Copyright DASSAULT SYSTEMES CATIA Part Design Advanced CATIA Training Foils Version 5 Release 8 January 2002 EDU-CAT-E-PDG-AF-V5R8

Copyright DASSAULT SYSTEMES day Course Presentation Objectives of the course In this course you will complete the knowledge acquired in the CATIA Part Design Fundamentals course Targeted audience New CATIA V5 users Prerequisites CATIA Part Design Fundamentals course

Copyright DASSAULT SYSTEMES Table of Contents (1/2) 1. Advanced Toolsp.5 Holes/Pockets/Pads not normal to sketch planep.6 Creating Groovesp.9 Creating Ribs and Slotsp.16 Creating Stiffenersp.27 Creating Loftsp32 3D Wireframep.67 Surface Based Featuresp.73 Advanced Draftp.80 Thicknessp.95 Using Transformationsp.97 3D Constraintsp.103 Local Axisp.108 Annotationp.116 Analysisp.127

Copyright DASSAULT SYSTEMES Table of Contents (2/2) 2. Part Managementp.137 Measure, Mean Dimensions, Scan, Parents-Childrenp.138 Cut, Paste, Isolate, Breakp.152 Inserting and Managing Bodiesp.159 Multi-Model Linksp.182 Scalingp.194

Copyright DASSAULT SYSTEMES Advanced Tools You will learn how to create and use other tools of Sketch-Based, Surface- Based and Dress-up Features. You will also learn tools of Transformations, 3D Constraints, Local Axis and Annotation. Holes/Pockets/Pads not Normal to Sketch Plane Creating Grooves Creating Ribs and Slots Creating Stiffeners Creating Lofts 3D Wireframe Elements Surface-Based Features Thickness Using Transformation 3D Constraints Local Axis Annotation

Copyright DASSAULT SYSTEMES You will learn how to create Holes, Pockets or Pads with their direction not perpendicular to their sketch Holes/Pockets/Pads not Normal to Sketch Plane Defining a direction

Copyright DASSAULT SYSTEMES Some Key Points: When creating a hole, a pocket or a pad, by default you get a result perpendicular to the sketch you have selected to get these features It is possible to define another direction by specifying a direction in the direction field The selected direction must not be in a plane parallel to the sketch plane nor in the same plane What are Holes/Pockets/Pads not Normal to Sketch Plane ?

Copyright DASSAULT SYSTEMES Holes/Pockets/Pads not Normal to Sketch Plane 1 If a Pad or Pocket, select Profile sketch to be used 2 De-Select Normal to Sketch and select reference 3 For this geometry, modify definition to include type Up to Plane and select Changes extrusion direction 4 Select the appropriate icon 5 Select limit surface on part You get:

Copyright DASSAULT SYSTEMES You will learn how to create grooves Creating Grooves Material removing according to a revolution body

Copyright DASSAULT SYSTEMES Creating Grooves 4 Select OK 2 Select the Groove icon 3 Define the limits of the groove Select the profile to be used for the groove (the sketch must contains an axis) 3 You get:

Copyright DASSAULT SYSTEMES Groove : 3d Line axis Select the Groove icon 1 2 Select the profile When creating a groove, it is possible to use a 3d line or a sketched line not included in the sketch of the profile as the rotation axis 3 Select the Axis field in the dialog box 4 Select the 3d line as the rotation axis You can modify the Limits parameters then select OK, you get: 5

Copyright DASSAULT SYSTEMES Groove : Reverse Side The Reverse Side button applies for open profiles only. This option lets you choose which side of the profile is to be extruded Select the Groove icon 1 Select the open sketch 2 Modify the Groove Limit Angles 3 Select the arrow to reverse the groove side (or click the Reverse Side button in the dialog box) 4 Select OK in the dialog box 5 You get:

Copyright DASSAULT SYSTEMES Additional Information (1/3) You can use sub-elements of a sketch to create grooves, like for pads or pockets

Copyright DASSAULT SYSTEMES Additional Information (2/3) You can create Grooves from sketches including several closed profiles. These profiles must not intersect

Copyright DASSAULT SYSTEMES Additional Information (3/3) If no sketches have been created when activating the Groove icon, you can access to the sketcher by selecting the Sketcher icon in the dialog box. When you have completed the sketch, you can leave the sketcher then you will return to the Groove creation Select the Sketcher icon in the dialog box

Copyright DASSAULT SYSTEMES In this lesson we will learn how to create the sketch based features known as Ribs and Slots Creating Ribs and Slots Creating Ribs Creating Slots

Copyright DASSAULT SYSTEMES A Rib is a profile swept along an open or closed Center Curve to create a 3D feature What is a Rib ? The profile can be swept along an open or a closed center curve to create the feature The center curve does not have to extend to the end, Merge Ends can be used to extend or shorten the rib to its proper wall The Profile of the Rib can be controlled by simply using one of the 3 choices under the Profile control section of the window

Copyright DASSAULT SYSTEMES A slot is a profile that is swept along an open or closed Center Curve to remove material from a solid What is a Slot ? The profile can be swept along an open or a closed center curve to remove the material The center curve does not have to extend to the end, Merge Ends can be used to extend or shorten the slot to its proper wall The Profile of the Slot can be controlled by simply using one of the 3 choices under the Profile control section of the window

Copyright DASSAULT SYSTEMES You will find Ribs useful when you need to sweep profiles from one surface to another When Should we Use Ribs and Slots ? Ribs and Slots will also be useful to create complex walls of parts that have many details in them. Here you can control your complexity in one sketch and not have many small sketches or geometric features to work with Slots and Ribs can be created on Planar as well as 3D Center Curves Also a Rib can be used to create a pipe by sweeping a profile along a center curve

Copyright DASSAULT SYSTEMES Creating a Simple Rib 1 Select the Rib icon 2 Select the 3D Center Curve 3 Select Pulling direction and then select the indicated surface Select the Profile to be swept 4 The Rib is displayed, select OK to create the Rib 5 The 3 Dimensional curve was created in the Wire Frame workbench

Copyright DASSAULT SYSTEMES Creating a Slot 1 Select the Slot icon 2 Select the Center Curve to Sweep around 3 The Slot is previewed and in this case the Profile Control is left at Keep Angle. Select OK to create the Rib Select the Profile to be swept 4 A Sketch for the Center Curve and the profile must exist prior to the icon being available for selection The depth of the profile must be equal to or less than the radius of the Center Curve

Copyright DASSAULT SYSTEMES Additional Information (1/5) Capability to edit the profile and center curve sketches during rib or slot creation or edition Access to to the sketcher for the profile Access to to the sketcher for the center curve

Copyright DASSAULT SYSTEMES Additional Information (2/5) You can use sub-elements of a sketch to create ribs, like for pads or pockets

Copyright DASSAULT SYSTEMES Additional Information (3/5) You can use sub-elements of a sketch to create slots, like for pads or pockets

