Copyright DASSAULT SYSTEMES Wireframe and Surface Design Fundamentals CATIA Training Foils Version 5 Release 8 January 2002 EDU-CAT-E-WFS-FF-V5R8
Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will see how to create wireframe construction elements and enrich existing 3D mechanical part design with wireframe and basic surface features. Targeted audience New CATIA V5 users Prerequisites Part Design, Sketcher 1 day
Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to Wireframe and Surface Designp.6 2. Creating Wireframe Geometryp.12 Creating Points in 3Dp.13 Creating Lines in 3Dp.21 Creating Planes p.29 Creating Curves in 3Dp Creating Basic Surfacesp.67 Creating a Surface from a Profilep.68 Creating a Spherical Surfacep.72 Creating a Swept Surfacep.74 Creating a Surface from another Surfacep.80 Creating a Surface from Boundariesp.85
Copyright DASSAULT SYSTEMES Table of Contents 4. Performing Operations on the Geometryp.117 Joining Elementsp.118 Healing Elementsp.123 Restoring Elementsp.126 Disassembling Elementsp.128 Splitting Elementsp.130 Trimming Elementsp.136 Creating Elements from Surfacesp.141 Transforming Elementsp.146 Extrapolating Elementsp.158 Creating a Near Elementp.164 Creating Patternsp Completing the Geometry in Part Designp Modifying the Geometryp.184
Copyright DASSAULT SYSTEMES Table of Contents 7. Using Toolsp.189 Stacking Commandp.190 Manipulating Elementsp.197 Creating Datum Featuresp.203 Working on Supportp.208 Updating a Partp.215 Managing Open-Bodiesp.219 Checking Connections between Elementsp.225
Copyright DASSAULT SYSTEMES Introduction to Wireframe and Surface Design You will become familiar with the Wireframe and Surface Design workbench Accessing the Wireframe and Surface Design Workbench Wireframe and Surface Design Workbench User Interface Wireframe and Surface Design Workbench Terminology Wireframe and Surface Design Workbench General Process
Copyright DASSAULT SYSTEMES Accessing the Workbench (1/2) To access the Wireframe and Surface Design Workbench start CATIA, then select the Start menu choosing Mechanical Design and Wireframe and Surface Design. Wireframe and Surface Design Workbench icon The first time you access the Wireframe and Surface Design Workbench, an Open body.1 is created which contains geometric elements.
Copyright DASSAULT SYSTEMES Accessing the Workbench (2/2) Once you are in the Wireframe and Surface Design workbench the associated toolbars are displayed : Wireframe GeometrySurface elements Operations and Transformations Tools Replication Tools
Copyright DASSAULT SYSTEMES You can work in 2D using the Sketcher The User Interface (1/2) You are in the Wireframe and Surface Design Workbench Operations on wireframe elements and surfaces Part tree You are creating elements in an Open body. Wireframe and surface features Standard tools Tools are provided in 6 toolbars.
Copyright DASSAULT SYSTEMES The User Interface (2/2) You also have access to the Wireframe and Surface Design tools through the menus.
Copyright DASSAULT SYSTEMES Part2 is a combination of PartBody and Open Body that means: PartBody contains the features used to create a solid Open body.1 contains the features used to create surface elements. It includes wireframe elements, sketch, etc... When you enter the Wireframe and Surface Design workbench an Open body is activated or created to contain wireframe and surface elements. At any time you can insert an Open body to create wireframe and surface elements. Terminology When you are in the Part Design workbench and you want to create Reference Elements as points, planes, lines, an Open body is automatically created inside PartBody to contain these elements.
Copyright DASSAULT SYSTEMES Creating Wireframe Geometry You will become familiar with the creation of wireframe geometric elements Creating Points in 3D Creating Lines in 3D Creating Planes in 3D Creating Curves in 3D
Copyright DASSAULT SYSTEMES You will learn the different ways to create points in 3D Creating Points in 3D
Copyright DASSAULT SYSTEMES What about points ? - A point can be defined by its coordinates from a reference point (origin or selected point). - A point can be defined with respect to an element. Default color codes for points:. Blue for point or projection of point in creation. White when created. Green for reference To support creation of all geometrical elements and to use them as reference for any creation. Why Do You Need Points ? Coordinates On plane Between On curve You can edit any type of point by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the Point Definition box. In some cases you can reverse the direction of creation of the point, clicking either the red arrow on point or the Reverse Direction button in the Point Definition box. Identification in tree
Copyright DASSAULT SYSTEMES The Point Definition dialog box offers you various methods to create points. 1 Click on Point Icon 2 Select one of these Point type options. 3 Enter point specifications in the Point Definition box and confirm. Let s see now the different ways to create points... The dialog box contents changes according to the selected Point Type option. Creating Points…
Copyright DASSAULT SYSTEMES Enter the coordinates of the point. Creating a Point Giving its Coordinates 3 Click OK to confirm point creation. 2+ Select the reference point if you want it different from the origin point. Origin point (0,0,0) Reference point Created point
Copyright DASSAULT SYSTEMES Select the curve on which the point will be created. If you do not select a reference point the default one will be the curve extremity. If the reference point you select is not on the curve it will be projected normally onto the curve. 3 Enter point specifications. Reference Point.2 Creating a Point on a Curve (1/3) Distance to reference = 50 Extremity Point.1 Extremity Point.3 Created Point.4 If you click on one of these buttons you directly create a point on the nearest extremity or at the middle of the curve. Curve Geodesic Euclidean
Copyright DASSAULT SYSTEMES Creating a Point on a Curve (2/3) If you want to create several points on the selected curve check the option Repeat object after OK. Click OK to continue. The created point is defined as an Object, i.e. the reference for creating the other points. 6.1 Define the number of points to be created. If no reference is selected for the Object point the default second point is the nearest extremity of the curve. In that case the arrow located on the Object point can be inverted to choose on which side of the curve the points will be created. If a reference is defined for the Object point the second point is identical to the reference point. You can create automatically the planes normal to the curve at each created point. The point instances are grouped in a new Open Body (unless you uncheck the option).
Copyright DASSAULT SYSTEMES Creating a Point on a Curve (3/3) 7 Click OK to confirm point creation. 6.2 You can also choose to define the number of points to be created and the spacing between the points. Reference Point.2 Object Point.4 Repeated Point.5 and Point.6
Copyright DASSAULT SYSTEMES Select the surface on which the point will be created and enter point specifications. If you do not select a reference point, the default one will be the surface center. If the reference point you select is not on the surface, it will be projected onto the plane. Created Point.5 Distance = 50 Components means direction from the reference point to the created point. You can choose another direction by selecting a line or a plane to get its normal. Creating a Point on a Surface Reference Point.3 3 Click OK to confirm point creation.
Copyright DASSAULT SYSTEMES You will learn the different ways to create lines in 3D Creating Lines in 3D Line between two points Line from a point and a direction Line with a curve as reference Line tangent to a curve Line normal to a surface Bisecting Line
Copyright DASSAULT SYSTEMES What about lines ? A line can be created: from points or vertices* on a curve on a support * Vertices are visible neither in the tree nor in the geometry ; they are auto-detected and selectable when passing the mouse over them. You can use lines as guide, reference, axis, direction or join to create other geometric elements. Why Do You Need Lines ? Identification in tree You can edit any type of line by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the Line Definition box. Point- Direction Angle/Normal to curve Tangent to curve Normal to surface Point-Point This option allows you to create the line on a support surface.
Copyright DASSAULT SYSTEMES In some cases you can reverse the direction of creation of the line, clicking either the red arrow on line origin or the Reverse Direction button in the Line Definition box. What about Lines ? Line origin Graphic manipulators Modification of line parameters (length, orientation) You can modify the line length keying in start and end value in the Line Definition box or dragging the graphic manipulators.
Copyright DASSAULT SYSTEMES The Line Definition dialog box offers you various methods to create a line. 1 Click on Line icon 2 Select one of these Line type options. The dialog box contents changes according to the selected Line Type option Let s see now the different ways to create lines... 3 Enter line specifications in the Line Definition box and confirm. Creating Lines…
Copyright DASSAULT SYSTEMES Select two points or vertices. Creating a Line between Two Points (1/2) Sketch vertexPoint.1 Line.1 is created between a vertex of Sketch.1 and Point.1. 3 Optional : extend the line at the start or/and end point(s). The Mirrored extent option allows you to impose the same extrapolation on either end of the line.
Copyright DASSAULT SYSTEMES Creating a Line between Two Points (2/2) 4 Optional : you can define a support (plane or surface) onto which the line will be projected. 5 Click OK to confirm line creation. Four vertices can be detected on the created line : the two initial points and the limit point of each extrapolation. Selectable vertices
Copyright DASSAULT SYSTEMES Select a reference point and a direction line then key in the start and end points of the line. 3 Click OK to confirm line creation. Creating a Line from a Point and a Direction Optional: You can define a support element onto which the line will be projected Reference point Direction Line length The Mirrored extent option allows you to impose the same extrapolation on either end of the line.
