Prismatic Machining Preparation Assistant

Transcription

1 Prismatic Machining Preparation Assistant Overview Conventions What's New Getting Started Open the Design Part and Start the Workbench Automatically Create All Machinable Features Open the Manufacturing View Browse Axial Machinable Features Browse Prismatic Machining Areas User Tasks Globally Create All Machinable Features Locally Create Machinable Features Create an Axial Operation on a Machinable Feature Create a Milling Operation on a Machinable Feature Select Machinable Features Using the Search Command Automatically Create Machining Patterns Create a Machining Pattern on Machinable Features Create a Machining Process for Machinable Features Apply a Machining Process on Machinable Features Associativity of Prismatic Machining Area Workbench Description Toolbars Reference Information Prismatic Machining Area Features Axial Machinable Features Associativity Glossary Index

2 Overview Welcome to the Prismatic Machining Preparation Assistant User's Guide. This guide is intended for users who need to become quickly familiar with the Prismatic Machining Preparation Assistant Version 5 product. This overview provides the following information: Prismatic Machining Preparation Assistant in a Nutshell Before Reading this Guide Getting the Most Out of this Guide Accessing Sample Documents Conventions Used in this Guide. Prismatic Machining Preparation Assistant in a Nutshell Prismatic Machining Preparation Assistant delivers Machinable Features recognition and associated functionalities for preparing a design part for Prismatic Machining. This product assists the NC programmer in making the link between Design and Manufacturing. It provides a set of functionalities that generate all Prismatic Machinable Features of the design part. It builds a real Manufacturing View of the design part with all the drilling and milling features to be machined. Thanks to its Machinable Features Recognition technology, Prismatic Machining Preparation Assistant allows Prismatic Machinable Features creation for all kinds of CATIA Version 5 design parts, including those with no Design Feature specifications, as well as non-catia Version 5 design parts. It is totally integrated with the Prismatic Machining and Advanced Machining products. It dramatically reduces programming times by automatically creating all geometric areas that must be machined with Prismatic Machining operations, reducing time spent in geometry selections. All Machinable Features can be fully machined with Prismatic Machining strategies by creating elementary machining operations or applying more complex machining processes in both drilling and milling domains. Prismatic Machining Preparation Assistant offers the following main capabilities: Automatically creates all Prismatic Machinable Features of a design part Locally creates a Prismatic Machining Feature of a design part Machinable Features integration in Prismatic Machining and Advanced Machining products Management of Recognized Prismatic Machinable Features in Manufacturing View (presentation, edition, highlight, and so on). Before Reading this Guide

3 Before reading this guide, you should be familiar with basic Version 5 concepts such as document windows, standard and view toolbars. Therefore, we recommend that you read the Infrastructure User's Guide that describes generic capabilities common to all Version 5 products. It also describes the general layout of V5 and the interoperability between workbenches. You may also like to read the following complementary product guides, for which the appropriate license is required: Prismatic Machining User's Guide: explains how to machine prismatic parts. NC Manufacturing Infrastructure User's Guide: explains how to use functionalities that are common to all Machining products. Getting the Most Out of this Guide To get the most out of this guide, we suggest that you start reading and performing the step-by-step Getting Started tutorial. This tutorial will show you how to prepare a basic prismatic part for machining. Once you have finished, you should move on to the User Tasks section, which gives more complete information about the product's functionalities. The Reference section provides useful complementary information. The Workbench Description section, which describes the commands that are specific to Prismatic Machining Preparation Assistant, will also certainly prove useful. Accessing Sample Documents To perform the scenarios, you will be using sample documents contained in the doc/online/mpaug_c2/samples or doc/online/mpaug_d2/samples folder. For more information about this, refer to Accessing Sample Documents in the Infrastructure User's Guide.

4 Conventions Certain conventions are used in CATIA, ENOVIA & DELMIA documentation to help you recognize and understand important concepts and specifications. Graphic Conventions The three categories of graphic conventions used are as follows: Graphic conventions structuring the tasks Graphic conventions indicating the configuration required Graphic conventions used in the table of contents Graphic Conventions Structuring the Tasks Graphic conventions structuring the tasks are denoted as follows: This icon... Identifies... estimated time to accomplish a task a target of a task the prerequisites the start of the scenario a tip a warning information basic concepts methodology reference information information regarding settings, customization, etc. the end of a task functionalities that are new or enhanced with this release allows you to switch back to the full-window viewing mode

5 Graphic Conventions Indicating the Configuration Required Graphic conventions indicating the configuration required are denoted as follows: This icon... Indicates functions that are... specific to the P1 configuration specific to the P2 configuration specific to the P3 configuration Graphic Conventions Used in the Table of Contents Graphic conventions used in the table of contents are denoted as follows: This icon... Gives access to... Site Map Split View mode What's New? Overview Getting Started Basic Tasks User Tasks or the Advanced Tasks Workbench Description Customizing Reference Methodology Glossary Index Text Conventions The following text conventions are used: The titles of CATIA, ENOVIA and DELMIA documents appear in this manner throughout the text. File -> New identifies the commands to be used.

