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The Part Design application makes it possible to design precise 3D mechanical parts with an intuitive and flexible user interface, from sketching in an assembly context to iterative detailed design. Part Design application will enable you to accommodate design requirements for parts of various complexities, from simple to advance. This application, which combines the power of feature-based design with the flexibility of a Boolean approach, offers a highly productive.

1 Opening a New CATPart Document.

This task shows you how to open a new CATPart document. Select the File -> New commands (or

click the New icon). The New dialog box is displayed, allowing you to choose the type of document you need. Select Part in the List of Types field and click OK. The Part Design workbench is loaded and a CATPart document opens. The Part Design workbench document is divided into: a) the specification tree, b) the geometry area, c) specific toolbars, a number of contextual commands available in the specification tree and in the geometry. Remember that these commands can also be accessed from the menu bar.

You will notice that CATIA provides three planes to let you start your design. Actually, designing a part from scratch will first require designing a sketch. Sketching profiles is performed in the Sketcher workbench, which is fully integrated into Part Design. To open it, just click the Sketcher

icon and select the work plane of your choice. The Sketcher workbench then provides a large number of tools allowing you to sketch the profiles you need.

2 Reference Elements

You can display the Reference Elements toolbar using the View -> Tool bars -> Reference Elements (extended/compact) command.

2.1 Creating Points

This task shows the various methods for creating points. Click the Point icon . The Point
Definition dialog box appears. Use the combo to choose the desired point type.

Coordinates: Creating point with X, Y, Z coordinates in the current axis-systemOn curve: Creating point on curve. On plane: Creating point on plane On surface: Creating point on a surface. Circle center: Creating point of a circle, ellipse.Tangent on curve: Creating point tangent to curve. Between: Creating point between two other points.

2 Creating Lines

Click the Line icon . The Line Definition dialog box appears. Use the combo to choose thedesired line type. A line type will be proposed automatically in some cases depending on your first element selection. Point – Point: Create line between the two points. Point – Direction: Create line from a point along a direction. Angle or normal to curve: Create line at an angle to curve. Tangent to curve: Create line tangent to curve. Normal to surface: Create line normal to surface. Bisecting: Create line for bisector of two lines.

Regardless of the line type, Start and End values are specified by entering distance values or by using the graphic manipulators. Check the Mirrored extent option to create a line symmetrically in relation to the selected Start point.

2.3 Creating Planes

This task shows the various methods for creating planes. Click the Plane icon . The Plane Definition dialog box appears. Use the combo to choose the desired Plane type. Once you have defined the plane, it is represented by a red square symbol, which you can move using the graphic manipulator. Offset from plane: Create a plane at a distance from reference plane. Parallel through point: Create a plane passing through a point & parallel to reference plane. Angle or normal to plane: Create a plane at an angle to reference plane. Through three points Through two lines Through point and line Through planar curve Tangent to surface Normal to curve Mean through points Equation

3 Sketch-Based Features

Features are entities you combine to make up your part. The features presented here are obtained by applying commands on initial profiles created in the Sketcher workbench or in the Generative Shape Design workbench. Some operations consist in adding material, others in removing material. In this section, you will learn how to create the following features: Pad, Pocket, Shaft, Groove, Rib, Slot, Loft, and Remove Loft.

3.1 PAD

Creating a pad means extruding a profile or a surface in one or two directions. The application lets you choose the limits of creation as well as the direction of extrusion. Select Sketch as the profile to be extruded. By default, if you extrude a profile, the application extrudes normal to the plane used to create the profile. You will notice that by default, the application specifies the length of your pad. But you can use the following options too: Up to Next ,Up to Last, Up to Plane, Up to Surface. You can increase or decrease length values by dragging LIM1 or LIM2 manipulators.

Reverse direction option lets you choose which side of the profile is to be extruded. Click the Mirrored extent option to extrude the profile in the opposite direction using the same length value. If you wish to define another length for this direction, you do not have to click the Mirrored extent button. Just click the More button and define the second limit.

3.2 Multi-Pad

With this task you can extrude multiple profiles belonging to a same sketch using different length values. The multi-pad capability lets you do this at one time. Select Sketch that contains the profiles to be extruded. Note that all profiles must be closed and must not intersect. The Multi-Pad Definition dialog box appears and the profiles are highlighted in green. For each of them, you can drag associated manipulators to define the extrusion value.