Copyright DASSAULT SYSTEMES Select a reference surface and a point. A vector normal to the surface is displayed at the reference point. 3 Click OK to confirm line creation. Creating a Line Normal to a Surface Reference point Reference surface Line length 2+2+ Check the Mirrored extent option to create the symmetry of the line with respect to the selected point.
Copyright DASSAULT SYSTEMES You will learn the different ways to create planes in 3D Creating Planes in 3D Plane offset from another plane Plane parallel to another plane through a point Plane with an angle or normal to a plane Plane through three points Plane through two lines Plane through a point and a line Plane through a planar curve Plane normal to a curve Plane tangent to a surface Plane created from its equation Plane mean through points Several planes between two planes
Copyright DASSAULT SYSTEMES What about planes ? You can create a plane from: another plane points, lines or curves its equation You can use planes as reference elements to create new geometry or as cutting elements. Identification in tree Angle/Normal to plane Equation Through 3 points Offset You can edit any type of plane by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the Plane Definition box. You can modify the plane location dragging it after clicking on the Move label. Why Do You Need Planes ?
Copyright DASSAULT SYSTEMES What About Planes ? You can modify the plane offset keying in the offset value in the Plane Definition box or dragging the graphic manipulator. Graphic manipulator Modification of plane parameters (offset, orientation) In some cases you can reverse the direction of creation of the plane, clicking either the red arrow on plane origin or the Reverse Direction button in the Plane Definition box. Plane origin
Copyright DASSAULT SYSTEMES The Plane Definition dialog box offers you various methods to create a plane. 1 Click on Plane icon 2 Select one of these Plane type options. The dialog box contents changes according to the selected Plane Type option. Let s see now the different ways to create planes... 3 Enter plane specifications in the Plane Definition box and confirm. Creating Planes…
Copyright DASSAULT SYSTEMES Creating an Offset Plane (1/2) 2 If you want to create several planes separated by the same offset value, check the option Repeat object after OK. 4 Select the reference element (plane, face, etc…). 3 Define the offset value, either in the Offset field or using the graphic manipulators. Reference plane
Copyright DASSAULT SYSTEMES Creating an Offset Plane (2/2) 6 Define the number of planes to be created. 7 Click OK to confirm plane creation. As many planes as indicated in the Object Repetition dialog box are created, in addition to the object plane. The planes are separated from the object plane by a multiple of the offset value. Object plane Plane instances in Open Body Click OK to continue. The created plane is defined as an Object, i.e. the reference for creating the other planes. 5 Object plane The plane instances are grouped in a new Open Body (unless you uncheck the option).
Copyright DASSAULT SYSTEMES Click OK to confirm plane creation. 1 Creating a Plane Parallel Through a Point 2 Select the reference element (plane or planar face) and the point. The plane parallel to the reference and passing through the point is displayed.
Copyright DASSAULT SYSTEMES Click OK to confirm plane creation. 1 Creating a Plane Through a Planar Curve 2 Select the planar curve. The plane passing through the curve is displayed. Planar curve
Copyright DASSAULT SYSTEMES Click OK to confirm plane creation. 2 Creating a Plane Normal to a Curve Select a reference curve and a point. A plane is displayed normal to the curve at the specified point. You can select any point. By default the middle point of the curve is selected.
Copyright DASSAULT SYSTEMES Click OK to confirm plane creation. 2 Select a surface and a point. The plane passing through the point and tangent to the surface is created. Creating a Plane Tangent to a Surface Surface Point
Copyright DASSAULT SYSTEMES You will learn the different ways to create curves in 3D Creating Curves in 3D Curve projected onto a support Combined curve Reflect line Intersection of geometric elements Curve parallel to another on a support Circle Corner Connect curve Conic Spline curve Helix Spiral Polyline
Copyright DASSAULT SYSTEMES What about curves ? a curve can be created from: points, other curves or surfaces You can use curves as guide or reference to create other geometric elements or as limits of a surface. Why Do You Need Curves ? A spline is a curve passing through selected points with the option to set tangency conditions at its extremities. You can edit any type of curve by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the corresponding definition box.
Copyright DASSAULT SYSTEMES A dialog box is displayed for each type of curve, e.g.: 1 Click on the icon corresponding to the selected type of curve. 2 Let s see now the different ways to create 3D curves... 3 Enter curve specifications in the dialog box and confirm. Creating Curves…
Copyright DASSAULT SYSTEMES Select the element(s) to project (Ctrl key if several elements) and the support ; you can keep the Normal direction or select a direction. Click OK to confirm projection curve creation. Support Projected elements Creating a Curve Projected onto a Support Elements to project 2+2+ Using the right mouse button on the Projected field you can access the list of elements to be projected and modify it.
Copyright DASSAULT SYSTEMES Creating a Combined Curve (1/2) Choose the Combine type from the combo: Normal or Along directions. Curve 1 Curve 2 Direction 1 Direction 2 Select the two curves to be combined and if needed the direction of extrusion for each curve. 3 A combined curve is the intersection of the extrusion of two planar curves.
Copyright DASSAULT SYSTEMES Creating a Combined Curve (2/2) Click OK to confirm combined curve creation. 4 The curve extrusion is performed normal to each curve. For each curve the direction of extrusion is defined by a line. Resulting combined curve Direction 1 Direction 2
Copyright DASSAULT SYSTEMES Select a support surface and a direction. Creating a Reflect Line 4 Click OK to confirm reflect line creation. Support Key in an angle representing the value between the selected direction and the normal to the surface. Direction 3 Reflect line
Copyright DASSAULT SYSTEMES Select the element(s) to intersect (Ctrl key if several elements) then the intersecting element. Creating the Intersection of Geometric Elements 3 Click OK to confirm intersection curve creation. Using the right mouse button on the Element 1 field you can access the list of elements to be intersected and modify it When possible, you can select the type of element created while computing the intersection.
Copyright DASSAULT SYSTEMES Creating a Curve Parallel to Another on a Support (1/2) 2 Select the reference curve and the support and key in the offset between the two curves. Click OK to continue. The curve created on the side of the red direction arrow is defined as an Object, i.e. the reference for creating the other curves. If you want to create several parallel curves separated by the same offset check the option Repeat object after OK. 4 5 Check the Both Sides option if you want one parallel curve on either side of the reference curve. 3 Reference curve Object parallel curve Parallel curve on second side
Copyright DASSAULT SYSTEMES Define the number of parallel curves to be created. 7 Click OK to confirm parallel curve creation. As many parallel curves as indicated in the Object Repetition dialog box are created, in addition to the object parallel curve. The parallel curves are separated from the object line by a multiple of the offset value. Creating a Curve Parallel to Another on a Support (2/2) Object parallel curve Parallel curve instances in Open Body The plane instances are grouped in a new Open Body (unless you uncheck the option). Second parallel curve
Copyright DASSAULT SYSTEMES According to the type of circle you want to create select the circle support, creation points and if needed key in the radius. Creating a Circle (1/4) 3 Define the circle limitations. 2+ Click OK to confirm circle creation. Center Support The support can be a plane or a surface. If it is a non planar surface the circle is projected normally onto the surface.
Copyright DASSAULT SYSTEMES Center and radius Center and point Two points and radius Three points Support Creating a Circle (2/4) You can create a circle on a support (surface or plane) from points and/or a radius value When you create a circle from two points and a radius, you can select one of the solutions proposed clicking the Next solution button. Solution 1 selected Solution 2 selected
Copyright DASSAULT SYSTEMES Creating a Circle (3/4) You can create a circle on a support (surface or plane) giving tangency conditions. Support 1 Bitangent & radius Bitangent & point Tritangent Solution 1 selected Solution 2 selected When you create a circle with tangency conditions, you can select one of the solutions proposed clicking the Next solution button. You can now select a point (not only a curve) to which the circle is to be tangent.
Copyright DASSAULT SYSTEMES Creating a Circle (4/4) You can either create a complete circle or a circular arc according to the selected limitation option. Circular arc which limits are defined by start and end angle values Complete circle Circular arc trimmed using two points or tangency points Complementary circular arc trimmed using two points or tangency points If several solutions are available you can either select one or click on the Next solution button.
Copyright DASSAULT SYSTEMES Select the two elements of the corner and the support (plane or surface on which the elements must lie), then enter the radius. Creating a Corner Click OK to confirm corner creation. 3 Element 1 You can choose to activate the Trim elements option to remove the portions of curve opposite to the corner. Click on this button to display the various solutions before choosing one of them. Element 2 Support Four available solutions Solution 2 selected Original elements trimmed First element of the corner can be a curve, a line or a point, second element must be a curve or a line. When two lines are selected you do not need to select a support.