Copyright DASSAULT SYSTEMES Additional Information (4/5) You can create Ribs and Slots from sketches including several closed profiles. These profiles must not intersect Rib Slot

Copyright DASSAULT SYSTEMES Additional Information (5/5) If no sketches have been created when activating the Rib or Slot icon, you can access to the sketcher by selecting the Sketcher icon. When you have completed the sketch, you can leave the sketcher then you will return to the Rib or Slot creation Select the Sketcher icon in the dialog box You could have use the same method to define the Center curve

Copyright DASSAULT SYSTEMES In this lesson we will learn how to create the sketch based features known as Stiffeners Creating Stiffeners Creating a Stiffener

Copyright DASSAULT SYSTEMES A Stiffener is a brace or rib that is added to a wall or a stand-off to add strength to the wall or stand-off and thus prevent breakage. It is commonly found on molded plastic parts or castings What is a Stiffener ? These two arrows are used to control the width of the part, it can be either symmetrical or all on one side or the other The other arrow is used to control the direction of the rib As with most features you can now access the sketch directly by selecting this button

Copyright DASSAULT SYSTEMES They can be used when you have a thin wall that you want to be more rigid without increasing the thickness of the wall When Should we Use Stiffener ? They can also be used when you have tall objects that are used to locate or support other objects and you want to prevent them from breaking off the surface they are attached to

Copyright DASSAULT SYSTEMES Creating Stiffeners 1 Select the Stiffener Icon 2 Key in the Thickness of the Stiffener 3 If the direction is correct select OK to create the Stiffener Make sure the sketch is highlighted 4 You will find that in many cases need to add a small line segment on to the top of the angled line used to create your stiffener. This allows for a coincidence constraint to be created between the rib and the part

Copyright DASSAULT SYSTEMES Additional Information You can use sub-elements of a sketch to create stiffeners, like for pads or pockets

Copyright DASSAULT SYSTEMES Creating Lofts You will learn how to create Lofts and Removed Lofts Creating a Simple Loft Remove Lofts Coupling Closing Points

Copyright DASSAULT SYSTEMES In this lesson we will learn how to create Lofts Creating Simple Lofts

Copyright DASSAULT SYSTEMES A Loft can be a Positive (add material) or Negative (substract material) solid that is generated by two or more planar sections swept along a spine What is a Loft ? The Planar sections can be connected with Guide Lines Be aware Closing Points on the sketch must be aligned to get the proper orientation of the sections otherwise the loft would be twisted Directional arrows are provided to get the proper orientation of the Loft Guide Line Closing Point

Copyright DASSAULT SYSTEMES Lofts can be used for several reasons. To create complex solids. Or to create some transition geometry between two existing solids in a part When Should we Use Lofts and Removed Lofts ? Removed Lofts are used the same way when you wish to subtract a transitioned surface from another solid

Copyright DASSAULT SYSTEMES Loft Creation : Guide Lines (1) 1 Select the Loft icon 2 Select the sections the loft is going to pass through. The order in which you select the sections is important, it will define the order of connection between the sections (4a) The loft is passing through the sections and it is limited by the guide lines (2a) (2b) (2c) 3 Select the Guide option from the dialog box (3) 4 Select the Guide lines (4b) (4c) (4d) 5 Select OK (5)

Copyright DASSAULT SYSTEMES Loft Creation : Spine (1) 1 Select the Loft icon 2 Select the sections the loft is going to pass through. The order in which you select the sections is important, it will define the order of connection between the sections (4) From the first to the last section, the solid is generated by doing a sweep along the spine. The sections always stay fix in space (2a) (2b) (2c) 3 Select the Spine tab from the dialog box (3) 4 Select the Spine 5 Select OK (5)

Copyright DASSAULT SYSTEMES Loft Creation : Closing Point and Orientation Orientation of the section When selecting another section, it might happen that the section is orientated in the other direction than the previous one, so, to reverse the section orientation select the arrow which indicates the section orientation Closing point of the section To change the closing point of a section, select another point on this section

Copyright DASSAULT SYSTEMES Loft Creation : Tangent Surfaces 1 Select the first section 2 Select the surface (corresponding to the first section) the loft will be tangent to 3 Select the intermediary sections 4 Select the last section 5 Select the surface (corresponding to the last section) the loft will be tangent to 6 Validate You get : Result with the same sections but without any tangent surfaces (1) (2) (3) (4) (5)

Copyright DASSAULT SYSTEMES In this lesson we will learn how to create Remove Lofts Remove Lofts Creating Simple Remove Lofts

Copyright DASSAULT SYSTEMES The Remove Loft capability generates lofted material, by sweeping one or more planar section curves along a computed or user-defined spine, and then removes this material. The material can be made to respect one or more guide curves What is Remove Loft Material ?

Copyright DASSAULT SYSTEMES Remove Loft Material (1) 1 Select the Remove Lofted Material icon 2 Select the sections the loft is going to pass through. The order in which you select the sections is important, it will define the order of connection between the sections (You could have defined a spine or several guide lines, if no spine is selected, the system computes a spine for you) (2a) (2b) (2c) 3 Select OK (3) (2d)(2e)

Copyright DASSAULT SYSTEMES Remove Loft Material : Closing Point and Orientation Orientation of the section When selecting another section, it might happen that the section is orientated in the other direction than the previous one, so, to reverse the section orientation select the arrow which indicates the section orientation Closing point of the section To change the closing point of a section, select another point on this section

Copyright DASSAULT SYSTEMES Remove Loft Material : Tangent Surfaces 1 Select the first section 2 Select the surface (corresponding to the first section) the removed loft will be tangent to 3 Select the intermediary sections 4 Select the last section 5 Select the surface (corresponding to the last section) the removed loft will be tangent to 6 Validate You get : Result with the same sections but without any tangent surfaces (2) (1) (3) (4) (5)

Copyright DASSAULT SYSTEMES In this lesson we will learn how to use Coupling when creating Lofts Coupling Coupling when Creating Loft

Copyright DASSAULT SYSTEMES A Coupling tab in the loft and remove loft functions to compute the loft using the total length of the sections (ratio) or between the vertices of the sections or between the curvature discontinuity points of the sections or between the tangency discontinuity points of the sections What is Coupling when Creating Loft ? Vertices, Curvature Discontinuity, Tangency Discontinuity Vertices, Curvature Discontinuity Vertex

Copyright DASSAULT SYSTEMES Coupling when Creating Loft 1 Activate the Loft icon and select and orient the sections. 2 Select the Coupling tab from the dialog box A coupling tab in the loft and remove loft functions to compute the loft on the total length of the sections (ratio) or between the vertices of the sections or between the curvature discontinuity points of the sections or between the tangency discontinuity points of the sections (2) 3 Select the desired kind of coupling from the combo (1) 4 Select OK (3) (4)

