Copyright DASSAULT SYSTEMES Sketcher Version 5 Release 8 January 2002 EDU-CAT-E-SKE-FF-V5R8 CATIA Training Foils
Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will learn how to sketch, constrain, and edit 2D profiles. These profiles are then used to generate solids and surfaces Targeted audience New users Prerequisites Course CATIA Basics 1 day
Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to CATIA Sketcherp.4 2. Sketching Simple Profilesp Sketching Pre-Defined Profilesp Editing Profilesp Operations On Profilesp Setting Constraintsp Managing Sketchesp.126
Copyright DASSAULT SYSTEMES Introduction to the CATIA Sketcher In this lesson you will see the V5 CATIA Sketcher user interface and basic functions
Copyright DASSAULT SYSTEMES The Sketcher is a set of tools to help the user quickly generate 2D Geometry. The completed Sketch can then be used to generate Solids and Surfaces The capability to define Constraints between elements in the Sketcher allows for quick modification of the Sketch and consequently the Solids or Surfaces that are based on it. Other tools such as Animate Constraints enable the user to explore design alternatives Why Using the Sketcher?
Copyright DASSAULT SYSTEMES You can also access the Sketcher by selecting the Sketcher icon from any Workbench where it is possible to do a sketch Select Start > Mechanical Design > Sketcher then select a plane or a face on an object Sketcher Workbench
Copyright DASSAULT SYSTEMES Sketcher Design tools... Exit to 3D Space Part tree Standard tools New Sketch A New Sketch will register in the Part Tree when entering the Sketcher Workbench Constraints Icons Tools & Operations Sketcher Interface (1/4): Sketcher Workbench general
Copyright DASSAULT SYSTEMES Exit Sketcher Profile Rectangles, Keyholes, Polygons... Circles, Ellipse, Arcs... Spline Ellipse Line Axis Points... Corner Chamfer Trim options... Symmetry Projection Constraints dialog box Constraint Auto Constraint Animate Constraint Profiles Operations Constraints Sketcher Interface (2/4): Sketcher Tools
Copyright DASSAULT SYSTEMES Insert menu or toolbars Sketcher Icons Predefined Profiles Circles Conic Line Point Sketcher Interface (3/4):Toolbars
Copyright DASSAULT SYSTEMES Once on the plane on which you want to sketch has been selected, it is displayed parallel to the screen (if Tools+ Option + mechanical Design + Sketcher + Position sketch plane parallel to screen is active) It is possible to do zoom panning and rotation (using the mouse). To reset a sketch plane rotation, select the Normal View icon If you select the Normal View icon when the sketch plane is already displayed parallel to the screen, you will turn the sketch plane and see its other side. Sketcher Interface (4/4): Sketcher Plane
Copyright DASSAULT SYSTEMES The Sketch is the holding point for a group 2D elements on a specific plane. There can be more than one Sketch using the same plane as support. The V-H Axis is the 0,0 for the Sketch. Sketches generally consist of a Profile, Constraints, and Dimensions (a type of Constraint). Profile Constraints Dimensions Terminology
Copyright DASSAULT SYSTEMES Access the Sketcher Workbench Create Geometric Elements Use the Sketch to Create a Solid or Surface Constrain the Geometric Elements Select a plane, a Solid Face, or a Planar Surface to Sketch on An In-Work Sketch is added to the Specifications Trees General Process
Copyright DASSAULT SYSTEMES Sketching Simple Profiles In this lesson you will learn how to create most of the Sketcher geometric elements. You will also learn how to use the various work modes available for the Sketcher Workbench. The Sketcher Work Modes Profile Points Lines Spline Circles and Arcs Conics Axis Recap Exercise
Copyright DASSAULT SYSTEMES Grid/Snap Standard/Construction Geometry Automatic Constraints Automatic Dimensions Section View Value Fields You will learn the Sketcher Work Modes by using The CATIA Sketcher Work Modes
Copyright DASSAULT SYSTEMES Why Sketcher Work Modes? The Sketcher Work Modes aid you while you sketch the geometry. They facilitate input of values, automate Geometrical/Dimensional Constraints creation, help visualize 3D geometry etc...
Copyright DASSAULT SYSTEMES To modify the grid parameters, select Tools + Options… from the top of the screen, select Mechanical Design from the dialog box then, select the Sketcher tab. When creating any lines ( profile, segment, circle, arc, curve, …), you can activate or deactivate the snap to point icon at any time. When the snap to point icon is active, the cursor only snaps on the points of the grid (graphical creation). If you enter coordinates when the snap to point icon is active, the system does not take into account the grid and place the point in accordance with the coordinates you have entered Using Grid/Snap
Copyright DASSAULT SYSTEMES Standard + Construction Elements Standard/Construction Geometry Two types of elements: Standard or Construction Standard elements represent the most commonly created elements Construction elements aim at helping you in sketching the required profile. They facilitate your design Creating standard or construction elements is based upon the same methodology. Clicking the icon switches from one mode to the other
Copyright DASSAULT SYSTEMES For the profile first point, you can define the Horizontal and Vertical coordinates. By pressing the tab key you access the Horizontal coordinate field, so you can enter it. By pressing the tab key once more, you access to the Vertical coordinate field, so you can enter it During sketching, you can enter exact coordinates/lengths/angles in the Tools bar. For the profile second point, you can also use the tab key to enter a coordinate, but you can also define the second point of the profile by entering the length of the segment between the first and the second point and/or by entering the angle between the Horizontal axis and the segment to be created. When profiling an arc, the tools bar allows you to enter the H and V coordinates of the last point of the arc but you can also enter a radius. You can enter these coordinates by using the tab key. If you enter only one of the coordinates (H, V, L, A or R) you fix it, this means that the other parameters can move graphically but not the fixed one Value Fields For example, in using the Profile tool...