Copyright DASSAULT SYSTEMES Select the first curve to connect and a point on this curve. Creating a Connect Curve (1/3) 4 If needed click on the red arrow located on either point to reverse the orientation of the associated curve. Curve 1 3 Select the second curve to connect and a point on this curve. Point 1 Point 2 Curve 2 Curve orientation
Copyright DASSAULT SYSTEMES Define the type of continuity between each curve and the connect curve. The type of continuity can be different for each curve. Creating a Connect Curve (2/3) 6 Define the tension of the connect curve at each point. You can key in the tension value or use the graphic manipulators. 7 You can select the Trim elements option to trim the two construction curves and join them to the connect curve. Click OK to confirm connect curve creation. 8
Copyright DASSAULT SYSTEMES Creating a Connect Curve (3/3) You will find below various combinations of continuity between the two curves and the connect curve. Curve 1 : Tangency Curve 2 : Tangency Curve 1 : Tangency Curve 2 : Point Curve 1 : Tangency Curve 2 : Curvature Curve 1 : Point Curve 2 : Point Curve 1 : Point Curve 2 : Curvature Curve 1 : Curvature Curve 2 : Curvature
Copyright DASSAULT SYSTEMES Creating a Conic (1/2) Choose the needed parameters. Click OK to confirm conic creation. 3 Support on which the conic will lie Start and end points of the conic Tangents associated with the start and end points of the conic and with the point located at the intersection of the tangents Parameter : - P=0.5 for parabola - P 0.5 for hyperbola Tangents associated with the two first passing points Point defining the tangents from the start and end points of the conic Intermediate passing points of the conic
Copyright DASSAULT SYSTEMES Creating a Conic (2/2) You can define a conic from various sets of data : Two points, two tangents and a parameter Two points, two tangents and a passing point Two points, a tangent intersection point and a parameter Two points, a tangent intersection point and a passing point Four points and a tangent Five points Start point End point Tangents Support Start point End point Tangents Passing point Support Start point End point Tangent intersection point Parameter : 0.7 Support Start point End point Support Passing points Tangent on point Start point End point Tangent intersection point Support Passing point 1 Start point End point Support Passing points 1 2 3
Copyright DASSAULT SYSTEMES Select the points through which the Spline will pass. Click OK to confirm Spline creation. Creating a Spline Curve (1/2) You can add, remove or replace a point during or after Spline definition. See on next screen the use of the Add Parameters button.
Copyright DASSAULT SYSTEMES Creating a Spline Curve (2/2) When you click on the Add Parameters button you display additional options in the Spline Definition box. 1- Select the point on which you want to impose a tangent 2- Click on this arrow to select the tangent type you want : 4- Confirm the new Spline specifications 3a- Explicit type : select a line or an axis to define the tangency. 3b- From curve type : select a curve containing the selected point to define the tangency.
Copyright DASSAULT SYSTEMES A helix can be reused as guide curve or spine in a Sweep operation. Creating a Helix (1/3) Starting Point Axis 1 2 Select the starting point and the axis of the helix.
Copyright DASSAULT SYSTEMES Creating a Helix (2/3) Choose a Constant law type and enter the pitch value. Define the total height of the helix Height Pitch Define the orientation of the helix. You can define a taper angle which leads the radius variation from one revolution to the other. Outward : the radius increases Inward : the radius decreases Taper angle You can also define a profile that the helix will follow. Profile Define a Starting Angle. Starting Point Starting angle Click OK to confirm helix creation With a Constant law 3a3a 4
Copyright DASSAULT SYSTEMES Creating a Helix (3/3) Click OK to confirm helix creation. Choose a S-type law type : the pitch will evolve according a cubic law. Select a profile that the helix will follow. Starting Point Profile Starting pitch End pitch With a S-type law 3b3b 4
Copyright DASSAULT SYSTEMES Creating a Spiral (1/2) Select the spiral support (plane), center point, reference direction (optional) and start radius. Start radius 1 2
Copyright DASSAULT SYSTEMES Creating a Spiral (2/2) Select the spiral orientation. Select the spiral type. Select the number of revolutions: End angle End radius Pitch You can define the spiral three different ways
Copyright DASSAULT SYSTEMES Click OK to create the Polyline. 1 2 Select already existing points Creating a Polyline 3 You can create a Polyline in one operation.
Copyright DASSAULT SYSTEMES Creating Basic Surfaces You will become familiar with the creation of basic surfaces Creating a Surface from a Profile Creating a Sphere Creating a Swept Surface Creating a Surface from Boundaries Creating a Surface from Another Surface Creating a Lofted Surface
Copyright DASSAULT SYSTEMES You will learn about the various types of surfaces created from a profile Creating a Surface from a Profile Extruded surface Surface of revolution
Copyright DASSAULT SYSTEMES Let s see now how to create those surfaces... Creating a Surface from a Profile… The extruded surface is created from an open or closed profile, giving a direction and limits. A surface of revolution is created from an open or closed profile, giving an axis of revolution and an angle.
Copyright DASSAULT SYSTEMES Select a profile, a direction and enter limits value (or use the graphic manipulators). Click OK to confirm extruded surface creation. Profile Direction can be specified by a line, a plane or components. Creating an Extruded Surface Limits
Copyright DASSAULT SYSTEMES Select a profile, an axis of revolution and key in the angle limits. Axis of revolution Profile Click OK to confirm surface creation. Creating a Surface of Revolution
Copyright DASSAULT SYSTEMES You will learn how to create a complete or partial sphere Creating a Spherical Surface Partial sphere Complete sphere
Copyright DASSAULT SYSTEMES Creating a Sphere Select the sphere center point and key in the sphere radius. Choose to create a complete sphere or a partial sphere. Complete Sphere Partial Sphere You can modify the partial sphere parameters in the Sphere Surface dialog box or dragging and dropping the arrows on geometry
Copyright DASSAULT SYSTEMES You will learn how to create an explicit-type swept surface Creating a Swept Surface
Copyright DASSAULT SYSTEMES Let s see now how to create those surfaces... Creating a Swept Surface… A swept surface is created from an open or closed profile, giving a guide curve and a reference surface or two guide curves.
Copyright DASSAULT SYSTEMES Confirm swept surface creation. Creating an Explicit-type Swept Surface (1/4) Select the guide curve and the profile. You can then choose to give a reference plane or surface (Reference tab) or to select another guide curve and if needed anchor points (Second Guide tab). Reference plane Guide curve Profile Guide curve 1 Guide curve 2 Profile If no spine is selected the guide curve is used as spine. Anchor point 2 Anchor point 1
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (2/4) You can define a reference surface and an angle (in the Position profile mode only ) controlling the position of the profile during the sweep. Reference plane Guide curve Profile The sweep surface is positioned with respect to the guide curve ; the profile is oriented with respect to the reference surface at a given angle. When the profile position is fixed with respect to the guide curve the sweep lies on the profile and on the guide curve (if it intersects the profile) or on the parallel to the guide curve crossing the profile (minimum distance). Green axis-system : current profile orientation Grey axis-system : profile reference axis If you modify the angle the sweep surface rotates around the guide curve with respect to the reference surface. Reference surface In the Position profile mode the reference is no more the profile but the guide curve.
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (3/4) Reference surface In the Position profile mode you can display parameters to modify the position of the sweep profile on the guide curve defining a new origin and a rotation angle or direction. These coordinates (or the selected point) define the position of the origin of the positioning axis system (green) in the first sweep plane. You can rotate the positioning axis system around the guide curve with respect to initial axis system of the profile. You may want to invert the orientation of the X or Y axes of the positioning axis system. You can select a point defining the origin of the axis system linked to the profile. The direction defines the X axis of the positioning axis system. Initial axis system of the profile Positioning axis system
Copyright DASSAULT SYSTEMES Guide curve 1 Guide curve 2 Profile Anchor point 2 Anchor point 1 Creating an Explicit-type Swept Surface (4/4) You can select a second guide curve to define the sweep. You may also select an anchor point for each guide curve. The anchor points lie on the guide curves from the beginning to the end of the sweep. Second guide If the sweep profile is positioned its length is not modified. If you work in the Position profile mode the end points of the profile are positioned on the guide curves. Guide curve 1 Guide curve 2 Profile If you check the Profile extremities inverted option, the profile extremities connected to the guides are inverted. If you check the Vertical orientation inverted option, the vertical orientation of the profile is inverted.
Copyright DASSAULT SYSTEMES You will learn how to create an offset surface Creating a Surface from Another Surface Single Repeat
Copyright DASSAULT SYSTEMES Let s see now how to create those surfaces... Creating a Surface from Another Surface… You can create several offset surfaces at the same time. The offset surface is created from an existing surface, giving an offset value and a direction. The resulting surface is parallel to the initial one.
