Copyright DASSAULT SYSTEMES Interactive Drafting CATIA Training Foils Version 5 Release 8 January 2002 EDU-CAT-E-ID1-FF-V5R8

Copyright DASSAULT SYSTEMES Table of Contents (1/2) 1. Introduction to Generative Drafting Interactive Drafting Workbench Presentation 2. Drawing the Front View Starting a Drawing Drawing Geometry 3. Adding Projection Views and Sections Adding Projection Views 4. Editing Views Layout and Properties Editing Properties: at Drawing, Sheet and View Level Moving Views and Adding Sheets Modifying a Section Hatching Representation 5. Dimensioning and Annotating Linear and Angular Dimensions Radius and Diameter Dimensions Chamfer Dimensions Thread Dimensions Hole / Coordinate Dimensions Half Dimensions System Dimensions Dimension Properties Adding Tolerances, Fits and GD&T Adding Symbols

Copyright DASSAULT SYSTEMES Table of Contents (2/2) 6. Finalizing the Drawing and Printing Create Texts Adding a Note View Adding a Title Block Printing 7. Setting Drafting Options Drafting Options and Generating Views 8. Saving a Drawing Document Saving a Drawing

Copyright DASSAULT SYSTEMES Introduction to Interactive Drafting In this lesson, you will learn about the Interactive Drafting Workbench by Interactive Drafting Workbench Presentation

Copyright DASSAULT SYSTEMES Interactive Drafting Workbench Presentation You will learn about the Interactive Drafting Workbench by : Understanding the general process Accessing the Workbench Exploring the User Interface and Terminology

Copyright DASSAULT SYSTEMES B - Dimension and Annotate View(s) Interactive Drafting - A - Create View(s) and Geometry Complete the Title Block The Generative Drafting workbench and Interactive Drafting workbench are exactly the same. However, the Generative Drafting workbench activates additional tools allowing the generation of the views geometry and dimensions from the 3D automatically. General Process Part Design Assembly Design Sketcher Associative link Available only with Generative Drafting workbench

Copyright DASSAULT SYSTEMES Blank sheet to start You can access the drafting workbench anywhere from : The Start menu The File menu 1 2 Accessing the Workbench

Copyright DASSAULT SYSTEMES Drawing 2 - Dimensioning 3 - Annotations 6 - Geometry Modification 4 - Dressup 5 - Geometry Creation On the right, view creation tools, tools for dimensioning & annotating views On the top and bottom, standards for dimensions, text & geometry Drafting Toolbars and Objects Dimension properties Text properties Graphic Properties

Copyright DASSAULT SYSTEMES Drafting Terminology View Frame Grid Active view (underlined in the tree and with a red frame) Specifications Tree Views Prompt zone

Copyright DASSAULT SYSTEMES Drafting (P2 Power Tools) Magnifier (on) Ø(View Menu) Drawing Overview (on)

Copyright DASSAULT SYSTEMES You had a quick tour of the process to create the views of a 3D part and how the access the Generative Drafting workbench You have seen the general layout of the user interface, terminology and the basic principles. In this introduction to the Generative Drafting Workbench, To Sum Up …

Copyright DASSAULT SYSTEMES Drawing the Front View In this lesson you will create a Front view and draw the geometry in that view Starting a Drawing Starting the Front View Drawing Geometry

Copyright DASSAULT SYSTEMES Starting a Drawing You will start a drawing.

Copyright DASSAULT SYSTEMES A CATDrawing file contains a structure listing of all the sheets and views contained in the document. A Drawing Document is a file that is also called a CATDrawing and is identified by its file extension (.CATDrawing). CATDrawing file extension identification. What is a Drawing?

Copyright DASSAULT SYSTEMES Select File + New + Drawing + OK When starting a drawing, you need to define the projection standard : ISO, ANSI or JIS (A) (C) (B) (D) (E) (F) ISO, ANSI and JIS standards are available. They will determine the default position of the projection views with respect to the front view as well as the dimensioning standard ANSI (3 rd Angle) ISO (1 st Angle) Drawing Projection Standard 1

Copyright DASSAULT SYSTEMES Un-Check this option to hide the black frame representing the paper format when ready to print The format setting can be modified later if necessary using the File + Page Setup menu Paper Sheet Size The following items maybe also be set: Standard (ISO, ANSI, etc…) Paper formats (A, B, C, or A0, A1, A2, etc..) Orientation (Landscape or Portrait) Sheet scale (1:1 is default and should only be changed with caution)

Copyright DASSAULT SYSTEMES Select the New View icon When a drawing document is created, a front view must be added before starting to create geometry. Place the view by clicking on the sheet Remember that you can use F3 to hide the specification tree on the left and display it again when ever necessary The Front view is added in the tree and on the Sheet. Displayed with a blue HV reference axis and a view frame View frame : By default, a view frame is displayed and always fits the content of the view and changes with it Starting the Front View 1 2

Copyright DASSAULT SYSTEMES Drawing Geometry You will draw basic drafting geometry

Copyright DASSAULT SYSTEMES Traditional tools are available to create and trim simple geometry such as point, line, curve, corner, trim, etc… The tools used to create and trim geometry are presented in the following foils. An overview of these tools is presented here. Points:Line: Create by clicking or keying in any field of the following: Circles and Curves:Relimitations: How to Create and Trim Simple Geometry ?

Copyright DASSAULT SYSTEMES Select the Coordinate Point icon Use the Coordinate Point icon to create a point relative to the origin. Use the Coordinate Point icon to create a point relative to an existing point. Select the Coordinate Point icon again Use the tab key to keep the cursor in the desired sector. Select the point created in step 2 as a reference point Key values of h = 50, v = 0 You will get : Key values for h and v which are relative to the active view origin (shown in blue) 2 5 Coordinate Points 50

Copyright DASSAULT SYSTEMES Select the Equidistant Point icon Use the Equidistant Point icon to create a defined number of new points along a supporting line or curve with a defined spacing. Select the line as a support for the points to travel along Key the Spacing distance (10 mm) and the number of New Points (10) Example Results : 10 new points that are equally spaced from the origin to the end of the 10mm line Select a reference point to begin the equidistant point spacing Equidistant Points

Copyright DASSAULT SYSTEMES Create intersection points between two lines Intersecting elements Intersection points Select the Intersection Point icon Select the intersecting elements 1 2 Example results: Point by Intersection

Copyright DASSAULT SYSTEMES Project one or several points (Ctrl key) onto a element Points to be projected Projected points Element on which the points will be projected Select the Projection Point icon Select the points to project 1 2 Select the element on which to project 3 Example results: Points will be projected perpendicular to the projection element Point by Projection

Copyright DASSAULT SYSTEMES Click anywhere (with or without the grid) to define the second point, the segment is created Select the segment icon If you see a blue segment before defining the second point, you are sure that the segment is perfectly aligned with the horizontal or vertical view axis Click anywhere (with or without the grid) to define the first point Drawing a Line Segment with the Mouse or

Copyright DASSAULT SYSTEMES Parallelism detection When drawing a line segment, the system is able to detect automatically the possible constraints between the segment you are drawing and the existing elements Perpendicularity detectionPoint ON a segment Point ON an extremityPassing through the center Aligned on an extremityTangent to a circle If a segment has been drawn with Create Detected Constraints ( ) on, the constraint are kept. In case of modification the constraints are still applied Automatic Detection of Constraints When Drawing a Line Segment

Copyright DASSAULT SYSTEMES Select the segment icon The first or the second point can be defined by a simple click in the view (A) Enter the first point : A : Horizontal coordinate B : Vertical coordinate (B) (A) Enter the second point : A : Horizontal coordinate B : Vertical coordinate (B) Depending on the customization of your Drafting workbench, the Tools bar may need to be dragged out of the bottom of the workbench to see the entry fields. Drawing a Line Segment by Keying Coordinates Use the TAB key to move between the options and press the ENTER key to confirm

Copyright DASSAULT SYSTEMES Select the segment icon The first point can be defined by a simple click in the view (A) Enter the first point : A : Horizontal coordinate B : Vertical coordinate (B) (A) Enter the Length and the Angle : A : Length B : Angle (B) The angle is defined with reference to the horizontal view axis and orientated in the counterclockwise direction Drawing a Line Segment by Giving a Length and an Angle Use the TAB key to move between the options and press the ENTER key to confirm