Copyright DASSAULT SYSTEMES Automatic Dimensions When activated: - corner dimensions - chamfer dimensions - dimensions entered into the value fields are automatically created during geometry construction. In sketcher, select the Dimensional Constraints Icon Multi-select two edges of existing rectangle 2 Select Corner icon Move the corner preview to desired location and click 4 With Dimensional Constraints on With Dimensional Constraints off 1 3
Copyright DASSAULT SYSTEMES Automatic Constraints 2 With Geometrical Constraints On With Geometrical Constraints Off 1 Start to sketch the geometry. Variations of valid Constraints will be proposed depending on where the Mouse is with respect to the existing geometry. When you see the Constraint you require, click on the Mouse to store the Constraint (and the new geometry). Notice that Tangency Constraints are created even when Geometrical Constraints is Off In Tools/Options/Mechanical Design/Sketcher/Constraint/SmartPick specify which Constraints you want detected In sketcher, select the Geometrical Constraints Icon 3
Copyright DASSAULT SYSTEMES Section View In order to see a Section View of the part while sketching, click on the Cutting Plane command in the Cut By Plane Toolbar. This is purely a visualization tool, no intersection curves are created from the intersection of the Solid with the Cutting Plane. If you need to Constrain to (or Dimension off from) the intersected outline of the Solid, use the Intersect 3D Elements Tool
Copyright DASSAULT SYSTEMES You will learn how to create a Profile element Profile in the Sketcher Profile seen in 3D Profiles
Copyright DASSAULT SYSTEMES A profile can be: "Closed" (the last element connects up with the first element in the series) or "Open" (the first and last elements in the series are not in contact). If a profile is "Closed", it can have other profiles contained inside its boundaries A profile, within a profile, is shown here to illustrate how "Inner Domains" work. Notice the reversals of the boolean operations between addition and subtraction as we progress from the outside inwards Open profile What are Profiles ? Closed or open ? A profile is a series of adjacent planar geometric elements such as points, lines, and curves Profiles are used to extrude Sketch-Based Features Inner profiles
Copyright DASSAULT SYSTEMES In Sketcher, Select Profile icon Select the line icon (default) and click on two points to create line 2 Select the tangent arc icon, select end point 3 Horizontal constraint Tangency constraint Select the line icon and drag vertically to create line and click 5 Select the Three Point Arc icon and click on two points to create arc 4 Drag horizontally and click to create line. Rather than using the Tangent arc icon to create the final arc, click, drag and release at the beginning of the arc and CATIA goes into the tangent arc mode automatically. 6 1 Creating Profiles
Copyright DASSAULT SYSTEMES You will learn the various methods to create points Points
Copyright DASSAULT SYSTEMES How are Points Created in the Sketcher ? Points can be created in the Sketcher in two ways: - By the user - By the system When the user creates a line, the lines end points are automatically created by the system. When the user creates a circle, the center point is created. The coordinates of these automatically created points can later be modified by double-clicking and entering new values. Alternatively, the user can first create the points directly. He can then create a line or any other geometry by selecting these points.
Copyright DASSAULT SYSTEMES Click the location where you want the point 2 In sketcher, select the Point by Clicking Coordinates icon For ease of placing the points, select the Snap to Point icon so the cursor will snap to the grid while trying to locate the point 1 Point by Identification
Copyright DASSAULT SYSTEMES Fill in the desired Cartesian or Polar coordinates 2 In sketcher, select the Point by clicking Coordinates icon 1 If the Dimensional Constraints mode is on, Polar dimensions will automatically be created in the case of Polar input. (Cartesian dimensions created in the case of Cartesian input) Points by Coordinates
Copyright DASSAULT SYSTEMES You will learn the various methods to create lines Lines
Copyright DASSAULT SYSTEMES What is a Line in CATIA V5? In CATIA V5, a line segment is described in the Specifications Tree by three nodes - two point nodes (Point.1 and Point.2) and one line node (Line.1). The line is supported by its parents - the points. When the position of a point is modified (either by double-clicking and entering new coordinates; or by dragging), the position of the line will change accordingly.
Copyright DASSAULT SYSTEMES In sketcher, select Line icon Click starting point of the line... …then click the end point OR… you can type the line specifications in the value fields of the Tools pallet Lines Between Two Points
Copyright DASSAULT SYSTEMES In sketcher, select the Bi- Tangent Line icon 1 Select the two elements you want the line to be tangent to... 2 The Bi-Tangent line is created Bi-Tangent Lines
Copyright DASSAULT SYSTEMES You will learn how to create a Spline in the Sketcher Splines
Copyright DASSAULT SYSTEMES Which Should I Use - Sketcher Spline or 3D Spline? Since the 3D Spline Tool - available within the Wireframe&Surfaces (WFS) or Generative Shape Design (GSD) Workbenches - can also be used in a 2D manner (with Geometry on Support being a plane), when should you use the Sketcher Spline and when is the 3D Spline more appropriate? In general, use the Sketcher Spline to create Sketches for generating solid Sketch-Based Features. (Although Pads and Pockets can be generated from 3D Splines) Use the 3D Spline when you need more control over the Spline - i.e. Tangent Tension, Curvature Direction, Curvature Radius. Surfaces can be generated from Splines created by either method.