Copyright DASSAULT SYSTEMES Creating an Offset Surface (1/3) 2 Select the reference surface and key in the offset value. Click OK to continue. The created offset surface is defined as an Object, i.e. the reference for creating the other surfaces. If you want to create several surfaces separated by the same offset check the option Repeat object after OK. 3 4 Object surface Reference surface
Copyright DASSAULT SYSTEMES Creating an Offset Surface (2/3) 5 Define the number of offset surfaces to be created. 6 Click OK to confirm surface creation. As many offset surfaces as indicated in the Object Repetition dialog box are created, in addition to the object surface. The surfaces are separated from the object surface by a multiple of the offset value. Object surface Surface instances in Open Body The surface instances are grouped in a new Open Body (unless you uncheck the option).
Copyright DASSAULT SYSTEMES Creating an Offset Surface (3/3) The resulting offset surface is parallel to the reference surface. Offset value between two surfaces : 20mm Side view
Copyright DASSAULT SYSTEMES You will learn about the types of surfaces created from boundaries Creating a Surface from Boundaries Fill surface Blend surface
Copyright DASSAULT SYSTEMES Let s see now how to create those surfaces... Creating a Surface from Boundaries… The blend surface is created between two curves lying each on a support ; the evolution of the surface between the two curves is defined by parameters. The fill surface is created between joined curves which may lie on a support ; the evolution of the surface inside the contour is defined by parameters.
Copyright DASSAULT SYSTEMES Creating a Fill Surface (1/2) Select the boundaries of the fill surface and, if needed, the support(s) associated with one or more boundary(ies). B 1 B 3 B 4 Support for B1 B 2 Support for B3 The result of the selections must be a closed boundary. During or after creation you can edit a fill surface, adding, replacing or removing a boundary or a support. The type of continuity between the support surface(s) and the fill surface can be chosen from the Continuity combo.
Copyright DASSAULT SYSTEMES Creating a Fill Surface (2/2) If you do not select any support or passing point the fill surface is simply created between the boundaries. Tangency continuity Point continuity 4 Confirm fill surface creation. 3 You can also define a point through which the surface will pass. The result depends on the selected type of continuity (Tangent or Point) between the support surfaces and the fill surface.
Copyright DASSAULT SYSTEMES Creating a Blend Surface (1/7) Select the two curves between which you will create the blend surface and, if needed, the support associated with each curve.
Copyright DASSAULT SYSTEMES Creating a Blend Surface (2/7) 3 If you have selected one or more support surface(s) define the type of continuity (Tangency, Curvature or Point) between each support surface and the blend surface. Tangency continuity Point continuity Curvature continuity You can use the combo to define a different type of continuity on each side of the blend surface. You can choose to trim the support to expand the blend surface up to the limits of the support.
Copyright DASSAULT SYSTEMES Creating a Blend Surface (3/7) 4 If you have selected one or more support surface(s) you can choose to make the borders of the blend surface tangent to the borders of the supports. For each border of the blend surface you can choose the extremity(ies) that will be tangent to the corresponding border of the support. First tangent border : None Second tangent border : None First support Second support First tangent border : Both extremities Second tangent border : Both extremities 1 st border, start First border Second border First tangent border : Start extremity Second tangent border : End extremity 2nd border, end
Copyright DASSAULT SYSTEMES Creating a Blend Surface (4/7) 5 Select the Tension tab to define the tension at the limits of the blend surface. Default tension Constant tension of 2.5 Linear tension from 1 to 2.5 You can keep the default tension or define a constant or linear tension at each limit of the blend surface.
Copyright DASSAULT SYSTEMES Creating a Blend Surface (5/7) Closing points You can define the orientation of the blend surface clicking the arrows located on the selected closing points to invert them. 6 In the case of a closed curve you can select the Closing Points tab and choose the closing point of each curve.
Copyright DASSAULT SYSTEMES Creating a Blend Surface (6/7) 7a7a According to the chosen options you will compute the blend surface : - using the total length of the sections (Ratio), - between the tangency discontinuity points of the curves (Tangency), - between the tangency discontinuity points of the curves then between the curvature discontinuity points of the curves (Tangency then curvature) - between the vertices of the curves (Vertices). Select the Coupling tab to define the type of coupling : - automatic with four options: Ratio, Tangency, Tangency then curvature or Vertices
Copyright DASSAULT SYSTEMES Creating a Blend Surface (7/7) 7b7b Select the Coupling tab to define the type of coupling : - manual coupling with definition of the coupling curve(s) Automatic coupling You can define several coupling curves. Coupling curvesManual coupling 8 Click OK to confirm blend surface creation.
Copyright DASSAULT SYSTEMES You will learn how to create lofted surfaces Creating a Lofted Surface
Copyright DASSAULT SYSTEMES Let s see now how to create lofted surfaces... Creating a Lofted Surface Several parameters can be set to define a lofted surface : Tangency Guide curve Closing point Spine Coupling Limitation Manual coupling
Copyright DASSAULT SYSTEMES For the start and end sections of the loft you can define a surface (containing the corresponding section curve) to which the lofted surface will be tangent. Section 4 Creating a Lofted Surface – Tangent Option Section 1 Section 4 The loft is tangent to the two extruded surfaces. Section 1 Extrude 1 Extrude 2 No tangency condition is imposed between the loft and the two extruded surfaces.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface - Closing Points (1/5) When you create a loft from closed sections a closing point can be defined for each section. The closing points are linked to each other to define the loft orientation. You can also change the closing point of one or more section(s) to modify the loft orientation. Vertex No closing point defined Closing point defined on each section The default orientation of the section is kept : the resulting loft is twisted. The closing points are linked to each other.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface - Closing Points (2/5) To create the lofted surface you will select and orient the sections then define the closing point for each of them. To define a closing point on a section, select the section then click on the adequate point. The point is mentioned in the Closing Point list in front of the corresponding section.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface - Closing Points (3/5) Adding a closing point to a section 1 Click on the section label using MB3 and select the Create Closing Point option. Check the displayed closing point. 2 Reference closing point Closing point to be created
Copyright DASSAULT SYSTEMES Creating a Lofted Surface - Closing Points (4/5) Adding a closing point to a section Define the parameters of the closing point. 3 Click OK to confirm point creation. 4
Copyright DASSAULT SYSTEMES Creating a Lofted Surface - Closing Points (5/5) Changing a closing point on a section 1 Select the sections. Click on the section label and select the closing point you want to define for this section. 2 For each section the starting point of the arrow defines the default closing point. If needed select the arrow to modify the orientation of the section. 3
Copyright DASSAULT SYSTEMES Guide curve 1 With Two Guide CurvesWithout Guide Curve Creating a Lofted Surface – Guide Curve To define the evolution of the lofted surface between two consecutive sections you can select one or more guide curve(s). The guide curve(s) must intersect all the sections of the loft. Section 1 Section 2 You can define a surface tangent to each guide curve and to which the lofted surface will also be tangent. Section 3 Guide curve 2
Copyright DASSAULT SYSTEMES Section 2 Spine With a User-Defined Spine With a Computed Spine Creating a Lofted Surface – Spine The spine guides the section orientation. You can either keep the default spine (automatically computed) or choose a user-defined spine selecting a line or a curve. Section 1 Section 3
Copyright DASSAULT SYSTEMES Creating a Lofted Surface - Coupling (1/6) The coupling tab in the loft function is used to compute the loft using the total length of the sections (ratio), between the vertices of the sections, between the curvature discontinuity points of the sections or between the tangency discontinuity points of the sections. Vertices, Curvature Discontinuity, Tangency Discontinuity Vertices, Curvature Discontinuity Vertex Ratio option Curvature discontinuities option
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Coupling (2/6) 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 discontinuities, we have sketched a profile as shown below : What types of points can CATIA 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 Creating a Lofted Surface – Coupling (3/6) Ratio-type coupling : to compute the loft using the total length of the sections The surface crosses the sections and the variation between the sections is computed by a ratio corresponding to the length of each section.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Coupling (4/6) The surface crosses the sections and each section is split at each tangency discontinuity point. The surface is computed between each split section. Tangency-type coupling : to compute the loft between the tangency discontinuity points of the sections
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Coupling (5/6) The surface crosses the sections and each section is split at each curvature discontinuity point. The surface is computed between each split section. Tangency then Curvature-type coupling : to compute the loft between the curvature discontinuity points of the sections
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Coupling (6/6) Vertices-type coupling : to compute the loft between the vertices of the sections The surface crosses the sections and each section is split at each vertex. The surface is computed between each split section.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Manual Coupling (1/4) When the sections of the lofted surface do not have the same number of vertices you need to define a manual coupling. 1 2 Define the sections and guide curves if needed. Select the Coupling tab from the Lofted Surface Definition window. 3 Double-click in the blue Coupling field to display the Coupling window.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Manual Coupling (2/4) 4 5 For each section select the vertex to be taken into account in the coupling then click OK to end coupling definition. You can visualize the coupling curve if the corresponding option is checked. 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. 6 Click OK to end lofted surface definition. At any time you can edit a coupling by double-clicking on the coupling name in the list and changing the coupling points using the contextual menu.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Manual Coupling (3/4) One coupling curve (1)One coupling curve (2)Two coupling curves You will find below various cases of manual coupling with one or more coupling curves.
