SETTING UP PRO/NC IN PREPARATION FOR CREATING TOOL PATHS

Transcription

1 SETTING UP PRO/NC IN PREPARATION FOR CREATING TOOL PATHS PTC Technical Support - Advanced Manufacturing Technique 140 Kendrick St Needham, MA, USA

2 Introduction This document introduces the basic processes and techniques used to 1) Create a manufacturing model in Pro/NC 2) Define the setup required to efficiently create toolpaths. Although this document is intended for use by new users of Pro/NC, the information contained within could prove helpful for mature users also. The intent of this document is to provide users with a clear understanding of the various configuration and setup options available within Pro/NC. Not everything mentioned in this document is required to make toolpaths. However, to determine the optimal use of Pro/NC within one s company, an understanding of the various functionalities mentioned in this document is key. The topics within this document are applicable for both Milling and Turning models. Note: Pro/ENGINEER Release 2001 will be used to demonstrate the functionalities listed below. Model Definition/Creation Operation Setup Machine Tool Setup Fixture Setup Tool Definition/Setup Site File Creation Tool Path Defaults PPRINT Setup Operator Messages Estimated time to complete technique: 3 Hours Copyright 2002 by PTC 2 PTC Technical Support

3 Setup For this technique, a previously created milling reference model is used in addition to a previously created fixture. Below are images of the abovementioned models respectively. An NC-Assembly Model was used for this technique. The model contains a reference model, workpiece, and fixture assembly. Figure 1 - Reference Model: GEAR_HOUSING Copyright 2002 by PTC 3 PTC Technical Support

4 Figure 2 - Fixture Assembly: VICE Example Files The example models used in this document can be downloaded at the following location: Example Part Files Copyright 2002 by PTC 4 PTC Technical Support

5 Fundamentals The Manufacturing Model The strategy used to machine a part within Pro/NC is to first define the manufacturing model. The manufacturing model is an assembly consisting of at least one reference part, and may include a workpiece (stock model) as well as fixtures used to hold the part while being machined. The Reference Model represents the completely machined end product. The Workpiece represents the raw stock geometry from which the part will be machined. In some instances, the workpiece may be a casting and resemble the reference model. In other instances, the workpiece will be a billet or bar of material. Two types of manufacturing models can be defined in Pro/NC. The default model type is NC Assembly. The NC Assembly sub-type is used for machining more than one reference part or a reference model consisting of an assembly of parts. One, or many workpieces may be used in the manufacturing model or no workpieces at all. The NC Assembly sub-type also allows for the use of both regular assemblies and manufacturing assemblies that have been previously created. Components of these previously defined assemblies can be classified as reference models, workpieces or fixtures. In an NC Assembly model, all of the features created in manufacturing mode are saved to the assembly (.asm) file. The second type of manufacturing model is NC Part. Multiple reference models can be used but there must be one and only one workpiece. The workpiece does not have to have solid geometry but does need to be present in the manufacturing assembly. Manufacturing features created during tool path development will be placed into the workpiece model. Note: The ability to create an NC Part type of manufacturing model has been removed from Pro/ENGINEER Wildfire. Four different file types will be associated with the manufacturing model. The file types include the.prt (for the reference model and workpiece),.asm (the assembly containing the reference part and workpiece as components), the.mfg (contains the manufacturing specific information) and the.tph file (an encrypted file containing the computed toolpath geometry for the sequences within the *.mfg file.). These four file types are typically stored in the working directory where the manufacturing model is created. Sometimes, the complexity of a model can make feature and tool path creation difficult. Simplified representations enable the user to capture different states of the reference model during the machining process. Simplified representations can be used to 1.) Simplify the model, eliminating geometry not required for the current operation, 2.) Capture in-process geometry using the reference model. Copyright 2002 by PTC 5 PTC Technical Support

6 Refer to the online help for additional information regarding the creation and use of simplified representations. See the Additional Information section of this document for links regarding Simplified Representations. Operations Operations are a series of NC sequences performed at a particular workcell and using a particular coordinate system for cutter location (CL) data output. The coordinate system used by an operation in Pro/NC is called Machine Zero and is synonymous with Program Zero, Part Zero or Zero Datum. Some parts will require more than one setup on the NC machine to reach all the surfaces where material is to be removed. These setups will typically require a new operation in Pro/NC because the part orientation changes in reference to the coordinate system used to generate the CL data. For instance, consider a square block with holes to be drilled on both the top face and one of the side faces. If the NC machine being used only has 3-axis capability, the machine operator would need to reposition the block, i.e. change the setup, in order to drill the holes on the second face. In Pro/NC, one operation would be defined for machining on the top face and another operation for the machining on the side face. Sometimes additional operations will be desirable even though the part setup has not changed. See the Additional Information section of this document for links regarding Operation setup. The NC Machine During the operation definition, the NC Machine is specified. The NC machine is often referred to as a Workcell in Pro/NC and in the Help documentation. The NC Machine is a feature that defines the machine tool attributes such as, the machine name, machine type, number of axes, associated tools, parameters, etc. The NC Machine types that can be defined are Mill, Lathe, Mill/Turn, and WEDM (Wire Electronic Discharge Machine). During the NC Machine definition, the user can also designate default values for settings related to the tool path creation. These default settings are stored in the form of a site file. Additional information regarding the machine tool is also defined such as spindle limitations, feed units, axis travel limits, workcell related comments, etc. Workcells can be saved to disk to be used in other operations or other manufacturing models. See the Additional Information section of this document for links regarding setup of the NC Machine setup. Copyright 2002 by PTC 6 PTC Technical Support

7 Fixtures Fixtures are defined in the Operation Setup dialog window. Fixtures are parts or assemblies that help orient and hold the workpiece during a manufacturing operation. In Pro/NC, Fixtures help to define tool paths such that the tool will not collide with positioning or fixturing equipment on the NC machine. Fixtures can be created and saved in Part or Assembly mode, prior to the manufacturing model creation, and then retrieved into manufacturing mode during fixture setup. They are assembled into the manufacturing model using standard component assembly procedures. Creating the fixture in Assembly mode is advantageous because fixtures can be created as needed, during the intermediate process steps, by referencing the workpiece., Fixtures can also be created from scratch within the Fixture Setup dialog or they can be retrieved from a library of existing models. The Pro/ENGINEER Tooling Library is an example of a library containing fixture and tooling models. See the Additional Information section of this document for links regarding Fixtures and Fixture Setup. Tooling Tooling refers to the cutting tools used to remove material. Cutting tools consist of three different types, Parameter, Sketched, and Solid. Parameter tools are typically defined within the manufacturing model in the Tools Setup dialog window. Parameter tools are created by entering values for predefined parameters that describe the tool type and the tool shape. Parameter tools can be saved to disk to be later used in other manufacturing models or other workcells. Sketched tools are also defined in the Tools Setup dialog but instead of defining the tool shape by entering numerical values, a sketch of the tool is created. Sketched tools are only used in Trajectory type sequences. Solid tools are created outside of the manufacturing module. Solid tools can be either a single part or consist of multiple components in an assembly. Solid tool models must include user-defined parameters that will be used by Pro/NC for correct tool path generation. Once a solid tool is created, it can be retrieved into the Tools Setup dialog. See the Additional Information section of this document for links regarding tooling setup. Copyright 2002 by PTC 7 PTC Technical Support

8 Defaults Within Pro/NC, a Site file is created to specify the default parameters to be used in NC Sequences and tool paths. Sites can be created for the different NC sequence types such as Mill, Turn, Holemaking, WEDM, etc. Parameters are modifiable values, which control the tool motions during NC sequences. Some parameters are common to all or the majority of sequences. For these commonly used parameters, the Sites enable the user to automatically define these values for newly created sequences. In addition, relations can be used in Sites to drive NC sequence parameter values. See the Additional Information section of this document for links regarding Site setup. PPRINTS Operator Messages PPRINTS are used to output information about the manufacturing model to the CL files. When Post Processing a CL file, the PPRINTS are passed to the G- code file for the operator to view on the machine controller display (if applicable). Information output to the CL file from PPRINTS is typically used by the machine operator for tasks such as part and fixture setup and tool setup. In addition, PPRINTS can be used to pass special instructions, and general tool path information to the CL file. See the Additional Information section of this document for links regarding PPRINT usage. Copyright 2002 by PTC 8 PTC Technical Support

9 Procedure 1.1 Creation of the Manufacturing Model The first step in creating any new Pro/NC Model is to select File, New from the drop down menus along the top of the main model window. The New dialog window (in Figure 3 below) opens and selecting Manufacturing populates the Sub-type section with the various manufacturing options. The valid options for Pro/NC are NC Assembly and NC Part, which are defined in the Fundamentals section above and in the Glossary. Select NC Assembly and enter an appropriate name for the new manufacturing model and pick the OK button. In this example, the manufacturing model is named GEAR_HOUSING. Figure 3 - New Model Creation Dialog Next, from the Menu Manager, select MFG Model, Assemble, Ref Model. When the Open dialog window appears, highlight the Pro/ENGINEER model that is to be used as the reference part and pick the Open button. If a workpiece has been previously created, select Assemble from the menu manager. Otherwise, select Create to define a new model to be used as the workpiece. For this example, the Assemble option is used. After the workpiece has been assembled, using standard assembly procedures, the model will look like Figure 4 below. Copyright 2002 by PTC 9 PTC Technical Support

10 Figure 4 - Manufacturing Model Quick Tip Two methods can be used to better view manufacturing models when using a workpiece. The two methods include: 1.) creating a component display 2.) assigning color and appearance to a component. For the model in this example (Figure 4 above), a component display was created to show the workpiece in wireframe while the reference model is shown as solid. To do this, select View from the main drop down menus and then select Model Setup, Component Display. From the Comp Display menu select Create, enter a descriptive name, Wireframe, Pick Mdl, and then pick the workpiece from the model window. Select Done from the Edit Display menu and Done/Return from the Comp Display menu. To change back to the original display with a solid workpiece, select View, Model Setup, Component Display, Set Current, Master Rep, Ok, Done/Return. To assign color and appearance to a component, first select View, Model Setup, Color and Appearance In the Appearances dialog select Modify From Model and then pick any of the green surfaces of the workpiece. Select the Advanced tab and set the Transparency as desired (typically between 50 and 85). Click OK, Close. In shaded mode the manufacturing model appears as shown in Figure 5 below. Copyright 2002 by PTC 10 PTC Technical Support

11 Figure 5 - Workpiece Appearance Set to Be Translucent Another method used to clear up the model display is to Right Mouse click on the workpiece in the Model Tree and select Hide. This will completely blank the workpiece. To show the workpiece after it has been hidden, Right Mouse click on it again in the model Tree and select Unhide. 1.2 Creation of an Operation After the manufacturing model is created, the next step is to define an operation. From the Manufacture menu, select Mfg Setup to open the Operation Setup dialog window as seen in Figure 6 below. The default name for the operation is OP010 but can be modified to be more descriptive. In the Operation Setup dialog window, red arrows appear next to the items that are required. Copyright 2002 by PTC 11 PTC Technical Support

12 Figure 6 - Operation Setup Dialog 1.3 Creation of an NC Machine The first required option in the Operation Setup dialog window is the NC Machine. Define the NC Machine or Workcell to be used for the operation by selecting the button. The Machine Tool Setup dialog opens as seen in Figure 7 below. In this dialog window, users can define the type of workcell, number of axes, post processor used to generate g-code files, tooling, axes limits, etc. For this example, the machine name has been changed from the default of MACH01to FADAL. A 3-axis Mill is defined. All other options in this dialog are optional. Copyright 2002 by PTC 12 PTC Technical Support

13 Figure 7 - Machine Tool Setup Dialog Select on the various tabs in the Machine Tool Setup dialog window to further define the NC Machine. Near the bottom of the dialog window is the section containing the Cutter Compensation options. To expand this section, pick on the blue right facing arrow next to the words Cutter Compensation. After all of the desired options have been defined, the workcell can be saved for future use in a different manufacturing model. When a workcell is saved, a.gph file, with the name of the workcell, is written to the directory specified by the configuration option pro_mf_workcell_dir. If this config option has not been set, the workcell file (fadal.gph in this example) will be saved to the current working directory. When a workcell is saved, any tools and parameter defaults (site) defined in the workcell are also saved in the.gph file. In contrast, PPRINTS defined in the workcell are not saved with the.gph file but can be retrieved into new workcells. Workcells, that have been saved, can be retrieved by selecting File, Open, in the Machine Tool Setup dialog or by picking the associated button. Since the tools and defaults are saved within the.gph file and the PPRINTS can be read into new workcells, users save a great deal of time (and in turn, money) when retrieving workcells into new operations. Once the NC Machine has been completely defined, pick OK to return to the Operation Setup dialog. Copyright 2002 by PTC 13 PTC Technical Support

14 For a reference with descriptions of the options in the Machine Tool Setup dialog, see the Additional Information section of this document Tooling Setup The cutting tools used in NC sequences can be defined using several different methods in Pro/NC. The first method is to select the Cutting Tools tab in the Machine Tool Setup dialog box when the NC machine is specified. The Machine Tool Setup dialog box can also be accessed by selecting, Mfg Setup, Workcell. In addition, selecting Mfg Setup, Tooling from the Menu Manager, will cause the Tools Setup dialog to open. If the icon along the top of the main Pro/ENGINEER model window is selected, tools can be defined for the active workcell. The final method is to define the tool to be used during the NC sequence creation. The Tools Setup dialog box is shown in Figure 8 below. Copyright 2002 by PTC 14 PTC Technical Support

15 Figure 8 - Tools Setup Dialog With the File menu option and associated buttons at the top of the Tools Setup dialog, new tools can be created from scratch, solid tools can be imported, tool parameters can be retrieved, and tools can be saved. When a tool is saved, the tool parameters are written to a text file called <name>.tpm, where <name> is the tool Name or toolid. This text file is saved in the directory defined by the pro_mf_tprm_dir configuration option. If the cutting data has been supplied, that is, the speeds and feeds for the Copyright 2002 by PTC 15 PTC Technical Support

16 tool, this data is stored in a <name>.tpm file in the appropriate Materials subdirectory. If the pro_mf_tprm_dir configuration option has not been set, the.tpm files will be saved to the current working directory. The Edit menu option enables the user to delete tools from the tool list, edit the tool comments in the tool list, or create a new, sketched tool. Note: When defining a tool during the creation of an NC sequence, the Sketch option will only be available for Trajectory type sequences. The View menu provides access to the information specific to each tool such as the tool parameters and sequences in which the tool is used. The tool Name, Type, Material, and Units can be defined for each tool. The tool Type is important because the tool type is specific to the sequence type. For example, a turning tool cannot be used in a milling sequence. The Material option is used to define the material the tool is made of, such as Cobalt or Carbide, and is only for information purposes. In other words,the CL output is not affected by the Material option value. The tool Units value will default to the manufacturing model units but the Units value is not required to be the same as the units for the model Geometry Tab The parameters on the Geometry tab are used to determine the dimensional shape of the tool. Parameters that are required are populated with default values. These dimension values are used in calculating the tool path and material removed, and should accurately reflect the actual tool dimensions and length units. The actual parameter names in this category depend on the tool type Settings Tab The Settings tab contains the text boxes for specifying the tool table elements and various optional parameters that define tool properties other than geometry. The options include, the tool number or pocket number, tool offsets, gauge lengths (for turning tools only), tool comments and the Long Tool option. The Long Tool option is used if the tool is too long to retract to the Rotation Clearance level during 4-axis machining. If the tool is marked as long, the tip of the tool moves to the Safe Rotary Point (specified in the Operation Setup dialog box) during table rotations. Copyright 2002 by PTC 16 PTC Technical Support

17 Speeds & Feeds Tab The Speeds & Feeds tabbed page lets the user supply cutting data (feed, speed, axial and radial depths) for roughing and finishing with this tool, based on the stock material type and condition. Note: In order to be able to specify the cutting data for a tool, you have to first set up the Material directory structure. See Setting Up A Materials Directory Structure below in section BOM Tab The BOM tabbed page provides information about the Bill of Materials for the tool. When you retrieve a solid tool model, the system automatically includes all the parts and assemblies used in the tool model into the Bill of Materials (BOM) for the tool. If the tool model is used By Reference, the tool BOM information is read-only. If you are using the tool model By Copy, you can edit the part names, if needed, or change the type; you can also add or remove the BOM components. For all other types of tools, you can provide the BOM information by typing the names of the components and specifying their type and quantity Setting Up A Materials Directory Structure In order to be able to specify the Stock Material for an Operation, import tools, retrieve tool parameters, or specify the cutting data for a tool, a Materials directory structure must be defined. Pro/NC stores all the cutting tool data in a Tooling directory, which is specified by using the pro_mf_tprm_dir configuration option. The user determines the name of this directory. In the GEAR_HOUSING example, this configuration option was set as follows: pro_mf_tprm_dir D:\ptc\tooling Pro/NC then places all the tool parameter files (.tpm files) in the D:\ptc\tooing directory. The directory structure can further be defined to differentiate between inch tools and metric tools. When inch tools are being used, the config option is set to the corresponding directory. The config option is modified for the use of metric tools as in the example below. For inch tools pro_mf_tprm_dir D:\ptc\tooling\inch_tools For metric tools pro_mf_tprm_dir D:\ptc\tooling\metric_tools Copyright 2002 by PTC 17 PTC Technical Support

18 To set up the material directory structure, create a subdirectory called materials in your Tooling directory. The directory name must be spelled exactly as shown. Under the materials directory, create subdirectories corresponding to commonly used stock materials and conditions. For example, subdirectories such as aluminum, copper, stainless-hard, etc can be created. The directory structure created under D:\ptc for this example is shown below in Figure 9. Figure 9 - Materials Directory Structure When defining the Stock Material in an operation, the system lists the available material subdirectories from which the user can choose. See Figure 10. Copyright 2002 by PTC 18 PTC Technical Support

19 Figure 10 - Operation Setup Dialog with Materials Defined In addition, when a cutting tool is defined the Stock Material option on the Settings tab will also list the available material subdirectories from which the user can choose. See Figure 11. Copyright 2002 by PTC 19 PTC Technical Support

20 Figure 11 - Tools Setup Dialog with Materials Defined After the materials directory structure has been set up, tools that include cutting data can be created and stored in an organized way. When you save the cutting tool data, the system stores two files. The tool geometry parameters are stored in a.tpm file, with the same name as the tool, in the Tooling directory. The system also creates another.tpm file, with the same file name, containing the feeds and speeds data, in the appropriate material Copyright 2002 by PTC 20 PTC Technical Support

21 subdirectory. This feeds and speeds data can be referenced to specify the manufacturing parameter values using relations. Note: If you do not use the pro_mf_tprm_dir configuration option, the system uses the current working directory as the Tooling directory. To retrieve saved tool parameters, use the File, Open Parameter File option and select the.tpm file associated with the tool to be used. Once the parameter values have been imported, the cutting data can be determined. To do this, go to the Settings tab and specify the Application (Roughing or Finishing) and the Stock Material. If a tool with the current name has been previously stored, the Read DB button can be picked to populate the Cutting Data values. If the tools name is not in the tooling directory structure for the Application and Stock Material defined, the cutting data can be entered and the tool saved. Saving the tool will add.tpm files to the corresponding locations in the tooling directory. For Example, to create a 2.25 inch High Speed Steel (HSS) flat end mill for machining aluminum and stainless steel, the following steps should be taken. Note: The tool does not currently exist in the Tooling directory. 1. Open the Tooling Setup dialog box using one of the methods described in section 3.1 (Tooling Setup) above. 2. In the Tooling Setup dialog, select the button to create a new tool or File, New. 3. Type in the Name of the tool, FLT2250 in this example, keep the default Type as Milling and enter HSS for the Material. 4. Fill in the values on the Geometry tab as shown Figure 12 below and Apply the changes. Copyright 2002 by PTC 21 PTC Technical Support

22 Figure 12 - Tools Setup Dialog with Tool Parameters Defined 5. Next, enter the values for Rouging in Aluminum on the Speeds_Feeds tab as shown in Figure 13 below. Copyright 2002 by PTC 22 PTC Technical Support

23 Figure 13 - Cutting Data for Roughing Aluminum 6. Change the Application to Finishing and enter values for Finishing in Aluminum. 7. Now change the Stock Material to Stainless-Hard and enter the values for Roughing and Finishing as shown in Figures 14 and 15. Figure 14 - Cutting Data for Roughing Stainless Steel Copyright 2002 by PTC 23 PTC Technical Support

24 Figure 15 - Cutting Data for Finishing Stainless Steel 8. Save the tool by highlighting the tool in the tool list and selecting File, Save Tool or the associated Save button. One.tpm file for this new tool is stored in the directory specified by the pro_mf_tprm_dir config option (i.e. D:\ptc\tooling\inch_tools). Two additional.tpm files are saved in the corresponding material directories (D:\ptc\tooling\inch_tools\materials\ALUMINUM and D:\ptc\tooling\inch_tools\materials\STAINLESS-HARD). The resulting.tpm files are shown in Figures 16 thru 18 below. Figure 16 - Parameters As Listed in the.tpm File Copyright 2002 by PTC 24 PTC Technical Support

25 Figure 17 - Cutting Data for Aluminum As Listed in the.tpm File Figure 18 - Cutting Data for Stainless Steel As Listed in the.tpm File Note: The.tpm files are text files that can be modified in any text editor PPRINT Operator Comments On the right side of the Output tab is the PPRINT button. Selecting this button allows the user to: 1.) Create a new set of PPRINTs 2.) Modify any PPRINTs currently assigned to the workcell 3.) Retrieve previously saved PPRINTs from disk 4.) Save currently assigned PPRINTs to disk or 5.) Show, in an information window, the current workcell PPRINTs. Selecting either the Create or Modify options opens the Acitvate PPRINT dialog as seen in Figure 19 below. If Save is selected, a.ppr text file will be written to the current working directory. Retrieve allows the user to read in PPRINT options from a previously saved.ppr file. Copyright 2002 by PTC 25 PTC Technical Support

26 Note: The directory specified by the pro_mf_param_dir config option does not affect where the.ppr file is saved. The.ppr is always saved to the current working directory. On the other hand, the system will retrieve.ppr files from the pro_mf_param_dir directory if this option is set. Figure 19 - Activate PPRINT Dialog for PPRINT Definition To include a PPRINT item in the CL file, highlight the item in the table and pick the Yes button. Note: Multiple items can be highlighted before picking the Yes button. Comments can be entered for each PPRINT item/option to provide additional information, instruction, or clarification. PPRINT comments cannot consist of more than 69 characters. Users need to be aware that comments entered for PPRINT items are separate from the comments defined for operations, sequences, tools, workcells, etc. An example of a CL file before PPRINTs have been defined is shown below in Figure 20. Copyright 2002 by PTC 26 PTC Technical Support

27 Figure 20 CL File Prior to PPRINT Definition In the GEAR_HOUSING example, the PPRINT options are set for the part name, operation, tool table, and sequence as shown in Figure 21 below. Copyright 2002 by PTC 27 PTC Technical Support

28 Figure 21 - PPRINT Definition for GEAR_HOUSING With the PPRINT options set, the resulting CL file will include those PPRINT items marked with Yes as well as any comments input. In Figure 22, the PPRINT output has been set to bold text. Notice the presence of both the operation comments defined in the operation as well as the comments entered for the OPERATION_COMMENTS PPRINT option. Copyright 2002 by PTC 28 PTC Technical Support

29 Figure 22 - CL File with PPRINT Output Defaults Site Files NC sequences, whether Milling, Turning, Holemaking, or WEDM have common parameters that must be defined. One way to automate the definition of these parameters is to create a what is called a Site in Pro/NC. Once a Site has been created, it can be used to specify parameters for NC sequences. If a site has been defined and is active in the model, the values of sequence parameters driven by the site will be enclosed in parenthesis. For example: STEP_DEPTH (.125) A site can be saved for use in other manufacturing models or with other workcells. To save a site select the Save option in the Site Setup menu. When a site is saved, a.sit file, with the same name as the site, is written to either the working directory or the directory specified by the pro_mf_param_dir configuration option, if the option is set. To use a Copyright 2002 by PTC 29 PTC Technical Support

30 previously saved site in another model or workcell, select Retrieve from the Site Setup menu. Although several site files can be used in one workcell, only one site can be active at a time. To toggle between active sites, use the Activate option from the Site Setup menu. Note: The.sit files are text files that can be modified in any text editor Site Creation To create a site, from the Menu Manager, select Mfg Setup, Param Setup, Site, Create. At the prompt, enter a name for the newly created site. Next, select a site type that reflects the type of sequences with which the site will be used. The Site Tree dialog window (in Figure 27) opens enabling the user to input parameter values, to be used as defaults, when creating NC sequences. Figure 27 - Site Tree Dialog Site Settings In the Site Tree dialog, settings for the individual parameters can be specified. The Default Value column is used to enter values that will be used as the defaults when creating an NC sequence. The Set Up Visible column will determine if the sequence parameter is listed in the parameter tree when creating or redefining a sequence. (For some parameters that are not used, the value in this column would be set to NO.) The Info Visible column specifies if the parameter should be listed when Manufacturing Info is Copyright 2002 by PTC 30 PTC Technical Support

31 displayed. The Inherit column is used to specify if the parameter value from the site is passed to the NC sequence. If the Inherit column is set to NO, the parameter value in the NC sequence parameter tree will not include parenthesis () and will be set to the system default Using Relations in Sites Sites become very powerful with the introduction of relations. Relations can be used to drive NC sequence parameters depending on the tool being used. For example, a user may decide the PLUNGE_FEED parameter value should always be two (2) times the CUT_FEED. For the value of the PLUNGE_FEED parameter, the user would enter =cut_feed*2. If the CUT_FEED parameter value is 5.75, the PLUNGE_FEED value will be 11.5 (5.75 * 2). In addition, tool parameters and cutting data can be referenced in the site using relations. For example, the TOOL_AXIAL_DEPTH parameter value, for the tool being used, is 1.08 (see Figure 21 above). For the value of the STEP_DEPTH parameter in the site, enter =TOOL_ROUGH_AXIAL_DEPTH. The STEP_DEPTH for the sequence will be For STEP_OVER, using the same tool the parameter value in the site should be =TOOL_ROUGH_RADIAL_DEPTH. If the application is FINISHING instead of ROUGHING, substitute 'FINISH' for 'ROUGH' in the above parameters. See the Additional Information section of this document for links regarding the use of cutting data parameters in sites. Copyright 2002 by PTC 31 PTC Technical Support

32 1.4 Creation of a Fixture Fixtures can be defined before or after the NC Machine is defined. By default, Pro/NC creates an empty fixture named FSETP0 for each operation. This default fixture can be redefined by selecting the button, which will open the Fixture Setup dialog as seen in Figure 23 below. In the Operation Setup dialog, the button is used to create a new fixture and the button is used to delete and existing fixture. In the Fixture Setup dialog, the button is used to create a new component of the fixture within the manufacturing model. The button is used to redefine the assembly constraints of a fixture component. Previously created components (parts or assemblies) can be added or removed from the fixture with the buttons respectively. The buttons control the fixture component display within the manufacturing model. Once a fixture is defined in a model, the setup can be copied to another fixture by selecting File, Copy or by selecting the associated button. Figure 23 - Fixture Setup Dialog As seen in the figure above, a vice assembly has been added to the fixture setup and is currently being displayed. The resulting manufacturing model is shown below in Figure 24. Copyright 2002 by PTC 32 PTC Technical Support

33 Figure Manufacturing Model with Fixture Included Quick Tip Included in the fixture models could be items such as a safe retract point or a home location. In addition, a good practice is to use standard fixtures typically used on the NC Machine Center. Cosmetic features can be very useful for simplifying key elements, features, and orientations of fixtures. For example, label the indexable orientations (such as 0, 90, 180, etc.) and safe retract zones on fixtures with Cosmetic features. Figure 25 below shows an example of a fixture labeled with cosmetic sketch features. Copyright 2002 by PTC 33 PTC Technical Support

34 Figure 25 - Cosmetic Sketch Features to Label Orientation See the Additional Information section of this document for links regarding fixture setup. Copyright 2002 by PTC 34 PTC Technical Support

35 1.5 Defining Machine Zero The Machine Zero option allows the user to define a location in the manufacturing model that represents the zero position for the NC machine tool. Machine Zero in Pro/NC is synonymous with Program Zero, Part Zero or Zero Datum. Selecting the selection arrow enables the user to define a coordinate system to be the Machine Zero. The axes of the coordinate system selected (or created) in the manufacturing model will correspond to the axes of motion on the NC Machine Center. The Machine Zero coordinate system can reside in any component within the manufacturing model. As indicated by the red arrow, the Machine Zero is a required option. In the GEAR_HOUSING example, an assembly level coordinate system was created at the top surface of the reference model. The coordinate system was then renamed to MACH_ZERO by selecting Setup, Name, Feature. The MACH_ZERO coordinate system is shown in red in Figure 26 below. Figure 26 - Machine Zero Shown In Red 1.6 Defining Stock Material The Operation Setup dialog box contains other useful options that are not required for creating sequences. The Stock Material option enables the user to define the material type of the workpiece. Only after creating the required Copyright 2002 by PTC 35 PTC Technical Support

36 directory structure will options other than Unspecified be available for selection. Details for creating the required materials directory structure are included in the Setting Up A Materials Directory Structure section (1.3.2) above. See the Additional Information section of this document for information regarding the options in the Operation Setup dialog box that have not been discussed. Copyright 2002 by PTC 36 PTC Technical Support

37 Review Taking the time to set up Pro/NC correctly can enable you, the user, to save considerable time and effort in future NC sequence definition. The topics discussed above will help to more efficiently define tool paths in Pro/NC. Efficient tool path definition begins with the creation of the Manufacturing Model. The manufacturing model will include at least one reference part and may contain a workpiece(s) and additional fixture components. Once the components have been assembled to create the manufacturing model, an Operation must be created. Operations are a series of NC sequences performed at a particular workcell and using a particular coordinate system for cutter location (CL) data output. As part of the Operation setup, the NC Machine is specified and fixtures are assembled. In addition, the Machine Zero is determined, the Stock Material is specified, and other information such as comments and From/Home locations are set. The NC Machine is a feature that defines the machine tool attributes such as, the machine name, machine type, number of axes, associated tools, parameters, etc. The NC machine is often referred to as a Workcell in Pro/NC and in the Help documentation. During the NC Machine definition, the user can designate default values for settings related to the tool path creation. These default settings are stored in the form of a site file. In addition, operator messages can be output to the CL file and in turn to the G-code with the use of PPRINTs. Furthermore additional information regarding the machine tool can be defined such as spindle limitations, feed units, axis travel limits, workcell related comments, etc. Workcells or NC Machines are saved to disk for future use in other operations or manufacturing models. In Pro/NC Fixtures help to define tools paths such that the tool will not collide with or gouge positioning and fixturing equipment on the NC machine tool. Fixtures are defined in the Operation Setup dialog window where they can either be created from scratch or retrieved from disk. Fixtures can be turned on or off in the manufacturing model and can be reused in operations within the manufacturing model. The Machine Zero option allows the user to define a location in the manufacturing model that represents the zero position for the NC machine tool. Tooling refers to the cutting tools used to remove material. Cutting tools consist of three different types, those types being Parameter, Sketched, and Solid. Parameter tools are defined by entering values for predefined parameters that describe the tool type and the tool shape. Sketched tools are only used in Trajectory type sequences and require a sketch of the tool profile. Solid tools are created outside of the manufacturing module and can be either a single part or consist of multiple components in an assembly. Copyright 2002 by PTC 37 PTC Technical Support

38 In order to be able to specify the Stock Material for an Operation, import tools, retrieve tool parameters, or specify the cutting data for a tool, a Materials directory structure must be defined. The directory structure can further be defined to differentiate between tool types such as inch and metric tools. One way to automate the defining of sequence parameters is to create a Site. Once a Site has been created, it can be used to automatically specify parameters for NC sequences. Site files can be saved for use in other manufacturing models or with other workcells. Sites become more useful with the introduction of relations. Relations are used to drive NC sequence parameters based on tool parameters and cutting data or other sequence parameters. Copyright 2002 by PTC 38 PTC Technical Support

39 Additional Information Fixtures Suggested Technique for Defining a Fixture Setup in a Manufacturing Model at Defining A Coordinate System In A Fixture As the Machine Zero Coordinate System In the Release 2001 Operation Dialog Window. The Fixture Setup Dialog Box About Fixtures To Activate a Fixture Setup Material Directory To Set Up the Material Directory Structure Example: Setting Up the Material Directory Structure NC Machines Machine Tool Settings To Create a Machine Tool (Workcell) Workcell Types Operations About Operations To Create an Operation Information regarding the Operation Setup dialog Copyright 2002 by PTC 39 PTC Technical Support

40 The Operation Setup Dialog Box How Can Sequences or Operations in One Manufacturing Model Be Copied to Another Manufacturing Model? PPRINTS To Set Up a PPRINT Table The PPRINT Table Information Regarding the Saving and Retrieving of PPRINT Table (.ppr) files. Simplified Representations About Simplified Representations About Creating Simplified Representations Suggested Technique for Managing the Display of Assemblies Using Simplified Representations About On-Demand Simplified Representations To Create Simplified Representations Using Definition Rules Suggested Technique for Using Rules to Create Simplified Representations To Create a Simplified Representation Sites Suggested Technique for Using Relations in Site Files to Control Sequence Parameters at Using Site Parameters To Automatically Drive Spindle Speed, Cut Feed, Step Depth, and Step Over From Tool Cutting Data. Copyright 2002 by PTC 40 PTC Technical Support

41 Associating a Site with a Workcell Using the Cutting Data Supplied for the Tool Tools About the Tool Setup Dialog Box Suggested Technique for Using a Solid Model as a Turning Tool Suggested Technique for Using the Tools Setup Dialog to Create Tools and Setup Workcell Tool Tables. To Retrieve Tool Parameters To Use a Tool Model To Specify the Cutting Data for the Tool About Elements of Tool Setup To Set Up Tools in Advance Sketching the Tools for Trajectory Milling Using the Cutting Data Supplied for the Tool Copyright 2002 by PTC 41 PTC Technical Support

42 Glossary CL File File containing data that describes the location of the cutter control point during an NC sequence. Fixture A part or assembly that helps orient and hold the workpiece during a manufacturing operation. Machine Zero Sometimes referred to as the Machine Coordinate system. Acts as the origin for all CL data. This coordinate system is specified at the time of operation setup using the Machine Zero option in the Operation Setup dialog window. All sequences created within a certain operation will use the same Machine Zero coordinate system. NC Assembly A manufacturing model sub-type used for machining more than one reference part or an assembly of reference parts. One, or many workpieces may be used in the manufacturing model or no workpieces at all. The NC Assembly sub-type also allows for the use of both regular and manufacturing assemblies that have been previously created. NC Machine A feature that defines the machine tool attributes such as the machine name, machine type, number of axes, associated tools, parameters, etc. The NC Machine is sometimes referred to as a Workcell. NC Part A manufacturing model sub-type used for machining one or more parts with only one workpiece. The NC Part sub-type requires a workpiece to be either created or assembled in the manufacturing model. Manufacturing features created during tool path development will be placed into the workpiece model. NC Sequence Is a feature within Pro/NC used to create a toolpath. It contains all the information and parameters needed to construct the required toolpath. Operation A series of NC sequences performed at a particular workcell and using a particular coordinate system for CL data output. Parameter A modifiable value, which controls the tool motions during NC sequences. Parameters are set when defining the NC Sequence or in advance using a site. PPRINT Information from the manufacturing model passed to the CL file and in turn to the G-code. Information output to the CL file from PPRINTS is typically used by the machine operator for tasks such as part and fixture setup and tool setup. In addition, PPRINTS can be used to pass special instructions, and general tool path information to the CL file and G-code. Reference Model The Pro/ENGNIEER design model representing the finished product. Features, surfaces and edges are all selected on the design model as references for tool paths. When the design/reference part is modified, all associated manufacturing operations are updated to reflect the change. Copyright 2002 by PTC 42 PTC Technical Support

43 Relation User defined equations written between symbolic dimensions and parameters. Relations capture design relationships within features or parts, or among assembly components thereby allowing users to control the effects of modifications on models. Simplified Representation Model representations used to improve regeneration, retrieval and display times, enabling the user to work more efficiently. Simplified representations can be defined to exclude or include features and components based on specified criteria such as name, size, etc. Site Predefined parameter values associated with the sequence types such as milling, turning, holemaking, and WEDM. Sites are used to quickly and consistently define parameter values for sequences. Tool - The cutting tools used to remove material such as end mills, drills, boring bars, etc. Cutting tools consist of three different types, Parameter, Sketched, and Solid. Workcell See NC Machine above. Workpiece The piece of material upon which manufacturing operations are performed until the workpiece resembles the reference model. Copyright 2002 by PTC 43 PTC Technical Support

44 Command Listing Create a Manufacturing Model: #File #New #Manufacturing #NC Assembly #OK Assemble a Reference Model Component: #Mfg Model #Assemble #Ref Model Assemble a Workpiece Model Component: #Mfg Model #Assemble #Workpiece Create, Modify or Redefine a Simplified Representation: #Mfg Model #Simplfd Rep Create Delete or Modify an Operation: #Mfg Setup #Operation Create, Delete or Modify a Workcell/ NC Machine: #Mfg Setup #Workcell Create, Delete or Modify a Fixture: #Mfg Setup #Operation, pick appropriate button Create, Delete or Modify Tools: 1.) #Mfg Setup #Workcell #Cutting Tools pick Tool Manager button 2.) #Mfg Setup #Tooling, pick the desired workcell. 3.) Select the icon along the top of the model window. (Used to setup tools for the active operation) Create, Delete, Modify Save, or Retrieve Defaults (Site): #Mfg Setup #Param Setup #Site Copyright 2002 by PTC 44 PTC Technical Support

45 Specify Defaults (Site) for a Workcell: #Mfg Setup #Workcell #Defaults, pick the site, #Done Sel #Done Activate a Site: #Mfg Setup #Param Setup #Site #Activate, pick the site, #Done Sel #Done #Done/Return Create, Modify, Retrieve, or Save PPRINT Settings: 1.) #Mfg Setup #Workcell #PPRINT 2.) #Mfg Setup #CL Setup #PPRINT Create a Wireframe Component Display for the Workpiece: #View #Model Setup #Component Display #Create, enter a name, #Wireframe #Pick Mdl #Pick, pick the workpiece from the model window, #Done Sel #Done #Done/Return Setup a Translucent Appearance for the Workpiece: #View #Model Setup #Color and Appearance #Modify From Model, pick the workpiece from the model window, #Advanced, move the slider bar in the Transparency section Hide the Workpiece: Right Mouse click on the workpiece in the model tree and select #Hide Create Cosmetic Features for Fixture Labeling: Open the fixture model. #Feature #Create #Cosmetic #Sketch etc. Copyright 2002 by PTC 45 PTC Technical Support