Content      ..     11      12      13      14     ..

9/Series CNC Lathe. Operation and Programming Manual - page 13

Chapter 14

Axis Motion

14.1.2

The format for linear interpolation mode is:

Linear Interpolation Mode

G01X ____ Z ____ F ____ ;

(G01)

Where :

Is :

G01

G01 establishes the linear interpolation mode. In linear interpolation mode, the

cutting tool is fed along a straight line at the currently programmed feedrate.

XZ

This is the location of the end point of the linear move in the current work

coordinate system.

F

The F-word represents the feedrate for axis moves that take place in the G01,

G02, and G03 modes. The F-word does not have to be programmed in the G01

block however, if the F-word is not programmed a feedrate must have been made

active in some previous block.

Linear interpolation can be performed in the absolute mode (G90), or the

incremental mode (G91).

Example 14.2

Linear Interpolation

Absolute command

Incremental command

G08;

G08;

G90G01X30.Z60.F.1;

G91G01X10.Z-65.F.1;

Figure 14.2

Results of Linear Interpolation (G01), Example 14.2

X

65

60

30

20

Z

14-3

Chapter 14

Axis Motion

Once the feedrate, F, is programmed it remains effective until another

feedrate is programmed (F is modal). You can override programmed

F-words. For details, see chapter 18.

Example 14.3

Modal Feedrates

Program Block

Comment

G91G01X10.Z20.F.1;

F.1 is effective until

Z35.;

another feedrate is

X40.Z35.;

programmed

Z44.F.3;

F.3 is effective

The feedrate for a multi-axis move is specified as the vectorial feedrate.

The control adjusts the individual axis feeds to obtain the programmed

feedrate. For details on feedrates, see chapter 18.

14.1.3

G02 and G03 establish the circular interpolation mode.

Circular Interpolation Mode

(G02, G03)

In this

The tool:

mode:

G02

moves along a clockwise arc

G03

moves along a counterclockwise arc.

Figure 14.3 shows clockwise and counterclockwise orientation relative to

the positive X and Z axes.

Figure 14.3

Circular Interpolation Direction

X

X

G02

G03

(clockwise arc)

(counterclockwise arc)

Z

Z

14-4

Chapter 14

Axis Motion

You must establish a plane before the control performs the correct arc.

This should have been done by your system installer, typically assigning

the Z and X axes to the G18 plane. This becomes the default plane that the

control assumes when:

power is turned on

E-Stop is reset

the control is reset

Circular interpolation can be performed in the absolute (G90) or

incremental (G91) mode.

Important: S--Curve Acc/Dec mode is not available with circular

interpolation mode.

The format for circular interpolation in the ZX plane is:

{G02} X__ Z__ I__ K__ F__ ;

G03

R__

Where :

Is :

X, Z

In absolute (G90) mode, these are the work coordinate values of the end point.

In incremental (G91) mode, these are the positions of the end point in reference

to the start point.

I, K

These determine the position of the arc center. They are the incremental

distance on each axis from the start point of the arc to the center point. These

values are always incremental, regardless of the established positioning mode

(absolute or incremental). I is parallel to X axis, and K is parallel to Z axis;, but

his can be configured in AMP. These are not necessary if programming the R

parameter.

R

Rather than defining a center with I, K, the option exists to define an arc radius

using R. The sign of this entry determines the arc centerpoint location. If R is

programmed as a positive value, the centerpoint is located so that an arc less

than 180°is generated. If R is programmed as a negative value, the centerpoint

is located so that an arc greater than 180°is generated. Refer to Figure 14.5 for

an example.

F

Another option is to enter a feedrate tangential to the arc. If omitted, the control

uses the feedrate active prior to this block.

14-5

Chapter 14

Axis Motion

Example 14.4

Circular Interpolation G18 (ZX Plane)

Absolute Mode

Incremental Mode

G08G02;

G08G02;

X50.Z45.I15.K0F.1;

X30.Z-15.I15.K0F.1;

or

or

G08G02;

G08G02;

X50.Z45.R15.F.1;

X30.Z-15.R15.F.1;

In Example 14.4, the K-word can be omitted. If either I or K is omitted

from the circular block, the control assumes they have a value of 0, unless

an R-word is present.