Copyright DASSAULT SYSTEMES Creating a Lofted Surface – Manual Coupling (4/4) For each coupling mode, the points that could not be coupled are displayed in the geometry with a specific symbol. On this loft the sections do not have the same number of vertices and have some discontinuities in curvature and tangency. Tangency Mode : Uncoupled tangency discontinuity points are represented by a square. Tangency then 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 Guides Start section End section Spine Creating a Lofted Surface – Limitation If the spine is an automatically computed spine and guides are selected the loft is limited by the guide extremities. By default the lofted surface is limited by the start and end sections. However you can choose to limit it only on one of the sections, on the spine or on the guide extremities. Guides If the spine is an automatically computed spine and no guide is selected the loft is limited to the start and end sections. When the limitation options are checked, the loft is limited to the start and/or end sections. If the spine is a user spine the loft is limited by the spine extremities. When the limitation options are unchecked, the loft is swept along the spine. Start section End section Start section End section Guides Start section End section Start section End section
Copyright DASSAULT SYSTEMES Performing Operations on the Geometry You will learn how to perform operations on the geometry Joining Elements Healing Elements Restoring Elements Disassembling Elements Splitting Elements Trimming Elements Extracting Elements Transforming Elements Extrapolating Elements Creating Near Elements Creating Patterns
Copyright DASSAULT SYSTEMES You will learn how to join wireframe or surface elements Joining Elements Element 1 Element 2Join result
Copyright DASSAULT SYSTEMES What about joined elements ? You can create joined elements from: - adjacent curves - adjacent surfaces You can join elements to use two or more elements as a single element in a further operation. Why Do You Need Joining Elements ? Four adjacent surfaces. Join result Two adjacent splines.
Copyright DASSAULT SYSTEMES Let s see now the way to join elements... Joining Elements… The original surfaces are transferred to the Hide space. You will select one by one these four adjacent surfaces to join them together. The four adjacent surfaces are joined into one single surface identified as Join element in the specification tree.
Copyright DASSAULT SYSTEMES Select one by one the elements to be joined together. Element 1 Joining Elements (1/2) 3 Click OK to confirm join operation. Element 2 To modify the join definition you can edit it and remove elements or replace an element by another. This option checks the connexity between the elements in the resulting join. CATIA will: - reduce the number of resulting elements - ignore the elements that do not allow the join to be created. You can define a merging distance, i.e. the maximum distance below which two elements are considered as only one element.
Copyright DASSAULT SYSTEMES Joining Elements (2/2) While joining elements you can exclude some sub-element from the joined surface. Face to be removed You can also select sub- elements to exclude from the joined surfaces. You can create another join surface with the excluded sub-elements.
Copyright DASSAULT SYSTEMES Healing Elements You will learn how to fill gaps between surfaces Gap Surface 1 Surface 2 Healing result
Copyright DASSAULT SYSTEMES Select the surfaces to be healed. You can also select a Join that needs to be healed. Healing Elements (1/2) Sweep.1 Sweep.2 Gap Define the Merging distance. The merging distance is the maximum distance between the surfaces below which the gap will be filled.
Copyright DASSAULT SYSTEMES Click OK to confirm the healing operation. Healing Elements (2/2) 5 4 Define the Distance objective. The distance objective is the threshold below which the gap will be ignored by the heal operation.
Copyright DASSAULT SYSTEMES Restoring Elements You will learn how to restore the limits of surfaces or curves which have been split before Split surface Cutting elements Restored surface
Copyright DASSAULT SYSTEMES Select the surface which limits will be restored. The Untrim window displays the number of selected elements and the number of resulting elements. Restoring a Surface Click OK to restore the surface. Initial surface First split Second split You can rebuild the limits of a surface which has been split one or several time(s). The surface limits will be restored from the second split. Second split The resulting surface is a datum feature : it cannot be modified. You can also restore the limits of a curve which was split before.
Copyright DASSAULT SYSTEMES Disassembling Elements You will learn how to disassemble multi-cell surfaces or curves into mono-cell elements One multi-cell extruded surface Thee mono- cell surfaces
Copyright DASSAULT SYSTEMES Select the element to be disassembled. The Disassemble window displays the number of selected elements and the number of resulting elements. Disassembling a Surface Click OK to disassemble the surface. Extruded surface The resulting surfaces are datum features : they cannot be modified. You can also disassemble a multi-cell curve.
Copyright DASSAULT SYSTEMES You will learn how to split a wireframe or surface element using one or more cutting elements Splitting Elements Cutting elements Element to be cut Split result
Copyright DASSAULT SYSTEMES What about splitting elements ? You can split : - a wireframe element by points, other wireframe elements or surfaces - a surface by wireframe elements or other surfaces. You can split an element when you need only part of this element in your model. You need the element to be cut and one or more cutting element(s). Why Do You Need Splitting Elements ? Element to cut Cutting element Split result Wireframe elements Surface elements Cutting elements Element to be cut Split result
Copyright DASSAULT SYSTEMES Let s see now how to split elements... Splitting Elements… You should make your selection by clicking on the portion that you want to keep after the split. You can also select the portion to be kept by clicking the Other side button. Cutting element Element to be cut The result is a Split type element.
Copyright DASSAULT SYSTEMES Splitting Elements (1/3) 1 Select the element to cut. 2 Element to cut Cutting elements Select the cutting element(s). You can split an element with several cutting elements at the same time. 3 If you select only one cutting element you can check this option to keep the two sides of the element to cut. In that case two split features are created. You can create the intersection between the cut element and the the cutting elements.
Copyright DASSAULT SYSTEMES Splitting Elements (2/3) For each selected cutting element check the side to be kept on the element to cut ; if you want to change it select the cutting element in the list and click on the Other side button. 4 The cutting elements and their orientation are defined. Click OK to confirm the split operation. 5 The initial cut element is transferred to the hide space.
Copyright DASSAULT SYSTEMES If the cutting element is a closed curve you may need to define more precisely the side of the cutted element you want to keep. Splitting Elements (3/3) Support Vn VtV Principle: - Vn : Vector normal to support - Vt : Vector tangent to cutting element - V=Vn*Vt (Vectorial product); indicates the side of the cutted element to keep Split result without support Split result with a support Support Cutting element Element to split
Copyright DASSAULT SYSTEMES You will learn how to trim a wireframe or surface element Trimming Elements Element 1 Element 2 Trim result
Copyright DASSAULT SYSTEMES What about trimming elements ? You can trim : - two wireframe elements, - two surfaces. You can trim elements between each other to only keep part of them in your model. You need two intersecting elements. Why Do You Need Trimming Elements ? Trim result Wireframe elements Surface elements
Copyright DASSAULT SYSTEMES Let s see now how to trim elements... Trimming Elements… You should make your selection by clicking on the portions that you want to keep after the trim. You can also select the portions to be kept by clicking the Other side button for each element. The result is a Trim type element.
Copyright DASSAULT SYSTEMES Select the elements to trim, clicking on the portions that you want to keep after the operation. Element 1 Element 2 Trimming Elements (1/2) 3 Click OK to confirm trim operation. The initial trimmed elements are transferred to the hide space. Click on one of these buttons to change the side to be kept for each element.
Copyright DASSAULT SYSTEMES Trimming Elements (2/2) While trimming closed wires, you may need to define more precisely the side of the elements you want to keep. Principle: The side of the trimmed elements to keep is given by the vectorial product between : - The vector tangent to the elements to trim. - The vector normal to the support. Using a support Using no support Elements to trim lying on the support
Copyright DASSAULT SYSTEMES You will learn how to create the boundaries of a surface and extract edges or faces from surfaces. Creating Elements from Surfaces Boundary with limits Edge extraction Face extraction
Copyright DASSAULT SYSTEMES Choose the propagation type and select the surface edge from which you want to create a boundary curve. You may also want to define limits to the created boundary curve. Creating the Boundaries of a Surface (1/2) 3 Click OK to confirm boundary creation. See next screen to display the various propagation types. Limit points Selected Edge You can create the external or internal boundaries of a surface, with or without limits.
Copyright DASSAULT SYSTEMES Creating the Boundaries of a Surface (2/2) You will select a propagation type to create exactly the necessary portion of curve. 1. Complete boundary 2. Point continuity 3. Tangent continuity 4. No propagation
Copyright DASSAULT SYSTEMES Select a surface edge and choose the propagation type. Click OK to confirm edge extraction. Extracting an Edge from a Surface Selected edge According to the selected propagation type you get : 1- No propagation3- Point continuity2- Tangent continuity Here there is an ambiguity about the propagation side you are prompted to select a support face. In this case, the dialog box dynamically updates and the Support field is added. You can extract one or several edges of a surface which can be either boundaries or limiting edges of faces. You cannot define limit points. Selected support face
Copyright DASSAULT SYSTEMES Select a face and choose the propagation type. Click OK to confirm face extraction. Extracting a Face from a Surface The initial and the extracted faces are superimposed. Selected face According to the selected propagation type you get : 1- No propagation2- Point continuity3- Tangent continuity You can extract one or several faces of a surface with or without propagation.
