented rectangle icon. This is useful any time you need a box type shape that is oriented at an angle instead of being horizontal and vertical. You have to specify a location for the rectangle to begin at and then specify the other end of the line representing a side of the rectangle. After doing that then you have to specify a location for the height of the rectangle and then the rectangle will be generated for you. Press and hold the left mouse button while on the down arrow of the rectangle icon. This allows you to access the sub-option icons. You will want the oriented rectangle icon. Release the button on top of the oriented rectangle icon. The icon should change to the oriented rectangle icon and highlight. Notice how the rectangle icon no longer appears; it has moved to the sub-options now. Remember you can always access the suboptions by holding down the left mouse button on the down arrow of the respective icon. Select the origin point of the sketch plane. This will specify one of the corners of your rectangle. The next location that you select will define the orientation of the rectangle. Select somewhere up and to the right. This defines the other end of a side of the oriented rectangle. The next location that you define will determine the height of the oriented rectangle. Select somewhere up and to the left of the last location. This defines the height of the oriented rectangle and it should appear similar to the one shown below.

Notice how the parallel constraints automatically appeared on the oriented rectangle. If you wish, you can save your document; call it oriented rectangle with your initials.




CATIA® V5R6

Parallelogram This will cover the steps necessary to build a parallelogram using the parallelogram icon. This is useful any time you need a shape where the sides are parallel to one another but they can be at any angle. This is similar to the oriented rectangle except the angle between sides does not have to be 90 degrees. You have to specify a corner point for the parallelogram, then a point for the other end of a line representing a side of the parallelogram. Finally, you have to specify the endpoint for one other side of the parallelogram. CATIA will generate a parallelogram using the given points. Press and hold the left mouse button while on the down arrow of the rectangle icon. (Note: The rectangle icon may not currently be showing; if not, select the down arrow on the icon that is showing in the rectangle spot. If you just completed the last exercise then the icon will be the oriented rectangle icon.) This allows you to access the sub-option icons. You will want the parallelogram icon. Release the button on top of the parallelogram icon. The icon should change to the parallelogram icon and highlight. Notice how the previous icon no longer appears; it has moved to the sub-options now. Remember you can always access the sub-options by hold down the left mouse button on the down arrow of the respective icon. Select the origin point of the sketch plane. This will specify one of the corners of your parallelogram. The next location that you select will define the endpoint of one of the sides of the parallelogram. Select somewhere up and to the right. This defines the other end of a side of the parallelogram. The next location that you define will determine the endpoint of the other side. Select somewhere up and to the right of the last location. This defines the endpoint of the other side of the parallelogram and it should appear similar to the one shown below.

Notice how the parallel constraints automatically appeared on the parallelogram. If you want, save your document and call it parallelogram with your initials.




CATIA® V5R6

Elongated Slot This will cover the steps necessary to build an elongated slot using the elongated slot icon. This is useful any time you need to define a slot that is linear and curved with a full radius on both ends. You have to specify a location for the center of one of the curved ends and then define a location for the center of the other curved end. After doing that then you have to specify a location defining the radius of the ends and then the elongated slot will be generated for you. Press and hold the left mouse button while on the down arrow of the rectangle icon. (Note: The rectangle icon may not currently be showing, just select the down arrow on the icon that is showing in the rectangle spot. If you just completed the last exercise then the icon will be the parallelogram icon.) This allows you to access the sub-option icons. You will want the elongated slot icon. Release the button on top of the elongated slot icon. The icon should change to the elongated slot icon and highlight. Notice how the previous icon no longer appears; it has moved to the sub-options now. Remember you can always access the sub-options by hold down the left mouse button on the down arrow of the respective icon. Select the origin point of the sketch plane. This will specify the center of one of the curved ends of your slot. The next location that you select will define the center of the other curved end of your slot. Select somewhere up and to the right. This defines the center of the other curved end of the slot. The next location that you define will determine the radius of the ends. Select somewhere up and to the right of the last location. This defines the radius of the ends of the slot and it should appear similar to the one shown below.

Notice how the parallel and tangency constraints automatically appeared on the elongated slot. If you desire you can save your work; call it elongated slot with your initials.




CATIA® V5R6

Elongated Curved Slot This will cover the steps necessary to build an elongated curved slot using the elongated curved slot icon. This is useful any time you need to define a slot that is circular and curved with a full radius on both ends. The first step is to specify a location for the center of the circular path that the slot is going to follow. Then you specify a location to define the radius of the circular path which also is the definition of the center of one of the curved ends. The next step is to specify the center of the other curved end along that radius. The last step is to specify a location that defines the width of the slot. After all that the elongated curved slot will be generated for you. Press and hold the left mouse button while on the down arrow of the rectangle icon of the current workbench. (Note: The rectangle icon may not currently be showing; just select the down arrow on the icon that is showing in the rectangle spot. If you just completed the last exercise then the icon will be the elongated slot icon.) This allows you to access the sub-option icons. You will want the elongated curved slot icon. Release the button on top of the elongated curved slot icon. The icon should change to the elongated curved slot icon and highlight. Notice how the previous icon no longer appears; it has moved to the sub-options now. Remember you can always access the sub-options by hold down the left mouse button on the down arrow of the respective icon. Select the origin point of the sketch plane. This will specify the center of the circular path. The next location that you select will define the radius of the circular path and the center of one of the curved ends.




CATIA® V5R6

Select out to the right. This defines the radius of the circular path that the slot is going to follow and the center of one of the curved ends of the slot. The next location that you define will be the center of the other curved end. Select somewhere down and out to the left of the last location. This defines the center of the other curved end of the slot. The next location will determine the width of the slot. Select somewhere above the last location. This determines the width of the slot and it should look similar to the one shown below.

Notice how the concentric and tangency constraints automatically appeared on the elongated curved slot. If you desire you can save the document and call it elongated curved slot with your initials.




CATIA® V5R6

Keyhole This will cover the steps necessary to build a keyhole shape using the keyhole icon. This is useful any time you need to define a keyhole. To get the keyhole, you need to define four locations, in order: the center of the large radius, the center of the small radius, the radius value of the small radius, and the radius value of the large radius. After all that the keyhole will be generated. Press and hold the left mouse button while on the down arrow of the rectangle icon. (Note: The rectangle icon may not currently be showing, just select the down arrow on the icon that is showing in the rectangle spot. If you just completed the last exercise then the icon will be the elongated curved slot icon.) This allows you to access the sub-option icons. You will want the keyhole icon. Release the button on top of the keyhole icon. The icon should change to the keyhole icon and highlight. Notice how the previous icon no longer appears; it has moved to the sub-options now. Remember you can always access the sub-options by hold down the left mouse button on the down arrow of the respective icon. Select the origin point of the sketch plane. This will specify the center of the larger radius of the keyhole. The next location that you select will define the center of the smaller radius of the keyhole. Select down below. This defines the center of the smaller radius of the keyhole. The next location that you specify will determine the smaller radius of the keyhole. Select to the right of the last location. This defines the radius of the smaller end of the keyhole. The next location will determine where the larger radius is to begin. Select somewhere above the last location. This determines the size of the larger radius, and it should look similar to the one shown below.

Notice how the parallel and tangency constraints automatically appeared on the keyhole. Save this document, if you wish, with the name keyhole, with your initials.




CATIA® V5R6

Hexagon This will cover the steps necessary to build a hexagon using the hexagon icon. This is useful any time you need to define a hexagon. All you have to specify is the center of the hexagon and the distance to a side. The hexagon will then be generated. Press and hold the left mouse button while on the down arrow of the rectangle icon. (Note: The rectangle icon may not currently be showing, just select the down arrow on the icon that is showing in the rectangle spot. If you just completed the last exercise, the icon will be the keyhole icon.) This allows you to access the sub-option icons. You will want the hexagon icon. Release the button on top of the hexagon icon. The icon should change to the hexagon icon and highlight. Notice how the previous icon no longer appears; it has moved to the sub-options now. Remember you can always access the sub-options by hold down the left mouse button on the down arrow of the respective icon. Select the origin point of the sketch plane. This will specify the center of the hexagon. The next location that you select will define the distance to a side of the hexagon. Select to the right. This defines the distance to a side and the hexagon should appear similar to the one shown below.

Notice how the parallel and coincidence constraints automatically appeared on the hexagon. Save your document, if you wish, giving it the name hexagon, with your initials.




CATIA® V5R6

Circle This will cover the steps necessary to build a circle using the circle icon. This icon is similar to the rectangle icon in the sense that it has many sub-options available. For the main option, all you need to do is specify two points, representing the center and radius of the circle, and the circle will be generated for you. Select the circle icon. Notice this icon has a down arrow on it similar to the rectangle icon. If you select the icon at the location of the arrow the various sub-option icons will appear. For now you just want the regular circle. Once you select the icon it should highlight. Select the origin point of the sketch plane. This will specify the center of the circle. The next location will define the radius of the circle. Select any location a short distance away from the center. This determines the radius of the circle. CATIA will generate a circle similar to the one shown below.

If you desire you can save your work: give it the name circle with your initials.




CATIA® V5R6

Circle through 3 points This will cover the steps necessary to build a circle passing through three points. You have to specify the three locations for the circle to pass through and then the circle will be generated for you. It is assumed that you know how to access the sub-options of a particular icon therefore the steps will just tell you to select the sub-option icon. If you have trouble, please refer back to the previous exercises. Select the three-point circle icon. icon. It should be highlighted.

This is located in the sub-options of the circle

Select the origin point of the sketch plane. This will specify one of the locations that the circle will pass through. The other two locations will finish the definition of the circle. Select up and to the right. This specifies the second location for the circle to pass through. Select to the left of the last location. This specifies the last location for the circle to pass through and the circle appears similar to the one shown below.

If you desire you can save this document, calling it 3ptcircle with your initials.




CATIA® V5R6

Circle with Cartesian coordinates This will cover the steps necessary to build a circle using coordinates. You have to specify the coordinates for the center of the circle and its radius and then the circle will be generated for you. Select the circle using coordinates icon. and the icon should be highlighted.

A Circle Definition window should appear

Notice that you can enter the coordinates using the Cartesian coordinate system or the polar coordinate system. You will want to use the Cartesian coordinate system for this exercise. Enter 2 for H, 2 for V and 1 for Radius. The circle appears similar to the one shown below.

Notice that the dimension constraints were automatically generated when you created the circle. If you desire you can save your document and call it circle coord with your initials.




CATIA® V5R6

Circle tangent to 3 elements This will cover the steps necessary to build a circle tangent to three elements. You have to specify the three elements that you want the circle to be tangent to and then the circle will be generated. Start a new part and go into the Sketcher with the yz plane. Select the circle using coordinates icon. You will use this icon to create three circles in order to see how the tri-tangent circle icon works. Create 3 circles using the following coordinates. H=0, V=3, Radius=1.5; H=4.5, V=3, Radius=2; H=1.5, V=-1, Radius=1. Three circles should appear as shown below. Next you will create a circle tangent to all three of these.

Select the tri-tangent circle icon.

It should be highlighted.

Select the three circles to be tangent to. This will specify the three elements that you want the circle to be tangent to and the circle appears similar to the one shown below. You can create a circle tangent to any three elements using this icon.

If you desire you can save your document and call it tritangent with your initials.




CATIA® V5R6

Arc through 3 points This will cover the steps necessary to build an arc passing through three points. You simply need to specify any three points and an arc will be generated which starts at the first point, ends at the third point and passes through the second point. Select the three point arc icon.

It should highlight.

Select the origin point of the sketch plane. This will specify one of the locations that the arc will pass through. The other two locations will finish the definition of the arc. Select up and to the left. This specifies the second location for the arc to pass through. Select up and to the right of the last location. This specifies the last location for the arc to pass through and the arc appears similar to the one shown below.

If you desire you can save your document and call it 3ptarc with your initials.




CATIA® V5R6

Arc through 3 points using limits This will cover the steps necessary to build an arc passing through three points. The difference between this method and the last one is the order used to specify the three points. In this icon, the first two points you select are the endpoints, and the third is an additional point the arc will pass through. Select the three point arc using limits icon.


Select the origin point of the sketch plane. This will specify one of the endpoints of the arc. The other two locations will finish the definition of the arc. Select up and to the right. This specifies the other endpoint of the arc. Select to the left of the last location. This specifies the location for the arc to pass through and the arc appears similar to the one shown below.

If you desire you can save your document and call it 3ptarclimits with your initials.




CATIA® V5R6

Arc This will cover the steps necessary to build an arc by specifying the center point and then the starting point and ending point of the arc. The first location that you define will be the center point of the arc. The second location determines the radius of the arc and the starting point of the arc. The third location defines the other endpoint of the arc. Select the arc icon.


Select the origin point of the sketch plane. This will specify the center of your arc. The other two locations will finish the definition of the arc. Select up and to the left. This specifies the starting point of the arc and the radius of the arc. Select to the right of the last location. This specifies the other endpoint of the arc and the arc appears similar to the one shown below.

If you desire you can save your document; call it arc with your initials.




CATIA® V5R6

Spline This will cover the steps necessary to build a spline. This icon is useful to create arbitrary smooth curves through a series of points. You need to specify a number of locations for the spline to pass through and it will create a smooth curve passing through them. The last point on the spline needs to be defined by double-clicking. Select the spline icon.


Select the origin point of the sketch plane. This will specify one endpoint for the spline. The other locations will define the shape of the spline. Select up and to the right. This specifies the second location for the spline to pass through. Select down and to the right of the previous location. This specifies the third location for the spline to pass through. Select up and to the right of the previous location. This specifies the fourth location for the spline to pass through. Double-click down and to the right of the previous location. By double-clicking this location you are telling the computer that this location is the other endpoint of the spline. The finished spline should appear similar to the one shown below.

Save your document, if you wish, under the name spline with your initials.




CATIA® V5R6

Connect Curve This will cover the steps necessary to build a connect curve. This icon is useful to create arbitrary smooth curves connecting two elements. You need to specify the two endpoints of the connecting curve along the existing elements that you wish to connect. This option has two sub-options which will appear to the right of your sketcher icons in the bottom toolbar or wherever you located them. This will connect the two elements with an arc This will connect the two elements with a spline In this exercise you will use the connect with spline option, but feel free to use both options. Select the spline icon.


Create two splines that look similar to the diagram shown below. You will have to refer to the previous exercise if you need help creating the splines.

Select the connect curve icon.





CATIA® V5R6

Select the connect with spline icon. This icon is located next to your sketcher icons in the bottom toolbar or wherever you located them. Select on the spline near the location shown below. Where you select the element determines one of the endpoints of the connect curve. Select on the other spline near the location shown below. This defines the other endpoint and generates the connect curve. It should appear similar to the diagram shown below.

If you desire you can save your document. Call it connect curve with your initials.




CATIA® V5R6

Ellipse This will cover the steps necessary to build an ellipse. This icon is useful to create elliptical shapes. This is a conic shape that has certain mathematical properties useful for some designs. The first location you define is the center of the ellipse; the second one gives both the orientation and one of the two diameters. Finally you define the other diameter by selecting another location. Select the ellipse icon.


Select the origin point of the sketch plane. This will specify the center of the ellipse. The next location determines the orientation and length of the ellipse. Select down and to the left. This determines the orientation and the length of the ellipse. The next location will define a location that the ellipse will pass through thereby defining the width of the ellipse. Select up and to the right of the previous location. This specifies a location that the ellipse will pass through determining the shape of the ellipse. It should appear similar to the one shown below.

If you desire you can save your document: call it ellipse with your initials.




CATIA® V5R6

Parabola This will cover the steps necessary to build a parabola. This icon is useful to create parabolic shapes. This is another conic curve that has certain mathematical properties useful for some designs. You have to define a location for the focus of the parabola and then the apex, or tip. Finally you must define the two endpoints for the parabola. Select the parabola icon.


Select the origin point of the sketch plane. This will specify the focus of the parabola. The next location determines the apex or tip of the parabola. Select below the origin. This determines the apex. A parabola’s shape is determined by the distance between the focus and the apex. The next two locations define the starting and ending points of the parabola. Select up and to the left of the previous location. This specifies the starting location for the parabola. Select up and to the right of the previous location. This specifies the ending location for the parabola and it should appear similar to the one shown below.

If you desire you can save your document. Call it parabola with your initials.




CATIA® V5R6

Hyperbola This will cover the steps necessary to build a hyperbola. A hyperbola is another conic curve that has certain mathematical properties useful for some designs. You have to define a location for the focus of the hyperbola and then the center of the hyperbola. After defining those locations then you must specify a location for the apex or tip of the hyperbola. Then you can define a starting point and ending point for the hyperbola. Select the hyperbola icon.


Select the origin point of the sketch plane. This will specify the focus of the hyperbola. The next location determines the center of the hyperbola. Select a location well above the origin. This determines the center of the hyperbola. The next location defines the apex, or tip. Select somewhere between the origin and the previous location. This determines the apex, or tip, of the hyperbola. The three locations you have specified so far—focus, center, and apex—determine the shape of the hyperbola. Next you will specify its endpoints. Select to the left of the origin point. This specifies one endpoint of the hyperbola. Select to the right of the origin point. This specifies the other endpoint. The finished hyperbola should appear similar to the one shown below.

If you desire you can save your document. Call it hyperbola with your initials.




CATIA® V5R6

Conic This will cover the steps necessary to create a conic. There are many sub-options available under this icon. Depending on which options you select will determine what you can define when creating the conic. You can define five points, tangency at the first end, tangency at the second end or tangency at both ends. This exercise will only cover creating a conic with tangency at both ends but feel free to use the other options until you are comfortable with them. Define tangency at the first end Define tangency at the second end Define tangency at both ends

Select the conic icon.


Select the tangency at both ends icon. This will allow you specify a location that will define the tangency at both ends of the conic. Select the origin point. This defines the first end point of the conic. Select a location to the right of the origin. This defines the second end point of the conic. Select a location above and between the two points. This defines the tangency at both ends, from the endpoint to this point. Select below the last location. This defines the actual shape of the conic based on the previously defined tangencies. The conic should appear.

If you desire you can save your document. Call it conic with your initials.




CATIA® V5R6

Line This will cover the steps necessary to build a line. Use this icon for straight edges of your profiles. To create a line, you only need to specify the two endpoints. Select the line icon.


Select the origin point of the sketch plane. This will specify one endpoint of the line. The next location specifies the other endpoint. Select up and to the right of the origin. This determines the other endpoint. The line should appear similar to the one shown below.

If you desire you can save your document. Call it line with your initials.




CATIA® V5R6

Unlimited Line This will cover the steps necessary to build an unlimited line. Use this icon for straight edges of your profiles that you do not want a specific length but instead you want it to go out essentially forever. This icon has three sub-options that will allow you to create a horizontal, vertical or point to point unlimited line. Depending on which sub-option you choose determines what is necessary to create the line. In this exercise you will just use the point to point sub-option but feel free to use the other options to get familiar with them. Select the unlimited line icon.


Select the origin point of the sketch plane. This will specify a point along the line. The next location specifies another point along the line. Select up and to the right of the origin. This defines another point along the line. The line should pass through those two locations and go out essentially forever. It should appear similar to the diagram shown below.

If you desire you can save your document. Call it unlimited line with your initials.




CATIA® V5R6

Bi-tangent Line This will cover the steps necessary to build a bi-tangent line. A bi-tangent line is tangent to two other elements such as circles. All you have to do is specify the two elements that you wish the line to be tangent to. Select the circle using coordinates icon.

You will create two circles using this icon.

Create 2 circles using the following coordinates. H=0, V=3, Radius=1; H=2, V=0, Radius=.5 Two circles should appear as shown below.

Select the bi-tangent line icon.


Select the right side of the larger circle. This will specify the line to be tangent to that side of the circle. The next location specifies the other element that the line is to be tangent to.




