Holemaking Parameters

The following parameters are specific to Holemaking 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. Follow the link under See Also to access this topic.

• You must supply a value for all parameters that have a default of –1 (this means that the default value is not set by the system).

• Length units for the NC sequence parameters (where applicable) are the same as the units of the workpiece.

There are several algorithms for automatically creating the Holemaking tool path:

• TYPE_1—By incrementing the Y coordinate and going back and forth in the X direction. In the following illustration, this scan type is shown in the left picture.

• TYPE_SPIRAL—Clockwise starting from the hole nearest to the coordinate system. In the following illustration, this scan type is shown in the middle picture.

• TYPE_ONE_DIR—By incrementing the X coordinate and decrementing the Y. In the following illustration, this scan type is shown in the right picture.

• PICK_ORDER—The holes will be drilled in the same order as they are selected. If one choice results in more than one hole being selected (for example, All Holes or Pattern selection), these holes will be drilled according to TYPE_1. Then the PICK_ORDER drilling will be resumed.

• SHORTEST (default)—The system determines which order of holes results in the shortest machine motion time.

For 5-Axis Holemaking inside a single step, determines how the SCAN_TYPE parameter is applied.

• NO (default)—Holes without consideration for their axis orientation have the SCAN_TYPE parameter applied to them.

Enables you to reverse the order in which the holes are machined. The values are: STANDARD (default) or REVERSE. REVERSE will make the system start with the last hole and go back to the first one. This functionality is helpful when you have to create multiple NC sequences on a large hole set: alternating direction of tool path for successive NC sequences lets you save time for repositioning the tool. If your tool path was created using the Customize functionality, CUT_DIRECTION will affect the Use Sketch segments, but not the Connect segments.

Specifies the output format for CL data of a Holemaking NC sequence. For all newly created NC sequences the default is COUPLET. The other option is FIXED (this is the default for NC sequences created prior to Release 12.0). Not applicable for BORE, REAM, and BREAKCHIP cycles (these are always output in COUPLET format).

Specifies the order of drilling for an automatically created Holemaking tool path when multiple Hole Sets are included in the NC sequence:

• BY_HOLE (default)—The SCAN_TYPE algorithm will be applied to all the selected holes, without considering which Hole Set they belong to. This results in a shorter traversal path of the tool.

• BY_HOLESET—The SCAN_TYPE algorithm will be applied to holes in each Hole Set separately. This will somewhat reduce the size of the CL file, because each Hole Set will only have one CYCLE / ... and CYCLE / OFF statement associated with it, instead of turning the cycle on and off every time the tool moves to a hole in a different Hole Set.

The system adds the BREAKOUT_DISTANCE value to the Z depth in the CYCLE statements associated with holes drilled Thru All, and with through holes drilled using the Auto depth option. You can use it for Blind holes, if you select Use breakout distance when defining a Hole Set. The default is 0.

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 all 3-Axis Holemaking NC sequences except Back boring.

Depth increment for each drilling pass. Default value is 0. If you select DEEP drilling, you have to specify non-zero PECK_DEPTH. Not available for Countersink drilling.

Used for TAP cycles only (instead of CUT_FEED) to specify feed rate. The default is not set (displayed as "–1").

TPI (default), MMPR, IPR. Applicable for TAP cycles only. Allows alternate pitch designations.

Used for the floating TAP cycle only. The feed rate is calculated as the THREAD_FEED value multiplied by FLOAT_TAP_FACTOR. The default is 1.

The feed rate at which the cutter moved away from the workpiece. The RETRACT_FEED value will be included in the ream cycle statement in CL file as ZFEED, for example CYCLE / REAM, DEPTH, 50.000000, MMPM, 1111.000000, CLEAR, 1.000000, ZFEED, 30.000000. In this example, the RETRACT_FEED parameter value is 30. This value reflects in the CL data when the CYCLE_FORMAT parameter is set to COUPLET. If the CYCLE_FORMAT parameter is set to GOTO, the RETRACT_FEED value will not be output in the CL data.

The RETRACT_FEED appears only in CL data and cannot be computed on the NC tab.

The rate at which the machine spindle rotates. The default is not set (displayed as "–1").

RETURN_SPINDLE_SPEED

The rate at which the machine spindle rotates during the return motion. This parameter is applicable for FixedTapping sequences.

The direction of spindle rotation. CW (clockwise—default), CCW (counterclockwise).

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).

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

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

CONST_RPM (constant revolutions per minute), CONST_SFM (constant surface feet per minute), CONST_SMM (constant surface meters per minute).

The default SPEED_CONTROL is CONST_RPM. CONST_SFM and CONST_SMM allow you to apply feed rate control to the contact surface between the tool and the workpiece, to create good surface finish.

Duration of dwelling at depth. The default is a dash (-), in which case there will be no delay. Not applicable for TAP and DEEP cycles.

SECONDS (default) or REV.

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.

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:

HOLE_REDUCTION_FACTOR

Used to generate the tool path when the drill diameter is more than the hole diameter. The drill diameter is reduced by the specified factor. The value must be less than 1 to generate an accurate tool path.

TAP_REDUCTION_FACTOR

Used to generate the tool path when the tap drill diameter is more than the hole diameter. The tap drill diameter is reduced by the specified factor. The value must be less than 1 to generate an accurate tool path.

The clearance distance above the top of the hole at which the PLUNGE_FEED ends and the CUT_FEED begins. The default is not set (displayed as "–1").

The clearance distance above the top of the hole at which the tool is positioned for 5-Axis Holemaking. Also defines how far the tool will retract after drilling a hole and before traversing to the next hole. The default value for CLEARANCE_OFFSET is a dash (-), in which case CLEAR_DIST will be used. Applicable for 5 Axis Holemaking only.

Allows for the tool to return to a point other than that defined by CLEAR_DIST. The default is a dash (-), in which case this parameter is not used.

If the default value is used, then the tool will return to the clearance distance (CLEAR_DIST) when moving to the next hole, and the cycle statement will not include the RETURN option.

If the value of PULLOUT_DIST is set to 0, then the tool will return to the retract plane when moving to the next hole.

In 5 Axis Holemaking, if PULLOUT_DIST is set to 0, the tool returns to CLEARANCE_OFFSET before moving to the next hole. The default value for CLEARANCE_OFFSET is a dash (-), in which case the CLEAR_DIST will be used.

Specifies the distance that the cutter will retract above the level of the cut to perform intermediate rapid motions. The default is a dash (-).

Allows for further rapid advance from CLEAR_DIST towards the top of the hole. The default is a dash (-), in which case this parameter is not used.

If set to a value other than 0 (the default), specifies full retraction out of the hole for BREAKCHIP cycle after a certain number of incremental steps. This number of steps is calculated as FULL_RETRACT_DEPTH / PECK_DEPTH.

Allows you to specify orientation of an asymmetric tool before backing it away from the hole wall before retracting. Applicable for BORE cycle and for back spotting only. The default is a dash (-), in which case this parameter is not used.

Allows you to specify the distance of backing an asymmetric tool away from the hole wall before retracting. Applicable for BORE cycle and for back spotting only. The default is a dash (-), in which case this parameter is not used.