Copyright DASSAULT SYSTEMES Transforming Elements Translation Rotation Symmetry Scaling Affinity Axis-to-Axis Transformation You will learn the various transformations you can apply to elements :
Copyright DASSAULT SYSTEMES What about transformations ? Six transformation types are available: Transformations are used to modify the size, location, orientation, etc. of a wireframe or a surface element. Why Do You Need Transformations ? Translation Rotation Symmetry Scaling Affinity Axis-to-Axis
Copyright DASSAULT SYSTEMES For each type of transformation a dialog box is displayed. 1 Click on any Transformation icon. 2 The dialog box contents changes according to the selected type of transformation. Let s see now the different ways to apply transformations... 3 Enter transformation specifications in the dialog box and confirm. Applying Transformations…
Copyright DASSAULT SYSTEMES Translating an Element (1/2) 2 Select the element to be translated and define the translation direction or components and the distance. Click OK to continue. The created translated element is defined as an Object, i.e. the reference for creating the other translated elements. If you want to create several translated elements check the option Repeat object after OK. 3 4 Object element Transformed element You can click this button to hide or show the initial element.
Copyright DASSAULT SYSTEMES Define the number of translated elements to be created. 6 Click OK to confirm element creation. As many translated elements as indicated in the Object Repetition dialog box are created, in addition to the object element. The translated elements are separated from the object element by a multiple of the distance. Object element Element instances in Open Body Translating an Element (2/2) The element instances are grouped in a new Open Body (unless you uncheck the option).
Copyright DASSAULT SYSTEMES Rotating an Element (1/2) 2 Select the element to be rotated and define the rotation axis and the angle. Click OK to continue. The created rotated element is defined as an Object, i.e. the reference for creating the other rotated elements. 3 4 Object element Initial element You can click this button to hide or show the initial element. If you want to create several rotated elements check the option Repeat object after OK.
Copyright DASSAULT SYSTEMES Define the number of rotated elements to be created. 6 Click OK to confirm element creation. As many rotated elements as indicated in the Object Repetition dialog box are created, in addition to the object element. The rotated elements are separated from the object element by a multiple of the angle value. Object element Element instances in Open Body Rotating an Element (2/2) The element instances are grouped in a new Open Body (unless you uncheck the option).
Copyright DASSAULT SYSTEMES Transformed element Symmetry along plane Symmetry by point Applying a Symmetry to an Element 1 2 Select the element and a point, line or plane as reference. 3 Click OK to confirm symmetry creation. Reference point Reference plane You can click this button to hide or show the initial element.
Copyright DASSAULT SYSTEMES Scaling an Element (1/2) 2 Select the element to be scaled and define the reference and the ratio. Click OK to continue. The created scaled element is defined as an Object, i.e. the reference for creating the other scaled elements. 3 4 Object element Initial element You can click this button to hide or show the initial element. If you want to create several scaled elements check the option Repeat object after OK. Initial element
Copyright DASSAULT SYSTEMES Define the number of scaled elements to be created. 6 Click OK to confirm element creation. As many scaled elements as indicated in the Object Repetition dialog box are created, in addition to the object element. The scaled elements are separated from the object element by a multiple of the ratio value. Object element Element instances in Open Body Scaling an Element (2/2) The element instances are grouped in a new Open Body (unless you uncheck the option).
Copyright DASSAULT SYSTEMES Select the element, define the reference axis-system and key in a ratio for each direction. Click OK to confirm affinity creation. Initial element Point 1 origin of reference axis-system Creating an Affinity Affinity You can click this button to hide or show the initial element.
Copyright DASSAULT SYSTEMES Click OK to create the transformed surface. 1 2 Select the element to transform. Applying an Axis-to-Axis transformation 3 Select the reference Axis System. 4 Select the target Axis System. 5
Copyright DASSAULT SYSTEMES Extrapolating Elements You will learn how to create extrapolated curves and surfaces. Curve extrapolation Surface extrapolation
Copyright DASSAULT SYSTEMES What about extrapolating elements ? You can extrapolate : - any type of curve or line, - any type of surface. Two extrapolation modes are available: - giving a length, - giving a limit (up to…). Why Do You Need Extrapolating Elements ? Curve elements Surface elements You may have to extrapolate a curve or surface to extend it to other geometry and thus be able to later trim, split or intersect these elements.
Copyright DASSAULT SYSTEMES Let s see now the way to extrapolate elements... Extrapolating Elements… Finally you will define the type of continuity and transition. First select the element boundary which will be extrapolated, then the element itself. You will then choose the extrapolation mode : length or limit.
Copyright DASSAULT SYSTEMES Extrapolating Elements (1/3) 2 Select the edge representing the boundary you want to extrapolate. For a curve the boundary is one of the curve extremities. Surface boundary 3 Select the surface to be extrapolated. For a curve select the curve itself. A temporary extrapolated surface is displayed. The default extrapolation mode is Length. Temporary extrapolated surface
Copyright DASSAULT SYSTEMES Extrapolating Elements (2/3) 4 Choose the extrapolation mode. - Length : key in the length of the extrapolated surface or curve, - Up to element : define the limit surface or plane. 5 6 Choose the type of continuity (for a curve) and the type of transition (for a curve or a surface). Refer to table on next page. Check the Assemble result option if you want the extrapolated surface to be assembled to the support surface. 7 Click OK to create the extrapolated surface.
Copyright DASSAULT SYSTEMES Extrapolating Elements (3/3) Extrapolation mode Options LengthUp to Element Extrapolating a curve Continuity Tangent: the extrapolation is tangent to the selected curve. Curvature: the extrapolation keeps the curvature of the selected curve. N/A Extrapolating a surface Continuity Tangent: the extrapolation is tangent to the selected surface. Curvature: the extrapolation keeps the curvature of the selected surface. N/A Extremities Only if tangent continuity: Tangent: the extrapolation is tangent to the edges adjacent to the surface boundary. Normal: the extrapolation is normal to the original surface boundary. Tangent: the extrapolation is tangent to the edges adjacent to the surface boundary. Normal: the extrapolation is normal to the original surface boundary.
Copyright DASSAULT SYSTEMES You will learn how to create a near element from a multi-entity element Creating Near Elements Entity 1 of extruded surface Entity 2 of extruded surface Near element created from entity 2 of extruded surface
Copyright DASSAULT SYSTEMES What about near elements ? You can create near elements from: - sketches - surfaces Why Do You Need Near Elements ? Near element created for one entity of the surface. Near element created for one entity of the sketch. Some construction elements are made up of several entities. You may need to use only part of a multi-entity element.
Copyright DASSAULT SYSTEMES Let s see now the way to create Near elements... Creating Near Elements… The original element is transferred to the Hide space. You will select the multiple element from which you want to create the Near element. You will then select a reference element, i.e. a point located next to the entity to be defined as Near element.
Copyright DASSAULT SYSTEMES Select an element composed of two disconnected entities. Creating a Near Element (1/3) This operation allows you to quickly extract a sub-element from multi-element geometry. Access the Near operation from the menu bar 3 Select a point located next to the entity you want to define as Near element. Select point 4 Click OK to create the Near element. The initial element is transferred into the Hide space.
Copyright DASSAULT SYSTEMES Creating a Near Element (2/3) When you use an element composed of disconnected entities as construction elements, you can either keep all the entities or choose one of them. 1 2 Select an element composed of two disconnected entities to define the profile to extrude. 3 Click OK to create the extruded surface : the Multi-Result Management window is displayed
Copyright DASSAULT SYSTEMES Creating a Near Element (3/3) 4.1 If you click No the extruded surface is created from the two entities of the element. 4.2 If you click Yes you have to choose the entity on which you want to create the extruded surface; the portion of extruded surface created from this entity will be defined as a Near element. Select point 5 Click OK to create the extruded surface and the Near element. The initial extruded surface is transferred into the No Show.
