Copyright DASSAULT SYSTEMES D Functional Tolerancing & Annotation CATIA Training Foils Version 5 Release 8 February 2002 EDU-CAT-E-FTD-FF-V5R8

Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will learn how to define Functional Tolerances and Annotation to geometric parts designed in 3D Wireframe or Solid geometry Targeted audience Catia V5 users Prerequisites Fundamentals about Catia V5 0.5 day

Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to FT&A Workbenchp.4 The User Settings p.5 Accessing theWorkbench p.9 The User Interfacep.12 General Processp Fundamentals of FT&Ap.16 Creating Annotation planesp.17 Creating Annotationsp.25 Use Propertiesp.41 Generate Check Reportp The 2D extractionp.61 View from 3Dp To Sum Up…p.64

Copyright DASSAULT SYSTEMES Introduction to FT&A Workbench You will become familiar with the Functional Tolerancing & Annotation Workbench by : The User Settings Accessing the Workbench The User Interface General Process

Copyright DASSAULT SYSTEMES The User Settings (1/4) Tools / Options / Mechanical Design / Functional Tolerancing and Annotation / Tolerancing whether note object attribute may be created by user or not enable or disable Note Object Attribute Creation icon or not It is possible to define: the default standard at creation provides: three conventional standards (ANSI – ISO – JIS) and three CATIA-CADAM standards (CCDANSI – CCDISO – CCDJIS) whether non semantic tolerances creation is allowed or not, whether non semantic dimensions creation is allowed or not whether leader annotations are perpendicular to their geometrical elements or not an angle value for rotating elements (this option is used to rotate used to rotate text elements (text, frame, or leader) whether the rotation will be snapped to the angle value or not.

Copyright DASSAULT SYSTEMES The User Settings (2/4) Tools / Options / Mechanical Design / Functional Tolerancing and Annotation / Display mark with a wavy red line, in the specification tree and the geometry, non- semantic annotations whether the axis of the active view can be visible or not. whether the axis of the active view can be zoomed or not. whether the profile of the active view can be visible or not

Copyright DASSAULT SYSTEMES The User Settings (3/4) Tools / Options / Mechanical Design / Functional Tolerancing and Annotation / Manipulators It is possible to define: the size value to the manipulators, whether manipulators can be zoomed in or not whether overrun extension lines can be modified or not during creation or modification, whether blanking can be modified or not during creation or modification, whether text can be inserted before or not during creation or modification, whether text can be inserted, whether only the value can be moved or not during creation or modification, whether only the dimension line can be moved or not during creation or modification, whether only the dimension line secondary part can be moved or not during creation or modification.

Copyright DASSAULT SYSTEMES The User Settings (4/4) Tools / Options / Mechanical Design / Functional Tolerancing and Annotation / Dimension It is possible to define: whether the dimension line is positioned according to the cursor or not, whether a dimension aligned to another automatically ends the command or not, whether the distance between the created dimension and the geometry remains the same when you move the geometry or not, the value at which the dimension is created from the geometry, the dimension you will create between a circle and another element will be either on the circle center or on the circle edge, whether the dimension will be snapped on the grid and/or the dimension value will be located at its default position between symbols (it will work only if the cursor is between the symbols) or not, whether only a dimension sub-part (text, line, etc...) will be moved or not.

Copyright DASSAULT SYSTEMES Accessing the Workbench (1/3) Functional Tolerancing & Annotation Workbench icon It is possible to work at Product level and at Process level in any CATProduct document respectively CATProcess document. As a consequence, it is possible to use CATProduct Workbench or CATPRrocess Workbench to perform scenarios instead of the CATPart Workbench. At Process level, it is possible to create FTA data in CATProcess document and perform FTA assignment to Process activity

Copyright DASSAULT SYSTEMES Accessing the Workbench (2/3) Once you are in the Functional Tolerancing and Annotation workbench the associated toolbars are displayed: Annotations Free Rotation Reporting Views Filtered Selection Available only in Functional Tolerancing and Annotation, Not in Product neither in Process Reference Elements Wireframe geometry Note Object Attribute Available only in Product Functional Tolerancing and Annotation, Not in Functional neither in Process

