Type Of Operation

Describes the function to be performed by the CYCLE command. This will be the first word following CYCLE (i.e., CYCLE/DRILL).

Subtype Of Operation

Is a description of the TYPE OF OPERATION to be performed (i.e., CYCLE/DRILL,DEEP).

Specific Parameters

Are parameters that pertain only to a specific TYPE or SUBTYPE OF OPERATION (i.e., CYCLE/DRILL,DEEP,STEP,n).

General Parameters

Direct the actions of CYCLE operations (i.e., CYCLE/DRILL,DEEP,RAPTO,.1).

Scalars

Usually accompany parameters. A SCALAR is a numeric value that limits the actions of the CYCLE (i.e., CYCLE/DRILL,DEEP,RAPTO,.1).

General Description:

The parameters define the approach distance, final depth distance, and retraction distance in relation to the CL point. The delta distances are algebraically signed from the CL point in the part coordinate system. The following descriptions are typical for all commands except where specifically noted.

Parameter Definitions:

1. "RAPTO,+a" - specifies a rapid clearance plane a delta direction and distance from the CL point Z dimension. A positive "a" defines a rapid clearance plane above the CL point Z dimension; a negative "a" below.

"RAPTO" is modal. If a programmed CYCLE command does not include a RAPTO value, the previous "RAPTO" will be used. The postprocessor initially assumes RAPTO,.1.

2. "FEDTO,+b" - specifies a depth plane a delta direction and distance from the correlating CL point Z dimension. A positive "b" defines a depth plane above the CL point Z dimension; a negative "b" below.

"FEDTO" is modal. If it is not programmed with the present CYCLE command, the previous "FEDTO" will be used. The postprocessor initially assumes FEDTO,0.

• NOTE: The "FEDTO" description is valid for all cycles except CSINK.

3. "RTRCTO,+c" - specifies a retraction plane a delta direction and distance from the CL point Z dimension. A positive "c" defines a retraction plane above the CL point Z dimension; a negative "c" below.

"RTRCTO,AUTO" specifies that if enabled in the MDF, the GPM will generate a G98 in the canned cycle block to cause a full retraction to initial Z plane. If RTRCTO,AUTO is not programmed a G99 will be generated to cause a retraction to the rapid clearance plane.

The "RTRCTO" parameter must be programmed with each CYCLE command (except CYCLE/ON) if different retraction planes are desired. If it is not programmed, the postprocessor will retract the tool to the rapid clearance plane (RAPTO,a) used for that CL point.

the type of input and the desired feed rate. IPR and MMPR specify the type of input and the desired feed rate per spindle revolution. Programming IPR or MMPR causes the direct feed rate in IPM or MMPM to be calculated on the basis of the present spindle speed revolutions per minute (uPM = uPR x RPM). The feed rate series parameter is modal. If it is not programmed with the present CYCLE command, the previous feed rate parameter will be used. The postprocessor initially assumes IPM,0.

The "DWELL" parameter must be programmed with each CYCLE command (except CYCLE/ON) if a delay at depth is desired. "t" and "REV,n" are modal. If they are not programmed with "DWELL", the previous "t" or "REV,n" will be used.

• NOTE: The DWELL parameter might not be valid for all cycles. See the individual postprocessor commands for validity.

If simulating a cycle, the DWELL parameter will be processed as though a DELAY had been programmed. This can produce warning messages if DELAY is not valid for the particular machine controller.

6. "OPTION" defines an alternate cycle. See MDFG for cycle type definition.

Considerations:

l. The number of scalars used with a multi-scalar parameter can be any quantity which does not make the unit value of the parameter string exceed the maximum number allowed (see POSTPROCESSOR CONVENTIONS and EXPANDING THE USAGE OF CYCLE COMMANDS).

General Description:

 The parameters define the approach distance, final depth distance, and retraction distance in relation to the CL point. The delta distances are algebraically signed from the CL point in the part coordinate system. The following descriptions are typical for all commands except where specifically noted.

Parameter Definitions:

1. "CLEAR" becomes "RAPTO".