Copyright DASSAULT SYSTEMES Coupling when Creating Loft : Ratio 1 Activate the Loft icon and select and orient the sections. 2 Select the Coupling tab from the dialog box A coupling tab in the loft and remove loft functions to compute the loft using the total length of the sections (ratio) (2) 3 Select Ratio from the combo (1) 4 Select OK (3) (4) The solid is passing through the sections and the variation between the sections is computed by a ratio corresponding to the length of each section You get :

Copyright DASSAULT SYSTEMES Coupling when Creating Loft : Tangency 1 Activate the Loft icon and select and orient the sections. 2 Select the Coupling tab from the dialog box (2) 3 Select Tangency Discontinuities from the combo (1) 4 Select OK (3) (4) The solid is passing through the sections and each section is split at each tangency discontinuity point. The solid is computed between each split section You get : A coupling tab in the loft and remove loft functions to compute the loft between the tangency discontinuity points of the sections

Copyright DASSAULT SYSTEMES Coupling when Creating Loft : Tangency then Curvature 1 Activate the Loft icon and select and orient the sections. 2 Select the Coupling tab from the dialog box (2) 3 Select Curvature Discontinuities from the combo (1) 4 Select OK (3) (4) The solid is passing through the sections and each section is split at each curvature discontinuity point. The solid is computed between each split section You get : A coupling tab in the loft and remove loft functions to compute the loft between the curvature discontinuity points of the sections

Copyright DASSAULT SYSTEMES Coupling when Creating Loft : Vertices 1 Activate the Loft icon and select and orient the sections. 2 Select the Coupling tab from the dialog box (2) 3 Select Vertices from the combo (1) 4 Select OK (3) (4) The solid is passing through the sections and each section is split at each vertex. The solid is calculated between each split section You get : A coupling tab in the loft and remove loft functions to compute the loft between the vertices of the sections

Copyright DASSAULT SYSTEMES Coupling when Creating Loft : Points of Discontinuity These two points are tangency and curvature discontinuity points. They are also vertices This point is a tangency and curvature continuity point. This point is a pure vertex To have a look at the different discontinuity, we have sketched a profile as shown below : These are the different kinds of points that CATIA can use to split the sections when creating lofts using coupling Segments Two arcs These two points are curvature discontinuity points. They are also vertices

Copyright DASSAULT SYSTEMES Loft: Manual Coupling (1/2) Activate the Loft icon select the sections and the guide curves (If necessary, change the section orientation) Double click in the Coupling field to display the Coupling window Select the Coupling tab then set the Sections coupling to Ratio When the sections of the lofted solid do not have the same number of vertices you may define a manual coupling instead of changing or creating closing points You get: Section1 Section2 Section3Guide1 Guide2 Guide3

Copyright DASSAULT SYSTEMES Loft: Manual Coupling (2/2) For each section select the vertex to be taken into account in the coupling. You can visualize the coupling curve if the corresponding option is checked. The Vertices selection must be done in the same order than the sections selection 4 5 Click OK to end lofted surface definition When the sections of the lofted solid do not have the same number of vertices you may define a manual coupling instead of changing or creating closing points You get: Note:To refine the shape of the lofted surface you can define another coupling curve : select the first coupling and click on the Add button, then define the new coupling curve as explained above. a b c Note: This is also possible with the Remove Loft command

Copyright DASSAULT SYSTEMES Manual Coupling: Displaying Uncoupled Points On this loft, the sections have not the same number of vertices and have some discontinuity in curvature and tangency For each coupling mode, the points that could not be coupled are displayed in the geometry with specific symbols Tangency mode : uncoupled tangency discontinuity points are represented by a square Tangency the Curvature mode : uncoupled tangency discontinuity points are represented by a square. Uncoupled curvature discontinuity points are represented by an empty circle Vertices mode : uncoupled vertices are represented by a full circle

Copyright DASSAULT SYSTEMES Loft: Relimitation (1/3) When the limitation option is checked, the loft is limited to the start or (and) end sections even is a larger spine or guide curves have been used By default the lofted surface is limited by the start and end sections. However you can choose to limit it on the spine or on the guide lines extremities Note: This is also possible with the Remove Loft command

Copyright DASSAULT SYSTEMES Loft: Relimitation (2/3) When the limitation option is unchecked, and when a spine has been used, the loft is limited by the spine extremities By default the lofted surface is limited by the start and end sections. However you can choose to limit it on the spine or on the guide lines extremities Note: This is also possible with the Remove Loft command

Copyright DASSAULT SYSTEMES Loft: Relimitation (3/3) When the limitation option is unchecked, and when guide lines have been used, the loft is limited by the guide lines extremities By default the lofted surface is limited by the start and end sections. However you can choose to limit it on the spine or on the guide lines extremities Note: This is also possible with the Remove Loft command Note: If a spine an guide lines have been used the loft will be limited on the shorter line

Copyright DASSAULT SYSTEMES In this lesson we will learn how to change the closing point when creating a Loft Changing the Closing Point

Copyright DASSAULT SYSTEMES When selecting the sections to create a loft (or remove loft), you can change the closing point after the selection of the sections and you can create a closing point anywhere on a section profile What is Changing the Closing Point when Creating Loft ?

Copyright DASSAULT SYSTEMES Changing the Closing Point when Creating Loft (1/6) 1 Activate the loft icon and select the first section 2 Select the second section (2) 3 Select the third section (1) (3)

Copyright DASSAULT SYSTEMES Changing the Closing Point when Creating Loft (2/6) 4 Click on Section2 (Label) 5 Select Replace Closing Point from the contextual menu, then select a new closing point (5) (4) (7) (5) 7 Select Replace Closing Point from the contextual menu, then select a new closing point (7) (6) 8 Select the arrows to reverse Section2 and Section3 (8) 6 Click on Section3 (Label)

Copyright DASSAULT SYSTEMES Changing the Closing Point when Creating Loft (3/6) 9 Check that the coupling is at Ratio then Select Apply in the dialog box You can see that the solid is twisted because the default closing point of Section1 is not aligned with the closing points of the other sections (9)

Copyright DASSAULT SYSTEMES Changing the Closing Point when Creating Loft (4/6) 10 In order to create a closing point on Section1, select the Section1 label with MB3, then select Remove Closing Point (10) A new dialog box corresponding to a point creation on a curve appears (11) The point appears in blue before validation 11 Then again, select Create Closing Point from the contextual menu

Copyright DASSAULT SYSTEMES Changing the Closing Point when Creating Loft (5/6) 12 Select the Distance on curve option (12) (14) 13 Select the Geodesic option 14 Enter 100 as the Length (13) 15 Select OK (15)

Copyright DASSAULT SYSTEMES Changing the Closing Point when Creating Loft (6/6) 16 Select the Coupling tab (16) (18) 17 Select Vertices option from the combo 18 Select OK (17) You get :

Copyright DASSAULT SYSTEMES You will learn more about 3D Wireframe Elements and how we use them to help construct our Part 3D Wireframe Elements Use of Wireframe Elements in Part Design

Copyright DASSAULT SYSTEMES What are 3D Wireframe Elements ? In the Part Design Workbench, we can create points, lines and planes without using the Sketcher. These elements belong to the Reference Element toolbar. In the Specification Tree, they are inserted under Open_Body which contain all 3D Wireframe elements. Even if these elements are some Wireframe Elements, we can use them with the Part Design Tools.