Copyright DASSAULT SYSTEMES Accessing the Workbench (3/3) Once you are in the Functional Tolerancing and Annotation workbench the associated toolbars are displayed Style Dimension Properties Text Properties Position and Orientation Dimension Numerical Display Dimension Tolerance Display

Copyright DASSAULT SYSTEMES The User Interface (1/3) You have access to the Functional Tolerancing & Annotation Workbench through the menu or toolbars

Copyright DASSAULT SYSTEMES The User Interface (2/3) You have access to the Product Functional Tolerancing & Annotation Workbench through the menu or toolbars

Copyright DASSAULT SYSTEMES The User Interface (3/3) You have access to the Process Functional Tolerancing & Annotation Workbench through the menu or toolbars

Copyright DASSAULT SYSTEMES General Process Part Design using Solid Geometry 1 Create 3D Annotations using FT&A 2 Use Drafting Workbench to generate a drawing with 3D annotations 3

Copyright DASSAULT SYSTEMES Fundamentals of FT&A You will become familiar with the fundamental functions of the Functional Tolerancing & Annotation Workbench. Creating Annotation Planes Creating Annotations Use Properties Generate Check Report

Copyright DASSAULT SYSTEMES Creating Annotation Planes (1/8) Front View This specific annotation plane allows you to manage 3D annotations: Located in planes both parallel to this annotation plane and in the background and foreground spaces bounded by this annotation plane (or in any plane of the direction of planes defined by this annotation plane), Related to the geometry finding an intersection with this annotation plane, Lying on / belonging to this annotation plane. Front View Annotation Planes can be created on a planar face or on a plane. This option allows you to specify a particular annotation plane for generating embedded 2D front / projection views, in the Generative Drafting workbench, during the 2D extraction of the 3D part and of the 3D annotations. Front View

Copyright DASSAULT SYSTEMES Creating Annotation Planes (2/8) Front View Front Views are represented by blue axis and identified as FrontView in the specification tree Front View

Copyright DASSAULT SYSTEMES Creating Annotation Planes (3/8) Section View This specific annotation plane allows you to manage 3D annotations: Located in planes both parallel to this annotation plane and in the background and foreground spaces bounded by this annotation plane, Related to the geometry finding an intersection with this annotation plane, Lying on / belonging to this annotation plane. Section View Annotation Planes can be created on a planar face or on a plane. This option allows you to specify a particular annotation plane for generating embedded 2D section views, in the Generative Drafting workbench, during the 2D extraction of the 3D part and of the 3D annotations. Section View

Copyright DASSAULT SYSTEMES Creating Annotation Planes (4/8) Front View Section Views are represented by green axis and identified as SectionView in the specification tree Section View

Copyright DASSAULT SYSTEMES Creating Annotation Planes (5/8) Section Cut This specific annotation plane allows you to manage 3D annotations: Only related to the geometry finding an intersection with this annotation plane, Only lying on / belonging to this annotation plane. Section Cut Annotation Planes can be created on a planar face or on a plane. This option allows you to specify a particular annotation plane for generating embedded 2D section cuts, in the Generative Drafting workbench, during the 2D extraction of the 3D part and of the 3D annotations. Section cut

Copyright DASSAULT SYSTEMES Creating Annotation Planes (6/8) Section Cut Section Cuts are represented by yellow axis and identified as SectionCut in the specification tree Section Cut

Copyright DASSAULT SYSTEMES Creating Annotation Planes (7/8) Annotation Planes Properties Edition Select any view (front, section or cut) from the specification tree. Right-click (MB3) and select the Properties contextual command. When the Properties dialog box is displayed, click the View tab. This task shows you how to rename an annotation plane and hide its frame

Copyright DASSAULT SYSTEMES Creating Annotation Planes (8/8) Annotation Planes Properties Edition To rename the annotation plane, enter Your_Name_View in the Prefix field. Uncheck the View Frame option to hide the annotation plane frame. The annotation plane is renamed and its frame is no longer visible