6 Enhancements are identified by a blue-colored background on the text. How to Use the Mouse The use of the mouse differs according to the type of action you need to perform. Use this mouse button... Whenever you read... Select (menus, commands, geometry in graphics area,...) Click (icons, dialog box buttons, tabs, selection of a location in the document window,...) Double-click Shift-click Ctrl-click Check (check boxes) Drag Drag and drop (icons onto objects, objects onto objects) Drag Move Right-click (to select contextual menu)

7 Enhanced Functionalities What's New? Pattern creation along with feature recognition You can now create machining patterns and axial machinable features in a single step by setting pattern creation options in the Global Feature Recognition dialog box. Capability to apply Global Feature Recognition on selected faces You can now select faces for global feature recognition (previously it was possible to select bodies only). All the features that open onto selected faces are created. New option to recognize holes or circular pockets/cutouts You can now choose to create holes or circular pocket/cutout features depending on the value of a limiting diameter in the Global Feature Recognition dialog box. Enhanced capacity to recognize features in selected machining direction only If a machining direction is selected, you can now choose to create features that open in that direction only. Capability to create machining patterns that group holes by tolerances retrieved from design features Fitting tolerances defined in design features can be retrieved for machinable axial features and used to group holes with the same tolerance in one pattern when creating machining patterns. Select fewer faces for Local Feature Recognition A machinable feature can now be recognized without selecting all the faces of the feature. Improved feedback for Local Feature Recognition Improved user feedback when locally creating machinable features.

8 Getting Started Before getting into the detailed instructions for using Prismatic Machining Preparation Assistant, this tutorial is intended to give you a feel of what you can accomplish with the product. It provides the following step-by-step scenario that shows you how to use some of the key functionalities. Open the Design Part and Start the Workbench Automatically Create All Machinable Features Open the Manufacturing View Browse Axial Machinable Features Browse Prismatic Machining Areas

9 Open the Design Part and Start the Workbench This first task shows you how to open the part that is to be prepared for machining and start the workbench. 1. Select File > Open then select the SampleMPA.CATPart document. 2. If you are working with Prismatic Machining, select Machining > Prismatic Machining from the Start menu. If you are working with Advanced Machining, select Machining > Advanced Machining from the Start menu. The selected workbench appears. The workbench includes the Prismatic Machining Preparation toolbar. Your design part is displayed in the Setup Editor window along with the manufacturing specification tree.

10

11 Automatically Create All Machinable Features This task shows you how to prepare a design part for manufacturing by automatically creating all recognizable prismatic machinable features. 1. Select the Global Feature Recognition icon. The Global Feature Recognition dialog box appears. 2. Select the part in the 3D view. 3. Select all the Feature checkboxes so that the part will be analyzed for all machinable feature types. 4. Click OK to start the feature recognition process. An information box appears giving the following information: List of input bodies selected Total Number of faces in all input bodies Number of faces used in created features Number of machining features created.

12 All recognized machinable features are added to the Manufacturing View.

13 Open the Manufacturing View This task shows you how to open the Manufacturing View to see the results of the global feature recognition step. 1. Select the Manufacturing View icon in the Machining Features toolbar. 2. The Manufacturing View dialog box appears. Right-click the Manufacturing View object and select the Sort by Machining Features contextual command. The view shows that 6 machinable axial features and 4 prismatic machining areas were created.

14 Browse an Axial Machinable Feature This task shows you how to browse axial machinable features. 1. In the Manufacturing View, select one of the axial machinable features as follows: In the example above, the selected feature is a counterbore hole. It is highlighted in the 3D view. 2. Double click the feature in the tree. A dialog box appears showing the characteristics of the feature.

15

16 Browse a Prismatic Machining Area This task shows you how to browse prismatic machining areas. 1. In the Manufacturing View, select one of the prismatic machining areas as follows: In the example above, the selected feature is a complex step. It is highlighted in the 3D view. 2. Double click the feature in the tree. A dialog box appears showing the characteristics of the feature.

17

18 User Tasks The user tasks you will perform with Prismatic Machining Preparation Assistant involve creating and managing machinable features. Globally Create All Machinable Features Locally Create Machinable Features Create an Axial Operation on a Machinable Feature Create a Milling Operation on a Machinable Feature Select Machinable Features Using the Search Command Automatically Create Machining Patterns Create a Machining Pattern on Machinable Features Create a Machining Process for Machinable Features Apply a Machining Process on Machinable Features Associativity of Prismatic Machining Area

19 Globally Create All Prismatic Machinable Features This task shows you how to prepare a design part for manufacturing by automatically creating all recognizable prismatic machinable features. The SampleMPA.CATPart document should be open. 1. Select the Global Feature Recognition icon. The Global Feature Recognition dialog box appears. 2. Set Selection Type to Body then select the part in the 3D view. The feature recognition takes the associated Body object into account. 3. Select all the Feature checkboxes so that the part will be analyzed for all machinable feature types. To create axial machining features only, just select the Hole checkbox. To create prismatic machining areas only, select all the checkboxes except the Hole checkbox. To create all holes included in a tab hole, select the Enable creation of tab hole components checkbox. A tab (or tabulated) hole is more complex than a Part Design hole in that its hole chain (that is, all faces) do not match a Part Design feature. If the checkbox is not selected, the holes belonging to the tab holes are not created (default behaviour).

