Airbus Catia v5 Sketcher

AIRBUS UK

CATIA V5 Foundation Course

Foundation Course Sketcher Compiled by: Kevin Burke

Approved by:

Authorised by:

Date:

Date:

Kevin Burke Date: 16/Apr/2003

AIRBUS UK Ltd. All rights reserved.

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Contents Session 3 – The Sketcher Workbench ......................................3 An Introduction to Sketcher ...................................................................................... 4 Renaming a Node name on the Specification Tree ................................................... 5 Accessing the Sketcher Workbench.......................................................................... 6 Selecting a Sketch Plane ....................................................................................... 7 The Sketcher Workbench .......................................................................................... 8 Sketcher Toolbars and Icons ................................................................................... 10 Selecting and Positioning Geometry....................................................................... 12 The Profile Toolbar ................................................................................................. 14 The Profile Icon................................................................................................... 14 Pre-Defined Profiles............................................................................................ 18 Circles and Arcs .................................................................................................. 22 2D Splines ........................................................................................................... 24 Conical Shapes .................................................................................................... 25 Lines .................................................................................................................... 26 Axis Line ............................................................................................................. 29 Points................................................................................................................... 29 Editing the Definition of an Element ...................................................................... 32 The Operations Toolbar .......................................................................................... 33 Create 2D Fillets.................................................................................................. 33 Relimitation or Trim functions............................................................................ 36 Transformation Tools.......................................................................................... 39 3D Geometry....................................................................................................... 45 Cutting the Part by Sketch plane ......................................................................... 49 Constraints............................................................................................................... 50 Constraint and Element Colours ............................................................................. 51 The Constraints Toolbar.......................................................................................... 53 Create Constraints using a dialog box................................................................. 53 Create Constraints by selecting elements............................................................ 54 Create Automatic Constraints ............................................................................. 56 Animates Constraints .......................................................................................... 58 Managing Constraints ............................................................................................. 58 Linking Constraints Together.................................................................................. 60 Further Sketcher Options ........................................................................................ 63 An alternative way of entering Sketcher ............................................................. 63 Editing a Sketch .................................................................................................. 64 Changing the Sketch Support.............................................................................. 64 Sketch Analysis Tool .......................................................................................... 65

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Session 3 – The Sketcher Workbench On completion of this session the trainee will: ♦ Be able to access the Sketcher Workbench. ♦ Understand the Sketcher Toolbars and Icons. ♦ Be able create and manipulate 2D Geometry. ♦ Be able to apply and manipulate Constraints.

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An Introduction to Sketcher The primary use for Sketcher is for the user to define precise and rapid 2D profiles, which can then be used in the definition of surfaces and solids. Within a sketch you can create 2D-wireframe geometry which can be used to produce Solids or surfaces and is represented by a solid line font. 2D-construction wireframe geometry can also be created which is used as an aid to produce the solid 2Dwireframe geometry. To position and control the size of the sketch, geometric and positional constraints are used which are displayed in green. A Sketch Node will be attached to the Specification Tree in which the Sketch Axis, Geometry and Constraints details are held. The Specification Tree can be expanded by selecting the ‘+’ symbol on the Tree Branch or collapsed by selecting the ‘-‘ symbol. Specification Tree

Geometric Constraints

Wireframe Geometry

Construction Wireframe Geometry

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Dimensional Constraints

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Renaming a Node name on the Specification Tree You can edit the name of a node on the Specification tree by selecting it with MB1 followed by MB3 to display a contextual menu. Now select Properties to display a Properties panel for the selected

Node name to be edited

In the Feature Name field on the Feature Properties tab is the name of the Node. Select this field and enter the new name for the Node and click OK to apply the change.

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Accessing the Sketcher Workbench To access the Sketcher workbench select > Start > Mechanical Design > Sketcher from the Start drop down menu or select the Sketcher Icon from any workbench that allows sketches to be created.

If a CATPart is not active a new part will be activated and you will be prompted to enter a part name by following panel on the desktop. Enter a name and click on OK and a new CATPart will open.

Note: If the part is to be stored on the vault the name must be in uppercase and conform to the relevant project naming convention.

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Selecting a Sketch Plane The sketcher icon will now be orange and you will be prompted to select a plane, a planar face or a sketch this is known as the Sketch Support. Select the required plane, face or sketch and the catia desktop will switch to the sketcher workench and graphic display.