Copyright DASSAULT SYSTEMES Creating Annotations (1/16) Easy creation of associative 3D tolerance specifications Avoiding the reliance on 2D drawings Annotate detail parts and products individually or in a assembly context Most currently used types of tolerance and annotation are provided Fast changes through Cut, copy, Paste, Drag & Drop of 3D Annotations Tolerancing Advisor Text with Leader Flag Note with Leader Datum Feature Datum Target Geometrical Tolerance Roughness Dimensions Automatic Default Annotation Note Object Attribute

Copyright DASSAULT SYSTEMES Creating Annotations (2/16) Tolerancing Advisor (1/2) This function will allow you to create from a geometrical element or an existing annotation : semantic annotations and non semantic (Text, Roughness, Flag note), datum, datum target, datum system.. Just select FIRST a face or a set of surfaces and activate Tolerancing Advisor. The semantic Tolerancing Advisor dialog box is displayed Click on Tolerancing Advisor icon 1 2 This dialog box as shown is an updated dialog box. The commands frame contains all the semantic annotations that will be created in relation with the selected element. If you did not have selected a face or a set of surfaces before clicking on the Tolerancing Advisor icon, the dialog box displayed does not contain commands.

Copyright DASSAULT SYSTEMES Creating Annotations (3/16) Tolerancing Advisor (2/2) Select a semantic annotation. The appropriate dialog box is displayed 3 4 Tolerancing Advisor Proposal of applicable tolerance types regarding the selected surfaces, Proposal of tolerance options when applicable, Tolerancing rules verification Help for an error-free tolerancing, Automatic support of annotation syntax, GUARANTEE of semantic and syntactic validity of the tolerancing, through the part / assembly life cycle.

Copyright DASSAULT SYSTEMES Creating Annotations (4/16) Text with Leader (1/2) This function will allow you to create a text with a Leader line. Just select a face or a set of surfaces to define a location for the arrow end of the leader and activate Text with Leader. A dialog box is displayed to write the text Click on Text with Leader icon The Leader is associated with the element you have selected

Copyright DASSAULT SYSTEMES Creating Annotations (5/16) Text with Leader (2/2) The text is assigned to an unlimited width text frame. There is a manipulator at the extremity of the arrow end. So, you can move this end point by dragging it. You can move horizontally the textual annotation using the arrow above or dragging it anywhere in the annotation plane If the active view is not valid, a message appears informing you can not use the active view. The annotation is displayed in an annotation plane normal to the selected face. You can set graphic properties, anchor point, text size… (Text properties Toolbar)

Copyright DASSAULT SYSTEMES Creating Annotations (6/16) Flag Note with Leader (1/2) This function will allow you to add hyperlinks to the document. Just select a face or a set of surfaces to define a location for the arrow end of the leader and activate Flag Note with Leader. Select the object you want to represent the hyperlink. The Manage Hyperlink dialog box appears. Enter a name for your Hyperlink. Enter the path to the destination file in the URL field then press OK. Or Click Browse.. And select the destination file in the Link to file dialog box. Click on Flag Note with Leader icon 1 2 The same message is displayed as in the previous function if the active view can not be used

Copyright DASSAULT SYSTEMES Creating Annotations (7/16) Flag Note with Leader (2/2) You can add hyperlinks to your document and then use them to jump to a variety of locations, for example to a marketing presentation, a Microsoft Excel spreadsheet or a HTML page on the intranet. You can add hyperlinks to models, products and parts as well as to any constituent elements. You can add more than one link. Simply enter another file. All links created are listed in the Link to file or URL box. Select a link then click Remove to remove existing links. To edit the display of the note, use the Properties contextual command. Select a link then click Go to to follow the link to the destination file.