Copyright DASSAULT SYSTEMES Click first point to start the spline 2 Double-Click to specify the spline End Point. 4 …then click the second point of the spline In sketcher, select the Spline Icon 3 5 …then click for the third point of the spline 4 Double-Click on a Spline Control Point to specify exact coordinates or to create a Tangency vector at that point. You can later apply Constraints on this vector (i.e. make it parallel to a line). 1 Double-Click on a Spline Control Point to specify exact coordinates or to define a Curvature after a tangency vector Creating a Spline
Copyright DASSAULT SYSTEMES Select the first curve 2 Select the second curve Select the Connect icon 3 1 You get: Connecting curve
Copyright DASSAULT SYSTEMES You will learn the various methods to create circles and arcs. Circles and Arcs
Copyright DASSAULT SYSTEMES What are Circles and Arcs in CATIA ? In CATIA V5, a Circle consists of two nodes: Point.1 specifying the coordinates of the Circle Center Circle.1 specifying the Radius of the Circle The Arc will have two additional nodes: Point.2 specifying the coordinates of one limit Point.3 specifying the coordinates of the second limit Note: When a Circle is Trimmed leaving only a portion of the complete circle. Two additional points are added to the Specifications Tree. In fact, the representation becomes the same as that of an Arc.
Copyright DASSAULT SYSTEMES Click once to define the center point of the circle, then drag the cursor 2 …and click again to define the circle size In the sketcher, select the Circle icon 1 3 Basic Circles
Copyright DASSAULT SYSTEMES In sketcher, select Three Point Circle icon Click three times to define 3 points. The circle will pass through these points Circles Through Three Points
Copyright DASSAULT SYSTEMES In sketcher, select Circle using Coordinates icon 1 Enter the absolute coordinates of the circle 2 Enter the size of the radius 3 Circle Using Coordinates
Copyright DASSAULT SYSTEMES Click first point to start the arc... 2 Then click the end point of the arc 4 …then click the second point of the arc In sketcher, select Three Point Arc icon 3 1 Three Points Arcs
Copyright DASSAULT SYSTEMES You will learn the various methods to create conics Conics
Copyright DASSAULT SYSTEMES Which Are the Conics that Can Be Created? ConicRequired Inputs EllipseCenter, Major Axis Limit, Point on Curve ParabolaFocus, Apex, Start Point, End Point HyperbolaFocus, Center, Apex, Start Point, End Point Ellipse Parabola Hyperbola
Copyright DASSAULT SYSTEMES Click to indicate center point of ellipse 2 The Tools Toolbar then displays values for defining the ellipse major axis endpoint …then click the second point for the major axis endpoint In sketcher, select Ellipse Icon 3 Center point coordinates can also be input in the Tools Toolbar 1 Creating an Ellipse (1/2)
Copyright DASSAULT SYSTEMES Click to indicate for minor axis endpoint 4 Creating an Ellipse (2/2)
Copyright DASSAULT SYSTEMES Click to indicate the Focus Point of the Parabola 2 Next indicate the two endpoints …then click the second point for the Apex In sketcher, select the Parabola Icon 3 As always, the Tools Toolbar is contextual and allows the user to input specific point coordinates during the creation steps 4 1 Creating a Parabola
Copyright DASSAULT SYSTEMES Click to indicate the Focus Point of the Hyperbola 2 Next indicate the two endpoints …then click the second point for the Center In sketcher, select the Hyperbola Icon 3 As always, the Tools Toolbar is contextual and allows the user to input specific point coordinates during the creation steps 5 … click the third point for the Apex 4 1 Creating a Hyperbola
Copyright DASSAULT SYSTEMES You will learn the method to create an Axis in Sketcher Axis
Copyright DASSAULT SYSTEMES What is the Axis Used for? An Axis element must be included in a Sketch from which a Shaft or Groove solid feature is created. The Profile to be swept around this axis must either be Closed or have its endpoints Coincident to the axis. An Axis drawn into a Sketch can also be used (but not required) to generate a Surface of Revolution. A separate Line or Solid Edge can also serve to specify the axis of revolution. Also, the Profile need not be Closed nor Coincident to the axis in this case.
Copyright DASSAULT SYSTEMES Axes cannot be converted into construction elements In sketcher, select Axis icon Click the first location for starting point of the axis... 2 …then click the end location You will need axes whenever using a symmetry command or creating a grove or shaft. Using the shaft command on our profile sketch, CATIA produces a shaft using the axis we defined 3 1 Creating an Axis
Copyright DASSAULT SYSTEMES Sketching Pre-Defined Profiles In this lesson you will learn how to Sketch the Pre-Defined Profiles Sketching Pre-Defined Profiles Recap Exercise
Copyright DASSAULT SYSTEMES You will learn the different ways to create pre-defined profiles Rectangle Oriented Rectangle Elongated Hole Cylindrical Elongated Hole Keyhole Profile Parallelogram Hexagon Sketching Pre-Defined Profiles
Copyright DASSAULT SYSTEMES Pre-Defined Profiles are tools to facilitate the creation of standard complex shapes with the minimal number of inputs that can fully describe all aspects of that shape. It increases productivity by reducing Mouse/Keyboard interactions What are Pre-Defined Profiles ?