Copyright DASSAULT SYSTEMES Create horizontal or vertical infinite line passing through a point or an oblique infinite line passing through two points Horizontal Line Vertical Line Infinite Line Line Through Two Points Select the Infinite Line icon Select the desire option: Horizontal Vertical Through two points 1 2 Select a location 3a Select a location 3b Select 1 st point location 3c Select 2 nd point location 4 Infinite Lines

Copyright DASSAULT SYSTEMES Create Bisect line by bisecting an infinite line between two lines Note: the bisecting line corresponds to a line symmetrically constrained to the two lines. If both selected lines are parallel to each others, a new line will be created between these lines. Select the 2 nd line to bisect Select the Bisect Line icon Select the 1 st line to bisect Example results: Bisect Lines

Copyright DASSAULT SYSTEMES icons under the circle icon allow you to draw circles in different ways: A - by entering a center and a radius B - by giving three points C - by the center coordinates and the radius D - by three tangent lines E - by defining an ellipse B E Circles and Ellipses A C D

Copyright DASSAULT SYSTEMES Select the circle icon Click anywhere (with or without the grid) to define the point the circle is going to pass through Click anywhere (with or without the grid) to define the center of the circle Drawing a Circle by Defining its Center and a Point 1 2 3

Copyright DASSAULT SYSTEMES Center aligned on a point When drawing a circle, the system is able to detect automatically the possible constraints between the circle (or the center) you are drawing and the existing elements Center on a lineCenter on a point Circle passing through a point Tangent to a circle If a segment has been drawn with Create Detected Constraints ( ) on, the constraint are kept. In case of modification the constraints are still applied Tangent to a segment Automatic Detection of Constraints When Drawing a Circle

Copyright DASSAULT SYSTEMES (A) Enter the center Horizontal (A) and vertical (B) coordinates and the radius then select OK (C) (B) Select the circle using coordinates icon The default option to define the center point is the Cartesian option. You can use the Polar option instead. (C) Drawing a Circle Using Coordinates 1 2

Copyright DASSAULT SYSTEMES Instead of entering the radius, you can define the coordinates of a point the circle is going to pass through. You can define this point with the mouse or by its coordinates (A) Enter the center : A : Horizontal coordinate B : Vertical coordinate (B) Enter the radius and press Enter Select the circle icon Drawing a Circle by Giving its Center Coordinates and a Radius Use the TAB key to move between the options and press the ENTER key to confirm

Copyright DASSAULT SYSTEMES Enter the first point : A : Horizontal coordinate B : Vertical coordinate (A) (B) (A)(B) Select the Three point circle icon Enter the second point : A : Horizontal coordinate B : Vertical coordinate Enter the third point : A : Horizontal coordinate B : Vertical coordinate You can replace one of the points by entering a radius. In this case you will draw a circle passing through 2 points with a given radius. (A) (B) Drawing a Circle Passing Through Three Points Use the TAB key to move between the options and press the ENTER key to confirm

Copyright DASSAULT SYSTEMES Click on the first geometric element Select the Tri -tangent circle icon Click on the second geometric element Click on the third geometric element to create the circle Drawing a Tri Tangent Circle

Copyright DASSAULT SYSTEMES (A) Enter the Ellipse center : A : Horizontal coordinate +Tab B : Vertical coordinate +Tab +Tab (B) (A) (B) Select the ellipse icon Enter the ellipse major semi axis end point : A : Horizontal coordinate B : Vertical coordinate Enter a point on the ellipse : A : Horizontal coordinate B : Vertical coordinate Instead of defining the major semi axis end point coordinates, you can enter the length of this semi axis and the its angle according to the horizontal view axis. (A) (B) Major semi axis Minor semi axis Drawing an Ellipse Use the TAB key to move between the options and press the ENTER key to confirm

Copyright DASSAULT SYSTEMES Creating a Conic: Five Points Select Curves icon in the Geometry Creation toolbar then Creates a Conic in Curves sub-toolbar Select the conic first point (A) You can create a conic passing through five points. According to the point position, you will get different kind of conics Select the conic last point (B) Select a point (C) Select a point (D) Select a point (E) (A) (B) (C) (D) (E) Example Results:

Copyright DASSAULT SYSTEMES Creating a Conic: Four Points and a Tangent You can create a conic passing through four points and by defining a tangent direction on the first or last point of the conic Example Results: Select the First Tangent icon in the Tools toolbar Click to define the tangent direction Select the conic last point Select a point Select Curves icon in the Geometry Creation toolbar then Creates a Conic in Curves sub-toolbar Select the conic first point (A) (B) (C) (D) (E)

Copyright DASSAULT SYSTEMES Creating a Conic: 3 Points and 2 Tangents You can create a conic passing through three points and by defining two tangent directions on the first and last point of the conic Click to define the tangent direction Select a Point Select Curves icon in the Geometry Creation toolbar then Creates a Conic in Curves sub-toolbar Select the conic first point Select the First Tangent icon in the Tools toolbar Click to define the tangent direction Select the conic last point Select the Second Tangent icon in the Tools toolbar Example Results: (A) (B) (C) (D) (E)

Copyright DASSAULT SYSTEMES Creating a Conic: Tangents Creation When creating a conic, you can define the first and second tangent separately or simultaneously Using this icon, define the first and the second tangent simultaneously by defining the intersection point between both tangent directions Using these two icons, define the first and the second tangent separately

Copyright DASSAULT SYSTEMES Create connect curves with a tangent arc Create connect curves with a tangent spline The point at which you perform these selections is highly important. They correspond to the spline starting and ending points. Select a curve 2 3 Example Results: Select Connect curve and tangent arc icon 1 Select a curve 2 3 Example Results: Select Connect curve and tangent spline icon 1 Connect curves

Copyright DASSAULT SYSTEMES (A) (B) Place the cursor in the desired sector Select the Corner icon Use the Corner icon to draw an arc tangent to two elements. Use the Trim options palette to control the ends of the elements after the corner Select the elements on which you want to add a corner Key the radius Trim both lines Trim the first selected element No trim Using the TAB key will keep the cursor in the desired sector while entering a radius value and pressing ENTER key to confirm. You can also key the radius value before selecting the elements to corner. Trim options: Corners

Copyright DASSAULT SYSTEMES (A) (B) Place the cursor in the desired sector Select the Chamfer icon Use the Chamfer icon to draw a line across two elements. Use the Trim options palette to control the ends of the elements after the chamfer Select the elements on which you want to add a corner Trim both lines Trim the first selected element No trim Using the TAB key will keep the cursor in the desired sector while entering a radius value and pressing ENTER key to confirm. You can also key the radius value before selecting the elements to corner. Trim options: 1 2 Chamfer (1/2)

Copyright DASSAULT SYSTEMES Length/Angle option: Length1/Length2 option Length1/Angle option: Select the desired creation option: Length/Angle, Lenght1/Length2, Lenght1/Angle 3 Using the TAB key will keep the cursor in the desired sector while entering a radius value and pressing ENTER key to confirm. You can also key the radius value before selecting the elements to corner. Key Length and Angle 4a Key Length 1 and Length 2 4b Key Angle and Length 1 4c Chamfer (2/2)

Copyright DASSAULT SYSTEMES Select the trim icon Trimming is used to erase a portion of an element when 2 elements intersect at a crossing point called breaking point. Select the elements to trim(A, B) then indicate the sector to be kept (C). Trim options : Trim all elements Trim the first element (A) (C) (B) 1 2 Trimming Elements Example results:

Copyright DASSAULT SYSTEMES Select the Break icon Select the element to be broken (A) then select the breaking element (B) Example results: two lines (L1 and L2) split at element B: (A) (B) Use break to split (break) one element into 2 independent segments by another element Breaking Elements 1 2 (B) (L1) (L2)

Copyright DASSAULT SYSTEMES Select the trim icon 1 Once trimmed, a circle, ellipse, or spline can be returned to the original shape by the close option. Click on the trimmed element in order to it recover his original shape 2 In the Tools toolbars, select the close icon. 3 Trimmed circle: Trimmed spline:Un-Trimmed (closed) spline: Closing Elements Un-Trimmed (closed) circle:

Copyright DASSAULT SYSTEMES Quick Trim deletes a portion of element between two other elements, or keeps a portion of an element between two other elements, or splits (breaks) an element by two elements which cross it Deletes Keeps Breaks Quick Trim The position of selection determines where to delete, keep or break Select the trim icon 1 Select the Quick trim option 2 Select the element to be trimmed 3 Example results Quick Trim

Copyright DASSAULT SYSTEMES A typical approach in sketching consists of creating some precise elements but mostly approximate ones which are made precise later. Creating a very efficient approach. This approach consists of three steps: Profile Creation - the creation of a shape mostly by approximating the size Creating Sketch Constraints - create controlling dimensions and impose geometric constraints such as tangency. Editing Constraints - edit controlling dimensions to make the size of the sketch precise Sketching is the ability to create any 2D shape using one tool. The Profile icon is capable of creating contiguous lines and curves while providing sketch direction such as vertical & horizontal, and relationships between elements such as tangency and perpendicularity. A sketch is a rough drawing by nature however it is possible to create precise elements. Sketching...