Copyright DASSAULT SYSTEMES Creating Annotations (8/16) Datum Feature (1/1) This function will allow you to create a Datum Feature attached to a surface. Just select the attachment surface of the datum feature and click on Datum Feature icon. A Datum Feature dialog box is displayed with a default identifier Click on Datum Feature icon The same message is displayed as in the previous function if the active view can not be used You can move the Datum Feature by dragging it anywhere in the annotation plane You can set graphic properties, anchor point, text size… (Text properties Toolbar)

Copyright DASSAULT SYSTEMES Creating Annotations (9/16) Datum Target (1/1) This function will allow you to create a Datum Target on datum elements. Just select the surface of the Datum Feature and click on Datum target icon. A Datum Target Modification dialog box is displayed. The name is in the left field, the length in the right, and, if it is a circular surface, you can use diameter icon Click on Datum Feature icon 1 2 The same message is displayed as in the previous function if the active view can not be used You can move the Datum Target by dragging it anywhere in the annotation plane and you can move the extremity of the arrow as Datum Feature 3 You can set some of its graphic properties (Text properties Toolbar)

Copyright DASSAULT SYSTEMES Creating Annotations (10/16) Geometrical Tolerance (1/2) This function will allow you to create a Geometrical Tolerance on any element. Just select a surface and click on Geometrical Tolerance icon. A dialog box is displayed in which you can define Specification, Tolerance Value and Datum Elements Click on Geometrical Tolerance icon 1 2 Specifications are defined by symbols in table Datum Element contains an empty entry field to set datum and Tolerance Feature modifiers symbols Tolerance Value includes the optional diameter zone, an empty entry field and Tolerance feature modifiers symbols

Copyright DASSAULT SYSTEMES Creating Annotations (11/16) Geometrical Tolerance (2/2) The same message is displayed as in the previous function if the active view can not be used You can move the Geometrical Tolerance by dragging it anywhere in the annotation plane You can set graphic properties, anchor point, text size… (Text properties Toolbar) 3 The Geometrical Tolerance symbol is created on the annotation plane

Copyright DASSAULT SYSTEMES Creating Annotations (12/16) Roughness (1/2) This function will allow you to create a Roughness Symbol annotation. Select a face or a set of surfaces and click on Roughness icon Click on Roughness icon 1 A dialog box is displayed, in which you can define Roughness characteristics (Rugosity, Rugosity Type, Rugosity Mode…) 2 3 The Roughness symbol is created You can move the Roughness symbol by dragging it anywhere in the annotation plane

Copyright DASSAULT SYSTEMES Creating Annotations (13/16) Roughness (2/2) Rugosity You can choose the Rugosity type You can select the Rugosity mode Contact Rugosity (circle) or not

Copyright DASSAULT SYSTEMES Creating Annotations (14/16) Dimensions (1/1) This function will allow to create a dimension annotation. Click on Dimensions icon 1 Select the elements (feature, faces…) to create the dimensions 2 3 The dimension is created You can move the dimension by dragging it anywhere in the annotation plane 4 Select the Dimension and in the Dimension Properties toolbar, select in the Tolerance Description combo box TOL_NUM2 and in the Tolerance combo box The dimension is toleranced

Copyright DASSAULT SYSTEMES Creating Annotations (15/16) Automatic Default Annotation (1/1) This function will allow to apply by default a tolerance or an annotation to a set of surfaces Manual selection : the default annotation is applied to a set of surfaces chosen by the user Automatic selection : the default annotation is applied to all surfaces of a given type or characteristic Select Insert -> Annotations -> Default Annotation menu Select the annotation as shown The Default Annotation dialog box appears and by select Automatic, and All faces option in the combo box and click OK, so the annotation will be applied to all the faces of the part

Copyright DASSAULT SYSTEMES Creating Annotations (16/16) Note Object Attribute (1/1) This function will allow to create a User Defined type of annotation Type and representation definition (the representation can be symbolic) Stored in a catalogue (company standard) Instantiated through catalogue capability Can be filtered by type Instance edition Comments definition Hyperlinks definition 3 2 1

