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4 DRESSING UP OF SOLIDS

4.1 Edge Fillet

Edge fillets are smooth transitional surfaces between two adjacent faces. With the use of a constant

radius: the same radius value is applied to the entire edges. Click the Edge Fillet icon . The Edge Fillet Definition dialog box appears. Select the edges. The edge selected then appears in the Objects to fillet field. CATIA displays the radius value. Clicking Preview previews the fillet to be created. Two propagation modes are available: Minimal, Tangency. If you set the Tangency mode, the option "Trim ribbons" becomes available; you can then trim the fillets to be created. Use Limiting Elements to limit the fillet. When filleting an edge, the fillet may sometimes affect other edges of the part, depending on the radius value you specified. With the Edges to keep option the application detects these edges and stops the fillet to these edges.

4.2 Face-Face Fillet

You generally use the Face-face fillet command when there is no intersection between the faces or when there are more than two sharp edges between the faces. Select the faces to be filleted. Click Preview to see the fillet to be created. Click OK. The faces are filleted. This creation is indicated in the specification tree. Instead of entering a radius value, you can use a "hold curve" to compute the fillet. Depending on the curve's shape, the fillet's radius value is then more or less variable.

4.3 Tritangent Fillet

The creation of tritangent fillets involves the removal of one of the three faces selected. You need three faces two of which are supporting faces. Select the faces to be filleted. Select the face to be removed. The fillet will be tangent to this face. Click Preview to see the fillet to be created. The creation of this fillet is indicated in the specification tree indicates the opposite portion of material. Click OK.

4.4 Chamfer

Chamfering consists in removing or adding a flat section from a selected edge to create a beveled surface between the two original faces common to that edge. The default parameters to be defined are Length1 and Angle. You can change this creation mode and set Length1 and Length2. Chamfers can be created by selecting a face; the application chamfers its edges. Click Preview to see the chamfers to be created. Click OK. The specification tree indicates this creation.

4.5 Basic Draft

Drafts are defined on molded parts to make them easier to remove from molds. The characteristic elements are:

Pulling direction: this direction corresponds to the reference from which the draft faces are defined. Draft angle: this is the angle that the draft faces make with the pulling direction. Parting element: this plane, face or surface cuts the part in two and each portion is drafted according to its previously defined direction. Neutral element: this element defines a neutral curve on which the drafted face will lie. This element will remain the same during the draft.

The Propagation option can be set to: None: there is no propagation, Smooth: the application integrates the faces propagated in tangency onto the neutral face to define the neutral element.

Parting = Neutral to reuse the plane you selected as the neutral element. If Keep Parting =Neutral, you then can also check the option Draft both sides. Click OK. Material has been removed & the face is drafted.

4.6 Variable Angle Draft

Click the Variable Angle Draft icon . The Draft Definition dialog box that appears, displays the variable angle draft option as activated. Select the face to be drafted. Select face as the neutral element. The application detects two vertices and displays two identical radius values. Increase the angle value: only one value is modified accordingly in the geometry. To edit the other angle value, select the value in the geometry and increase it in the dialog box. To add a point on the edge, click the Points field. You can add as many points as you wish. Click OK to confirm.

4.7 Draft from Reflect Lines

This will draft a face by using reflect lines as neutral lines from which the resulting faces will be

generated. Click the Draft from Reflect Lines icon . The Draft from Reflect Lines Definition dialog box is displayed and an arrow appears, indicating the default pulling direction. Select the face. The application detects reflect line and displays it in pink. This line is used to support the drafted faces. Enter an angle value in the Angle field. The reflect line is moved accordingly. Click Preview to get an idea of what the draft will look like.

4.8 Shell

Shelling a feature means emptying it, while keeping a given thickness on its sides. Shelling may

also consist in adding thickness to the outside. Click the Shell icon . The Shell Definition dialog box appears. The selected face becomes purple. Select the face to be removed. Enter the Default inside thickness field. Click OK. The feature is shelled.