Figure 14.4

Results of Circular Interpolation, Example 14.4

X

60

15

R15

50

20

Z

When you program an arc using the radius (R) value, two arcs are possible

(Figure 14.5). Program the R-word with a positive or negative value to

distinguish between these arcs.

14-6

Chapter 14

Axis Motion

Example 14.5

Arc Programmed Using Radius

Arc 1

Arc 2

center angle less than

center angle greater than

180 degrees

180 degrees

G90G02X25.Z40.R18.F.1;

G90G02X25.Z40.R-18.F.1;

Figure 14.5

Results of An Arc Programmed with Radius Command, Example 14.5

X

Arc 2

start

R-18

point

25

Arc 1

R18

end point

Z

40

Important: Any axis that is not specified when programming a circle

remains at its current axis position value. This results in the arc’s end point

having the same coordinate value as the start point of the arc for that axis.

If you do not specify the end point of the arc, or if the end point is the same

as the start point, two results are possible:

if you use I and/or K to program the arc center, the control cuts a full

circle

if you use R to program the radius of the arc, no arc is made (the control

does not move either axis)

14-7

Chapter 14

Axis Motion

Example 14.6

Arc End Points Same As Start Points

Arc 1-Full Circle

Arc 2-No Motion

G02I-5.K5.F.1;

G02R7.07F.1;

or

or

G02X15.Z5.I-5.K5.F.1;

G02X15.Z5.R7.07F.1;

Figure 14.6

Results of An Arc with End Point Equal To Start Point, Example 14.6

Arc 1

Arc 2

Full circle

0 degree center angle arc

(no axis motion)

X

X

start

start

15

15

end

end

10

10

Center defined

Center defined by R

by I and J

Z

Z

5

10

5

10

If you program a radius command, R, in the same block as I, and/or K, the

control gives the R priority. The I-, and/or K-words are then ignored.

Important: Your system installer can specify the maximum allowed

difference between the starting radius of the arc and the ending radius of

the arc. If the difference exceeds the allowed value set in AMP, an error

occurs.

14-8

Chapter 14

Axis Motion

In incremental mode (G91), the rotary axis is programmed to move in an

angular distance (not to a specified angle as in absolute). The maximum

incremental departure depends on the programming format selected in

AMP by your system installer. The sign of the angle determines what

direction the rotary axis rotates. For example, if the current C axis position

is 25°and this block is programmed:

G91C50;

the C axis would rotate 50°in the positive direction. The new C axis

position would be 75°.

If the current C axis position is 25°and this block is programmed:

G91C-50;

the C axis would rotate 50°in the negative direction. The new C axis

position would be 335°.

In this mode:

you:

incremental (G91)

program a value greater than the rollover amount results in the rotary

axis making one or more complete revolutions.

absolute (G90)

cannot program a rotary axis move greater than the rollover amount.

circular interpolation

cannot program a rotary axis move unless these conditions are met::

(G02 or G03)

· the rotary axis cannot be in the active plane

· the rotary axis must be programmed in the same block as a valid

circular move made with the axes in the active plane

Important: You can program the largest move with a rotary axis is equal

to the rollover amount. Any attempt to program a move that generates

more motion than the rollover amount is truncated and moved to the

position that has the same numerical endpoint as the programmed position.

For example if this incremental move is programmed from a position of

10°:

G91C370;

the actual endpoint of the above move is still 20°; however, the rotary axis

did not get there by revolving one revolution. Instead, it positioned itself

directly to 20°without passing 20 once as expected.

14-10

Chapter 14

Axis Motion

Determining Rotary Axis Feedrates

The feedrate for a rotary axis is determined in much the same way as linear

axes.

When the control is in rapid mode (G00), the feedrate for the rotary axis is

the rapid feedrate for that axis as set in AMP. Remember that if other axes

are moving in the same block, the feedrate for the block is limited by the

axis that takes the longest time to complete its programmed move at its

rapid speed. (see chapter 18 for details).

When the control is in one of the cutting modes (G01, G02, or G03), the

control uses the programmed feedrate to calculate the angular velocity of

the rotary axis. This feedrate is still limited to the maximum cutting

feedrate (feedrate clamp) as determined in AMP.

When you program in this mode:

The rotary feedrate units are in:

G94 feed per minute

degrees per minute.

