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7.Generative Drafting workbench

The Generative Drafting workbench provides a simple method to create and modify views on a predefined sheet. You may also add, modify and/or delete dressup and 2D elements to these views. All this is performed on a sheet which may include a frame and a title block and will eventually be printed.

7.1 Creating a New Drawing

This task will show you how to create more or less automatically a new drawing with pre-defined views generated from a part. Select the Start -> Mechanical Design commands. Select the Drafting

dialog box appears with information on views that can possibly be created, as well as information on the drawing standards. Select the views you want to be automatically created on your drawing from the New Drawing Creation dialog box. Click OK.

7.2 Managing A Sheet

The Generative Drafting workbench provides a simple method for managing a sheet. A sheet contains: a main view: a view which supports the geometry directly created in the sheet, a background view: a view dedicated to frames and title blocks, interactive or generated views. Click

the New icon from the Standard toolbar or select File -> New... from the menu bar. Select the Drawing workbench, and click OK. From the New Drawing dialog box, select the ISO standard, or the A0 ISO format. Select the orientation type. Select the 1:1 scale, and then click OK.

7.3 Adding a new sheet

You can add new sheets at any time. These new sheets will be assigned the same standard, format and orientation as the sheet first created and defined using the New Drawing dialog (default setting). Even though you then delete sheet1, the sheets newly created will keep the same name.

Click the New Sheet icon from the Drawing toolbar. The new sheet automatically appears.

7.4 Front View Creation

The Generative Drafting workbench provides a simple method to create views on a predefined sheet. What is the Active View? The active view is the view from which other views will be generated. This is also the view in which all the modifications will be performed. The active view is framed in red. The non-active views are framed in blue. When you create a view, until you click at the desired view location, the view to be created is framed in green. If you click this view, it becomes the active view and is framed in red.

Start creating the front view. Click the Front View icon from the Views toolbar. Select object. Click on sheet to place front view. Blue arrows appear. Click the right or left arrow to visualize the right or left side, respectively. Click the bottom arrow to visualize the bottom side. Click the counterclockwise arrow to rotate the reference plane. Click inside the sheet to generate the view. Right-click the frame of the view, select the Properties option from the contextual menu, View tab and check the required options in the Properties dialog box.

7.5 2D/3D Associativity

On Views: A generative view results from specifications in a 3D document. This specification corresponds either to the whole document or to a feature in the document. Any modification applied to the specifications, before the generated view(s) is/are updated, is detected. You can

perform an update. You can update all views or a selection of views. The Update icon is active in the Update toolbar when a sheet (or drawing) contains views that need to be updated (this can be all views in the sheet or some of them only). You can update all views in the active sheet by

clicking this icon. An update symbol appears in the specification tree for the views that need to be updated. You can update a selection of views by selecting and right-clicking the view(s) you

want to update and choosing Update Selection from the contextual menu.

On Generated Dimensions: Generated dimensions are associative with the 3D part constraints on the condition you checked the Generation dimensions when updating the sheet option from the Options dialog box (Tools -> Options -> Mechanical Design -> Drafting -> Generation tab). Note that these dimensions will be re-generated in accordance with the other options checked/un-checked in the Options dialog box.

7.6 Creating a Projection View

This task will show you how to create projection views on the sheet, relatively to the front view

previously generated. Click the Drawing window, and double-click the Projection View icon from the Views toolbar (Projections subtoolbar). As you move the cursor, a previewed projection view in a green frame appears on the sheet. Define the projection view position by positioning the cursor at the desired view location, for example the right view position. Click inside the green frame to generate the view.

7.7 Creating an Auxiliary View

This task will show you how to create an auxiliary view. Many objects are of such shape that their principal faces cannot always be assumed parallel to the regular planes of projection. Creating an auxiliary view allows showing the true shapes by assuming a direction of sight perpendicular to planes that are perpendicular of the curves. This auxiliary view, together with the top view,

completely describes the object. Click the Auxiliary View icon from the Views toolbar (Projections subtoolbar).

