Milling Parameters

The following parameters are specific to milling NC sequences. They are listed under a heading corresponding to the name of the branch when you set up the parameters.

For description of the common manufacturing parameters, available for all the NC sequence types, see the topic Common NC Sequence Parameters. For description of parameters specific to Roughing and Reroughing NC sequences, see the topic Milling Parameters Specific to Roughing and Reroughing. Follow the appropriate link under See Also to access these topics.

Note:

Cut Option

SCAN_TYPE

Applicable for Volume, Surface, Face, Pocket, and Plunge milling.

For Volume milling, refers to the way a milling tool scans the horizontal cross-section of a milling volume and avoids islands. The options are:

The following illustration shows the scan types for Volume milling.

image\img00066_shg.gif

  1. TYPE_1

  2. TYPE_SPIRAL

  3. TYPE_2

  4. TYPE_3

  5. TYPE_ONE_DIR

  6. TYPE_1_CONNECT

For Straight Cut Surface milling:

For Isolines Surface milling:

 

For Cut Line Surface milling:

image\img00067_shg.gif

  1. Start cutline (the top surface boundary)

  2. End cutline (the bottom surface boundary)

For Projected Cuts Surface milling, the scan types are the same as for Volume milling (with the exception of TYPE_1_CONNECT and CONSTANT_LOAD). They refer to the way the flat pattern of the tool path is created.

For Swarf milling:

For Face milling:

image\img00068_shg.gif

  1. TYPE_1

  2. TYPE_3

For Pocketing, the scan types are the same as for Volume milling (with the exception of TYPE_1_CONNECT and CONSTANT_LOAD). They refer to the way the tool scans the bottom of the pocket.

For Plunge milling, you can not change the scan type when the tool has Insert_Width smaller than Cutter_Diam/2. For a regular flat tool the following scan types are available:

ROUGH_OPTION

Controls whether a profiling pass occurs during a Volume milling NC sequence. The options are:

Note: A tool path similar to ROUGH_&_CLEAN_UP with TYPE_ONE_DIR can be obtained by using 3-Axis Straight Cut Surface milling with ROUGH_STEP_DEPTH.

The following illustration shows the cutter path depending on the ROUGH_OPTION.

image\img00069_shg.gif

  1. ROUGH_ONLY

  2. PROF_ONLY

  3. Profiling after rough cut

  4. Profiling first

  5. ROUGH_&_PROF

  6. PROF_&_ROUGH

 

image\img00070_shg.gif

  1. ROUGH_&_CLEAN_UP with TYPE_3

  2. ROUGH_&_CLEAN_UP with TYPE_ONE_DIR

The following illustration shows the tool path for ROUGH_&_CLEAN_UP with TYPE_ONE_DIR.

image\img00071_shg.gif

  1. Tool path

  2. STEP_DEPTH

  3. Mill volume walls (side view)

  4. STEP_DEPTH + CUTTER_DIAM/2

 

POCKET_EXTEND

Defines the positioning of the tool when machining the open edges of the planar faces inside a volume (for example, island tops). The values are:

This parameter is used when ROUGH_OPTION is set to POCKETING or FACES_ONLY.

TRIM_TO_WORKPIECE

In Volume milling, if set to FULL_TRIM, confines the milling volume to that inside the workpiece boundaries, in order to avoid air machining. If set to TRIM_TO_TOP (default), trimming is done only in the Z direction.

Note:

 

image\img00072_shg.gif

  1. Milling volume (with offset)

 

In 3-Axis Straight Cut Surface and Face milling, if set to YES (the default is NO), makes the tool machine one zone of the workpiece before going to the next. The actual tool path depends on the SCAN_TYPE parameter value. The following illustration shows Face milling with SCAN_TYPE set to TYPE_ONE_DIR.

 

image\img00073_shg.gif

  1. TRIM_TO_WORKPIECE NO

  2. TRIM_TO_WORKPIECE YES

 

CUT_DIRECTION

For Volume milling, allows you to reverse direction of tool motion within a slice. The values are STANDARD and REVERSE.

For Profile milling, STANDARD (the default) machines selected surfaces from top to bottom, that is, starting with the top slice; REVERSE machines from bottom to top, that is, starting with the lowest slice.

STEPOVER_ADJUST

If set to YES (the default), adjusts the step-over distance (defined by the STEP_OVER and NUMBER_PASSES parameters) to make both the beginning and the end of the cutter path for one pass close to the edges. The adjusted step-over distance does not exceed the original one. If set to NO, the step-over distance will be exactly as defined by the combination of the STEP_OVER and NUMBER_PASSES parameters.

image\img00074_shg.gif

  1. STEPOVER_ADJUST NO

  2. STEPOVER_ADJUST YES

 

CUT_TYPE

Combined with SPINDLE_SENSE, controls where material is relative to the tool when it is removing material during profiling NC sequences or slices; bottom slices, such as in pocket milling, are not affected by this parameter. The options are CLIMB, UPCUT, and ZIG_ZAG. The possible combinations and the resulting tool path are:

Note: CUT_TYPE parameter for Volume milling can be specified when ROUGH_OPTION is specified as ROUGH_&_PROF, PROF_&_ROUGH, or PROF_ONLY or when the SCAN_TYPE is TYPE_SPIRAL.

For Local milling, there is an additional option NONE, which makes the tool move back and forth when cleaning up material.