Copyright DASSAULT SYSTEMES In creating all the Pre-Defined Profiles, it is always useful to read the prompts at the bottom left corner of the screen OR… you can type the rectangle specifications in the value fields of the Tools pallet 3 In sketcher, select Rectangle icon Click the starting corner of the rectangle... 2 …then click the diagonal corner 1 Rectangles
Copyright DASSAULT SYSTEMES OR… you can type the Parallelogram specifications in the value fields of the Tools pallet 3 In sketcher, select Parallelogram icon 1 Click the starting corner of the Parallelogram... 2 …then click for the second corner … finally, click to determine the width and internal angles of the Parallelogram 4 Parallelogram
Copyright DASSAULT SYSTEMES OR… you can type the hole specifications in the value fields of the Tools pallet 3 In sketcher, select the Elongated Hole icon 1 Indicate the first center of the hole... 2 … indicate the second center... … finally, click to determine the radius of the Elongated Hole 4 Elongated Hole
Copyright DASSAULT SYSTEMES Editing Profiles In this lesson will learn tools to help you edit Sketcher elements Modifying Profile Geometry Recap Exercise
Copyright DASSAULT SYSTEMES You will learn how modify 2D sketch elements to propagate changes to 3D parts Modifying Profile Geometry After ChangeBefore
Copyright DASSAULT SYSTEMES Sketch-based features rely on profiles for their shape Especially if defined with the proper constraints that represent the design intent of the part, the profile geometry can easily be changed for downstream design changes Modified cube Why Modify Profile Geometry? Corner removed from sketch Changing the sketch that defines a feature propagates that change to all subsequent operations involving the feature Design change
Copyright DASSAULT SYSTEMES Alter the existing coordinates of the line to new parameters (V: 50mm) 2 H: -40 V: 50 This method works on most construction entities, opening the appropriate dialog for the entity selected Double click line to edit its coordinates 1 Modifying Profile Element Coordinates
Copyright DASSAULT SYSTEMES You have modified the shape of the profile without the use of any intermediary menu options The profile stretches based on where you move the element and the constraints you have applied 2 Click and drag the line downward to its new location 1 Editing Profile Shape and Size
Copyright DASSAULT SYSTEMES Select the Undo command to restore deleted elements. The Undo command will remember all changes up to the last time the part was saved Select sketching element to delete 1 Select Edit->Delete and the element is erased. Now multi-select additional elements to delete 2 Use the contextual menu (select Mouse Button 3 while cursor is on one of the selected elements) to delete 3 Deleting Sketcher Elements
Copyright DASSAULT SYSTEMES Double click on the spline to be edited 1 Select the control point to be edited 2 You will see: 3 You can edit a spline modifying, adding or removing the spline control points Editing a Spline (1/3)
Copyright DASSAULT SYSTEMES Select the Add Point After option 4 Select the control point to be edited 5 You will see: 6 Click a point Using the same method, you can add a point before the current point or to replace the current point by another one Editing a Spline (2/3)
Copyright DASSAULT SYSTEMES Do not forget to select OK in the dialog box to validate the modifications You can also close the spine You can also define a tangency or/and a curvature on the current point Editing a Spline (3/3)
Copyright DASSAULT SYSTEMES Auto Search is a multi-selection tool. Once selected, we can use the Contextual menu to delete or change the properties of all the elements in one go. Commands such as Auto Search that are found in the Menubar can be added as an Icon into a Toolbar if desired Drag down to Auto Search from the Edit Menubar. All elements in the Profile are selected. 2 Select one element in the Profile 1 Auto Search
Copyright DASSAULT SYSTEMES Operations on Profiles In this lesson you will learn how to reuse existing geometry Re-limiting Operations Transformation Operations Offset Operation on 3D Geometry Recap Exercise
Copyright DASSAULT SYSTEMES You will learn how to re-limit geometry using Corner, Chamfer, Trim, and Break Operations After RelimitationsBefore Relimitations Re-Limiting Operations
Copyright DASSAULT SYSTEMES In general, there is much less need to re-limit geometry in V5. Each one of the closed profiles below was completely sketched with a single activation of the Profile tool. (Refer back to the Profile section for help in sketching these profiles) In fact, using the Profile tool whenever possible is the preferred practice since it will cut down on the number of user interactions. For a large number of cases, however, re-limitation of sketched geometry using Trim or Break is still necessary to achieve Design Intent. Why Re-Limiting Geometry?
Copyright DASSAULT SYSTEMES Select the two lines 2 Select the Corner Icon 1 Select the Mode - Trim All, Trim First Element, or No Trim 3 Move the mouse around so that the corner is visualized in the correct quadrant Type in the radius required and hit Enter 4 5 If Dimensional Constraints is activated, the radius dimension will be created on the Sketch. Corner
Copyright DASSAULT SYSTEMES Chamfer (1/3) 1 Select the Chamfer icon The chamfer command allows you to create a chamfer between two lines trimming either all, the first or none of the elements 2 Select the first line on which the chamfer will be created You get: 3 Select the second line on which the chamfer will be created 4 Select the desired chamfer trim option 5 Select the desired chamfer definition option 6 Using the TAB key, enter the chamfer parameters 6 Press the Enter key to validate the chamfer creation
Copyright DASSAULT SYSTEMES Chamfer (2/3) Chamfer trim options a b a b a b Trim all elementsTrim first elementNo trim
Copyright DASSAULT SYSTEMES Chamfer (3/3) Chamfer definition options Length/Angle option: Length1/Length2 option Length1/Angle option:
Copyright DASSAULT SYSTEMES Select the trim icon 1 Use the trim icon to keep/erase segments before or after an intersection point between two curves or lines Select the lines you want to trim on the sides you want kept. 2 According to the selected trim option (Trim All or Trim First Element), you will get : Trim all elementsTrim the first element Move the mouse around before selecting the second line - notice that the system shows you the various solutions possible depending on where you select this line. Trimming lines (1/5)
Copyright DASSAULT SYSTEMES Deletes Keeps Select the Quick Trim icon 1 Select the line (a) to be trimmed 2 Select the Quick trim option 3 Using Quick Trim when trimming lines and curves, allows you quickly remove unwanted segments Breaks You get : Trimming lines (2/5) - Quick Trim
Copyright DASSAULT SYSTEMES Using Close allows you to close an arc into a full circle. 2 Select the arc to be closed You will get : Select the Close icon 1 Trimming lines (3/5) - Close
Copyright DASSAULT SYSTEMES Select the Close icon from the Operation toolbar Select the part of the ellipse you want to close You can close an opened ellipse using the Close icon 1 2 You get: 3 Trimming lines (4/5) - Close
Copyright DASSAULT SYSTEMES You can also close an opened ellipse using the contextual menu of the ellipse Select the Close command from the ellipse contextual menu (MB3) 1 You get: 2 Trimming lines (5/5) - Close
Copyright DASSAULT SYSTEMES Select the Break icon 1 Use Break to split a line or curve into two parts. Select the line to be broken (a) then select the breaking line (b) 2 You will get two lines (L1 and L2) : (a) (b) Breaking
Copyright DASSAULT SYSTEMES You will learn how to perform transformations such as Rotation, Translation, Scaling and Symmetry on Sketcher Geometry Transformation Operations 7 X 45 Degrees Rotation in Duplicate Mode
Copyright DASSAULT SYSTEMES Using Transformations helps the user avoid repetitive work by enabling the user to reuse existing geometry to help define new geometrically-related Sketcher elements. Why Transform Geometry?