Click an edge on the view. The selected edge becomes a line that you can position where desired using the cursor. This line/callout will be automatically used as the plane. Click to position the callout. The reference plane is automatically positioned according to the selected edge. Positioning the auxiliary view callout amounts to defining the auxiliary view direction. Click to position the auxiliary view.

7.8 Creating an Offset Section View / Cut

This task will show you how to create an offset section view/cut using a cutting profile as cutting plane. In sectioning through irregular objects, it is often desirable to show several features that do not lie in a straight line by offsetting or bending the cutting plane. Click the Drawing window, and

click the Offset Section View icon or the Offset Section Cut icon from the Views toolbar (Sections subtoolbar). Select the holes and points required for sketching the cutting profile. If you

are not satisfied with the profile you create, you can, at any time, use Undo or Redo icons. The section plane appears on the 3D part and moves dynamically on the part. Double-click to end

the cutting profile creation. OFFSET SECTION CUT: In this particular case, only cut portion of solid is visible in section view.

7.9 Creating an Aligned Section View / Cut

This task will show you how to create an aligned section view and/or aligned section cut using a cutting profile as cutting plane. An aligned section view / cut is a view created from a cutting profile defined from non-parallel planes. In order to include in a section certain angled elements, the cutting plane may be bent so as to pass through those features. The plane and feature are then imagined to be revolved into the original plane. Click the Drawing window, and click the Aligned

Section Cut . Select the points and circles required for sketching the cutting profile. The section plane also appears on the 3D part and moves dynamically on the part. Double-click to end the cutting profile creation. Click to generate the view.

7.10 Creating a Detail View / Detail View Profile

A detail view is a partial generated view that shows only what is necessary in the clear description of the object. It shows you how to create from the 3D a detail view using either a circle as callout or a sketched profile. In this particular case, we create a detail view using a sketched profile as we create this detail view from an oblong part. Note that for creating a detail view using a circle, the

dialog is exactly the same. Click the Drawing window, and click the Detail View icon from the Views toolbar (Details subtoolbar). Click the callout center. Drag to select the callout radius and click a point to terminate the selection. Or, if you create a detail view using a sketched profile, you

will click the Detail View Profile icon . Create the points required for sketching a polygon used as profile. Double click to end the cutting profile creation. Click to generate the detail view. The default scale is 2 (twice the scale of the active view). You can modify this scale.

7.11 Creating a Clipping View and/or a Clipping View Profile

A clipping view is a partial view that shows only what is necessary in the clear description of the object. This operation is applied directly onto the active view. Here we will see how to create both a clipping view using a circle as callout. You can also use a roughly sketched profile. Click

the Drawing window, and click the Clipping View icon from the Views toolbar (Clippings subtoolbar). If you create a clipping view using a sketched profile, you will select the Clipping

Profile View icon . Select the center of the circle or select the required points for sketching a polygon. Double-click to end the cutting profile creation.

7.12 Creating an Isometric View

To produce an isometric projection, it is necessary to place the object so that its principal edges make equal angles with the plane of projection and are therefore foreshortened equally. Click the

Drawing window, and click the Isometric View icon from the Views toolbar (Projections 86

subtoolbar). Click the 3D part. A green frame with the preview of the isometric view to be created, as well as blue manipulators appear. You can re-define the view to be created position using these manipulators: to the bottom, the left, the right, the top, or rotated using a given snapping or according to an edited rotation angle.

7.13 Creating a Broken View

A broken view is a view that allows shortening an elongated object. Here we will see how create a broken view from an active and up to date generative view. We will define two profiles

corresponding to the part to be broken from the view extremities. Click the Broken View icon from the Views toolbar. Click a first point corresponding to the first extremity of the first profile. A green dotted profile appears which allows you to position the profile either vertically or horizontally. Click a second point corresponding to the profile second extremity. If needed, translate the profile. Red zones appear. Click a point for defining the position of the second green profile that appears. Click on the sheet.

7.14 Creating a Breakout View

Here we will remove locally material from a generated view in order to visualize the remaining visible internal part. A breakout view is one not in direct projection from the view containing the cutting profile. A breakout view is often a partial section. Click the Drawing window, and click the

Breakout View icon from the Views toolbar (Break View sub toolbar). Click the first point of the breakout profile. Click as many points as desired for creating the profile. Double-click to end the profile creation and automatically close this profile. Or Click on the profile first point to close and end the profile creation.