For Profile milling, the ZIG_ZAG option can be used when profiling open contours. It provides lace-type connection between slices, while CLIMB and UPCUT make the tool retract and rapidly traverse to the beginning of the next slice.

image\img00075_shg.gif

  1. CUT_TYPE CLIMB

  2. CUT_TYPE ZIG_ZAG

For 3-Axis Straight Cut Surface milling, CUT_TYPE, combined with SPINDLE_SENSE and CUT_DIRECTION, controls the start point and direction of machining the surface. The LACE_OPTION parameter must be set to NO.

 

PLUNGE_PREVIOUS

For Volume milling with SCAN_TYPE TYPE_3, determines where the tool plunges when starting to machine a new zone:

FIX_SKIPPED_SLICES

By default (NO), if NC Manufacturing cannot create a slice at a certain Z depth when milling a volume (for example, because of geometry problems), this slice will be skipped and the tool will go to the next slice. If this parameter is set to YES, then, whenever a slice cannot be created, NC Manufacturing will generate the next slice and repeat it at the level of the skipped slice. In other words, if a slice can not be created, the next slice will be repeated twice: at the Z level of the skipped slice and at its own Z level. The system will issue a warning every time a slice cannot be generated.

LACE_OPTION

For Finishing, Straight Cut Surface milling and for Cut Line machining, controls whether the tool retracts at the end of a cutting pass (as shown in the following illustration). If set to NO (which is the default for Straight Cut Surface milling), the tool retracts after each cut, so that all cuts are in the same direction. Other values cause the tool to cut back and forth, and specify the shape of connection between the endpoints of neighboring cuts:

Note: If you set LACE_OPTION to LINE_CONNECT for 3-Axis Straight Cut Surface milling, the system automatically degouges connecting motions and switches to CURVE_CONNECT if LINE_CONNECT causes gouging. In 4- and 5-Axis NC sequences, if LINE_CONNECT causes gouging, the tool will retract. To avoid such retracts, use CURVE_CONNECT.

 

image\img00076_shg.gif

  1. LACE_OPTION   NO

  2. LACE_OPTION   LINE_CONNECT

 

ALLOW_NEG_Z_MOVES

If set to NO, eliminates negative Z moves for 3-Axis Straight Cut Surface milling NC sequences. The default is YES. If you set ALLOW_NEG_Z_MOVES to NO, you have to also set SCAN_TYPE to TYPE_1 and LACE_OPTION to NO. The following illustration shows an example of a tool path with ALLOW_NEG_Z_MOVES set to NO.

image\img00077_shg.gif

 

RETRACT_OPTION

Controls the number and level of retracts in Volume milling, Roughing and Reroughing.

In Volume milling, the values are:

Note: If Approach or Exit path is specified for each slice using Build Cut, the RETRACT_OPTION parameter will be ignored.

In Roughing and Reroughing, the values are:

 

GOUGE_AVOID_OPTION

In Swarf milling, specifies whether the tool will retract to avoid gouging:

 

GOUGE_AVOID_TYPE

For 3-Axis Profiling: TIP_&_SIDES (the default) will make the system detect undercuts when degouging the tool path. If you want to be able to machine an undercut, set GOUGE_AVOID_TYPE to TIP_ONLY.
For 5-Axis Profiling: if set to TIP_&_SIDES, the system degouges with respect to the whole tool (as defined by the tool parameters). The tool will retract if an undercut is detected. The default is TIP_ONLY, in which case the system does not detect undercuts.

Note: GOUGE_AVOID_TYPE setting cannot be changed when modifying parameters. Use Redefine.

 

REMAINDER_SURFACE

Applicable for Straight Cut Surface milling and 3-Axis Isolines and Cut Line Surface milling NC sequences. If it is set to YES (the default is NO), the system will generate a surface representing the leftover material (to be removed by a subsequent Local Mill NC sequence). This surface will belong to the current NC sequence, and will be regenerated upon regenerating the tool path.

Note: The remainder surface will be generated based on the SCALLOP_HGT parameter value.

 

AUTO_SYNCHRONIZE

Applicable for Cut Line Surface milling only. If set to YES (the default), the system will attempt to use edges crossing all the selected cut lines as synch lines. If this is not satisfactory, set AUTO_SYNCHRONIZE to NO and specify the synch lines or synch points manually.

 

AUTO_INNER_CUTLINE

Applicable for Cut Line Surface milling only. If set to YES, the system will attempt to use edges crossing all the specified synch lines as inner cut lines. The default is NO.

 

CUTLINE_TYPE

Applicable for Cut Line Surface milling only. Allows you to select which algorithm the system uses when it calculates cut line distribution. The values are:

 

CUTLINE_EXT_TYPE

Applicable for Cut Line Surface milling only. Specifies how the system handles the case when a cut line does not extend the whole length of the surface selected for machining. The values are:

 

image\img00078_shg.gif

  1. Surface selected for machining

  2. Start cut line

  3. End cut line

  4. CUTLINE_EXT_TYPE   BOUNDARY

  5. CUTLINE_EXT_TYPE   NONE

 

AXIS_DEF_CONTROL

Applicable for 5-Axis Cut Line Surface and Trajectory milling, and for Swarf milling.

For 5-Axis Cut Line Surface milling and Swarf milling, the values are:

For 5-Axis Trajectory milling, this parameter is used for Automatic Cut motions created using the Surfaces command. Another way to specify axis definitons is to use the Axis Control command in the CUTMOTION SETUP menu. The AXIS_DEF_CONTROL parameter specifies the approximation type between the explicit axes definitions. The values are:

 

LEADING_EDGE_MACHINING

If set to YES (the default is NO), ensures that the tool always cuts with the leading edge, even in areas with high curvature, while maintaining contact with the drive surface. Applicable for 5-axis Trajectory milling using Surfaces. Particularly useful in turbine blade machining.