2. "DEPTH" becomes "FEDTO". This must be a positive value.

3. "RETURN" becomes "RTRCTO".

4. "PERREV" becomes "IPR or MMPR" depending upon the UNITS command. "PERMIN" becomes "IPM or MMPM" depending upon the UNITS command.

5. "REV" becomes "DWELL,REV".

Description:

 This command is used to cancel, reinstate, or modify a previously programmed CYCLE command.

Parameter Definitions:

1. "CYCLE/OFF" cancels a previously defined CYCLE. The CL points following "CYCLE/OFF" will cause position under contouring mode until another CYCLE or RAPID is programmed.

2. "CYCLE/ON" with no other parameters reinstates the last programmed CYCLE (excluding CYCLE/OFF) until a new CYCLE command is encountered.

Subtype operations that were valid for the last programmed CYCLE command can be changed or added through the use of CYCLE/ON (i.e., CYCLE/ON, subtype of operation). The same is true for changing or adding parameters.

Description:

This command generates code to position the cutter for milling with the tool at a defined depth plane.

Parameter Definitions:

(Letters shown below correspond to steps illustrated in adjoining diagram.)

1. "CYCLE/MILL" will generate the following sequence:

A. Rapid to the position and on to the clearance plane;

B. Feed to the depth plane at the commanded feed rate.

C. The tool will remain at depth and will position in the contouring mode to subsequent CL points.

Considerations:

l. Defining a RAPTO plane that is equal to the FEDTO plane (a1=b1) will cause rapid to depth.

2. The part programmer is responsible for withdrawing the tool from the part after milling is completed.

3. The feed rate defined in the CYCLE/MILL command refers to spindle feed rate. A FEDRAT/ command is required before CYCLE/MILL to define table feed rate. See FEDRAT/ command for further information.

4. Programming another CYCLE command, CYCLE/OFF or LOAD will cancel CYCLE/MILL.

Description:

This command generates code for a drilling or drilling with dwell cycle.

Parameter Definitions:

(Letters shown below correspond to steps illustrated in adjoining diagrams.)

1. "CYCLE/DRILL" generates coding for the following drilling sequence:

A. Rapid to the X,Y position and the clearance plane;

B. Feed to the depth plane;

C. Rapid back to the clearance plane (or to the RTRCTO plane if it is programmed).

2. "CYCLE/DRILL,DWELL" generates coding for the following drilling sequence:

A. Rapid to the X,Y position and the clearance plane;

B. Feed to the depth plane;

C. Dwell for the time of DWELL specified;

D. Rapid back to the clearance plane (or to the RTRCTO plane if it is programmed).

Description:

This command generates code to perform a countersink operation. The postprocessor calculates the countersink depth.

Parameter Definitions:

l."CYCLE/DRILL,CSINK,CSKDIA,n,TLANGL,n...,DWELL..." generates the following countersinking sequence at each CL point:

A.Rapid to the X,Y position and on the clearance plane (calculated clearance plane if "HOLDIA" is programmed);

B.Feed to calculated depth;

C.(Optional) Dwell for the time of DWELL specified;

D.Rapid retract to the defined clearance plane (or RTRCTO plane, if specified).

2."HOLDIA,h" specifies a hole diameter for following CSINK CL points. This parameter allows the postprocessor to calculate a rapid clearance plane for each specified CL point that is a RAPTO distance from the cutter edge instead of the cutter tip.

HOLDIA is not modal; therefore, if it is to be used for calculation of rapid clearance planes, it must be programmed with each DRILL,CSINK command except CYCLE/ON.

Considerations:

1.The postprocessor calculates the depth of the countersink using the countersink diameter (CSKDIA,n) and the tool angle (TLANGL,n). Any FEDTO programmed for a countersink operation will be ignored.

A

is the tool angle (TLANGL)

H

is the hole diameter (HOLDIA)

DIA

is the countersink diameter (CSKDIA)

R1

is the rapid clearance distance from the top of the part to the tool tip. This rapid clearance distance is programmed as the RAPTO parameter and is used when the HOLDIA parameter is not specified.

R2

is the rapid clearance distance from the top of the part to the tool tip when the HOLDIA parameter is specified. This distance is calculated, based on the programmed RAPTO, TLANGL, and HOLDIA.

This calculated rapid clearance distance allows the cutter_edge to be positioned to the programmed RAPTO distance above the hole to be countersunk. This distance is indicated in the above illustration as R3. R3 = R1.

D

is the calculated depth of cut based on the programmed CSKDIA and TLANGL.

Description:

This command generates code to perform a countersink operation. The postprocessor calculates the countersink depth.

Parameter Definitions:

l. "CSINK" becomes "DRILL,CSINK".
2. "DIAMET" becomes "CSKDIA".

Description:

 This command generates code for a tapping cycle.

Parameter Definitions:

(Letters shown below correspond to steps illustrated in adjoining diagram.)

1. "CYCLE/TAP" generates the following tapping sequence at each CL point.A.Rapid to the X,Y position and on the clearance plane;

B. Feed to the depth plane;

C. Reverse the spindle direction;

D. Feed back to the clearance plane (or RTRCTO plane if specified);

E. Reinstate the original spindle direction.

Description:

This command generates code for bore cycles. The type of boring cycle is dependent upon which subtype of operation, if any, is specified.

Parameter Definitions:

(Letters shown below correspond to steps illustrated in adjoining diagrams.)

1. "CYCLE/BORE" (no subtype of operation) generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Feed to depth plane;

C. Feed back to the clearance plane (or "RTRCTO" plane if programmed).

2. "CYCLE/BORE,DWELL" generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Feed to depth plane;

C. Dwell for the time of DWELL specified;

D. Feed back to the clearance or RTRCTO plane.

3. "CYCLE/BORE,DRAG" generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and clearance plane;

B. Feed to depth plane;

C. Stop the spindle;

D. Rapid back to the clearance or RTRCTO plane;

E. Reinstate previous spindle condition.

Figure 1-4 CYCLE/STEP Description

4. "CYCLE/BORE,MANUAL" generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Feed to the depth plane;

C. Machine is stopped with a program stop;

*D. MANUAL retraction of spindle (and cycle start button must be pushed to read the next block);

E. Reinstate previous spindle condition.

5. "CYCLE/BORE,MANUAL,DWELL" generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Feed to the depth plane;

C. Dwell for the time of DWELL specified;

D. Machine is stopped with a program stop;

*E. MANUAL retraction of the spindle (and cycle start button must be pushed to read the next block);

F. Reinstate previous spindle condition.

6. "CYCLE/BORE,NODRAG[,n]" generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Feed to the depth plane;

C. Spindle stop and orient;

D. X or Y offset rapid movement;

E. Rapid back to the clearance or RTRCTO plane;

F. Previous spindle conditions and X/Y position reinstated.

7. "CYCLE/BORE,BACK[,n] generates the following boring sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Spindle stop and orient tool;

C. X or Y offset rapid movement.

D. Feed to depth plane.

E. Rapid to RTRCTO plane.

F. Previous spindle conditions and X/Y position reinstated.

8. The optional parameters NODRAG[,n] and BACK[,n] can be output in the canned cycle block to define the X and/or Y offset motions.

• CAUTION: The postprocessor assumes that the tool is manually retracted clear of the workpiece. It is the part programmer's responsibility to ensure that this is done before any x,y movement is made.

Description:

This command generates code for constructing simulated cycles.

Parameter Definitions:

(Letters shown below correspond to steps illustrated in adjoining diagram.)

1. "CYCLE/MANUAL" generates the following sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane;

B. Feed to depth specified.

Description:

This command generates code for a deep or breakchip drill cycle. For either cycle, a series of cuts at different feed rates can be specified for each CL point.

Parameter Definitions:

l. "STEP,m,n" "m" specifies the initial delta depth that will be used to reach the final depth (FEDTO) for either extended drilling cycle. "n" specifies a machine dependent feed increment modifier. Both "m" and "n" can be output by the GPM in the DEEP and BRKCHP canned cycle blocks.

Since the FEDTO parameter defines the direction of the feed, STEP values are unsigned.

If the STEP parameter is omitted, the previous STEP value will be used. If STEP has not been previously specified, the postprocessor will output a warning and default to CYCLE/DRILL.

If STEP is programmed, it must immediately follow DEEP or BRKCHP, (Letters shown below correspond to steps illustrated in adjoining diagram.)

2. "CYCLE/DRILL,DEEP" generates the following deep drilling sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane (RAPTO,a);

B. Feed to the first depth (RAPTO,a,+STEP,n);

C. Rapid back to a clearance plane;

D. Rapid to a clearance distance from the first depth and feed to the second depth (d+STEP,n);

E. Rapid back to the clearance plane;

F. Repeat steps D and E above until the final depth (FEDTO,b) is reached;

G. Rapid back to the clearance plane or to the RTRCTO plane, if programmed.

(Letters shown below correspond to steps illustrated in adjoining diagram.)

3. "CYCLE/DRILL,BRKCHP" generates the following breakchip drilling sequence at each CL point:

A. Rapid to the X,Y position and on the clearance plane (RAPTO,a);

B. Feed to the first depth (RAPTO,a,+STEP,n);

C. Rapid to a clearance distance (+d) from the first depth;

D. Feed to the second depth (d+STEP,n);

E. Rapid to a clearance distance from the second depth;

F. Repeat steps D and E above until the final depth defined by FEDTO,b is reached;

G. Rapid back to the clearance plane or to the RTRCTO plane, if programmed.

Description:

The CYCLE command generates the proper coding for the specified type of PUNCH or nibble operation. The CYCLE command is modal and will remain in effect until another CYCLE command is encountered or is terminated by programming CYCLE/OFF. After a CYCLE command has been programmed, all succeeding motion to CL points within a series will be followed by the specified cycle operation. A CL point series includes all CL points that are programmed after a CYCLE command (excluding CYCLE/OFF and RAPID modes) until a CYCLE/OFF command or another CYCLE command is programmed. The CL points following the second CYCLE command would be another series. Any CL points following CYCLE/OFF are not part of a series. All CL points input for CYCLE commands are with regard to the part coordinate system zero point.

Parameter Definitions:

1. "CYCLE/ON" causes the last programmed CYCLE command (excluding OFF) to become effective until a new CYCLE command is encountered.

2. "CYCLE/OFF" cancels a previously defined CYCLE command. Unless another CYCLE command is programmed, all the CL points following "CYCLE/OFF" will position with the punch or nibble cycle off.

3. "CYCLE/PUNCH" generates a punch cycle which consists of motion to position with a single punch at the programmed CL points.

4. "CYCLE/STEP,n" or CYCLE/SCALOP,s" generates a nibbling cycle for the following CL points. A STEP distance will be the programmed as "n" and output will be generated to control the distance between punch centers. A SCALOP cycle will calculate the distance based on the radius of the tool and the programmed "s", the height of the scallop that will be left. A linear interpolation G code will be output for a linear nibble and a circular interpolation G code will be output for a circular nibble (see MOTION ELEMENT for further explanation). The nibble cycle will position to the first CL point and punch and then nibble to subsequent points.

5. "CYCLE/AVOID" will cancel the "STEP" or "SCALOP" mode for the next CL point only. A punch cycle will occur at the programmed CL point. The "STEP" or "SCALOP" mode will continue for all following CL points.

6. "DIAMTR,+d" defines the diameter for the tool to be loaded. This parameter must be specified for "CYCLE/SCALOP,s". The postprocessor uses this to calculate the radius.

7. "ATANGL,+a" defines the starting angle for a rotating punch. The programmed angle is output in the cycle block.

Figure 1-5 CYCLE/STEP Description

Figure 1-6 CYCLE/SCALOP,s (circular move)

Parameters:

This option allows you to control the order and format of the canned cycle block. You have the following PARAMETERS options.

Cycle X,Y Positioning Format - allows you to specify X, Y line positioning format that the GPM will use in moving to the non-spindle axes (usually X and Y) positions of the canned cycle.

In the following menus X,Y refers to the non-spindle axes. If Y is the spindle, then X and Z would be positioned and if X is the spindle axis Y and Z would be positioned.

Select the option that describes the positioning prior to canned cycle for your machine. The options cause the system to work as follows.

X,Y Output In Canned Cycle Block - The X and/or Y coordinates are output in the same block as the canned cycle G code.

X,Y Output Before Canned Cycle Block - The X and/or Y coordinates are output before the block with the canned cycle G code in a rapid traverse block.

X,Y And Rapid Clearance Point Output Before Can Cyc Blk Repeat In Can Cyc Blk - GPM will output X,Y and Z plus the RAPTO value in a rapid traverse block before the canned cycle block and for every motion point until cycle is cancelled. If the spindle is moving into the part, the X and the Y will be output before the Z. If the spindle is moving away from the part the Z will be output before the X and the Y moves. Controls that must have this feature are Bridgeport and Deckel.

X,Y And Rapid Clearance Point Output Before Can Cyc Blk After Load Repeat X Or Y In Can Cyc Blk - If this is the first motion after a LOAD command GPM will output X,Y and Z plus the RAPTO or RTRCTO, whichever is greater, value in a rapid traverse block before the canned cycle block for each motion point until cycle is cancelled. Otherwise the X and/or Y coordinates are output before the block with the canned cycle G code in a rapid traverse block. On the Z move after a LOAD command the tool length adjust offsets are applied. Controls that must use this feature are Fanuc, Yasnac, General Numeric, Sinumerik and Tosnuc.

X,Y,Z Output With Cycle/On G-code To Execute Previously Defined Cycle(Maho, Tree) - The GPM will output only the X,Y,Z coordinates of the canned cycle with a G-code to perform a previously defined canned cycle. Controls that need this option are Maho and Tree.

X,Y,Z+Rapto Output In Rapid Mode To Execute Previously Defined Canned Cycle (Bostomatic) - GPM will output X,Y and Z plus the RAPTO value in a rapid traverse block and for each motion point until cycle is cancelled to perform a previously defined canned cycle. If the spindle is moving into the part, the X Y move will be output before the Z. If the spindle is moving away from the part the Z move will be output before the X and the Y moves.

Xy+Rapid Clearance Point Output Before Can Cyc Blk. X,Y Not Repeated In Can Cyc Blk - GPM will output X,Y and the rapid clearance point in a rapid traverse block before the canned cycle block. The X, or Y motion is not repeated in the canned cycle.

X,Y OUTPUT AFTER THE CANNED CYCLE BLOCK - This allows X and Y positioning data to be output after the canned cycle data block.

Rapid Clearance Point (Rapto) - defines the output format for the rapid approach position within the canned cycle G code block.

• NOTE: Rapid Clearance Plane (RCP) is the programmed spindle axis coordinate (usually CL Z) plus the programmed RAPTO value.

Rapid Clearance Point In Canned Cycle Block - In this option the RCP is output with Word Address (usually R) in the block with a canned cycle G code. Most controls use this option.

Rapid Clearance Point Not Output In Canned Cycle Block - the RCP is not output at all in the canned cycle block. This option is used for controls that do not have RCP parameters and need them output before the canned cycle block. Controls that need this option are usually Bridgeports.

Rapid Clearance Point Defined In Cycle Definition Block Before Cycle Execution - With this option, the entire canned cycle is defined before any X,Y,Z coordinate output. The RCP is defined in the cycle definition block as the actual programmed RAPTO parameter. Controls that must have this option are Maho and Tree.

Rapid Clearance Point Is Defined As Programmed Rapto Value - With this option the actual programmed RAPTO parameter is output in the canned cycle block. The GPM assumes this position to be machine Z (or spindle axis) plus programmed RAPTO value for time calculations.