Select a Plane from the Specification Tree or Graphically. For additional information on creating user defined Planes see the Part Design Session

Select a Planar face on an existing solid

Select an existing Sketch on the Specification Tree

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The Sketcher Workbench Part Specification Tree

Sketch Axis

Sketch Grid

Geometry

Sketcher Workbench Toolbars

Sketch Tools Toolba

On entering the Sketcher graphics window a Yellow 2D Axis is displayed containing a vertical Axis ‘V’, a Horizontal Axis ‘H’ and a origin point. This is the Sketch Absolute Axis and you can use these elements to position geometry on the sketch plane by the use of Constraints.

H Axis V Axis

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The graphic display area will have a Grid displayed on the sketch plane to which geometry can be snapped. It is possible to change sketcher interface features such as the grid size by selecting Tools>Options from the Tools drop down menu followed by the Mechanical Design>Sketcher branch on the displayed panel. The Grid section controls the visibility, size and whether grid snapping is used. The Sketch Plane section allows the sketch plane to be shaded and to automatically position the sketch plane parallel to the screen. The Geometry section allows the creation of circle/ellipse centre points and the manipulation of geometry by the use of the mouse. The Constraints section switches on automatic constraints where appropriate. The Colors section controls element colours.

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Sketcher Toolbars and Icons

Sketcher Workbench Icon

There are four main toolbars within the sketcher workbench: 1. Profile Creation – used for the creation of geometric elements.

Exit Sketcher

2. Operations – for dressing-up (Filleting, Trimming, etc.) and manipulating geometry (Mirroring, Translating, etc.).

Selection Icon

3. Constraints – for controlling geometry size and position.

Constraints

4. The Sketch Tools toolbar – is used for positioning and controlling geometry and is described on the following page. The above commands are also accessible via the Insert drop down menu

Profile Creation

Operations

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Sketch Tools – for controlling grid snapping, construction geometry and applying automatic constraints. Construction geometry toggle (orange indicates construction geometry will be created).

Grid snapping toggle (orange indicates grid snapping is on).

Automatic Dimensional constraints (orange indicates dimensional constraints will be created).

Automatic Geometric constraints (orange indicates geometric constraints will be created).

Fields for entering constraint value manually.

When automatic geometric constraints are enabled geometric controls are applied to the element being created, automatic dimension constraints are only created on fillet radii and chamfers or when entered in the relevant field on the Sketch tools toolbar. All the constraints will appear in the specification tree under the Sketch node. Unwanted constraints can be deleted by selecting the constraint with the left mouse button followed by the Delete key or use the right mouse button and select delete from the context menu. A more in depth explanation of constraints is given further on in this session.

Geometric Constraint

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Selecting and Positioning Geometry Individual geometry can be selected by either graphically or from the specification tree using the left mouse button. Two or more elements can be selected by pressing the Ctrl Key in conjunction with the left mouse button. Finally selection can be performed by using one of the selection icons and the left mouse button.

Paint Stroke Selection

Select

Selection Trap

Intersecting Trap

Polygon Trap

Standard Select - Select by clicking on an element or by clicking and dragging a rectangle around the elements you wish to select, when the mouse button is released all the elements fully contained within the rectangle are selected.

Selection Trap - Similar to the standard select command except individual element cannot be selected. Select by clicking and dragging a rectangle around the elements you wish to select, when the mouse button is released only the elements fully contained within the rectangle are selected.

Intersecting Trap - Select by clicking and dragging a rectangle around the elements you wish to select. All elements contained within and crossing the rectangle are selected.

Polygon Trap – Select by enclosing the required elements within a polygon which is formed by clicking with the left mouse button. Double clicking completes the selection. Only elements contained fully within the polygon are selected.

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Paint Stroke Selection – Select by clicking and dragging a curve through the elements that you wish to select. When you double click the mouse button all elements that are crossed by the curve are selected.

In all cases the selected geometry will turn orange. Once you selected the geometry it can be repositioned by click and dragging the left mouse button to the desired position. Remember that all elements that are linked or constrained to the moving elements will also be affected. To deselect the all the elements click anywhere on the graphics window with the left mouse button

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The Profile Toolbar Used to create wireframe geometry with sketcher Creates a profile consisting of lines and arcs. Creates pre-defined profiles. Creates circles and arcs. Creates 2D Splines. Creates Conical shapes. Creates lines. Creates an axis line. Creates Points. Note: By using automatic geometric constraints when creating elements the shape will be maintained if an element within the profile is moved. The profiles can be defined either by selecting graphic locations, entering the values via the sketch tools toolbar or by snapping to existing geometry in the current sketch

The Profile Icon Creates a profile consisting of lines and arcs. On selecting this icon the sketch tools toolbar changes to display further options and you are prompt to enter the start point of the profile. By default the first element will be a Line as indicated by the icon being highlighted in the toolbar, although you can start with an Arc. With the automatic dimensions constraint icon selected it is possible to create a profile two ways. 1. You can enter the ordinates of the start and end points of the line in the ordinate fields followed by the Enter Key for each point, this will display both the start and end points plus the constraint values on the screen. 2. You can click on the sketch plane to indicate the start and end points but no constraints will be generated, although they can be added at any time. This is the easier way to create geometry.

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Having created the start point you have to enter an end point using either method, for this example will use the mouse clicks to define the profile. Click on the sketch plane to indicate the end point of the line. The length and angle of the line is displayed on the sketch tools toolbar. In some case the element will be displayed in blue before you click, this indicates a constraint can be automatically generated if the automatic geometric constraint icon is selected. In this case a horizontal constraint is created. Line length and Angle

To create a tangent arc you can either: 1. Select the Tangent Arc icon and click to indicate the end of the arc. 2. Click and dragging the mouse pointer in the direction you wish the arc to appear, then release the button and the sketch tool will switch to insert tangent arc mode. Now click to indicate the end of the arc. Again the arc will turn blue if automatic geometric constraints are available. The size of the radius is dynamically displayed on the sketch tools toolbar again you could enter the size directly into this field. Tangent Arc

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Radius Value

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The sketch tools toolbar switches back to insert line mode once the arc is completed. Indicate the end point for the line using the left mouse button, again the line length is displayed on the toolbar.

Finally click and drag from the end of the line to switch to insert arc mode, then select the start of the first line to close the profile. As you hover over the start point of the line a blue circle with a solid blue dot will appear, which indicates the end of the arc will snap to the start of the line if you click. Once the profile is closed the command is completed. If an open profile is required you can either double click after completing an element or deselect the profile icon to terminate the command. If a mistake is made when defining a profile, you can click on the Undo icon during the command to step back through the profile.

Element snapping indicator

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Starting a Profile with a three point Arc. To start the profile with a arc rather than a line the following method can be used. 1. Select the Profile icon then click to indicate start point of the arc followed by the insert three point arc icon on the sketch tools toolbar.

Insert 3 Point Arc

Arc start point

2. Click to indicate the second point.

3. Finally click to indicate the end point of the arc.

The profile command will now switch back to insert line mode. Note: Complete circles can not be produced using this icon

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Pre-Defined Profiles Creates pre-defined profiles. Insert an Oriented Rectangle

Insert a Rectangle

Insert an Elongated Hole

Insert a Parallelogram

Insert a Cylindrical Elongated Hole

Insert a Keyhole Profile

Insert a Hexagon

. Creates a rectangle using 2 points or locations. Click to indicate the first corner of the rectangle followed by second click to indicate the diagonally opposite corner. Ordinate values of the points

Size of rectangle

First point Second point

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Creates an Orientated Rectangle using 3 points or locations. Click to indicate the first corner of the rectangle followed a second click to complete the first side. Finally click a location to indicate the diagonally opposite corner.

First point

Third point

Second point

Creates a Parrallelogram using 3 points or locations. Click to indicate the first corner of the Parrallelogram followed by the second click to complete the first side. Finally click a location to indicate the diagonally opposite corner.

Third point

Second point

First point

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Creates an Elongated Hole or Slot using 3 points or locations. The first two points selected using the mouse will define the position and length of the slot axis. The third selection controls the size of the slot.

Second point

First point

Slot Axis

Third point

Creates a Cylindrical Elongated Hole or Slot. The first selection indicates the centre point of the radial axis of the slot. The second and third selections define the radius and radial length of the slot. The final selection defines the size of the slot.

Second point

Slot Axis

First point (Centre of slot axis)

Fourth point Third point

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Creates a Keyhole profile using 4 points or locations. The first selection indicates the centre of the large radius of the profile. The second indicates the centre of the small radius, the third selection defines the size of the small radius and finally the last selection indicates the size of the large radius.

Fourth point

First point

Third point

Second point

Creates a Hexagon profile using 2 points or locations. The first selection indicates the centre of the Hexagon and the second define the size of the profile.

Second point

First point

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Circles and Arcs Creates Circles and arcs. Insert a 3 Point circle

Insert Circle

Insert a Tri-Tangent Circle

Insert a Circle by ordinates

Insert a 3 Point Arc

Insert a 3 Point Circle with limits

Insert Arc

Creates a Circle using 2 points or locations. The first selection indicates the centre of the circle and second defines its size.

Creates a Circle through 3 points or locations.

Creates a Circle using Cartesian or Polar ordinates. After selecting the icon a Circle Definition panel will appear. Select either the Cartesian or Polar Tab and enter the Center Point ordinates as required. Enter the radius size in the Radius field and click the OK button to insert the circle. The circle is generated with the controlling constraints. The Center Point constraints are relative to the sketch axis H and V.

Constraints

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Creates a Circle tangent between 3 elements. After selecting the icon select the 3 elements you wish the Circle to be tangent to.

Circle tangent to 3 Lines

Circle tangent to 3 Circles

Circle tangent to a Line, Spline and a Point

Creates an Arc through 3 points or locations. Select 3 locations to create the Arc (Start point, Mid point and then End point). The arc can be changed to a full circle or compliment arc by using use the right mouse button to access the contextual menu whilst the arc is highlighted in orange, you can then select the Circle. object tab to access the Close and Complement options.

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Creates an Arc using 3 points or locations starting with its limits. Select 3 locations (Start point, End point and then Mid point). Again the contextual menu can be used to close to a circle or create a complement arc.

Creates an Arc using 3 points or locations. The first selection indicates the centre point of the arc, the second defines the radius and its start point. The final selection defines the end of the arc.

2D Splines Creates 2D Splines and Connect Curves.

Insert 2D Spline

Insert a Connect Curve

Creates a 2D Spline through a series of Control points or locations. Select a series of locations known as Control Points through which a 2D Spline is generated as you define the control point locations. Double click the finish the Spline.

Spline

Control Points

Creates a Connect Curve between to elements. Select 2 elements to produce a trimmed circle between them. The contextual menu can be used to produce a closed circle or complement arc.

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Conical Shapes Creates Conical shaped elements. Insert a Parabola

Insert a Conic

Insert an Ellipse

Insert Hyperbola

Creates an Ellipse using 3 points or locations. Firstly select a location to indicate the centre of the ellipse followed by a location to define the Major axis radius and finally a location to define the Minor axis radius. Remember the sketch tools toolbar displays the geometric values of the ellipse as it is being define.

Second point

First point Third point

Creates a Parabola defined by its Focus point using 4 points or locations. The first selection defines the Focus point, the second defines the Apex, the third and fourth define the start and end points of the Parabola. Creates a Hyperbola defined by its Focus point using 5 points or locations. First select the Focus point, followed by the centre intersect point. The third selection defines the Apex, the fourth and fifth define the start and end points of the Hyperbola.

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Creates a Conic using 5 points or locations. The first and second selection indicates the start and end points of the conic, the third defines the Apex, the fourth and fifth defines the shape of the conic.

First point

Second point

Fourth point

Fifth point Third (Apex) point

Lines Creates Line type elements. Insert an Infinite Line

Insert a Bisecting Line

Insert a Bi-Tangent Line

Insert a Line

Create Lines using 2 points or locations. There are two methods of creating a lines. 1. Create a line by defining its start and end points(default option). The first selection indicates the start point of the line and the second defines the end point.

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2. Create a line symetrically about a mid point. To create a line in this way select the Insert Line icon followed by the Symmetrical Extension icon on the sketch tools toolbar. The first selection indicates the mid point of the line followed by a second which defines one end of the line and generates the other end symetrically about the mid point. Symmetrical Extension Icon

Mid Point Selection

End point selection

Symmetrical End

Note: If automatic contraints are selected a symmetrical constraint is applied to the line to ensure that in the event that the length of the line is changed the symmetry is maintained. Creates Infinite length Lines. You can create infinite horizontal and vertical lines using one point or an inifinite angle line using 2 points. To create horizontal and vertical line select the Insert Infinite Line icon followed by the Horizontal Line (default option) or Vertical Line icon on the sketch tools toolbar and select a location for the line. To create a angled line after selecting the Insert Infinate Line icon select Line Through Two Points icon on the sketch tools toolbar and select two locations to generate the line. There are 3

Horizontal Line

Line Through Two Points

Vertical Line

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Creates a Line tangent between to elements. After selecting the icon select the two elements that between which you want to create the line between.

A Tangent Line between two Splines

A Tangent Line between two Circles

Note: The line attempts to attach to the element at the point you select. Again use automatic geometric constraints are selected to maintain tangency when the elements are moved or resized. Creates an Infinite Bisecting Line between two existing lines. Select the icon followed by the two existing lines.

Infinite Bisecting Line

Existing Lines

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Axis Line The Axis Line is used to create revolved Solids and Groove features. To create an Axis line select the icon and followed by to points or locations to define the length and position of the line.

Profile Axis Line

Note: Only one Axis line is allowed per sketch and it can not be a construction element.

Points Creates Point type elements. Insert a Intersection Point

Insert Point by co-ordinates

Insert Point by clicking

Insert equally spaced Points

Insert a Projected Point

Creates a Point by selecting locations. Creates a Point using Co-ordinates. After selecting this icon a Point Definition panel will appear and either use the Cartesian or Polar tab to enter the position of the point relative to the sketch axis H and V.

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Creates equally spaced multiple points along a line or curve. Select the icon followed by the line curve on which you require the points. An Equidistant Point Definition panel will appear. Enter the number of point required in the New Points field. Reverse direction can only be used on a line and will result in the points appearing off the line at one end.

Number of point (excluding end points) Preview of point positions

Resulting Points on a line Note: If the automatic geometric constraint icon is not selected during point creation the resulting points will not be associated to the line or curve. If automatic dimensional constraints are selected the resulting points will have constraint applied to them that control the spacing, unfortunately they do not updated when the original line or curve is changed in length.

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Creates a point at intersection of two elements. After selecting the icon select the two elements to intersect.

Auto. Generated Geometric Constraints using the Dimensional constraints icon

Intersection Points Note: You can only intersect two elements. To maintain associativity between the two elements and the intersection points Geometric constraints can be used but they are applied by selecting the Dimensional constraints icon and not the Geometric constraints icon. Creates a point by projecting existing point onto an element. Select the icon and then proceed to select the points that you wish to project. Finally select the element on which the points are to be projected. Again use the automatic dimensional icon to apply geometric constraints to maintain associativity between the points and the element.

Points to be projected

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Editing the Definition of an Element The majority of the elements and features created in workbenches can be edited once they have been created. To perform this task either double click on the element that is to be edited or select it using the left mouse button followed by the MB3 to access the contextual menu. Select the XXXX.Object from the menu followed by Definition to access the Definition panel for the element.

Edit the element properties as required and then click OK to execute the change.

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The Operations Toolbar Operations are used for dressing-up (Filleting, Trimming, etc.), manipulating geometry (Mirroring, Translating, etc.) and Projecting 3D elements.

Corner or Fillet Chamfer Relimitations or Trim Transformations 3D Geometry

Create 2D Fillets. There are two methods for creating 2D fillets: 1. Between two elements by selecting the icon and then two elements that meet or will cross each other. Then either enter the radius value in the sketch tools toolbar or click a location to indicate an approximate size of the fillet. If the automatic Geometric and Dimensional constraints are selected the radius will be created with tangency to the adjacent elements and the radius size. By default both adjacent elements are trimmed as the fillet is created. You can elect to trim the first element only or no element trimming by clicking on the relevant icons on toolbar. Trim the first element only No element Trimming Trim both elements

Constraints

First element Radius size Fillet

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2. Filleting multiple elements by multi selecting the vertices or corner points of two elements in a profile. To multi select hold down the CTRL key, then select the required vertices or corner points and finally select the fillet icon. You can now enter the radius size in the sketch tools toolbar.

Radius size

Vertex Points With the automatic Geometric and Dimensional constraints selected both tangency and the radius size is controlled. The radius size is applied to all vertices and is controlled by the use of formulae between the fillet of the first vertex and all subsequent fillets. Therefore by changing the first radius size all the other radii update. The f(x) symbol indicates that the constraint is controlled by a formula. An overview in the use of formulas is covered later. Controlled Radius

Controlling Radius

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Create 2D chamfers After selecting the icon select the two elements that meet or will cross each other. As with filleting either enter the chamfer values using the sketch tools toolbar or select a location to indicate an approximate size. Again use the automatic constraints icon to control the size of the chamfer. It is also possible to control the trimming from trim both elements being chamfered, trim the first elements only and no element trimming. There are three constraint options available: 1. Constraints applied to the hypotenuse and angle. 2. Applied to both elements from their intersection point. 3. Finally constraints are applied to first element and an angle. Trimming Options

Constraint Options

Chamfer size

Constraints option 1 Constraints option 3 Constraints option 2

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Relimitation or Trim functions Close

Break

Trim

Quick Trim

Complement

Trim Elements. There are three options with the trim command: 1. Select the element to trim using the left mouse button and the element will now dynamically extend or shorten with the mouse pointer. If you click a location the element will then be trimmed to that length. 2. After select the Trim icon ensure the Trim All Elements icon is selected on the Sketch Tools toolbar. Then select two elements to trim together by selecting the first element on the portion of it that you wish to keep and then select the second element on the portion you wish to keep. Trim All Elements Icon

Resulting Trimmed elements First Element

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Second Element

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3. After selecting the Trim icon ensure the Trim First Element icon is selected on the Sketch Tools toolbar.. Now select the first element on the portion you wish to keep followed by the second element to trim to.

Trim First Element Icon

First Element

Second Element

Create a Break in an element. After selecting the icon select the element to be broken followed by the breaking element or you can select any location along the element to indicate the break point.