Copyright DASSAULT SYSTEMES Creating Patterns You will learn how to replicate geometry using rectangular or circular patterns. Rectangular pattern Circular pattern
Copyright DASSAULT SYSTEMES Creating a Rectangular Pattern (1/2) 1 Select the object to pattern. 2 Object to pattern For each direction define the parameters : - instance(s) : number of patterns in the current direction - spacing : distance between two patterns in the current direction - length : total length of the pattern in the current direction 3 Three parameter combinations are available : - Instance(s) and Length - Instance(s) and Spacing - Spacing and Length
Copyright DASSAULT SYSTEMES Creating a Rectangular Pattern (2/2) Select the plane on which the pattern will lie : the temporary pattern is displayed. 4 To define a direction you may select a line, a planar face or surface edge. If needed you can modify the position of the object to pattern and/or rotate the pattern ; click the More>> button to access the options. 5 First direction Second direction New object position Click OK to create the rectangular pattern. 6
Copyright DASSAULT SYSTEMES Creating a Circular Pattern (1/3) 1 Select the object to pattern. 2 Define the parameters of the circular pattern : - instance(s) : number of patterns - angular spacing : angle between two patterns - length : total angle of the pattern 3 Four parameter combinations are available : - Instance(s) and total angle - Instance(s) and angular spacing - Angular spacing and total angle - Complete crown Object to pattern
Copyright DASSAULT SYSTEMES Creating a Circular Pattern (2/3) Define the parameters of the crown : - circle(s) : number of circles - circle spacing : distance between two circles - crown thickness : distance between the object to pattern and the outer circle 4 Three parameter combinations are available : - Circle(s) and crown thickness - Circle(s) and circle spacing - Circle spacing and crown thickness You will modify the Crown Definition parameters only if you need to create several instances of the crown, as shown on the opposite example. In the present case you will create one single crown. Crown 1 Crown 2 Crown 3 Object to pattern
Copyright DASSAULT SYSTEMES Creating a Circular Pattern (3/3) Select the element which will define the rotation axis of the pattern : the temporary pattern is displayed. 5 To define the rotation axis you may select a face, a line, an edge, a plane or a point. If needed you can modify the position of the object to pattern, rotate the pattern and/or modify the rotation of the instances; click the More>> button to access the options. 5 Click OK to create the circular pattern. 6 This option allows you to define whether the rotation of the instances will be radial or they keep the same orientation as the object.
Copyright DASSAULT SYSTEMES Creating a Solid from Surfaces Completing the Geometry in Part Design You will learn how to complete the surface geometry in Part Design
Copyright DASSAULT SYSTEMES You will learn how to create a solid from surfaces Creating a Solid from Surfaces
Copyright DASSAULT SYSTEMES What about solids created from surfaces ? You can use a surface to: - split a solid body - create a solid body by thickening the surface - close it into a solid body - sew it onto a solid body You may need to create a surface just for using it in a solid body. The surface is integrated into the body design. Why Do You Need to Create a Solid from Surfaces ? Split Body Thicken Surface Close Surface Sew Surface
Copyright DASSAULT SYSTEMES For each type of feature a dialog box is displayed. 1 Click on any Surface-Based Features icon. 2 Select the surface to be processed. Let s see now the different ways to create surface-based features... 3 Confirm feature creation. Creating a Solid from a Surface …
Copyright DASSAULT SYSTEMES Splitting a Body with a Surface Select the surface used as splitting element and orient the arrow towards the material to be kept. Splitting surface Material to be kept 3 Click OK to split the body.
Copyright DASSAULT SYSTEMES Thickening a Surface Select the surface to be thickened. Surface to be thickened 3 Click OK to thicken the surface. Offset direction
Copyright DASSAULT SYSTEMES Closing a Surface into a Body Select the surface to be closed. Surface to be closed 3 Click OK to close the surface.
Copyright DASSAULT SYSTEMES Sewing a Surface to a Body Select the surface to be sewn onto the body and orient the arrow towards the material to be kept. Surface to be sewn Material to be kept 3 Click OK to sew the surface to the body.
Copyright DASSAULT SYSTEMES Editing Surface and Wireframe Definition Modifying the Geometry You will learn how to modify the geometry after creation
Copyright DASSAULT SYSTEMES You will learn how to edit the definition of wireframe or surface elements Editing Surface and Wireframe Definition Element to edit
Copyright DASSAULT SYSTEMES What about editing elements ? You can edit in the same way: - wireframe elements - surface elements You can edit elements after part creation to change some of the parameters and thus make a new version of the part. Why Do You Need Editing Elements ? Editing the surface parameters. Editing the definition of some points modifies the associated spline.
Copyright DASSAULT SYSTEMES Let s see now the different ways to edit elements... Editing Elements… The surface is updated according to the new parameters. You will modify the axis and the angle of revolution of this surface. You can modify parameters either entering new values or making new selections.
Copyright DASSAULT SYSTEMES Modify the definition of the element by selecting new references or changing values. 3 Confirm element modification. Editing Elements Activate the Definition box of the element: Select the element then choose the xxx.object > Definition command. Double-click on the element or on the element identifier in the specification tree. 2
Copyright DASSAULT SYSTEMES Stacking Commands Manipulating Elements Creating Datum Features Working on a Support Updating a Part Managing Open Bodies Checking Connections Between Elements Using Tools You will become familiar with some tools used for managing wireframe and surfaces.
Copyright DASSAULT SYSTEMES You will learn how to stack commands while creating wireframe elements. 4Stacking Commands
Copyright DASSAULT SYSTEMES What about stacking commands ? You can create the following construction elements: - points,- planes, - intersections. - lines,- projections, You have access to the stacking commands capability while creating: - points,- circles,- translations, - lines,- conics- rotations, - planes, - corners, - symmetry. Why Do You Need to Stack Commands ? Stacking commands allows you to create construction elements while creating an element which requires those construction elements. Using mouse button 3 you display a contextual menu listing all the elements you can create using the stacking commands capability.
Copyright DASSAULT SYSTEMES You define the parameters of the construction element. Let s see now the way to stack commands... Stacking Commands… While creating an element you may need a construction element that you will create on the fly. The construction element is created and selected at the same time. When using the stacking command capability you can check the status of the stack in the Running Commands window.
Copyright DASSAULT SYSTEMES Stacking Commands (1/4) Select the type of plane you want to create. When you create some wireframe elements (point, line, plane, circle, corner, conic) or when you perform a translation, a rotation or a symmetry on an object you can create on the fly the missing construction elements, i.e. points, lines, planes, intersections or projections. In the following example you will see how to create a plane from scratch. 3 Using mouse button 3 click in the Point field and select the Create Point option. The Point Definition window is displayed.
Copyright DASSAULT SYSTEMES Stacking Commands (2/4) 4 Define the parameters to create the point. The status of the stacking commands is also displayed in the Running Commands window. 5 Click OK to accept point creation. The Plane Definition window is displayed again with Point.1 in the Point field. The Point button next to the Point field allows you to edit the point parameters. 6 Using mouse button 3 click in the Line field and select the Create Line option. The Line Definition window is displayed.
Copyright DASSAULT SYSTEMES Stacking Commands (3/4) 7 Define the parameters to create the line. The status of the stacking commands is also displayed in the Running Commands window. 8 To create the points needed for the line you can also use the stacking commands. In that case the Running Commands window will look like this:
Copyright DASSAULT SYSTEMES Stacking Commands (4/4) 9 Once the two points are created click OK to accept the line creation. The Plane Definition window is displayed again with Line.1 in the Line field. The Line button next to the Line field allows you to edit the Line parameters. 10 Click OK to accept the plane creation. If you want to modify a parameter of the plane you can also double-click on its identifier in the specification tree. Point.1 Point.2 Point.3 Line.1 Plane.1
Copyright DASSAULT SYSTEMES You will learn how to cut/copy and paste elements and how to delete one or several elements. Manipulating Elements
Copyright DASSAULT SYSTEMES What about manipulating elements ? Cut : you remove an element and store it in the clipboard ; you can use it afterwards. Copy : you keep the original element and store a copy to the clipboard ; you can use it afterwards. Paste : you take an element from the clipboard and paste it in the specification tree. Delete : you remove an element from the specification tree or the geometry. When you are building a part you may need the same element several times with different parameters ; you may also have to erase some unused elements. Why Do You Need to Cut, Copy, Paste or Delete Elements ? The tools used to cut, copy, paste and delete elements are located either in the Edit menu, in the contextual menu or in the Standard toolbar. You can select the element in the geometry or in the specification tree.
Copyright DASSAULT SYSTEMES Let s see now the ways to manipulate elements... Cutting, Copying, Pasting and Deleting Elements… You will cut or copy one or several elements. Then select the element after which you want to position the cut/copied elements and paste them. or You can also delete an element from the specification tree.
Copyright DASSAULT SYSTEMES Cutting, Copying, Pasting and Deleting Elements (1/3) Select the elements you want to copy, here the circle and its center point. You can select the elements from the geometry or the specification tree. 3 Select the element after which you want to paste the copied elements. Select the Copy icon either in the Standard toolbar or from the contextual menu. or
Copyright DASSAULT SYSTEMES Cutting, Copying, Pasting and Deleting Elements (2/3) 5 Modify the position of the created point on the surface. The point is moved together with the duplicated circle. Select the Paste icon either in the Standard toolbar or from the contextual menu. or The elements are duplicated. You can check the result in the specification tree. However the pasted elements cannot be visualized in the geometry since they are located on the initial elements.
