5.2.1 Drilling, centering CYCLE81

Programming:

CYCLE81 (RTP, RFP, SFD, DEP, RDP)

Parameters:

RTP

Real

Retraction plane (absolute)

RFP

Real

Reference plane (absolute)

SFD

Real

Safety clearance (enter without sign)

DEP

Real

Final drilling depth (absolute)

RDP

Real

Final drilling depth relative to the reference plane (enter without sign

                                                       Fig.5.1 CYCLE81

Explanation of parameters:

1. RFP and RTP (reference plane and retraction plane): Normally, reference plane (RFP) and return plane (RTP) have different values. The cycle assumes that the retraction plane precedes the reference plane. This means that the distance from the retraction plane to the final drilling depth is larger than the distance from the reference plane to the final drilling depth.

2. SFD(safety clearance): The safety clearance (SFD) acts with reference to the reference plane. This is brought forward by the safety clearance. The direction in which the safety clearance is active is automatically determined by the cycle.

3. DEP and RDP(final drilling depth): The final drilling depth can be specified either absolute (DEP) or relative (RDP) to the reference plane. With relative specification, the cycle will calculate the resulting depth automatically using the positions of reference and retraction planes.

Function:

The tool drills at the programmed spindle speed and feedrate to the entered final drilling depth.

Sequence:

1. Approach of the reference plane brought forward by the safety clearance by using G00

2. Traversing to the final drilling depth at the feedrate programmed in the calling program (G01)

3. Retraction to the retraction plane with G00

Example:

This program produces one hole on the end face using the CYCLE81 drilling cycle. The drilling axis is always the Z axis. Programming zero point is the center of end face.

N10 G00 G90 G17 G40 T1 D1 S400 M03

Specification of technology values

N20 G95 G01 Z10 X0 F0.2

Approach drilling cycles starting position

N30 CYCLE81(10, 0, 1, -5, 5)

Cycle call

N40 G00 Z10

Next position

N50 M02

End of program

0 (0)
Article Rating (No Votes)
Rate this article
Attachments
There are no attachments for this article.
Comments
There are no comments for this article. Be the first to post a comment.
Full Name
Email Address
Security Code Security Code
Related Articles RSS Feed
1.3 Subroutine
Viewed 1483 times since Thu, Aug 25, 2016
2.2 Dimensions in metric units and inches: G70/G71
Viewed 1433 times since Thu, Aug 25, 2016
2.6 Work plane G17/G18/G19
Viewed 4012 times since Thu, Aug 25, 2016
5.2.6 Boring (boring 2) CYCLE86
Viewed 11099 times since Fri, Aug 26, 2016
1.6 Program structure
Viewed 1450 times since Thu, Aug 25, 2016
5.2.2 Drilling, counterboring CYCLE82
Viewed 1989 times since Fri, Aug 26, 2016
3.2 Tool offset number D
Viewed 1296 times since Fri, Aug 26, 2016
2.9 Exact stop/continuous-path control mode: G09/G60/G64
Viewed 1894 times since Thu, Aug 25, 2016
5.2.9 Reaming 2 (boring 5) CYCLE89
Viewed 1255 times since Fri, Aug 26, 2016
1.8 G function group
Viewed 1670 times since Thu, Aug 25, 2016