7.15 Creating Views via the Wizard

This task will show you how to create views using a wizard. These views are views that are generated automatically once the CATDrawing document is opened. Click the Drawing window,

and click the Wizard icon from the Views toolbar (Wizard subtoolbar). Select the desired view configuration from the View Wizard. Click next add any other view if required. Click the FINISH

87 button from the View Wizard. Select the CATPart document. Click on the desired 3D part plane to be used as reference plane The views now appear on the CATDrawing document: they are previewed in green frames and can be re-oriented thanks to the blue arrows that appear. Use the blue arrows to have the views re-oriented as desired. Once you are satisfied, click on the sheet to make the views be actually created.

7.16 Isolating Generated Views

This task will show you how isolate either a selection of generated views (one or more), or all views in the drawing. Isolating a view amounts to: suppressing associativity between an existing CATPart (or CATProduct) and the corresponding generated view, transforming a generated view into an interactive view. Select the views you want to isolate (for example, the Top view, Bottom view, Left view and Right view), and right-click them. From the contextual menu, select Selected objects -> isolate.

7.17 Not Aligning a View

This task will show you how not to align a right projection view to the parent front view. At creation, views are by default linked to the parent view. You will then reposition the parent view as well as the still-aligned child views. Right-click the frame of the view not to be aligned. Select the View Positioning -> Do Not Align View option from the displayed contextual menu. Select & Drag the left projection view to the required location. Click to position the left view.

7.18 Scaling a View

This task will show you how to modify the scale of a view. Right-click the frame of the view to be modified. In this case, right-click the detail view. Select the Properties option from the displayed contextual menu. Enter the new Scale value in the Properties dialog box. Click OK. The detail view is updated.

7.19 Adding a Generative Bill of Material

This task will show you how to insert Bill of Material information into the active view. This Bill of Material corresponds to information on the product element which the views were generated from. This Bill of Material, or parts list, consists of an itemized list of the several parts of a structure shown on a cat drawing or on an assembly. Click the Insert Bill of Material icon , if you are in the background view. Click the Product from the specification tree in the CATProduct document. Click the point at which the Bill of Material is to be inserted. Before positioning the Bill of Material, you can pre-define the position. To modify the contents of the Bill of Material and display given properties, go to Product Structure workbench, select from the menu bar: Analyze->Bill of Material ->Listing Report.

7.20 Generating Balloons on a View

This task will show you how to generate in the active view balloons corresponding to references defined on the different parts of an assembly. Double-click the view in which you want to generate the balloons. In this particular case, double-click the front view. This view is now active. Select the

Generate Balloons icon on the Dimension Generation toolbar. The balloons that were previously created on the CAT Product are automatically generated onto the active view. If needed, multi-select these balloons and modify the font size from the Text Properties toolbar. You can also select and drag a balloon to change its position. Balloons generated

7.21 Modifying a Callout Geometry

This task will show you how to modify the geometrical characteristics of a callout used when creating detail views, section views and section cuts. For modifying the detail and section callout, you will go through some kind of a sub-workbench and modify the existing callout geometry, reverse the callout direction or replace the callout. Double-click the callout to be modified. The Edit/Replace toolbar appears. Drag one of the element components to the desired location. Click

the End Profile Edition icon from the Edit/Replace toolbar. After the callout arrow is properly positioned, the section view is automatically updated.

7.22 Modifying a Pattern

This task will show you how to modify the pattern of a view and apply a material to this pattern. You can recover a material applied to a part on the section view pattern. Right-click the pattern to be modified. Select Properties from the displayed contextual menu. The Properties dialog box displays the view current pattern. Select Pattern table switch and select a new pattern from the Pattern table that appears. Then click OK in this Pattern table. Click OK in the Properties table to confirm your operation. You can also customize different hatching types by entering the desired values in the box called Hatching.