 

USE_VARIABLE_TILT

If set to YES (the default is NO), the tool will tilt to avoid gouging. Available for Swarf milling only.

 

IGNORE_RULINGS

If set to NO (the default), the tool will be parallel to the ruling lines when machining ruled surfaces. If set to YES, the tool will ignore the ruling lines of the ruled surfaces. Available for Swarf milling only.

 

4X_LEAD_RANGE_OPT

If set to YES (the default is NO), the system will attempt to use variable lead angle to avoid gouging. That is, if gouging occurs with the specified 4X_LEAD_ANGLE, the system will try to use another angle in the range between 4X_MIN_LEAD_ANGLE and 4X_MAX_LEAD_ANGLE. Applicable for 4-axis milling only.

 

FOLLOW_TOP_EDGE_3AX

In 3-axis Trajectory milling, allows you to machine the top edge of a boss or hole with a tapered tool (SIDE_ANGLE > 0). If set to YES (the default is NO), the system will automatically calculate the necessary offset in the XY plane for the tool (1) to follow the top edge of the boss (2) or hole with its side, as shown in the following schematic.

 

CUSTOMIZE_AUTO_RETRACT

If set to NO (the default is YES), the tool will not perform the automatic retract when following the default tool path.

 

SLICE_PATH_SCAN

Defines the order of machining multiple passes within multiple step depths (slices). The values are:

 

CONNECTION_TYPE

Controls the intermediate tool retracts for multi-step and multi-pass 3-axis and 2-axis trajectory milling. The values are:

 

MACHINING_ORDER

For Local milling by previous tool, specifies the order of removing the leftover material in the corners and on the surfaces. The values are:

 

SURFACE_CLEANUP

For Local milling by previous tool, specifies whether cleaning up the surfaces is done in a single pass or in step depth increments. The values are:

 

CORNER_CLEANUP

For Local milling by previous tool, specifies how the corners are machined. The values are:

 

RETRACT_TRANSITION

For high-speed Volume milling, as well as for Roughing and Reroughing, specifies how the tool transitions between a vertical retract move and a traverse move (a horizontal move at the retract plane or intermediate traverse plane level), and then between the traverse move and a vertical plunge move. The values are:

 

RETRACT_RADIUS

Specifies the radius of the transition arc (if the RETRACT_TRANSITION parameter is set to ARC_TRANSITION). The default is a dash (-). If you set RETRACT_TRANSITION to ARC_TRANSITION, you have to specify a RETRACT_RADIUS value.

Cut Param

 

STEP_DEPTH

The incremental depth of each pass during rough cut NC sequences. The STEP_DEPTH must be greater than zero. The default is not set (displayed as "1").

For Engraving, the default is a dash (-), that is, not used. If you set STEP_DEPTH to a value smaller than the GROOVE_DEPTH, Engraving will be performed in multiple step increments.

MIN_STEP_DEPTH

For Volume and Profile milling, specifies the minimum acceptable distance between slices. By default, all planar surfaces that are normal to the Z-axis of the NC Sequence coordinate system produce additional slices. A slice along such a planar surface will be skipped if the distance between it and the previous slice is less than the value of MIN_STEP_DEPTH.

NUMBER_CUTS

For Face milling, gives you additional control over the number of cuts to depth (also controlled by the STEP_DEPTH parameter). The system will compute number of cuts using the STEP_DEPTH parameter value, compare it with the NUMBER_CUTS value, and use the greater one. The default is a dash (-), that is, not used.

For Cutline machining, allows you to perform milling in step depth increments. This has to be used together with the next parameter OFFSET_INCREMENT. The default is a dash (-), that is, not used.

For Engraving, lets you limit the number of cuts when the STEP_DEPTH parameter is also specified. The default is a dash (-), that is, not used. If you specify a number, for example, 3, the tool will make three cutting passes at STEP_DEPTH increments, with the last pass defined by the GROOVE_DEPTH value.

OFFSET_INCREMENT

Together with NUMBER_CUTS, allows you to perform Cut Line machining in step depth increments. The tool will make the first slice at (OFFSET_INCREMENT * (NUMBER_CUTS1) + PROF_STOCK_ALLOW) above the selected surfaces and perform NUMBER_CUTS slices at OFFSET_INCREMENT distance from each other, so that the last slice is at PROF_STOCK_ALLOW above the selected surfaces. If SCALLOP_HGT is specified, it will affect the last slice only. At the end of each slice, the tool will retract, move to the beginning of the next slice, and plunge. If LACE_OPTION is set to NO, the tool will additionally retract after each cutting pass across the surface(s) being machined. The default is a dash (-), that is, not used.

ROUGH_STEP_DEPTH

Available for 3-Axis Straight Cut Surface milling only. The default is a dash (-). If you specify a value other than the default, the system performs surface milling in depth increments, defined by the appropriate horizontal slices. This allows you to create Volume-like tool paths without actually defining a Mill Volume, which is especially helpful when machining imported (nonsolid) surfaces. The NC sequence removes the same material and has the same automatic degouging capabilities as the regular 3-Axis Straight Cut Surface milling sequences.

The following illustration shows 3-Axis Straight Cut Surface milling in depth increments.

image\img00079_shg.gif

  1. Select this surface.

 

WALL_SCALLOP_HGT

Controls the step depth for Volume milling. The WALL_SCALLOP_HGT (wsh) must be less than or equal to the cutter radius, that is, wsh <= d/2. The default is 0.