4.9 Thickness

You can add or remove thickness to parts. Click the Thickness icon . The Thickness Definition dialog box is displayed. Select the faces to thicken. Enter a positive value. Click OK. The part is thickened accordingly. This creation appears in the specification tree.

4.10 Thread/Tap

The Thread/Tap capability creates threads or taps, depending on the cylindrical entity of interest.
 

Click the Thread/Tap icon . The Thread/Tap Definition dialog box is displayed. Select the cylindrical surface you wish to thread. Select the upper face as the limit face. Limit faces must be planar. The application previews the thread. The Numerical Definition frame provides 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.

Enter the thread depth, pitch value. Check the Left-Threaded option. Click Preview. Red linesprovide a simplified representation of the thread. Click OK to confirm. There is no geometrical representation is the geometry area, but the thread (identified as Thread.xxx) is added to the specification tree.

5 Transformation Features

Following are different transformation features available

5.1 Translation

The Translate command applies to current bodies. This task shows you how to translate a body.

Click the Translate icon . The Translate Definition dialog box appears. Select a line to take its orientation as the translation direction or a plane to take its normal as the translation direction. You can also specify the direction by means of X, Y, Z vector components by using the contextual menu on the Direction area. Specify the translation distance by entering a value. Click OK to create the translated element. The element (identified as Translate.xxx) is added to the specification tree.

5.2 Rotation

This task shows you how to rotate geometry about an axis. The command applies to current

bodies. Click the Rotate icon . The Rotate Definition dialog box appears. Select an edge as the rotation axis. Enter a value for the rotation angle. The element is rotated. You can drag it by using the graphic manipulator to adjust the rotation. Click OK to create the rotated element. The element (identified as Rotate.xxx) is added to the specification tree.

5.3 Symmetry

This task shows how to transform geometry by means of a symmetry operation. The Symmetry

command applies to current bodies. Click the Symmetry icon

.The Symmetry Definition dialog box appears. Select a point, line or plane as reference element. Click OK to create the symmetrical element. The original element is no longer visible but remains in the specification tree. The new element (identified as Symmetry.xxx) is added to the specification tree.

5.4 Mirror

Mirroring a body or a list of features consists in duplicating these elements using symmetry. You can select a face or a plane to define the mirror reference. Multi-select both pads as the features to

be mirrored. Click the Mirror icon . The Mirror Definition dialog box appears. Select the lateral face to define the mirror reference. The application previews the material to be created. Click OK to confirm the operation. The pads are mirrored. The specification tree mentions this creation.

5.5 Rectangular Pattern

You may need to duplicate the whole geometry of one or more features and to position this geometry on a part. Patterns let you do so. CATIA allows you to define three types of patterns: rectangular, circular and user patterns. These features accelerate the creation process.

Rectangular Pattern task shows you how to duplicate the geometry of one pocket right away at the location of your choice using a rectangular pattern. Select the feature you wish to copy. Click

the Rectangular Pattern icon . The Rectangular Pattern Definition dialog box that appears displays the name of the geometry to pattern. Click the Reference element field and select the edge to specify the first direction of creation. An arrow is displayed on the pad. If needed, check the Reverse button or click the arrow to modify the direction. The parameters you can choose are: Instances & Length, Instances & Spacing, Spacing & Length. Choosing Instances & Spacing dims. Enter 3 as the number of instances you wish to obtain in the first direction. Defining the spacing along the grid. Checking the Keep specifications option creates instances with the limit Up to Next (Up to Last, Up to Plane or Up to Surface) defined for the original feature. Now, click the Second Direction tab to define other parameters. Note that defining a second direction is not compulsory. Creating a rectangular defining only one direction is possible. Click the Reference element field and select the edge to the left to define the second direction. Let the Instances & Spacing option. Click Preview to make sure the pattern meets your needs. Additional pockets will be aligned along this second direction. Click OK.This is the resulting pattern. The feature "RectPattern.1" is displayed in the specification tree

