Sketcher Overview

Sketcher Overview ________________________________________ Overview: Sketcher enables you to create parametric, planar geometry on faces and planes. After you draw the geometry, you use the sketch to create pads, pockets, shafts, and surface geometry. ________________________________________ Sketches Sketches are sets of 2D, fully-parametric curves. In a typical sketch, you first create base curves, and then add geometric and dimensional constraints to control the size and shape of the curves. By adding these constraints to the sketch curves, you can capture and define your design intent. This approach makes it much easier to modify the sketch shape later. Sketch Usage Sketches are commonly used to define section curves for pads, pockets, shafts, grooves, or surface geometry. Sketches maintain associativity to their parent and child features. If you change the geometry in a sketch, the solid model changes accordingly. Similarly, if a plane or face changes orientation or moves, any sketches attached to that plane or face move with it. You can also add dimensional and geometric constraints to the sketch. Using dimensional constraints, you can create system-defined expressions and link them to other sketch dimensions or to other features of the solid. Using Sketcher intelligently allows you to quickly modify the model to reflect changes during the product life cycle. Sketch Placement You create sketches on a plane or solid planar face. A sketch remains associative to its placement face. If the face changes orientation or location, the sketch changes with it. When you pick a plane or face as the sketch plane, CATIA sets the horizontal and vertical directions as the main axis of the selected plane. You can manually control the horizontal and vertical directions by selecting the horizontal and vertical reference edges, and the placement face, before creating the sketch. Sketch Management Organizing the data within a CAD file is always important when different people are potentially going to use the data. Data organization is especially important when using sketches because you can define sketch information in many geometrical sets, with different sketch names. Depending on the complexity of a design, even a simple, single solid model can contain over 20 sketches. With this amount of data, it is prudent to use good techniques to manage your sketches. CATIA automatically makes a sketch invisible once you use it to create a feature, such as a pad or pocket. However, it is a good practice to place each sketch into a geometric set. This makes it easier to find the information required in the Graphics window. It is also advantageous to give each sketch a descriptive name by editing the properties of the sketch. ________________________________________ Tips • Always assign the In Work object to the appropriate geometrical set before creating a sketch. Although you can move objects, it may be easier to initially create objects in the correct location. Creating Sketches ________________________________________ Path: Insert | Sketcher | Sketch Insert | Sketcher | Positioned Sketch Located on the Sketcher toolbar. ________________________________________ Use this to ... • Create a new sketch. ________________________________________ Key Points • In CATIA, there are two ways to create a sketch: Sliding (also known as a Non-positioned sketch) and Positioned. In a sliding sketch, you do not have control over the origin or orientation. This can lead to potential errors in your model, such as, if base sketches update, later sketches can become out of place. It is good modeling practice that all the sketches you create are positioned sketches. However, you can update a non-positioned sketch to a positioned sketch. ________________________________________ Process: Creating a Sliding Sketch (Non-positioned Sketch) 1. Select Insert | Sketcher | Sketch. CATIA prompts you to pick a face or plane. 2. In the Graphics window, pick the sketch placement face to activate the Sketcher workbench. 3. On the Workbench toolbar, click Exit Workbench to return to the modeling application. ________________________________________ Process: Creating a Positioned Sketch 1. Select Insert | Sketcher | Positioned Sketch. The Sketch Positioning dialog displays. 2. In the Graphics window, pick a placement face. CATIA projects the sketch origin onto the selected plane or face origin. 3. In the Origin Type list, select the origin definition method. In the Graphics window, pick the geometry to define the origin. 4. In the Orientation Type list, select the orientation method options. In the Graphics window, pick the geometry to define the orientation. 5. Click OK to create the sketch. 6. On the Workbench toolbar, click Exit Workbench to return to the modeling application. ________________________________________ Options Sketch Positioning Defines the two options for creating a sketch. Positioned Defines the sketch by selecting a planar face or plane, or by defining two axes. A positioned sketch allows you to define the origin and the reference direction. Using existing edges as references for the sketch direction means the directions update if you modify the underlying edges. Using a positioned sketch is the recommended method of creating a sketch. Sliding Creates a non-positioned sketch. The default origin and directions of the selected plane or face define the origin and direction of the sketch. Sliding sketches can be updated to positioned sketches by selecting new reference directions. Origin These options define the methods to position the origin of the sketch. Implicit Defines the origin as the default origin of the face or plane. Selecting two lines places the origin at the intersection of the two lines. The H direction is collinear with the first line; the second line only defines the side on which the V direction is created, not the orientation. Part Origin Defines the sketch origin as the absolute origin of the part. Projection Point Defines an origin by projecting a point onto the sketch positioning face or plane. Intersection 2 Lines Defines the origin at the intersection of two lines. Curve Intersection Defines the origin at the intersection of two curves. Middle Point Defines the origin at the mid-point of a line or edge. Barycenter Defines the origin at the center of a face. Orientation Defines the H and V directions of the sketch. When defining the direction, you can control either the H or V direction. You also have the ability to reverse the direction. Implicit Defines the sketch directions as the default directions of the sketch support. X Axis Defines the active direction along the X-axis. Y Axis Defines the active direction along the Y-axis. Z Axis Defines the active direction along the Z-axis. Components Defines the active direction by entering vector components. Through Point Defines the active direction as the vector through a point. Parallel to Line Defines the active direction as parallel to a selected line. Intersection Plane Defines the active direction as the line created by the intersection of two planes. H Direction Lets you define the H direction of the sketch. V Direction Lets you define the V direction of the sketch. Reverse H Reverses the H vector. Reverse V Reverses the V vector. Swap Swaps the H and V directions. ________________________________________ Frequently Asked Questions 1. Can I modify the sketch directions and origin? A: Yes, you can modify all the sketch definitions by picking the sketch in the Specification Tree and selecting Edit | | Change Sketch Support, or right-click to display the pop-up menu. ________________________________________ Tips • Click Exit workbench to quickly exit Sketcher. Sketch Tools Toolbar ________________________________________ ________________________________________ Sketch Tools Toolbar The Sketch tools toolbar (select View | Toolbars | Sketch tools) is invaluable when creating sketch geometry. The toolbar enables you to automatically create constraints, and it changes to display the coordinates, lengths, and other information in the context of command you are using. The Sketch tools toolbar also provides feedback as you dynamically move the cursor in the Graphics window, showing you the current length of a line or the diameter of the circle. This information is helpful because sketches are much easier to constrain when the initial geometry is drawn close to the desired size. Additionally, toolbar functions allow you to snap the curves to a grid and create construction geometry. The Sketch tools toolbar has several distinct areas. The first section contains: Grid, Snap to Point, Construction/Standard Element, and Geometrical and Dimensional Constraints. These first five commands are always present and are the same, regardless of the active sketch command. The next section contains options that vary, depending on what geometry you are creating or what command you are using to modify your existing geometry. For example, when creating a line, the Sketch tools toolbar displays several different text boxes. Initially, the toolbar allows you to specify the H (horizontal) and V (vertical) start coordinates. Then the toolbar changes to display the end coordinates. The length of the line and the angle text boxes display at all times while the line command is active. The Sketch tools toolbar for creating a sketch chamfer has options for how to trim the selections. After you select the geometry, the toolbar displays text boxes for the offset(s) and/or the angle. You can simply click in the text boxes and enter the values or press TAB to cycle to the next text box. When you finish an entry, press TAB to accept the value. After specifying all the values for a particular geometric parameter, like an endpoint, CATIA modifies the text boxes in the toolbar, allowing you to enter the next piece of geometric information. The advantage in using the Sketch tools toolbar, instead of picking in the Graphics window, is that dimensional constraints are applied automatically to the geometry. Grid This option creates a visual grid on which you create sketches. Turn this option on by clicking Grid on the Sketch tools toolbar. Other grid options are set under Tools | Options. Snap to Point Locates curve endpoints onto the grid points. Construction/Standard Element Creates sketch geometry using any of the creation modes described