7.23 Dimension Generation

The Generative Drafting workbench provides a simple method for generating dimensions. Generated dimensions are associative to the elements created from a part or an assembly. Note that for views that are generated from surfaces, only sketched constraints are generated. The generated dimensions are positioned according to the views that are most representative. The generated dimensions will be positioned according to the following criteria:

0. On the view for which the dimension are generated.

0. On the view on which the dimension is better visualized. For example, a view on which elements are visualized in non-hidden lines instead of hidden lines.

0. On the view with a bigger scale.

0. On views including more dimensions.

What About the Dimensions that may be Generated from Constrained 3D Elements

Constrained 3D Elements Generated Dimension Types

Sketcher All dimensions: angle, distance, radius, diameter 3D part Angle, distance

Features: The dimensions below: Pad distance Pocket distance Shaft/Groove angle

Hole Constraints and associated dimensions Fillet constraint variable Radius/Radii

Shell Distance Thickness Distance Stiffener Distance

Assembly constraints All assembly dimensions

7.23.1 Generating Dimensions in One Shot

This task will show you how to generate dimensions in one shot from the constraints of a 3D part. Only the following constraints can be generated: distance, length, angle, radius and diameter. Constraints may be of three kinds: created manually (i) via the sketcher or (ii) via the 3D part, or

else (iii) automatically created via internal parameters. Click the Generating Dimensions icon from the Generation toolbar (Dimension Generation subtoolbar). In the case of drawings with several views, by default, dimensions are generated on all the views. The Generated Dimensions Analysis dialog box showing the dimensions and constraints generated for each part (in this case, there is only one) is automatically displayed. Click OK to close the dialog box.

7.23.2 Generating Dimensions Semi-Automatically

This task will show you how to generate dimensions step by step from the constraints of a 3D part.

Click the Generating dimensions step by step icon from the Generation toolbar (Dimension Generation subtoolbar). The Step-by-step generation dialog box displays and will remain displayed until the end of the dimension generation. Check the Visualization in 3D & Timeout options. Click

the Next Dimension Generation switch button to start the dimension generation. Dimensions appear one after the other on the views.

Click the Not Generated option , constraint is automatically excluded and the dimension will

not generated. Note that you can stop at anytime the generation by clicking or, on the contrary,

accelerate the process by clicking

7.24 Creating a Datum Feature

This task will show you how to create a datum feature. Click the Datum Feature icon from the Dimensioning toolbar. Select the point at which you want the datum feature to be attached (attachment point). Select the point at which you want the datum feature to be anchored (anchor point). The Datum Feature Creation dialog box is displayed with A as default value (incremental value). Enter the desired character string, if needed. Click OK. The datum feature is created.

7.25 Creating a Geometrical Tolerance

This task shows you how to create a geometrical tolerance (annotation). You can also copy an existing geometric tolerance. You can set text properties either before or after you create the text.

Click the Geometric Tolerance icon from the Dimensioning toolbar. Select an element (geometry, dimension, text or point) or click in the free space to position the anchor point of the geometrical tolerance. If you select an element, the anchor point will be an arrow. If you select a point in the free space, the anchor point will be a small balloon. If you select a dimension or a text, no leader will be created. The geometric tolerance will be displayed just below the element you selected. Move the cursor to position the geometrical tolerance and then click at the chosen location. The Geometrical Tolerance dialog box appears. Specify the tolerance type by clicking the Tolerance Symbol button and selecting the appropriate symbol. Click OK when you're done. The geometrical tolerance is created.

7.26 Annotations

7.26.1 Setting Text Properties

This task explains how to set the properties of a text, such as font style, size, justification, etc. Text properties can be applied to text, dimension text, text with leader, balloon and datum target, as well as to text included in datum features and geometrical tolerances. You can set the properties of a text either before or after creating it. Choose View -> Toolbars, and select Text Properties.

The Text Properties toolbar is displayed. Set the properties of a text.

7.26.2 Creating a Text With a Leader

This task shows you how to create a text with a leader either in the free space or associated with an element. You can set text properties either before or after you create the text. Click the Text With

Leader icon from the Annotations toolbar. Click the point on the element you want the leader to begin (arrow end). A red frame appears. Click in the free space to define a location for the text. If needed, drag the frame and/or arrow to a new location. The Text Editor dialog box is displayed. Enter the text in the Text Editor dialog box or directly on the drawing.

7.26.3 Creating a Balloon

This task will show you how to create a balloon. You can set text properties either before or after

you create the text. Click the Balloon icon from the Annotations toolbar (Text subtoolbar). Select an element. Click to define the balloon anchor point. The Balloon Creation dialog box appears; with the value 1 is pre-entered in the field. You can enter another string or value as needed. Click OK.

7.26.4 Creating Associative Balloons on Generated Product Views

This task will show you how to create associative balloons on views generated from a product. Open any CATProduct document. On this CATProduct document, Product Structure sub products have already been assigned numbers (Generate Numbering icon). Go to Generative Drafting workbench by opening CATDrawing document for same assembly product. Click the Balloon icon

from the Annotations toolbar. Go over one of the part with your cursor. Create a balloon by selecting an edge. The number of the balloon corresponds to the number of the subproduct created in the product which the views were generated from. Note that if you modify the numbering in the product and then regenerate the product, the balloon modification will be applied to the generated views only after you perform a view update.

7.26.5 Creating a Roughness Symbol

This task will show you how to create a roughness symbol. You can set text properties either

before or after you create the roughness symbol. Click the Roughness Symbol icon from the Annotations toolbar. Select the attachment point of the roughness symbol. The Roughness Symbol Editor dialog box is displayed. Enter values in the desired field(s). For example, Ra=1.6. Click OK. If needed, modify the roughness symbol position by dragging it to the required location. Click in the free space to validate the roughness symbol creation.

7.26.6 Creating a Welding Symbol

This task will show you how to create a welding symbol. You can set text properties either before

or after you create the text. Click the Welding Symbol icon from the Annotations toolbar. Select an element or click in the free space to position the anchor point of the welding symbol, and then click to validate. The welding leader will appear. Move the cursor to position the welding symbol and then click at the chosen location. The Welding creation dialog box is displayed. Type the desired values in the upper and/or lower field(s). Click the symbol buttons to choose the welding symbol, complementary symbols and/or finish symbols. The welding symbols available depend on your standard. Click OK. The welding symbol is created.

7.26.7 Creating a Geometry Weld

This task will show you how to create a geometry weld. Click the Weld icon from the Annotations toolbar. Select the two elements. The geometry default weld symbol automatically appears on the drawing. The Welding Editor dialog box is displayed. If needed, modify the geometry-welding symbol. If needed, modify the type of the geometry-welding symbol by selecting the Change Type option from the Welding Editor dialog box. Click OK.

7.26.8 Creating/Modifying a Table

This task shows you how to create and edit a table. In this table, you can add text, insert columns, rows, merges cells, invert lines, invert columns, switch lines and columns, and insert views. You

can also split a table, import a table, and insert a view in a table. Click the icon

to launch the command. Click a point in the drawing to choose the table position. The following panel allows you to set the number of columns and rows you want for the table. The line height corresponds to the height of a string. The line width corresponds to 5 times a string height. Click ok to validate the creation.

7.27 Editing Properties

This section discusses how to quickly access and edit information on 2D geometry, dress-up elements, annotations and dimensions in a single dialog box, provided you use the Edit->Properties contextual command.

a) Editing View Properties

This task explains how to edit view properties. Right-click on the front view and select properties. Choose the View tab. Choose your options. Visualization and behavior: Display view frame: show/hide the view frame, Lock view: if you check this option, no more modification allowed in the view. Visual clipping: let’s you reframe a view so as to display only part of it. Scale and Orientation Angle: the angle between the view and the sheet, Scale: the scale of the view. Dress up: Hidden lines, Center line, 3D spec, Axis, Thread, 3D Wireframe, 3D Colors, Fillets, 3DPoints. View Name: Allows you to modify the name of the view. Among other things, you can create a formula for the view name.

b) Editing 2D Geometry Graphic &Feature Properties

This task shows you how to access and, if needed, edit information on 2D geometry features (name and stamp). Select a 2D element on the CATDrawing you opened. Select the Edit->Properties command and click the Feature Properties tab. You can also right click the 2D element and then select the Properties command from the displayed contextual menu. Click the Graphic Tab, Lines and Curves option; Pickable option and Layers options are available for changing graphic properties. Click OK.