Copyright DASSAULT SYSTEMES Remember that there are a variety of Multi-Selection Tools available Select a line or Axis to specify the Line of Symmetry 2 Select (or Multi-Select) the element(s) to apply the Symmetry 1 Select the Symmetry Icon 3 Symmetry
Copyright DASSAULT SYSTEMES In general, once a value is entered, it is temporarily fixed. The remaining values continue to float. In the example below, if the length of translation is entered, the user is still capable of moving the mouse around to change the direction of the translation. Select a first point on the Grid to define the origin of the translation 2 Select (or Multi-Select) the element(s) to apply the Translation 1 Select the Translation Icon 3 4 Options: A) Select a second point of the Grid to define the distance and direction for the translation B) Type in the coordinates of the second point into the Tools Toolbar C) Make the Translation Definition window active and type in the Length of translation. Indicate the preferred direction. (Press the TAB key to go between fields) Number of Copies Translation
Copyright DASSAULT SYSTEMES When Snap Mode is active (as in the Rotation Definition window), the angle values that are proposed as the user moves the mouse around will take on Integer increments Select the Center Point for the Rotation 2 Select (or Multi-Select) the element(s) to apply the Rotation 1 Select the Rotation Icon 3 4 Options: A) Select two points on the Grid with respect to the center to define the angle B) Type in the coordinates of the two points into the Tools Toolbar C) Make the Rotation Definition window active and type in the Angle of Rotation (Press the TAB key to go between fields) Rotation
Copyright DASSAULT SYSTEMES When Duplicate Mode is not active, the geometry selected is transformed (no new elements are created) 2 Select (or Multi-Select) the element(s) to apply the Scaling 1 Select the Scaling Icon 3 Options: A) Select the Center Point and a second point on the Grid with respect to the center to define the magnitude of the Scaling B) Type in the coordinates of these two points into the Tools Toolbar C) Select a center point. Make the Scale Definition window active and type in the Scaling Factor (Press the TAB key to go between fields) Scaling
Copyright DASSAULT SYSTEMES You will learn how the Offset tool is used Offset
Copyright DASSAULT SYSTEMES Offset is a local operation which allows you to duplicate one or several elements of a profile. These elements will be duplicated keeping the parallelism between the selected elements and the duplicated ones What is the Offset Operation? The offset can be positive or negative to determine on which side of the profile the offset profile will be created
Copyright DASSAULT SYSTEMES Offsetting Element (1/2) Once in the sketcher, select one of the element to be offset 1 3 In order to select the connected element of the profile, select the Point Propagation icon The Offset command allows you to duplicate one or several elements in the sketcher. These elements will be duplicated keeping the parallelism between the selected elements and the duplicated ones Select the Offset icon 2
Copyright DASSAULT SYSTEMES Offsetting Element (2/2) 4 In the Tools bar, enter the Offset value: 2 The Offset command allows you to duplicate one or several elements in the sketcher. These elements will be duplicated keeping the parallelism between the selected elements and the duplicated ones 5 Press the Enter key You get: 6 To validate, click on the side you want to get the offset profile
Copyright DASSAULT SYSTEMES Instead of entering an offset value, you can define a point the offset profile will pass through by entering its coordinates Additional Information Different options to define an offset To offset only the selected element To offset only the tangent elements To offset only in both directions To define several instances
Copyright DASSAULT SYSTEMES You will learn what tools operate on 3D Geometry from Sketch Mode and why they are important Operations on 3D Geometry
Copyright DASSAULT SYSTEMES Project- projects elements that are off the current Sketch plane into the Sketch. - Projection is associative to the parent 3D geometry Intersect- intersects 3D elements with the Sketch plane - Intersection is associative to the parent 3D geometry Isolate- Breaks the links that Projected and Intersected elements have with their parent 3D geometry so that they may be edited independently What are the Tools that Operate on 3D Geometry and why are they Important? The Profile of the Tray is linked to the Profile of the Support through a Projection Tray Support
Copyright DASSAULT SYSTEMES Here … a projected Solid Edge (a Spline contour) is used as part of the closed profile for the current Sketch 2 Select (or Multi-Select) the elements to project into the Sketch plane. (Selecting Solid Faces or Surfaces will project the boundary curves of these elements) 1 Select the Projection Icon Project 3D Element
Copyright DASSAULT SYSTEMES Select (or Multi-Select) the elements to intersect with the Sketch plane. 1 Select the Intersection Icon If the shape of the surface should change, this contour will also change accordingly Here … the curve generated by intersecting the surface with the Sketch plane can be used as part of the closed profile for the current Sketch Intersect 3D Element
Copyright DASSAULT SYSTEMES The Project 3D Silhouette Edges command shows how to create silhouette edges to be used in sketches as geometry or reference elements. Limitations are same as Projection/Intersection command, as far as associativity is concerned. You can only create a silhouette edge from a canonical surface whose axis is parallel to the Sketch plane. Select the Project 3D Silhouette Edges icon 1 Select the element to be projected 2 You get: Project 3D Silhouette Edges
Copyright DASSAULT SYSTEMES The isolated lines turn white to indicate that they are no longer linked. The user can now drag these lines to new locations or change them in any way he chooses The Isolate command breaks the links that Projected and Intersected elements have with their parents 3D geometry so that they may be edited independently 2 Select (or Multi-Select) the elements to be isolated (Here … two of the edges from the projected face) 1 Activate the Isolate command from the Menubar - Insert/Operation/3D Geometry A Projected or Intersected curve does not need to be isolated in order for it to be re-limited (position is not modified) Isolate