3.3 Pocket

Creating a pocket consists in extruding a profile or a surface and removing the material resulting from the extrusion. The application lets you choose the limits of creation as well as the direction of extrusion. The limits you can use are the same as those available for creating pads. Select the

profile to be extruded. Click the Pocket icon . You can define a specific depth for your pocket or set one of these options: up to next, up to last, up to plane, up to surface.

To define a specific depth, set the Type parameter to Dimension. Alternatively, select LIM1 manipulator and drag it downwards. By default, if you extrude a profile, the application extrudes normal to the plane used to create the profile. To specify another direction, click the more button to display the whole Pocket Definition dialog box, uncheck the Normal to sketch option and select a new creation direction. Optionally click Preview to see the result. Click OK to create the pocket. The specification tree indicates this creation. Double-click Pocket to edit it.

3.4 Multi-Pocket

This task shows you how to create a pocket feature from distinct profiles belonging to a same sketch and this, using different length values. The multi-pocket capability lets you do this at one

time. Click the Multi-Pocket icon . Select Sketch that contains the profiles to be extruded. Note that all profiles must be closed and must not intersect. The Multi-Pocket Definition dialog box appears and the profiles are highlighted in green. For each of them, you can drag associated manipulators to define the extrusion value.

3.3.5 Thin Solids

When creating pads, pockets and stiffeners, you can now add thickness to both sides of their profiles. The resulting features are then called "thin solids". This task shows you how to add

thickness to a pad. The method described here is also valid for pockets. Enter Thickness1 's value, and click Preview to see the result. A thickness has been added to the profile as it is extruded. The profile is previewed in dotted line. Enter Thickness2 's value, and click Preview to see the result. Material has been added to the other side of the profile. To add material equally to both sides of the profile, check "Neutral fiber" and click Preview to see the result. Checking the "Merge Ends" option trims extrusions to existing material.

3.6 Shaft

This task illustrates how to create a shaft that is a revolved feature. You need an open or closed profile, and an axis about which the feature will revolve. Note that you can use wireframe

geometry as your profile and axes. Select the open profile. Click the Shaft icon . The Shaft Definition dialog box is displayed. The application displays the name of the selected sketch in the Selection field from the Profile frame. For the purposes of our scenario, the profile and the axis belong to the same sketch. Consequently, you do not have to select the axis. You can create shafts from sketches including several closed profiles. These profiles must not intersect and they must be on the same side of the axis. If needed, you can change the sketch by clicking the field and by selecting another sketch in the geometry or in the specification tree. But

you can also edit your sketch by clicking the icon that opens the Sketcher. Once you have done your modifications, the Shaft Definition dialog box reappears to let you finish your design. The application previews limits LIM1 that corresponds to the first angle value, and LIM2 that corresponds to the second angle value. The first angle value is by default 360 degrees. Enter the values of your choice in the fields First angle and Second angle. Alternatively, select LIM1 or LIM2 manipulator and drag them onto the value of your choice. Click Preview to see the result. Click OK to confirm. The shaft is created. The specification tree mentions it has been created.

3.7 Groove

Grooves are revolved features that remove material from existing features. This task shows you how to create a groove, that is how to revolve a profile about an axis (or construction line). You

can use wireframe geometry as your profile and axes. Click the Groove icon . Select the profile. The Groove Definition dialog box is displayed. The application displays the name of the selected sketch in the Selection field from the Profile frame. The Selection field in the Axis frame is reserved for the axes you explicitly select. For the purposes of our scenario, the profile and the axis belong to the same sketch. Consequently, you do not have to select the axis. The system previews a groove entirely revolving about the axis. You can create grooves from sketches including several closed profiles. These profiles must not intersect and they must be on the same side of the axis. If needed, you can change the sketch by clicking the Selection field and by selecting another sketch in the geometry or in the specification tree. The application previews the limits LIM1 and LIM2 of the groove to be created. You can select these limits and drag them onto the desired value or enter angle values in the appropriate fields. Click the Reverse Direction button to inverse the revolution direction. Click OK to confirm the operation. CATIA removes material around the cylinder. The specification tree indicates the groove has been created. This is your groove: Click OK to confirm.

3.8 Hole

Creating a hole consists in removing material from a body. Various shapes of standard holes can be created. These holes are:

Simple Tapered Counter Bored Countersunk CounterDrilled

If you wish to use the Up to Plane or Up to Surface option, you can then define an offset between the limit plane (or surface) and the bottom of the hole. By default, the application creates the hole normal to the sketch face. But you can also define a creation direction not normal to the face by unchecking the Normal to surface option and selecting an edge or a line.