First Element

Second Element (Breaking Element) Third Element created

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Quick trims an element to other elements in a single selection. Select the element to be trimmed. This will result in the element being trimmed to the nearest available elements from the location you select on the element. Constraints are automatically generated linking the elements together. Automatic Constraints

Element portion selected

Trimming Element Resulting Trim

Element portion selected

Resulting Trim

Trimming Elements

Closes arcs, fillets or broken circle into full circles.

Creates a complement arc, ellipses, etc.

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Transformation Tools Translate

Scale

Offset

Symmetry Rotate Creates symmetry or mirror of selected elements.

Select the elements to be mirrored followed by a line, Construction Line or axis line to indicate the mirror plane. The mirrored elements will now be created. Profile to be mirrored

Mirror Plane Line

Mirrored profile with Constraints

Note: When using the symmetry command it is advisable to use the automatic geometric constraints to maintain the link to the original profile.

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If the profile to be mirrored is a connected profile it is possible to use the contextual menu to Auto Search for all the elements in the profile. Prior to selecting the symmetry icon select one of the elements in the profile followed by using the right mouse to access the contextual menu. Select the *****.Object followed by Auto Search. The rest of the profile will now be selected. Now the symmetry icon can be selected.

Translates or Duplicates elements. Select the elements to be translated then select the translate icon or vice versa. A Translation Definition Panel will now appear. Select Duplicate mode if you wish to copy the selected elements and enter the instances or number of copies required. If Conservation of the constraints is checked the existing profile constraints are copied to the duplicate elements. The Length option is only available after you have selected the first origin point of the translation. If Snap Mode is checked the distance between the duplicate instances is set to the value entered in the Length>Value field. If this option is not used the step distance is defined by the select a location on the screen.

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After completing the required fields in the definition panel click OK to apply. To finish the command you must select a second location to indicate the translation vector and /or the step size.

Original Elements

Duplicate Elements

Note: Automatic geometric constraints will not work with this command therefore there is no link to the original elements, so if a change is made to the size and position of the original elements the duplicates will not update. Rotates and duplicates Elements. Select the elements to be rotated followed by the Rotate icon. As with the Translate command a Rotation Definition will now appear. The duplicate options are the same as the translate command. The Angle>Value is the angular step between the duplicated elements and is only accessible after you have selected a location for the centre of rotation. After selecting the centre of rotation you can either: 1. Enter the angular value for the step and click OK

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Centre of Rotation

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2. Select a location on the screen to indicate the start angle of the step and select a second location to define the step size.

Start angle of step End angle of step Centre of Rotation

Duplicate Elements Note: Again automatic geometric constraints will not work with this command.

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Scale Elements. Select the elements that require scaling and select the scaling icon. A Scaling Definition panel will appear. Select the duplicate mode if required and either enter the scale value followed by clicking OK or use the mouse the location to define the scale.

Scaled Elements Original Elements

Note: Again automatic geometric constraints will not work with this command. Element creation by using Offset. Select the elements to be offset and select the offset icon. The Sketch Tools Toolbar will now display the following options: 1. Default is offset with no propagation (one element). Offset Element

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2. Offset with Tangent Propagation (Only elements that are tangent to the selected element are offset).

Offset Elements

3. Offset with Point Propagation (Offset all elements that are connected in the profile of the select element).

Offset Elements

4. Bilateral Element Offset. This can be used in conjunction with the propagation options.

Offset Elements

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5. On the Sketch Tools Toolbar you enter the multiple offset using the instances field, the location point of the offset and its size.

3D Geometry Creates elements from 3D Geometry. Intersect 3D Elements

Project 3D Elements

Project 3D Silhouette Edges

Creates elements by Projecting 3D geometry on to the current sketch plane. Select the 3D geometry to be projected using MB1 and the Ctrl key if you are multiselecting elements followed by the 3D Project icon. The elements are then generated on the sketch plane. The elements are coloured yellow, which signifies that they are linked to the 3D elements and cannot be moved although they can be trimmed. Elements to be projected

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Sketch Plane Projected sketch elements

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You can isolate the elements by selecting them and then use the contextual menu via MB3 to Isolate them. The elements can then be moved and will no longer update if the 3D elements changed. By using the Definition button on the contextual menu you can highlight the 3D elements that the sketch elements have been projected from.

Contextual Menu

Selected element

The command can project 3D Lines, Arcs, Points and Splines together with Solid, Face and Surface Edges.