Copyright DASSAULT SYSTEMES A dialog Box is displayed 2 In Reference Toolbar, select Point by clicking on icon 1 Notice that we can choose between several types of points 3 The created point appears under Open_Body We create the desired point Creating 3D Wireframe Point

Copyright DASSAULT SYSTEMES A dialog Box is displayed 2 In Reference Toolbar, select Line by clicking on icon 1 Notice that we can choose between several types of lines 3 The created line appears under Open_Body We create the desired line Creating 3D Wireframe Line

Copyright DASSAULT SYSTEMES A dialog Box is displayed 2 In Reference Toolbar, select Plane by clicking on icon 1 Notice that we can choose between several types of planes 3 The created plane appears under Open_Body We create the desired plane Creating 3D Wireframe Plane

Copyright DASSAULT SYSTEMES Using 3D Wireframe Elements to Create a 3D Curve 1 You can create points in space according to their coordinates by using the Points tool from the Reference Element tool bar 2 Create the 3D curve by using the Curve in Space tool from the Free-Style Workbench This curve can now be used to extrude a rib or create a slot

Copyright DASSAULT SYSTEMES We will learn how to use all of the various types of Surfaced Based Features Split, Thick Surface, Close Surface and Sew Surfaces Surface Based Features Split Thick Surface Close Surface Sew Surface

Copyright DASSAULT SYSTEMES There are four Surface Based Features What is a Surface Based Feature and when Do You Use It (1/2) ? Thick Surface: Used to create solids from surfaces. Material can be added from either or both sides of the surface Split: Used to split a solid with either a plane or a surface.

Copyright DASSAULT SYSTEMES There are four Surface Based Features What is a Surface Based Feature and when Do You Use It (2/2) ? Sew Surface: Used to glue a surface feature to an existing 3D solid. Close Surface: Used to take a closed surface and turn it into a solid.

Copyright DASSAULT SYSTEMES Split 1 Select body to be split 2 Select splitting element 3 You can split a body with a plane, face or surface. A typical use is where internal structure must be trimmed and associated to an outer aerodynamic shape to allow rapid future change Select Split icon an arrow pointing to material to keep appears. Click to change direction if needed

Copyright DASSAULT SYSTEMES Thick Surface 1 Select surface to be thickened 2 Modify thickness offsets 3 The resulting feature does not keep the color of the original surface Select Thick Surface icon and the preview shows the corresponding upper and lower thickness

Copyright DASSAULT SYSTEMES Close Surface 1 Select Close Surface icon 2 Closed Surface appears in specification tree 3 Select surface to be closed

Copyright DASSAULT SYSTEMES Sew Surface 1 Select the object to sew surface to 2 Select surface to sew 3 Sewing means joining together a surface and a body. This capability consists in computing the intersection between a given surface and a body while removing useless material Select Sew Surface icon an arrow pointing to material to keep appears. Click to change direction if needed

Copyright DASSAULT SYSTEMES Advance Draft In this lesson we will see the Advanced Draft command Advanced Draft

Copyright DASSAULT SYSTEMES Select the View -> Toolbars -> Advanced Draft command to get the Advanced Draft toolbar The Advanced Draft command lets you draft basic parts or parts with reflect lines but it also lets you specify two different angle values for drafting complex parts. This task shows you how to draft two faces with reflect lines, and this by specifying two different angle values and by using both modes available. What is the Advance Draft Command ? (1/5) By default, the Advanced Draft toolbar is not accessible from CATIA, so in order to get it, you will have to select Views -> Toolbars -> Advanced Draft You will see the following toolbar:

Copyright DASSAULT SYSTEMES With the Advanced Draft command, you can define if you want to draft both sides or not and if you want to draft with reflect lines or not. To do so, you will have to activate one or two buttons as described hereafter What is the Advance Draft Command ? (2/5)

Copyright DASSAULT SYSTEMES The 1 st side tab is used to define the characteristics of the draft angle for the selected faces. If you have decided to draft both sides, you will have to define the draft angle characteristics for the second side using the 2 nd side tab. When drafting both sides with reflect lines, you can decide to get the draft angles independent or not What is the Advance Draft Command ? (3/5) To define the Faces to be drafted To define the neutral element To define the pulling direction To define the draft angle value To define if the angle are the same or not when drafting both sides

Copyright DASSAULT SYSTEMES To define the Parting Element, you will have to used the parting tab. The parting Element can be a plane, a surface or a face What is the Advance Draft Command ? (4/5) To define the parting element

Copyright DASSAULT SYSTEMES When you have decided to draft both sides with independent angle, you have to define the second side characteristics What is the Advance Draft Command ? (5/5) Neutral element To define the pulling direction To define the draft angle value To define if the angle are the same or not when drafting both sides

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (1/9) Select the Advanced Draft icon 1 You are going to see how to draft both sides using the Advanced Draft icon Activate these two buttons 2

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (2/9) As the object to be drafted, select this face 3

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (3/9) Select the No Selection option from the Neutral Element combo, then select the indicated plane 4

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (4/9) Enter 21 in the angle field 5 Select the parting tab 6

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (5/9) Select the Parting Element button 7 Select the Parting Element field 8

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (6/9) Select the indicated plane 9 Select the 2 nd side tab 10

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (7/9) Select the No Selection option from the Neutral Element combo, then select the indicated plane 11

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (8/9) Enter 45 in the angle field 12 Select Preview 13

Copyright DASSAULT SYSTEMES Advanced Draft Angle: Draft Both Sides (9/9) Select OK in the dialog box 14 You will see You get:

Copyright DASSAULT SYSTEMES We will see how to add material on a selected face by defining a thickness Thickness Thickness Creation

Copyright DASSAULT SYSTEMES Thickness 1 Multi-select faces to be thickened 2 Modify thickness definition of material to add in the dialog box 3 A standard use of thickness is when material has to be added or removed before machining a part. Thickness captures the design intent and allows rapid change Select Thickness icon Select the Other thickness faces field then select another face 4 Enter –5 in the Other thickness field then select OK 5 You get: –5mm

Copyright DASSAULT SYSTEMES In this lesson we will learn how to use all of the various types of Transformations Using Transformations