Copyright DASSAULT SYSTEMES There are several sketching aides available in menu TOOLS + OPTIONS + DRAFTING in the General and Geometry tabs. Using these aides will minimize the need to Edit Constraints to make the sketch precise. The Allow Distortions option allows independent changes to the scale of H and V on the grid Sketching Aides

Copyright DASSAULT SYSTEMES Select the Profile icon Profile icon helps eliminate the use of multiple icons such as line, curve and trim. Profiles do not need to be created precisely which speeds up sketching. (a) (2) Select the Tangent Arc icon Click to create the arc when it is inline with the vertical axis. Click on the origin to close the profile. Example results : Profile Creation 1 Enter values for the First Point, Length and Angle. 2 Enter values L: 50mm & A: 90deg 3 Click to create angle (A) and click again to create a horizontal line (B). Blue indicates horizontal. (A) (B)

Copyright DASSAULT SYSTEMES Select the vertical line (A) and arc (B), then select the Constraint icon and tangency (C) A profile can be constrained by keying values during creation, creating controlling dimensions which can be edited, or with geometric constraints such as tangency used to establish geometric relationships which can be created manually or implicitly. Create dimensions to constrain the profile: (A) Length of lower horizontal line (B) Distance between horizontal lines (C) Radius (D) Angle of chamfer relative to vertical (E) Distance of chamfer width relative to right side of profile and chamfer point (A) (B) (C) (A) (B) (C) (E) (D) Implicit constraints such as h (horizontal and v (vertical) were a result of having the Created detected Constraints icon ( ) active during Profile Creation. To dimension the elements select and the element(s) and indicate a location 1 2 Creating Sketch Constraints

Copyright DASSAULT SYSTEMES Creating Explicit Geometrical Constraints Note: A predetermined Geometric Constraint will be displayed (in dim letters) next to the cursor. If this is the desired constraint, select the drawing background to confirm. Explicit Geometric Constraints can be created between sketched elements or between sketched and generated geometry. Select the Geometric Constraint icon 1 Select the element(s) to Geometric Constrain 2 Using the contextual menu (mouse button 3), Select the Geometric Constraint 3

Copyright DASSAULT SYSTEMES Notice the vertical dimension changed and the horizontal dimension remained fixed because 70 was not a keyed value during Profile Creation and 100 was. Double click the following dimensions, select Drive Geometry and change the values accordingly. Profiles are edited when dimensions drive the geometry and orientation is controlled with geometric constraints such as h & v. Once a profile is constrained it can be moved by simply editing the coordinate of a profile point, transformations, or position constraints. (A) Change to 20mm (B) Change to 45 degrees (C) Change to 10mm (A) (C) (B) Example results: Double click the lower left point of the profile (D) and change the h & v values to zero (0) to locate the profile on the view origin. (D) Editing Constraints 1 2 Only the 2D interactive elements move. Any generated elements remain fixed. The driving geometry is displayed in green and the driving dimension is displayed in blue.

Copyright DASSAULT SYSTEMES Transformations are used to replace or duplicate one or more geometric elements. For example Translate+Replace allows a group of elements to be moved a specific distance, Rotate+Duplicate creates patterns which eliminates re-creation time, and Offset and Contour Offset copies and moves an element a specific distance. Types of Transformations: Translate and Replace offer transformation definitions that include number of instances, ability to duplicate, and the spacing between instances. Direction is controlled by Auto Detection or keying a coordinate. Symmetry, Scale and Offset have different interfaces that generally require less input. Transformations...

Copyright DASSAULT SYSTEMES Select the translate icon Transformations such as translate, rotate and offset can be very helpful to duplicate or move geometry. Translate is used here to create a linear pattern. Select the translation start point Key Instances (10) and Length value (8.5) Position the cursor for proper orientation and click Translate 1 Multi-select the slot as the geometry to be translated

Copyright DASSAULT SYSTEMES Select the rotate icon Rotate is used here to create a circular pattern. Select the rotation center point Multi-select the slot as the geometry to be translated Key 4 Instances and 90 for Angle value Example results: Rotate

Copyright DASSAULT SYSTEMES Offset allows you to duplicate a line, arc, circle or profile. (1) Offsetting Elements Options to offset: (2) (3)(4) 1- No propagation : offset a mono-element 2- Tangent propagation : offset an element using propagation 3- Point propagation : offset and duplicate multiple element 4- Both sides : offset an element symmetrically to another If you position the cursor outside the zone that is allowed for creating a given element, the symbol appears. The Offset function can duplicate open profiles

Copyright DASSAULT SYSTEMES Select the offset icon No Propagation Offset Select the No Propagation icon in the Tools toolbar Select geometry. The preview of the offset appears Preview Once the preview has appeared, enter an offset value in the Tools toolbar The Ctrl key allow you to select several geometries You can select a location on the drawing to define the position of the offset 4a 4b

Copyright DASSAULT SYSTEMES Select the offset icon Tangent Propagation Offset Select the Tangent Propagation icon in the Tools toolbar Select geometry. The preview of the offset appears Once the preview has appeared, enter an offset value in the Tools toolbar The Ctrl key allow you to select several geometries. Instance allow you to duplicate multiple elements. tangency Select a location on the drawing to define the position of the offset 4a 4b

Copyright DASSAULT SYSTEMES Select the offset icon Point Propagation Offset Select the Point Propagation icon in the Tools toolbar Once the preview has appeared, enter an offset value in the Tools toolbar The Ctrl key allow you to select several geometries. Instance allow you to duplicate multiple elements. 1 2 Click on a geometry. A preview of the offset appears 3 Select on the drawing to define the position of the offset 4a 4b

Copyright DASSAULT SYSTEMES Select the offset icon Both Side Offset Combine two icons to get your desired Both side Offset Once the preview has appeared, enter an offset value in the Tools toolbar The Ctrl key allow you to select several geometries. Instance allow you to duplicate multiple elements. 1 2 Select geometry. A preview of the offset appears 3 Select on the drawing to define the position of the offset 4a 4b

Copyright DASSAULT SYSTEMES In this lesson you have seen… How to start a drawing How to create a Front view How to create, trim, and translate geometry To Sum Up...

Copyright DASSAULT SYSTEMES Adding Projection Views and Sections In this lesson you will add views Adding Projection Views right, left, top and bottom views section views

Copyright DASSAULT SYSTEMES Adding Projection Views You will create additional projection views on a drawing.

Copyright DASSAULT SYSTEMES Added Views are usually created as projections of the Front view. The New View icon is used to create projection views one at a time. When an existing view is active, added views are created as projections of that view based on 1st or 3rd Angle Projection. Any view that is made active becomes the primary view, and added views that are created become a projection of this primary view. Projection from a Front View is a Bottom View based on 1st Angle Projection Projection from a Bottom View Results in a Rear View based on 1st Angle Projection What is the general method to add Views ?

Copyright DASSAULT SYSTEMES Select the new view icon The views added on the drawing are projected from the active view in accordance with the selected standard Place the view by positioning the cursor according to the desired View; for example: - in ISO, above the Front view will give a Bottom view - in ANSI, above the Front view will give a Top view ISO Select on sheet to create the view Adding Views 1 2 3

Copyright DASSAULT SYSTEMES Activate the view in which you want to receive the construction lines by double-clicking on its frame or on its name in the specification tree To assist drawing geometry in the views, you can use the construction lines (called Folding Lines). The construction lines are projections of the lines of one view into the active one and can be used to draw other geometry. Place cursor on the view frame from which you want to get the construction lines. Then, using the third mouse button, select Show Folding Lines from the contextual menu Construction Lines 12

Copyright DASSAULT SYSTEMES Select the Rectangle icon. When construction geometry is present Auto Detection recognizes it to anchor newly created geometry. Select the left construction line using auto detection to begin the rectangle. Select the right construction line using auto detection to complete the rectangle. Select the line icon. Then use the intersections of the construction line and the rectangle to complete the line Create Geometry using Construction Lines 4

Copyright DASSAULT SYSTEMES Select the Multiple View Projection icon Select the view where you want the projection to appear Creating a Multiple View Projection (1/2) This function allows you to generate geometry in a view by projecting geometry from previously defined views. The projected geometry retains the same attributes it had in the original multi-view. 1 2

Copyright DASSAULT SYSTEMES Select object defining target plane or surface Select one by one the geometry elements (four) which compose the feature (elongated hole). The result appears automatically Creating a Multiple View Projection (2/2) Two lines and two arcs The result 3 4

Copyright DASSAULT SYSTEMES Select the Area Fill icon To draw a section cut, you need to add a sectioning symbol to represent the material. You can choose between several types of symbols in a Pattern Table. If necessary, select the type of pattern from the pattern table Select in the zone to fill Adding a Pattern on a Section 1 3 2

Copyright DASSAULT SYSTEMES Select the Center Line icon Centerlines for various applications are available with the aid of five icons. Centerlines can be resized after creation. Select the circle Select the Axis Line icon Select two reference lines to fit the axis line between. Result 1 Center Lines 2 1 2

Copyright DASSAULT SYSTEMES In this lesson you have seen… How to add projection views How to use construction lines to create geometry How to add a pattern and center lines in a section view To Sum Up...

Copyright DASSAULT SYSTEMES Editing Views Layout & Properties In this lesson you will change the layout of views on a drawing and the properties of the views. Editing Properties: at Drawing, Sheet and View level Moving Views and Adding Sheets Modifying a Section Hatching Representation

Copyright DASSAULT SYSTEMES Editing Views You will edit the view and sheet properties.

Copyright DASSAULT SYSTEMES What are view and sheet properties? View and Sheet properties control all the variables related to specific views and sheets of the drawing.

Copyright DASSAULT SYSTEMES Select the view to modify in the tree or View frame and Properties with the contextual menu 2 1 Select the View or Graphic tab and change the necessary options, here : (A) View name (B) Dressup to have fillets on (C) Visualization to remove the frame Multi-selection of views is allowed on a single sheet or on different sheets A B C View Properties

Copyright DASSAULT SYSTEMES Select the Sheet (Sheet1) in the tree and Properties in the contextual menu to change its name. 2 Use this option to generate the views on the sheet using the 3rd angle projection method (ANSI) 1 Modify the Sheet name, scale, or projection method (ANSI or ISO). (1) (2) Sheet Properties

Copyright DASSAULT SYSTEMES Adding sheets to a drawing You will add a sheet to a one sheet drawing

Copyright DASSAULT SYSTEMES Sheets are added to a drawing to improve clarity and manage views or annotations that are cluttering a single sheet drawing. Sheet 1 of 2 Sheet 2 of 2 Why add sheets to a drawing?

Copyright DASSAULT SYSTEMES Select the New Sheet icon It creates an empty sheet with the next sheet number (Sheet 2) Adding a sheet to a drawing 1 The new sheet is assigned the same standard, format and orientation as the first created sheet

Copyright DASSAULT SYSTEMES Repositioning Views You will reposition views on a single sheet and move views from one sheet to another sheet.

Copyright DASSAULT SYSTEMES Select the frame of the view to move and drag it to the correct position 2 Select the Do not align views in the contextual menu first if the desired position is to be not aligned with the Front view. Repositioning views on sheet 1 View frame A view can be repositioned (moved) to another location Multi-selection of views is allowed

Copyright DASSAULT SYSTEMES Cut the view on the sheet to be moved Moving views from one sheet to another sheet Paste the cut view on the desired sheet in the specification tree Contextual Menu

Copyright DASSAULT SYSTEMES They can be deleted with the following options: 1) Edit + Delete to delete the selected views 2) Contextual Menu Delete option 3) Using the Delete key on the keyboard to delete the selected views Deleting Views 1 More than one view can be deleted by Multi- selecting from the tree or the geometry. 2 Views can be selected from the specification tree or from the geometry on the drawing.

Copyright DASSAULT SYSTEMES Modifying a Section Hatching Representation You will Modifying a section Hatching Representation

Copyright DASSAULT SYSTEMES Hatching Patterns are changed to modify the default material that was assigned to the 3D part or to accommodate the size of the part or the size of the view. Why Change Hatching Pattern?

Copyright DASSAULT SYSTEMES To change the steel cross hatching to an aluminum pattern. 1 Select the hatching pattern to modify. Select the properties using the right mouse button. 2 Activate the Pattern table (see next page) 3 Changing Hatching Pattern (1/2)

Copyright DASSAULT SYSTEMES Using the Next button, display the Aluminum pattern. Select it and select OK. 4 The pattern is changed on the section. Select OK in the Properties window. 5 2 Changing Hatching Pattern (2/2)

Copyright DASSAULT SYSTEMES In this lesson you have seen… How to edit view properties How to move views How to change a hatching pattern To Sum Up...

Copyright DASSAULT SYSTEMES Dimensioning and Annotating In this lesson you will dimension and annotate a drawing and learn how to control every aspect of a dimension or a text. Terminology Linear and Angular Dimensions Radius and Diameter Dimensions Chamfer Dimensions Thread Dimensions Hole / Coordinate Dimension Tables Half Dimensions Dimension Systems Dimension Properties Tolerance and GD&Ts (Geometric Tolerance) Adding Symbols

Copyright DASSAULT SYSTEMES Dimensioning Introduction and Terminology You will be introduced to dimensioning and the dimensioning terminology

Copyright DASSAULT SYSTEMES Dimensions define the size and functional intent of a part. These dimensions are used to create a fabrication drawing for a manufacturer to build the Part. Fabrication Drawing Part What are Dimensions ?

Copyright DASSAULT SYSTEMES Tolerance Text above the main value Main Value Text under the main value Text before the main value Text after the main value Dimension line Extension line Extension gap (Blanking) Overrun Terminology: Tools: Dimension Automatic Dimensioning Weld Text Text with Leader Geometric Tolerances Datum Roughness symbol Datum Target Weld Symbol Balloon Cumulated Dimension Stacked Dimension Text Replicate Dimensioning Terminology and Tools

Copyright DASSAULT SYSTEMES Manual Dimensioning You will create and modify the different types of manual dimensions.

Copyright DASSAULT SYSTEMES CATIA allows you to generate different types of manual dimensions Linear Dimensions Angular Dimensions Radius Dimensions What are the Different Types of Manual Dimensions? (1/2) Diameter Dimensions

Copyright DASSAULT SYSTEMES What are the Different Types of Manual Dimensions? (2/2) CATIA allows you to generate different types of manual dimensions Coordinate Dimensions Chamfer Dimensions Hole Dimension Table Thread Dimensions Coordinate Dimension Table

Copyright DASSAULT SYSTEMES CATIA allows you to locate manual dimensions with five types of positioning tools Projection Dimensions The placement of the cursor determines the dimension that will be created Cursor position Forced on element Forced Horizontal Forced Vertical Regardless of the cursor placement the dimension is forced to be parallel with the element selected Regardless of the cursor placement the dimension is forced Horizontal to the element selected Regardless of the cursor placement the dimension is forced Vertical to the element selected True length Regardless of the view orientation the dimension is the exact length of the 3D element selected During the dimension creation the contextual menu offers all five positioning tools. What are the Different Types of Dimension Locators?

Copyright DASSAULT SYSTEMES Creating and Modifying Linear Dimensions You will create and modify the presentation of linear dimensions Create Modify

Copyright DASSAULT SYSTEMES Distance: Length: Locating holes: Locating features: What is a Linear Dimensions Used For ?

Copyright DASSAULT SYSTEMES Select the dimension line, and drag it to the desired place, then release the mouse button Select Dimension icon with the Projected placement option In order to validate the dimension creation, select anywhere on the drawing : 1 Select the edge you want to dimension Dragging the dimension into place only needs to be done when dimension are created with the Dimension Tools + options set to manual mode Dimensioning a Length

Copyright DASSAULT SYSTEMES Select the dimension line and drag it to the desired position, then release the mouse button In order to validate the dimension, select anywhere on the drawing with the left mouse button Select the second edgeSelect the first edge Select Dimension icon with the Projected placement option 1 If the Tools options dimension setting is not set to manual mode the dimensions will be created at a predetermined spacing off of the selected geometry Dimensioning a Distance

Copyright DASSAULT SYSTEMES In order to validate the dimensions, select anywhere on the drawing with the left mouse button Select the first circle Select the second circle 3 5 Select the dimension line, and drag it to the desired place, then release the mouse button 4 Select Dimension icon with the Projected placement option 1 Dressup elements like center lines can also be selected and still be associative with the 3D geometry. During the dimension creation, yellow handles and numbers appears to adjust the location of the dimension. When cylinders (not dressup elements) are selected, the yellow handle allows control of the dimension attachment to the cylinder center or tangency by moving the yellow handle to one of the other numbers. Locating Holes

Copyright DASSAULT SYSTEMES Select an element in an Isometric View In order to validate the dimensions, select anywhere on the drawing with the left mouse button 1 Select the true Dimension length dimension mode 3 5 Select the dimension line, and drag it to the desired place, then release the mouse button 4 Select Dimension icon True Length Dimension

Copyright DASSAULT SYSTEMES Moving a dimension value: Moving a dimension line: Extending the extension lines: Modifying the Gap Adding Text Before or After the Dimension Value Modifying a Dimensions Presentation...

Copyright DASSAULT SYSTEMES Select the dimension to modify When the text is correctly placed, release the mouse button Select the dimension value, and drag it along the dimension line 3a Select the dimension line and drag it to the desired place Release the mouse button to confirm the modification 3b 1 2a 2b Moving a Dimension Value and Moving a Dimension Line Moving a dimension value:Moving a dimension line:

Copyright DASSAULT SYSTEMES Select the dimension to be modified Both extension lines are modified at the same time. At the desired length, release the mouse button 3a Select one of the upper extension line extremity and drag the extension line to increase or decrease its size 3b 2a 2b Both extension gaps are modified at the same time. At the desired gap, release the mouse button Select one of the lower extension line extremity and drag the extension line to increase or decrease the extension gap 1 Press the Ctrl key and drag the desired manipulator for modifying one extension line. Extending Extension Lines and Modifying the Gap (1/2) Extending the extension lines: Modifying the Gap

Copyright DASSAULT SYSTEMES Click on an extension line (1) to activate overrun/blanking manipulators You can also right-click the dimension and select Properties option from the displayed contextual menu. Select the Extension Line tab and modify the desired value(s) of the Overrun / Blanking Extremities option(s). This method allow you to modify the value(s) of the Overrun/blanking extremities Check the Apply to both sides option to modify the two overrun or blanking extremities at the same time. Un-check the Apply to both sides option to modify only one overrun or blanking extremity. Click OK to see the result Extending Extension Lines and Modifying the Gap (2/2) 1 Double-click on the overrun or blanking manipulator(s) (2) to display the Overrun/blanking Edition dialog box 2 The Overrun or Blanking Edition dialog box appears 3 5 4b 4a

Copyright DASSAULT SYSTEMES Interrupted extension lines Interrupt manually one or more extension lines of one or more dimensions Once created, the contextual menu changes to allow for the removal of the interruption Right click on the dimension 1 Select option Dimension object and Create Interruption 2 Select first extension line interruption location 3 Select second extension line interruption location 4 Example results:

Copyright DASSAULT SYSTEMES Right click a created dimension to space it relative to the profile (3) Key an offset of 20mm 4 Select (5) Select an existing dimension to align Select another edge to create a dimension (6) 1 3 Select an edge as a reference Spacing and Aligning Dimensions

Copyright DASSAULT SYSTEMES Select the dimension to modify Enter the text in the dialog box and click on OK Select the red arrow after the dimension value 2 The dimension becomes 4b 2a 2b Select the red arrow before the dimension value The dimension becomes 4a Adding a Text Before or After a Dimension Value 1 3 Selecting the drop down arrow gives access to several texts previously associated to the Text Before or After.

Copyright DASSAULT SYSTEMES Creating and Modifying Angle Dimensions You will create and modify angle dimensions. Create Modify

Copyright DASSAULT SYSTEMES Direct or Complementary Angle: Simple Angle: Chain Angles: What are Angle Dimensions Used For?

Copyright DASSAULT SYSTEMES Select the dimension line and drag the dimension to the desired position, then release the mouse button In order to validate the dimension, select anywhere on the drawing Select the second edge Select the first edge Select Dimension icon The location of the cursor determines the quadrant of the angle value or contextually with the angle sector option. Simple Angle Dimension

Copyright DASSAULT SYSTEMES Select the first edge 1 Select the second edge 2 If the cursor is positioned above or below the geometry the result is the following 3 During the the creation of angle dimensions the complimentary angle can be accomplished through the contextual menu Select anywhere on the drawing to validate the dimension creation 5 Select the contextual menu option Angle sector and select the Complementary option 4 Getting the Complementary Angle

Copyright DASSAULT SYSTEMES Select the second edge In order to validate the dimensions, select anywhere on the drawing 1 Select the first edge 3 6 Select the next edge 4 5 Select Dimension icon Chain Angle Dimensions

Copyright DASSAULT SYSTEMES Moving an Angular Value: Changing the extension line and gap: Adding before and after text: Modifying an Angle Dimension...

Copyright DASSAULT SYSTEMES Select the dimension to modify When the text is correctly placed, release mouse button Select the dimension value, and drag it along the dimension line 3a Select the dimension to modify When correctly placed, release mouse button Select the dimension line and drag it to the desired place 2a 1a 3b 2b 1b Moving an Angular Value and Dimension Line Moving an Angular Value:Moving an Dimension Line:

Copyright DASSAULT SYSTEMES Select the dimension to modify Both extension lines are modified at the same time. When they have the desired length, release the mouse button Select one of the upper extension line extremity and drag the extension line to increase or decrease its size 3a 2a 1 Both extension gaps are modified at the same time. When you get the desired gap, release the mouse button Select one of the lower extension line extremity and drag it to increase or decrease the extension gap 2b 3b Press the Ctrl key and drag the desired manipulator for modifying one extension line. Changing the Angle Extension Lines and Gap (1/2)

Copyright DASSAULT SYSTEMES Click on an extension line (1) to activate overrun/blanking manipulators Double-click on the overrun or blanking manipulator(s) (2) to display the Overrun/blanking Edition dialog box This method allow you to modify the value(s) of the Overrun/blanking extremities Check the Apply to both sides option to modify the two overrun or blanking extremities at the same time. Un-check the Apply to both sides option to modify only one overrun or blanking extremity. Click OK to see the result Changing the Angle Extension Lines and Gap (2/2) 1 You can also right-click the dimension and select Properties option from the displayed contextual menu. Select the Extension Line tab and modify the desired value(s) of the Overrun / Blanking Extremities option(s). 2 The Overrun or Blanking Edition dialog box appears 3 5 4b 4a

Copyright DASSAULT SYSTEMES Select the dimension to modify Enter the text in the dialog box then select OK 3 Select the red arrow before or after the dimension value (Before) Example Results: 4a (After) 2 4b 1 Adding Text Before or After an Angle Value Selecting the drop down arrow gives access to several texts previously associated to the Text Before or After.

Copyright DASSAULT SYSTEMES Creating and Modifying Radius Dimensions You will create and modify radius dimensions. Create Modify

Copyright DASSAULT SYSTEMES Select the radius you want to dimension 2 3 The dimension may appear by default as a diameter dimension (it is the same as the last radial dimension done), in that case, we need to turn it to a radius one Select the dimension line, and with the left mouse button held down, drag in rotation the dimension to the desired place, then release the mouse button 5 In order to validate the dimension creation, select anywhere on the drawing: 6 Select Dimension icon Simple Radius Dimension Place the cursor on the dimension then, with the right mouse button held down, move the cursor to the Dimension type -> Radius Center option then release the mouse button 4

Copyright DASSAULT SYSTEMES Adding Before and After Text : Moving a Radius Value: Moving a Broken Radius Value: Breaking a Radius dimension Line: Modifying a Radius Dimension...

Copyright DASSAULT SYSTEMES Select the dimension to modify When the text is correctly placed, release the mouse button Select the dimension value, and drag it along the dimension line 3a 1a 2a Example results: 3b Select the dimension to break 1b Select the dimension line option icon, then select the desired dimension line type 2b Moving the Radius Value and Breaking its Dimension Line Moving a Radius Value:Breaking a Radius dimension Line:

Copyright DASSAULT SYSTEMES Select the dimension to modify Example results: 3a 2a Select the text and drag it to the desired position Moving the Text Along the Dimension Line 1 Select the following dimension line and drag the line to the desired position (you can drag and rotate) 2b Example results: 3b Extending the Dimension Line Moving a Broken Radius Dimension

Copyright DASSAULT SYSTEMES Enter the text in the dialog box then click on OK 3 Select the red arrow after the radius value for a text after, or the red arrow before the value for a text before 2 (After) (Before) Select the dimension to modify 1 4b 4a Adding a Text Before or After a Radius Value Example results:

Copyright DASSAULT SYSTEMES Creating and Modifying Diameter Dimensions You will create and modify diameter dimensions. Create Modify

Copyright DASSAULT SYSTEMES Select the dimension line, and drag in rotation the dimension to the desired place, then release the mouse button 4 Select the circle to dimension 2 (2) The diameter dimension appears as shown below 3 In order to validate the dimension creation, select anywhere on the drawing : 5 1 Select Dimension icon Diameter Dimension

Copyright DASSAULT SYSTEMES Adding Before and After Text : Moving a Diameter Value: Moving a Broken Diameter Value: Breaking a Diameter dimension Line: Modifying a Diameter Dimension...

Copyright DASSAULT SYSTEMES Select the dimension to modify When the text is correctly placed, release the mouse button Select the dimension value and drag it along the dimension line Select the dimension line option icon, then select the desired dimension line type 3a 2a Example results: 3b 1b 2b 1a Select the dimension to modify Moving the Diameter Value and Breaking its Dimension Line Moving the Diameter ValueBreaking Dimension Line

Copyright DASSAULT SYSTEMES Select the dimension to modify Example results: 3a 2a Select the text and drag it to the desired position Moving the Text Along the Dimension Line 1 Select the following dimension line and drag the line to the desired position (you can drag and rotate to obtain 5b) 2b Example results: 3b Extending the Dimension Line a b Moving a Broken Diameter Dimension

Copyright DASSAULT SYSTEMES Select the red arrow after the radius value for a text after, or the red arrow before the value for a text before Enter the text in the dialog box then click on OK 3 Example results: 2 (After) (Before) 1 4b 4a 4 Adding a Text Before or After a Diameter Value Select the dimension to modify

Copyright DASSAULT SYSTEMES Creating and Modifying Chamfer Dimensions You will create and modify chamfer dimensions. Create Modify

Copyright DASSAULT SYSTEMES Select a chamfer line or surface to be dimensioned. 3 Select the first, then the second reference surface 4 Click in the free space to end the chamfer dimension creation. Select the Chamfer Dimension icon, under the Dimensions icon, and the Chamfer format and representation from the Tools toolbar. 1 You can customize the format of the chamfer dimension as any other type of dimension. Edit the properties with a contextual menu, then under the Chamfer tab change the value format… Chamfer Dimensions

Copyright DASSAULT SYSTEMES Adding Before and After Text : Moving a Chamfer Value: Moving a Broken Diameter Value: Breaking a Chamfer dimension Line: Modifying a Chamfer Dimension...

Copyright DASSAULT SYSTEMES Select the dimension to modify When the text is correctly placed, release the mouse button Select the dimension value and drag it along the dimension line Select the dimension line option icon, then select the desired dimension line type 3a 2a Example results: 3b 1b 2b 1a Select the dimension to modify Moving the Chamfer Value and Breaking its Dimension Line Moving the Chamfer ValueBreaking Dimension Line

Copyright DASSAULT SYSTEMES Select the dimension to modify Example results: 3a 2a Select the text and drag it to the desired position Moving the Text Along the Dimension Line 1 Select the following dimension line and drag the line to the desired position 2b Example results: 3b Extending the Dimension Line Moving a Broken Chamfer Dimension

Copyright DASSAULT SYSTEMES Select the dimension to modify Enter the text in the dialog box then click on OK 3 Example results: Select the red arrow after the radius value for a text after, or the red arrow before the value for a text before 2 (After) (Before) 1 4 Adding a Text Before or After a Chamfer Value 4b 4a

Copyright DASSAULT SYSTEMES Create Creating Thread Dimensions You will create thread dimensions.

Copyright DASSAULT SYSTEMES Create associative thread dimensions For top view representation For side view projection Creating Thread Dimensions Apply the Thread specifications Select the Thread representation to dimension 3 Example results: Select the Thread Dimension icon b 4a To select the Thread, the Thread representation and not the hole geometry must be selected

Copyright DASSAULT SYSTEMES Create Creating a Hole / Coordinate Dimension Tables You will create a Hole / Coordinate Dimension Table. Hole Dimension Table Coordinate Dimension Table

Copyright DASSAULT SYSTEMES T o create Hole Tables Select the Hole definitions (circles, cutouts, or axis lines) 2 1 Select the Hole Table icon. 3 Define the Table and Origin parameters. 4 Select the Hole Table location. Creating Hole Tables (1/2) Note: The process and panel is the same for creating coordinate dimension tables

Copyright DASSAULT SYSTEMES Below are the parameters to create hole tables Origin reference – defines the starting point for reference of the holes. Table Format – defines the format for the hole table (Alpha or Numeric). Title – shows/defines the title for the hole table or columns. Column – shows/defines the label for the hole table columns and sorting preferences. Transpose Table – switches the format from vertical to horizontal. Creating Hole Tables (2/2) Note: The panel is the same for creating coordinate dimension tables

Copyright DASSAULT SYSTEMES Creating and Modifying Half-Dimensions You will create and modify half-dimensions. Create Modify

Copyright DASSAULT SYSTEMES Select the dimension icon Select the first edge (A) then the second one (B). The dimension appears. (A) Creating Half-Dimensions (1/2) Half-Dimensions function allow you to dimension big symmetrical or circular part. You can create half-dimensions on distance, angle, diameter, cylinders, diameter edges and diameter-tangents but not on cumulate dimensions. (B) The half-diameter dimension is associated to the axis and the element, whereas a standard diameter is associated to both symmetrical elements. 1 2

Copyright DASSAULT SYSTEMES Once you select the Half-dimension option from the contextual menu, all the following dimensions you create will be assigned the half-dimension mode. If you want to create dimensions in the standard mode, go back to the contextual menu and de-activate the Half-dimension option. Creating Half-Dimensions (2/2) Drag the dimension line to get a better visualization and select on the MB3 to display the contextual menu. Check half-dimension option. The half-dimension appears automatically. Select anywhere on the drawing to validate. 3 4

Copyright DASSAULT SYSTEMES Adding Before and After Text : Moving a Value: Breaking a Half-Dimension Line: Modifying a Half-Dimension...

Copyright DASSAULT SYSTEMES Select the dimension to modify When the text is correctly placed, release the mouse button Select the dimension value and drag it along the dimension line Select the dimension line option icon, then select the desired dimension line type 3a 2a Example results: 3b 1b 2b 1a Select the dimension to modify Moving the Value and Breaking its Dimension Line Moving the ValueBreaking Dimension Line

Copyright DASSAULT SYSTEMES Select the dimension to modify Select the red arrow after the radius value for a text after, or the red arrow before the value for a text before Enter the text in the dialog box then click on OK 3 Example results: 2 (After) (Before) 1 4 Adding a Text Before or After a Half-Dimension Value 4a 4b

Copyright DASSAULT SYSTEMES Select the Quick Dimension icon (Optional): select another element; a dimension is created 3a 2 Select an element to dimension; a linear dimension is created Linear Dimensions 1 Quick Dimension allows the creation of Linear, Angular, Radius, or Diameter dimensions using one icon The dimensions are created using the default dimension properties. (Optional): select another element; a dimension is created 3b (Optional): select another element; a dimension is created 3c Quick Dimension (1/2)

Copyright DASSAULT SYSTEMES Quick Dimension allows the creation of Linear, Angular, Radius, or Diameter dimensions using one icon The dimensions are created using the default dimension properties. Select the Quick Dimension icon (Optional): To change the type; right click on dimension and select desired option 3 2 Select an element to dimension; a dimension is created Radius/Diameter Dimensions 1 Example results: Quick Dimension (2/2)

Copyright DASSAULT SYSTEMES Creating System Dimensions You will create system dimensions. Chained: Stacked: Cumulated:

Copyright DASSAULT SYSTEMES Select the second edge In order to validate the dimensions, select anywhere on the drawing 1 Select the first edge 36 Select the next edge 4 5 Select Dimension icon Chain Dimensions

Copyright DASSAULT SYSTEMES Select the origin point or edge of your cumulated system. 3 Select all the other points or edges of your cumulated system (as many as you want). 4 Select in the free space to end the cumulated dimension system creation. Select the Stacked Dimensions icon under the Dimensions icon. 1 The alignment and spacing between the system dimensions is the one defined in the Option dialog box (Tools+Options+Drafting Dimension tab, Line Up paragraph). Stacked Dimensions

Copyright DASSAULT SYSTEMES Select the origin point or edge of your cumulated system. 3 Select all the other points or edges of your cumulated system (as many as you want). 4 Select in the free space to end the cumulated dimension system creation. Select the Cumulated Dimensions icon under the Dimensions icon. 1 Cumulated Dimensions

Copyright DASSAULT SYSTEMES Dimension Properties You will edit the dimension properties. Toolbar Properties Contextual Menu Properties

Copyright DASSAULT SYSTEMES Dimension properties control all the variables related to dimensions. What are Dimension Properties ?

Copyright DASSAULT SYSTEMES They are organized in 8 tabs: The most often used properties are available in the top toolbar: All properties are available from the contextual menu: The properties for Chamfer dimensions have one additional tab to control the Chamfer representation Modifying Dimension Properties

Copyright DASSAULT SYSTEMES To get the dimensions properties window, place the cursor on the dimension you want to get the properties. 1 Keeping the right mouse button held down, move the cursor on the Properties function and release the mouse button 2 These are the different properties 3 Accessing Dimension Properties

Copyright DASSAULT SYSTEMES To define the main value reference orientation To define the main value orientation in accordance with the reference Dimension Properties : Value

Copyright DASSAULT SYSTEMES The tolerance properties are used to define the tolerance and fit parameters on dimensions Dimension Properties : Tolerance

Copyright DASSAULT SYSTEMES The dimension line properties are used to define the geometric characteristics of dimension lines Dimension Properties : Dimension Line

Copyright DASSAULT SYSTEMES The extension line properties are used to define the geometric characteristics of dimensions extension lines Dimension Properties : Extension Line

Copyright DASSAULT SYSTEMES You can add a prefix or a suffix to your dimension using this icon and choosing the symbol. Dimension Properties : Dimensions Texts

Copyright DASSAULT SYSTEMES To define the main value type of fonts To underline the main value To define the main value style To define the main value text height To define the main value text color Dimension Properties : Font

Copyright DASSAULT SYSTEMES To define a frame around the main value To control the Dimension text graphical properties To control the Dimension text positioning Dimension Properties : Text

Copyright DASSAULT SYSTEMES The graphic properties are used to define the graphic characteristic of dimensions Dimension Properties : Graphic

Copyright DASSAULT SYSTEMES Adding Tolerances, Fits and GD&T You will add Tolerances, Fits, Datum, Geometric Tolerances and Functional Tolerancing to refine the specifications of the part

Copyright DASSAULT SYSTEMES Simple Tolerance: Fit dimension: Datum and Geometric Tolerance: What are Tolerances, Fits, Datum and Geometric Tolerances?

Copyright DASSAULT SYSTEMES Select anywhere to validate the tolerance creation Create the following tolerance: Enter +/- tolerance (+0.01/-0.05), or select from the pull down options Select the dimension Select from the list of tolerance representations Adding a Tolerance

Copyright DASSAULT SYSTEMES Select anywhere to validate the fit Create the following fit: Select H7 from the pull down list Select the dimension 1 Select the TOL_ALP1 for the Fit tolerance representation Adding a Fit

Copyright DASSAULT SYSTEMES Create this datum: Select the Datum icon 1 Select the reference element 2 Example results: 5 Select the symbol location 3 Enter the name of the Datum then OK 4 Adding a Datum Feature The GDT orientation can be swapped during creation: with the « ctrl » key, swap from vertical to horizontal or with the « shift » key, free or lock perpendicular the leader

Copyright DASSAULT SYSTEMES Create this perpendicularity: Select tolerance icon Enter tolerance value (0.1) then press the TAB key Enter datum name (A) then OK Select anywhere to validate the tolerance creation Select the reference element Select the symbol location 3 Select the Datum type and description then OK Adding a Geometric Tolerance The GDT orientation can be swapped during creation: with the « ctrl » key, swap from vertical to horizontal or with the « shift » key, free or lock perpendicular the leader

Copyright DASSAULT SYSTEMES Adding Symbols You will add symbols to better define the specifications of the part

Copyright DASSAULT SYSTEMES Weld Symbols: Welds:` Roughness: What are the Different Types of Symbols ?

Copyright DASSAULT SYSTEMES Create the following roughness symbol: Select the surface element 2 Select Roughness Symbol icon 1 Select roughness type (Ra), enter value (0.6) then select OK 3 Adding a Roughness Symbol Select desired Rugosity type 4 Select desired Rugosity value 5 Select desired Rugosity mode, then select OK 6

Copyright DASSAULT SYSTEMES Create the following Weld symbol: Select Weld Symbol icon 1 Select the weld element 2 Select the desired symbols and enter any text (2X), then OK 4 (2x) Select an orientation point, drag the symbol to the desired position and select to confirm location 3 Adding a Weld Symbol A-Weld modifier B-Length of weld C-Type of weld D-Type modifier E-Size of weld F-Reference text

Copyright DASSAULT SYSTEMES Select Weld icon Select the weld representation, key a weld thickness, angle and OK 1 3 Select two elements to create a weld between 2 Adding a Weld Create the following Weld representation on a drawing: Example Results: Two types of weld representations are available; external welds (blue icons) and internal welds (red icons). The symbols are contextual and are displayed according to the selected elements

Copyright DASSAULT SYSTEMES In this lesson you have created and modified… To Sum Up... Linear Dimensions Angle Dimensions Radius Dimensions Diameter Dimensions Chamfer Dimensions Thread Dimensions Hole / Coordinate Dimensions Half Dimensions System Dimensions Dimension Properties Tolerance, Fit and GD&T Symbols

Copyright DASSAULT SYSTEMES Finalizing the Drawing and Printing In this lesson you will create text for annotations and a view dedicated to notes and printing. Create text Adding a note view Creating / Editing a Table Adding Title Block Inserting a picture Printing

Copyright DASSAULT SYSTEMES Creating Text You will create text for notes and to fill in the title block

Copyright DASSAULT SYSTEMES Text can be created with or without leaders and can have many properties to customize the font and frame style (shown on the right). Special symbols can also be inserted into the Text as needed. Text

Copyright DASSAULT SYSTEMES Select the Text icon to create text without a leader Text without leaders with a customize symbol and frame style. Select the text anchor (starting) point Example results: Select anywhere to end the text. Key the desired text with the appropriate framing or embedded symbols; for example: (a) Key HOLE then spacebar (b) Select from the Symbol icon then select from the Symbol icon and press spacebar (c) Key SIZE 3 then press ENTER to start new line (d) Key SEE NOTE then press spacebar (e) Select from the Frame icon (f) Key 1. Text

Copyright DASSAULT SYSTEMES Select the Text with Leader icon Text with leaders. Select the text anchor point Key desired text (ITEM 4) Select an anchor point for the arrow head Select anywhere to end the leader text Text with Leader Example results: The orientation can be swapped during creation: with the « ctrl » key, swap from vertical to horizontal or with the « shift » key, free or lock perpendicular the leader

Copyright DASSAULT SYSTEMES Select the Text with Leader Text with multiple leaders and breakpoints. Using the contextual menu, select a breakpoint and the Add an Extremity item. Using the contextual menu, Select the anchor point (yellow symbol) and Add a Breakpoint item. Select an element or location to end the leader Text with Breakpoints and Multiple Leaders Example results: Add Breakpoint: Add Leader: Select the breakpoint and drag to desired location 3

Copyright DASSAULT SYSTEMES Double click text to open the Text Editor. Text can be manipulated in the following ways: Edited, Repositioned and/or Leaders added or removed Swipe the cursor across the text (second line) within the Text Editor window and edit or delete. Select the text to edit (3) directly from the drawing and key new text. Right click the anchor point of a leader arrow choose any of these options To add a leader; Right click the note and select: Select any part of a note and drag to reposition it Indicate or select an element to anchor the arrow head. Select the anchor point of a leader arrow and drag it to reposition it This process can be repeated to create multiple leaders Text Manipulation

Copyright DASSAULT SYSTEMES Define a link to 2D geometry to determine the orientation of text Note: as the element rotates, the text will flip to avoid being backwards or upside down unless the text property Auto Flip is disabled Right click on the text 1 Select option Orientation Link and Create 2 Select orientation element 3 Associated text (Orientation Link)

Copyright DASSAULT SYSTEMES Right click Sheet1 and select Activate The Note View will be created as a stand alone view that is not projected from an existing Front View. Change the View Name Prefix to Note view Adding a Note View 1 Right click the new Front view and select Properties 3 4 Click on sheet to create a new Front view 2

Copyright DASSAULT SYSTEMES Activate the Note view Create notes using the points for reference Create a vertical grid of points to attach notes to Example results: Using the Note View 1 2 3

Copyright DASSAULT SYSTEMES Select the key Table icon Creating a Table 1 To create a Table of data for Bill of Material list, Revision Notes, or etc... Key the number of columns and rows for the Table 3 Select the Table location 2 Double click the Table to select it. 4 Double click a Table cell to edit it. 5 Note: Continue step 5 to fill in all necessary cells.