5.6 Circular Pattern

This task will show you how to duplicate geometry of one or more features right away at the location of your choice using a circular pattern. Make sure the item you wish to duplicate is correctly located in relation to the circular rotation axis. Select the pad which geometry you wish

to copy. Click the Circular Pattern icon . The Circular Pattern Definition dialog box is displayed and the feature's name appears in the Object field. The Parameters field lets you choose the type of parameters you wish to specify so that the application will be able to compute the location of the items copied. These parameters are: Instances & total angle, Instances & angular spacing, Angular spacing & total angle, complete crown. Set the Instances & Angular spacing options to define the parameters you wish to specify. Enter 7 as the number of pads you wish to obtain. Enter 50 degrees as the angular spacing. Click the Reference element field and select the upper face to determine the rotation axis. This axis will be normal to the face. Two arrows are then displayed on the pad. To define a direction, you can select an edge or a planar face. Click Preview. The pad will be repeated seven times. Now, you are going to add a crown to your part. To do so, click the Crown Definition tab. Enter 2 in the Circle(s) field. Enter -18 mm in the Circle spacing field. Click OK. One more ring of pads will be added.

5.7 User Pattern

The User Pattern command lets you duplicate a feature as many times as you wish at the locations of your choice. Locating instances consists in specifying anchor points. These points are created in

the Sketch. Select the feature you wish to duplicate. Click the User Pattern icon . The User Pattern dialog box is displayed. The feature appears in the Object field. Select 'Sketch ' in the specification tree and click Preview. Click OK. The specification tree indicates this creation.

5.8 Scaling

Scaling a body means resizing it to the dimension you specify. Select the body to be scaled. Click

the Scaling icon . The Scaling Definition dialog box appears. Select the reference point located on the body. Enter a value in the Ratio field or select the manipulator and drag it. The ratio increases as you drag the manipulator in the direction pointed by the right end arrow. Click OK. The body is scaled. The specification tree indicates you performed this operation.

6 Measuring

6.1 Measuring Distances & Angles between Geometrical

Entities & Points

This task explains how to measure minimum distances and angles between geometrical entities

(surfaces, edges, vertices and entire products) or between points. Click the Measure Between icon. The Measure Between dialog box appears. The Measure Item command is accessible from

the Measure Between dialog box. Simply click the Measure Item icon in the Definition box. Select the desired measure type.

Any geometry (default mode): measures distances and angles between defined geometrical entities (points, edges, surfaces, etc.). Exact else approximate (default mode): measures access exact data and wherever possible true values are given. If exact values cannot be measured, approximate values are given (identified by a ~ sign). Approximate: measures are made on tessellated objects and approximate values are given (identified by a ~ sign). Click to select a surface, edge or vertex, or an entire product (selection 1). Click to select another surface, edge or vertex, or an entire product (selection 2).

A line representing the minimum distance vector is drawn between the selected items in the geometry area. Appropriate distance values are displayed in the dialog box.

6.2 Measuring Properties

This task explains how to measure the properties associated to a selected item (points, edges, surfaces and entire products). This command lets you choose the selection mode, the calculation mode and axis system when measuring properties. Switch to Design Mode. Set View -> Render

Style to Shading with Edges. Click the Measure Item icon. The Measure Item dialog box appears. By default, properties of active products are measured with respect to the product axis system. Properties of active parts are measured with respect to the part axis system. The Keep Measure option lets you keep current and subsequent measures as features. This is useful if you want to keep measures as annotations for example.

6.3 Measuring Inertia

This task explains how to measure the inertia properties of an object. You can measure the inertia properties of both surfaces and volumes. The area, density, mass and volume (volumes only) of the object are also calculated. Measures are persistent: a Keep Measure option in the Measure Inertia dialog box lets you keep the current measure as a feature in the specification tree.