20 4. Click OK to start the feature recognition process. All recognized machinable features are added to the Manufacturing View. Note that Selection Type can be set to Face. In this case, all recognized features that open onto selected faces will created. However, suppose a pocket has a child pocket and the top face of upper pocket is selected. The child pocket will not be created as it does not open directly onto the selected face. Graphic and Text Feedback about Machinable Features When you select or move the mouse over a Machinable Axial Feature in the Manufacturing View, feedback in 3D Viewer shows: Highlight of flank RSURs referenced by the Machinable Axial Feature The entry point and entry vector of the feature.

21 Machining direction of a recognized through feature can be reversed by right clicking that feature in Manufacturing View and selecting the Reverse Machining Direction contextual command. This command is not available for the blind features, as they can be machined in only one direction. This command cannot be accessed if the feature is machined. The identifier of the Machinable Axial Feature is shown as follows: Machinable Axial Feature.1 (Simple Hole Diameter=12mm Depth=20mm) representing in a summary the parameters of the feature. If you rename the feature: MyFeature.1 (Simple Hole Diameter=12mm Depth=20mm) Both the graphical representation and the feature in the Manufacturing View are associative and always up-to-date, positioned and filled according to design changes. When geometry can no longer be retrieved from a feature (referenced RSURs are no longer in Design Part, for example) no user representation is displayed. Advanced Parameters The Advanced tab page of the Global Feature Recognition dialog box contains a number of parameters for specific processing.

22 Machining Direction You can specify a machining direction by selecting a face, a line or an edge. Created features will then have a machining axis parallel to the selected direction. By specifying a machining direction, you can choose to create features that open in that direction only. For example, this may correspond to the machining direction of a particular machine setup. If no machining direction is selected, the Create features only in this direction checkbox cannot be selected. Hole / Pocket or Cutout You can choose to create holes or circular pocket/cutout features depending on the value assigned for the maximum hole diameter. Using this capability: large diameter holes can be created as Pockets small diameter intersecting holes can be created as Holes instead of a single complex pocket. Make sure you have selected the appropriate Feature type in the Basic tab page (for example, if you want to recognize a hole as a pocket, select the Hole and Complex Pocket checkboxes or just the Complex Pocket checkbox).

23 Ignore Tapered Hole Component You can choose to ignore the fact that the hole type is tapered during feature recognition. In this way, you can force chamfered holes to be recognized as simple holes. Chamfered hole: Recognized hole: Selection of Bodies One or more Bodies can be selected. For feature recognition, the In-Work object must be either a Body or the last component of a Body. For example, in the figures below: if you want to use Body.2 for feature recognition, the In-Work object must be either Body.2 or Hole.2. Body.2 and Hole.1 are valid In-Work objects. The identifier of the In-Work object is underlined in the tree.

24 Locally Create a Machinable Feature This task shows you how to locally create a prismatic machinable feature in a design part. The SampleMPA.CATPart document should be open. 1. Select the Local Feature Recognition icon. The Local Feature Recognition dialog box appears. 2. Select the type of feature to be recognized using the combo (Complex Step, for example). 3. Click the Faces to Process: No selection field, then in the 3D view locally select one of the contour faces of the complex step:

25 In previous releases, all the faces of the feature had to be selected to allow the feature to be recognized. Now, a feature can be recognized by selecting either the bottom face or one or more contour faces. To deselect a selected face, just reselect it. To deselect all selected faces, just click Remove All. 4. Click Recognize. An information box appears giving the following information about the recognized feature: The created feature appears in the Manufacturing View.

26 In the SampleMPA.CAtPart, to create: one of the simple holes, you need to locally select either the bottom or side face one of the counterbored holes, you need to locally select either the bottom or side face the complex cutout, you need to locally select either the bottom or a flank face the complex pocket, you need to locally select either the bottom or a flank face. If needed, you can specify a preferred machining direction for through features by selecting a face, line or an edge. The through features are given a machining axis direction parallel to the selected direction. Unsuccessful Local Feature Recognition In case of local feature recognition failure, an appropriate error message is issued. Whenever possible, the elements that caused the failure are highlighted. Some examples are given below. Feature type does not match. The recognized feature is not of the specified type. You must select at least one face that uniquely belongs to the feature. If you do not select a unique face, feature recognition will fail. Duplicate feature creation. When you try to recognize a feature that is already present in the manufacturing view, no new feature will be created. Non-machinable feature due to very small dimension. When machining parameters such as depth are very small so as to make them non-machinable, such features are not recognized. Non-machinable feature due to invalid face or edge contour. Feature creation is not possible because of the machinability checks applied on face or edge contour during feature creation.

27 Advanced Parameters The Advanced tab page of the Local Feature Recognition dialog box contains a number of parameters for specific processing. For more information, please refer to: Machining Direction Hole / Pocket or Cutout. Tips for Local Creation of Machinable Features with Feature Recognition In general, a feature can be recognized by selecting either the bottom face or one or more contour faces. To recognize a hole, you must select all the faces of the hole that will be machined: flank faces and, in case of a blind hole, the bottom face. Never select the top face.

28 To recognize a feature with fillets, you must select all the fillets to be able to recognize the feature. Note that features surrounded by convex fillets are not considered as prismatic features and are not managed by the feature recognition capability. In all cases, selection of non-adjacent faces will not allow feature recognition. In the image below, selection of all the red faces will not recognize a complex step feature.

29 In the case of intersecting holes, feature recognition will create as many holes as separate surfaces. In the image below, three features are recognized: one for each surface color. The blue and yellow surfaces do not generate a single machining feature.

30 Create an Axial Operation on an Axial Machinable Feature This task shows you how to create a Counterboring operation using an axial machinable feature. You can make use of one of the Counterbored Hole features created in the Globally Create All Prismatic Machinable Features task. 1. Select the Manufacturing View icon in the Machining Features toolbar. Use the Sort by Machining Features contextual command to display the desired view. 2.Select a Counterbored Hole feature in the view. 3. Select the Counterboring icon. The Counterboring dialog box appears. The operation is initialized with the feature geometry as well as default parameters for machining strategy, feeds and speeds, and tool. You can edit any of these values, if desired. 4.Select the Tool tab page and choose a suitable Counterbore tool according to the feature characteristics displayed in the Geometry page.

31 5. Click the Replay icon to verify the tool path. 6.Click OK to create the Counterboring operation. The operation is added to the Manufacturing View and to the program in the PPR tree.

32 Create a Milling Operation on a Prismatic Machining Area This task shows you how to create a pocketing operation on a prismatic machining area. You can make use of the Complex Step feature created in the Locally Create a Machinable Feature task. 1. Select the Manufacturing View icon in the Machining Features toolbar. Use the Sort by Machining Features contextual command to display the desired view. 2. Select the Complex Step feature in the view. 3. Select the Pocketing icon. The Pocketing dialog box appears. 4. The operation is initialized with the feature geometry as well as default parameters for machining strategy, feeds and speeds, and tool. You can edit any of these values, if desired. 5. Click the Replay icon to verify the tool path.

33 6. Click OK to create the pocketing operation. The operation is added to the Manufacturing View and to the program in the PPR tree.

34 Select Machinable Features Using the Search Command This task shows you how to select machinable features by means of search criteria. Features selected in this way can be used for: creating machining operations machining processes machining patterns. Open the Manufacturing View with the result of the Globally Create All Machinable Features task. 1. Select the Edit>Search command or run the command using the Ctrl+F shortcut. The Search dialog box appears. 2. Select the Advanced tab. 3. Set the Workbench, Type and Attribute search criteria as shown below. 4. To find all axial machinable features with a counterbore diameter of at least 10mm, specify the following search criteria in the dialog box that appears. Click OK. 5. Click the Search icon. The search result is displayed in the dialog box.

35 6. Click OK to select all the features corresponding to the search criteria. They are highlighted in the Part and in the Manufacturing View. A description of all feature attributes is given in Prismatic Machining Areas and Axial Machining Features.

36 Automatically Create Machining Patterns This task shows you how to automatically create axial machinable features and a machining pattern in a single step. Open the HoleMakingOperations.CATPart document, then select the desired Machining workbench from the Start menu. 1. Select the Global Feature Recognition icon. The Global Feature Recognition dialog box appears. 2. In the Basic tab page, select the Hole checkbox to create axial machinable features only. Select the top face of the part in the 3D view. 6. In the Pattern tab page, set the parameters for pattern creation as follows.

37 With these parameters you will create a pattern on threaded holes whose diameter is included in a specified range of diameters (that is, between 17 and 20mm). 7. Select the Manufacturing View icon and display the view sorted by patterns. The created machining pattern is displayed.

38 8. Double click the machining pattern node to display the Machining pattern dialog box to obtain more information about the pattern.

39 Geometry Considerations for Pattern Creation Pattern creation operates on a set of axial features selected from the Manufacturing View, a set of faces, or an entire body. For a set of axial features, pattern creation applies the matching criteria only to that set of features. For a set of planar faces, pattern creation applies the matching criteria to all axial features from each face in the set. Note that all features in a pattern will have identical axes. If a reference direction is defined, the matching criteria only applies to axial machinable features parallel to this axis. For a set of non-planar faces, pattern creation applies the matching criteria to all axial features from each face in the set. Features in the pattern can have different axes. If a reference direction is defined, automatic pattern creation only applies to axial machinable features parallel to this axis. For a body, pattern creation applies the matching criteria to all axial features. Note that all features in a pattern will have identical axes. If a reference direction is defined, automatic pattern creation only applies to axial machinable features parallel to this axis. Using Tolerances in Pattern Creation You can retrieve the fitting tolerances defined in design features when machinable axial features are created. You can match these tolerance values in the pattern creation functionality. The Tolerance Value checkbox for matching the fitting tolerance for pattern creation. You can create patterns of holes having same tolerance values. Matching is done for both tabulated (H7, and so on) as well as minimum/maximum tolerance values. Features having the same tolerance values are grouped in the same pattern. Other holes, for which the tolerance value is not defined, will form a separate pattern. The fitting tolerance value is retrieved and information is displayed to user: in the dialog box of the Machinable axial feature:

40 in the Manufacturing View on the created pattern:

41 Create a Machining Pattern on Machinable Features This task shows you how to create a machining pattern on machinable features. You can make use of the features created in the Globally Create All Prismatic Machinable Features task. 1. Select the Pattern Creation icon. The Pattern Creation dialog box appears. 2. Set Selection Type to Body then select the part in the 3D view. The pattern creation will take the associated Body object into account.

42 2. Click the Machining direction field, then select a geometric element to specify the machining direction (for example, selecting a face as shown means that the machining direction will be taken perpendicular to that face). Only those axial machinable features in the specified machining direction will be taken into account for the pattern. 3. Click OK to create the machining pattern. You can use the Sort by Patterns contextual command to check that the pattern is added to the Manufacturing View. 4. Double-click the pattern identifier to display the Machining Pattern dialog box.

43 The pattern is visualized in the part:

44 Create a Machining Process for Machinable Features This task shows how to create a machining process that will be used to apply a sequence of axial machining operations to machinable features. More information about creating machining processes with formula, checks and tool queries is available in Create a Machining Process in the NC Manufacturing Infrastructure User's Guide. 1. Select the Machining Process View icon. The Machining Process View dialog box appears. 2. Select the Machining Process icon. The dialog box is updated with a new machining process as shown. 3. Select the Spot Drilling icon. The Operation Definition dialog box appears, if the Start Edit mode is selected in the Tools > Options > Machining > Operation settings. 4. Just click OK to add a reference Spot Drilling operation to the machining process. You can associate Formulas or Checks to this reference operation and specify a Tool Query. 5. In the same way add Drilling and Tapping operations to the machining process by selecting first the Drilling icon then the Tapping icon. The Machining Process View dialog box is updated as shown.

45 6. Double click the Tool Query associated to the Spot Drilling operation. The Tool Query Definition dialog box appears. 7. Select the tool repository ToolsSampleMP using the Look in combo. Define a query to look for a spot drill whose nominal diameter is equal to the diameter of the machining axial feature. Click OK to assign the tool query to the Spot Drilling operation. You can assign simple tool queries to the Drilling and Tapping operations: Name=Drill D10.5 and Name=Tap D12, for example.

46 8. Select File > Save As to save the machining process in a CATProcess document called AxialMachiningProcess1.CATProcess, for example. 9. Right click the Machining Process in the Machining Process View and select the Save in Catalog contextual command. 10. The Save in Catalog dialog box appears. Click the [...] button and specify a new catalog name (catalogaxialmp1.catalog, for example). Click OK to save the machining process as a component in the specified catalog. The following are initialized automatically: family name: Machining Process component name: name given to the machining process using File > Save As. However, you can change family or component in the Catalog Editor workbench. Click here to see how you can organize machining processes in a catalog using the Catalog Editor workbench. For the next step in the procedure, please refer to Apply Machining Process on Machinable Features.

47 Apply a Machining Process on Machinable Features This task shows how to apply a machining process on machinable features. Open the desired CATPart document, then select the desired Machining workbench from the Start menu. 1. Select the Open Catalog icon and open the catalog you created in the previous task: catalogaxialmp1.catalog. 2. Double click the Machining Process family: AxialMachiningProcesses. 3. Double click the Machining Process to be applied: AxialMachiningProcess1.

48 The Insert Object dialog box appears allowing you to apply the machining process. 4. Select the geometry to be machined. This can be one of the following: a design feature a machining pattern an axial machinable feature a machining pattern of axial machinable features a prismatic machining area.

49 Then click OK in the Insert Object dialog box. 5. The program is updated with the operations contained in the machining process: spot drilling drilling tapping. These operations reference the selected geometry and make use of any formula defined in the machining process. In addition, the tool queries are resolved so that each operation references the desired tool.

50 Associativity of Prismatic Machining Area This task illustrates the associativity of prismatic machining areas. A prismatic machining area in the manufacturing view has associated geometry in the part document. Typical geometry could be: Top element Bottom element Boundary profile Other Prismatic machining area parameters such as minimum corner radius. If the geometry is modified in the part document, then corresponding parameters and RSUR information for prismatic machining area is updated in manufacturing view to reflect correct values. 1. Select File > Open then select the PrismaticMachining.CATPart document. 2. Select the Global Feature Recognition icon and create a Complex Pocket. 3. Select the Manufacturing View icon in the Machining Features toolbar. Right-click the Manufacturing View object and select the Sort by Machining Features contextual command.

