5.2.8 Drilling with stop 2 (boring 4) CYCLE88

Programming:

CYCLE88 (RTP, RFP, SFD, DEP, RDP, DTB, SDIR)

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)

DTB

Int

Dwell time at final drilling depth (chip breakage)

SDIR

Int

Direction of rotation Values: 3 (for M03), 4 (for M04)

 

                                                                  Fig.5.9 CYCLE88

Function:

The tool drills at the programmed spindle speed and feedrate to the entered final drilling depth. During boring pass 4, a dwell time, a spindle stop without orientation M05 and a programmed stop M 0 are generated when the final drilling depth is reached. Pressing the NC START key traverses the outward movement at rapid traverse until the retraction plane is reached.

Sequence:

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

2. Traversing to final drilling depth with G1 and the feedrate programmed prior to the cycle call

3. Dwell time at final drilling depth

4. Spindle stop with M05, program stop with M00

5. Press the NC START key.

6. Retraction to the retraction plane with G00

Explanation of the parameters:

1. For parameters RTP,RFP,SFD,DEP,RDP, see CYCLE81;

2. DTB(dwell time): The dwell time to the final drilling depth is programmed under DTB in seconds.

3. SDIR(direction of rotation): This parameter determines the direction of rotation with which the drilling operation is carried out in the cycle. If values other than 3 or 4 (M03/M04) are generated, alarm is generated and the cycle is aborted.

Example:

CYCLE88 is used for boring with stop 2. The drilling axis is the Z axis. Programming zero point is the center of end face. Dwell time is 1 second.

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 CYCLE88(10, 0, 1, -20, 20, 1, 3)

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
3.4 Tool group TGROUP
Viewed 1684 times since Fri, Aug 26, 2016
6.1 Outer contouring
Viewed 1499 times since Fri, Aug 26, 2016
2.6 Work plane G17/G18/G19
Viewed 6314 times since Thu, Aug 25, 2016
5.3.3 Rough turning CYCLE95
Viewed 11250 times since Fri, Aug 26, 2016
3.2 Tool offset number D
Viewed 1696 times since Fri, Aug 26, 2016
1.9 M function group
Viewed 8479 times since Thu, Aug 25, 2016
5.3.5 Thread cutting CYCLE97
Viewed 6170 times since Fri, Aug 26, 2016
5.2.2 Drilling, counterboring CYCLE82
Viewed 2442 times since Fri, Aug 26, 2016
5.2.6 Boring (boring 2) CYCLE86
Viewed 11855 times since Fri, Aug 26, 2016
5.2.5 Reaming1 (boring 1) CYCLE85
Viewed 10348 times since Fri, Aug 26, 2016