BOTTOM_SCALLOP_HGT

Similarly used to control step-over distance for Volume milling.

SCALLOP_HGT

Similarly used to control step-over distance for Surface milling and Local milling By Previous Tool.

The STEP_DEPTH and the WALL_SCALLOP_HGT parameters are illustrated in the following graphic. NC Manufacturing handles these parameters as follows:

  1. If you specify WALL_SCALLOP_HGT as zero (wsh = 0), a scallop height is calculated using STEP_DEPTH.

  2. If you specify wsh > 0, a step depth is calculated using wsh. This calculated value is compared to the STEP_DEPTH you defined. NC Manufacturing uses the lesser of the two.

The same is true for STEP_OVER and BOTTOM_SCALLOP_HGT (for Volume milling) or SCALLOP_HGT (for Surface milling).

The following graphic illustrates STEP_DEPTH and WALL_SCALLOP_HGT.

image\img00080_shg.gif

  1. STEP_OVER

  2. Tool path

  3. WALL_SCALLOP_HGT

  4. STEP_DEPTH

 

ROUGH_STOCK_ALLOW

and

PROF_STOCK_ALLOW

The amount of stock left after the rough cut for the finish cut. Both parameters are used in Volume milling NC sequences and signify different stock allowances for roughing and profiling cuts. PROF_STOCK_ALLOW must be set to a value less than or equal to ROUGH_STOCK_ALLOW. When geometry is displayed after Automatic material removal, NC Manufacturing uses PROF_STOCK_ALLOW.

 

image\img00081_shg.gif

  1. PROF_STOCK_ALLOW

  2. ROUGH_STOCK_ALLOW

  3. Pocket

In Roughing and Reroughing NC sequences, only ROUGH_STOCK_ALLOW is used to specify the amount of stock left after the cut.

 

BOTTOM_STOCK_ALLOW

For Volume milling, the amount of stock left after a rough NC sequence on planar surfaces parallel to the retract plane. The default is a dash (-), in which case the BOTTOM_STOCK_ALLOW parameter is ignored and PROF_STOCK_ALLOW is used instead.

For Face milling, specifies the amount of stock left on the selected face. The default, a dash (-), sets the stock allowance to 0.

WALL_TOLERANCE

Lets you specify the amount of material that can be left along the walls after the previous NC sequence, without the Local Mill NC sequence cleaning it up. The default is 0. Applicable for Local milling NC sequences referencing a previous Volume NC sequence.

STEP_OVER

Controls the lateral depth of cut of either type of endmill. The STEP_OVER must be a positive value less than or equal to the cutter diameter. The default is not set (displayed as "1").

TOOL_OVERLAP

An alternative to STEP_OVER. Indicates the amount that the tool should overlap the region machined during the previous pass. If TOOL_OVERLAP is specified and STEP_OVER is not, STEP_OVER will be calculated as
(CUTTER_DIAM TOOL_OVERLAP).

 

PLUNGE_STEP

Controls the distance between successive plunges of the tool. The default is a dash (-), in which case:

Applicable for Plunge milling only.

 

CORNER_ROUND_RADIUS

Specifies the minimum radius allowed for concave corners in high speed machining. Available for Volume milling, Roughing and Reroughing. The default is 0.

NUMBER_PASSES

Gives you additional control over the number of tool passes per slice (also controlled by the STEP_OVER parameter). The system will compute step-over distance using the NUMBER_PASSES parameter value (if other than 0), compare it with the STEP_OVER value, and use the one that is smaller. Applicable for Volume milling and Facing. For Facing, if NUMBER_PASSES is set to 1, it will override the STEP_OVER value, so that only one pass per slice will be made.

ONE_PASS_OFFSET

Allows you to offset the tool path for a one-pass Face milling NC sequence (that is, when NUMBER_PASSES is 1). The positive value offsets the pass to the left with respect to the cut direction, the negative to the right. The default is 0.

INITIAL_EDGE_OFFSET

Allows you to offset the first pass for Face milling with respect to the edge of the surface being milled. The default is 0, in which case the tip trajectory at first pass will coincide with the surface edge; the positive value offsets the first pass into the surface, the negative off the surface. Cannot be greater than the STEP_OVER value.

FINAL_EDGE_OFFSET

Allows you to offset the last pass for Face milling with respect to the edge of the surface being milled. The default is 0, in which case the tip trajectory at last pass will coincide with the surface edge; the positive value offsets the last pass into the surface, the negative off the surface. Cannot be greater than the STEP_OVER value.

CUT_ANGLE

The angle between the cut direction and the X-axis of the NC Sequence coordinate system. The default CUT_ANGLE is 0, which is parallel to the X axis. Valid for Volume and Plunge milling, Pocketing, Facing, Straight Cut Surface milling, and Projected Cuts Surface milling. CUT_ANGLE will be ignored for Volume and Plunge milling, Pocketing, and Projected Cuts Surface milling if SCAN_TYPE is TYPE_SPIRAL.

image\img00082_shg.gif

  1. CUT_ANGLE 0

  2. CUT_ANGLE 90

 

LEAD_ANGLE

Together with TILT_ANGLE, defines the tool orientation with respect to the surface normal for 5-Axis Surface milling NC sequences. LEAD_ANGLE is specified in degrees from the surface normal with respect to the tool travel direction: positive value tilts the tool forward, negative backward.

TILT_ANGLE

Together with LEAD_ANGLE, defines the tool orientation with respect to the surface normal for 5-Axis Surface milling NC sequences. TILT_ANGLE is specified in degrees from the surface normal with respect to the tool travel direction: positive value tilts the tool to the right, negative to the left.