c) Editing Annotation Font Properties

This task explains how to access and, if needed, edit annotation font properties. Double-click the text to switch it to edit mode. Select the whole text (you can also select only part of the text) and then select the Edit-> Properties command. In the Properties dialog box that appears, click the Font tab. The associated panel is displayed. Change Annotation Font Properties as per requirement.

d) Editing Dimension Text Properties

This task explains how to access and, if needed, edit dimension text properties. Select a dimension (whatever the type) on the CATDrawing you opened. Select the Edit-> Properties command and click the Dimension Texts tab. Modify the available options.

f) Editing Dimension Value Properties

This task explains how to access and, if needed, edit dimension value properties. Select a dimension (whatever the type) on the CATDrawing you opened. Select the Edit-> Properties command and click the Value tab. Modify the available options. Fake Dimension: check this option to display fake dimensions, you can choose to display numerical or alphanumerical fake dimensions.

7.28 Customizing for Generative Drafting

a) General Settings

This task shows you how to set general settings to be used in the Drafting workbench. Select the Tools->Options command. The Options dialog box appears. Ruler: Checking the Show Ruler option displays the ruler in your sheet. It means you visualize thecursor coordinates as you are drawing.

Grid: To define your grid, enter the values of your choice in the Primary fields. The Primary spacing option lets you define the spacing between the major lines of the grid. The Graduations field lets you set the number of graduations between the major lines of the grid, which actually consists in defining a secondary grid. The Display option allows displaying the grid in your session. The Snap to point option needs be checked if the geometry needs to begin or end on the points of the grid. Rotation: The Rotation Snap Angle option allows snapping with a given angle for rotating elements. This option is used to rotate text elements (text, frame, or leader). In other words, it defines the snapping value used when rotating an element using the Select or Rotate commands. Colors: You can customize given options for modifying the drawing background color. Tree: You can display or not parameters and relations in the specification tree. View axis: When you activate a view, you can choose to visualize the view axis. In addition, you can define whether these axes can be zoomed.

b) Dimension Creation

You can customize given options when creating or re-positioning dimensions. Select the Dimension tab in Options. Dimension Creation: Dimension following the mouse (ctrl toggles): you can decide that the dimension line is positioned according to the cursor, following it dynamically during the creation process. Constant offset between dimension line and geometry: the distance between the created dimension and the geometry remains the same when you move the geometry. Default dimension line/geometry distance: if you position the dimension according to the cursor, you can define the value at which the dimension is created. If you create associativity between the dimension and the geometry, you can define the value at which the dimension will remain positioned. If you click the Associativity on 3D switch button the following dialog box appears: A link can be applied between a dimension and the 3D part. As a result, when you update the drawing, the dimension is automatically re-computed. Create driving dimensions: the dimension you will create will drive the geometry.

Move: The Configure switch button allows you to choose either the dimension to be snapped on the grid or/and the dimension value to be located at its default position between symbols (it will work only if the cursor is between the symbols). Line-Up: You can organize dimensions into a system with a linear offset. The offset will align the dimensions to each other as well as the smallest dimension to the reference element. Analysis Display Mode: Colors can be customized with the Activate analysis display mode option. To activate this mode, select this option and then click the Types and colors button. The Types and colors of dimensions dialog box lets you assign the desired color(s) to the selected dimension types.

c) Geometry and Dimension Generation

You can customize given options for controlling geometry and dimension generation whenever you need to update sheets. Select the Generation tab. Geometry generation / Dress up: The following geometry is possibly generated (provided you check the desired options using the contextual menu, Properties option, View tab): Generate axis, Generate threads, Generate centerlines, Hidden lines, Generate fillet, 3D colors inheritance, Project 3D wireframe, Project 3D points, Apply 3D specification. Dimension generation: The generated dimensions are positioned according to the views most representative. The dimensions are generated on the views on the condition the settings were previously switched to the dimension generation option. Generate dimensions when updating the sheet , Filters before generation, Automatic positioning after generation, Allow automatic transfer between views, Analysis after generation, Generate dimensions from parts included in assembly views, Delay between generations for step-by-step mode, Balloon generation: If you select Creation of a balloon for each instance of a product, a balloon will be generated for each instance of a component: therefore, if a component is used two times within a product, then the balloon will be generated twice.

d) Geometry Creation

You can customize given options when creating 2D geometry, either or not using SmartPick, or still adding constraints to this geometry. Select the Geometry tab.