Rapto Value Used Only For Time Calculation - the RAPTO Value is included in the time calculations. There is no output to the machine tool.

Rapto Compensation Value - Enter the R word adjustment value ( this value is subtracted from R) for those machine tools requiring a R value. This option pertains primarily to old Cincinnati controls.

Feed Depth Point (Fedto) - defines the format for indicating the bottom of the hole.

• NOTE: Since the feed depth is a numerical value, the number of characters, decimals places sign suppression, and zero suppression should agree with the format of other numbers/coordinates the GPM outputs.

• NOTE: The bottom of the hole is the present spindle position (usually Z) plus the FEDTO value.

Select the one that describes how the Feed Depth plane should be output for your machines.

Feed Depth Output In Canned Cycle Block - the absolute value of the feed to depth position is output in the canned cycle. Most controls use this option. Specify whether the FEDTO Word Address code is modal.

Negative Incremental Distance From Rapid To Feed Depth Clearance Plane - is for the control that needs a signed distance to the bottom of the hole from the rapid clearance plane output in the canned cycle block. Controls that usually need this option are Cincinnati and Bridgeport. Specify whether the FEDTO Word Address code is modal.

Positive Incremental Distance From Rapid To Feed Depth Clearance Plane - is selected for controls that need an unsigned distance to the bottom of the hole from the rapid clearance plane output in the canned cycle block. Specify whether the FEDTO Word Address code is modal.

Programmed Fedto Value Out Put In Canned Cycle Block - the entire canned cycle is defined before any X,Y,Z coordinate output. To feed to depth plane is defined in the cycle definition block as the actual programmed FEDTO parameter. Controls that must have this option are Maho and Tree. Specify whether the FEDTO Word Address code is modal.

Fedto Value Used Only For Time Calculation - the FEDTO value is included in the time calculations. There is no output to the machine tool.

Retract Clearance Point - defines the output format for a retraction clearance plane above the rapid clearance plane during a canned cycle.

• NOTE: The command RTRCTO is the distance from the top of the hole to the retraction clearance plane.

You have the following options.

The RTRCTO Move Will Be Output After The Canned Cycle Block If The Move Is Above The RAPTO Point - When the retraction clearance plane is higher than the rapid clearance plane the retraction clearance plane will be output at rapid traverse after the canned cycle block is output. In the Rapid motion parameters menu you can specify that the cycle is turned off before the rapid traverse move. Most controls use this option.

An Automatic Retract Plane G-code Will Be Output In The Canned Cycle Block - If RTRCTO,AUTO is programmed, you can change the default G-code, 98 to another machine tool automatic cycle retract code. It is output in the same block as the canned cycle G-code. This causes a retraction to the last programmed Z value before the canned cycle by the controller after each cycle. If RTRCTO,AUTO is not programmed, a G99 is output and the controller causes retraction only to the rapid clearance plane. The postprocessor then functions the same as the previous option (The RTRCTO Move Will Be Output After The Canned Cycle Block If The Move Is Above The RAPTO Point.) Controls that use this feature are Fanuc, General Numeric, Sinumerik, Yasnac and Tosnuc.

The numerical value for the Z RTRCTO position in the G99 code is not needed. The system defaults to the CYCLE PARAMETERS menu.

The RTRCTO Move Will Be Output In The Canned Cycle Block - The retraction clearance point is output with Word Address format (usually K) in the canned cycle block. Controls that need this feature are Giddings and Lewis.

The Programmed RTRCTO Value Minus The Rapto Value Will Be Output In The Canned Cycle Block. The incremental distance from the rapid clearance point to the retraction clearance point is output in the canned cycle block. Controls that use this function are Deckel.

The Programmed RTRCTO Value Will Be Output In The Canned Cycle Block - The actual programmed RTRCTO parameter is output in the canned cycle block. The GPM assumes the final machine Z (or spindle axis) position to be machine Z plus RTRCTO. This position is used for time calculations and subsequent work plane changes.