Copyright DASSAULT SYSTEMES Use Properties (1/19) Easy modification of associative 3D tolerance specifications Marking Non-Semantic Annotations Free Rotation Text Properties Use Default Properties Copy Object Format Dimensions Properties Grouping Annotations Other Properties Enable / Disable annotation sets by list Enable / Disable 3D Annotations Queries Filters Mirror Annotations Clipping Plane Control of Leader Orientation Geometry Connection Management Enovia Integration

Copyright DASSAULT SYSTEMES Use Properties (2/19) Marking non-semantic annotations (1/1) This function will allow you to locate in 3D and graph, non semantic annotations for which semantic annotations axist (datum, datum target, geometrical tolerance and dimensions text Elements (text, frame or leader) This function is activated by setting.

Copyright DASSAULT SYSTEMES Use Properties (3/19) Free Rotation (1/1) This function will allow you to rotate text Elements (text, frame or leader) Just select the frame you want to rotate, activate the Free Rotation and drag corner point. Click on Free Rotation icon You can set a Rotation snap angle in Tools/Options/Mechanical Design/Tolerancing. If Automatic snapping is activated, the value of the snap angle is taken into account for the rotation of the annotation

Copyright DASSAULT SYSTEMES Use Properties (4/19) Text Properties (1/2) Once selected, you can change the text properties of a frame: By using the Properties contextual menu of the feature (MB3):

Copyright DASSAULT SYSTEMES Use Properties (5/19) Text Properties (2/2) By using Text Properties Toolbar: You can insert several symbol type in the Text editor You can change the position of the point that connects the text to the drawing or to an element Different kind of frame for the Text Editor are possible The text can be justified suing the well-known icon The text properties allows you to modify Font, Style, Size…

Copyright DASSAULT SYSTEMES Use Properties (6/19) Use Default Properties (1/1) You can set the graphic properties of a frame as default properties. To define the default properties, select the textual annotation to be used as the default one. Right-click to select the Set as default option in the contextual menu Every time you want to create a textual annotation with these same properties, click the Only User Default Properties icon and then create a new annotation

Copyright DASSAULT SYSTEMES Use Properties (7/19) Copy Object Format (1/1) You can apply the Graphic properties of a textual annotation to other existing ones. 2 First, you select the annotation to be modified Now, graphic properties of both annotations are identical 1 3 Then, click on Copy Object Format icon and select the reference object

Copyright DASSAULT SYSTEMES Use Properties (8/19) Dimensions Properties (1/1) You can modify Dimension Properties by using Toolbar Dimension Line You can change the tolerance description Tolerance value Numerical Display Description (depends on the selected feature or on the set of surfaces) Projected dimension Force Dimension on Element Force Horizontal Dimension in View Force Vertical Dimension in View True Length Dimension These options are only available when Dimensions icon is activated and when you want to create a new dimension Precision

Copyright DASSAULT SYSTEMES Use Properties (9/19) Grouping annotations (1/1) You can attach an annotation you are creating to an existing annotation. Groups of annotations can gather as many annotations as you wish. First, click the annotation icon you want to create to specify a new element. Then, select the annotation to which you want to attach the annotation you are going to specify. Click OK to confirm the creation of the new annotation, the two annotations are grouped. It is possible to drag and drop the group to the location of your choice. It is possible to edit the properties (MB3) of the group.

Copyright DASSAULT SYSTEMES Use Properties (10/19) Others (1/1) In the pop up menu (MB3) annotations, you can access some other properties. You can add a Leader In the pop up menu (MB3) of a Breakpoint, you can access some other properties Type of Annotation You can create some positional links (between annotations and geometry or between two annotations) and check them You can transfer existing 3D annotations to another Annotation plane. You can also transfer an annotation to a new view while creating this annotation. Remove a Leader Change the symbol of the Leader extremity Add or Remove breakpoint

Copyright DASSAULT SYSTEMES Use Properties (11/19) Enable / Disable annotation sets by list (1/2) Ability to select by list the annotation sets to be displayed or not in the CATIA session Click on Enable / Disable annotation sets by list icon 1 This window is displayed. You can choose which set must be disable. Then click OK. 2