Copyright DASSAULT SYSTEMES Cutting, Copying, Pasting and Deleting Elements (3/3) Now select the initial circle either in the geometry or in the specification tree. 7 Select the Delete option from the contextual menu. 8 If needed check some of the options proposed in the dialog box. Check this option to delete also the geometry used to create the circle only. Check this option to delete also all the elements created from the circle. 9 Click OK to delete the circle.
Copyright DASSAULT SYSTEMES You will learn how to create datum features Creating Datum Features
Copyright DASSAULT SYSTEMES What about datum features ? A datum feature is a non-modifiable element. Even if you change the definition of its parent element(s) the datum feature remains unchanged. Why Do You Need to Create Datum Features ? If you click on the Create Datum icon only the element to be created will be defined as datum feature. If you double-click on the Create Datum icon all the elements will be defined as datum features until you click the icon again to de-activate it. A datum feature is an element which has no link (history) with the elements used to build it (parent elements).
Copyright DASSAULT SYSTEMES Let s see now the way to create datum features... Creating Datum Features… Clicking on the Create Datum icon de-activates the History mode. You will then create the datum feature element… … and finally modify one of its parents.
Copyright DASSAULT SYSTEMES Creating Datum Features (1/2) Define the surface parameters : profile, direction and limits. 4 Click OK to create the surface. 3 Note that the identifier of the extruded surface in the specification tree is not Extrude.1 but Surface.1 and that the datum symbol is visible.
Copyright DASSAULT SYSTEMES Creating Datum Features (2/2) Click OK to accept point modification. 6 The spline passing through this point is modified but the surface created from the spline remains unchanged. Modify one of the points defining the spline.
Copyright DASSAULT SYSTEMES You will learn how to define a planar or non-planar support, work on it with or without a grid and snap to a point. Working on a Support
Copyright DASSAULT SYSTEMES What about support ? If you define a plane as a support a grid is displayed and positioned in the plane of the screen. In that case you have access to the Snap to Point capability. If you define a surface as a support the elements created after selection of the surface will be located on the surface by default. Why Do You Need to Work on a Support ? You can select a plane or a surface to use it as a support for further element creation. Support plane = YZ With the Snap to Point capability the created points are located at the nearest intersection of the grid. Support surface = Extrude.1 When you create a point after selecting the surface as a support the Point Definition window automatically displays the option On surface.
Copyright DASSAULT SYSTEMES Working on a Support – Plane Support (1/3) 1 2 Select the plane you want to define as a support, here the YZ plane. The Work on Support window is displayed. A Working support.1 feature is added to the specification tree under the Working supports entry. By default the last created working support (current) is displayed in red in the specification tree. The not current working supports are displayed in blue.
Copyright DASSAULT SYSTEMES Working on a Support – Plane Support (2/3) The Work on Support window changes and displays several options to define the grid. Define the number of steps in a grid subdivision Selected plane Define the total length of the grid subdivision Check this option if you want a different primary spacing in the second direction Define which axis is taken as H direction in the 2D plane 3 Click OK to confirm grid creation. Set the grid visualization parallel to the screen If you enter coordinates when the Snap to point icon is active, the system does not take the grid into account. 4 If you want your cursor to move directly to an intersection point of the grid click on the Snap to Point icon.
Copyright DASSAULT SYSTEMES Working on a Support – Plane Support (3/3) Here you are creating a point. Note that : - the point type is automatically set to On plane, - the cursor points only on the grid intersection points. Create an element on the support. 5 Exit the working support : 6 Using the Working Supports Activity icon Using the Set as Not Current option in the contextual menu
Copyright DASSAULT SYSTEMES Working on a Support – Surface Support (1/2) 1 2 Select the surface you want to define as a support, here the extruded surface. The Work on Support window is displayed. A Working support.1 feature is added to the specification tree under the Working supports entry. By default the last created working support (current) is displayed in red in the specification tree. The not current working supports are displayed in blue.
Copyright DASSAULT SYSTEMES Working on a Support – Surface Support (2/2) 3 Click OK to confirm grid creation. Here you are creating a point. Note that the point type is automatically set to On surface. Create an element on the support. 4 Exit the working support : 5 Using the Working Supports Activity icon Using the Set as Not Current option in the contextual menu
Copyright DASSAULT SYSTEMES You will learn how to update your part in case you have chosen the manual update mode. Updating a Part Part to be updated
Copyright DASSAULT SYSTEMES What about update ? In the Manual mode you know that the part needs to be updated when: Why Do You Need to Update a Part ? You can choose to work in the Automatic or Manual update mode. If you work in the Automatic mode your part is automatically updated. If you work in the Manual mode you can update your part whenever you want. The part is displayed in bright red. The Update symbol appears next to the part name. The Update icon is available.
Copyright DASSAULT SYSTEMES Let s see now the way to update a part... Updating a Part… The Automatic Update mode is the default mode set in the Options. You can change the default update mode in Tools + Options + Shape. Note that the chosen update mode is the same in Wireframe and Surface Design and in Part Design.
Copyright DASSAULT SYSTEMES Update the part to display the new spline and surface: click on the Update icon in the Tools toolbar select Edit + Update in the menu bar select the Local Update option from the contextual menu positioning the cursor on the Part identifier Updating a Part 1 2 Perform a modification for which an update is required. Set the update mode to Manual as explained before. Initial part Modification of a point 3 If you position the cursor on a feature and select Local update from the contextual menu only the feature is updated. Here the spline and the surface need to be updated. Resulting part
Copyright DASSAULT SYSTEMES You will learn how to insert, select and rename an open body and how to manage the elements belonging to an open body. Managing Open Bodies
Copyright DASSAULT SYSTEMES What about open bodies ? When you enter the Wireframe and Surface Design workbench an open body is automatically created. You can create as many open bodies as you need. Once you make an open body current, all the elements created in the part will belong to this open body. You can move elements within an open body or from an open body to another without modifying the geometry. Why Do You Need Open Bodies ? Open bodies are useful to show clearly the structure of your part. Elements belonging to the Wireframe open body Current open body (underlined) ; you define an open body as current : - clicking on it with mouse button 3 and selecting Define in Work Object, - selecting it in the body selector available in the Tools toolbar.
Copyright DASSAULT SYSTEMES Let s see now the ways to manage open bodies... Managing Open Bodies… You will first insert a new open body… … then rename it in the body selector… … create new elements in the current open body… … and move some of them to the relevant open body.
Copyright DASSAULT SYSTEMES Inserting, Renaming and Selecting an Open Body 1 2 In the Body selector rename Open_Body.4 into Operations. Create a new open body. The new open body is created after the last element of the current open body in the specification tree and is automatically made current. 3 In the Body selector select basic Surfaces as new current open body.
Copyright DASSAULT SYSTEMES Moving an Element to another Open Body In the same way you can move an element to another open body without modifying the geometry. Select the element to be moved using mouse button 3, display its contextual menu then choose the Change Body option in the element object menu. 1 In the specification tree select the open body to which you want to move the selected element. To place the element precisely you can select the element above which you want to move it. 2 The Change Body window is displayed. Click OK to move the element in the specification tree. 3
Copyright DASSAULT SYSTEMES Moving an Element within an Open Body You can move an element to another location within an open body without modifying the geometry. Select the element to be moved using mouse button 3, display its contextual menu then choose the Change Body option in the element object menu. 1 In the specification tree select the element above which you want to locate it, here Sketch.2. 2 The Change Body window is displayed. Click OK to move the element in the specification tree. 3
Copyright DASSAULT SYSTEMES You will learn how to check connections between surfaces or between curves. Checking Connections Between Elements
Copyright DASSAULT SYSTEMES Multi-Select the two surfaces between which you would like to check the connection Checking Connections Between Surfaces (1/2) 3 Select the Connect Checker Icon Choose the Analysis Type : distance, tangency or curvature 4 5 Adjust the color ranges taking account your Minimum and Maximum values Choose the type of Display you require. Note the Minimum and Maximum values between the two surfaces.
Copyright DASSAULT SYSTEMES Checking Connections Between Surfaces (2/2) Click OK to confirm. The Connection Analysis is added to the specification tree 7 The number of selected elements and the number of detected connections are displayed. Select the Quick button to obtain a simplified analysis taking into account tolerances (distance, tangency and curvature). Check the analysis result on the geometry. 6
Copyright DASSAULT SYSTEMES This tool allows you to detect the point, tangency and curvature discontinuities on curves. Checking Connections Between Curves (1/2) Distance analysis Tangency analysis Curvature analysis The point discontinuities are displayed on the analysed curve. The curvature discontinuities are displayed on the analysed curve. The tangency discontinuities are displayed on the analysed curve.
Copyright DASSAULT SYSTEMES Checking Connections Between Curves (2/2) The Quick option allows the user to give thresholds bellow which the discontinuity is not detected. If both tangency and curvature discontinuities are detected, only the tangency discontinuity is displayed. Display of the maximum discontinuity values on the curve.