The Programmed RTRCTO Value Will Be Used Only For Time Calculations - When you select option 6, the RTRCTO value is used only in the time calculations. There is no output to the machine tool.

Canned Cycle Cam - This allows you to define machine CAM Cycles in setting predefined depths. Usually you will want to turn off RAPTO and FEDTO. You can also use this option to output a machine tool specific parameter.

Canned Cycle Dwell - This allows you to define the format and validity of Dwell parameter in Canned Cycles. Some machines require you to specify the length of Dwell in the Canned Cycle block.

You can further specify the maximum and minimum Dwell in seconds and the conversion factor to be used for multiplying to the dwell, and make it valid for the cycle dwell.

Incremental Feeds In Deep And BRKCHP (Step) - This option defines the format for controlling the values for deep drilling and chip breaking cycles. The STEP values can have one or two numbers following it. The first value is the initial feed increment. The second value is a modifier that can alter the feed increment for successive steps.

Feed Increment (Step) Parameter Not Tape Controlled - The feed increments in this case are set manually on the control, no postprocessor output is generated for the STEP parameter.

Feed Increment (Step) Output In Canned Cycle Block - The actual programmed STEP parameter value is output in the canned cycle block in Word Address format.

Feed Increment And Feed Increment Modifier Are Both Output In Canned Cycle Block - You are prompted to specify both the program Step value and Feed Increment modifier formats. Both are output in the canned cycle block in Word Address formats.

Feed Increment Output In Block Before Cycle Motion Block (Ti and Fi For Swinc) - This is the Swinc deep and break chip cycle type. You are prompted to specify both the program Step value and Feed Increment modifier formats. Both are output in the canned cycle block in Word Address formats.

Cycle/Bore,Nodrag -This option allows you to specify the validity and value for the CYCLE/BORE,NODRAG orientation parameter.

Canned Cycle/Bore,Back - This option allows you to specify the validity and value for the CYCLE/BORE,BACK clearance parameter.

Canned Cycle Spindle Axis - The spindle axis for canned cycles can be defined in any one of the three planes, XY, YZ or ZX. A different Word Address character can be assigned to the rapid clearance point, feed to depth point, retract to clearance point and step parameters of each of the valid planes. The characters displayed in the previous options (rapid clearance point, feed to depth point, retraction clearance point, and step parameters) are for the default spindle axis.

The GPM Post Processor command SET/TOOL permits switching between different spindle axes for canned cycles such as when using a right angle head. This option also applies to work plane changes along the spindle axis for Rapid moves during cycle and non-cycle.

• NOTE: The rapid clearance point, feed to depth point, retract clearance point and step parameters must be specified before changes can be made to the canned spindle axis parameters.

Indicate the Spindle Axis validity for the spindle along the X, Y, and Z axes.

Specify the default Spindle Axis mode; either the X axis, the Y axis, the Z (W or V) axis, or specify that there is No Tape Controlled Spindle Axis and spindle axis movement is not output.

When you select Entry Complete you are prompted for the Word Address character for the Rapid Clearance Point, the Feed Depth Point, the Retract Clearance Point, the Step Increment, and the Step Modifier for each of the X, the Y, and the Z axes.

Rotary Moves Output Prior To Canned Cycle - This option allows you to output the rotary moves before or within the canned cycle block.

Cycle/On G Code (Definition Block Cycles) - this allows you to specify the validity, value, and modality of the CYCLE/ON G code. This G code executes a previously defined canned cycle. This CYCLE/ON G code is output with every Goto following a canned cycle until the cycle is cancelled. Controllers that use this option are Maho and Tree.

• NOTE: Use this option only with the XY Cycle Positioning Blocks menu option X,Y,Z Output With Cycle/On G-code To Execute Previously Defined Cycle(Maho, Tree.)

Cancel Cycle For Non Cycle Motion - allows you to specify whether the Postprocessor will output a CYCLE/OFF G code when it encounters a non-cycle motion. Example: During the canned cycle, a GOHOME is programmed. The postprocessor would output a CYCLE/OFF G CODE before outputting the GOHOME.