AXIS_SHIFT

Allows you to shift the CL data along the tool axis. If set to a positive value, will shift all CL data down along the tool axis; a negative value will shift the CL data up. The default is 0.

Note: AXIS_SHIFT is applied after gouge checking has been performed. Use the Gouge Check functionality to make sure there is no gouging.

image\img00083_shg.gif

  1. Tool

  2. Model

  3. AXIS_SHIFT

 

NUM_PROF_PASSES

Together with PROF_INCREMENT, allows you to create multiple profiling or trajectory passes horizontally offset from each other. NUM_PROF_PASSES specifies the amount of passes that will be generated (the default is 1). Applicable for Volume milling when ROUGH_OPTION is set to PROF_ONLY, for Profiling, and for Trajectory milling. If another value of the ROUGH_OPTION parameter is specified for Volume milling, NUM_PROF_PASSES will be ignored.

PROF_INCREMENT

Specifies the horizontal distance between the passes generated according to NUM_PROF_PASSES, which means that the first pass will be offset from the final pass by:
(NUM_PROF_PASSES1)*PROF_INCREMENT.
The default is 0. Applicable for Volume milling when ROUGH_OPTION is set to PROF_ONLY, for Profiling, and for Trajectory milling. If another value of the ROUGH_OPTION parameter is specified for Volume milling, NUM_PROF_PASSES will be ignored.

The following graphic illustrates NUM_PROF_PASSES and PROF_INCREMENT.

 

image\img00084_shg.gif

  1. NUM_PROF_PASSES = 1

  2. NUM_PROF_PASSES = 4

  3. PROF_INCREMENT

  4. First pass

  5. Final pass

 

CORNER_OFFSET

Specifies the amount of material to be removed by a Local Mill NC sequence using Corner Edges. The default is 0.

SLOPE_ANGLE

In Local Milling and Finishing, the angular value with respect to the XY plane that divides the material to be removed into steep (near vertical) and shallow (near horizontal) regions. For example in Local Milling, if you are removing material left over in a pocket with slanted walls, specifying the value of the SLOPE_ANGLE less than the wall slope will make the tool machine the bottom edges of the pocket first, and then remove the material in the corners between the walls. The default SLOPE_ANGLE for newly created Local Milling NC sequences is 30 degrees. For NC sequences created prior to Release 2000i2, the default value is 90 degrees. The default SLOPE_ANGLE for Finishing NC sequences is 45 degrees.

START_OVERTRAVEL

Specifies the distance from the tool to the surface outline for all passes except the first one for each slice (see also APPROACH_DISTANCE). The default is 0. Applicable for Facing only.

END_OVERTRAVEL

Specifies the distance that the tool overtravels past the surface outline on all passes except the last one for each slice (see also EXIT_DISTANCE). The default is 0. Applicable for Facing only.

GROOVE_DEPTH

The depth of the groove. The default is not set (displayed as "1"). Applicable for Engraving only.

4X_TILT_ANGLE

Specifies the angle (in degrees) between the tool axis and the 4 Axis Plane. Normally, the tool axis is parallel to this plane (the default 4X_TILT_ANGLE is 0). Applicable for 4-axis milling only.

4X_LEAD_ANGLE

Specifies the angle (in degrees) between the tool axis and the projection of the surface normal on the 4 Axis Plane (the default is 0). Applicable for 4-axis milling only.

4X_MAX_LEAD_ANGLE

Specifies the maximum lead angle allowed when trying to avoid gouging. The default is a dash (-), but you have to specify a value if 4X_LEAD_RANGE_OPT is set to YES. Applicable for 4-axis milling only.

4X_MIN_LEAD_ANGLE

Specifies the minimum lead angle allowed when trying to avoid gouging. The default is a dash (-), but you have to specify a value if 4X_LEAD_RANGE_OPT is set to YES. Applicable for 4-axis milling only.

CHK_SRF_STOCK_ALLOW

Allows you to specify stock allowance to be used with check surfaces. The default is a dash (-), that is, ignore. This parameter is available for Milling NC sequences that utilize the Check Surfs functionality (that is, Surface, Trajectory, Profile milling, and for Local Milling referencing a Surface milling NC sequence).

Note: Be careful when specifying CHK_SRF_STOCK_ALLOW for NC sequences where all the reference part surfaces are selected as check surfaces.

TOOLPATH_CREATION_TYPE

In Surface milling, allows you to specify how the tool path is created. The values are:

Feed

ARC_FEED

Allows you to control the cut feed around arcs. The default is a dash (-), in which case the CUT_FEED will be used. If set to 0, the RAPID statement will be output before the CIRCLE statement.

ARC_FEED_CONTROL

Determines how the value for cut feed around arcs is calculated. The options are:

For internal radii:

feed = ARC_FEED * (circle radius / (circle radius + CUTTER_DIAM/2))

For external radii:

feed = ARC_FEED * (circle radius / (circle radius - CUTTER_DIAM/2))

 

TRAVERSE_FEED

Allows you to set a feed rate for all traverse tool motions. The default is a dash (-), in which case the RAPID command will be output to the CL file.

WALL_PROFILE_CUT_FEED

For certain types of high-speed Volume milling (when SCAN_TYPE is set to SPIRAL_MAINTAIN_CUT_TYPE or SPIRAL_MAINTAIN_CUT_DIRECTION), allows you to set a lower feed rate for the first cut, when the tool is cutting the material on both sides. The default is a dash (-), in which case the CUT_FEED value will be used.