3.9 Threaded Holes

The Thread capability removes material surrounding the hole. To define a thread, you can enter the values of your choice, but you can use standard values. You can define three different thread types: No Standard: uses values entered by the user, Metric Thin Pitch: uses AFNOR standard values, Metric Thick Pitch: uses AFNOR standard values. Define the parameters as per your requirement to create threaded hole.

3.10 Rib

This task shows you how to create a rib that is how to sweep a profile along a center curve to create material. To define a rib, you need a center curve, a planar profile and possibly a reference element or a pulling direction. It should be kept in mind that 3D curve if selected as center curves must be continuous in tangency & if the center curve is planar, it can be discontinuous in

tangency. To create Rib, Click the Rib icon . The Rib Definition dialog box is displayed. Select the profile you wish to sweep. Your profile has been designed in a plane normal to the plane used to define the center curve. It should be a closed profile. The application now previews the rib to be created. You can control its position by choosing one of the following options:

Keep Angle: keeps the angle value between the sketch plane used for the profile and the tangent of the center curve. Pulling Direction: sweeps the profile with respect to a specified direction. To define thisdirection, you can select a plane or an edge. Reference Surface: the angle value between axis and the reference surface is constant.

The Merge ends option is to be used in specific cases. It creates materials between the ends of therib and existing material provided that existing material trims both ends. Check the Thick Profile option to add thickness to both sides of Sketch.2. New options are then available. Click OK. Therib is created. The specification tree mentions this creation.

3.11 Slot

This task shows you how to create a slot that is how to sweep a profile along a center curve to remove material. To define a slot, you need a center curve, a planar profile, a reference element and optionally a pulling direction.

Click the Slot icon . The Slot Definition dialog box is displayed. Select the profile. The profile has been designed in a plane normal to the plane used to define the center curve. It is closed. Slots can also be created from sketches including several profiles. These profiles must be closed and must not intersect. You can control the profile position by choosing one of the following options: Keep angle, Pulling direction, Reference surface. The Merge ends option is to be used in specific cases. It lets the application create material between the ends of the slot and existing material. Check the Thick Profile option to add thickness to both sides.

3.12 Loft

You can generate a loft feature by sweeping one or more planar section curves along a computed or user-defined spine. The feature can be made to respect one or more guide curves. The resulting feature is a closed volume.

Click the Loft icon

.The Loft Definition dialog box appears. Select the three section curves. They are highlighted in the geometry area. The Loft capability assumes that the section curves to be used do not intersect. Click Apply to preview the loft to be created. You can note that by default, tangency discontinuity points are coupled. Several coupling types are available in the Coupling tab: Ratio, Tangency, Tangency then curvature, Vertices.

By default, the application computes a spine, but if you wish to impose a curve as the spine to be used, you just need to click the Spine tab then the Spine field and select the spine of your choice in the geometry. Click OK to create the volume. The feature (identified as Loft.xxx) is added to the specification tree.

3.13 Remove Lofted Material

This task shows how to remove lofted material. The Remove Loft capability generates lofted material surface by sweeping one or several planar section curves along a computed or user-defined spine then removes this material.

Click the Remove Loft icon . The Remove Loft Definition dialog box appears. Select required sections & guide curves if needed. By default, the application computes a spine, but if you wish to impose a curve as the spine to be used, you just need to click the Spine tab then the Spine field and select the spine of your choice in the geometry. Click OK to create the lofted surface. The feature (identified as Loft.xxx) is added to the specification tree.

3.14 Stiffener

This task shows you how to create a stiffener by specifying creation directions. Select the profile to be extruded. This profile has to be created in a plane normal to the face on which the stiffener will lie. You can use wireframe geometry as your profile. If you need to use an open profile, make sure

that existing material can fully limit the extrusion of this profile. Click the Stiffener icon . The Stiffener Definition dialog box is displayed.

Two creation modes are available:

From side: the extrusion is performed in the profile's plane and the thickness is added normal to the plane. Check the Neutral Fiber option. This option adds material equally to both sides of the profile. Optionally click Preview to see the result. Click OK. The stiffener is created. The specification tree indicates it has been created. From Top: the extrusion is performed normal to the profile's plane and the thickness is added in the profile's plane. The "Neutral Fiber" option adds the same thickness to both sides of the profile. You just need to specify the value of your choice in "Thickness 1" field and this thickness is evenly added to each side of the profile. Conversely, if you wish to add different thickness on both sides of the profile, just uncheck the "Neutral Fiber" option and then specify the value of your choice in "Thickness 2" field.

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