Copyright DASSAULT SYSTEMES Transformation is the ability to move a body either by translating it along an axis, rotating it around an axis or moving it symmetrically around a plane What is Transformation ? Geometry cannot be duplicated using a transformation Transformations come in 3 types : - Translation along an edge - Rotation about an axis -Symmetry around a plane

Copyright DASSAULT SYSTEMES Transformations are useful when you have created some geometry and decide that it needs to be moved, or rotated into a specific position When Should we Use a Transformation ? Transformations can only be used on either the whole Part Body or an individual Body within the Part There are some cases where it would not be easy to create the geometry in the plane that it is needed in because it requires the use of geometry not in the plane. You can create the geometry in the wrong plane and then rotate or translate to its proper position

Copyright DASSAULT SYSTEMES Translation 4 1 Select OK Select the Translation icon Enter the amount of translation or drag the icon, then select OK You can also define the direction using the contextual menu on the Direction field 3

Copyright DASSAULT SYSTEMES Select the Rotation icon Select an edge for rotation axis... …and enter the amount of rotation or drag the icon Rotation 1 2 You can also define the axis using the contextual menu on the Axis field Select OK 3

Copyright DASSAULT SYSTEMES Select OK Select plane defining the symmetry Select the Symmetry icon Symmetry Instead of a plane, you can use a Point as the Reference element Instead of a plane, you can use a Segment as the Reference element You can also define the Reference using the contextual menu on the Reference field

Copyright DASSAULT SYSTEMES In this lesson we will learn how to use 3D constraints 3D Constraints Creating and Using 3D Constraints

Copyright DASSAULT SYSTEMES A 3D Constraint is the same as any other constraint only it is applied in the 3D model itself. Basically you will note that some are reference type constraints and others are regular constraints. Creation is the same as in the sketcher, so we will concentrate on their usage here What is a 3D Constraint ? Normally, 3D constraints are modifiable and can be linked and driven as others are in the sketcher They are reference because there are general other constraints in the sketcher or implicit to the geometry that are constraining the geometry Reference constraints are shown in parenthesis and cannot be modified

Copyright DASSAULT SYSTEMES They can be used whenever you have 3D geometry that you wish to link to some type of 3D datum plane or surface When Do we Use 3D Constraints ? You may also find it useful when you are using Copy and Paste to locate the pasted piece of Geometry from where you wish They are also useful when you need to drive the location of a piece of geometry created earlier in the design from a piece of geometry created later in the model. Thus this will limit some of the need to re-ordering of the part

Copyright DASSAULT SYSTEMES Creating 3D Constraints 1 Select the Constraint icon and create a constraint between the left side surface and the hole on the left side of the part 2 Note: The first dimension created was not a reference dimension. No Parenthesis were on the value. The second dimension was a reference dimension because the hole is located with the sketch for the hole from the same or the right side edge Now repeat the process from the same side to the hole on the left side of the part

Copyright DASSAULT SYSTEMES Using 3D Constraints 1 We want to drive the location of Pocket.1 from Hole.2 created after it in the tree 2 Modify the constraint indicated in red to 25mm and the Pocket.1 is now driven from the Hole.2 location 3 Create the two constraints shown below from the center line of Hole.2 to the edges of the Pocket.1 Note: This capability will allow you to drive location of features in the tree from features created after them without having to do re-location of features in the tree.

Copyright DASSAULT SYSTEMES You will learn how to create a local axis in order to define local coordinates Local Axis

Copyright DASSAULT SYSTEMES It is possible to create a local axis in order to define local coordinates. For example, it is, sometime, easier to build a point by coordinates in a local axis rather than creating it in the absolute coordinates system What is a Local Axis ? Point created in the local coordinates system

Copyright DASSAULT SYSTEMES Local Axis : Creation It is possible to create a local axis in order to define local coordinates. For example, it is, sometime, easier to build a point by coordinates in a local axis rather than creating it in the absolute coordinates system Select the Axis System icon Select the local axis origin point (2) Select the OX direction Select the OY direction You get : (3) (4) Select OK in the dialog box (5)

Copyright DASSAULT SYSTEMES Local Axis : Use It is possible to create a local axis in order to define local coordinates. For example, it is, sometime, easier to build a point by coordinates in a local axis rather than creating it in the absolute coordinates system Set the axis system As the Current one with the contextual menu You get : Using the Point function (Coordinates options), create a point with X=0, Y=0 and Z=100 (1) 1 2

Copyright DASSAULT SYSTEMES Customizing Local Axis (1/3) Check Create an Axis System when creating a new part if you wish to create a three axis system which origin point is defined by the intersection of the default planes that is plane XY, plane YZ and plane ZX Select Tools -> Options 1

Copyright DASSAULT SYSTEMES Customizing Local Axis (2/3) In the Options dialog box, select Mechanical Design -> Part Design then the Part Document tab 2 Select the Create an Axis System when creating a new part option 3 Select OK 4

Copyright DASSAULT SYSTEMES Customizing Local Axis (3/3) Double click on Part in the dialog box 5 Select the File -> New command 6 The local axis is automatically created:

Copyright DASSAULT SYSTEMES Additional Information Local Axis dialog box To expand the dialog box To shrink the dialog box To define the axis system origin To define the OX axis To define the Oy axis To define the Oz axis To reverse the OZ axis To reverse the OY axis To reverse the OX axis

Copyright DASSAULT SYSTEMES Text with Leader Flag Note with Leader Annotation You will learn how to attach a text to a part and how to add hyperlinks to your document and then use them to jump to a variety of locations

Copyright DASSAULT SYSTEMES You will learn how to attach a text to a part Text with Leader

Copyright DASSAULT SYSTEMES A text with leader can be attached to a part in order to give information for example on surface treatment. This text can appears on the drawing What are Texts with Leader? Text Leader

Copyright DASSAULT SYSTEMES Select the Text with Leader icon Texts with Leader 1 Select the position of the leader on the part 2 Enter the text in the dialog box then select OK 3 Place the text and the leader by dragging the arrow or the square points 4 You get:

Copyright DASSAULT SYSTEMES Double click Additional Information To Modify the text of a text with leader, double click on the text, you will recover the dialog box where you can change the text Using the Properties command from the contextual menu will give you access to text, font and graphic modifications

Copyright DASSAULT SYSTEMES You will learn how to add hyperlinks to your document and then use them to jump to a variety of locations Flag Note with Leader

Copyright DASSAULT SYSTEMES A flag note with leader can be attached to a part in order to give information for example on surface treatment. This flag is an hyperlink that can start any documents such as a presentation, a Microsoft Excel spreadsheet or a HTML page on the intranet What are Flag Notes with Leader?