Click the Measure Inertia icon. Click to select the desired item in the specification tree. The Dialog Box expands to display the results for the selected item. The measure is made on the selection, geometry or assembly. To measure the inertia of individual sub-products making up an assembly and see the results in the document window, you must select the desired sub-product. In addition to the center of gravity G, the principal moments of inertia M and the matrix of inertia calculated with respect to the center of gravity, the dialog box also gives the area, volume (volumes only), density and mass of the selected item.

7 Surface-Based Features

7.1 Split

You can split a body with a plane, face or surface. Select the blue pad as the body to be split. Click

the Split icon . Select the splitting surface. The Split Definition dialog box is displayed, indicating the splitting element. An arrow appears indicating the portion of body that will be kept. If the arrow points in the wrong direction, you can click it to reverse the direction. Click OK. The body is split. Material has been removed. The specification tree indicates you performed the operation.

 

7.2 Thick Surface

You can add material to a surface in two opposite directions by using the Thick Surface capability.

Select the object you wish to thicken, that is the extrude element. Click the Thick Surface icon . The Thick Surface Definition dialog box is displayed. In the geometry area, the arrow that appears on the extrude element indicates the first offset direction. If you need to reverse the arrow, just click it. Enter 10mm as the first offset value and 6mm as the second offset value. Click OK. The surface is thickened. The specification tree indicates you performed the operation.

 

7.3 Close Surface

This task shows you to close surfaces. Select the surface to be closed. Click the Close Surface icon

. The Close Surface Definition dialog box is displayed. Click OK. The surface is closed . The specification tree indicates you performed the operation.

 

INITIAL FINAL
 

7.4 Sew Surface

Sewing means joining together a surface and a body. This capability consists in computing the intersection between a given surface and a body while removing useless material. You can sew all types of surfaces onto bodies. Select the surface you wish to sew onto the body. Click the Sew

Surface icon . The Sew Surface Definition dialog box is displayed, indicating the object to be sewn. An arrow appears indicating the portion of material that will be kept. Click the arrow to reverse the direction. Click OK. The surface is sewn onto the body. Some material has been removed. The specification tree indicates you performed the operation.

 

INITIAL FINAL

8 Advanced Tasks

This section will explain and illustrate how to perform operations on bodies and will provide recommendations about how to optimize the use of the application.

8.1 Inserting a New Body

This task shows you how to insert a new body into the part. When your part includes several bodies, you can then associate these bodies in different ways to obtain the final shape of the part.

Click the Insert Body icon. The result is immediate. CATIA displays this new body referred to as "Body.x" in the specification tree. It is underlined, indicating that it is the active body. You can now construct this new body using the diverse commands available in this workbench or in other workbenches. You will notice that Part Body and Body.x are autonomous. The operations you would accomplish on any of them would not affect the integrity of the other one. Now, if you wish to combine them, refer to the following tasks showing the different ways of attaching bodies: Adding Bodies, Assembling Bodies, Intersecting Bodies, Removing Bodies, Trimming Bodies.

8.2 Assembling Bodies

Assembling is an operation integrating your part specifications. It allows you to create complex geometry. Example: you are going to assemble a pocket on Part Body. You will note that as this pocket is the first feature of the body, material has been added. To assemble them, select Body 2

and click the Assemble icon . The Assemble dialog box displays to let you determine the operation you wish to perform. By default, CATIA proposes to assemble the selected body to Part Body. Click OK to confirm. During the operation, CATIA removes the material defined by the pocket from Part Body. This is your new Part Body.

 

 

8.3 Adding Bodies

This task illustrates how to add a body to another body. Adding a body to another one means

uniting them. Click the Add icon . The Add dialog box that appears displays the name of the selected body and the Part Body. By default, the application proposes to add the selected body to Part Body. Click OK. You will note that: the material common to Part Body and Body.1 has been removed.

8.4 Removing Bodies

This task illustrates how to remove a body from another body. Click the Remove icon

proposes to remove the selected body from Part Body.