CATIA® V5R6

Select left side of the smaller circle. This makes the line tangent to that side of the circle as well. The line should appear similar to the one shown below.

If you desire you can save your document with the name bitangent with your initials.




CATIA® V5R6

Bisect Line This will cover the steps necessary to build a bisect line. A bisect line splits the angle between two other lines. All you have to do is specify the two lines that you wish to bisect and the bisecting line will be created. Select the line icon.


Create two lines similar to the ones shown below. Start each line at the origin.

Select the bisect line icon.


Select one of the lines. This defines one side of the sector that will be bisected. Select the other line. A bisecting line should appear similar to the one shown below.

If you desire you can save your document with the name bisect with your initials.




CATIA® V5R6

Axis This will cover the steps necessary to build an axis. An axis can be used for mirroring or for creating a shaft or groove in Part Design. To create an axis, all you have to do is specify two endpoints. Select the axis icon.


Select the origin point of the sketch plane. This will specify one endpoint of the axis. Next you will specify the other endpoint. Select above the origin. This determines the other endpoint of the axis and it should appear similar to the one shown below.

If you desire you can save your document. Call it axis with your initials.




CATIA® V5R6

Point This will cover the steps necessary to build a point. Points are useful for constraining your profile. All you have to do is specify a location for the point. Select the point icon.


Select up and to the right of the origin. This will specify a location for the point. You also have the option of selecting an element to put the point on the element at the specified location. That option will automatically add a coincidence constraint. The point should appear similar to the one shown below.

If you desire you can save your document and call it point with your initials.




CATIA® V5R6

Point using coordinates This will cover the steps necessary to build a point using coordinates. This icon is useful for generating points at specific locations. Normally this is used to position an item within your profile. All you have to do is enter the coordinates in the window that opens. Select the point using coordinates icon. and the icon should be highlighted.

A Point Definition window should appear

Notice that you can enter the coordinates using the cartesian coordinate system or the polar coordinate system. You will want to use the cartesian coordinate system for this exercise. Enter 2 for H and 2 for V. This will generate a point at that coordinate and it should appear similar to the one shown below.

Notice the dimension constraints were automatically generated when you created the point. If you desire you can save your document and call it coord point with your initials.




CATIA® V5R6

Equidistant points This will cover the steps necessary to build equidistant points. This icon is useful for generating points equidistant along an element. You have to specify an element and then specify the origin or the starting location for your spacing. Then you have to specify the spacing and the number of points to be spaced. Select the three point arc icon.


Select the origin point of the sketch plane. This specifies an endpoint of the arc. The other two locations will determine the shape of the arc. Select up and to the right of the origin. This defines the second location for the arc. Select down and to the right of the previous location. This defines the third location for the arc to pass through and the arc should appear similar to the one shown below.

Select the equidistant points icon. It should highlight. You will now have to specify the element you want to create equidistant points on. Select the arc. This is the element that you are going to create equidistant points along. The next location will determine the starting point for the spacing of the points. Select the right end of the arc. This determines the starting point for the creation of the equidistant points. An Equidistant Point Definition window should appear.

There are three different Parameters options. Points & Length, Points & Spacing, and Spacing & Length. In this exercise you will choose the Points & Spacing parameter.




CATIA® V5R6

Enter 1 for Spacing and 3 for New Points. This specifies the distance between the points and how many points that you want generated. Select OK. The points should appear similar to the ones shown below.

Notice that constraints were automatically generated for you. If you desire you can save your document and call it equidist point with your initials.




CATIA® V5R6

Intersection Point This will cover the steps necessary to create a point at the intersection of two elements. All you have to do to create an intersection point is select the two elements. Select the line icon.


Create two lines as shown below.

Select the intersection point icon.


Select one of the lines. It will use this line as one of the intersecting elements. Select the other line. The two lines do not have to actually intersect as long as they would intersect if they were to continue in length. The intersection point should appear with constraints as shown below.

If you desire you can save your document and call it intersection point with your initials.




CATIA® V5R6

Projection Point This will cover the steps necessary to create a point by projecting a point to an element. All you have to do to create a projection point is select a point that you want to project and then select the element that you want to project the point to. Select the line icon.


Create a line as shown below.

Select the point icon.


Create a point as shown below.

Select the projection point icon.


Select the point. You will use this point to project to the line.




CATIA® V5R6

Select the line. A projected point is created and should appear with constraints as shown below.

If you desire you can save your document and call it projection point with your initials.




CATIA® V5R6

Profiles This part will discuss the profile icon which the most commonly used icon when defining sketches. The purpose of these exercises are to demonstrate the usefulness of the profile icon and how to use it effectively. You can use it to generate basic shapes or more involved shapes all in one operation. The most common use is to specify corner points of your desired profile and it will generate lines between those points until you either click on the profile icon again, double-click a location or select a location that closes the profile. You also can use two other icons that are located in the bottom toolbar to generate curves as you are defining the profile. Also while using the line icon of profile you can generate curves by holding down the left mouse button and dragging it in the direction you want the curve to go and it will know to create a circular curve from that location. As you are defining the profile occasionally the element will appear in blue before defining the endpoint or a constraint may appear in blue. If you select the endpoint while the element or the constraint is blue then it will automatically put those constraints on the geometry when it is created. This is useful when defining horizontal and vertical lines because if they appear in blue while you are defining them then the horizontal and vertical constraint will automatically be generated on the element. You will now build various profiles to get experience using the various capabilities of the profile icon. The first profile you are going to build looks like the one shown below.

Start a new part and go into the Sketcher with the yz plane. Select the profile icon.


Select the origin point of the sketch plane. This specifies the starting point for your profile. When you specify the next location make sure the line appears blue before selecting the location. This will put the vertical constraint on your element automatically.

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Select a location above the origin. If the line appeared blue before you selected the second location then it should appear with the vertical constraint on it like the one shown below. Make sure when you specify the other locations that those elements appear blue as well before selecting the location.

Select a location to the right of the previous location. It should appear with the horizontal constraint on the element and look similar to the diagram shown below.

Select a location below the previous location along the H axis. It should appear similar to the diagram shown below.


Profiles, Page 67


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Select a location to the left of the previous location. It should appear similar to the diagram shown below.

Select a location above the previous location. It should appear similar to the diagram shown below.

Select a location to the left of the previous location. It should appear similar to the diagram shown below.

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Select a location below the previous location. It should appear similar to the diagram shown below.

Select the origin point of the sketch again. The profile should appear similar to the diagram shown below and exit the profile icon.

If you desire you can save your document and call it profile1 with your initials. Save the document and close it.


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You will now perform a sketch of a part using the three point arc icon in the bottom toolbar during the sketch. This icon allows you to define a three point arc while using the profile icon. The second profile you are going to build looks like the one shown below.



Select the origin point of the sketch plane. This specifies the starting point for your profile. When you specify the next location make sure the line appears blue before selecting the location. This will put the vertical constraint on your element automatically. Select a location above the origin. If the line appeared blue before you selected the second location then it should appear with the vertical constraint on it like the one shown below. Make sure when you specify the other locations for the lines that they appear blue as well before selecting the location.

Select a location to the right of the previous location. It should appear similar to the diagram shown below.

Profiles, Page 70



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Select the three point arc icon in the bottom toolbar. This icon will allow you to specify a location for the arc to pass through and an ending location for the arc. The arc will begin at the last location specified which is the endpoint of the line. Select up and to the right of the previous location. This specifies the location that the arc should pass through. The next point specifies the endpoint of the arc. Select down and to the right of the previous location. This location should be straight across from the start of the arc. It should appear similar to the diagram shown below. Notice how the three point arc icon in the bottom toolbar automatically turned off and the line icon turned on.

Select to the right of the previous location. It should appear similar to the diagram shown below.

Select below the previous location. It should appear similar to the diagram shown below.


Profiles, Page 71


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Select to the left of the previous location. It should appear similar to the diagram shown below.

Select above the previous location. It should appear similar to the diagram shown below.


Select the three point arc icon in the bottom toolbar. This icon will allow you to specify a location for the arc to pass through and an ending location for the arc. The arc will begin at the last location specified which is the endpoint of the line. Select up and to the left of the previous location. This specifies the location that the arc should pass through. The next point specifies the endpoint of the arc.

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Select down and to the left of the previous location. This location should be straight across from the start of the arc. It should appear similar to the diagram shown below. Notice how the three point arc icon in the bottom toolbar automatically turned off and the line icon turned on.


Select below the previous location. It should appear similar to the diagram shown below.


Profiles, Page 73


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Select the origin point of the sketch again. The profile should appear similar to the diagram shown below and exit the profile icon.


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You will now perform a sketch of a part using the tangent arc icon in the bottom toolbar during the sketch. This icon allows you to define an arc tangent to the last line while using the profile icon. The third profile you are going to build looks like the one shown below.



Select the origin point of the sketch plane. This specifies the starting point for your profile. Select to the right of the origin. If the line appeared blue before you selected the second location then it should appear with the horizontal constraint. It should appear similar to the diagram shown below.

Select the tangent arc icon in the bottom toolbar. This icon will allow you to specify an endpoint for an arc starting at the last location. It will automatically put a tangency constraint on your profile at the initial point.


Profiles, Page 75


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Select up and to the right of the previous location. This specifies the endpoint of the arc. It should appear similar to the diagram shown below.

Select up and to the right of the previous location. It should look similar to the diagram shown below.

Select the tangent arc icon in the bottom toolbar. This icon will allow you to specify an endpoint for an arc starting at the last location. It will automatically put a tangency constraint on your profile at the initial point. Select up and to the left of the previous location. This specifies the endpoint of the arc. It should appear similar to the diagram shown below.

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Select the tangent arc icon in the bottom toolbar. This icon will allow you to specify an endpoint for an arc starting at the last location. It will automatically put a tangency constraint on your profile at the initial point. Select down and to the left of the previous location. This specifies the endpoint of the arc. It should appear similar to the diagram shown below.


Profiles, Page 77


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Select down and to the right of the previous location. It should look similar to the diagram shown below.

Select the tangent arc icon in the bottom toolbar. This icon will allow you to specify an endpoint for an arc starting at the last location. It will automatically put a tangency constraint on your profile at the initial point. Select the origin point of the sketch plane. This specifies the endpoint of the arc. It should appear similar to the diagram shown below.


Profiles, Page 78



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You can also create tangent arcs using the mouse instead of using the tangent arc icon in the bottom toolbar. In order to create an arc instead of a line you need to press and hold the left mouse button down and drag the mouse in the general shape of the arc. Then you can select the endpoint of the arc. The following steps will walk you through the steps necessary to perform this operation, however you may need to see it done in order to really understand how it works. You will generate the same profile you created in the previous exercise except you will use the mouse to generate the arcs instead of the tangent arc icon. The final sketch should look similar to the one shown below.



Select the origin point of the sketch plane. This specifies the starting point for your profile. Press and hold the left mouse button at a location to the right of the origin. This specifies the endpoint of the line. You need to continue holding the left mouse button down in order to specify the tangent arc which will begin at this location. While holding down the left mouse button drag your mouse in the direction that you want the arc to follow. Select a location up and to the right of the previous location. This will specify the endpoint of the arc. It should appear similar to the diagram shown below.


Profiles, Page 79


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You can continue this process to complete the sketch. You will probably need to practice this sketch a few times using this option in order to become proficient. It is a much quicker method of creating tangent arcs then using the icon in the bottom toolbar. Finish sketching the part using the drag option for the tangent arcs. It should appear similar to the one shown below.

There is no need to save this sketch since it is similar to the previous one.

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Now that you have tried the various options with the profile icon you are ready to sketch some practice sketches. Try sketching the following sketches and save them as profile4, profile5 and profile6 respectively. Sketch the profile shown below and save as profile4 with your initials.


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Sketch the profile shown below and save as profile5 with your initials.

Sketch the profile shown below and save as profile6 with your initials.

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Constraints Constraints are similar to dimensions and they allow you to force your sketch to be an exact shape. Sketches without constraints generally are not accurate enough for your design and therefore it is necessary to put constraints on your sketch to make it an exact size. There are many types of constraints and most are listed below. Dimensional Constraints Distance

distance between two elements

Length

length of an element

Angle

angle between two elements

Radius/Diameter

radius or diameter of a circle or arc

Semimajor axis

semimajor axis of an ellipse

Semiminor axis

semiminor axis of an ellipse

Geometrical Constraints Symmetry

symmetric about an axis or line

Midpoint

forces an element to be located at the midpoint of another element

Equidistant point

forces three points to be equidistant from each other

Fix

positions an element so it will not move

Coincidence

aligns one element with another

Concentricity

makes a circle or arc positioned concentric to another circle or arc

Tangency

makes an element tangent to another element

Parallelism

forces a line to be parallel to another line

Perpendicularity

forces a line to be perpendicular to another line

Horizontality

makes a line be positioned horizontally

Verticality

makes a line be positioned vertically


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When defining constraints on your sketch the color of the elements of the sketch will change color depending on the status of the element. The table below shows the default colors and the corresponding status. Color

Status

White

Not constrained

Green

Perfectly constrained

Purple

Over constrained

Black

Unresolved constraint

Red

Invalid geometry

There are a few icons that allow you to generate constraints. Those icons are shown below. Constraint by dialog icon allows you to define constraints by selecting them from a window. Most commonly used constraint icon to define basic constraints on elements and between elements. Allows the computer to automatically put constraints on your sketch. Sometimes this is useful to get a start on the constraints. Allows for the animation of constraints. This is useful to see how the sketch would change based on a constraint varying in size. Normally, the goal is to perfectly constrain your sketch so that it is completely defined according to your specifications. Therefore you normally want your sketch to appear green when leaving the Sketcher to go to Part Design. The first thing you need to remember is that sometimes when you built your sketch constraints were automatically generated. This was caused by two icons located in the bottom toolbar. One is for geometrical constraints and the other is for dimensional constraints. Geometrical constraints Dimensional constraints By default these two icons are selected. You should have seen some of the geometrical and dimensional constraints generated in your previous exercises. In the following exercises you will sketch the shape shown and then the steps will walk you through constraining the sketch.




CATIA® V5R6

Sketch the profile shown below and save as constraint1 with your initials. You should make sure that the coincidence constraint appears in blue when defining the origin point of your sketch. That constraint will not appear after creating the sketch it is implied.

Notice some constraints were automatically generated. You will now put additional constraints on your profile to make it perfectly constrained. Select the constraint icon.


This will allow you to define a constraint.



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Select the bottom horizontal line and locate the constraint below the line. A length constraint should appear underneath the horizontal line. The value that appears for you may not be the same as shown below.

You can use the constraint icon for almost all of the dimensional constraints. You will now use it to generate a constraint between two elements. Select the constraint icon.


Select the horizontal line above the bottom one. This defines the first element. You will now define the second element to create a distance constraint between the two elements.




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Select the horizontal line above the previous one and position the constraint to the right. It should appear similar to the diagram shown below except the value may be different.

You can also use the constraint icon to put some geometric constraints on elements. You will now use the constraint icon to make the angled line have the horizontal constraint. Select the constraint icon.


Select the angled line. A constraint will appear but instead of positioning the constraint at a location you will now press the right mouse button on the constraint.




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Press the right mouse button while on the constraint. Various options appear in a window as shown below.

Select the Horizontal option. This puts the horizontal constraint on the element. It should appear similar to the diagram shown below.

You will learn more about the other options that appear in the window later. Since it is not always convenient to have to press the constraint icon each time you want to generate a constraint, there is a way to make it active for multiple constraints. To do this you have to double click on the icon using the left mouse button. This will keep the icon activated until it is turned off. You will do that and then finish constraining your sketch.



CATIA Part Design & Sketcher Double click on the constraint icon with the left mouse button. icon for multiple uses.

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This activates the

Select the bottom right vertical line and position the constraint to the right. It should appear similar to the diagram shown below but it may have a different value.




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Select bottom horizontal line and then the horizontal line above the 1.5 line and position it to the right. It should appear similar to the diagram shown below but it may have a different value.




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Select the bottom horizontal line and then the top horizontal line and position it to the right. It should appear similar to the diagram shown below but it may have a different value.




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Put the horizontal and vertical constraints on all of the elements that do not already have them by selecting the element and then right clicking the constraint and choosing Horizontal or Vertical. It should appear similar to the diagram shown below.

You will now put a coincidence constraint on two elements while the constraint icon is still active. Select the vertical line between the base and the shelf. This selects the first element, but instead of positioning a constraint you will now select a second element. Select the vertical line between the shelf and the top of the sketch. This selects the second element. Now, you will right click on the constraint and choose the Coincidence option.




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Press the right mouse button while on the constraint. Various options appear in a window as shown below.

Select the Coincidence option. This makes the two elements coincident with one another, meaning that they line up with one another. Your sketch should now appear similar to the one shown below but it may have different values.

Notice the part is almost perfectly constrained (green color). You will now finish constraining the sketch while the constraint icon is still active. © Wichita State University



CATIA® V5R6

Select the left most vertical line and then the next top vertical line and position the constraint above the sketch. This constrains the location of both of the coincident lines due to the coincidence constraint. All that is left is the vertical line of the shelf. It should appear similar to the diagram shown below but it may have different values.




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Select the left most vertical line and the vertical line at the end of the shelf and position the constraint above the sketch. This will put the final constraint on your sketch and it should appear all in green. It should also look similar to the diagram shown below but may have different values.

You will now modify the values of your constraints to force your sketch to be a specific size. You can change the values of the constraints any time after they are created, you do not have to perfectly constrain your part ahead of time. The first thing you have to do is to deactivate the constraint icon.




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Select the constraint icon to turn it off. The icon should no longer appear highlighted. As you experienced, it is much faster to constrain a sketch by forcing the constraint icon to stay active by double clicking on it instead of having to select it each time. To change the values of the constraints all you have to do is double click on the value and then key in a new value. You can move the position of the constraint as well by selecting the constraint and holding down the left mouse button you can drag the constraint to a new position. If you want to relocate just the value then you can hold down the left mouse button on the value, however, if you want to relocate the value along with the constraint arrows then you must hold down the left mouse button on the arrow lines. Double click on the constraint representing the total height of the sketch. A window appears as shown below but it may have a different initial value.

Change the value to 7.00 and press OK. Notice that the sketch automatically changed so that the height is now seven inches. You will continue to change values until all of the constraints are set to their proper values.




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Change all of the constraints to the values shown below. The sketch should look just like the one shown below.

Save your document.




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Normally you do not have to put all of the horizontal and vertical constraints on your sketch to make it perfectly constrained. When you put a distance constraint between one element and another it is assumed that the two elements are parallel to each other. Remember those constraint option windows that appeared when right clicking the constraint.

These allow you to specify various constraints using the constraint icon that you normally could not define. Most of the options are the same as the options that were described before. However there are a few new options that you need to be aware of in order to effectively use this icon. Reference

This creates a reference dimension that is shown only to let you know the value. You can not change the value of a reference dimension, it only reflects the actual value of the dimension. Therefore if you put constraints on your sketch that changes that dimension it will be reflected in the value.

Notice that a reference dimension has parentheses around the value.




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Horizontal Measure Direction

Puts the distance or length constraint to measure horizontally instead of the default orientation.

Vertical Measure Direction

Puts the distance or length constraint to measure vertically instead of the default orientation.

Default

Horizontal

Vertical



CATIA Part Design & Sketcher Swap Location

Before:

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This swaps the constraint to go to the other side of the element. Sometimes when you sketch you may get a line to the wrong side with respect to another and when you constrain it, you can not give it a negative value in order for it to switch sides. This is a good option to use in that circumstance, however, you can also just drag an element over using the left mouse button. After:

Allow symmetry line This allows you to define a symmetry line after selecting two elements that you want to be symmetric to each other. After selecting the two elements, use your third mouse button to activate the menu, select Allow symmetry line and then select the symmetry line.




