G04 (Dwell) The G04 code is used to enter a set time delay into the program (called a "dwell"). A G04 command is written in the following format: G04 X _ _ _ _ ; or G04 P _ _ _ _ ; where, The dwell value is programmed using the address letters X (time in seconds) or P (time in 1/1000 seconds), followed by a number indicating this dwell value. For example, G04 X1.5 ; This command is read perform a dwell of 1.5 seconds duration. For example, G04 P2500 ; This command is read perform a dwell of 2.5 seconds duration . Note: G04 U2.0 Preferred at lathe only (seconds)

G73 - G89 (Canned Cycles):

G73 - G89 (Canned Cycles) A canned cycle simplifies the program by replacing complex machining sequences, programmed by several blocks of information, with just one or two blocks

Sequence of Six Operations:

Sequence of Six Operations Operation 1 - Positioning of the X and Y axes Operation 2 - Rapid traverse in the Z axis to the "R" point Operation 3 - Hole machining procedure Operation 4 - Operation at bottom of hole Operation 5 - Retraction to R point Operation 6 - Rapid traverse in the Z axis to the Initial level

Return Point Level Command Modes:

Return Point Level Command Modes

Types:

Types G81 Drilling canned cycle G82 Drilling canned cycle with variable peck (drilling step) G83 Deep hole drilling canned cycle with constant peck (drilling step) G84 Tapping canned cycle G85 Reaming canned cycle G86 Boring canned cycle G87 Rectangular pocket canned cycle G88 Circular pocket canned cycle Other functions related to canned cycles: G80 Canned cycle cancellation G98 The tool, after the canned cycle is done, returns to the starting plane G99 The tool, after the canned cycle is done, returns to the reference plane

Influence zone of a canned cycle:

Influence zone of a canned cycle The canned cycle is modal. Once a canned cycle has been defined, by program or MDI/MDA, it stays active until its cancellation is programmed or until one the conditions that cancels it occurs Canned cycle cancellation: A cycle is cancelled as follows Using function G80 that may be programmed in any block After defining a new canned cycle. The new canned cycle cancels and replaces any other cycle that may be active After executing M02, M30 or after an emergency or reset When doing a home search using function G74 Selecting another longitudinal axis, with G20 or with #TOOL AX Selecting a new work plane

Canned Cycle Format:

Canned Cycle Format The format for machining data in a canned cycle is written as follows: (G90 or G91) (G98 or G99) G.... X.... Y.... R.... Z.... P.... Q.... I.... J.... F.... K....; where, G.... is defined as the canned cycle X.... Y.... is defined as the hole position, in absolute or incremental value R.... is defined as the distance from the initial level to the R point level in incremental mode, or the position of the Z datum in relation to the R point level in absolute mode Z.... is defined as the distance from the R point to the bottom of the hole in incremental mode, or the position of the hole bottom in absolute mode P.... is defined as the dwell time to be performed at the bottom of the hole Q.... is defined as the cut-in distance value or shift value (Incremental value) I.... J.... is defined as the shift amount in the direction of X & Y simultaneously F.... is defined as the feedrate for machining K.... is defined as the number of repeats, for a series of holes. When not specified, K=1. The addresses P and Q are omitted within some canned cycles Once the drilling data has been specified and read into the machine controller, it is retained until it is either changed, or the canned cycle cancelled. All the required data must be specified when the canned cycle is started and only the data to be changed has to be specified during the cycle

Canned Cycle Example Programs:

Canned Cycle Example Programs The following example shows a canned cycle for drilling 4 holes, where the third hole is to be machined 10mm deeper: G90 G99 G81 X10 Y10 Z-15 R2 F100 ; X20 ; (X axis move) X30 Z-25 ; (X and Z change) X40 Z-15 ; (X and Z change) G80 ; (Cancel) The following example shows a repeat canned cycle: G91 G99 G81 X10 Y6 Z-10 R-8 K4 F100 ;

G81 (Drilling - Spot Boring):

G81 (Drilling - Spot Boring) A G81 (Drilling - Spot Boring) command is written in the following format: (G90 or G91) (G98 or G99) G81 X.... Y.... R.... Z.... F.... ; Sequence of moves: Op 1) Rapid position to X, Y and Z (the Initial level). Op 2) Rapid traverse to R point level. Op 3) Feed to Z depth. Op 4) Rapid traverse to Initial level (G98) or R point level (G99) Mainly used for drilling and centre drilling If used for boring, G81 produce a scratch on the hole cylinder during retract

G82 (Drilling - Counter Boring) A G82 (Drilling - Counter Boring) command is written in the following format: (G90 or G91) (G98 or G99) G82 X.... Y.... R.... Z.... P.... F.... ; Sequence of moves: Op 1) Rapid position to X, Y and Z (the Initial level). Op 2) Rapid traverse to R point level. Op 3) Feed to Z depth. Op 4) Dwell for value P. Op 5) Rapid traverse to Initial level (G98) or R point level (G99). Used for center drilling, spot drilling, spot facing, countersinking, etc Anytime a smooth finish is required at the bottom of the hole

G83 (Deep Hole Peck Drilling):