Copyright DASSAULT SYSTEMES You can see the mark characteristics and you can transform the mark in a construction element. The mark can come from a projection or an intersection In the sketcher, double click on the projection 1 The mark is now a construction element In the dialog box, select the Construction element button 2 Select OK 3 You get: Edit Mark Definition
Copyright DASSAULT SYSTEMES You can edit Projections and Intersections Double click on Projection.4 1 Double click New edge Select a new edge to be projected, then select OK 2 When leaving the sketcher, you will get: Edit and Modify Import Properties
Copyright DASSAULT SYSTEMES You can edit an element Parents/Children and Constraints from the Parents Select Parent/Children from the constraint contextual menu 1 Select Show All Parents from Offset.12 2 Editing Parents Children and Constraints (1/2)
Copyright DASSAULT SYSTEMES Select Edit from Pad.1 3 You can, now, edit the pad Editing Parents Children and Constraints (2/2)
Copyright DASSAULT SYSTEMES Setting Constraints In this lesson, you will learn how to use dimensional and geometric constraints in order to precisely define your sketch Introduction to Constraints Quick Constraints Modification of Constraints Auto Constraint Animating Constraints Relations Between Dimensions Recap Exercise
Copyright DASSAULT SYSTEMES What are Constraints and why do we need them? Sketching in Context Introduction to Constraints You will learn the different ways to create constraints
Copyright DASSAULT SYSTEMES Without Constraints, geometry can be moved freely just by using the mouse to drag them. If Sketcher profiles are moved, so do the solids that are supported by them. In the context of an assembly, if one part moves, another part that is related to it may also move. Although in CATIA V5 geometry will remain in place when put there, without Constraints any subsequent movement of elements by the user may go unnoticed and affect Form Fit and Function of entire assemblies. Hence, Constraints serve to mathematically fix geometry in space. They also can specifically relate one element to another and serve as visual feedback to the user on what these relationships are. After Constraints are created, they are easily modified by merely changing their values or placement. From the ease at which Constraints may be modified and from the inherent downstream associativity of V5, the user can quickly explore alternative designs. Why Constraints? Movement of 4 Unconstrained Lines
Copyright DASSAULT SYSTEMES A Geometric constraint is a specification of how two geometric elements are related to one another: are the elements coincident (located at the same place), are they concentric, tangent, perpendicular or parallel to one another? Dimensional constraint What are Geometric and Dimensional Constraints ? A Dimensional Constraint, one type of Geometric Constraint, specifies the distance between two elements. This distance can be specified as a linear distance, an angular distance, or a radial distance depending on the type of geometric elements involved Geometric constraint Geometric constraints Dimensional constraints (here distance) (here concentricity)
Copyright DASSAULT SYSTEMES Sketching in context is using existing geometry to create new geometry When sketching with CATIA V5 space geometry is visualized. You can use it to guide your sketch 3D geometry used to sketch and constrain profiles What Does Sketching in Context Mean ? At first, the sketch has to only be made to conform to the spatial intent i.e. the left or right of a hole, on the inside or outside of a pocket, on the top or bottom of a pad, etc. Later, the exact dimensions or precise geometric constraints (concentricity, parallelism, coincidence...) can be applied to the sketch (or profile) to define it precisely From rough to precise sketch
Copyright DASSAULT SYSTEMES You can add constraints between the active sketch and any part edges, vertices or other sketches. Activate the constraint icon Select the edge of the part then the segment to be constrained Select the Distance constraint from the contextual menu (MB3) Place the constraint and modify it if necessary) 4 Sketching in Context
Copyright DASSAULT SYSTEMES Quick Constraints Dimension Constraints Contact Constraints
Copyright DASSAULT SYSTEMES Dimension constraints and Contact constraints are frequently used. Hence, they are made accessible with just one click. Why Quick Constraints? Other constraints are chosen from a Constraint Definition Box
Copyright DASSAULT SYSTEMES Post selecting the circle produces a diameter dimension... 4 Select Constraint icon Select sketch line to apply dimensional constraint 1 Select location of dimension 3 Select Constraint icon 3 …but then selecting the line tells CATIA to reconsider the dimension and put in a distance dimension 5 2 Setting Dimensional Constraints
Copyright DASSAULT SYSTEMES Generally, the first element selected will remain in its current position. The second element selected will move. For more control, use the Fix Constraint beforehand. Select the Contact Quick Constraints 2 Select the two elements to be made in contact 1 Setting Contact Constraints
Copyright DASSAULT SYSTEMES Modification of Constraints
Copyright DASSAULT SYSTEMES All geometric and dimensional constraints may be deleted using the Contextual Menu (third mouse button) What Kind of Modifications Can be Done on Constraints? Values of dimensions may be changed by double-clicking on them The location of dimensions and the extension lines can be modified by dragging with the left mouse button The type of Constraints applied on an element can be modified by reentering the Constraints Dialog Box and making modifications there A geometric or dimensional constraint attached to an element (i.e. line, circle etc …) can be reconnected to a different element. The geometry will change to conform to the new Constraint setup
Copyright DASSAULT SYSTEMES Select a new constraint i.e. Verticality 1 5 Select Constraint Dialog Box icon 2 Deselect the Perpendicularity Box 3 Click OK to Exit Select the two lines linked with the Perpendicularity constraint 4 Modification in the Constraints Dialog Box
Copyright DASSAULT SYSTEMES Click on More 3 2 Select the Line component 3 Select Reconnect Select the unassociated line in the Sketcher window 4 Double Click on the Tangency Constraint Click OK to save and exit 6 Reconnecting a Constraint
Copyright DASSAULT SYSTEMES To modify the position of a dimension's value: To modify the position of the dimension line: Click the icon Select the dimension line Drag the line to the new position Click the icon Select the value text of the dimension Drag the value text to the new position Dimension line: Dimension value: Additional Information...