8.5 Intersecting Bodies

The material resulting from an intersection operation between two bodies is the material shared by these bodies. When working in a CATProduct document, it is no longer necessary to copy and paste the bodies belonging to distinct parts before associating them. You can directly associate

these bodies using the same steps as described in this task. Click the Intersect... icon. The Intersect dialog box displays to let you determine the second body you wish to use. By default, the application proposes to intersect the selected body to Part Body. Click OK to confirm. Click OK to confirm. CATIA computes the intersection between the two bodies.

8.6 Trimming Bodies

Applying the Union Trim command on a body entails defining the elements to be kept or removed while performing the union operation. You need to select the required bodies and specify the faces

you wish to keep or remove. Click the Union Trim icon . Select the body you wish to trim, i.e. Body.2. The Trim Definition dialog box is displayed. The faces you cannot select are displayed in red. Click the Faces to remove field and select Body.2 's inner face. The selected face appears in pink, meaning that the application is going to remove it. Click the Faces to keep field and select Part Body. 's inner face. This face becomes blue, meaning that the application is going to keep it. Clicking the Preview button lets you check if your specifications meet your needs or not. To

restore the view, you simply need to click the Undo command. Click OK to confirm. The application computes the material to be removed. The operation (identified as Trim.xxx) is added to the specification tree.

 

8.7 Remove Lump

The Remove Lump command lets you reshape a body by removing material. To remove material, either you specify the faces you wish to remove or conversely, the faces you wish to keep. In some cases, you need to specify both the faces to remove and the faces to keep. Select the body you wish

to reshape, that is Part Body. Click the Remove Lump icon . The Remove Lump dialog box appears. The application prompts you to specify the faces you wish to remove as well as the faces you need to keep. Click the Faces to remove field and select the colored face. The selected face appears in pink, meaning that it will be removed during the operation. Click OK.

 

9 Customizing a Part Design Work Bench

9.1 Customizing a CATPart document

This task shows you how to set general settings. Select the Tools -> Options... command. Click the Infrastructure category, the Part Infrastructure subcategory, then the Part Document tab. The tab appears, containing one option:

New Part Check Create an Axis System when creating a new part if you wish to create a three-axis system which origin point is defined by the intersection of the three default planes that is plane xy, plane yz, and plane zx. When the CATPart is open, the axis system is displayed both in the geometry and in the specification tree

9.2 Customizing General Settings

This task shows you how to set general settings. Select the Tools -> Options... command Click the Infrastructure category, then the Part Infrastructure subcategory. The General tab appears, containing three categories of options: External References, Update, and Delete Operation. External References- Checking the Keep link with selected object option lets you maintain the links between external references, copied elements for example, and their origins when you are editing these elements. This option is used as you are editing parts included in assemblies. If later you need to cut the link between external references and their origin, you just need to use the Isolate command.- Check Create external references in Show mode to define the visualization mode for the elements while they are being created.- Check Confirm when creating a link with selected object- Check Only use published elements for external selection if you want to make only published elements valid for selection. Update- Check Manual: you wish to control your update operations. Check Automatic: parts are updated automatically. Check Synchronize all external references for update to make sure that CATIA updates elements copied from other parts. Delete Operation - Check Display the Delete dialog box if you wish to access filters for deletion Check Delete referenced sketches if you wish to delete sketches associated to features while you are deleting those features. Sketches will be deleted only if they are exclusive, which means that if they are shared by other features, they will not be deleted.

9.3 Customizing the Tree and Geometry Views

This task shows you how to control the display of the elements you create in the specification tree. It also shows you how to control the display of features in the geometry area. Select the Tools -> Options command. The Options dialog box is displayed. Click the Infrastructure category, then the Part Infrastructure subcategory, then Display tab. The tab appears, containing two categories of options: Specification tree, Geometry, from where we can customize the Tree and Geometry Views.

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