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Creates sketch elements by intersecting 3D geometry with the sketch plane. Select the 3D geometry to intersect with followed by the Intersect icon, again you can use the Ctrl key to multi-select.. The elements are then created on the sketch plane in yellow signifying their link the 3D elements. You can use the contextual menu to Isolate and highlight the Definition elements. Selected elements

Sketch elements

This command can be used to intersect with 3D-wireframe geometry, Solids and Surfaces.

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Creates 3D Projected Silhouette edges on a sketch plane. Select the 3D geometry followed by the 3D Projected Silhouette edges icon. The silhouette elements will now be created.

Silhouette elements

Selected 3D Geometry

Note: This command will only create silhouette elements from conical Faces and Surfaces who’s Axis are parallel to the sketch plane.

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Cutting the Part by Sketch plane Cut Part by Sketch Plane allows the user to quickly view the appropriate sections through existing solids. After entering into a Sketcher, by selecting the Cut Part by Sketch Plane icon on the bottom toolbar a section cut is performed on any Solid element that intersects the Sketch plane. This is a visualisation aid only and the resultant section does not affect the solid. The edges of the section can not be selected or constrained to.

Cut Plane (sketch plane)

Solid before cutting

Solid after cutting

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Constraints Constraints are used to control an element size, position and its relationship to other elements. There are two types of constraint: 1. Geometric – Controls the relationship between elements i.e. Tangency, Parallelism, Coincidence, etc. and may also be used to control the orientation of an element i.e. Vertical and Horizontal. 2. Dimensional – Controls the size of an element i.e. the length of a line, the radius of an arc, etc. They can also control the distance and angle between elements. Following graphic symbols represents constraints: Geometric: Fix – Holds the elements in a fix position. Horizontal and Vertical – Holds the element parallel to the sketch axis.

Perpendicular – Holds two elements perpendicular to each other. Coincidence – Applies coincidence between two elements. Parallelism – Applies parallelism between two elements. Dimensional:

Angular

Diametric

Radial

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Linear

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Constraint and Element Colours Constraints and elements can be display in the following colours, which depict different states. Unconstrained or partially constrained elements are displayed in white. A green constraint indicates the constraint is valid and up to date.

Green elements indicate that they are fully constrained.

Brown constraints and elements indicate over-defined or inconsistent constraints, which can be resolved by deleting the relevant constraint.

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Purple constraints and elements indicate that the elements are over-constrained. Remove the unnecessary constraint to resolve the problem.

Unnecessary Constraint

Red constraints and elements indicate that the at least one of the constraints has to be changed.

Remember all constraints are displayed in the Specification Tree. Some Constraints can only be created by using this panel i.e. ‘Equidistant point’

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The Constraints Toolbar The following toolbar is used to apply constraints in sketcher. Generally you can either select elements to be constraint and then the command icon or vice versus. Constraints Defined in a Dialogue box Constraint Auto-Constraint Animate Constraint

Create Constraints using a dialog box Select the element/elements to be constrained followed by the Constraint Dialog Box icon. A Constraints Definition panel will appear from which you can select the desired constraints by using the check boxes followed by clicking OK to apply them.

Selected Element

Applied Constraints

Note: You can only apply constraint types that are highlighted to an element.

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Create Constraints by selecting elements

Create Geometric and Dimensional Constraint

Create Contact Constraint

Creates Geometric and Dimensional Constraints by selecting elements. After selecting the Constraint icon you can either: 1. Select a single element to apply a constraint to. This will result in the default constraint being generated based on the element that is selected. If you apply the same constraint to the element a reference constraint will be created which is denoted by brackets around the value and as such can not be used to control the element. Default Constraints

Reference Constraints

You can drag the Constraint using the Mouse Pointer to give different results

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When selecting the element you can use the contextual menu MB3 to apply different constraints i.e. Vertical/Horizontal Dimensions, Distance, Angle, Parallelism, etc.

2. Select two elements to apply a constraint between them.

Again the contextual menu can be used to apply different constraints.

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Creates contact constraints between two elements. Select the icon followed by the two elements to be constrained. The relevant constraint is automatically generated, i.e. Coincidence and Tangent.

Applied Constraints

Create Automatic Constraints Generates constraints automatic on selected elements. This is a quick method of adding constraints to a profile although some editing may be required.

Selected Element

Select the elements that you wish to AutoConstraint followed by the Auto-Constraint icon. An Auto Constraint panel will now appear with the follow options: Elements to be constrained – Lists the elements that you selected to constraint. If the wrong is selected you can deselect it by clicking on the element again. Reference elements – Allows you to select elements to control position a profile i.e. the Sketch axis H and V. Symmetry lines – If elements are selected as symmetry lines Catia will attempt to apply symmetry constraints to the elements to be constrained. Constraint Mode – Allows you to select the display representation of the constraint either Chained or Stacked. This option is only available when Reference elements are selected.