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For the rest of the constraint exercises the initial sketch will be provided for you to make it easier for you to concentrate on the actual constraints. Open the constraint2 document and save with your initials. This will open the part called constraint2. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and then you can start adding constraints. A diagram of the sketch is shown below.

Notice that the bottom horizontal line is already constrained. You will now be constraining this sketch to look like the following diagram.



CATIA Part Design & Sketcher Double click on the constraint icon with the left mouse button. the constraint icon to be used more than once.

CATIA® V5R6

This will activate

Select the bottom horizontal line and position the constraint below the line. It should appear similar to the diagram shown below.

Select the bottom horizontal line and the bottom right angled line and position the constraint to the right. It should appear similar to the diagram shown below.




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Select the bottom horizontal line and the bottom left angled line and position the constraint to the left. It should appear similar to the diagram shown below.

Select the left curve and the bottom left angled line. This will make a constraint but you are going to press the right mouse button to choose the Tangency option. Press the right mouse button while on the constraint. A window should appear with constraint options.

Select the Tangency option. This will force the line and the curve to be tangent to one another.




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Select the left curve and position the constraint to the left. This puts a radius constraint on your curve. Select the right curve and position the constraint to the right. This puts a radius constraint on your curve. It should look similar to the diagram shown below.

Select the bottom left angled line and then the top left angled line. Press the right mouse button while on the constraint. A window should appear with constraint options.

Select the Allow symmetry line option. This will allow you to define a symmetry line. Select the dashed line. This will put a symmetry constraint on the two angled lines using the dashed line as a symmetry line. It is important to select the symmetry line last. Also, it should be noted that this symmetry line is a construction line not a standard line and therefore will not show up in Part Design. You will learn more about construction elements later in this course.




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Select the bottom horizontal line and then the top line. Press the right mouse button while on the constraint and select the Allow symmetry line option. This will allow you to define a symmetry line. Select the dashed line. This puts the symmetry constraint on the two lines using the dashed line as the symmetry line. Select the bottom right angled line and then the top right angled line. Press the right mouse button while on the constraint and select the Allow symmetry line option. This will allow you to define a symmetry line.




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Select the dashed line. This puts the symmetry constraint on the two lines using the dashed line as the symmetry line. It should appear similar to the diagram shown below.

Select the bottom horizontal line and the dashed line and position the constraint to the right. This puts a distance constraint between the two elements. It should look similar to the diagram shown below.




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The external profile should all be green now because it is perfectly constrained. However you still need to constrain the circles. Select the left circle and position the constraint up and to the left. This puts a diameter constraint on your circle. Select the right circle and position the constraint up and to the right. This puts a diameter constraint on your circle. It should appear similar to the diagram shown below.

You will now put a concentric constraint between the circles and the curves. Select the circle on the left and the curve on the left and then press the right mouse button while on the constraint. A window should appear showing you some constraint options.




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Select the Concentricity option. This forces the circle to be concentric with the curve. Meaning that they have the same center point location. It should appear similar to the diagram shown below.

You will now repeat the same procedure to put the concentric constraint on the other circle and curve. Select the circle on the right and the curve on the right and then press the right mouse button while on the constraint. The window should appear again. Select the Concentricity option. This forces the circle to be concentric with the curve. It should appear similar to the diagram shown below.




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Now the entire sketch is perfectly constrained. You will now change the values to match those shown below. Change the values of the constraints to match the diagram shown below. Remember you have to exit the constraint icon by selecting it. Then you just have to double click on a value and a window will appear. After you change the value press the Enter key or select OK.

Save your document.




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Open the constraint3 document and save with your initials. This will open the part called constraint3. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and then you can start adding constraints. A diagram of the sketch is shown below.

You will now be constraining this sketch to look like the following diagram.



CATIA Part Design & Sketcher Double click on the constraint icon with the left mouse button. the constraint icon to be used more than once.

CATIA® V5R6

This will activate

Select the bottom horizontal line and position the constraint below the line. It should appear similar to the diagram shown below.

Select the left vertical line and position the constraint to the left of the line. It should appear similar to the diagram shown below.




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Select the top horizontal line and position the constraint above the line. It should appear similar to the diagram shown below.

Select the left angled line and position the constraint below and to the left of the angled line. It should appear similar to the diagram shown below.

You are now going to exit the constraint icon and change the values of the constraints. You will then finish constraining the sketch using the constraint by dialog icon.




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Change the values of the constraints to match the diagram shown below. Remember you have to exit the constraint icon by selecting it. Then you just have to double click on a value and a window will appear. After you change the value press the Enter key or select OK.

You are going to the use the constraint by dialog icon to finish putting the constraints on your sketch. However, it is important to remember that you could just use the regular constraint icon to finish the constraints. In order to select two elements at the same time you must press and hold the Ctrl key when selecting the second element. Select the bottom horizontal line. It highlights letting you know that it has been selected. Press and hold the Ctrl key while selecting the horizontal line above the previous line. This allows you to select a second element while keeping the first element highlighted. Select the constraint by dialog icon.


This opens a Constraint Definition window.



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Using that window you can specify which constraint or constraints you would like to put using the elements that you currently have selected. Select the Distance option. A check should appear in the Distance box. Select OK. A distance constraint should appear between the two elements. Press and hold the left mouse button while on the constraint and drag it above the top line. It should appear similar to the diagram shown below.

It is important to note that double clicking the constraint by dialog icon will not keep the icon active for multiple uses since you must select the element or elements before selecting the icon. Select the left angled line. It highlights letting you know that it has been selected. Press and hold the Ctrl key while selecting the bottom end line. This allows you to select a second element while keeping the first element highlighted. Select the constraint by dialog icon.





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Select the Perpendicularity option and select OK. This generates the perpendicular constraint between those two elements. It should appear similar to the diagram shown below.

Select the left angled line. It highlights letting you know that it has been selected. Press and hold the Ctrl key while selecting the right angled line above the previous line. This allows you to select a second element while keeping the first element highlighted. Select the constraint by dialog icon.


Select the Parallelism option and select OK. This generates the parallel constraint between the two elements. It should appear similar to the diagram shown below.




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Select the end line. This is the line at the end of the two angled lines. Select the constraint by dialog icon.


Select the Length option and select OK. This will generate a length constraint. Press and hold the left mouse button on the new constraint’s arrow and drag it down and to the right. By selecting the arrow you can move the entire constraint down and to the right, however, if you press and hold the left mouse button on the value then it would only move the value. It should appear similar to the diagram shown below.

Select the right angled line. It highlights letting you know that it has been selected. Press and hold the Ctrl key while selecting the connecting horizontal line. This allows you to select a second element while keeping the first element highlighted. Select the constraint by dialog icon.


Select the Angle option and select OK. This generates an angle constraint between the two elements.




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Press and hold the left mouse button while on the angle constraint and drag it to the right of the angled line. It should appear similar to the diagram shown below.

Change the values of the constraints to match the diagram shown below. You have to double click on a value and a window will appear. After you change the value press the Enter key or select OK.

Save your document.




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Up to now you have used the constraint and the constraint by dialog icons to generate constraints. Next you will learn how the auto constraint icon and the animate constraint icon works. Open the constraint4 document and save with your initials. This will open the part called constraint4. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and then you can start adding constraints. There are two profiles in this sketch and you will try the auto constraint icon on both profiles. Using the left mouse button box in the first profile shown below. Press and hold the left mouse button while being up and to the left of the first profile and drag a box around the profile. This will select all of the elements in the box.

You can either select the elements before choosing the auto constraint icon or after you select the auto constraint icon. In this case you selected the elements before selecting the icon. Select the auto constraint icon. shown below.


This will open up an auto constraint window as



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Elements to be constrained

specifies what elements are to be constrained

Reference elements

allows you to specify an element or elements to use as a reference for its constraints

Symmetry lines

allows you to specify the center lines it should use when assigning symmetry constraints

Constraint Mode

if you specified a reference element then this will determine if you want the constraints to be defined one at the end of another (Chained) or if you want all constraints to be defined from the reference element (Stacked)

Select OK. Since this sketch does not have any symmetry lines and it is referenced by the origin location there is not a need to set any of the other options. It should appear similar to the diagram shown below.

You are now going to use the auto constraint icon to constrain the other profile within this sketch.




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Using the left mouse button box in the second profile shown below. Press and hold the left mouse button while being up and to the left of the second profile and drag a box around the profile. This will select all of the elements in the box.

Select the auto constraint icon. shown below.


Select OK. Constraints appear on the profile, however it is not perfectly constrained since it is not referenced to any location. It should appear similar to the diagram shown below.

You will now undo the these constraints and you will try using the auto constraint icon using reference elements. Select the undo icon in the bottom toolbar. All of the constraints should disappear and the profile should appear highlighted. If they do not disappear, keep selecting the undo icon until they disappear. If the profile does not appear highlighted then select the profile like you did earlier.



CATIA Part Design & Sketcher Select the auto constraint icon. shown below.

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Select in the box for Reference elements. You need to select on the area where it says No Selection in front of the label Reference elements. Select the vertical line and horizontal line from the other profile that are at the origin. This makes those two elements the reference elements for the constraints. The window should now appear as shown below.

You have two options on the Constraint Mode, either Chained or Stacked. This exercise will have you choose the Stacked option, however both diagrams are shown for your reference. You may want to try one and then undo it and try the other option. Select the Stacked option for the Constraint Mode. You have to select the down arrow to access the drop down list and then select the Stacked option.




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Select OK. Constraints appear on the profile. Notice how all of the constraints originate from the reference elements. If you use the Chained option then the first constraints originate from the reference elements but the other constraints originate at the ends of the previous constraints. Both diagrams are shown below for your comparison.

Stacked

Chained Save your document. Constraints, Page 122



CATIA® V5R6

You will now try using the animate constraint icon on a constrained sketch. You can use this icon at any time to see how your sketch changes as the value of a constraint varies. In this exercise you will try using this icon on a perfectly constrained sketch. Open the constraint5 document and save with your initials. This will open the part called constraint5. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and it should appear similar to the diagram shown below.

You will now use the animate constraint icon on a couple of the constraints. Select the animate constraint icon. This icon allows you to select a constraint and animate what happens as this constraint changes values.




CATIA® V5R6

Select the 1 inch radius constraint in the upper left of the sketch. An Animate Constraint window appears.

First value

the starting value for the animation

Last value

the ending value for the animation

Number of steps

determines the number of steps shown as the value varies between the first value and the last value

Actions plays the animation backwards pauses the animation stops the animation plays the animation forwards Options plays the animation once from start to finish plays the animation from start to finish and then back to the start continuously loops the animation forwards and backwards repeats the animation always showing it from start to finish Hide constraints


hides the constraints so all you see animating is the geometry



CATIA® V5R6

Change the First value to be .5, the Last value to be 2, and the Number of steps to be 20. You are now ready to see the animation. Select the one way icon under Options and then select the forward icon under Actions. Notice how the sketch changes shape as the constraint varies from its starting value to its ending value. Select the Hide constraints button and then select the forward icon again. Notice how all of the constraints are not seen anymore. This option only shows the actual geometry of the sketch. Select the round trip icon under Options and then select the forward icon under Actions. This time the animation plays from start to finish and then returns back to the start. Select the loop icon under Options and then select the forward icon under Actions. This time the animation plays from start to finish and then returns back to the start over and over again. Select the stop icon

under Actions. This stops the animation.

Select the repeat icon under Options and then select the forward icon Actions. This time the animation plays from start to finish over and over again. Select the stop icon

under

under Actions. This stops the animation.

Select Cancel. Your sketch returns to the original shape and the constraints appear again. You should practice animating other constraints using the animate constraint icon.




CATIA® V5R6

Modifications to profiles This involves modifying the geometry of your sketch to generate the desired profile. The options include cornering, chamfering, trimming and breaking geometry. If we have the geometrical and dimensional constraint options selected in the bottom toolbar then some constraints may automatically be generated when performing these options. Corner There are three new icons that appear on the bottom toolbar when you are in the corner option. trims both elements back to the corner trims the first element selected back to the corner generates the corner without trimming the elements Open the corner document and save with your initials. This will open the part called corner. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and it should appear similar to the diagram shown below.

Modifications to profiles, Page 126


CATIA Part Design & Sketcher Select the corner icon. bottom toolbar.

CATIA® V5R6

This activates the option and three new icons appear on the

Make sure that the trim all icon is selected on the bottom toolbar. This is normally the default choice. This exercise is only going to cover this option since it is the one most commonly used. It is suggested that you try out the other options on your own in order to make sure you understand their operation. Select the left vertical line and the top horizontal line. This specifies the two elements that you wish to generate a corner between. You now have to arbitrarily locate your corner which will determine its initial size. Select somewhere inside the corner. The corner should appear with tangency constraints generated on the two line and a radius constraint generated on the corner. It should appear similar to the diagram shown below.

You can change the value of the corner the same way you changed the value of constraints previously. Change the radius value to be .5 inches. The corner changes size. Undo the creation of the corner to get back your original sketch. You are now going to generate radius corners at all intersection of your sketch with a specified value.




CATIA® V5R6

Select all of the sketch. You can do this by pressing and holding the left mouse button up and to the left of the profile and then dragging the mouse down to the lower right, boxing in the entire profile. Select the corner icon.

A radius text box appears on the bottom toolbar.

Enter a value of .5 in the Radius box and press Enter. Corners appear at every intersection at a value of 0.5. It should appear similar to the diagram shown below.

Notice that most of the .5 constraints have a f(x) symbol next to it. This means that a formula has been applied to determine that constraint. In this case one of the corner constraints is specified and then all of the other ones are set to be equal to that one. If you were to change that one value then all of the other values would change because of the formulas. In the diagram shown above the upper left constraint is the driving constraint. Change the value of the driving constraint to be 0.75. This is the constraint that does not have a f(x) symbol next to it. Notice that all of the constraints change to that value. You will learn more about formulas later in this course. Save your document.




CATIA® V5R6

Chamfer There are three new icons that appear on the bottom toolbar when you are in the chamfer option. trims both elements back to the chamfer trims the first element selected back to the chamfer generates the chamfer without trimming the elements After choosing one of those icons and selecting the elements that you want to use to chamfer, three more icons appear. These determine what type of information you can enter and what is generated when the chamfer is created. hypotenuse and an angle two lengths one length and an angle Open the chamfer document and save with your initials. This will open the part called chamfer. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and it should appear similar to the diagram shown below.



CATIA Part Design & Sketcher Select the chamfer icon. bottom toolbar.

CATIA® V5R6


Make sure that the trim all icon is selected on the bottom toolbar. This is normally the default choice. This exercise is only going to cover this option since it is the one most commonly used. It is suggested that you try out the other options on your own in order to make sure you understand their operation. Select the left vertical line and the top left horizontal line. This specifies the two elements that you wish to generate a chamfer between. You can now arbitrarily locate your chamfer which will determine its initial size. Select the one length and an angle icon. This will generate a length from the sharp corner back to the beginning of the chamfer along the first element selected and the angle is the angle of the chamfer. Select somewhere inside the corner. The chamfer should appear with a length constraint and an angle constraint generated. It should appear similar to the diagram shown below.

Change the value of the length and angle to .5 and 30 respectively. Notice the chamfer changes size and angle. Luckily the 1.5 and 2.5 constraints were generated as distance constraints between two lines instead of length constraints. If they were generated as length constraints then a window would appear telling you that they would be converted to distance constraints because the chamfer will change the length of those lines.



CATIA Part Design & Sketcher Select the chamfer icon. bottom toolbar.

CATIA® V5R6


Make sure that the trim all icon the default choice.

is selected on the bottom toolbar. This is normally

Select the right vertical line and the top right horizontal line. This specifies the two elements that you wish to generate a chamfer between. You can now arbitrarily locate your chamfer which will determine its initial size. Select the one length and an angle icon. This will generate a length from the sharp corner back to the beginning of the chamfer along the first element selected and the angle is the angle of the chamfer. Select somewhere inside the corner. The chamfer should appear with a length constraint and an angle constraint generated. Change the value of the length and angle to .5 and 30 respectively. The final sketch should appear similar to the one shown below.

Save your document.




CATIA® V5R6

Trim and Break There are four icons that can be used to trim or break elements in the sketcher. trims both elements back to the intersection or just trims a single element back to the intersection trims both elements trims only the first element breaks an element at an intersection or at an arbitrary location quickly trims elements, there are three sub-options to this icon which determine how it works trims the element back to the nearest intersections, getting rid of the side you select trims the element back to the nearest intersections, keeping the side you select breaks the element at the nearest intersections closes a partial circle back to a full circle Open the trim document and save with your initials. This will open the part called trim. In order to work with the sketch you will need to go to the Sketcher and choose the sketch from the specification tree. Select the Sketcher icon and then select the Sketch from the specification tree. This takes you into the sketch and it should appear similar to the diagram shown below.



CATIA Part Design & Sketcher Select the quick trim icon.

CATIA® V5R6

The icon becomes activated.

Select the break and rubber in icon. This will allow you to break an element and trim it to the nearest intersections getting rid of the portion you select. Select the top horizontal line inside the circle. The line breaks at each intersection of the circle and is removed from the inside of the circle. Select the quick trim icon.

The icon becomes activated.

Select the break and rubber in icon. This will allow you to break an element and trim it to the nearest intersections getting rid of the portion you select. Select the bottom horizontal line inside the circle. The line breaks at each intersection of the circle and is removed from the inside of the circle. It should appear similar to the diagram shown below.

Select the break icon.

This will allow you break an element in to two pieces.

Select the circle and then the top left horizontal line. The circle breaks at the intersection of the line. A circle in CATIA has a natural break in order for the circle to have ends. Therefore it is not necessary to break a circle more than once to get two pieces. Notice that coincident constraints appeared on the broken elements automatically. Now that the circle is broken you can trim the two pieces to the appropriate intersections. Double click on the trim icon. on the bottom toolbar.

This activates the option and four new icons appear

Make sure that the trim all icon is selected.


This is normally the default choice.



CATIA® V5R6

Select the top right horizontal line and the top right portion of the circle. The circle should trim up to the intersection. Select the bottom right horizontal line and the bottom right portion of the circle. The circle should trim down to the intersection. Select the bottom left horizontal line and the bottom left portion of the circle. The circle should trim down to the intersection. The sketch should appear similar to the diagram shown below.

Sometimes it can be confusing seeing the curve between the lines but it appears only to show the coincidence between the two circles.




CATIA® V5R6

Now that you have gone through most of the constraint options you are ready to constrain some sketches for practice. Save the constrained sketches as constraint6, constraint7 and constraint8 respectively. Open the constraint6 document and go to the sketch and constrain the sketch to appear like the diagram shown below. You will want to generate the four corners using the corner option first and then constrain the circles concentric to the corners.

Open the constraint7 document and go to the sketch and constrain the sketch to appear like the diagram shown below.




CATIA® V5R6

Open the constraint8 document and go to the sketch and constrain the sketch to appear like the diagram shown below.

This ends the basic Sketcher section and you are now ready to start producing parts using the Part Design workbench. From now on it is assumed that you know how to use the various options that were covered in this section. If at any time you get stuck please refer back to this section.




CATIA® V5R6

Hide/Show This small exercise is to cover the steps necessary to hide and show geometry, whether it be sketcher geometry or part design geometry. Open the hide show document and go to the sketch. You will now hide and show some geometry. Select the hide/show icon.

This will allow you hide some of your geometry.

Select the circle. The circle disappears but it is not deleted. Select all four edges of the window on the right. You can do this by selecting up and to the left of the window and dragging the cursor over the entire window using the first mouse button. Select the hide/show icon.

All four lines disappear but they are not deleted.

Select the swap visible space icon. Notice your background changes color and the only geometry you see is the circle and the window that you hid earlier. You have just switched to the hidden side of your part. Select the hide/show icon. Select the circle. The circle disappears and returns to the visible or show side of your part. Select all four lines and then select the hide/show icon. lines to the visible side of your part. Select the swap visible space icon. should see all of your geometry.

This will return the four

This returns you to the visible side and you

The procedure for hiding or showing geometry is always the same whether it is using sketch geometry or part design geometry. There will be times when you are going to want to hide some of your geometry because it starts cluttering up your display and you are not ready to delete it or you cannot delete it because it is associated with other geometry. Save your document.


Hide/Show, Page 137


CATIA® V5R6


Hide/Show, Page 138



CATIA® V5R6

Basic Part Design This section will cover the basic use of the part design workbench to create parts. This section will consist of three parts: basic shapes, modifications to shapes and interfacing between part design and sketcher. Basic Shapes This part will discuss the various shapes that can be created in part design using the icons on the Part Design workbench. The purpose of this group of exercises is to introduce how to use those icons and their options. The usefulness of them depend on the part you are trying to create. It is important for you to understand how to use each of these icons in conjunction with your sketches to produce your final part.




CATIA® V5R6

Pad The pad icon allows you to use a sketch and extrude it in a linear direction producing a solid pad. When you create a pad a Pad Definition window appears like the one shown below.

Initially the window will appear with only the First Limit and then you have the option to select the More>> option to see the Second Limit. Since the options are the same for both limits they will be discussed only once. Type

Dimension

allows you to key in a Length

Up to next

goes to the next side of an existing part

Up to last

goes to the last side of an existing part

Up to plane

goes to a specified plane which is its Limit

Up to surface

goes to a specified surface which is its Limit

When you select a Type other than Dimension you will have the option to specify an Offset value from the corresponding limit. Profile Selection

specifies which sketch will be used, you have the option to modify the sketch using the sketcher icon next to the box

Mirrored extent

applies to the Type Dimension, it will go the same distance in both directions, thereby not being able to specify a second limit

Reverse Direction

changes the direction to the opposite direction

Direction Normal to profile

the direction will be in the normal direction of the sketch

Reference

allows you to specify an element that defines the direction




CATIA® V5R6

Open the pad1 document and save with your initials. You should see two sketches already created for you. Select the pad icon. This will allow you to create a pad using one of the sketches. This exercise is going to cover the various methods that you can use to create pads. Select Sketch.1. This specifies that you want to use that sketch to define the profile of your pad. A Pad Definition window should appear similar to the one shown below.

For this pad you are going to use the basic option of keying in a length for pad. You will also preview what the Mirrored extent and Reverse Direction options allow you to do. Change the value in Length to be 4. Do not press enter or else it will automatically create the pad with that value. Normally you would just enter the value and press Enter, however you are going to want to Apply in order for you see what it is going to do until you understand the different options. Select Preview. A preview of what the pad will look like appears. You will now change some of the other options to see the difference between them. Select Mirrored extent and select Preview. As you can see instead of the pad extending in only the one direction 4 inches it now extends both directions 4 inches each. It basically is using your current sketch as the mirror plane. Select Mirrored extent again to turn it off and select Preview. Now you are going to reverse the direction in order for the pad to be created in the opposite direction. Select Reverse Direction and select Preview. Notice that the pad is still going to be 4 inches wide but it is now going in the opposite direction. This is the pad you want to create.




CATIA® V5R6

Select OK. The pad should be created and appear similar to the diagram shown below. Notice that the sketch automatically was hidden after being used by the pad. This is true when using most of the options because of a setting under the pull down menu Tools, Options.

You are now going to explore some of the other Types that you can use to define limits for pads that you create. Select the pad icon. Select Sketch.2. This specifies the sketch that you want to use to create the next pad. A Pad Definition window appears as shown below.

Select Reverse Direction so that the direction is toward the other pad. Now you are going to see what the other Types allow you to do.




CATIA® V5R6

Change the Type to Up to next and select Preview. Notice that the pad only goes to the next side of the other pad. It should appear similar to the diagram shown below.

Change the Type to Up to last and select Preview. Notice that the pad goes all the way to the last side of the previous part. It should appear similar to the diagram shown below.

Change the Type to Up to plane. When you use this option you have to specify a plane or a planar side that you want the pad to be limited by.




CATIA® V5R6

Select the plane that is away from the origin and select Preview. Notice that the pad goes up to the plane and then stops. It should appear similar to the diagram shown below.

You may have to rotate the part around in order to see the limitation better. The Up to surface option works very similar to the Up to plane option except that you can specify a surface instead of a plane. Select the More>> option. This expands the window and shows some other options. The window should appear similar to the one shown below.

Currently the Direction is specified to be Normal to profile. You will turn that off and specify an element to be used as the direction. Once again this is just to show you the capabilities of the option. Select Normal to profile to turn it off. The Normal to profile option is no longer activated. Select in the Reference box. This allows you to specify an element to be used as the direction.




CATIA® V5R6

Select the angled line closest to the origin and select Preview. The pad extrudes in the direction of the line and stops at the plane that was specified earlier. It should appear similar to the diagram shown below.

Select Normal to profile. This changes the direction back to being normal to the sketch. You are now going to use a First Limit and a Second Limit to create the pad. Under the First Limit select the Limit box. This will allow you to specify a new plane for your limit. Select the angled side closest to the sketch. This defines the First Limit. You will now define the Second Limit. Under the Second Limit change the Type to Up to plane. Under the Second Limit select the Limit box.




CATIA® V5R6

Select the angled side farthest from the sketch and select Preview. This defines the Second Limit and shows you a preview of your new pad. It should appear similar to the diagram shown below.

Select OK. The final part should look similar to the diagram shown below.

This exercise showed most of the options available when creating a pad. There are other shapes that have these same options and they work the same. Hopefully you have a good understanding of what each option allows you to do. Note: Open profiles (sketches) can be used to create pads or pockets as long as they will be closed by the other faces of your existing part. Save your document. Basic Shapes, Page 146



CATIA® V5R6

Open the pad2 document and save with your initials. You should see three sketches already created for you. Select the pad icon.

This will allow you to create a pad using one of the sketches.

Select Sketch.1. This specifies that you want to use that sketch to define the profile of your pad. Using the Type Dimension and a Length of .75 create the pad. The pad should appear similar to the diagram shown below.

Select the pad icon.

This will allow you to create a pad using one of the sketches.

Select Sketch.2. This specifies that you want to use that sketch to define the profile of your pad. Using the Type Dimension and a Length of .75 create the pad. The pad should appear similar to the diagram shown below.




CATIA® V5R6

Pocket The pocket icon allows you to use a sketch and extrude it in a linear direction producing a pocket. When you create a pocket a Pocket Definition window appears like the one shown below.

Initially the window will appear with only the First Limit and then you have the option to select the More>> option to see the Second Limit. Notice that the options are exactly the same as the options for creating a pad. The major difference between pad and pocket is that a pocket is removed instead of added to your part. Type

Dimension

allows you to key in a Length

Up to next


Up to last


Up to plane


Up to surface


When you select a Type other than Dimension you will have the option to specify an Offset value from the corresponding limit. Profile Selection


Mirrored extent

applies to the Type Dimension, it will go the same distance in both directions, thereby not being able to specify a second limit

Reverse Direction

changes the direction to the opposite direction

Direction Normal to profile

the direction will be in the normal direction of the sketch

Reference

allows you to specify an element that defines the direction




CATIA® V5R6

You will now create a pocket in the existing part using Sketch.3. Select the pocket icon. sketches.

This will allow you to create a pocket using one of the

Select Sketch.3. This specifies that you want to use that sketch to define the profile of your pocket. Select Reverse Direction. Using the Type Up to next create the pocket. The pocket should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

Open the pocket document and save with your initials. You should see a pad and a sketch that have been created for you. Select the pocket icon.

This will allow you to create a pocket using the sketch.

Select Sketch.2. This specifies that you want to use that sketch to define the profile of your pocket. Change the Type to Up to next and select Preview. A preview of the pocket should appear. It should appear similar to the diagram shown below.

Change the Type to Up to last and select Preview. A preview of the pocket should appear. It should appear similar to the diagram shown below.

Select OK. The pocket appears. Save your document.




CATIA® V5R6

Multiple Profiles You can create objects using a single profile of a sketch that contains multiple profiles. This allows you to create multiple profiles on the same sketch and then using pad or pocket you can have each profile extrude a different distance as if they were separate sketches. When you do this each pad or pocket will reference the same sketch just a different part of the sketch. Open the multiple profiles document and save with your initials. You should see a sketch that has already been created for you. Select the pad icon. In the Selection box press the third mouse button and select Go to profile definition. The Profile Definition window appears as shown below.

This will allow you to select the sub-elements of a sketch. Select the box portion of the sketch. Notice just by selecting an edge that entire profile was selected but not the whole sketch. Select OK. This closes the Profile Definition window and returns to the Pad Definition window with the Selection being Complex. Change the Length to be 1 and select OK. The pad is created using just the one profile of the sketch. Notice that the sketch still remains shown because you did not use the entire sketch therefore it did not automatically hide.




CATIA® V5R6

Repeat the steps and create pads out of the other two profiles 1 inch in length. It should appear similar to the diagram shown below.

The specification tree should have each pad using the same sketch as shown below.

It is normally a better idea to create a separate sketch for each object but there are times when this capability becomes extremely useful, especially when constraining. Remember this option is only available with pad and pocket. Save your document.




CATIA® V5R6

Shaft The shaft icon allows you to use a sketch and rotate it in a circular direction producing a solid revolution. It is necessary to have an axis defined in your sketch in order to create a shaft. The axis needs to represent the center of the revolution. When you create a shaft a Shaft Definition window appears like the one shown below.

As you can see there are few options when creating a shaft compared to creating a pad. Limits First angle

the angle in the initial direction from the sketch

Second angle the angle in the opposite direction from the sketch Profile Selection


Selection

defines the axis that the profile will be rotated around

Axis




CATIA® V5R6

Open the shaft document and save with your initials. You should see two sketches that have been created for you. Select the shaft icon.

This will allow you to create a shaft using a sketch.

Select Sketch.1. This specifies that you want to use that sketch to define the profile of your shaft. Change the First angle value to 90 and the Second angle value to 135 and select Preview. Notice that the shaft went 90 degrees in the one direction and 135 degrees in the other direction. It should appear similar to the diagram shown below. You can also use a negative value to get the shaft to start and end at a different location then where the sketch is.

Change the First angle value to -90 and the Second angle value to 270 and select Preview. Notice that the shaft begins at -90 and ends at 270. The total angle that the shaft covers is the addition of the two angles, therefore it is necessary that the sum does not exceed 360. It should appear similar to the diagram shown below.




CATIA® V5R6

Change the First angle value to 90 and the Second angle value to 90 and select Preview. Now the shaft is defined for the other half. It should appear similar to the diagram shown below.

Change the Second angle value to 0 and the First angle value to 360 and select OK. The shaft is created as a full revolution. It should appear similar to the diagram shown below.




CATIA® V5R6

Groove The groove icon allows you to use a sketch and rotate it in a circular direction producing a solid revolution that is removed from the current part. It is necessary to have an axis defined in your sketch in order to create a groove. The axis needs to represent the center of the revolution. When you create a groove a Groove Definition window appears like the one shown below.

Notice that the options are exactly the same as the options for creating a shaft. The major difference between shaft and groove is that a groove is removed instead of added to your part. Limits First angle

the angle in the initial direction from the sketch

Second angle the angle in the opposite direction from the sketch Profile Selection


Selection

defines the axis that the profile will be rotated around

Axis



CATIA Part Design & Sketcher Select the groove icon.

CATIA® V5R6

This will allow you to create a groove using a sketch.

Select Sketch.2. This specifies that you want to use that sketch to define the profile of your groove. Change the First angle value to 360 and the Second angle value to 0 and select OK. It should appear similar to the diagram shown below.

You can define the angles the same way as you define the angles for a shaft. Save your document.




CATIA® V5R6

Open the groove document and save with your initials. You should see a shaft and a sketch that have been created for you. Select the groove icon.

This will allow you to create a groove using a sketch.

Select Sketch.2. This specifies that you want to use that sketch to define the profile of your groove. Change the First angle value to -15 and the Second angle value to 345 and select Apply. Notice that the groove has a 30 degree gap in it centered around the sketch. It should appear similar to the diagram shown below.

Select OK. Save your document.




CATIA® V5R6

Hole The hole icon allows you to create a variety of holes from simple holes to counterdrilled holes. When you create a hole a Hole Definition window appears like the one shown below.

There are many options for creating a hole. The various options are spread over three tabs, Extension, Type and Thread Definition. The Extension options are explained below. There are five different options for defining the length of the hole, many of which are similar to the pad and pocket options. Blind

goes a certain distance

Up To Next


Up To Last


Up To Plane


Up To Surface


Diameter

the diameter of the hole

Depth

the length of the hole, only applies to Blind

Limit

defines the limit element, only applies to Up to Plane and Up to Surface

Offset

the offset distance from the limit




CATIA® V5R6

Axis Reverse

reverses the direction of the hole

Normal to surface

aligns the axis of the hole normal to the surface if selected otherwise you can specify the direction using the box below the option

Positioning Sketch

allows you to constrain the center of the hole before creating

Bottom Flat

the hole will be flat on the bottom, only applies to Blind

V-Bottom

the hole will have a v-shaped bottom, only applies to Blind, the angle of the v-shape can be specified in the Angle box under the option

The Type options are explained below. Simple

a straight hole with no parameters

Tapered

the parameters define the angle of the taper



CATIA Part Design & Sketcher Counterbored

CATIA® V5R6

the parameters define the size and the depth of the counterbore

The counterbore diameter must be greater than the hole diameter and the hole depth must be greater than the counterbore depth. Countersunk

the parameters define the depth and angle of the countersunk

The countersink diameter must be greater than the hole diameter and the countersink angle must be greater than 0 and less than 180 degrees.



CATIA Part Design & Sketcher Counterdrilled

CATIA® V5R6

the parameters define the diameter and depth of the counterbore and the angle from the bottom of the counterbore to the diameter of the hole.

The counterdrill diameter must be greater than the hole diameter, the hole depth must be greater than the counterdrill depth and the counterdrill angle must be greater than 0 and less than 180 degrees.




CATIA® V5R6

The Thread Definition options are explained below.

Thread Definition Type No Standard

Allows the user to enter the values

Metric Thin Pitch

Uses AFNOR standard values

Metric Thick Pitch

Uses AFNOR standard values

Thread Diameter

Diameter of the thread

Hole Diameter

Diameter of the hole

Thread Depth

How far the thread extends in the hole

Hole Depth

The depth of the hole

Pitch

The distance the thread drops in one revolution

Right-Threaded or Left-Threaded

Determines which way the thread will be revolved

Standards Add

Allows you to create a standard thread definition

Remove

Allows you to remove a standard thread definition




CATIA® V5R6

Open the hole document and save with your initials. You should see a part already created for you. You will probably want to rotate the part so that you can see the top surfaces easier. Select the hole icon. This will allow you to create a hole. The nice thing about using the hole icon is that you do not have to generate a sketch ahead of time. It will create a sketch for you specifying the center of the hole. You can go in to the sketch and put parameters on the sketch to position the hole. You can also have it automatically generate parameters by selecting an edge or edges before defining the surface that you want the hole to appear on. You will now try creating some holes using various options. Select the top inner edge of the rim. This specifies that you want the hole to be concentric with this edge.

Select the flat surface at the bottom of the pocket. This specifies the surface where you want the hole to be located. The Hole Definition window should appear. Using the Extension tab change the mode to Up To Last and the Diameter to 1 inch.




CATIA® V5R6

Using the Type tab change the type to Simple and select OK. This is the default type so it may not be necessary to change it. The hole should appear similar to the diagram shown below.

Select the hole icon.

This will allow you to create a hole.

Select the bottom inner edge of the rim. This specifies that you want the hole to be concentric with this edge.

Select the flat surface at the bottom of the pocket. This specifies the surface where you want the hole to be located. The Hole Definition window should appear.




CATIA® V5R6

Using the Extension tab change the mode to Up To Last and the Diameter to 1 inch. It may already have those settings, if it does then it is not necessary to change them. Using the Type tab change the type to Simple and select OK. This is the default type so it may not be necessary to change it. The hole should appear similar to the diagram shown below.

Select the hole icon.


Select the top surface of the bottom plate as indicated by the arrow. This specifies that you want the hole to be approximately between the small radius and large radius on that surface. The Hole Definition window should appear.




CATIA® V5R6

Using the Extension tab change the mode to Up To Last and the Diameter to 1 inch. It may already have those settings, if it does then it is not necessary to change them. Using the Type tab change the type to Tapered and change the Angle to 45 and select Preview. The hole should appear similar to the diagram shown below.

Using the Type tab change the type to Counterbored, the Diameter to 1.5 and the Depth to .25 and select Preview. The hole should appear similar to the diagram shown below.




CATIA® V5R6

Using the Type tab change the type to Counterdrilled, the Diameter to 1.5, the Depth to .25 and the Angle to 120 and select Preview. The hole should appear similar to the diagram shown below.

Using the Type tab change the type to Countersunk, the Depth to .25 and the Angle to 90 and select OK. The hole should appear similar to the diagram shown below.

The previous steps took you through the different types of holes that you can create. There are some other options available under the Extension tab. Most of those options apply to Blind holes and you should make sure you are aware of them. The option that is not covered in this exercise that you definitely want to understand is the option to change the direction of the hole. This option works exactly the same as it did when you created pads. The thread options are not covered in this exercise but if you use those options, your hole icon in your specification tree will appear with a thread notation. When you create a drawing from this part the thread notation will appear in the appropriate views. Basic Shapes, Page 168



CATIA® V5R6

To finish this exercise you are going to create five more holes on the top surface of the bottom plate and then constrain all of them and the previous hole. All the holes are countersunk holes using a depth of .25 and an angle of 90. Select the hole icon.


Create five holes at the approximate locations indicated by the arrows. The holes should be Countersunk, with a Depth of .25 and an Angle of 90. The diagram shown below shows the locations. If you have trouble, please refer back to the previous steps.

After you have finished creating the holes the part should appear similar to the diagram shown below.




CATIA® V5R6

Constrain the locations of the six holes using the constraints as shown below. This diagram is given just to show you the constraint values, you will have to constrain each hole individually. It is suggested that you use the planes when constructing your constraints. Notice that only the previous holes appear when you constrain, this is because of the location you are at in the specification tree. You will get more involved with the specification tree at a later time.

Note: This is not the suggested method to use when creating a group of identical holes. Later in class you will learn how to define a pattern that can be applied to an object such as a hole. Save your document.




CATIA® V5R6

Rib The rib icon allows you to use a sketch to define a profile and then use another sketch to determine the path that the profile will follow. When you create a rib a Rib Definition window appears like the one shown below.

The options are discussed below. Profile

defines the shape that is supposed to be used for the rib

Center curve defines the path that is to be followed by the profile Profile control Keep angle

keeps the profile at the same orientation with respect to the center curve as it is initially as it follows the curve

Pulling direction

defines an orientation that you want the profile to keep as it follows the center curve

Reference surface

defines a surface that controls the orientation of the profile to be normal to the surface as it follows the center curve

Merge ends

creates material between the ends of the rib and existing material in specific cases

Open the rib document and save with your initials. You should see three sketches that have been created for you. Select the rib icon.

This will allow you to create a rib using the sketches.

Select Sketch.1. This specifies that you want to use that sketch to define the profile of your rib. Select Sketch.2. This specifies the center curve that you want your profile to follow. You are going to use the Keep angle option therefore you are ready to select Preview.




CATIA® V5R6

Select Preview. A preview of the rib appears and should look similar to the diagram shown below.

Notice that the orientation with respect to the center curve is the same from beginning to end as it followed the curve. The orientation was determined by the initial orientation the sketch had with the center curve. Next you will define a pulling direction using the third sketch to see the difference. Change the Profile control to Pulling direction. You now have to define a direction. Select the vertical line of Sketch.3 and select Preview. This defines that edge as the pulling direction for the rib. Select OK. The rib appears similar to the diagram shown below.

Save your document. Basic Shapes, Page 172



CATIA® V5R6

Slot The slot icon allows you to use a sketch to define a profile and then use another sketch to determine the path that the profile will follow. The main difference between a slot and a rib is that the slot will remove the material instead of add material. When you create a slot a Slot Definition window appears like the one shown below.

The options are the same as the rib options but they are still discussed below. Profile

defines the shape that is supposed to be used for the slot

Center curve defines the path that is to be followed by the profile Profile control Keep angle

keeps the profile at the same orientation with respect to the center curve as it is initially as it follows the curve

Pulling direction

defines an orientation that you want the profile to keep as it follows the center curve

Reference surface

defines a surface that controls the orientation of the profile to be normal to the surface as it follows the center curve

Merge ends

removes material between the ends of the slot and existing material in specific cases

Open the slot document and save with your initials. You should see a pad and a few sketches that have been created for you. Select the slot icon.

This will allow you to create a slot using the sketches.

Select Sketch.2. This specifies that you want to use that sketch to define the profile of your slot. Select Sketch.3. This specifies the center curve that you want your profile to follow. You are going to use the Keep angle option therefore you are ready to select OK.




CATIA® V5R6

Select OK. The slot appears and should look similar to the diagram shown below.

Save your document.




CATIA® V5R6

Stiffener The stiffener icon allows you to create a stiffener by defining the shape of the stiffener in a sketch. It will fill in the area between that sketch and the rest of the part. When you create a stiffener a Stiffener Definition window appears like the one shown below.

The options are explained below. Thickness

defines the thickness of the stiffener

Mirrored extent Depth

toggle between having the stiffener centered around the original sketch or having it extrude in only one direction

specifies which direction you want the stiffener to follow toward the part in order to make the stiffener

Profile Selection


This option is useful since you do not have to create a closed profile in your sketch. All you have to do is create the outside edge of your stiffener and it will limit itself to the boundaries of your existing part similar to pad. In this exercise you will see that it does not extend underneath the existing part are into the hole area of the part. Open the stiffener document and save with your initials. You should see a part made up of a few shapes. Select the stiffener icon. sketches.

This will allow you to create a stiffener using one of the

Select Sketch.8. This sketch is used to define the shape of the stiffener. A Stiffener Definition window should appear. Change the Thickness to .625 and make sure that Mirrored extent is on. You are now ready to build the stiffener. © Wichita State University



CATIA® V5R6

Select OK. The stiffener is created and should appear similar to the diagram shown below.

If you rotate your part around you will see that the stiffener limited itself to the existing part. It did not continue into the hole or underneath the part.

Later in this course you will learn how to use edges of your part to help constrain your sketches. If you want to attempt to do this now you can try building a sketch on the center plane by using the line option and constraining it to be tangent to both curved edges. After creating the sketch you can create a stiffener on that side of the part as well. Save your document.




CATIA® V5R6

Modifications to Shapes This part of the book will cover the icons that are available to let you modify your parts. These options include filleting, chamfering, applying draft angles, shelling, adding thickness and adding thread definition to your existing part. You will also learn how to modify the values that were used when creating basic shapes. Fillet The fillet icon allows you to create fillets on interior edges and rounds on exterior edges. The program will determine whether you want a fillet or a rounded edge based on the type of edge that is selected. There are a few options when creating fillets. creates a fillet or round along edges of your part

Radius

the radius of the fillet or round

Object(s) to fillet

the edge or face that needs to be filleted

Propagation

Tangency

will propagate around tangencies

Minimal

will only fillet the selected edge

Edge(s) to keep


defines rolling edges for your fillet

Modifications to Shapes, Page 177


CATIA® V5R6

creates a variable radius fillet or round along edges of your part

Points

the locations along an edge that you can specify a different radius

Variation

Cubic

maintains tangencies as it varies

Linear

varies linearly, following a straight line

Circle Fillet

allows you to create a fillet that maintains its circular shape while using a spine, this option could be used to create a fillet along two consecutive edges that are not tangent continuous that you want to be treated as a single edge

creates a fillet connecting two faces

Faces to fillet

the faces that you want to use to fillet between

creates a tri-tangent fillet using three faces

Face to remove

the third tangent face that will be removed when the fillet is generated




CATIA® V5R6

Open the fillet document and save with your initials. You should see the following part.

Select the tritangent fillet icon. This will allow you to create a fillet using two faces to determine the sides of the fillet and a third face that the fillet will be tangent to. Select the left flat side. The side should highlight. You may have to rotate the part in order to select the other side. Select the right flat side. The side should highlight. Notice in the Tritangent Fillet Definition window that it automatically moved to Face to remove. The next face that you select will be removed and the fillet will be created tangent to that face. Select the front end of the part. This is the end that does not have the stiffener. Select OK. The front end of the part is filleted. It should appear similar to the diagram shown below.




CATIA® V5R6

Select the edge fillet icon. This will allow you to specify a radius and then select edges that you want filleted or rounded. Change the radius to .125. Select the edges as shown in the diagrams below. Sometimes the fillet outcome can vary depending on which edges you select first. For our case select the angled lines first.

Select OK. The fillets should appear similar to the diagram shown below.

Notice that in the corners the fillets come to a sharp edge. This is because you missed selecting two of the edges. Fortunately this is not your fault because that is what you were instructed to do. This gives you an opportunity to modify your fillet and include those two edges.




CATIA® V5R6

Double click on EdgeFillet.1 in the specification tree. This opens up the Edge Fillet Definition window and allows you to either add or remove edges to be filleted. Select the two edges shown in the diagram below. Notice that the other seven edges remain selected since you selected them the first time.


Save your document.




CATIA® V5R6

Open the other fillets document and save with your initials. You should see the following part.

Select the edge fillet icon. edges of the part.

This will allow you to put radius corners on the front two

Change the value of the Radius to be .5 and select the two front edges of the part as shown above. Select OK. The fillets should appear similar to the diagram shown below.

Select the edge fillet icon.

This time you are going to define edges to keep.

Select the More>> option and then select in the Edge(s) to keep box. This will allow you to select the rolling edges.




CATIA® V5R6

Select the three edges as shown below. The edges should turn a pink color.

Select in the Object(s) to fillet box and select the edges as shown below. The radius value should still be 0.5.





CATIA® V5R6

Select the variable radius fillet icon. This will allow you to create a variable radius fillet along the top outside edge of the base. Select the top outside edges of the base as shown below. Radius values should appear at the ends of each edge selected.

Change the radii on the two sides to be 0.25 (4 places) and the radii on the front edge to be 0.125 (2 places) and select OK. The fillet should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

Chamfer The chamfer icon allows you to create chamfers either by using two lengths or using a length and an angle. This will basically remove a sharp corner and replace it with an angled corner. The Chamfer Definition window appears below along with an explanation of its options.

Mode

Length1/Angle

the length is the distance from the sharp corner back to the start of the chamfer and the angle is the angle the chamfer will use when created

Length1/Length2

the lengths specify the distance from the sharp corner back to the start and end of the chamfer

Object(s) to chamfer these are the edges or faces that you wish to chamfer Propagation

Reverse

Tangency

will propagate around tangencies

Minimal

will only chamfer the selected edge

reverses the direction of the first length

Open the chamfer2 document and save with your initials. You should see the following part.




CATIA® V5R6

Select the chamfer icon. This will allow you to create a chamfer along an edge. The Chamfer Definition window should appear. Change the Mode to Length1/Length2. This allows you to specify two lengths which are the distances from the sharp corner to the beginning and ending of the chamfer. Change Length1 to be 1 inch and Length2 to be .5 inches. You want the chamfer to begin 1 inch from the sharp corner and end .5 inches from the corner in the other direction. Select the edges shown in the diagram below.

Make sure the direction is pointing across and not down, if it is not select the Reverse box. This will force the chamfer to start 1 inch over and end .5 inches down. Select OK. The chamfer is created and should look similar to the diagram shown below.

Save your document.




CATIA® V5R6

Draft Angle The draft angle icon allows you to put draft angles on your part. This is useful when designing molded parts since it is necessary for them to have draft angles in order for the part to be removed from the mold. There are two options when creating draft angles. creates draft angles along faces of a part

Angle

angle of the draft

Face(s) to draft

faces to be drafted

Selection by neutral face

selects the faces that are adjacent to the neutral face

Neutral Element Selection

the element that is to remain neutral and the angle is based off of this neutral

Propagation

None

uses the element that is selected only

Smooth

uses the element that is selected and adjacent elements that are tangent to the selected element

Pulling Direction Selection

the direction that the mold would be removed

Controlled by reference

if toggled on then when you modify the pulling direction element the draft will modify accordingly




CATIA® V5R6

Parting Element Parting = Neutral

uses the neutral element as a parting element

Draft both sides

applies the draft angle to both sides of the parting element

Define parting element

allows you to define a parting element other than the neutral element

Selection

the element that is used as the parting element

This has some of the same options as discussed earlier except you can choose a curved face and use its reflect lines to draft a side or sides. The draft option uses colors to signify the different elements. The neutral element is blue, the neutral curve is pink and the faces to be drafted are dark red. Open the document called draft and save it with your initials. If you prefer you could open your chamfer2 document and save it with the name draft. You should see the following part.




CATIA® V5R6

Select the draft angle icon. This will allow you to put draft angles on faces of your part. The Draft Definition window appears. Change the Angle to 20 degrees. Select the front face and the back face of the part. You will have to rotate the part around in order to select the back face. Select in the Selection box under Neutral Element and select the top face of your part. This makes the top face the neutral element. Make sure the pulling direction is pointing up. If the arrow is not pointing up then you need to select it to reverse its direction. Select OK. The draft angles are applied to your part and it should appear similar to the diagram shown below.

You will now try applying a draft angle using the reflect lines option. Select the draft reflect line icon. This allows you to select a curved face and apply draft angles to that side using the reflect lines of the curved face. The Draft Reflect Line Definition window appears.




CATIA® V5R6

Select the four curved faces of the part. There are two curved faces on the left side and two curved faces on the right side. You can refer to the diagram shown above for a reference. You may have to rotate your part around in order to select the other curved faces. Notice that neutral lines or reflect lines appear on the curved faces. Make sure that the Angle is set to 20 degrees and that the pulling direction is pointing up and select OK. The draft angles are applied to the sides of the part and it should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

Shell The shell icon allows you to hollow out a part by selecting which faces you want removed and then specifying a wall thickness. This is a great option when working with thin walled parts. The Shell Definition window and its options are discussed below.

Default inside thickness

how far in the wall thickness will go from the existing part

Default outside thickness

how far out the wall thickness will go from the existing part

Faces to remove

the faces that are going to be removed

Other thickness faces

allows you to select faces and then specify a thickness from those faces other than the default thicknesses specified earlier

Open the document called shell and save it with your initials. The part should look like the one shown below.

Select the shell icon. This will allow you to hollow out this part. The Shell Definition window should appear. Select the top face of the part. This is the face that is going to be removed leaving a wall thickness. You can specify more than one face to be removed but in this case you will not.




CATIA® V5R6

Change the Default inside thickness to .125 inches and the Default outside thickness to 0 inches. When you specify a thickness you have to be careful not to specify too large of a thickness because you can violate the radius of your curved faces. For example, this part has radii of .25 and if you specify an Inside thickness equal to or greater than .25 then it will not be able to perform the shell. Select OK. The shell is performed and it should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

Thickness The thickness icon allows you to either add or remove thickness on a side of a part. You would normally use this option when you need to add thickness to a side made up of several basic shapes. Otherwise, you would just modify the shape that needs to be a different thickness. The Thickness Definition window and its options are discussed below.

Default thickness

the default amount of thickness that you want added or removed, a negative value removes thickness

Default thickness faces

the faces that you want the Default thickness to be applied to

Other thickness faces

the faces that you want a different thickness applied to other than the Default thickness

Open the thick document and save it with your initials. The part should appear like the one shown below.

Select the thickness icon. This will allow you to add or remove thickness to a side. The Thickness Definition window should appear.




CATIA® V5R6

Select the inside curved face of the outside cylinder. The face should highlight. Notice that it propagated around to all tangent faces. Change the Default thickness to .125 inches. This will add .125 inches to the thickness of that face. Select OK. It should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

Modifying values When you create any of the basic shapes or perform any of the modifications to your part using the options discussed earlier they appear in the specification tree. The values used to make up those shapes or modifications are stored in those items. If you want to modify the values all you have to do is double click on the item in the tree and the definition window for that item will appear. This allows you to change any of the specifications in the window. You can also modify the sketch of any of the basic shapes by double clicking on them as well. This will take you to sketcher mode and then you can modify the constraints of the sketch. The following exercises will have you make changes to some existing parts. Open the modify1 document and save it with your initials. The part should appear similar to the one shown below.

Double click on Pad.2. Notice that the Pad Definition window appears. Also the only thing shown on the screen now is from Pad.2 on up, everything that occurred after Pad.2 does not presently appear. Change the Length to .5 inches and select OK. The pad becomes thicker. Double click on EdgeFillet.2. Notice that the Edge Fillet Definition window appears.




CATIA® V5R6

Change the Radius to .125 inches and select OK. The fillets change size. The part should now appear similar to the one shown below.

Rotate the part so you can see the pocket in the middle of the part. It should look similar to the diagram shown below.

You are now going to modify the sketch of the pocket.




CATIA® V5R6

Double click on Sketch.8. Notice that it automatically went into sketcher mode. You should see all of the constraints for the sketch.

Change the .25 radius constraint to be .375 inches. The sketch should change shape but still be perfectly constrained. Exit the sketcher by selecting the icon. This exits the sketcher and returns you to your part. The part automatically updates reflecting the change you made to the sketch of the pocket.

Save your document. © Wichita State University



CATIA® V5R6

Open the modify2 document and save it with your initials. It should appear similar to the one shown below.

Modify Hole.1 to have a diameter of 1.5 inches. Change Hole.4 to use Up to Surface and select the inside of the big cylinder. You should be able to see the hole extend into the middle cylinder of the part. Modify EdgeFillet.1 to use a radius of .625 inches. Modify EdgeFillet.2 to use a radius of .125 inches. The part should look similar to the diagram shown below.

Save your document.




CATIA® V5R6

Open the modify3 document and save it with your initials. It should appear similar to the one shown below.

Modify Pad.3 to be .375 inches thick. Modify Pad.4 to be Mirrored extent with a Length of .25 inches. This will make the pad .5 inches thick. Modify EdgeFillet.2 to use a radius of .125 inches. Change Hole.2 to be countersunk instead of counterbored and use an angle of 90 degrees. Change Hole.3 to use a 1 inch diameter and to be countersunk with an angle of 90 degrees. The part should look similar to the diagram shown below.

Save your document.




CATIA® V5R6

Interfacing with Sketcher In order to create many of the parts that you will be creating it is necessary for you to be able to use existing part geometry to assist in making a sketch. This part of the book covers how to use existing sides of your part to define a sketch plane and how to use existing edges of your part to constrain your sketch. Open the interface document and save it with your initials. A single pad should appear already created for you. Select the sketcher icon and select the face of the part as shown below.

Notice that you were able to select a face of an existing part and use it to define the sketch plane. This gives you added flexibility instead of always using the three primary planes. Create a box using the rectangle icon. It should be positioned and look similar to the diagram shown below.

Constrain the left side of the rectangle to be coincident with the left edge of the face. Notice that you will use the edge of the part to force the left side of the current sketch to be coincident with the left edge of that face. Constrain the right side of the rectangle to be coincident with the right edge of the face. Constrain the bottom of the rectangle to be coincident with the bottom edge of the face.

Interfacing with Sketcher, Page 200



CATIA® V5R6

Constrain the length of the right side to be 2.5 inches. The sketch should be perfectly constrained and appear similar to the one shown below.

Exit the sketcher and create a pad using this sketch that is .625 thick, it should extrude into the existing part. The part now includes your new pad. Select the sketcher icon and select the face of the part as shown.




CATIA® V5R6

Create and constrain the sketch as shown below. Notice that you will be using edges of the existing part to constrain some of your elements.

Exit the sketcher and create a pocket using this sketch and have it go all the way through the part. Select the sketcher icon and select the face of the part as shown.




CATIA® V5R6


Exit the sketcher and create a pad using this sketch, it should go .125 inches above the existing face and go .75 inches below the existing face. This creates a .125 extension on both sides of the part. Select the sketcher icon and select the face of the part as shown.




CATIA® V5R6


Exit the sketcher and create a pocket using this sketch and have it go all the way through the part. It should appear similar to the diagram shown below.

Notice that it is not any harder to use part edges and faces to create your sketches. In fact it makes life easier because you do not have to create planes in order to define your sketch plane, you can just use a face of the part. Also your constraints can then be based on the edges of your part and therefore will change if you modify that particular item. However, you must be careful because sometimes that can result in to problems. Now that you understand the basics of part design you will now learn some advanced techniques using the sketcher. Save your document.




CATIA® V5R6

Advanced Sketcher This section discusses the advanced features of sketcher and how they can be used to help you design parts. It will cover how to get 3-D elements from your part onto your sketch plane, use formulas, use construction geometry and use transformations. 3-D Elements on Sketch Plane This part will cover how to get 3-D geometry from your part projected onto the sketch plane. If the geometry is projected properly it will update when the part is modified. An example of this is if an edge of a pad was projected, then that edge was moved due to some modification, the projected elements would also be moved. Projected geometry is especially useful when working with construction geometry covered later in this course. There are two icons that will allow this to happen. Project 3D Elements

projects 3-D geometry to the sketch plane

Intersect 3D Elements

intersects 3-D geometry with the sketch plane

Project 3D Silhouette Edges projects the implied edges of curved 3-D geometry Open the 3D elements document and save with your initials. This part has two planes pre-defined. A blue plane that is parallel to the YZ plane, and a green plane that is parallel to the XY plane. Begin a sketch on the blue plane. This plane is going to have geometry projected to it. Select the project 3-D element icon. Geometry will be projected in two different methods, selecting a face and selecting an edge. Select the face that is shown in the diagram below. The boundary of the face is projected to the plane as geometry.

Notice that the projected geometry is yellow. This means that the geometry is associated to the part. If the part changes then the projected geometry will also change. You have the option of isolating the geometry using the third mouse button while on the geometry.


3-D Elements on Sketch Plane, Page 205


CATIA® V5R6

Select the project 3-D element icon. This time, geometry will be projected in such a manner that it will be updated when the pad is modified. Select the edge that is shown in the diagram below. This time you will only project a single edge to the sketch plane.

Exit the sketch. You will see that the geometry was actually projected to the blue plane as shown below.

Start a sketch on the green plane. This time, geometry will be intersected with the sketch plane instead of projected. Select the intersect 3-D elements icon. sketch plane.


You will intersect the geometry with the



CATIA® V5R6

Select Rear Body from the specification tree. A warning message is displayed. It is telling you that the geometry is not associated with the part and will not be updated when the part is changed.

Select OK. Select intersect 3-D elements icon. the part.

This time, you will intersect selecting a face of

Select a side face of the Stiffener as shown below. This time the geometry is associated with the part, and will change when the part is changed.




CATIA® V5R6

Exit the sketch. The sketch geometry is displayed on the sketch plane as shown in the diagram below.

If geometry is selected that does not intersect the sketch plane, then an error message will be displayed, and nothing will happen.

Save your document.




CATIA® V5R6

Open the 3D elements 2 document and save with your initials. This part has a pulley and a plane pre-defined. The plane is parallel to the zx plane. Begin a sketch on the parallel plane. This plane is going to have geometry projected to it. Select the project 3-D elements icon. of the pulley to the sketch plane.

You are going to try to project the curved edge

Select the curved edge (face) of the pulley as shown below. You will notice only the center line shows up.

Select the undo icon. You were trying to get the curved edge projected not the centerline therefore you are undoing that projection. Select the project 3-D silhouette edges icon. circular edges of a part.

This will allow you to project the

Select the curved edge (face) of the pulley again. The boundary of the face is projected to the plane as geometry. Notice both edges the right and left side were projected to the sketch plane and are associated to the 3-D geometry. Exit the sketcher. It should appear similar to the diagram shown below.

Save your document. © Wichita State University



CATIA® V5R6

Construction Geometry Construction geometry is useful when you need an element to exist in order to constrain your sketch but you do not want that element to be part of your sketch when in part design. This part of the book will use construction geometry, as well as projected 3-D elements to build sketches. Open the construction geometry document and save with your initials. This part has a pad already built for you. Start a sketch on the top face. On this face you are going to sketch a slot that is constrained using construction geometry and projected elements. Project the top face to the sketch plane. This will project the elements, while keeping them associated with the original pad. While the geometry is highlighted, select the construction/standard element icon from the bottom toolbar. This will turn the geometry to construction geometry (geometry that only exists in the sketch plane). The geometry should now be dashed, rather than solid. Project the bottom edge to the sketch plane as shown below. This will complete the construction geometry needed from the existing part. Other construction geometry will be created as needed.

Notice the geometry is already set as construction. The construction/standard icon will stay highlighted until it is selected again. Switch back to a normal view of the sketch plane. Sketch a vertical line down the center of the part. This line will be the center of the part. Notice that the line is construction geometry. Make sure that the line is not highlighted before continuing. Construction Geometry, Page 210



CATIA® V5R6

Select the constraint icon. You are going to constrain the vertical line to be in the center of the other two vertical lines. Select the left vertical line, then the right vertical line and using the third mouse button while on the constraint select Allow symmetry line. Select the center vertical line. This will define the outside lines to be symmetric to the center line forcing the center line to be centered between the two lines. Select the construction/standard element icon. geometry instead of construction geometry.

This allows you to create standard

Sketch a slot on the bottom half of the part as shown below. Remember the slot icon under the rectangle icon.

The center of the slot created is a construction line. That construction line is going to be centered between the bottom two horizontal projected lines.


Construction Geometry, Page 211


CATIA® V5R6

Constrain the center line of the slot to be centered between the bottom two projected horizontal lines. The construction line should turn green, and symmetry symbols should appear. Constrain the slot as shown below using the projected geometry.

Now the slot is completely constrained. You will now create two circles and constrain them with the center vertical line. Create two circles and constrain them as shown below.

Exit the sketch. Using the sketch use pocket to remove the material with the Type set to Up to last. The pocket is now made. Now, when the pad changes, the sketch will modify with it. Change the Length of Pad.1 to 10 inches instead of 6 inches. Notice the slot changed dimensions with the changing of the pad and the two holes stayed 1.25 inches from the center line. You do not see the center line because it is construction geometry and is only seen in the sketcher.




CATIA® V5R6

Change the sketch of Pad.1 to be 7 inches wide instead of 5 inches. Notice that the slot moved to stay centered and the holes moved to stay 1.25 inches from the bottom edge. The part should appear similar to the diagram shown below.

Construction geometry does not always need to be generated. The edges of the part can be used directly from the part. Start a new sketch on the top of the part. This time you are going to create another slot around the current one. You want the new slot to be .25 inches away from the other slot, while the centers of the ends stay in the same place. Sketch a slot in the same place as the other slot, but larger.

Constrain the sketch so that the two curved ends are concentric with the existing slot and that they are .25 inches away from the existing slot. Exit the sketch.




CATIA® V5R6

Using the sketch use pocket to remove the material with the Type set to Up to plane and select the face as shown below. The pocket is now made. Now, when the pad changes, the sketch will modify with it.

Any changes made to the part will be reflected in the slots. Try making modifications to the pad definition, or the original pad sketch and notice how they affect the position of the holes and slots.

Save your document.

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Advanced Constraints This part will cover advanced constraining methods. You will also be using construction geometry to define some of your advanced constraints. Open the advanced constraints document and save with your initials. This document has a pre-defined sketch and constraints. Double click on the Profile Sketch. This will allow you to modify the sketch. Notice the sketch is over constrained.

Press the third mouse button while on the leftmost distance constraint (3.55). This will bring up a menu of options that can be performed on this constraint.




CATIA® V5R6

Select the Offset.19 object option. This will bring up a window with more options.

Select Definition... This will bring up the Constraint Definition window. This option allows you to change the value of the constraint or you can specify that it is a reference dimension only and therefore is not used as a constraint. If this is done then as the sketch is modified, the reference dimension will change as that distance changes but it does not force that distance to be any certain amount.

Select the Reference box and select OK. This will change the constraint to be a reference dimension rather than an actual constraint. Notice that the sketch is perfectly constrained and that the dimension appears in parentheses signifying that it is reference only.

Press the third mouse button while on the constraint next to the reference dimension (1.902). This will bring up a menu of options that can be performed on this constraint.




CATIA® V5R6

Select the Offset.21 object option. This will bring up a window with more options. Select Edit formula. This will bring up the Formula Editor window.

The Formula Editor will allow you to enter a variety of formulas. Simple mathematical formulas to advanced formulas, such as engineering strain equations, can be entered in the Formula Editor. Based on the formula, a value will be calculated. Many times these formulas depend on other constraints in the sketch, so when that constraint is modified, the formulated constraint will automatically recalculate. This class will cover simple formulas but feel free to make them as complex as necessary to get the proper results. Notice that the first box contains the current constraint name and the second box is where the formula is entered. You are going to enter a formula that will make this constraint be half the distance of the reference dimension that you specified earlier. Enter 0.5* in the second box. You are going to make this constraint equal to half of the referenced dimension. In order to specify the referenced dimension you just have to select the value and it will automatically put it in the box for you. Select the referenced dimension (3.55) and select OK. The constraint adjusts, and a f(x) symbol appears next to it. This denotes a formulated constraint, and cannot be modified directly. If the constraint is to be modified, then the formula has to be deleted.

Edit the formula of the bottom constraint (1.372). Use the same process as previously covered. The Formula Editor window should appear. © Wichita State University



CATIA® V5R6

In the Formula Editor window set the constraint to equal the previously formulated constraint and select OK (1.775). This will set the constraint to be exactly the same as the other. Edit the formula on the top constraint (4.369). You are going to make this constraint equal two inches more than the bottom constraint. The Formula Editor window should appear. Select the bottom constraint (1.775). This enters that constraint to be used in the formula. Key +2in after the constraint name in the second box. The (in) is mandatory, otherwise, the system does not know what units you are using. The units used can be any length unit: in, ft, mi, mm, cm, km, etc.

Select OK. The length is now two inches longer than the bottom constraint.

Edit the formula on the radius. You are now going to make the radius equal to 1/3 the value of the bottom constraint. The Formula Editor window should appear. Key 1/3* in the second box. This will make the new constraint be one third of the next constraint you select. Putting the fraction in the parentheses is necessary.




CATIA® V5R6

Select the bottom constraint (1.775). This will make the value of the radius equal one third the length of that constraint. If you were to use a fraction after a value then you need to put the fraction in parentheses in order for it to calculate that value first. Modify the right dimension (2.197) to be twice the length of the dimension just below it (1.354). Notice how some of the constraint changed automatically because they are based of that length.

Modify the bottom unformulated constraint (5.482) to be four times the length of the (1.354) constraint. Change the angle constraint to be 70 degrees. You will not put a formula on the angle constraint. You are now going to animate your last dimension constraint to visualize the formulas in action.

Select the animate constraint icon and select the last unformulated length (1.354). This will bring up the Animate Constraint window.




CATIA® V5R6

Set the First value to 1.0, the Last value to 3.0, and the Number of steps to 40. This will make our constraint animate between 1 and 3 inches, with forty intermediate steps. Select the loop icon from the Animate Constraint window. animation run continuously.

This will make the

Select the forward icon and watch the other dimensions change with the animated constraint. Select Cancel. This will stop the animation of the constraints, and return them back to the original position. Change the 1.354 constraint to be 1.5. Press the third mouse button while on the 1.5 constraint. This will bring up a menu of options that can be performed on this constraint. Select the Length.10 object option. This will bring up a window with more options. Select Display with Leader. This will allow you to display the constraint with a leader arrow. Press and hold the first mouse button while on the 1.5 constraint and drag it out to the right. You see a leader arrow appear similar to the diagram shown below.

You can turn the leader back off by following the same steps but now the option is to Display without Leader. You can also display the name and value instead of just the value of the constraint. You are going to do that now.




CATIA® V5R6

Press the third mouse button while on the 1.5 constraint. This will bring up a menu of options that can be performed on this constraint. Select the Length.10 object option. This will bring up a window with more options. Select Name/Value Display. This will allow you to display the constraint name along with its value. It should appear similar to the diagram shown below.

You can change the display back to just the value by following the same steps but now the option is Value Display. Using similar options you can also Deactivate and Activate the constraint. When you deactivate a constraint a little () symbol appears near the constraint. This exercise will not have you deactivate or activate any constraints but try it out on your own. The last thing you will do with the constraint is to rename it. Press the third mouse button while on the Length.10=1.5 constraint. This will bring up a menu of options that can be performed on this constraint. Select the Length.10 object option. This will bring up a window with more options. Select Rename parameter. This will bring up an Edit Parameter window.




CATIA® V5R6

In the left box change the name to be Lower_Height.

Select OK. Now you can reference that constraint using formulas in another sketch or even in Part Design by using this parameter name. This is an excellent way of building “knowledge” into your design. You will explore some of those options a little later in the course. Exit the sketch, and create a pad 6 inches wide using the sketch.

You do not have to use formulas for every sketch, however, with the use of formulas you can make your sketch easier to modify and you start to add “knowledge” to your geometry. Sometimes formulas are generated automatically when performing actions such as cornering multiple corners at the same time. Save your document.




CATIA® V5R6

Sketch Transformations This part will cover the various transformation icons within the sketcher. There are a variety of options when performing transformations on your sketch. You can symmetry, translate, rotate, scale and offset existing geometry using transformations. symmetry

copies geometry across a symmetry line

translate

moves or copies geometry in a specified direction

rotate

rotates geometry, it can duplicate or replace

scale

scales geometry, it can duplicate or replace

offset

offsets geometry in a normal direction while copying

Open the sketch transformation symmetry document and save with your initials. Symmetry transformations are the most useful of the transformations. Symmetry constraints are built when the transformation is applied, hence, this could be very useful when making a symmetric part of any type. This part has a sketch pre-built. You are going to symmetry the sketch about the given center lines Edit the sketch. The sketch is fully constrained (the constraints are hidden) except for position with two symmetry lines.

Select the symmetry icon. elements about a line.


You will be able to symmetry any number of geometric

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Select the profile. Using the mouse you can select the entire profile by holding down the first mouse button and dragging a box around the profile. This will allow all of the geometry to be selected. For this exercise, it is not necessary to select all the geometry at the same time, but when working with a more complex document, it may be desirable to select many elements at the same time. When selecting the profile be careful not to select geometry that crosses the mirror line because this can cause an artificial edge to be generated when you use this sketch in part design. Select the vertical construction line. This will define the mirror line. The geometry is duplicated on the other side of the symmetry line. Notice the symmetry symbols on both profiles. These elements are now linked to one another and when the left profile is changed, the right profile will change also.

If you want you can symmetry both profile across the horizontal construction line. Note: The symmetry line does not have to be a construction line. The line can be standard or construction. Also, the geometry that you are using can be selected either before or after selecting the icon. Feel free to show the constraints and change them to visualize the symmetry working. Exit the sketch. Save your document.




CATIA® V5R6

Open the sketch transformation translate offset document and save with your initials. This is another document with a pre-defined sketch. This sketch is to have translations and offsets applied to it. Edit the sketch. Select the translate icon.

This will allow geometry to be translated.

Duplicate Instance(s)

defines how many instances will be created, only applies in Duplicate mode

Duplicate mode

duplicates the geometry when translated

Conservation of the constraints

reproduces similar constraints on the translated profile when in Duplicate mode

Length Value

defines the length of the translation

Snap Mode

forces the length to snap to the grid defined in your sketcher

Translations work in three steps. First you define what is to be translated, then you select the reference point, and then define a destination point. Select the spline. A blue cursor will appear. This means that it is ready for you to select the reference point. Select the point closest to the axis. This defines the point that is to be translated. This point can be on the geometric element but it does not have to be. The next point can either be at an exact location, or just an arbitrary location. To obtain an exact distance, key a distance in the Translation Definition window, or another known point can be selected.




CATIA® V5R6

Select about six inches above and to the right of the current spline. This will create a new, duplicated spline. Notice no special constraints are added. Select the undo icon. Translate the spline again this time using the Conservation of the constraints option. Notice that constraints were automatically generated on the new spline similar to the ones that were on the original spline. Select the undo icon. You may want to try out the various options to make sure you have a good understanding of them. These options are available when using some of the other transformations as well. Select the offset icon. There are many sub-options that appear when defining an offset, they are explained below. Once you specify the element the options appear and you can define an offset by either just selecting a location or by specifying a distance in the Offset area.

offsets a single element offsets the element selected and propagates along any tangencies offsets the element selected and propagates along any connected geometry will perform a double offset and can be used in conjunction with any of the other three options Make sure the single element icon is selected with double offset being off and select the spline. This defines what is to be offset. Select just above the spline. This creates a spline offset, parallel, to the original. You will now use the other profile and try out the other options of offsetting.




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The rest of this exercise uses the other profile found in this sketch as shown below.

You are going to do a series of offsets using different options each time and then undoing them. Select the offset icon. Select the single element icon. Select the top line and select a location above it. Only that line gets offset.

Select the undo icon.




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Select the tangency propagation icon. This will grab all elements that are continuous in tangency to the selected element. Select the top line and select a location above it. Notice that the curve and other line were offset as well because they were tangency continuous to the selected element.

Select the undo icon. Select the point propagation icon. with the selected element.

This will grab all elements that are connected

Select the top line and select a location above it. Notice that the entire profile was selected since it is a closed profile and all of the geometry is connected to the selected element through points.

Select the undo icon.




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Select the double offset icon. This will allow the geometry to be offset in both directions at the same time. The point propagation icon should still be activated. Select the top line and select a location above it. Notice that the entire profile was offset in both directions.

If a red symbol appears when you are trying to select your offset location you cannot select there because it violates a dimension. This is common when offsetting a circle inward and you try to offset it beyond the radius of the circle. Hopefully this gives you a good idea what each option allows you to do. Save your document.




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Open the sketch transformation rotate document and save with your initials. This document also has a pre-defined sketch. In the sketch there is a keyhole that needs to be rotated about the center multiple times. Edit the sketch. Select the rotate icon. The rotate option is a four step process. You must define the geometry to be rotated, a point of rotation, a reference line and then an angle. You may also define a starting point and ending point to determine the angle instead of defining a reference line and an angle.

The various options are the same as translate except you can define an angle instead of a length. Select all of the keyhole. This can either be accomplished by holding Ctrl and selecting the geometry, or by selecting and dragging a box around the keyhole. Change the number of Instance(s) to 5, make sure Duplicate mode is on and Conservation of the constraints is off. This will make five duplicates of the keyhole at equal distances around the rotation axis. You now have to define the rotation point or the center of the rotation. Select in the center of the sketch. This will define the point that you want the geometry to rotate around. Instead of defining a reference line and then an angle you are going to define a starting point of the angle and then the ending point of the angle. Select the outside corner just below the keyhole. This defines the beginning of the angle.




CATIA® V5R6

Select the outside corner just above the keyhole. Notice the five keyholes fan out as the cursor is moved towards the second corner. This defines the end of the angle.

There should be a total of six keyholes evenly spaced about the center of the part. Notice there are no constraints on any of the other keyholes. Be sure no elements are selected before the next step. Select the scale icon.

This will allow you to scale geometry larger or smaller.

The options are the same as translate except you specify a value for the scale instead of a length. Make sure the Duplicate mode is off. Select all of the sketch. Next, a scale point will need to be defined.




CATIA® V5R6

Select in the center of the HV axis. The part will now be scaled about this point. Change the Value to be 1.5 and select OK. This will scale the sketch to be one and a half times its original size. Save your document.




CATIA® V5R6

Sketch Analysis Open the sketch analysis document and save with your initials. This document also has a pre-defined sketch. Select the pad icon and select the sketch. A Feature Definition Error window appears, stating that your sketch has points that are standard geometry and they need to be construction geometry.

Select No. This will close the error window. Deactivate the pad icon. This gets out of the pad creation mode. Edit the sketch. You will now correct the problem using the Sketch Analysis option under the Tools pull down menu. Select Sketch Analysis under the Tools pull down menu. This will run a sketch analysis on your sketch and display a window with the results as shown below.




CATIA® V5R6

If you have a good sketch then there should only be closed profiles under Detailed Information. As you can see there is an open profile, an isolated line and an isolated point. The error message you received earlier gave you an idea that there was a problem with a point but that was it. You should notice three icons under Corrective Actions, these icons allow you to quickly fix your sketch and are described below. changes the geometry to construction geometry closes the open sections of a profile erases the geometry In this case you will change the point to construction geometry. Select Point.22 in the Sketch Analysis window. Select the construction geometry icon in the window. Notice that the point disappears from the Sketch Analysis window because it is no longer considered to be a problem. Select Close. This will exit the Sketch Analysis window. You will now try to make a pad out of this sketch again even though the sketch analysis still shows some problems. Exit the sketcher. Try to create a pad with the sketch. Another Feature Definition Error window appears as shown below.

Notice that this error message now tells you that you have open contours (profiles) or some geometry that needs to be construction geometry instead of standard. You will now go back in to your sketch and correct those problems using the sketch analysis tool. Select No. This will close the error window. Deactivate the pad icon. This gets out of the pad creation mode. Edit the sketch. You will now correct the problem using the Sketch Analysis option under the Tools pull down menu. Select Sketch Analysis under the Tools pull down menu. This will run a sketch analysis on your sketch again.




CATIA® V5R6

Select Line.6 from the Sketch Analysis window. Select the construction geometry icon. The line disappears from the window because it is no longer considered to be a problem. Notice that the center line has changed to construction geometry, that was Line.6. You still have an open profile that needs to be closed. If you look at the lower right corner you will see that is where the problem is located. Select the open profile in the window. Select the close icon. This will close the profile changing the status to closed as shown in the window.

Note: You need to be careful using the close option because if you have two lines that have a break in between them and you close the profile it will just trim one of the lines to the other. What you would want to do is erase one of the lines and then trim the other one, otherwise you generate a false edge on your pad. You are now ready to create the pad. Select Close. This will close the Sketch Analysis window. Exit the sketcher and create a 1 inch pad using the sketch. Save your document.




CATIA® V5R6





CATIA® V5R6

Advanced Part Design Part Transformations This section will cover how to perform transformations on your part. The available transformations are translate, rotate, symmetry, mirror and scale. These icons can be very useful for increasing your efficiency in your part design. The icons are explained below. translates your part a specified direction and distance without copying rotates your part around a specified axis and angle without copying mirrors your part around a specified plane without copying mirrors an object or list of objects around a specified plane while copying scales your part based off a reference point and specified scale Note: It is important to remember that all of these options other than the mirror option work on the entire part from current position in the specification tree on up. Open the transformations document and save with your initials. This part has been pre-created for you. This section will translate, rotate, symmetry, mirror, and scale this part. Select the translation icon. This will allow a part to be translated along a selected direction. The Translation Definition window appears. You have to define a Direction and a Distance.


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Select the lower straight edge of part as shown below. By selecting an edge of your part, you define a direction for the translation.

A green symbol will appear on your part with two arrows. If you wanted to you could select one of those arrows and drag it to define the translation otherwise you can key in a specific distance in the window. Change the Distance to 2.0. The distance is measured in the positive direction of the edge. Select OK. The part is now translated two inches to the left. A Translate branch appears in your specification tree. Now you will rotate the part. Select the rotate icon. This will allow the part to be rotated about any given axis, a given angle. The Rotate Definition window appears. You have to define an Axis and an Angle.

Select the same edge of the part. This defines the rotation axis. The part will rotate about this line, positive direction being clockwise. Once again a green symbol appears with two arrows. You can define the rotation using these arrows or key in a specific angle. Change the Angle to be 270. This will change the part to be vertical. The alternative to 270 degrees would be -90 degrees. Select OK. The part is now rotated 270 degrees about the axis selected. A Rotate branch appears in your specification tree. Next, you will symmetry the part along the open face to make a right-handed part versus a left handed part.




CATIA® V5R6

Select the symmetry icon. This will allow symmetrical parts to be made about any given face or plane, while not keeping the original part. The Symmetry Definition window appears. You have to define a Reference element for the part to mirrored across.

Select the open face as shown below. The symmetry side of the part is displayed as wireframe, giving a preview of the part that is going to be created.

Select OK. The part is now a mirror image of the original part. A Symmetry branch appears in your specification tree. This is useful for making left handed parts out of right handed parts or vice versa. Delete the three previous transformations. The part returns back to the original position. You are now going to mirror some of the geometry about a mirror plane. The difference between mirror and symmetry is that mirror will duplicate the geometry. The other difference with mirror is that it can be applied to a specific object or list of objects in the tree instead of to the whole body. If you want the mirror option to use something other than the entire body you must select those objects before selecting the mirror icon. Select Pad.1 from the specification tree. It will use just this object when mirroring.




CATIA® V5R6

Select the mirror icon. This will allow for the object to be mirrored, while keeping the original object. The Mirror Definition window appears.

Select the face shown below as the Mirroring element. This will mirror the pad across this face.

Select OK. The part has been mirrored making a closed loop. Notice only the pad was mirrored and not the pockets. Normally in this case you would probably of wanted the pockets as well but this is just an exercise. From here, holes, slots and other manipulations can be made to the part as though it was created as one piece. Select the scaling icon. You can scale the part about any given plane or any point. Scaling about a plane will only make the scale ratio effect the part in the normal direction of the plane. Scaling about a point will make the entire part scale about that point. The Scaling Definition window appears. You have to define a Reference element and a Ratio.




CATIA® V5R6

Select the point in the center of the three axis planes. This will define the point about which the part will be scaled. Notice the green symbol with the arrows. You can adjust the scale using them or you can specify a ratio in the window. Change the Ratio to 2.0. A wireframe model is displayed showing a preview. Select OK. The part is now scaled to twice its original size. A Scaling branch appears in the specification tree.

Note: It is important to remember that the placement of the transformations in the specification tree can drastically effect the results. Save your document.




CATIA® V5R6

Patterns In this section patterns will be applied to different holes and pockets on a part. Patterns are also useful to quickly replicate any type of sketch across a part in a variety of ways. creates a rectangular pattern

The First Direction and Second Direction tabs have the same options. Parameters

There are three options for which parameters you are going to use to create the rectangular pattern. They are Instance(s) & Spacing, Instance(s) & Length and Spacing & Length.

Instance(s)

the number of items you want the pattern to have in that direction

Spacing

the distance between each instance

Length

the total length of the pattern in that direction

Reference Direction Reference element

the element that specifies the direction for the pattern

Reverse

reverses the reference direction

Object to Pattern Object

the item that is to be used when creating the pattern

Keep specifications

keeps the specifications of the object, such as Up to next.

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Position of Object in Pattern Row in direction 1

the row where the original element should exist

Row in direction 2

the row where the original element should exist

Rotation angle

the angle of the pattern in reference to the original element

Pattern Representation Simplified representation

allows you to specify which elements of the pattern you wish not to see in order to speed up response time when dealing with large patterns

The circular pattern has similar options under More>>, but they deal with angular and radial directions instead of first and second. Patterns can use either the entire part, a single object of the part or multiple objects of the part. If you want to use multiple objects you need to select them before you select the icon.


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creates a circular pattern Some options are the same as the rectangular pattern so they will not be covered again.

Axial Reference Parameters

There are four options for which parameters you are going to use to create the circular pattern. They are Instance(s) & angular spacing, Instance(s) & total angle, Angular spacing & total angle and Complete crown.

Instance(s)

the number of items you want the pattern to have in each circle

Angular spacing

the space between instances measured in degrees

Total angle

the total span that the pattern should be defined in

Crown Definition Parameters

There are three options for which parameters you are going to use to create the circular pattern. They are Circle(s) & circle spacing, Circle(s) & crown thickness and Circle spacing & crown thickness.

Circle(s)

how many circles should be used in the pattern

Circle spacing

the distance between each circle

Crown thickness

the total distance between the first and last circle

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creates a user defined pattern

Instances Positions

the sketch that is used to define the positions of the instances

Object to Pattern Anchor

defines how the pattern is positioned with respect to the original object

The following exercise will explore the various pattern definitions to create pegs and holes. Open the patterns document and save with your initials. This part has several holes in it as well as a square pocket that will be distributed throughout the part using patterns. Select the rectangular pattern icon. selected item or the entire part.


This will generate rectangular patterns using a

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Select the Peg. The peg can either be selected off of the tree, or from the part. The Rectangular Pattern Definition window appears.

There are two directions that can be specified when creating a rectangular pattern. They are the First Direction and the Second Direction. When a Reference element is selected, a 1 and 2 vector will be displayed. The vectors can be reversed by selecting the Reverse button in the window. Select the Reference element box in the window. The box will highlight. In order to create a pattern the Reference element has to be defined. Depending on what element is selected, the pattern will be defined in different ways. Select the bottom pocket face as shown below. This defines the face that will be the reference for the pattern. This also defines the positive direction for the 1 and 2 vector, these directions are the H and V axis directions of the sketch of the object that contains that face.

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In the First Direction tab the following options need to be set: Parameters needs to be Instance(s) & Spacing, Instance(s) needs to be 3 and Spacing needs to be 2 inches. This defines that in the first direction there should be 3 pegs with 2 inches between each one. In the Second Direction tab the following options need to be set: Parameters needs to be Spacing & Length, Spacing needs to be 1.5 inches and Length needs to be 4 inches. This defines that in the second direction the pegs should use 4 inches of space with 1.5 inches between the pegs. This will create as many instances as necessary in order to not exceed a total length of 4 inches with 1.5 inches between each peg, which ends up defining three rows. Select OK. A square pattern of nine pegs have now been created. It should appear similar to the diagram shown below.

Next, the same type of pattern will be created, but this time it will be skewed to fit in the other end of the part. Select the rectangular pattern icon. Select the Large Hole. This defines the object that is to be used for the pattern. Select the Reference element box in the window. Select the same bottom pocket face. This will define the reference for the pattern. This time the same pattern that was used before is displayed. The pattern is in the wrong direction and not slanted. Select the Reverse button for the First Direction. This will make the 1 vector reversed bringing the holes back to the part. Select the More>> button. This will bring up additional options for your pattern. You will change the Rotation angle so that the pattern will fit in between the sides of the part. Change the Rotation angle to -15. This will rotate the pattern negative fifteen degrees. Now the pattern lines up nicely with the tab. © Wichita State University

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Select OK. The pattern is created and set in place at the angle you designated. It should appear similar to the diagram shown below.

Save your document.

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Next a circular pattern will be created with the smaller hole in the center. Select the circular pattern icon. This allows you to create a circular pattern. Circular patterns work similar to rectangular patterns in that they can be defined in two directions. With circular patterns, they are defined using an Axial Reference and a Crown Definition. The Axial Reference defines how many times the holes are repeated around the axis as well as the spacing of the holes as they rotate around the axis. The Crown Definition defines how many holes there are in the radial direction. Select the Center Hole. This can be selected from the tree or by selecting the part. The Circular Pattern Definition window should appear.

Select the Reference element box in the window. As with the rectangular pattern, a reference element still has to be defined. Select the bottom pocket face. This will display the wireframe holes before they are created. This will use the origin of the sketch of the object that contains that face as the center of the circular pattern. In the Axial Reference tab the following options need to be set: Parameters needs to be Complete crown and the Instance(s) needs to be 8. This will have the pattern generate in a complete circle using eight holes equally spaced. In the Crown Definition tab the following options need to be set: Parameters needs to be Circle(s) & circle spacing, Circle(s) needs to be 3 and Circle spacing needs to be 1.25 inches. This will force the pattern to used 3 circles with 1.25 inches between each circle.


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Select OK. This finishes the pattern definition. It should appear similar to the diagram shown below.

Save your document. There are times when holes, cutouts, or other geometry need to appear in a pattern that is neither rectangular or circular. The user pattern icon is useful because it allows you to define your pattern using a sketch of points. The item that is used for the pattern will be centered on each point. Select the user pattern icon. sketch of points.

The pattern can now be defined by a user defined

Select the Square Cutout. This defines the object that will be used in the pattern. Select the Flange Sketch. This is a sketch of points that are constrained to define the center of the square cutout at various locations.

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Select OK. This will create square cutouts at all the locations of the pattern. It should appear similar to the diagram shown below.

By defining a series of points any type of pattern can be created, not just rectangular or circular. If you wanted to use a sketch but not use all of the points in the sketch you have the option of selecting the points after you have selected the sketch to remove them from the pattern. The other advantage of using a user defined pattern is that adding or removing elements of the pattern is as easy as creating or deleting a point from the sketch that was used. There are situations that occur when you need to change the size of one of the elements in the pattern but not all of the elements in the pattern. The options you have are to redefine the pattern and then add the additional element or to explode your pattern. Exploding your pattern will cause each element in the pattern to be generated as an individual element. You are going to do this now. Using the third mouse button select on RectPattern.1. This will open a window with various options on it.


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Select the RectPattern.1 object at the bottom of the window. A new window should appear similar to the one shown below.

Select Explode. Notice a whole bunch of pegs appear in your specification tree and your part needs to be updated. These pegs are the result of CATIA creating a new pad for element in the rectangular pattern. Select the update icon. Your part should update. Now that each peg is independent you can change just one of them. Save your document.

Patterns, Page 252



CATIA® V5R6

Modifying Parts Many times it is necessary to modify parts after they have been finished. This is usually the case for many production parts as they go through the manufacturing process. The following documents will have multiple modifications made to the part operations themselves, not the sketches. Modification of the sketches was covered earlier in the book along with making basic changes to the parameters of parts. You can modify the constraints of a sketch when you are modifying the object that is using the sketch. As you will see when you double click on an object the sketch constraints of that object will appear on the screen and you can double click on them to change their values without having to go in to the sketch. These exercises will have you make some basic changes along with some more involved changes to a part. Open the modify4 document and save with your initials. This part has several different types of operations applied. You will make several modifications to this part. Change the Length of the Main Body to be 4 inches. This will change the height of the Main Body to 4 inches instead of 3 inches. Notice the slot no longer cuts all the way through the part. Change the slot to go all the way through the main body. The disadvantage of using a dimension value to define a pocket is that if your part changes the dimension value does not automatically change. Whereas using the other options the length of the pocket is defined by an element or a side of the part. Therefore when you change the part the pocket will automatically adjust to the those changes in most cases. It is suggested that you change the limit Type of the pocket instead of just increasing the value of the dimension. Change the Length of the Back Mount 1 to be 1 inch. This will change the pad definition to be 1 inch tall. Change the Small Hole Definition to have a .625 inch Diameter. This changes the diameter of all the holes in the part. The hole pattern also needs to be changed to add three more rows of holes to the part. Change the Small Hole Pattern to have 7 Instances. The hole pattern now has seven rows of holes instead of four. Next, the hook slot will be changed so that it is parallel to the main body instead of at an angle.


Modifying Parts, Page 253


CATIA® V5R6

Change the Second Angle of the Hook Base to be 90 degrees. The Hook Base, Hook Top, and Hook Web all change with respect to the new angle. Next, the Hook Web will be changed to be thicker. Change the Hook Web to have a Thickness of .375 inches. The web thickness is now .75 (.375 mirrored) instead of .5 in. All of those changes were just a matter of modifying the parameters of the various elements. You can also insert new objects into your tree by defining which object is the Work Object and then the next operation will occur right after that object. The object that is underlined in the tree is the Work Object. You are going to insert a new pad in your part right after the Back Mount 1 object. Select the third mouse button while on the Back Mount 1 object. An options panel will display.

Select the Define In Work Object option. This will display the part back to the point that it was at when the Back Mount 1 pad was made. This can be done at any point in the tree. This is very useful when wanting to go back and add to the part.




CATIA® V5R6

Create a sketch on the bottom of the part. A rectangular mounting plate is going to be added to the front of the part. Create and constrain the sketch as shown below.

Create a pad that is .75 inches thick using the sketch. The pad should go from the botton of the part up .75 inches so you need to make sure your direction is correct. This adds the pad into the part just after the Back Mount 1. Notice that the new pad is underlined because it is the Work Object, therefore your part only displays what has occurred up to that point. You will change the Work Object so that it will display the entire part taking in to account all the operations. Change the PartBody to be the Work Object. You do this the same way as you did before using the third mouse button. This will show all the part operations that have been applied to the PartBody. Now you will add fillets to the new pad. Double Select on the Fillets. The Edge Fillet Definition window displays. However instead of changing the size of the fillets you are going to add additional edges to your fillet operation.




CATIA® V5R6

Where the new pad is located, select all the edges next to the Main Body and those along the top of the pad. The diagram shown below will show you which edges on one side of the part except for the hidden edge. You will need to select those same edges on the other side. In the end, you should have selected an additional 16 edges, 8 on each side, making a total of 58 edges selected. You can also remove edges from your fillet definition by selecting edges that have already been defined.

Select OK. The new fillets are now added in. It should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

You can also change the properties of your objects or of the whole body. You will continue working with this part and change some of the graphic properties of your part along with renaming your part body. Select the third mouse button while on PartBody. This brings up the options panel. You will be changing the properties of the body. Select Properties from the window. This opens a new window similar to the one shown below. You will change the name of the body first and then some of the graphic properties.

Select the Feature Properties tab. You will see a Name box and you can change the name by changing the text in the box. Change the name from PartBody to Finished. The name should change but until you select OK or Apply it will not appear in the tree. Select Apply. The name changes in the tree.




CATIA® V5R6

Select the Graphic tab. The window should change to look similar to the one shown below.

Change the Weight of the Edges to be 1. This will make the edges of your part appear thinner. This will not take effect until you select Apply. When changing color you can select the down arrow and a little window will appear with various colors. You have the option of selecting one of those colors or you can select the More colors... option at the bottom of the list. Select Color arrow under Fill. This will allow you to change the color of the faces of the part opposed to just the edges. A color list will appear similar to the one shown below.




CATIA® V5R6

Select the More Colors option. You may have to scroll down in order to see the More Colors option. Another window opens with color options.

You can select a color from the Basic Colors or you can select a color from the Custom Colors. Custom Colors are ones that you create using the Define Custom Colors >> option. You are going to create a Custom Color and then Apply it to your part body. Select the Define Custom Colors >> option. The window changes to appear similar to the one shown below.

You can define a color by selecting in the color span or you can adjust the values for the various options. When you get a color that you like you can add it the Custom Colors by selecting Add to Custom Colors.




CATIA® V5R6

Create a color of your choice and select Add to Custom Colors. The color appears in the Custom Colors. Select the color you just added and select OK. This takes you back to the original properties window. Select OK. This applies and accepts the settings for the part body.

Save your document.




CATIA® V5R6

In this exercise you will learn how to replace a sketch with another sketch and how to change the sketch support for a sketch. This allows you to make a complete change to the shape of an object without having to create a new object and then inserting it in the correct location and then removing the old object. Open the modify5 document and save with your initials. The slot that has already been created in the part needs to be curved instead of straight across. Instead of going in and modifying the sketch you will create a new sketch and then replace the current one with the new one.

Create the sketch on the face as shown above and constrain it as shown below. You have to be careful not to constrain your sketch using elements that do not get generated until after the sketch you are replacing.




CATIA® V5R6

Exit the sketcher. You will now replace Sketch.3 with your new sketch. Press the third mouse button while on Sketch.3 and select Replace. The Replace window appears as shown below.

You have the option of checking the Delete replaced elements and exclusive parents box if you want the item you are replacing deleted instead of moved to the bottom of the tree. Select the Delete replaced elements and exclusive parents option. This will erase Sketch.3 when it is replaced by your new sketch. Select your new sketch from the tree and select OK. Notice that the slot changed to be curved instead of straight across. If you look in the tree you can see that your new sketch is located where Sketch.3 used to be. The part should look similar to the one shown below.

After replacing that sketch you realized that you do not need the slot to go through the front wall just the back wall. Unfortunately you created that sketch using the front face as the sketch support. You could modify Pocket.1 to use different faces for its limits or another option is to change the sketch support for that sketch. You are going to change the sketch support to be the front face of the back wall instead of the front face of the front wall.




CATIA® V5R6

Press the third mouse button while on the sketch of Pocket.1. You will select the bottom option which is the name of the sketch and then select the Change sketch support option from the new window. The current sketch support appears highlighted. You will now select the new sketch support. Select the front face of the back wall as shown in the diagram below.

Notice that the slot appears only in the back wall. The parameters of the pocket did not change, it is still Up to last. The only difference is that the sketch now belongs on the front face of the back wall. You can also cut, copy and paste elements on your part. After much discussion with your team, they decide that the front extension needs two holes in order for the part to be bolted down more securely. You want the same size hole therefore instead of recreating the hole you are going to just copy and paste the hole. Select the third mouse button while on Hole.3 and select Copy. Nothing appears to happen but it did copy the hole. While having the cursor on the PartBody in your tree, press the third mouse button and select Paste. This will paste the hole you copied earlier at the end of the tree. An Update Diagnosis window appears because the hole is pasted right on top of the hole you copied. Once you change the location of the hole the update will work fine.




CATIA® V5R6

Select Close. Edit the sketch of Hole.4. You are going to constrain the sketch so that the hole is located at a different position. Constrain the sketch of the hole as it appears below.

Notice that the center of the hole was constrained to be equidistant between the two lines and then one inch from the left edge. Exit the sketcher and the part will update with the change.

Sometimes it is necessary to reorder the elements in your specification tree because you need one element before the other for constraint purposes or to have an operation occur or not occur on additional objects, such as when using transformations. In this exercise you are going to reorder Hole.2 to be before Hole.1 in the specification tree.




CATIA® V5R6

Select the third mouse button while on Hole.2. You will select the bottom option which is the name of the hole and then select the Reorder option from the new window. This will open the Feature Reorder window which will allow you to specify after which object you would like Hole.2 to go.

Select Pocket.1 from the specification tree. Select OK. This puts Hole.2 after the pocket and before Hole.1. Another option you have available to you is to scan through the tree looking at the various stages of your part design. Select the pull down menu Edit and select Scan or Define In Work Object. This will open a Scan window that will allow you to run through your specification tree.

Press the forward button continuously until you go all way through your tree. This is a good way to walk through a part design to get a better understanding of the method of creation when you were not the one who created the initial part. These exercises were to demonstrate various options that you have when modifying your parts. A lot of them depend on how you constrained your part in the first place. You want to make sure you pre-plan your approach before you start designing your parts in order to make it easy to modify. Save your document.