51 4. Double click the created Prismatic machining area in the tree. A dialog box appears showing the characteristics of the feature. 5. Right click the green flank area of the pocket in the sensitive icon and select the Analyze contextual command. The Geometry Analyser appears showing that the status of each of the guide elements making up the pocket is Up to date. Analyze the bottom element in the same way to check that its status is also Up to date.

52 6. Modify the geometry of the pocket (for example by reducing the pocket depth). 7. In the Manufacturing View, analyze the new guide elements and bottom of the pockets. Their status is Up to date, showing the associative nature of the prismatic machining area. Some geometry modifications to a part document can change the feature type. For example: the depth of complex pocket can be changed so that it becomes complex cutout the boundary profile of a complex pocket can be modified in such a way that it becomes a complex step, blind slot or through slot. Such changes are not associative.

53 Workbench Description This section contains the description of the specific commands that are added to your Prismatic Machining or Advanced Machining workbench when Prismatic Machining Preparation Assistant is installed. Toolbars

54 Prismatic Machining Preparation Assistant Toolbars When Prismatic Machining Preparation Assistant is installed the Prismatic Machining Preparation toolbar is added to the Prismatic Machining or Advanced Machining workbench. This toolbar contains the following commands: Global Feature Recognition See Globally Create All Prismatic Machinable Features Local Feature Recognition See Locally Create a Machinable Feature Pattern Creation See Create a Machining Pattern on Machinable Features The commands of the other toolbars of the Prismatic Machining workbench are documented in the Prismatic Machining User's Guide. The commands of the other toolbars of the Advanced Machining workbench are documented in the Advanced Machining User's Guide. It is useful to note that the Machining Features toolbar gives access to the Manufacturing View. Manufacturing View See Open the Manufacturing View.

55 Reference Information Reference information about Prismatic machinable features is given in this section. Prismatic Machining Areas Axial Machinable Features Associativity.

56 Prismatic Machining Areas This section provides reference information that is intended to help you: create Prismatic Machining Area features from your design part use Prismatic Machining Area features in the Prismatic Machining or Advanced Machining product: for machining process formulas, checks and tooling queries (for example, to find the appropriate tool to machine the machining area) for search queries.

57 The following Prismatic Machining Area features are supported: complex pocket complex step through slot blind slot complex cutout. Islands can be included Pocket and Step type machinable features. Complex Pocket

58 A complex pocket is a closed multi-sided recess. Specifications on part: A bottom stamp as a hard stamp A top element as a top limit A boundary comprising a series of ordered faces. Results in Prismatic Machining Area: A depth from top to bottom A minimum corner radius A minimum channel width A maximum channel width A top plane A bottom plane A wire frame contour. Complex Step A complex step is an open multi-sided recess. Specifications on part: A bottom stamp as a hard stamp A top element as a top limit A boundary comprising a series of ordered faces with hard and soft qualifications. Through Slot A through slot is a specific step whose contour is two parallel faces as a hard boundary and two other faces as limits. Results in Prismatic Machining Area: A depth from top to bottom A minimum corner radius A minimum channel width A maximum channel width A top plane A bottom plane A wire frame contour with a series of elements qualified as soft and hard. Specifications on part: A bottom stamp as a hard stamp A top element as a top limit A boundary comprising a series of 4 ordered faces with hard and soft qualifications. Blind Slot Results in Prismatic Machining Area: A minimum corner radius A minimum channel width A maximum channel width A top plane A bottom plane A wireframe contour with 4 elements: 2 lines and two other elements.

59 A blind slot is a specific step with two parallel lines and a corner between them. It has an open boundary. Specifications on part: A bottom stamp as a hard stamp A top element as a top limit A boundary comprising a series of 4 ordered faces with hard and soft qualifications. Results in Prismatic Machining Area: A depth from top to bottom A minimum corner radius A minimum channel width A maximum channel width A top plane A bottom plane A wireframe contour with 4 elements: 2 lines, 1 half circle and one other element. Complex Cutout A complex cutout is a multi-sided opening through the part. Specifications on part: A bottom element as a bottom limit A top element as a top limit A boundary comprising a series of ordered faces. Results in Prismatic Machining Area: A depth from top to bottom A minimum corner radius A minimum channel width A maximum channel width A top plane A bottom plane A wireframe contour. Management of Islands Islands can be recognized and associated to Pocket and Step type machinable features. Islands can be associated to features without necessarily sharing a bottom face. See examples below:

60

61 Specifications on part: A bottom stamp as a hard stamp A top element as a top limit A boundary comprising a series of ordered faces. Results in Prismatic Machining Area: A depth from top to bottom A top plane and a bottom plane A wireframe contour.