Copyright DASSAULT SYSTEMES Enter Part Process in the Name field Select the Flag Note with Leader icon Flag Notes with Leader (1/2) 1 Select the position of the leader on the part 2 3

Copyright DASSAULT SYSTEMES Flag Notes with Leader (2/2) You get: Place the text and the leader by dragging the arrow or the square points 5 Select the Browse button then select the file to which you want to be linked then select OK 4

Copyright DASSAULT SYSTEMES Select the Go to button in the dialog box Double click on the flag Using Flag Notes with Leader 1 Select the Link in the dialog box 2 3 The linked file is now started

Copyright DASSAULT SYSTEMES Additional Information To Modify the text of a flag note with leader, double click on the text, you will recover the dialog box where you can change the text Using the Properties command from the contextual menu will give you access to text, font and graphic modifications Double click You can have several files linked to a flag note

Copyright DASSAULT SYSTEMES Analysis You will learn how to analyze part in order to display the threads and tap, and to check if a part can be removed from mold in accordance with its draft angles Analysing Threads and Taps Draft Analysis

Copyright DASSAULT SYSTEMES You will learn how to display and filter out information about threads and taps contained in a part Analysing Threads and Taps

Copyright DASSAULT SYSTEMES When a part has been created with threads and taps, CATIA does not physically displays these features. There is a way to quickly know all the information about threads and taps by using the Thread and Taps Analysis icon What is the Threads and Tap Analysis ? You can display the threads or the taps or both of them You can display the threads and taps numerical values You can display threads or/and taps of a given diameter value

Copyright DASSAULT SYSTEMES Analysing Threads and Taps (1/2) You can display and filter out information about threads and taps contained in a Part Select the Tap – Thread Analysis icon Expand the dialog box using the More button 1 2 Select the criteria that will define the types of threads and taps that will be displayed 3 To show the threads or taps geometry To show the threads or taps values To show diameters with a given value To show taps To show threads

Copyright DASSAULT SYSTEMES Analysing Threads and Taps (2/2) Select Apply in the dialog box You get: 4

Copyright DASSAULT SYSTEMES You will learn how to analyze the draft angle on the surface of a part Draft Analysis

Copyright DASSAULT SYSTEMES The Draft Analysis command lets you analyze the draft angle on the surface of a part. You will be able to detect if the part you drafted will be easily removed from the associated mold What is the Draft Analysis ? This type of analysis is performed based on color ranges identifying zones on the analyzed element where the deviation from the draft direction, represented by the normal to the surface at a given point, corresponds to specified values The cursor manipulation for colors is limited to -20 and 20 but the analysis is performed between -90 and 90 degrees. To get a result, the view mode must be turned to Material display

Copyright DASSAULT SYSTEMES The Draft Analysis command lets you analyze the draft angle on the surface of a part. You will be able to detect if the part you drafted will be easily removed from the associated mold Select the Draft Analysis icon 1 Draft Analysis (1/2) Drag the red point of the Compass and drag it onto a face perpendicular to the direction of extraction 2

Copyright DASSAULT SYSTEMES Select the Invert analysis direction in the dialog box Draft Analysis (2/2) 2 You get: Everything in green is correct Everything in red is incorrect You have to take care of the light blue faces but it might correct You have to take care of the dark blue faces because it is certainly incorrect

Copyright DASSAULT SYSTEMES Additional Information Draft Analysis dialog box You can customize these colors by double clicking To smooth the analysis To fix a direction of extraction, uncheck the Locked direction option, and select a direction (a line, or a plane which normal is used), or use the compass manipulators, when available If you move the pointer over the green arrow (Normal), the inverted normal is displayed in dotted line Circles are displayed indicating the plane tangent to the surface at this point

Copyright DASSAULT SYSTEMES Measure, Mean Dimensions, Scan, Parents-Children Cut, Paste, Isolate, Break Inserting and Managing Bodies Multi-Model Links Sketch Selection with Multi-Documents Links Scaling Part Management You will learn Part Management tools that you will need to design complex parts and integrate these parts into a Multi-model Environment

Copyright DASSAULT SYSTEMES In this lesson, you will see how to measure angle and distance between geometrical entities, then how to replay the construction history of a part and isolate temporarily any feature to work locally, then to provide an accurate view of genealogical links between elements. We recommend you to use it before deleting elements Measure, Mean Dimensions, Scan, Parents-Children Measuring Elements Mean Dimensions Scanning a Part Parents-Children Relationship

Copyright DASSAULT SYSTEMES Measuring Elements means to get the angle and the distance between two geometric entities What is Measuring Elements ? Results Elements to be measured

Copyright DASSAULT SYSTEMES Measuring Elements 1 2 Set the desired type of Measurement Select the Measure Between icon 3 Select your reference (1) and target (2) elements 4 Minimum distance and angle (if you customize your dialog box) are displayed on the geometry and in the results Window

Copyright DASSAULT SYSTEMES When creating dimensional constraints, you can define a tolerance. Using the Mean Dimensions icon you can compute the mean dimensions and the part will be updated. This can be useful for a part to be machined What are Mean Dimensions? Dimension with a Tolerance Mean dimension

Copyright DASSAULT SYSTEMES Mean Dimensions (1/4) 1 2 Double click on the indicated dimension We are going to add tolerances on dimensions which have been created in the sketch of the shaft. Double click on Sketch.1

Copyright DASSAULT SYSTEMES Mean Dimensions (2/4) 3 4 In the appearing dialog box, enter 0.2 in the Maximum tolerance filed and enter 0.1 in the Minimum tolerance field then select OK Using the contextual menu on the Value field, select the Add Tolerance command 5 The tolerance is created. Select Ok in the Constraint Definition dialog box then Exit the sketcher Dimension with a tolerance

Copyright DASSAULT SYSTEMES Mean Dimensions (3/4) 6 7 Select OK To compute the mean dimensions, select the Mean Dimension icon 8 Select the Update All icon If you look at the dimensions in Sketch.1, you will see that they are changed to their means. The part is also updated

Copyright DASSAULT SYSTEMES Mean Dimensions (4/4) 9 10 Select OK To come back to nominal dimensions, select the Mean Dimension icon 11 Select OK 12 Select the Update All icon If you look at the dimensions in Sketch.1, you will see that they are changed to their nominal size. The part is also updated

Copyright DASSAULT SYSTEMES Scanning a part means to replay the construction history of a part and isolate temporarily any feature to work locally What is Scanning a Part ?