Copyright DASSAULT SYSTEMES Use Properties (12/19) Enable / Disable annotation sets by list (2/2) All annotations are hidden in the CATIA session. There are also no annotations in the navigation tree 3 All annotations are hidden By the same method, it is possible to display annotations which have been hidden before

Copyright DASSAULT SYSTEMES Use Properties (13/19) Enable / Disable 3D annotations Queries (1/1) The option is activated by default. When picking an annotation around the 3D part or product or in the navigation tree, the related geometry features are highlighted in 3D. When picking geometry, the related 3D annotations are highlighted in 3D and in the navigation tree. Note that the option is activated by default When picking the annotation, the geometry or the navigation tree, then all the entities are highlighted if this option is activated

Copyright DASSAULT SYSTEMES Use Properties (14/19) Filters (1/1) You can apply filters in order to show only some entities. You can filter the display of annotations in the 3D viewer using the following criteria: by type (non semantic), by sub-type (text, datums, datum targets, geometrical tolerances), by feature or geometrical element, by annotation plane. The default filter is ALL to display all the FT&A annotations. In the Results window, you can see some indications resulting of applied filter FT&A objects are accessible by type and attributes using Edit+Search capabilities

Copyright DASSAULT SYSTEMES Use Properties (15/19) Mirror Annotations (1/1) This function will allow you to mirror reversed annotation relative to the screen view. Select the annotation to be mirrored 1 3 The annotation is mirrored in order to make it readable Click on Mirror Annotations icon 2

Copyright DASSAULT SYSTEMES Use Properties (16/19) Clipping Plane (1/1) This function will allow you to clip a part according to the annotation plane in relation to its normal. Click on Clipping Plane icon The part is clipped according to the annotation plane in relation to its normal Annotation Plane

Copyright DASSAULT SYSTEMES Use Properties (17/19) Control of Leader orientation (1/1) This function will allow you to manage the orientation of the leaders Default orientation is defined by settings 3

Copyright DASSAULT SYSTEMES Use Properties (18/19) Geometry Connection Management (1/1) This function will allow you to Add/Remove/Replace of components or geometry Management the impact of a modification Check the validity Rename a component a part according to the annotation plane in relation to its normal. Acces to this function by MB3 key

Copyright DASSAULT SYSTEMES Use Properties (19/19) ENOVIA Integration (1/1) Save of FTA data in ENOVIA All the sets of annotations attached to each level of the product structure are stored individually in the database The FTA set of annotations and their links to the parts are exposed in the ENOVIA application On demand, load of FTA data from the ENOVIA application

Copyright DASSAULT SYSTEMES Generate Check Report Report customisation and Report You can generate different settings in order to generate a check report: a set of rules extracted from tolerancing standards is checked for each datum and tolerance specification. Activate this function to generate a check report taking into account the settings defined on the right. It indicates which rules are break (identical to knowledgeware report capabilities for a rule base. The option Show Results allows you to organize your report data into categories To include or nor help messages in the report file Available output formats and directory To include only information about the features for which the checks are valid, invalid or both

Copyright DASSAULT SYSTEMES The 2D extraction You will become familiar with how to extract view in order to create a drawing from Annotation plane. View from 3D

Copyright DASSAULT SYSTEMES View from 3D (1/2) A 3D view can be extracted in a drawing (including geometry and annotations). Generative Drafting Workbench FT&A Workbench Annotations have been transferred between views

Copyright DASSAULT SYSTEMES View from 3D (2/2) In the drafting workbench, you can use the View from 3D function which allows you to extract some Views from the 3D part. Generative Drafting Workbench View from 3D You can see on the drawing only the annotations defined in the view you have projected. The drawing is generative. All the annotations planes can be used for 2D extraction.

Copyright DASSAULT SYSTEMES To Sum Up In this course you have seen : You can quickly start to add 3D Annotations to a 3D model How easy it is to mange views How to create different 3D Annotations How to manage a 2D extraction to obtain a drawing including the 3D Annotations How to manage and modify 3D Annotations