62 Axial Machinable Features This section provides reference information that is intended to help you: create Axial Machinable Features from your design part use Axial Machinable Features in the Prismatic Machining or Advanced Machining product: for machining process formulas and checks for search queries. A number of hole types are supported. They are identified according to the evaluation of the Hole type attribute as follows. Hole type Name 0 Simple hole 1 Tapered hole 2 Counterbored hole 3 Counterdrilled hole 4 Countersunk hole 5 Unknown

63 Simple Hole Simple hole is characterized by: origin point and direction hole depth and diameter extension type identified according to the evaluation of the Extension attribute: 1 = blind 2 = through for blind holes, bottom type identified according to the evaluation of the Hole bottom type attribute: Flat Bottom V Bottom. for V-bottom holes, bottom angle identified according to the value of the Hole bottom angle attribute. the hole can be threaded. Tapered Hole Tapered hole is characterized by: origin point and direction Counterbored Hole hole depth, diameter and angle Counterbored hole is characterized by: origin point and direction extension type identified according to the evaluation of the Extension attribute: 1 = blind 2 = through. for blind holes, bottom type identified according to the evaluation of the Hole bottom type attribute: Flat Bottom V Bottom. for V-bottom holes, bottom angle identified according to the value of the Hole bottom angle attribute. hole depth and diameter counterbored depth and diameter extension type identified according to the evaluation of the Extension attribute: 1 = blind 2 = through. for blind holes, bottom type identified according to the evaluation of the Hole bottom type attribute: Flat Bottom V Bottom. for V-bottom holes, bottom angle identified according to the value of the Hole bottom angle attribute. the hole can be threaded.

64 Counterdrilled Hole Counterdrilled hole is characterized by: origin point and direction hole depth and diameter countersunk angle counterbored depth and diameter extension type identified according to the evaluation of the Extension attribute: 1 = blind 2 = through. for blind holes, bottom type identified according to the evaluation of the Hole bottom type attribute: Flat Bottom V Bottom. for V-bottom holes, bottom angle identified according to the value of the Hole bottom angle attribute. the hole can be threaded. Countersunk Hole Countersunk hole is characterized by: origin point and direction hole depth and diameter countersunk angle and diameter countersunk depth extension type identified according to the evaluation of the Extension attribute: 1 = blind 2 = through. for blind holes, bottom type identified according to the evaluation of the Hole bottom type attribute: Flat Bottom V Bottom. for V-bottom holes, bottom angle identified according to the value of the Hole bottom angle attribute. the hole can be threaded. Please note that the Countersunk depth can be obtained by means of the following formula: Countersunk depth=(countersunk diameter-hole diameter)/(2*tan(countersunk angle/2)) Threaded Holes The following attributes on the axial machinable feature allow you to access threaded hole information (in

65 the Search function, machining process definition, machining operations that require thread information, and so on). Threaded: True or False Thread diameter (length value) Thread depth (length value) Pitch (length value) Thread direction: 0 = Right-threaded 1 = Left-threaded. The attribute values are read from the design threaded hole (that is, as specification).

66 Associativity of Machinable Axial Features This section describes the associativity behaviour of a Machinable Axial Feature after a design change (modification, move or delete) of the shape referenced by the feature. This is best illustrated by the following scenarios. Scenario 1 Modify the shape of faces referenced by a Machinable Axial Feature (iso-topology) Move the shape of faces referenced by a Machinable Axial Feature (iso-topology) Move the products where faces of a Machinable Axial Feature are referenced. The expected result is as follows. When editing the Machinable Axial Feature all the parameters are updated according to the new specifications. When updating the status of any Drilling operation referencing a Machinable Axial Feature, an Update mask must be displayed on the operation in the PPR tree. When editing any Drilling operation referencing a Machinable Axial Feature, Feature parameters displayed in Geometry tab page are updated according to the new specifications When replaying any Drilling operation referencing a Machinable Axial Feature using the editor, Tool Path replay must show tool path at appropriate location (except if locked). When replaying any Drilling operation referencing a Machinable Axial Feature not using the editor, Tool Path Replay must show tool path at appropriate location (except if locked). Scenario 2 The following design change is made: remove faces of a shape referenced by a Machinable Axial Feature from the Design Part. The expected result is as follows. When updating the status of any Drilling operation referencing a Machinable Axial Feature, an exclamation mask must be displayed on the operation in the PPR tree. Therefore replay is not available.

67 Glossary A approach macro auxiliary command axial machining operation Motion defined for approaching the operation start point A control function such as tool change or machine table rotation. These commands may be interpreted by a specific post-processor. Operation in which machining is done along a single axis and is mainly intended for hole making (drilling, counter boring, and so on). B bottom plane A planar geometric element that represents the bottom surface of an area to machine. It is normal to the tool axis. C clearance macro climb milling conventional milling Motion that involves retracting to a safety plane, a linear trajectory in that plane and then plunging from that plane. Milling in which the advancing tool rotates down into the material. Chips of cut material tend to be thrown behind the tool, which results to give good surface finish. Compare with conventional milling. Milling in which the advancing tool rotates up into the material. Chips of cut material tend to be carried around with the tool, which often impairs good surface finish. Compare with climb milling. D DPM Digital Process for Manufacturing. E extension type Defines the end type of a hole as being through hole or blind. F Facing operation Fault feedrate fixture A surfacing operation in which material is removed in one cut or several axial cuts of equal depth according to a pre-defined machining strategy. Boundaries of the planar area to be machined are soft. Types of faults in material removal simulation are gouge, undercut, and tool clash. Rate at which a cutter advances into a work piece. Measured in linear or angular units (mm/min or mm/rev, for example). Elements used to secure or support the workpiece on a machine.