INVERSE_FEED

Enables you to specify the inverse time feed rate, or the rate of rotation, for machines with rotary axes. Available for 4- and 5-Axis NC sequences only. If you set INVERSE_FEED to YES (the default is NO), the system outputs the following line in the CL data file before the first cutting feed statement:

FEDRAT / INVERS, AUTO

At the end of the CL data file, the system outputs the following line:

FEDRAT / INVERS, OFF

RAMP_FEED

See Entry/Exit parameters.

APPROACH_FEED

See Entry/Exit parameters.

THREAD_FEED

Defines the thread pitch. Applicable for Thread milling only.

THREAD_FEED_UNITS

TPI (default), MMPR, IPR. Applicable for Thread milling only.

EXIT_FEED

See Entry/Exit parameters.

Machine

SPINDLE_SPEED

The rate at which the machine spindle rotates (RPM). The default is 1.

WALL_PROFILE_SPINDLE_SPEED

For certain types of high-speed Volume milling (when SCAN_TYPE is set to SPIRAL_MAINTAIN_CUT_TYPE or SPIRAL_MAINTAIN_CUT_DIRECTION), allows you to set a lower spindle speed for the first cut, when the tool is cutting the material on both sides. The default is a dash (-), in which case the SPINDLE_SPEED value will be used.

SPINDLE_SENSE

The direction of spindle rotation. CW (clockwisedefault), CCW (counterclockwise).

SPINDLE_RANGE

NO_RANGE (default), LOW, MEDIUM, HIGH, NUMBER. If a value other than NO_RANGE is set, range will be included in the SPINDL command in the CL file (for example, "RANGE, LOW"). If set to NUMBER, the RANGE_NUMBER parameter value will be used in the SPINDL command (for example, "RANGE, 4", where 4 is the RANGE_NUMBER parameter value).

RANGE_NUMBER

Will be output in the SPINDL command if SPINDLE_RANGE is set to NUMBER. The default is 0.

MAX_SPINDLE_RPM

If set to a value other than a dash (-) (which is the default), the MAXRPM attribute will be added to the SPINDL command.

SPEED_CONTROL

The default SPEED_CONTROL is CONST_RPM (constant revolutions per minute). CONST_SFM (constant surface feet per minute) and CONST_SMM (constant surface meters per minute) allow you to apply feed rate control to the contact surface between the tool and the workpiece, to create good surface finish.

CUTCOM

Controls tool compensation. The options are:

CUTCOM_REGISTER

Specifies the number of the register of the machine controller that holds the tool compensation data. The default is 0.

NUMBER_CUTCOM_PTS

Specifies if colinear points in approach and exit motions should be stripped or added. The values are:

The following illustration shows the number and location of GOTO points for the following NUMBER_CUTCOM_PTS values:

 

image\img00085_shg.gif

  1. 1st GOTO point

  2. 2nd GOTO point

  3. 3rd GOTO point

  4. 4th GOTO point

  5. Approach move

  6. Cut motion

  7. Part

 

CUTCOM_LOC_APPR

Specifies location of CUTCOM statement on the approach motion if multiple cutcom points are specified. Cutcom points are numbered from 0 to n, where n is the value of NUMBER_CUTCOM_PTS. The default is 1.

CUTCOM_LOC_EXIT

Specifies location of CUTCOM statement on the exit motion if multiple cutcom points are specified. Cutcom points are numbered from 0 to n, where n is the value of NUMBER_CUTCOM_PTS. The default is 0.

The following illustrations shows the locations and numbering of cutcom points for approach and exit motions if NUMBER_CUTCOM_PTS is 2.

 

image\img00086_shg.gif

  1. 1st GOTO point (cutcom point 0)

  2. 2nd GOTO point (cutcom point 1)

  3. 3rd GOTO point (cutcom point 2)

  4. 4th GOTO point

  5. 5th GOTO point

  6. 6th GOTO point (cutcom point 0)

  7. 7th GOTO point (cutcom point 1)

  8. 8th GOTO point (cutcom point 2)

  9. Approach move

  10. Cut motion

  11. Exit move

  12. Part

 

HOLDER_DIAMETER

Along with HOLDER_LENGTH, allows you to use holder dimensions for automatic gouge avoidance. The default is a dash (-). If specified, will also be reflected when displaying CL data and when the tool is displayed in the Preview window of the Tool Setup dialog box. Applicable for Trajectory, Straight Cut and Isolines Surface milling.

HOLDER_LENGTH

Along with HOLDER_DIAMETER, allows you to use holder dimensions for automatic gouge avoidance. The default is a dash (-). If specified, will also be reflected when displaying CL data and when the tool is displayed in the Preview window of the Tool Setup dialog box. Applicable for Trajectory, Straight Cut and Isolines Surface milling.

OSETNO_VAL

Specifies the tool gauge length register. The default is a dash (-), in which case the Offset value from the Tool Table is used. Not available if you use the multiple tip tool functionality.

Z_GAUGE_OFFSET

Shifts CL output by a specified value along the tool axis. If you specify a positive value, CL data is shifted in the positive Z-direction of the tool coordinate system; a negative value shifts CL data in the opposite direction. The default is a dash (-). Not available if you use the multiple tip tool functionality.

TIP_CONTROL_POINT

If you are using a multi-tip tool for the NC sequence, lets you specify which tip is to be used as control point for computing the tool path. The values available from the drop-down list correspond to the number of tips in the tool currently selected for the NC sequence.