G83 (Deep Hole Peck Drilling) A G83 (Deep Hole Peck Drilling) command is written in the following format: (G90 or G91) (G98 or G99) G83 X.... Y.... Z.... Q.... F.... ; G.... is defined as the canned cycle. X.... Y.... is defined as the hole position, in absolute or incremental value. Z.... is defined as the distance from the R point to the bottom of the hole in incremental mode, or the position of the hole bottom in absolute mode. R.... is defined as the distance from the initial level to the R point level in incremental mode, or the position of the Z datum in relation to the R point level in absolute mode P.... is defined as the dwell time to be performed at the bottom of the hole (see the G04 code for more details). Q.... is defined as the cut-in distance value or shift value (Note - this is always specified as an incremental value). K.... is defined as the number of repeats, for a series of holes. When not specified, K=1. F.... is defined as the feedrate for machining Sequence of moves: Op 1) Rapid position to X, Y and Z (the initial level). Op 2) Rapid traverse to R point level. Op 3) Feed in to the value of Q. Op 4) Rapid traverse out to R point. Rapid traverse back to within 1mm of depth of Q cut. Operation moves 2 and 4 are repeated until Z depth is reached. Op 5) Rapid traverse to Initial level (G98) or R point level (G99).

G73 (High Speed Peck Drilling):

G73 (High Speed Peck Drilling) A G73 (High Speed Peck Drilling) command is written in the following format: (G90 or G91) (G98 or G99) G73 X.... Y.... R.... Z.... Q.... F....; The drill will rapid traverse to the R point level and begin to feed in, until a cut-in distance of Q is attained At this point, the drill will retract a small distance (set within the machine controller). A cut-in distance of Q at the same feedrate will begin again, followed by a similar retraction These movements will continue until the total Z depth has been reached

G84 (Tapping):

G84 (Tapping) A G84 (Tapping) command is written in the following format: (G90 or G91) (G98 or G99) G84 X.... Y.... R.... Z.... P.... F.... ; Sequence of moves: Op 1) Rapid position to X, Y and Z (the initial level). Op 2) Rapid traverse to R point level. Op 3) Feed to Z depth. Op 4) Dwell P (time for spindle stop and start CCW direction). Op 5) Feed to R point level. Op 6) Dwell P (time for spindle stop and start CW direction). If the G98 code is programmed within the cycle, the next move will be a rapid traverse to the Initial level. If the G99 code is programmed within the cycle, there will be no movement. F (Feed) = RPM x Pitch

G74 (Counter Tapping):

G74 (Counter Tapping) A G74 (Counter/Left Hand Tapping) command is written in the following format: (G90 or G91) (G98 or G99) G74 X.... Y.... R.... Z.... P.... F....; Sequence of moves: Op 1) Rapid position to X, Y and Z (the Initial level). Op 2) Rapid traverse to R point level. Op 3) Feed to Z depth. Op 4) Dwell P (time for spindle stop and start CW direction). Op 5) Feed to R point level. Op 6) Dwell P (time for spindle stop and start CCW direction). If the G98 code is programmed within the cycle, the next move will be a rapid traverse to the Initial level. If the G99 code is programmed within the cycle, there will be no movement. F (Feed) = RPM x Pitch

G85 (Boring):

G85 (Boring) A G85 (Boring) command is written in the following format: (G90 or G91) (G98 or G99) G85 X.... Y.... R.... Z.... F.... ; Sequence of moves: Op 1) Rapid position to X, Y and Z (the initial level). Op 2) Rapid traverse to R point level. Op 3) Feed in to the Z depth. Op 4) Feed back to R point level. If the G98 code is programmed within the cycle, the next move will be a rapid traverse to the Initial level. If the G99 code is programmed within the cycle, there will be no movement. ALSO known as Reaming canned cycle

G86 (Boring):

G86 (Boring) A G86 (Boring) command is written in the following format: (G90 or G91) (G98 or G99) G86 X.... Y.... Z.... R.... F....; Sequence of moves: Op 1) Rapid position to X, Y and Z (the initial level). Op 2) Rapid traverse to R point level. Op 3) Feed to Z depth and spindle stop. Op 4) Rapid traverse to the initial level and spindle CW for G98, or rapid traverse to R point level and spindle CW for G99.

G87 Back Boring:

G87 Back Boring

G88 – Boring cycle:

G88 – Boring cycle The G88 cycle is intended for boring. This cycle uses a P value, where P specifies the number of seconds to dwell. Preliminary motion, as described above. Move the Z-axis only at the current feed rate to the Z position. Dwell for the given number of seconds. Stop the spindle turning. Stop the program so the operator can retract the spindle manually. Restart the spindle in the direction it was going. It is unclear how the operator is to manually move the tool because a change to manual mode resets the program to the top. We will attempt to clarify that step in this procedure

G89 – Boring cycle:

G89 – Boring cycle The G89 cycle is intended for boring. This cycle uses a P value, where P specifies the number of seconds to dwell. Preliminary motion, as described above. Move the Z-axis only at the current feed rate to the Z position. Dwell for the given number of seconds. Retract the Z-axis at the current feed rate to clear Z. This cycle is like G82 except that the tool is drawn back at feed rate rather than rapid Circular pocket canned cycle G88 G98/G99 X Y Z I J B C D H L V Boring cycle with withdrawal at feedrate G89 G98/G99 X Y Z I K

G76 – Precision Boring cycle:

G76 – Precision Boring cycle

Thanks:

Thanks M.Ganesh Murugan

You do not have the permission to view this presentation. In order to view it, please
contact the author of the presentation.