68 G gouge Area where the tool has removed too much material from the workpiece. H hard high speed milling (HSM) A geometric element (such as a boundary or a bottom face) that the tool cannot pass beyond. Functionality that is supported for Pocketing and Facing operations in which corners and transitions in the tool path are rounded to ensure a smooth and continuous cutting effort. I inward helical island Machining in which motion starts from a point inside the domain to machine and follows paths parallel to the domain boundary towards the center of the domain. Compare with outward helical. Inner domain of a pocket that is to be avoided during machining. It has a closed hard boundary. L linking motion Motion that involves retracting to a safety plane, a linear trajectory in that plane and then plunging from that plane. M machine rotation machining axis system machining feature machining operation machining process An auxiliary command in the program that corresponds to a rotation of the machine table. Reference axis system in which coordinates of points of the tool path are given. A feature instance representing a volume of material to be removed, a machining axis, tolerances, and other technological attributes. These features may be hole type or milling type. Contains all the necessary information for machining a part of the workpiece using a single tool. An ordered list of machining operations, PP instructions and, possibly, machine rotations. It can be used in two ways: to generate a complete subprogram by defining all the operations from geometrical information which will be solved when the machining process is instantiated into another CATProcess file. to generate a subprogram by defining all the operations without any geometrical information (design or manufacturing geometrical features): this way is dedicated to the settings mode. machining tolerance manufacturing process manufacturing program The maximum allowed difference between the theoretical and computed tool path. Defines the sequence of part operations necessary for the complete manufacture of a part. Describes the processing order of the NC entities that are taken into account for tool path computation: machining operations, auxiliary commands and PP instructions.

69 manufacturing view maximum channel width minimum channel width minimum corner radius multi-level operation The set of machining features defined in the part operation. The diameter of the largest circle that fits inside the machining domain boundary (including islands). The maximum channel width may be used to determine the roughing tool. The smallest opening in the boundary profile (including islands) that the tool must pass through in order to completely machine the profile. Limit value: For particular geometrical cases, no minimum channel width exist. In this case the minimum channel width value must be equal to the maximum channel width value. The smallest radius of the Prismatic Machining Area boundary (including islands) that cause a constraint on the tool to be used for machining the domain. The minimum corner radius may be used to determine the finishing tool. Limit value: if an angle is detected on the profile (or islands) the minimum corner radius is 0. Milling operation (such as Pocketing or Profile Contouring) that is done in a series of axial cuts. O offset outward helical Specifies a virtual displacement of a reference geometric element in an operation (such as the offset on the bottom plane of a pocket, for example). Compare with thickness. Machining in which motion starts from a point inside the domain to machine and follows paths parallel to the domain boundary away from the center of the domain. Compare with inward helical. P part operation Links all the operations necessary for machining a part based on a unique part registration on a machine. The part operation links these operations with the associated fixture and set-up entities. pocket An area to be machined that is defined by an open or closed boundary and a bottom plane. The pocket definition may also include a top plane and one or more islands. Pocketing operation A machining operation in which material is removed from a pocket in one or several axial cuts of equal depth according to a pre-defined machining strategy. The tool path style is either Inward helical, Outward helical or Back and forth. Point to Point operation A milling operation in which the tool moves in straight line segments between user-defined points. PP instruction Instructions that control certain functions that are auxiliary to the tool-part relationship. They may be interpreted by a specific post processor. PPR Process Product Resources. Profile Contouring operation A milling operation in which the tool follows a guide curve and possibly other guide elements while respecting user-defined geometric limitations and machining strategy parameters. R retract macro Motion defined for retracting from the operation end point

70 return macro Motion for linking between paths or between levels. It involves retracting to a safety plane, a linear trajectory in that plane and then plunging from that plane. S safety plane set up soft spindle speed stock A plane normal to the tool axis in which the tool tip can move or remain a clearance distance away from the workpiece, fixture or machine. Describes how the part, stock and fixture are positioned on the machine. A geometric element (such as a boundary or a bottom face) that the tool can pass beyond. The angular speed of the machine spindle. Measured in linear or angular units (m/min or rev/min, for example). Workpiece prior to machining by the operations of a part operation. T thickness top plane tool axis tool change tool clash tool path total depth Specifies a thickness of material to be removed by machining. Compare with offset. A planar geometric element that represents the top surface of an area to machine. It is always normal to the associated tool's rotational axis. Center line of the cutter. An auxiliary command in the program that corresponds to a change of tool. Area where the tool collided with the workpiece during a rapid move. The path that the center of the tool tip follows during a machining operation. The total depth including breakthrough distance that is machined in a hole making operation. U undercut Area where the tool has left material behind on the workpiece.