Copyright DASSAULT SYSTEMES Auto-Constraint
Copyright DASSAULT SYSTEMES What is Auto-Constraint? The AutoConstraint Tool: The AutoConstraint tool automatically detects possible constraints between selected elements and imposes these constraints once detected Elements to be constrained Fixed Elements (Independent elements from which other elements can be constrained from - normally the Sketcher Axes) Symmetry Lines (If selected will cause Symmetry Constraints to be created between elements symmetrical to these lines - the symmetry lines themselves will not be constrained)
Copyright DASSAULT SYSTEMES Auto-Selection tools such as Auto-Search and Trap can be helpful Multi-Select the lines in this closed profile. 2 Select the Auto-Constraint Icon 1 Select the Reference Elements Field then select the Vertical and Horizontal Axes 4 Click OK to create Constraints 5 Select the elements to be constrained 3 Auto-Constraint
Copyright DASSAULT SYSTEMES Animating Constraints
Copyright DASSAULT SYSTEMES What is Animating Constraints? The Animate Constraint Tool: The Animate Constraints tool allows you to see how a constrained system reacts when you decide to make one constraint vary. In this way, it is a tool for understanding the limitations imposed on the geometry by the current set of constraints. It can be a very useful tool for exploring design alternatives.
Copyright DASSAULT SYSTEMES The Animate Constraint panel works like a tape-recorder panel. The user can play forward and backwards, rewind, or play in cyclic repeat mode. Select the dimension you would like to vary 2 Select the Animate Constraint Icon 1 Input the initial and final values and the number of intermediate steps to display 3 Press the Play button. Cancel when done 4 Animating Constraints
Copyright DASSAULT SYSTEMES Relations Between Dimensions
Copyright DASSAULT SYSTEMES What are Relations Between Dimensions? Relations between Dimensions: Dependencies can be established between dimensions (For example, A=B+C/2) Originally a part of the Knowledgeware set of products, this functionality has been incorporated into the V5 infrastructure and is generally accessible from all Workbenches. In CATIA V5, in addition to relationships between dimension values, dimensions can be made dependent on other parameters such as Forces, Temperature, Time, or Material Properties etc...
Copyright DASSAULT SYSTEMES When required, open ( and Close ) parentheses can be used to indicate the order of evaluation for the expression Select the dimension you would like to be made dependent 2 Use the Contextual Menu (third mouse button) and drag down to Edit Formula 1 1) Select the 40 dimension 2) Type in + 3) Select the 10 dimension 4) Type in /2 3 Select OK to create the relation 4 Creating a Relation Between Dimensions
Copyright DASSAULT SYSTEMES Managing Sketches In this lesson, you will learn ways to manage Sketches within a 3D environment Creating Planes Replacing a Sketch Changing Sketch Support Sketch Analysis Change Body Recap Exercise
Copyright DASSAULT SYSTEMES You will learn how to create Planes in space for use as sketching planes Creating Planes Planes
Copyright DASSAULT SYSTEMES Sometimes we will need to create Planes to use as Sketching Planes Angled planes Why Creating Planes ? Offset planes Offset Planes sometimes will need to be created to help define the extrusion extents of a Sketch-Based Feature Angled Planes are used to define Sketch-Based Features that are angled with respect to the other features Offset planesAngled planes
Copyright DASSAULT SYSTEMES Select Plane Icon (Available from the WireFrame&Surfaces (WFS) or the Generative Shape Design (GSD) Workbenches 1 For Angle to Plane creation type, select edge as reference to rotate resulting plane about 2 Select the upper face as the reference plane to rotate from. A preview plane that can be dragged to a new location is shown 3 The resulting plane (Plane.3) is 45deg to the face, rotated about the selected edge 4 Creating an Angled Plane
Copyright DASSAULT SYSTEMES Select Plane Icon (Available from the WireFrame&Surfaces (WFS) or the Generative Shape Design (GSD) Workbenches 2 Select Face 1 The offset distance from the reference face can be set by typing the value in the dialog or dragging the circular handle on the graphic screen 3 Creating an Offset Plane
Copyright DASSAULT SYSTEMES The plane definition dialog box provides various methods for creating a plane: Different planes Different planes: Additional Information...