below. This geometry is used to create solids and surfaces. When the icon is active (highlighted), any new geometry is created as construction geometry. Construction geometry is gray by default, has a dashed line type, and does not display outside the Sketcher workbench. You can convert from standard to construction elements and vice versa by selecting existing curves and then changing the status of the Construction/Standard Element icon. Geometrical Constraints Creates automatic geometric constraints in conjunction with SmartPick when creating geometry. When deactivated, geometric constraints are only applied at the time of creation. After you draw curves, CATIA does not save the constraints. It is very likely that that this will be active all of the time. Dimensional Constraints Creates automatic dimensional constraints when entering values in the Sketch tools toolbar to create exact geometry. It is very likely that that this will be active all the time. ________________________________________ Tips • Roughly create the profile you need. Then use dimensional and geometrical constraints to finalize the profile. • When creating a continuous profile, you can activate the Tangent Arc command by clicking and dragging the cursor away from the endpoint of the line. Release to activate the Tangent Arc command. Curve Creation Techniques ________________________________________ Overview: When you create sketch geometry, there are different methods that you can use to define the shape, size, and position of the curves. ________________________________________ Clicking in the Graphics Window Versus Entering Values on the Sketch Tools Toolbar The two methods of creating curve geometry include picking in the Graphics window and applying the constraints separately, or to using the Sketch tools toolbar to enter specific data. The advantage in using the Graphics window is that you can quickly create the rough profile and then use the exact constraints that you need to finalize the geometry. The disadvantage is that there are more open degrees of freedom to constrain, initially making curves more difficult to control. As you become more comfortable with constraints, creating curves on-the-fly is the fastest and easiest method for defining a profile with the proper design intent, especially when used in conjunction with SmartPicks and active Geometrical Constraints. The advantage in using the toolbar method is that the constraints can be applied at the time of creation, (if Dimensional Constraints is active on the Sketch tools toolbar). The disadvantage is that many of the automatic dimensional constraints may not properly define your design intent, such that you will have to delete and recreate, or redefine the constraint. Entering a value in the Sketch tools toolbar locks that value, allowing you to either pick in the Graphics window to define the rest of the geometry or use the toolbar to enter the rest of the definition. Using a combination of methods allows you to use defined values, while still having the flexibility of picking in the Graphics window. Pay close attention to what you are entering in the Sketch tools toolbar. Remember that the Sketch tools toolbar asks for different information, depending on what curves you are creating, and changes as you progress through the definition. In other words, after entering data, the toolbar changes and then looks for the next set of values. Use TAB to move between text boxes in the toolbar. TAB stores the entered value in the toolbar and makes the next text box active. Pressing ENTER only stores the entered value. Pop-up Menu During Curve Creation The pop-up menu is also an invaluable tool when constructing geometry. Right-clicking another element when creating geometry displays the pop-up menu. Depending on your selections, the pop-up menu changes, allowing you to create geometric constraints between the two elements. For lines, the pop-up menu allows you to apply parallel and perpendicular constraints. Right-clicking a circle or arc during line creation allows you to apply tangency constraints. Right-clicking geometry also allows you to copy the geometric properties of the curve, such as length and radii. Right-clicking a dimensional constraint allows you to copy the constraint value and paste it into another constraint. ________________________________________ Tips • Use a horizontal or vertical constraint instead of specifying an angle of 0, 90, 180, or 270 degrees. Options - Sketcher Overview: The Options dialog is where you set various sketch options, such as, Grid, Sketch Plane, Geometry, Constraint, and Colors. All these options are available by selecting Tools | Options, Mechanical Design, Sketcher. • ________________________________________ Grid Controls the virtual grid that displays on the sketch plane. You can use the grid as a reference when creating geometry. Activate Snap to point to restrict the cursor movement to the grid intersections. Specify the horizontal distance between grid lines by entering values in the Primary spacing text box and specify the spacing between each grid line in the Graduations text box. To specify different vertical grid lines activate Allow Distortions.