2.4.7 Tapping with compensating chuck - CYCLE840

Size: px

Start display at page:

Download "2.4.7 Tapping with compensating chuck - CYCLE840"

Conrad Page
5 years ago
Views:

1 2.4.7 Tapping with compensating chuck - CYCLE840 Programming CYCLE840 (RTP, RFP, SDIS, DP, DPR, DTB, SDR, SDAC, ENC, MPIT, PIT, AXN) Parameters Parameter Data type Description RTP REAL Retraction plane (absolute) RFP REAL Reference plane (absolute) SDIS REAL Safety clearance (enter without sign) DP REAL Final drilling depth (absolute) DPR REAL Final drilling depth relative to the reference plane (enter without sign) DTB REAL Dwell time at thread depth (chip breakage) SDR INT Direction of rotation for retraction Values: 0 (automatic direction reversal), 3 or 4 (for M3 or M4) SDAC INT Direction of rotation after end of cycle Values: 3, 4 or 5 (for M3, M4 or M5) ENC INT Tapping with/without encoder Values: 0 = with encoder, 1 = without encoder MPIT REAL Thread lead as a thread size (signed): Range of values 3 (for M3) to 48 (for M48) PST REAL Thread lead as a value (signed) AXN INT Range of values: mm Tool axis Values 1) : 1: 1st axis of the current plane 2: 2nd axis of the current plane 3: 3rd axis of the current plane 1) The definition of the 1st, 2nd, and 3rd axes depends upon the current plane selected. Function The tool drills at the programmed spindle speed and feedrate to the entered final thread depth. This cycle is used to program tapping with the compensating chuck: Without encoder With encoder. Programming and Operating Manual, 12/2012, 6FC5398-4DP10-0BA0 141

2 Sequence Tapping with compensating chuck without encoder Position reached prior to cycle start: The drilling position is the position in the two axes of the selected plane. The cycle creates the following sequence of motions: Approach of the reference plane brought forward by the safety clearance by using G0 Tapping to the final drilling depth Dwell time at tapping depth (parameter DTB) Retraction to the reference plane brought forward by the safety clearance Retraction to the retraction plane with G0 Sequence of operations Tapping with compensating chuck with encoder Position reached prior to cycle start: The drilling position is the position in the two axes of the selected plane. 142 Programming and Operating Manual, 12/2012, 6FC5398-4DP10-0BA0

3 The cycle creates the following sequence of motions: Approach of the reference plane brought forward by the safety clearance by using G0 Tapping to the final drilling depth Dwell time at thread depth (parameter DTB) Retraction to the reference plane brought forward by the safety clearance Retraction to the retraction plane with G0 Explanation of the parameters For the parameters RTP, RFP, SDIS, DP, DPR, refer to Section "Drilling, centering - CYCLE81 (Page 122)". DTB (dwell time) The dwell time must be programmed in seconds. SDR (direction of rotation for retraction) SDR=0 must be set if the spindle direction is to reverse automatically. If the machine data is defined such that no encoder is set (in this case, machine data MD30200 $MA_NUM_ENCS is 0), the parameter must be assigned the value 3 or 4 for the direction of rotation; otherwise, alarm "No spindle direction programmed" is output and the cycle is aborted. SDAC (direction of rotation) Because the cycle can also be called modally (see Section "Graphical cycle support in the program editor (Page 118)"), it requires a direction of rotation for tapping further threaded holes. This is programmed in parameter SDAC and corresponds to the direction of rotation programmed before the first call in the higher-level program. If SDR=0, the value assigned to SDAC has no meaning in the cycle and can be omitted in the parameterization. ENC (tapping) If tapping is to be performed without encoder although an encoder exists, parameter ENC must be assigned value 1. If, however, no encoder is installed and the parameter is assigned the value 0, it is ignored in the cycle. Programming and Operating Manual, 12/2012, 6FC5398-4DP10-0BA0 143

4 MPIT and PIT (thread lead as a thread size and as a value) The parameter for the lead is only relevant if tapping is performed with encoder. The cycle calculates the feedrate from the spindle speed and the lead. The value for the thread lead can be defined either as the thread size (for metric threads between M3 and M48 only) or as a value (distance from one thread turn to the next as a numerical value). Any parameters not required are omitted in the call or assigned the value zero. If the two lead parameters have conflicting values, alarm "Thread lead wrong" is generated by the cycle and cycle execution is aborted. Note Depending on the settings in machine data MD30200 $MA_NUM_ENCS, the cycle selects whether tapping is to be performed with or without encoder. The direction of rotation for the spindle must be programmed with M3 or M4. In thread blocks with G63, the values of the feedrate override switch and spindle speed override switch are frozen to 100%. A longer compensating chuck is usually required for tapping without encoder. AXN (tool axis) The following figure presents the options for the drilling axes to be selected. With G17: AXN=1; Corresponds to X AXN=2; Corresponds to Y AXN=3; Corresponds to Z 144 Programming and Operating Manual, 12/2012, 6FC5398-4DP10-0BA0

5 Using AXN (number of the drilling axis) to program the drilling axis enables the drilling axis to be directly programmed. AXN=1 AXN=2 AXN=3 1st axis of the current plane 2nd axis of the current plane 3rd axis of the current plane For example, to machine a hole in the G17 plane with Z axis, you program: G17 AXN=3 Programming example: Tapping without encoder In this program, a thread is tapped without encoder at position X35 Y35 in the XY plane; the tapping axis is the Z axis. The parameters SDR and SDAC for the direction of rotation must be assigned; parameter ENC is assigned the value 1, the value for the depth is the absolute value. Lead parameter PIT can be omitted. A compensating chuck is used in machining. N10 G90 G0 T11 D1 S500 M3 N20 G17 X35 Y35 Z60 N30 G1 F200 ; Specification of technology values ; Approach drilling position ; Setting the path feedrate N40 CYCLE840(20,0,3,-15,,1,3,4,1,6,,3) Cycle call, dwell time 1 s, direction of rotation for retraction M4, direction of rotation after cycle M3, no safety clearance, parameters MPIT and PIT have been omitted N50 M02 ; End of program Programming and Operating Manual, 12/2012, 6FC5398-4DP10-0BA0 145

6 Programming example: Tapping with encoder In this program, a thread is tapped with encoder at position X35 Y35 in the XY plane. The drilling axis is the Z axis. The lead parameter must be defined, automatic reversal of the direction of rotation is programmed. A compensating chuck is used in machining. N10 G90 G0 T11 D1 S500 M4 N20 G17 X35 Y35 Z60 N30 CYCLE840(20,0,3,-15,,1,3,4,1,6,,3) N40 M02 ; Specification of technology values ; Approach drilling position ; Cycle call, without safety clearance, with absolute depth specification ; End of program 146 Programming and Operating Manual, 12/2012, 6FC5398-4DP10-0BA0

CHAPTER 12. CNC Program Codes. Miscellaneous CNC Program Symbols. D - Tool Diameter Offset Number. E - Select Work Coordinate System.

CHAPTER 12. CNC Program Codes. Miscellaneous CNC Program Symbols. D - Tool Diameter Offset Number. E - Select Work Coordinate System. General CHAPTER 12 CNC Program Codes The next three chapters contain a description of the CNC program codes and parameters supported by the M-Series Control. The M-Series Control has some G codes and parameters