Copyright DASSAULT SYSTEMES Scanning a Part 1 2 Use the Scan tools to navigate through the part structure Select Edit > Scan... Menu option Backward: goes to the previous feature in the tree Forward: goes to the next feature in the tree Starting feature: feature active when starting scanning Last feature: last feature in the tree Exit: when you exit the active feature becomes in work (it is underlined in the tree) Initial part The Mirror.1 feature is in work: you can make local changes 3 4 To work again on the whole part, click the last feature in the tree and select the Define in work option in the contextual menu (MB3)

Copyright DASSAULT SYSTEMES The parents-children relationship provides an accurate view of genealogical links between elements. We recommend you to use it before deleting elements What is Parents-Children Relationship ? parents children Pad 1 Pad 2 Pad 3

Copyright DASSAULT SYSTEMES Pad 1 Parents-Children Relationship 2 Select the Parent-Children option 3 Activate the contextual menu on the desired feature (here, Pad.1) 1 The graph allows you to show all parents / children (MB3) Double-click a component to show/hide parents or children parents children

Copyright DASSAULT SYSTEMES Parents-Children (Edition) (1/2) Select the Parent/Children command from the contextual menu Parent Children command lets you edit features 1 2 You get:

Copyright DASSAULT SYSTEMES Parents-Children (Edition) (2/2) Select the Edit command from the fillet contextual menu Modify the fillet radius then select OK 3 4 You get: 5

Copyright DASSAULT SYSTEMES In this lesson, you will see how to cut or copy a feature and paste it onto a body and you will also see how to isolate or break 3D geometry from their parents Cut, Paste, Isolate, Break Cut/Copy and Paste (Drag and Drop) Isolate/Break

Copyright DASSAULT SYSTEMES Cut/Copy then Paste captures the node specified into the clipboard and either replaces (Cut) or copies (Copy) the content into a different selected point in the part structure. The action is interpreted by the system in a context sensitive manner. For example, if a pad is copied onto a different sketch, the new sketch is used for the profile and information on extrusion limits will be those of the pad. However, if pad1 is copied onto pad2, since this action has no real meaning, it is interpreted as generically copying the clipboards content into the part. The effect is to create another copy of pad1 (with its original sketch) in the part structure. This copy will be placed after whatever node is currently the In Work node What is Cut/Copy and Paste (Drag and Drop) ? Cut/Copy then Paste an be achieved by drag and drop. If the CTRL key is pressed during the drag and drop, the action is interpreted as a copy

Copyright DASSAULT SYSTEMES One way we can copy the limits of the circular pad to apply to the rectangular pad is to work within the Part tree and use the 3rd. Mouse button to Copy Pad.2 and Paste onto Sketch.3 Another variation for the fillet - Keeping the CTRL key pressed, Drag with the 1st. Mouse button to one of the base edges of the rectangular pad We can copy the draft by using another variation - 3rd. Mouse button to copy Draft.1 from the tree then select a vertical face on the rectangular pad and 3rd. Mouse button to Paste Cut/Copy and Paste (Drag and Drop) 2 3 1

Copyright DASSAULT SYSTEMES Isolate is used when 3D geometry is projected into a sketch in order to be modified and used as part of the sketchs profile. Isolate duplicates the element since the original element cannot be changed since other geometry depend on it What are Isolate and Break ? Break is used to divide an isolated element into two parts at a specified point (usually to use one side of this element in the sketch)

Copyright DASSAULT SYSTEMES Using the Trim and Break icon in the sketcher, modify the sketch as follows, then exit the sketcher Starting with the geometry below, we want to add a pad Isolate, Break (1/3) 2 1 Lines Added pad Diameter 100 Pad Intersection between the pad and the sketch plane Diameter 50 Create a pad with an length of 20 3

Copyright DASSAULT SYSTEMES Edit the Sketch of the first pad then change the circle diameter to 50 Select the Undo icon (may be several times) in order to come back to diameter 100 Exit the sketcher (Sketch.1) then, if necessary, Update the part. You will get: Isolate, Break (2/3) Edit Sketch.2, then place the cursor on the yellow line then select Isolate from the contextual menu 7

Copyright DASSAULT SYSTEMES Create two Coincidence between the isolated arcs and the cylinder then exit the sketcher Exit the sketcher then, if necessary, Update the part. You will get: Edit the Sketch (Sketch.1) of the first pad then change the circle diameter to 50 Isolate, Break (3/3)

Copyright DASSAULT SYSTEMES You will learn ways to manage Bodies using tools such as Assembling, Intersecting, Adding, Removing, and Trimming bodies Inserting and Managing Bodies Inserting a Body Assembling/Intersecting/Adding/Removing Bodies Union Trimming Bodies Removing Lumps Replacing a Body Change Boolean Type

Copyright DASSAULT SYSTEMES Using several bodies in a part allows you to design different step of a part without any operations between bodies. You will be able to perform operations (add, assemble, remove, …) later. This method can be use when, for example, you create a mold part. You can create the outside of the part in a body and the core in another one then you can remove the core from the main part. Later it will be easy for you to separate the part and it core What is Inserting a Body?

Copyright DASSAULT SYSTEMES A body is added in the tree In order to insert a Body, select the Insert -> Body command Inserting a Body 2 1 You can work in the PartBody or in Body.2. Top Switch from one Body to another, select the Define in workobject command from the contextual menu of the desired body

Copyright DASSAULT SYSTEMES Assembling/Adding : If Body2 is Assembled or Added to Body1, the operation between the bodies is a Union. The only difference between the two is that Assemble will respect the nature of features. If Body2 contains as its first node a Pocket feature (permissible), Assemble will see it as a Pocket and remove material from Body1. In this case, if Add is used, the Pocket will be seen by Body1 as a Pad What is Inserting and Managing Bodies ? Intersecting : The resulting material is the intersection between the two bodies Removing : If Body2 is Removed from Body1, the operation is Body1 minus Body2 Union Trim : The Union Trim is basically a Union with an option to remove or keep one side or the other. In the picture on the right, the purple face is selected to remove the right side and the blue face is selected to keep only the top side. For the Union Trim to work, the geometry must have sides that are clearly defined Remove Lump : All the above options work between two bodies. The Remove Lump works on geometry within a specific Body. If a single Body has material that is completely disconnected, each piece of disconnected material is defined as a Lump. The user can delete any Lump as a single entity even if the Lump is a combination of numerous features

Copyright DASSAULT SYSTEMES With the cursor on Body.2, select Assemble from the contextual menu (MB3) We want to assemble Body.2 with PartBody Assemble 2 1 You get: Body.2 contains a groove Because Body.2 contains a groove which is a feature that removes material, the result of the assemble operation is also removing material Select OK in the Dialog box 3

Copyright DASSAULT SYSTEMES With the cursor on Body.2, select Add from the contextual menu (MB3) We want to add Body.2 with PartBody Add 2 1 You get: Body.2 contains a groove Body.2 contains a single groove, so it is appears as a solid (even if it normally removes material). When you Add a Body, CATIA keeps the feature like it appears before the addition. Select OK in the Dialog box 3

Copyright DASSAULT SYSTEMES With the cursor on Body.2, select Remove from the contextual menu (MB3) We want to remove Body.2 from PartBody Remove 2 1 Select OK in the Dialog box 3 You get:

Copyright DASSAULT SYSTEMES Intersect We want to intersect Body.2 with PartBody 1 With the cursor on Body.2, select Intersect from the contextual menu (MB3) 2 Select OK in the Dialog box 3 You get:

Copyright DASSAULT SYSTEMES Union Trimming Bodies We want to do an Union Trim of Body.2 with PartBody 1 With the cursor on Body.2, select Union Trim from the contextual menu (MB3) 2 Select the Face to remove then the face to keep (Activate the corresponding field before in the dialog box) 3 You get: Select OK 4

Copyright DASSAULT SYSTEMES Removing Lumps (1/3) Cavity After certain operations, it may happen that some Lumps or Cavities appear in the part. We need to remove them. The Remove Lump command allows you to remove Lumps and Cavities Lumps Shell Pockets

Copyright DASSAULT SYSTEMES Removing Lumps (2/3) With the cursor on PartBody, select Remove Lump from the contextual menu (MB3) 1 Select the Faces to remove field in the dialog box 2 Select the two following faces belonging to the lumps to be removed 3

Copyright DASSAULT SYSTEMES Removing Lumps (3/3) In order to select a face of the cavity, place the cursor on the cavity to be remove then press the Up arrow key on the keyboard 4 Using the small arrows, highlight one of the cavity face 5 To confirm the face selection select the circle 6 Select OK 7 You get:

Copyright DASSAULT SYSTEMES Assembling a Set of Bodies (1/3) Assembling a set of bodies (Multi selected via the Ctrl key) is possible Using the Ctrl key, select the three following bodies to be assembled 1

Copyright DASSAULT SYSTEMES Assembling a Set of Bodies (2/3) With the cursor placed on the last body, select the Assemble command from the contextual menu 2

Copyright DASSAULT SYSTEMES Assembling a Set of Bodies (3/3) Select OK in the dialog box 3 You get:

Copyright DASSAULT SYSTEMES You can replace a body use in an operation by another one What is Replacing a Body?

Copyright DASSAULT SYSTEMES Select the Replace command from Body.3 contextual menu Replacing a Body (1/3) 1 Body to be replaced Replacing body Select Body.4 2

Copyright DASSAULT SYSTEMES Select the following line in the dialog box Replacing a Body (2/3) 3 Select the following face. This face is the face that will be removed during the Union Trim operation 4 Select OK 5

Copyright DASSAULT SYSTEMES If necessary, update the part by selecting the Update All icon Replacing a Body (3/3) 6 You get:

Copyright DASSAULT SYSTEMES Change Boolean Type (1/4) The initial part is composed of three bodies. Assemble Body.1 to Part Body. 1 Remove Body.2 from Assemble.1. You obtain Remove.1. 2

Copyright DASSAULT SYSTEMES Change Boolean Type (2/4) Click with the right button mouse on Remove.1. In the contextual menu, select Remove.1 object 3 Choose now the new operation. For example, click on Change To Assemble. 4

Copyright DASSAULT SYSTEMES Change Boolean Type (3/4) You obtain : 5 Change now Assemble.2 to Union Trim. You obtain : 6

Copyright DASSAULT SYSTEMES Change Boolean Type (4/4) You can edit Trim.1. For instance, select the cylinder's top face as the face to keep. You obtain : 7

Copyright DASSAULT SYSTEMES You will learn ways to use Multi-model links to help propagate design changes Multi-Model Links Establishing Multi-Model Links

Copyright DASSAULT SYSTEMES The concept of working within an independent Body and then having the ability to Add, Remove, or Intersect this Body with our Master PartBody gives us this added modeling flexibility What are Multi-Model Links ? There are different ways that the independently modeled Body can be assimilated into the PartBody

Copyright DASSAULT SYSTEMES In a CATIA session you have two separate parts Establishing Multi-Model Links (1/3) 1 Using the Contextual Menu, copy the PartBody of Part2 2 Place the cursor on the PartBody of Part1 then Select Paste Special from the contextual menu 3

Copyright DASSAULT SYSTEMES In the dialog box, select AsResultWithLink and the Paste button, then select OK Establishing Multi-Model Links (2/3) Part1 becomes: 4 In Sketch.1 of part1, create a distance (10mm) between the circle and the copied cylinder then exit the sketcher 5 3

Copyright DASSAULT SYSTEMES Now, in Sketch.1 of part2, create a diameter constraint of 50 then exit the sketcher Establishing Multi-Model Links (3/3) Part1 becomes: 7 With Part1 active, select the Update All icon 8 6 You get:

Copyright DASSAULT SYSTEMES Sketch Selection with Multi-Documents Links It is now possible to copy and paste with link a sketch from a document to another one

Copyright DASSAULT SYSTEMES Sketch Selection with Multi-Documents Links (1/5) After loading a part containing a sketch, start a new part using the File + New command 1 2 Display the two parts using the Window + Tile Horizontally command You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case of modification of the original sketch the document in which the copy is used will be also modified You get:

Copyright DASSAULT SYSTEMES Sketch Selection with Multi-Documents Links (2/5) With the cursor on Sketch.1 in the tree, select the Copy command from the contextual menu (MB3) 3 4 In the second part, place the cursor on PartBody, then select Paste Special from the contextual menu (MB3) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case of modification of the original sketch the document in which the copy is used will be also modified

Copyright DASSAULT SYSTEMES Sketch Selection with Multi-Documents Links (3/5) Select AsResultWithLink in the dialog box 5 6 Expand Sketch.1 in order to see what has been copied (by selecting +) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case of modification of the original sketch the document in which the copy is used will be also modified

Copyright DASSAULT SYSTEMES Sketch Selection with Multi-Documents Links (4/5) Create a 20mm height pad using the copied sketch 7 8 In the first part, modify the sketch as follows You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case of modification of the original sketch the document in which the copy is used will be also modified

Copyright DASSAULT SYSTEMES Sketch Selection with Multi-Documents Links (5/5) To take the modification into account in the second part (the one which contains the copied sketch), place the cursor on Part2 then select the Part2object + Update All Links command 9 You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case of modification of the original sketch the document in which the copy is used will be also modified You get:

Copyright DASSAULT SYSTEMES As specified in Part document: The copied element can be modified and has no link with the original one. The original element is duplicated AsResultWithLink: The copied element cannot be modify (it is a datum)but in case of modification of the original element, the copied one is updated Additional Information The different Paste Special options:

Copyright DASSAULT SYSTEMES You will learn how to apply an affinity to a part with reference to a point Scaling Scaling/Affinity

Copyright DASSAULT SYSTEMES A scaling is a part transformation which is calculated by selecting a reference point and by entering a ratio What is Scaling ? The system computes the distance between all the points of the outer skin of the part and the reference point, then these distances are multiplied by the ratio to get the new distances between the reference point and all the point of the new outer skin

Copyright DASSAULT SYSTEMES You can also resize a body in relation to a face or plane by selecting it instead of a reference point. The body will scale with it. You will obtain an affinity Select the reference point Select the Scaling icon Modify scaling ratio then select OK Scaling/Affinity You get: