Machine Tool 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 is automatically incremented by Creo NC. You can type any name.
When you save the machine tool data on disk, Creo NC uses the machine name as a filename with the .gph extension.
• Type—The machine type can be Mill, Lathe, Mill-Turn, or Wire EDM.
• 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.
• Milling Axes—Depending on the machine type, can be:
◦ For Mill—3 Axis (default), 4 Axis, or 5 Axis.
◦ For Lathe—1 Turret (default) or 2 Turrets.
◦ For Mill-Turn—2 Axis, 3 Axis, 4 Axis, or 5 Axis (default).
◦ For Wire EDM—2 Axis (default) or 4 Axis.
Apart from the Work Centre types, the following options are also available:
◦ User-Defined Work Center—Enables you to retrieve a work center along with its parameters.
◦ Save Work Center—Enables you to save the current work center, along with its parameters.
• Number of Heads
—Specify whether the work center has one, two, three, or four heads. When the work center is Lathe, the option Number of Turrets is available.
• Number of Spindles
—Specify whether the work center has one or two spindles. . Two spindles are available for 3-, 4-, and 5-Axis Mill-Turn work centers and Lathe work centers .By default, a single spindle is available, which is the main spindle. Specifying a sub spindle is optional.
• Enable probing—Allows CMM step definition within an NC session. You must have the CMM license.
• Swiss turning—Enables you to select a swiss-type turning capability for a machine. The swiss-type toolpaths are governed by the SWISS_TURN parameter.
The following tabs on the Work Center dialog box enable you to specify various parameters of a machine tool.
Output
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 statement in the operation CL data file:
◦ Modal (default)—The LOADTL statement 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.
◦ Not Modal on Position Moves—Outputs the LOADTL statement when the Z-axis orientation changes between adjacent steps.
• 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.
Rotation Section
These multiple Axis Output options become accessible only for a Mill type machine tool when you set Number of Axes to 4 Axis.
• Use Rotation—If this option is not selected (default), all CL data is transformed and output in the coordinates of the Program Zero coordinate system. When you select this option, Creo NC outputs the applicable TRANS and ROTABL commands to specify linear and rotational transformations. Select this option only when indexing to a new table position is desired.
The following options are available when you select Use Rotation.
• Rotation Mode—Available only when Use Rotation is selected. Controls output of ROTABL statements. The values are: Incremental (default) and Absolute. In Absolute mode, zero position is defined by the Program Zero.
• Rotation Direction—Available only when Use Rotate Output is selected. Allows you to specify that rotation is performed in a particular direction (this may occur when there is an obstruction in one rotation direction but not another). The values are:
◦ Shortest (default)—Make the shortest possible move to the new position.
◦ CLW—Always rotate in the clockwise direction.
◦ CCLW—Always rotate in the counterclockwise direction.
• Rotation Axis—Specify the rotation axis: A-Axis or B-Axis (default).
Sub-spindle Section
This section is accessible if you have set up a Mill-Turn or Lathe work center with two spindles.
• Program Zero—The following options are available:
◦ Main Spindle Program Zero—Outputs all steps using the main spindle program zero, irrespective of the spindle used for creating the steps.
◦ Per Spindle Program Zero—Outputs the steps corresponding to the program zero of the spindle used for creating the steps.
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 determines the smallest concave corner radius that can be safely machined, which must be slightly bigger than the tool radius. When Creo NC calculates the tool path for an NC sequence, it checks that the radius of every concave corner being machined is no less than Cutter Diameter/2 + Safe Radius. If a corner does not meet this condition, Creo NC issues an error message. You can either reduce the Safe Radius value, if possible, or use a smaller tool. If your actual cutting tool diameter is greater than the programmed cutting tool diameter, use the Comp. Oversize parameter on the Settings tab of the Tools Setup dialog box. In this case, the smallest safe concave radius is calculated as (Cutter Diameter + Comp.Oversize)/2 + Safe Radius).
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—Creo NC 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.
Tools
• Mill-Turn Section
These options are available for a Mill-Turn type machine tool.
• Head 1,Head 2, Head 3, or Head 4— Click Tools to open the Tool Setup dialog box that enables you set up the cutting tools associated with a machine tool head. For example, if you click Tools for Head 1, the Tools Setup (Head 1) dialog box opens.
• 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.
You can specify the following machining capabilities for Head 1, Head 2, Head 3, and Head 4:
• Milling
—Select to make available milling on a particular head. This is the default selection for Head 1.
• Turning—This is selected by default for all heads for a Mill/Turn workcell.
• Flash Turning Tool
—Specifies whether the turning tool can be rotated 180 degrees in its holder and cut with the same tip in the opposite direction. Available only for 5-axis Mill/Turn workcells.
• Position Turning Tool
—Specifies whether the turning tool can be rotated about the B-axis of the machine tool. Available only for 5-axis Mill/Turn workcells.
• Rotation—Specifies rotation of the turning tool. This option is available only when the Position Turning Tool check box is selected for one or both heads. The TOOL_POSITION_ANGLE parameter determines the tool’s rotational direction.
◦ Standard
—If you select Standard and have set a positive value for the TOOL_POSITION_ANGLE parameter in the NC step, the tool rotates in the counterclockwise direction about the B-axis. A negative value for TOOL_POSITION_ANGLE results in the tool rotating in the clockwise direction.
◦ Reverse
—If you select Reverse and have set a positive value for the TOOL_POSITION_ANGLE parameter in the NC step, the tool rotates in the clockwise direction about the B-axis. A negative value for TOOL_POSITION_ANGLE results in the tool rotating in the counterclockwise direction.
 |
Changing the value for the TOOL_POSITION_ANGLE parameter does not affect the TOOL_ORIENTATION parameter. A positive value for TOOL_ORIENTATION indicates a counterclockwise rotation about the B-axis.
|
If you select the Milling option on a specific head when defining the machine capabilities, commands related to that head appear on the Milling and Turning tabs when creating NC sequences. For example, if you select the Milling option on Head 1 and Head 2 when defining the machine capabilities, Head 1 and Head 2 commands appear on the Milling and Turning tabs when creating Milling NC sequences.
The head that you use while creating a Milling, Turning, or Holemaking sequence is output to the CL file.
If you do not select the Milling option for any of the heads when defining the machine capabilities, milling sequences are not available but turning and drilling sequences will have the selected head options while creating NC sequences.
|
|
When you have a step referencing the workcell, you cannot edit any defined machine capability. In case you try to edit, Creo NC displays an appropriate warning message.
|
Lathe
These options are available for a Lathe type machine tool. For 2-turret Lathe you get separate cutting tool setup buttons for both the turrets.
• Turret 1 and Turret 2— Click Tools to open the Tool Setup dialog box that enables you set up the cutting tools associated with a machine tool head. For example, if you click Tools for Turret 1, the Tools Setup (Head 1) dialog box opens.
Parameters
• 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
|
|
If you have a work center with two spindles, these parameters are available in the Main Spindle and Sub Spindle sections of the Parameters tab.
|
• Rapid Feed Rate—Type the value of the feed rate used for rapid traverse (optional).
• Machine Frequency—Specifies the feed velocity, that is, the rate at which the probe moves when measuring. This field is accessible after you enable CMM probing.
• Defaults—Lets you associate a site with the workcell.
• PPRINT—Opens the PPRINT menu to let you set up your PPRINT options.
• DMIS—Opens the DMIS TEXT menu to let you set up your DMIS Text options. You must have CMM probing enabled.
Assembly
• 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.
• Orientation—(Available only for Lathe or Mill-Turn machine tools.) Specifies the lathe orientation, that is, Horizontal (default) or Vertical. This option defines the default Sketcher orientation when you later create Turning NC sequences in this workcell:
◦ For Horizontal, the z-axis of the NC Sequence coordinate system points horizontally to the right, and the x-axis points vertically upward.
◦ For Vertical, the z axis of the NC Sequence coordinate system points vertically upward, and the x-axis points horizontally to the right.
Travel
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 appears, 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.
Cycles
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.
Properties
• 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 boxor 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.