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Auto-constraint 4 elements with H and V Axis selected as Reference elements in Chained mode

Auto-constraint 4 elements only

Auto-constraint 4 elements with H and V Axis selected as Reference elements in Stacked mode DMS42188 AN—UG0300111

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Animates Constraints Allows a single constraint to be animated. Select the constraint to be animated followed by the Animate Constraint icon. A Animate Constraint panel will now appear. The following options are have to be entered: First value – Is the start value. Last value- Is the end value. Number of steps – Defines the number of steps used during the animation between the first value and last value. The Actions buttons are used to Start, Stop and Pause the animation. The Options buttons are used to set up the type of replay required from single play, single loop, continuous loop and repeat single play.. The Hide constraints check box switches off the constraints temporarily.

Managing Constraints You can delete any constraints by selecting the desired constraints and either using the Delete key, MB3 > Delete or on the Delete from the Edit drop down menu. When applying constraints that result in over constraining errors it is advisable to correct the error immediately rather than leaving all corrections to the end. The quickest method of editing a constraint definition is to double click on the constraint, which will display the Constraint Definition panel. This panel can be used to change the following: 1. The value of the constraint. 2. Switch it to a Reference constraint. 3. Swap its location. 4. The name of the constraint. 5. Which element/elements the constraint is linked to.

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The panel also displays what type of constraint it is and wheather it is up to date.

Use the More button to expand the panel

After changing the required values click the OK button to apply the changes. In some cases it may be easier to delete the constraint and generate a new one rather than editing it. You can also use MB3 > *****.Object > Definition or the Edit drop down menu to access the definition panel. Note: When you have to constrain sketch elements to 3D Geometry it may be better to use Projected 3D elements on the sketch plane rather than the originals.

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Linking Constraints Together It is possible to use a one Constraint to control another by the use of a Formula. This is performed using the following method: 1. Select the constraint you wish to be controlled or Driven. 2. Using MB3 select the Radius.** object tab followed by Edit Formula from the Contextual Menu. Selected Constraint

3. An Formula Editor panel will now appear which contains the following fields:The top field contains the name of the Constraint that you have selected to be Driven. The next field contains the name of the constraint that you have selected control or Drive the first constraint it may also contain an equation that can be used to control the constraint. The main window contains a list of parameters available. The bottom field displays the name and value of the controlling constraint.

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4. Now select the Constraint that you wish to control or Drive the first Constraint. This will then populate the panel with name and value of the constraint.

Constraint to be controlled or Driven.

Controlling Constraint or Driver

5. Click OK to complete the operation. The Driven constraint value will now update and a FX symbol will appear next to value to indicate that it has a formula attached to it.

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To delete a formula from a Constraint double click on the constraint to display the Constraint Definition panel. Note: The Radius value field is not accessible due to the fact that that constraint is controlled by a formula, which also indicated, by the presence of a FX button next to the field.

Now select the FX button to display the Formula Editor panel and delete the contents of the second field.

Click OK to complete the deletion process. It is also possible to delete a Formula from the Specification Tree by expanding the Relations node (if present) and selecting the required followed by Delete on the MB3 contextual menu or keyboard.

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Further Sketcher Options An alternative way of entering Sketcher There is a second way of creating a Sketch by selecting the Sketch with Absolute Axis definition icon. This will allow you to define the Sketch support, its Origin and any Orientation required. On selecting the icon a Sketch Positioning panel will appear. You then select elements to define the Sketch Support position and if required the Origin and the Orientation elements. By default the origin and orientation is derived Implicit(ly) from support elements. Click OK to create the sketch. Sketch Support elements

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Editing a Sketch To edit existing sketches you can double click on the sketch node in the Specification Tree, select the node follow by MB3>*****.Object>Edit or use the Edit drop down menu. You will then enter the sketch.

Changing the Sketch Support You can change the Sketch Support by either selecting the sketch node followed by MB3>>*****.Object>Change Sketch Support or again use Edit drop down menu. You will then have to re-select the support plane element. Note: Elements and sketches linked or constrained to the sketch that you are repositioning may be affected by this change.

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Sketch Analysis Tool This analysis tool can be used to check a sketch for error i.e. open profiles, overlapping elements, isolated elements, etc. To access this tool select Sketch Analysis from the Tools drop down menu whilst you are in the Sketch. The analysis is now performed on all the elements contained within the sketch and a Sketch Analysis panel is displayed. The Geometry tab specifies whether the geometry passes the check or if there are problems. The Projection/Intersections and Diagnostics tabs give details geometry status.

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