TLCHG_TIP_NUMBER

For a multi-tip tool, lets you specify which tip is to be used as control point to go to Start and End point, if they are defined in the NC Sequence. The values are:

SMOOTH_RADIUS

Specifies the radius for filleting or smooth corner machining. The minimum value must be 10% of the tool diameter if the SMOOTH_SHARP_CORNERS parameter is defined and not set to CONSTANT_RADIUS. The maximum allowable value is 50% of the step-over distance. Corner rounding is available for line-line, line-arc, and arc-arc (if they are not tangent) connections. Available for Volume milling, Roughing, Reroughing, and Local milling (Prev NC Seq only).

Note: If filleting is not possible, Pro/ENGINEER displays a message.

SMOOTH_SHARP_CORNERS

Specifies the way sharp tool path corners are rounded while machining. Available for Volume milling, Roughing, Reroughing, and Local milling (Prev NC Seq only).

Angle

Rounding radius

less than 5 degrees

10% of the SMOOTH_RADIUS value

less than 10 degrees

20% of the SMOOTH_RADIUS value

less than 20 degrees

40% of the SMOOTH_RADIUS value

less than 30 degrees

60% of the SMOOTH_RADIUS value

less than 60 degrees

80% of the SMOOTH_RADIUS value

less than 180 degrees

100% of the SMOOTH_RADIUS value

Note: For arcs, the angle is computed using the tangent at the corner.

CORNER_SLOWDOWN

Specifies the use of a progressive slowdown in the feed rate before a corner followed by an acceleration to the cut feed rate after the corner. The default is NO. Available for Volume milling, Roughing, Reroughing, and Local milling (Prev NC Seq only).

Note: If the slowdown is not possible, Pro/ENGINEER displays a message.

SLOWDOWN_LENGTH

Specifies the length of the move for the slowdown. The same length is used for the acceleration after the corner. The length is measured from the sharp edge or the beginning of the rounding fillet, if any. If one of the edges is an arc, the distance is taken along the arc. Available for Volume milling, Roughing, Reroughing, and Local milling (Prev NC Seq only).

SLOWDOWN_PERCENT

Specifies the feed rate at the end of the slowdown. For example, if the cut feed rate is 30 inches per minute and the value of the SLOWDOWN_PERCENT is 10, then the feed rate at the end of the slowdown is 3 inches per minute. Available for Volume milling, Roughing, Reroughing, and Local milling (Prev NC Seq only).

NUMBER_SLOWDOWN_STEPS

Specifies the number of steps in which the slowdown takes place. A larger number of steps results in a smoother slowdown. At each step, the feed rate is reduced by (100-SLOWDOWN_PERCENT)/NUMBER_SLOWDOWN_STEPS. Available for Volume milling, Roughing, Reroughing, and Local milling (Prev NC Seq only).

During acceleration after the corner, the number of steps is halved.

Entry/Exit

RAMP_ANGLE

The angle at which the tool enters the workpiece during a plunge cut. The default RAMP_ANGLE is 90, which enters the workpiece parallel to the Z-axis. Not applicable for Facing or Trajectory NC sequences.

RAMP_FEED

The rate at which the tool moves upon entering the workpiece during a plunge cut. The default is a dash (-), in which case the CUT_FEED will be used. Not applicable for Facing or Trajectory NC sequences.

CLEAR_DIST

The clearance distance above the surface to be milled (for example, the previous slice level) at which the rapid motion ends and the PLUNGE_FEED begins. The default is not set (displayed as "1").

PULLOUT_DIST

Specifies the height above the level of the cut (for example, the slice just milled) up to which the tip of the tool will retract at CUT_FEED and then change to RETRACT_FEED. The default is a dash (-), that is, 0.

INTER_RET_HEIGHT

Specifies the distance that the cutter will retract above the level of the cut to perform intermediate rapid motions. The default is a dash (-), in which case the cutter will retract all the way to the retract surface. Applicable for Facing only.

LEAD_IN

If set to YES, makes the tool enter the workpiece along a tangent circular path when profiling. The arc radius is set by LEAD_RADIUS, the arc angle by ENTRY_ANGLE. You can also specify the length of the adjacent straight portion of Lead In trajectory using TANGENT_LEAD_STEP, and the length of a straight segment normal to it using NORMAL_LEAD_STEP.

For closed contours, if start point is not set, the tool will enter at a location determined by the system. If not satisfied with this location, specify your own Start Point axis. The tool will enter at the point along the profile which is closest to the start point axis.

The following graphic illustrates LEAD_IN and LEAD_OUT.

image\img00087_shg.gif

  1. ENTRY_ANGLE

  2. LEAD_RADIUS

  3. LEAD_IN

  4. LEAD_OUT

  5. NORMAL_LEAD_STEP

  6. TANGENT_LEAD_STEP

  7. EXIT_ANGLE

  8. LEAD_IN

  9. Start point

  10. LEAD_OUT

  11. Open profile

  12. Closed profile

 

If a closed contour contains multiple loops, LEAD_IN and LEAD_OUT will be applied to each loop.

 

image\img00088_shg.gif

If LEAD_IN is set to YES with a zero radius, the tool will go directly to the point closest to the Start Point specified and start cutting. When LEAD_IN is set to NO, cutting will begin at the default point of the contour determined by the system. In the following illustration, the graphic on the left shows the tool path for LEAD_IN set to NO, while the graphic on the right shows the tool path for LEAD_IN set to YES and LEAD_RADIUS set to 0.

 

image\img00089_shg.gif

  1. Default start of the contour

  2. Start Point axis

  3. Tool path

  4. Start point axis

  5. Tool path

 

LEAD_OUT

Makes the tool exit the workpiece along a tangent circular path when profiling. Works similarly to LEAD_IN. If the end point is specified it will be used for LEAD_OUT, otherwise the default 90 arc (and the default exit point for closed contours) will be used.