CATIA® V5R6

Inserting Bodies and Boolean Operations Since there are some operations that affect the whole part body, there are times when it is necessary to use multiple part bodies in your part. In order to generate a part that is composed of one main body it is necessary to use boolean operations to combine the various bodies of the part. The disadvantage to using multiple bodies is that you can not perform some operations across bodies unless they have been combined. This exercise will have you insert bodies and then use boolean operations to combine the bodies into a single element. Inserting Part Bodies Open the assembly document and save with your initials. This document has several bodies in it. They will all be combined into one body using various boolean operations to build the part. Select the pull down menu Insert and select Body. This allows you to insert a new body into the part. The body gets inserted at the bottom of the specification tree, you may have to scroll down in order to see it. You should notice that it is the current in work object since it is underlined. Create a sketch on the zx plane, constrained as shown below.

These two circles will be used to create two pegs in the part. Pad the sketch 6 inches in the first direction and .25 inches in the second direction. Two pegs are now created completely through the part. This part is constructed in a common fashion as Version 4 solids were modeled. Every object is a separate body and then boolean operations are used to combine them in a variety of ways. The next page discusses the different options that are available to combine your multiple bodies into a single body.

Inserting Bodies and Boolean Operations, Page 266



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Boolean operations Assemble

similar to Add but will add or remove material depending on the objects in the body, most useful to add pockets and holes to other prejoined bodies

Add

adds one body with another body

Remove

removes one body from another body

Intersect

keeps the common material between two bodies

Union Trim

adds several bodies together while allowing multiple faces to be removed or trimmed back to the combined part

Remove Lump

removes a separated piece of the part, normally you can avoid using this option by modifying your sketch or adjusting part bodies

You are going to start combining the bodies of the part together using the boolean operations. The exercise will cover a few options for selecting the boolean options. You are going to start by adding the Front Body with the Main Body. Select the Front Body from the tree. This will define what body you are going to be working on. Select the pull down menu Insert, Boolean Operations, Add. This will tell the system that the Front Body will be added to another body.

Select in the After box and select the Main Body from the tree. This will define the body that the Front Body will be added to. Select OK. The two parts now act and behave as a single part. Notice how the bodies appear in the tree. The Front Body appears underneath an Add.1 branch which is under the Main Body now. Select Body.9 from the tree. This is the body created earlier. You may have to scroll down in order to see it. You are going to add this to the Side Holes. Press the third mouse button while on Body.9 and select Body.9 object, Add. This is another way to select boolean operations. You can use either option to select the boolean operation, both ways work the same way. The advantage of using the third mouse button is that you do not have to go up to the top and select a pull down menu.




CATIA® V5R6

Select in the After box and select Side Holes and select OK. This will define where Body.9 will be added. The two bodies are now added together as one. Next you are going to remove the holes from the Main Body. Select the object Side Holes. Notice all five holes are highlighted. Select the boolean operation Remove. You can use either of the previous methods to select the operation. Select in the After box and select the Main Body and then select OK. The holes are now removed from the Main Body. You will use the Assemble operation to add the Lg Hole to the Main Body. Select the object Lg Hole. This hole will be assembled to the Main Body. Select the boolean operation Assemble. Select in the After box and select the Main Body and then select OK. Notice the hole was removed from the Main Body. Since the Lg Hole was defined as a pocket, the pocket was placed in the tree, and was then pocketed out as though it were defined on a single body. If you would have used the Add operation then the pocket would not have been removed it would of just been added to the Main Body. Next, a more advanced type of boolean operation will be performed. Make the Rear Guide Tubes the current object. You can do this by using the Define In Work Object option using the third button of the mouse. Select the object Stiffener for Tubes. You are going to union (add) this body with the tubes but you are going to trim back the inside edges to the tube walls. Select the boolean operation Union Trim. This will allow the part to be unioned (added) with the tubes and have faces trimmed back in the same operation.

Select the Faces to remove box. This is where you can define the faces that you want removed when the body is unioned.




CATIA® V5R6

Select the faces of the stiffener that are inside the tubes. You’ll probably have to zoom in and rotate the part to select the faces on the inside of the tubes. The diagram shows the faces that you need to select.

Select OK. The stiffener will now be trimmed back to the tubes, and then unioned to the tubes. Next, the Rear Guide Tubes will be unioned and trimmed with the Main Body. Make the Main Body the current object. Select the boolean operation Union Trim on the Rear Guide Tubes. Select the Faces to remove box and select the faces of the Main Body that are inside the tubes. Again, this will define what is going to be removed when the tubes are unioned to the Main Body. The diagram shows you which faces to select.




CATIA® V5R6

Select OK. Now the tubes are unioned to the Main Body. To finish the part you are going to intersect the Contour body with the Main Body. You will not see the Contour body because it is hidden at the moment. If you want to see the Contour before you intersect it then you can show it. Select the boolean operation Intersect on the Contour. The Intersect window appears. Select OK. The Contour is intersected with the Main Body since it is the current work object. You are now finished with the part. It should look similar to the one shown below.

Save your document.




CATIA® V5R6

Part Design Lofts This section will cover two ways to generate a part using multiple sketches using the loft icons. Open the loft create document and save with your initials. This document has several sketches that contain circles and ovals. These sketches will be used to define the contour of your part. Select the loft icon. This will allow multiple contours as well as guide and spine curves to be utilized in a single part. Guide curves and spines will not be used here. Creating such curves will be covered in the Wireframe and Surfaces Class.

Select Curve 1 from the tree. This will define the first profile of the part. Select Curve 2 through Curve 5 in order. This will finish the definition of the part. The section curves are not limited to just round or circular curves. They can be of any profile shape desired. Note the arrows along the right side of each section curve. These arrows must be along the same side of the curves and they also must be pointing in the same direction. If they are not then the result will be a twisted part. Select OK. A part is created that passes through each of the section curves defined in the order that you selected them. In the specification tree you should notice the loft branch added and underneath that branch is all of the sketches that were used to create this loft. You can modify those sketches at any time and the loft will automatically update.


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Shell the part with an Outside thickness of .25 inches and an Inside thickness of 0 inches while removing the two ends. This will turn the part into a tube with the inside passing through the sketches defined. It should appear similar to the diagram shown below.

Save your document. Open the loft remove document and save with your initials. This exercise uses the same set of curves. The difference is, this time the loft will be removed from the cylindrical pad. Select the loft remove icon. This will create the loft as before, and then automatically remove it as though it were a pocket. Select Curve 1 through Curve 5 in order and select OK. The loft is created and then removed.

Save your document.

Part Design Lofts, Page 272



CATIA® V5R6

Part Design Using Surfaces The next couple of exercises will utilize surfaces to generate parts. The surfaces will be provided for you. If you wish to learn about building surfaces, they will be covered in the Wireframe and Surfaces class. The thing to remember is that you are capable of integrating surfaces in to your part design. In doing so, you are able to make modifications to the surfaces that are used and the part will automatically update. Even though this course only covers the use of surfaces to a small degree be aware that it is extremely important that you understand how to integrate surfaces in to your part design if you want to be able to create specific contoured parts. Open the sew & split surface document and save with your initials. This part has two surfaces. The part is going to be split with the top surface and the bottom surface is going to be sewn in. Select the split icon.

This will split a part with any given surface or plane.

Select the top surface. This will display an arrow on the surface, and the Split Definition window will appear.

Make sure the arrow points towards the part. The direction the arrow is pointing is what is kept in the split operation. Select OK. The part now has the contour of the surface. Hide the top surface. This shows the top contour much better. Next, the bottom surface will be sewn into the part.


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Select sew surface icon. When the four sides of a surface come in contact with a part and the sew operation is used, the area between the surface and the part gets filled in. Select the bottom surface. The Sew Surface Definition window appears and again an arrow is displayed on the surface.

Make sure the arrow points towards the part and select OK. The area between the surface and the part is now filled in. Hide the bottom surface. These options are very useful if a specialized contour is needed on a part. It should appear similar to the diagram shown below.

Save your document.




CATIA® V5R6

Open the thick surface document and save with your initials. This document has a single surface in a circular shape. Select the thick surface icon. surface.

This will allow a thickness to be added to a face or a

Select the surface. The Thick Surface Definition window appears. An arrow will be displayed on the surface indicating the direction of the First Offset.

Make the First Offset 1 inch and the Second Offset .5 inches. This will make the total pad 1.5 inches thick. Select OK. The surface has the thickness applied and a part is created. Select the thickness surface icon again. This time the end of the part will have a thickness added. Select the face on the end of the newly created part as shown below.

Change the First Offset to 5 inches and the Second Offset to 0 inches and make sure the arrow points away from the thickness. Select OK. The side of this part has now been extended (thickened) linearly by five inches. It is important to note that the thickness is applied linearly instead of following the tangency of the part. Even though you applied the thickness to the end of the part it still added the thickness straight out ignoring the fact that the part is curved going to that end. This happens because it is adding the thickness in the normal direction of the selected face. Therefore, if you add thickness to a curved side then it will add thickness in the normal direction to the curved surface. Save your document. © Wichita State University



CATIA® V5R6

Open the close surface document and save with your initials. This document has one surface in the shape of an airfoil. The surface is completely wrapped around, but is open on each end.

Select the close surface icon. solid part.

This will allow closed surfaces to be enclosed with a

Select the Airfoil Surface. The Close Surface Definition window appears.

Select OK and hide the Airfoil Surface. The surface was enclosed with a solid part and now other operations can be added to the part.

Save your document.




CATIA® V5R6

Applying Materials This section will cover applying materials to a defined part. Open the materials document and save with your initials. Materials from the material library will be applied to this part. Select the apply material icon from the bottom toolbar. material library.

This will display the

The Material Library contains many different types of materials. Each material stores information about itself such as texture, density, drafting pattern and other engineering properties. The materials are broken down into several categories. The categories are construction, fabrics, metal, other, stone and wood. Any type of material can be applied to any type of part, but only one material can be applied per part. Assemblies must be used in order to have multiple parts with different materials applied. Diagrams of each material window can be found in Appendix C. Select the Metal tab. This tab contains the various types of metal definitions in CATIA. Other definitions can be added, but this is not within the scope of this course. Select Aluminum. This will be the material applied to the part. Select the Mounting Bracket and select OK. This will apply the material to the part. You should notice an aluminum branch added to the tree. Double selecting this branch will display the various properties of the aluminum which are shown in Appendix C as well. In order for the part to appear aluminum you have to change the render style.


Applying Materials, Page 277


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Press and hold the first mouse button while on the render style icon on the bottom toolbar. Release the mouse button while on the customized view parameters icon. This will allow a customized shading method. This icon will bring up the Customized View Modes window. If this icon has already been initialized then it will appear differently and you will have to use the pull down menu View, Render Style, Customize View in order to bring up the Custom View Modes window.

Set the options so that only Materials and Shading are on. This will shade the part using the material texture. Select OK. The part is now shaded with the Aluminum property.

All other materials are applied in the same manner. You can apply another material and it will replace the current material that is applied. You may want to try out a few of the materials just to see what they look like. Save your document.

Applying Materials, Page 278



CATIA® V5R6

Reference Geometry As you have gone through some of the exercises you may have noticed various planes in addition to the default ones. These were created using the reference elements toolbar. Planes are very useful to define supports for sketches, to split geometry and to define limits for your objects. In future courses you will find other uses for planes as well. This exercise is going to introduce you to the various options available to create planes. Open the planes document and save with your initials. The first thing you are going to have to do is add the reference elements toolbar to your workbench. Add the Reference Elements (Compact) toolbar to your workbench. You can do this by using the pull down menu View, Toolbars, Reference Elements (Compact). You should see a new icon appear on your workbench that appears as a point.

There are three icons in this toolbar: point focus on the plane icon.

, line

and plane

. This exercise will

Offset from plane Select the plane icon. This will open the Plane Definition window. Most of the plane types will be covered in this exercise. Change the Plane type to Offset from plane. This will allow you create a plane offset from the yz plane.


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Use the yz plane as the Reference and change the Offset to 3 and select OK. A new plane appears three inches from the yz plane and parallel to it.

Parallel through point Select the plane icon. Change the Plane type to Parallel through point.

Use the yz plane as the Reference and the end point of the line for the Point as shown above and select OK. A plane appears parallel to the yz plane passing through the point.




CATIA® V5R6

Angle/Normal to plane Select the plane icon. Change the Plane type to Angle/Normal to plane.

Use the line as the Rotation axis, the yz plane as the Reference, change the Angle to 45 and select OK. A plane appears passing through the line and at a 45 degree angle to the yz plane. Through three points Select the plane icon. Change the Plane type to Through three points.




CATIA® V5R6

Select the three points as shown below and select OK. A plane appears passing through the three points.

Through two lines Select the plane icon. Change the Plane type to Through two lines.

Select the line and the H axis of Sketch.2 and select OK. You will know if it is Sketch.2’s H axis because when you put your cursor on it, Sketch.2 will highlight in the specification tree. A plane appears passing through the two lines.




CATIA® V5R6

Through point and line Select the plane icon. Change the Plane type to Through point and line.

Select the top end point of the spline as the Point and select the line and then select OK. A plane appears at the point passing through the line. Through planar curve Select the plane icon. Change the Plane type to Through planar curve.

Select the curve and select OK. A plane appears passing through the curve.




CATIA® V5R6

Normal to curve Select the plane icon. Change the Plane type to Normal to curve.

Select the curve and leave the Point to be Default (Middle) and select OK. A plane appears normal to the curve and passing through the midpoint of the curve. Equation Select the plane icon. Change the Plane type to Equation.

Change the value of D to be 2 and select OK. A plane appears 2 inches in the z direction. You can use this option to key in a variety of planes using the equation of a plane.




CATIA® V5R6

It should appear similar to the diagram shown below.

The other two options, Tangent to surface and Mean through points will not be covered in this course. If you were to use these planes in your part design and then you modify the plane the part will update automatically. Most of the time you can see the part update dynamically as you move a plane.




CATIA® V5R6





CATIA® V5R6

Problems Problem #1.0


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CATIA® V5R6

Appendix A This section is to introduce you to the various options that are available under the pull down menu Tools, Customize. This will only give you a brief overview of the various options. Customize - Start Menu

This allows you to specify what workbenches you want available to you on the start menu. You can access these workbenches by selecting the change workbench icon on each workbench. An example of what you could possibly see is shown below.


Appendix A, Page 315


CATIA® V5R6

Customize - User Workbenches

Allows you to define their own workbenches with their own toolbars on the workbench. Customize - Toolbars

Allows you to modify existing toolbars or create your own toolbars.




CATIA® V5R6

Customize - Commands

Allows you to add or delete commands from toolbars. You can also set up hot keys for various options if you Show Properties. Customize - Options

Allows you toggle on or off the Large Icons or Tooltips.




CATIA® V5R6





CATIA® V5R6

Appendix B This will give a general overview of some of the options available through the pull down menu Tools, Options. Not all of the options will be covered, just the ones that are pertinent to this course. General - Display - Tree

Tree Type

allows you to change how the tree appears based on the type selected

Tree Orientation

orients the tree either horizontally or vertically

Tree Item Size

this pertains to the size of the text in the tree

Tree Show/NoShow

if turned on, items in your tree that are hidden will have their icons blurred or appear fuzzy


Appendix B, Page 319


CATIA® V5R6

General - Display - Visualization

Colors Graduated color background if turned on the background color will appear graduated from top to bottom instead of solid Background

color of the background

Selected elements

color of elements that you have selected

Selected edges

color of edges that have been selected

Preselected element linetype linetype of preselected elements Low-intensity elements

color of elements that appear in low-intensity

Update needed

color you part will appear when an update is needed

Handles

color of the various handles that appear, such as the handle that appears when translating




CATIA® V5R6

General - Parameters - Symbols

Constraint Style

allows you to change the color of the constraints based on their condition

Display at Creation

allows you to change the default display of your constraints to be either value, value and name, or value and name and formula




CATIA® V5R6

General - Parameters - Units

Units

allows you to select the magnitude and then specify the units that you want to use for that magnitude

Dimensions display

you can specify if you want trailing zeros, when to use exponential notation and how many decimal places you want to see displayed




CATIA® V5R6

Mechanical Design - Part Design - General

Update

sets whether or not your part gets updated automatically when a change occurs or you have to manually update it, you also can turn on or off having the update stop on the first error

Delete Operation

toggle on or off whether you want the delete dialog box to appear when you delete and you can toggle whether you want referenced sketches deleted




CATIA® V5R6

Mechanical Design - Part Design - Display

Specification tree


determines what gets displayed by default in the specification tree, the options not selected will be collapsed underneath their respective object



CATIA® V5R6

Mechanical Design - Sketcher

Grid

allows you to toggle the display of the grid and the snap to point option on the sketch plane

Sketch Plane toggle for having the sketch plane appear shaded and for positioning the sketch plane parallel to the screen Geometry

toggle for the creation of center points automatically when a circle or ellipse is created and the direct manipulation allows you to select an element of the sketch and drag it to manipulate the sketch

Constraint

toggle for automatically generating geometrical and dimensional constraints

Colors

change the default color of sketch elements and to change the color of elements when they are over constrained, construction geometry, associated geometry, etc.




CATIA® V5R6





CATIA® V5R6

Appendix C Material Library Materials are used to attach structural properties to parts as well as allow them to be displayed in a more accurate manner. They will also automatically produce patterns corresponding to the material when drawings are created from the parts. The following pages show you diagrams of the available materials that come with CATIA. Construction


Appendix C, Page 327


CATIA® V5R6

Fabrics




CATIA® V5R6

Metal




CATIA® V5R6

Other




CATIA® V5R6

Stone




CATIA® V5R6

Wood

You can add additional materials to the library but that topic is beyond the scope of this course. However, your company will probably populate this library with the various materials that are commonly used and you will be able to apply them in the same manner to which you apply these materials.




CATIA® V5R6

Applying a material In order to apply a material to a part, all you have to do is select the apply material icon in the bottom toolbar, select the material, select the body and select OK. Select the apply material icon. Select the material desired. Select the part body that you want this material to be applied to. Select OK. In order to see the material shaded on your part you need to make sure your customized render style includes materials and shading. You can configure this by using the pull down menu View, Render Style, Customize View. If this is set up then you just have to activate that render style by choosing it from the bottom toolbar.




CATIA® V5R6

Properties of a material Using the third mouse button while on the material in the specification tree you can access the properties of the material. There are many tabs with various properties on each tab depending on the material that is being used. The tabs are Rendering, Inheritance, Feature Properties, Analysis and Drafting. The following diagrams relate to Italian Marble however they should be similar to many of the other materials. Rendering

As you can see there are two tabs located under Rendering: Lighting and Texture. The Material size pertains to the size of the texture, for small parts you will want the size to be smaller and for large parts you will want it to be larger. You can also change the mapping style using the icon. The Lighting options are self defining as long as you are familiar with the graphic arts language. The important thing to note is that you can adjust all of those values. The Texture options tell you the tif file that it is using for the texture and the rest of the options allow you to adjust that texture.




CATIA® V5R6

Inheritance

Determines what features will be affected with this material. This pertains to the parent and child elements of the part body that has the material. This is more useful when working with assemblies then with parts. Feature Properties

Allows you to change the name of the material as it is displayed in the specification tree.




CATIA® V5R6

Analysis

This contains the structural properties of the material. Drafting

This allows you to adjust the pattern that is going to be used when you create drawings from this part. You can choose a different pattern by using the Pattern table button.




CATIA® V5R6

When you select the Pattern table button the Pattern Chooser window appears.

This allows you specify the pattern that you would like to use when a drawing is created. You can filter the pattern options by categories: Hatching, Dots and Color or you can choose All types. In order to see the rest of your options you have to select the Next button. This overview was meant to introduce you to various options involving materials, you will need to use the various options in order to get a better understanding of them.




CATIA® V5R6




Catia+Part+Design+Book

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