CATIA Tutor

8. Interactive Drafting

The basic tasks you will perform in the Interactive Drafting workbench mainly deal with creating and modifying 2D elements and their related attributes on a predefined sheet.

8.1 Tools Toolbar

The Tools toolbar displays both command options and given fields/values that appear in accordance with the command you select. The Tools toolbar provides the following options:

Grid,

Snap to Point,

Analysis Display Mode: This option allows visualizing the colors assigned to the different types of dimensions. These displayed colors correspond to the colors customized in the Options dialog box. To modify these colors, go to Tools -> Options -> Mechanical Design -> Drafting (Dimension tab). Then check Activate analysis display mode and, if needed, click the Types and colors switch button to assign the desired color(s) to the desired dimension types.

Create Constraints,

Create Detected Constraints,

Filter Generated Elements Depending on the selected command, the Tools toolbar may also provide the following options:

Projected Dimension, Force Dimension on Element, Force Horizontal Dimension in View, Force Vertical Dimension in View, True Length Dimension

8.2 Creating Views

Interactive Drafting elements necessarily need to be positioned in a view. In other words, you will first create a view on a sheet and then add 2D geometry, dimensions, annotations and/or dress-up elements in this view. Click the New View icon . Click the Drawing window. A blue axis displays in a red frame. The front view created & displayed in the specification tree. You can now

create 2D geometry in this view. Click the New View icon again and select a projection direction to create more views. The views created are projection views as they are linked to the front view. From an active front view, you can create: a top view, a bottom view, a left view and a right view.

8.3 Defining the View Plane

This task will show you how to define the plane of a view (a front view, an isometric view or an auxiliary view). Any created view lies on a 3D plane. In other words, a view lies on some kind of a 3D plane whose definition can be accessed using the Plane Definition dialog box. The view plane can be defined and if needed, modified in this dialog box. The view plane will be defined in accordance with two vectors and an origin point. Define the front view plane: Activate the view in which you want to change the plane definition, by double-clicking on this view. Click the View Plane Definition icon from the Multi View toolbar. Select the desired options from the View Plane Definition dialog box. Press OK.

Define the isometric view plane: Click the New View icon

in order to create an empty view. In this case, position the cursor so as to create an isometric view. Make sure the view in which you want to change the plane definition is active. For this, double-click on this isometric view. Click the View Plane Definition icon from the Multi View toolbar. The Plane Definition dialog box appears. Enter the desired options from the dialog box (Isometric). Press OK.

8.4 Creating Views Using Folding Lines

This task will show you how to add geometry in views using folding lines as an assistant. This is true for any kind of view, as long as the planes they correspond to are not parallel. For example, you cannot have folding lines between a front view and a rear view. Make sure the view in which you are going to create geometry using folding lines is active. Right-click the view used as

reference. Select the object ->Show folding Lines option. Click the Profile icon and create geometry in the top view using auto detection on folding lines. At any time, you can right-click the view and suppress these folding line using the option in contextual menu.

8.5 Creating a Multiple View Projection

This task will show you how to generate geometry in a view by projecting geometry from previously defined views. Selected objects are projected onto a plane or ruled surface defined by the user, and then transformed into the receiving view. Projected geometry retains the same attributes it had in the original multi-view. You will first add elements to an existing view, using the Action-Object mode. You will then create an isometric view from scratch, using the Object-Action mode.

Add elements to an existing view, using the Action-Object mode. Click the Multiple View

from the Multi View toolbar Select the Tools -> Multi View -> Multiple View Projection command from the menu bar. Select the object defining the target plane or surface to be used. This element can be any mono-parametered elements (line, circle, ellipse, parabola, hyperbola, curve). In this case, select an arc of a circle in the front view. Select, in another view, the object to be projected. In this case, select a circle in the top view. Select more elements to be projected, if needed, or click in the open space or still another command if you want to terminate this command.

Create an isometric view from scratch, using the Object-Action mode. Make the isometric view active (double-click). Multi-select the elements to be projected into the isometric empty

view. In this case, select the whole front view. Click the Multiple View projection icon from the Multi View toolbar. Select the object defining the view to be created. All the elements are automatically projected onto the active view. Repeat the steps above (Object-Action) with the various elements to be projected that will allow generating the isometric view.

8.6 Reframing a View

In this task, you will learn how to reframe a view so as to display only part of it. Select the view and right-click the view frame. In the contextual menu, choose Properties. Click the View tab. In the Visualization and Behavior area, select the Visual Clipping check box. Click OK. The new frame appears as a rectangle in the view. You can now define the position and size of your frame on the view. Click on the frame to select it. Drag the manipulators to resize the frame, as you want. The frame can only be rectangular. You can reframe any type of view: front views, isometric views, details views, clipping views, etc.

8.7 Constraints

A constraint is a geometric or dimension relation between two elements. A constraint is defined by: a type: for example, a distance constraint, a mode: measured or constraining mode, a configuration. If you want constraints to be created, before inserting constraints make sure the constraint creation option command is active in the Tools toolbar. A constraint is a kind of relationship that allows specifying the geometry. In other words, if you modify the geometry afterwards via the geometry itself, these relations will be taken into account. Two kinds of constraint can be applied geometrical constraints & dimensional constraints.

8.8 Creating Geometrical Constraints

This task shows you how to set a relationship that forces a limitation between one or more

geometrical elements. Make sure the Show Constraints command option is active (Tools toolbar). Select the geometrical elements to be constrained to each others. Click the Constraint

with Dialog Box icon

from the Geometry Modification toolbar. The Constraint Definition dialog box appears. Modify the Constraint Definition dialog box. It is impossible to create constraints between 2D and generated elements via the Constraint Definition dialog box. In the Constraint Definition dialog box, you can only create constraints between similar elements. In other words, you can create constraints either between 2D elements, or between generated elements, but not between a mix of these.

8.9 Creating Constraints Between 2D and Generated Elements

This task shows you how to create associative constraints between 2D elements and generated elements. Click the geometrical constraints command icon and select the line. The most logical constraint is automatically offered. Select an edge from the drawing you have opened. The software proposes you parallelism by default. If you choose this constraint, click in the drawing, otherwise right-click and select Perpendicularity in the contextual menu. A constraint is created between a generated element and a sketched element. You can delete this constraint: right-click on the created constraint and select delete in the contextual menu.

8.10 Creating Dimensions

In this task, you will learn how to create dimensions. When creating dimensions on elements, you can preview the dimensions to be created. On the Dimensioning toolbar, click the Dimensions

icon. Click a first element in the view. If needed, click a second element in the view. The

dimension type is automatically defined according to the selected elements ( or in the Tools toolbar). If you right-click the dimension before creation, a contextual menu lets you modify the dimension type and value orientation as well as add funnels. Using this contextual menu once the dimension is created, you can also access the Properties options.

8.11 Re-routing Dimensions

This task will show you how to re-route dimensions, i.e. to recalculate dimensions taking into account new geometry elements which are compatible with the re-routed dimension type. Select

the Re-route Dimension icon from the Dimensioning toolbar (Extension Line Interruptions sub-toolbar). Select the dimension. You can notice that the cursor indicates the type of dimension you are selecting. Select the first element you want to take into account for the dimension re-routing, and then the second element. A preview of the re-routed angle dimension is displayed. Click to validate the dimension creation.

8.12 Dress-Up Elements

The Interactive Drafting workbench provides a simple method to create the following view dress up elements on existing 2D elements.

a) Creating Center Lines (No Reference)

This task will show you how to apply a pair of centerlines to a circle or an ellipse. Click the Center

Line icon from the Dress up toolbar. Select a circle. Centerlines are automatically applied to the circle Click in the drawing to confirm the creation and select the centerlines.

b) Creating Center Lines (Reference)

This task will show you how to apply a pair of centerlines to a circle or an ellipse with respect to a

reference (linear or circular). Click the Center Line with Reference icon from the Dress up toolbar. You can multi-select circles before you enter the command to create centerlines for all selected circles. Select the circle to be applied a pair of centerlines. Select the reference line. The centerline created is associative with the reference line. To modify a pair of centerlines at one or more end(s) of this/these centerlines, click the centerline. Red end points appear. Select any end point and drag to move all the centerline extremities to a new position.

c) Creating Threads (No Reference)

This task will show you how to create a thread without a reference. In this particular case, you will

apply a thread to a hole. Click the Drawing window, and click the Thread icon from the Dress

up toolbar. You can also multi-select holes before clicking the Thread icon . Activating this

command displays two options in the Tools toolbar. The Tap type option (Tools toolbar) is

activated by default. Select the Thread type option (Tools toolbar). Select the hole (or circle) to which you want to apply a thread. The thread is created. Select an axis line manipulator and drag it along a direction. Thread axis lines are modified symmetrically.

d) Creating Threads (Reference)

This task shows you how to create a thread with a reference, either circular (circle or point) or

linear (line). Click the Drawing window, and click the Thread with Reference icon from the

Dress up toolbar. Select the Reference Thread type option (Tools toolbar). Select a reference line. The thread is created according to this reference.

e) Creating Axis Lines

This task will show you how to create an axis line. Click the Drawing window, and click the Axis

Line icon from the Dress up toolbar. Select two lines. The axis line is created.

f) Creating Axis Lines and Center Lines

This task will show you how to create simultaneously axis and centerlines on several circles. Click

the Drawing window, and click the Axis Line and Center Line icon from the Dress up toolbar. Select two circles. The axes and centerlines are created.

g) Creating an Area Fill

An area fill is a closed area on which you then apply graphical dress-up element called patterns (these can be hatching, dotting or coloring). You can create area fills on the following elements: sketched elements, generated elements, part-sketched, part-generated elements. Define boundaries for your area fill by creating lines. The boundaries for your area fill may consist of both sketched and generated elements. In the Graphic Properties toolbar, click the down arrow besides

the Pattern icon. In the Pattern dialog box, select a pattern for your area fill and click OK.

Click the Area Fill icon from the Dress Up toolbar. The Area Detection dialog box appears. Click the Automatic option and then click inside the area for which you just defined

boundaries, under the line, which represents the fillet edge. The software automatically detects the area to fill based on where you clicked and fills this area with the selected pattern. The Areas to Fill dialog box disappears.

f) Creating Arrows

This task will show you how to create an arrow. For the purpose of this exercise, you will use an arrow to illustrate the kind of hole you want to apply to a circle. Click the Drawing window, and select Insert->Dress up->Arrow from the menu bar. Click a point or select an object to define the arrow starting point (the tail). Click another point or select another object to define the arrow extremity (the head). The arrow is created. The arrow and the selected object are associative. To modify the position of the arrow, click the arrow and use the yellow manipulators to drag it to its new location. To add a breakpoint to the arrow, select it and right-click on a yellow manipulator. A contextual menu appears. Select Add a Breakpoint. A breakpoint is added to the arrow; you can drag it to change the arrow path.