G95 feed per revolution

degrees per revolution of the spindle.

In any event, if a rotary axis is programmed in a block with other axis

moves in either rapid (G00) or cutting (G01, G02, or G03) modes, all axes

reach their destinations at the same instant.

CAUTION: When programming a rotary axis remember that

the programmed feedrate is in units of angular velocity. This

means that the actual cutting feedrate depends on the tools

distance from the center of rotation of the rotary axis.

14.1.5

Your system installer has the option of controlling selected axes through

the PAL program. When an axis is under PAL control, the operator and

PAL Axis Mover

part program have no control on that axis. Jog commands, as well as part

program commands, are typically ignored unless PAL has been written to

manipulate these values in some manner.

Be aware that it is possible to disable axis position displays on the CRT for

an axis under PAL control. Refer to the documentation provided by your

system installer for details on an axis controlled by PAL.

Important: S--Curve Acc/Dec mode is not available with PAL Axis

Mover.

14-11

Chapter 14

Axis Motion

14.2

Machine tools have a fixed machine home position that is used to establish

the coordinate systems. The 9/Series control offers two methods for

Automatic Motion To and

homing a machine after power up.

From Machine Home

Operation:

Description:

Manual machine home

uses switches or buttons on the MTB panel provided solely for this

purpose. Manual homing is described in detail in chapter 4.

Automatic machine home

uses a programmed machine home code.

14.2.1

You accomplish automatic homing by the using a G28 code. When

Automatic Machine Homing

programmed as the first motion block in a part program, (or through MDI)

a G28 automatically homes any axes programmed in the G28 block that

(G28)

have not yet been homed. Only axes that have their axis words

programmed in the G28 block are homed.

Homing follows the sequence of homing events described in chapter 4.

The coordinate values that are programmed with the axis words in a G28

block are stored by the control as intermediate point values (described in

the next section).

If all the axes programmed in the G28 block have already been homed

when the G28 code is executed, then the control considers it an “Automatic

Return to Machine Home” as described in the next section.

Important: When a homing request is made the feedback device for the

axis (typically an encoder) must encounter at least one marker before

tripping the homing limit switch. If the axis is close to the home limit

switch you should jog the axis away from this switch before attempting a

homing operation.

Automatic Machine Homing (G28) with Distance Coded Markers

The following outlines automatic machine homing (G28) for an axis with

DCM feedback if the axis has not already been homed:

1.

The axis moves at a speed and direction defined in AMP by G28

Home Speed and G28 Direction to Home, respectively.

The axis will come to a stop once the axis crosses three consecutive

markers on the DCM scale.

Important: To determine an absolute position using DCMs, you must

encounter at least three consecutive markers. Thus, if the axis position will

not accommodate this assumption, the axis must be moved to another

position before attempting a homing operation.

14-12

Chapter 14

Axis Motion

Figure 14.7

Automatic Return to Machine Home (G28)

Machine home

Intermediate point

Z

Usually a G28 is followed by a G29 (automatic return from machine

home) in a part program; however, the control stores the intermediate point

in memory for use with any subsequent G29 block executed before power

down. Only one intermediate point is stored for each axis. When a G28 is

programmed with a new intermediate point, any axis not programmed in

that block remains at the old value.

For example:

N1 G28 X4.0 Z3.0;

Intermediate point X=4 Z=3

N2 G28 Z2.0;

New intermediate point X=4, Z=2

Important: When the control executes a G28 or G30 block it temporarily

removes any tool offsets and cutter compensation during the axis move to

the intermediate point. The offsets and/or cutter compensation are

automatically re-activated during the first block containing axis motion

following the G28 or G30, unless that block is a G29 block. If a G29

follows, the offsets and/or cutter compensation remain deactivated on the

way to the intermediate point and are re-activated when the axis moves

from the intermediate point back to the point indicated in the G29 block.

14-14

Chapter 14

Axis Motion

14.2.3

When a G29 is executed in a part program (or through MDI), the axis or

axes move first to the intermediate point, and then to the position indicated

Automatic Return from

in the G29 block. If a G28 was just executed, then this has the effect of

Machine Home (G29)

returning the axis from machine home.