LEAD_RADIUS

The radius of the tangential circular movement of the tool when leading in or out. The default is 0.

TANGENT_LEAD_STEP

The length of the linear movement that is tangent to the circular lead-in or lead-out motion. The default is 0.

NORMAL_LEAD_STEP

The length of the linear movement that is normal to the tangent portion of the lead-in or lead-out motion. The default is 0.

HELICAL_DIAMETER

Allows you to replace the plunge motion between the slices for Rough Volume milling with a helical entry motion. The helical diameter will be formed by the outside of the tool as it approaches the beginning of a Rough slice; the angle of descent is defined by the RAMP_ANGLE parameter value. If a Start Point axis is specified, the helix center will be at the axis location; if the helical motion violates the Mill Volume, the system will issue a warning and stop machining. If a Start Point axis is not specified,the helix will be created as close to the start point of the lower slice as possible. To move from the end of the previous slice, the tool will lift off the surface by PULLOUT_DIST and horizontally move at RETRACT_FEED to the start of the helical entry into the lower slice. If you have specified Approach Walls for the NC sequence, the helical motion will not be created when the tool moves down outside the Approach Walls; however, if the tool moves down inside the Mill Volume, the system will use the helical entry. The default HELICAL_DIAMETER is a dash (-), in which case the helical motion will not be performed.

APPR_EXIT_EXT

Applicable for Volume milling only. Defines the maximum distance between the periphery of the tool and the Approach Wall of the mill volume for approach and exit motions within a slice.

APPR_EXIT_PATH

Applicable for Profiling and for the profiling pass of Volume milling NC sequences. Allows you to trim the sketched approach or exit path by the outline of the profiling tool motion. For approach path, only the first portion (from the start point up to the first intersection with the profiling outline) will be kept. For exit path, only the last portion (from the last intersection with the profiling outline to the end point) will be kept. If the approach/exit path is set to not be trimmed, the tool will follow the whole path as sketched. The values are:

 

image\img00090_shg.gif

  1. Approach path

  2. Approach path (trimmed)

 

APPR_EXIT_HEIGHT

Applicable for Volume, Local, Profile milling, and Engraving. Allows you to control the depth of the approach and exit path specified during Build Slice. The options are:

OVERTRAVEL_DISTANCE

For 3-Axis Straight Cut Surface milling, specifies the distance that the tool travels past the surface outline, both at the beginning and end of each cutting pass.

APPROACH_DISTANCE

Specifies the length of approach motions. For Facing, also specifies the additional (with respect to START_OVERTRAVEL) distance from the tool to the surface outline for the first pass in each slice. The default is a dash (-), that is, 0.

EXIT_DISTANCE

Specifies the length of exit motions. For Facing, also specifies the additional (with respect to END_OVERTRAVEL) distance that the tool overtravels past the surface outline for the last pass in each slice. The default is a dash (-), that is, 0.

APPROACH_FEED

The rate at which the tool approaches the surface during a Facing NC sequence. The default is a dash (-), in which case CUT_FEED is used.

EXIT_FEED

The rate at which the tool overtravels past the surface edge during a Facing NC sequence. The default is a dash (-), in which case CUT_FEED is used.

CLEARANCE_EDGE

Specifies which point of the tool is to be used for measuring the exit motions and the overtravel motions when the tool leaves the material:

Applicable for Facing only.

ENTRY_EDGE

Specifies which point of the tool is to be used for measuring the approach motions and the overtravel motions when the tool approaches the material:

Applicable for Facing only.

APPROACH_TYPE

Allows you to automatically create an approach motion in Thread milling and Local milling By Previous Tool.

In Thread milling, the values are:

In Local milling By Previous Tool, the values are:

EXIT_TYPE

Allows you to automatically create an exit motion in Thread milling and Local milling By Previous Tool.

In Thread milling, the values are:

In Local milling By Previous Tool, the values are:

ENTRY_ANGLE

The angle of the arc created by the circular movement of the tool when leading in. Used when creating Lead In motions. The default is 90.

In Thread milling, defines the angle of the helical approach motion. If the angle is 0, the helical motion will still be created, but it will only contain one point. However, you will be able to modify the motion parameters in order to change this.

EXIT_ANGLE

The angle of the arc created by the circular movement of the tool when leading out. Used when creating Lead Out motions. The default is 90.

In Thread milling, defines the angle of the helical exit motion. If the angle is 0, the helical motion will still be created, but it will only contain one point. However, you will be able to modify the motion parameters in order to change this.

CUT_ENTRY_EXT

For Surface and Swarf milling, specifies the default entry move type for intermediate cuts. The values correspond to the Each Cut entry move types available in the Entry/Exit Move dialog box.

CUT_EXIT_EXT

For Surface and Swarf milling, specifies the default exit move type for intermediate cuts. The values correspond to the Each Cut exit move types available in the Entry/Exit Move dialog box.

INITIAL_ENTRY_EXT

For Surface and Swarf milling, specifies the default entry move type for the first cut. The values correspond to the First Cut entry move types available in the Entry/Exit Move dialog box.

FINAL_EXIT_EXT

For Surface and Swarf milling, specifies the default exit move type for the last cut. The values correspond to the Last Cut exit move types available in the Entry/Exit Move dialog box.

Thread

THREAD_DIAMETER

Defines the minor diameter for an External thread or the major diameter for an Internal thread. Applicable for Thread milling only.

See Also

Return to Pro/ENGINEER Index