Copyright DASSAULT SYSTEMES You will learn how to replace a Sketch being used to support a Solid or Surface element with a different Sketch Replacing a Sketch
Copyright DASSAULT SYSTEMES Replacing a Sketch is quick way to modify solids or surfaces using that Sketch for their definition. The user creates a new Sketch with the new profile that he requires. He then merely replaces the old Sketch with the new one. The solids or surfaces that depended on the previous Sketch do not have to be re-created since they will be modified automatically and pointed to the new Sketch. Why Replace a Sketch ?
Copyright DASSAULT SYSTEMES Replacing a Sketch 1 4 Check what plane the original sketch lies on. You can use the Parent/Children analysis from the Contextual Menu (third mouse button on the Sketch) if you like Create the new sketch on the same plane (Note: although this is normally the case - it is not a requirement) 2 Right click on the the original sketch and drag down to Replace. Click on your new sketch as the replacing sketch 3
Copyright DASSAULT SYSTEMES Changing Sketch Support
Copyright DASSAULT SYSTEMES What is Changing a Sketchs Support? Changing a Sketchs Support: By changing its supporting plane, a Sketch can be moved to a new plane without having to recreate the Sketch Copies of a Sketch can be moved onto different planes in this way
Copyright DASSAULT SYSTEMES Naturally, any Solid or Surface elements attached to the Sketch will also be moved accordingly 1 While outside the Sketcher mode, use the Contextual Menu on the Sketch to be modified and drag down to Change Sketch Support Select the new plane for the Sketch 2 Changing Sketch Support
Copyright DASSAULT SYSTEMES Sketch Analysis You will learn how to analyze sketched geometry, projection and intersection. You will be provided either a global or individual status and will be allowed to correct any problem
Copyright DASSAULT SYSTEMES What is Analyzing a Sketch (Geometry)? Most of the time, we draw a sketch in order to use it to build a sketch based feature (e.g.: a pad). Sometimes, when we try to use the sketch, CATIA refuses to build the feature because the sketch is not closed (or overlapping) and it is sometimes quiet difficult to see where the sketch is opened (or overlapping). The Tools + Sketch Analysis command allows us to check if a sketch can be used to create a sketch based feature
Copyright DASSAULT SYSTEMES What is Analyzing a Sketch (Geometry)? During the sketch analysis, it is possible to do Corrective Actions: Set in Construction Mode Close Opened Profile Delete Geometry
Copyright DASSAULT SYSTEMES What is Analyzing a Sketch (Projection/Intersection)? The Sketch Analysis command can be used to check projection or intersection with 3d elements
Copyright DASSAULT SYSTEMES What is Analyzing a Sketch (Projection/Intersection)? During the sketch analysis, it is possible to do Corrective Actions: Isolate Geometry Activate / Deactivate Delete Geometry Replace 3D Geometry
Copyright DASSAULT SYSTEMES Analyzing a Sketch: Geometry (1/2) In order to edit the sketcher, double click on Sketch.1 in the tree 1 2 Select the Tools+ Sketch Analysis command The Tools + Sketch Analysis command allows us to check if a sketch can be used to create a sketch based feature
Copyright DASSAULT SYSTEMES Analyzing a Sketch: Geometry (2/2) If necessary, select the Geometry tab in the dialog box 34 In order to better see the sketch, select the Hide constraints button, the constraints will be hidden The Tools + Sketch Analysis command allows us to check if a sketch can be used to create a sketch based feature You can now see where the sketch is opened and you can correct it
Copyright DASSAULT SYSTEMES Analyzing a Sketch: Projection/Intersection (1/2) In order to edit the sketcher, double click on Sketch.3 in the tree 1 2 Select the Tools+ Sketch Analysis command The Tools + Sketch Analysis command allows us to check if a sketch can be used to create a sketch based feature
Copyright DASSAULT SYSTEMES Analyzing a Sketch: Projection/Intersection (2/2) If necessary, select the Projection/Intersection tab in the dialog box 34 You can now check if the intersections and projections contained in the sketcher are valid or not The Tools + Sketch Analysis command allows us to check if a sketch can be used to create a sketch based feature Intersection between 3d elements Projection of 3d elements
Copyright DASSAULT SYSTEMES Additional Information Different Corrective Actions that can be done when analyzing a sketch: Set in Construction ModeClose Opened ProfileDelete Geometry Analyzing a Sketch: Geometry
Copyright DASSAULT SYSTEMES Additional Information Different Corrective Actions that can be done when analyzing a sketch: Isolate Geometry: When using this icon, the selected projected or intersecting element is separated from its 3d components Activate/Deactivate: When using this icon, the selected element (of the sketch) is no more taken into account when creating a sketch based feature, but the element still exists Delete Geometry: When using this icon, the selected element is remove from the sketch Replace 3d Geometry: When using this icon with a projected or intersecting element (intersection or projection with 3d objects), you can select another 3d element to modify the projection or the intersection Analyzing a Sketch: Projection/Intersection
Copyright DASSAULT SYSTEMES Change Body You will learn how to move one sketch from a body to another one
Copyright DASSAULT SYSTEMES Why Moving one Sketch from a Body to Another one ? When working with several bodies, you may want to create a sketch base feature (a pad for example) and the necessary sketch has been created in a body different from the active one. In this case you may want to transfer the sketch from its body of creation into the active one (it is not mandatory but it is helpful to understand the part structure
Copyright DASSAULT SYSTEMES Change Body You can move one sketch from a body to another one Select the Change body command from the sketch contextual menu 1 You get: 2 Select the body in which you want to move the sketch, then select OK