Geometry: You can decide that you want to create circle and ellipses centers and that you want to be able to drag elements, end points included. Constraints creation: You can create or not the geometrical or dimensional constraints detected by the SmartPick tool. If all of the detection options are unchecked, the Create detected constraints option is not available.SmartPick: (switch button) As you create more and more elements, Smart Pick detects multiple directions and positions, and more and more relationships with existing elements. The SmartPick category provides these options: Support lines and circles, Alignment, Parallelism,perpendicularity and tangency, Horizontality and verticality. Constraints Visualization: Check the Visualize constraints option to visualize the logical constraints specific to the elements. Colors: Two types of colors may be applied to sketched elements. These two types of colorscorrespond to colors illustrating: Graphical properties-Colors that can be modified.

Constraint diagnostics- Colors that represent constraint diagnostics are colors that are imposed to elements whatever the graphical properties previously assigned to these elements and in accordance with given diagnostics. Over-constrained elements: the dimensioning scheme is over-constrained: too many dimensions were applied to the geometry. Inconsistent elements: At least one dimension value needs to be changed. This is also the case when elements are under-constrained and the system proposes defaults that do not lead to a solution. Not-changed elements: Some geometrical elements are over-defined or not consistent. As a result, geometry that depend(s)on the problematic area will not be recalculated. Iso-constrained elements: All the relevant dimensions are satisfied. The geometry is fixed and cannot be moved from its geometrical support.

If you click the other color of the elements switch button, the following dialog box appears. Isolated elements: use-edge that no more depends on the 3D. Protected elements: non-modifiable elements. Construction elements: A construction element is an element that is internal to, and only visualized by, the sketch. This element is used as positioning reference. It is not used for creating solid primitives. SmartPick: colors used for SmartPick assistant elements and symbols.

e) View and Sheet Layout

You can customize given options when creating views or when adding sheets. Select the Layout tab. It contains the following sets of options: View creation: When creating a view, you can define that you want or not the view name, scaling factor or frame to appear, and that you want broken and breakout specifications to be reproduced. New sheet: You can define that when creating a new sheet, you want the source sheet to be the first or one sheet from another drawing. Background view: You can specify the path to the directory-containing frame and title block. Section/Projection Callout: You can choose the callout elements size not to be dependant on theview scale. For this before callout creation check this option.

f) Annotations

You can customize given options when creating annotations. Select the Annotation tab. It contains the following sets of options: Annotation Creation: Select the items you want to snap: text and/or leader. Snapping will be performed when the Activate Snapping box is checked, taking into account the option selected in the Activate snapping dialog box Move: Select Activate Snapping to activate snapping. Click the Configure button to specify whether you want the annotation to be snapped on the grid, according to the orientation, or both. This will apply to the annotations selected in the Annotation Creation area. To deactivate snapping when creating or moving annotations, press the shift key. 2D Component Creation: Select Create all 2D component instances with the same size if you want all 2D component instances to have the same size when you create them, no matter what the view scale is.

7.29 Loading/Saving a CATDrawing

This task will show you how to load and save a CATDrawing document from an existing CATPart document. In this particular case, all the links that exist between the CATPart document and the CATDrawing document will be resolved, as you will choose to load the referenced document. You can now modify your CATPart choosing not to update the related CATDrawing document. It is now possible to customize the settings. Activate the settings. For this: Select the Tools -> Options... command. Click General in the list of objects to the left of the Options dialog box (General tab). Make sure the Load referenced documents option (default option) is actually checked. Press OK. Open the CATDrawing document for your CATPART document. Make sure the specification tree actually appears. Make sure the symbols are not broken which would means that links between the CATPart and the projection views are unresolved. Select the Edit->Links command. The Links dialog box appears with the existing links between the CATDrawing and its related CATPart. Press OK.

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