8.

Programming manual

8.3

Collision detection (G41 N, G42 N)

Using this option, the CNC analyzes in advance the blocks to be executed in order to detect loops

(profile intersections with itself) or collisions of the programmed profile. The number of blocks to be analyzed (up to 50) may be defined by the user.

The example shows machining errors (E) due to a collision in the programmed profile. This type of errors may be avoided using collision detection.

When detecting a loop or a collision, the blocks that caused it will not be executed and a warning will be issued for each loop or collision eliminated.

Possible cases: a step on a straight path, a step in a circular path and tool radius compensation too large.

The information contained in the eliminated blocks, not being the moving in the active plane, will be executed (including the movements of the axes).

Block detection is defined and activated with tool radius compensation functions G41 and G42. A new parameter N (G41 N y G42 N) has been added to activate the feature and define the number of blocks to analyze.

Possible values from N3 to N50. Without "N", or with N0, N1 and N2 , it behaves like in older versions.

In CAD generated programs that are made up of lots of very short blocks, it is recommended to use very low N values (around 5) so as not to jeopardize block processing time.

When this function is active, the history of active G functions shows G41 N or G42 N.

CNC 8055

CNC 8055i

·T· M ODEL

S OFT : V01.6

X

·148·

CANNED CYCLES

9

This CNC offers the following machining canned cycles:

G66 Pattern repeat canned cycle.

G68

G69

Stock removal cycle along X axis.

Stock removal canned cycle along Z axis.

G81

G82

G83

G84

Turning canned cycle with straight sections.

Facing canned cycle with straight sections.

Drilling canned cycle.

Turning canned cycle with arcs.

G85

G86

G87

G88

G89

Facing canned cycle with arcs.

Longitudinal threading canned cycle.

Face threading canned cycle.

Grooving canned cycle along the X axis.

Z axis grooving canned cycle.

Machining canned cycles with live tool:

G60 Face drilling / tapping canned cycle.

G61

G62

G63

Drilling / tapping canned cycle on the side of the part.

Slot milling canned cycle on the side of the part.

Slot milling canned cycle on the face of the part

A canned cycle is defined by the G function indicating the canned cycle and its corresponding parameters. A canned cycle may be defined anywhere in the program, that is, in the main program as well as in a subroutine.

When working in a plane other than the ZX, for example: G16 WX, the CNC interprets the canned cycle parameters as follows:

Parameter Z and all those related to it, with the abscissa axis.

Parameter Z and all those related to it, with the ordinate axis.

ZX plane

Z axis

X axis

WX plane

W axis

X axis

AB plane

A axis

B axis

CNC 8055

CNC 8055i

·T· M ODEL

S OFT : V01.6

X

·149·