Copyright DASSAULT SYSTEMES Select the key Table icon Creating a Table from a csv file 1 To create a Table of data from a csv file for Bill of Material list, Revision Notes, or etc... Select a location for the Table 3 Select the csv file 2

Copyright DASSAULT SYSTEMES Double click the Table to select it Editing a Table 1 To edit a Table element to add or delete rows and columns, resize the rows or columns, and invert the rows or columns. Double click a Table cell to edit, Use the contextual menu to select the item to modify or select a row/column marker to resize. 2

Copyright DASSAULT SYSTEMES Adding a Title Block You will add a title block to the drawing

Copyright DASSAULT SYSTEMES Adding a Title Block (1/2) Change to the sheet Background with Edit + Background menu 1 2 Select Insert + Drawing + Frame and Title Block menu, to set the 2 main frames Note the blue axis is on the sheet to indicate that you are in the background

Copyright DASSAULT SYSTEMES Adding a Title Block (2/2) (a)Use the geometric tools (lines, circles, etc.) to draw the title block (b)Use the Text icon and the Text Properties to fill in all necessary information (c)Use a VB script to complete the Title block geometry and text. 3 When finished, do not forget to go back to (select) Working View from the Edit menu 4 3a 3b 3c

Copyright DASSAULT SYSTEMES Inserting a Picture Select menu Insert and item Picture 1 Select the image 2 To insert a picture type image into a drawing. The picture can be of Raster (bmp, jpg, tif, etc…) or Vector (hpgl, cgm, etc…) type Select Picture location 3 Note: properties may be used to change the scale, crop, and location of the picture.

Copyright DASSAULT SYSTEMES Select File + Page Setup menu 1 Drawing size can be changed anytime in the drafting process. Select the new size format, the desired orientation, the sheets effected and OK. 2 While changing drawing size an option to insert a Background view from another document is available. Changing Drawing size

Copyright DASSAULT SYSTEMES Printing the Drawing You will learn how to Print the drawing

Copyright DASSAULT SYSTEMES Printing a Drawing From the File menu, 1. use Print to direct the drawing to the selected printer or plotter 2. use Preview button… to check what will be printed 1 2

Copyright DASSAULT SYSTEMES ) Printer: Select the printer or key in a file name to print to. 2) Position and Size: Define the position and size of the geometry on the page 3) Print Area: Define the area to print (Whole Document, Display, Selection) 4) Page Setup: Define the paper size and margins 5) Print Options: Define the print options (shown on next page) Print User Interface

Copyright DASSAULT SYSTEMES Three options tabs are provided for customizing the printed output Printing Options

Copyright DASSAULT SYSTEMES To Sum Up... In this lesson you have seen… How to create text How to create a note view How to use a note view How to create a Table How to create a title block How to insert a Picture How to Print a drawing

Copyright DASSAULT SYSTEMES Setting Drafting Options You will learn how to set the sessions default drafting options

Copyright DASSAULT SYSTEMES For Interactive Drafting there are primarily six Drafting Option tabs that allow the user to customize the drafting interface. (1) General - Determine display of ruler, grid, background colors and Tree Display (2) Layout - Determine display of View name, scale, frame and determines new sheet parameters settings (3) Geometry - Aides to create geometry such as display of center points, auto-detection for orientation, and constraint creation and display (4) Dimension - Position, Line-up dimensions and Analysis display mode (5) Manipulators – Turns on/Off the manipulators for dimension creation or modification (6) Annotation – Turns on/off the controls for annotations What are Drafting Options ?

Copyright DASSAULT SYSTEMES Snap to Point and grid display can also be controlled from the standard toolbars. Set the following General options: 1) Show Ruler: In the OFF position the ruler along the top and left side of the screen will not be displayed 2) Grid: With the Display turned ON and Snap to point turned ON. Adjust the Primary spacing and graduations to aid in dimension placement. 3) Allow distortions: Allow you to change the scale of H and V on the grid 1 2 Example with Ruler ON General Options (1/2)

Copyright DASSAULT SYSTEMES Set the following General options: 1 3 1) Rotation: Allows to set the View manipulator default rotation angle 2) Colors: Allows easy identification of a Detail sheet by altering the background color 3) Tree: Allows parameters and relations to be displayed in the graph tree 4) View Axis: Provides a blue axis in the view that is current 2 General Options (2/2) 4

Copyright DASSAULT SYSTEMES Set the following view Layout options: 1) View name: Check that it is OFF since primary and projected view names are not normally necessary 2) Scaling factor: Check that it is OFF since primary and projected view scale will be declared on the drawing as a global scale for the drawing 3) View frame: Turn on to easily understand which view is active and to quickly access view properties 4) Propagation of broken and breakout specifications: Allows the propagation a Broken or Break-out specification during the creation of a projection or auxiliary view 5) Auxiliary and/or section views orientation according to profile: Allow the view axis to be orientation according to profile 6) New Sheet : Allows the selection to determine where the sheet properties will be copied from and an option to copy the background view Layout Options 4 6

Copyright DASSAULT SYSTEMES Set the following view Geometry options: 1 2 1)Geometry: Interactive geometry creates circle and ellipse centers and end points included with drag elements 2)Constraint Creation : Allows for creation of feature based constraints 3)Constraint Visualization: Allows what constraints will be visualized and the constraints color and size 4)Colors: Allows you to visualize and choose colors for geometry elements 3 4 Geometry Options

Copyright DASSAULT SYSTEMES )Manual positioning at creation: allows full freedom for dimension positioning. 2)End dimension creation at line-up: use if line-up is the last step in the normal dimension creation process. 3)Create associativity dimension line/geometry: the distance between the created dimension and the geometry remains the same as set by the value. 4)Associativity on 3D : 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. If you do not check this option, when you perform the update, you need to re-create the dimension afterwards. 5)Line-Up default: a default spacing between dimensions when a Line-Up and a reference dimension are selected 6)Activate analysis display mode: Displays dimension status of Non up-to- date dimensions, Non associative dimensions, converted dimensions, Fake dimensions, Driving dimensions and True dimensions Before creating any dimensions, turn on the following Dimension options: Dimension Options 3

Copyright DASSAULT SYSTEMES Dimension Manipulators Option to enable dimension manipulators to control the precise location or properties during creation or modification of dimensions a 3a 4a

Copyright DASSAULT SYSTEMES Annotation Options Annotation Option for Text, Leader Text, and GDT Settings to choose the leader default behavior Stay Horizontal/Vertical with leader creation Free orientation Ability to Swap the text or GDT orientation during creation With the « ctrl » key, swap from vertical to horizontal With the « shift » key, free or lock perpendicular the leader

Copyright DASSAULT SYSTEMES Drawing Size and Orientation Format: on/off Menu File + Page Setup Properties: Drafting Page (Drawing) Settings Drawing Standard

Copyright DASSAULT SYSTEMES How to set drafting options using the Dimension, Display, General, Generation, Geometry, and Layout tabs How to set the drafting page standards In this lesson you have seen… To Sum Up…

Copyright DASSAULT SYSTEMES Saving a Drawing Document You will learn how to save an Drawing Document

Copyright DASSAULT SYSTEMES There are various ways to save a Drawing Document Save will save the active drawing document Save As... is similar to Save, but it allows you to specify the name and folder for the active document Save All will propose saving all open documents and children of these document, but you can control which documents actually get saved Only those documents that been modified will be saved or proposed to save. Saving a Document...

Copyright DASSAULT SYSTEMES How to save a drawing In this lesson you have seen… To Sum Up…

Copyright DASSAULT SYSTEMES Introduction to the Interactive Drafting Workbench How to start a drawing and view generation In this course you have seen… To Sum Up… How to create any additional section, auxiliary, or isometric views How to edit a views layout and properties How to finalize a drawing and print How to set the drafting options How to save a drawing document