Work Center Settings
A machine tool or work center is identified by the following elements:
• Name — The machine name identifies the machine tool within the manufacturing process. The default machine names have the format MACH01, MACH02, where the number gets automatically incremented by the system. You can type any name.
When you save the machine tool data on disk, the system uses the machine name as a filename (with the .cel extension.
• Type — The machine type is Mill.
• CNC Control— The controller name (optional).
• Post Processor — The name of the default post-processor associated with the machine. Type the name in the text box.
• ID — Set a post-processor ID from the list. The ID may be from 1 to 99.
• Number of Axes — Can be 3 Axis (default), 4 Axis, or 5 Axis.
• Enable probing — Allows CMM step definition within an NC session. You must have the CMM license.
The following tabs on the Milling Work Center dialog box enable you to specify the following parameters of a machine tool.
The Output tab
Commands Section
• FROM — Specifies how the FROM statement will be output to an operation CL data file:
◦ Do Not Output (default) — No FROM statements are output. If a From point is specified, its location is output as a GOTO statement at positioning feed.
◦ Only at Start — A FROM statement is output at the beginning of the file. It corresponds to the location of the From point, if specified, or to the first location on the tool path for the first machining feature. All other tool paths are added to the operation without a FROM statement.
◦ At Every Tool Path— FROM statements are output at the beginning of each tool path for a machining feature. For the first tool path, this FROM statement corresponds to the location of the operation From point, if specified, or to the first location on the tool path for this machining feature.
• LOADTL — Controls the output of the LOADTL command in the operation CL data file:
◦ Modal (default) — The LOADTL command is output at the beginning of CL data for a feature tool path only if a tool change is needed.
◦ Not Modal — Outputs the LOADTL statement at the beginning of each feature tool path, regardless of whether the tool is the same or changed.
• COOLNT/OFF — Controls the output of the COOLNT/OFF statement.
◦ Output (default) — The COOLNT/OFF statement is output at the end of each feature tool path.
◦ Do Not Output— COOLNT/OFF is output only once, at the end of the file.
• SPINDL/OFF— Controls the output of the SPINDL /OFF statement.
◦ Output(default) — The SPINDL /OFF statement is output at the end of each feature tool path.
◦ Do Not Output — SPINDL /OFF is output only once, at the end of the file.
Cutter Compensation Section
• Output Point
◦ Tool Center — Cutter location (CL) data is output with respect to the tool center.
◦ Tool Edge— Cutter location (CL) data is output with respect to the cutting edge of the tool. If you select this option, type the desired value in the Safe Radius text box. This value represents the smallest concave corner radius that can be safely machined, and must be slightly bigger than the radius (Cutter Diameter/2) of the biggest tool on the machine.
The Adjust Corner drop-down list gives you a choice of corner condition options for convex corners:
▪ Straight— When passing a convex corner, the tool path consists of two straight segments extended until they intersect.
▪ Fillet — When passing a convex corner, the tool path consists of two straight segments connected with an arc.
▪ Automatic — The system adds a fillet corner condition at all the convex corners on the outside contour of the part, and a loop corner condition at all the convex corners on the inside contour of the part.
Probe Compensation Section
This section is accessible after you enable CMM probing.
• Output Point — The following options are available:
◦ Stylus Center — Outputs coordinates into the DMIS files with respect to the coordinates of the probe tip center, that is, the center of the probe stylus sphere.
◦ Contact Point— Outputs coordinates into the DMIS files with respect to the coordinates of the contact point.
The Tools tab
The following options are available:
• Tool Setup— Click to open the Tool Setup dialog box that enables you set up the cutting tools associated with the machine tool. For 4- or 5-axis Mill-Turn machines, you get separate cutting tool setup buttons for Head 1 and Head 2, respectively.
• Probe Setup — Is accessible after you enable CMM probing. It opens the Probe Setup dialog box so you can add a default probe or a probe from the probe library.
• Tool Change Time — Time needed for changing a tool, in seconds (optional). Type the value in the text box, or use the UP and DOWN arrows next to the text box to increase or decrease the value, respectively.
The Parameters tab
• Maximum Speed— Maximum allowable spindle speed for the machine tool (optional). Type the maximum speed value in RPM (revolutions per minute).
• Horsepower— Spindle horsepower (optional).
• Rapid Traverse — Specifies the rapid feed rate units. The values are:
◦ IPM (default) — inches per minute
◦ MMPM— millimeters per minute
◦ FPM — feet per minute
◦ FPR — feet per revolution
◦ IPR— inches per revolution
◦ MMPR— millimeters per revolution
• Rapid Feed Rate — Type the value of the feed rate used for rapid traverse (optional).
• Defaults — Lets you associate a site with the workcell.
• PPRINT — Opens the PPRINT menu to let you set up your PPRINT options.
The Assembly tab
• Machine Assembly — Allows you to specify the machine assembly to be used when displaying tool motion on the machine tool. Use the configuration option pro_mf_workcell_dir to specify the default directory for the machine assembly files. Creo NC locates the machine assembly files in the following order:
◦ Default directory, if set
◦ All first level sub directories of the default directory, if default directory is set
◦ Current directory
To enable motion kinematics, the components of the machine assembly should be connected to each other only using sliders and pins. That is, the relative motions between the components should be defined.
You must name the components of the machine assembly as follows:
◦ Define the absolute origin of the machine assembly using a coordinate system named MACH_ZERO. This coordinate system is used to assemble the manufacturing model.
◦ Define the spindle loading position of the machine assembly using a coordinate system named TOOL_POINT.
◦ Any solid tool model present in the machine assembly should contain a coordinate system named TOOL_POINT. This coordinate system is used to assemble the solid tool model.
You can access a library of basic machine assemblies by searching the PTC Knowledge Database with the keyword Machine Kinematics from the NC Central Page at www.ptc.com.
 |
To clear the selection of the machine assembly, place the mouse pointer in the Machine Assembly field, right-click, and click Remove.
|
• Coordinate System — Allows you to specify the reference coordinate system for the machine assembly. During simulation, this coordinate system is aligned with the MACH_POINT coordinate system defined in the machine assembly. To clear the selection of the coordinate system, right click in this field and click Remove on the context menu that appears.
The Travel tab
Lets you specify the travel limits and the stroke for the machine tool along X-, Y-, and Z-axes: X min, X max, X stroke, Y min, Y max, Y stroke, Z min, Z max, and Z stroke. Specifying these values is optional. Values for the travel limits along the axes should be the actual dimensions that indicate the extent of the machine tool workspace relative to the Program Zero coordinate system.
For example, if a machine tool is 60 inches wide, and the origin of the Program Zero coordinate system is located halfway between the ends, you can specify any of the following as the machine limits:
• X min as –30, X max as 30
• X min as –30 andX stroke as 60
• X max as 30 and X stroke as 60
• X stroke as 60
If you display or otherwise output the CL data for a machining feature that exceeds the limitations of the machine tool where it is defined, the Information Window will appear, listing the values of the limits that have been exceeded and their corresponding actual values.
Similarly, the Status column in the Process Table also indicates machine tool over travel. If a machine tool used in a step or an operation travels over the specified limits, the status of the step or operation in the process table changes to Over Travel or Adjust Oper CSYS.
The Cycles tab
Lets you set up custom cycles for Holemaking. Click Add to add a custom cycle using options on the Customize Cycle dialog box that opens.
The Properties tab
• Name — Displays the name of the work center or workcell.
• Location — Specifies the location of the machine tool.
• Comments — Type the comments associated with the machine tool in the text box or use the following options:
◦ 
— Read in an existing text file containing comments for the work center and replace any current comments.
— Read in an existing text file containing comments for the work center and replace any current comments.◦ 
— Insert the contents of an existing text file of comments for the work center at the cursor location. Preserve any current comments.
— Insert the contents of an existing text file of comments for the work center at the cursor location. Preserve any current comments.◦ 
— Save current comments of the work center in a text file.
— Save current comments of the work center in a text file.◦ 
— Accept the current comments of the work center.
— Accept the current comments of the work center.