For example, executing the block:

G29 X7.0 Z1.5;

in absolute mode would move the axes to (7.0, 1.5) after passing through

the intermediate point stored in control memory. In incremental mode, this

block would move the axes to a position that is X7.0 and Z1.5 units away

from the home point.

The intermediate point is stored in control memory after a G28 return to

machine home or a G30 move to alternate home is executed. A G29 block

is usually executed after a G28 or G30 block, typically to return the cutting

tool to the part after a tool change.

Although this command moves the axes at rapid feedrate as if in G00

mode, it is not modal. If G01, G02, or G03 modes are active, they are

temporarily canceled for the return from home moves.

Only the axes specified in the G29 block are moved. For example:

N1 G28 X5.0 Z1.0;

(X and Z axes are moved to home after moving to X=5.0

Z=1.0)

N2 G29 X3.;

(X moves to X=5.0 then to X=3.0 -- -- -- Z does not move)

Example 14.7

Automatic Return From Machine Home

N00010

X100.Z50.;

N00020

Z150.;

N00030

G28X150.Z180.;

N00040

G29X200.Z100.;

14-15

Chapter 14

Axis Motion

Figure 14.8

Automatic Return From Machine Home, Results of Example 14.7

X

Machine home

200

N30

150

N40

N30

N10

N20

100

50

Z

50

100

150

200

Important: When a G29 is executed, tool offsets and/or cutter

compensation are deactivated on the way to the intermediate point, and

they are re-activated when the axis moves from the intermediate point back

to the point indicated in the G29 block.

14.2.4

A G27 causes the control to move the axes at rapid directly to the machine

Machine Home Return

home position. Only the axes included in the G27 block are moved.

Check (G27)

G27 X__ Z__;

The value entered with the axis name in the G27 block must be the

machine home coordinate for that axis. If it is not, no axis motion takes

place and the control issues the error message:

“INVALID ENDPOINT IN G27 BLOCK”

Aside from this endpoint check, the only difference between a G27 block

and a G00 block requesting a move to the machine home coordinates is

that the G27 is not modal. If G01, G02, or G03 modes were active before

the G27 was executed, they are reactivated immediately after the G27

block is completed.

G27 block commands are usually given after tool offset modes have been

cancelled.

14-16

Chapter 14

Axis Motion

14.3.2

In the G95 mode (feed per revolution), G04 suspends execution of

commands in the next block for the time it takes the controlling spindle to

Dwell - Number of Spindle

turn a designated number of revolutions.

Revolutions

G95G04

P__;

X__;

U__;

Specify the required dwell length by either a P-, X-, or U-word in units of

spindle revolutions. It does not matter which of these three words you use,

as long as only one appears in the same block. The allowable range is

0.001 - 99999.999 revolutions.

14.4

There are two types of mirroring. They are:

Mirror Image (G50.1, G51.1)

Mirror image:

Activate through:

programmable

programming a G50.1 and G51.1

manual

PAL or the {FRONT PANEL} softkey

Programmable Mirror Image (G50.1, G51.1)

Use the programmable mirror image feature to mirror (duplicate yet

reversed) axis motion commands about some defined plane. Activate this

feature using the G51.1 code. Cancel it using the G50.1 code. Mirroring

takes place about the axis position specified in the G51.1 code.

The format for the G51.1 code is:

G51.1X__ Z__ ;

The axis motion commands in any following blocks are executed with the

motion direction reversed (including incremental moves) as if a mirror

were placed on the designated point parallel with the axis. The G51.1 code

is modal and remains in effect until cancelled by a G50.1 command.

Use the axis word programmed with the G51.1 command to define the

mirroring location. The defined location intercepts the programmed axis at

the programmed position. If only one axis is programmed, the mirroring

plane is perpendicular to that axis. If more than one axis is programmed,

the mirror plane passes through these points.

Important: The control mirrors only those axes that are programmed out

in the G51.1 block. Axes not programmed in the G51.1 block execute

normally.

A G50.1 block cancels the mirror image function.

G50.1X__ Z__ ;

14-19

Chapter 14

Axis Motion

Figure 14.9

Programmable Mirror Image, Results of Example 14.8

X

120

90

Start point

75

End point

60

30

Z

0

30

60

75

90

120

When the mirror image function is active on only one of a pair of axes, the

control:

executes a reverse of programmed G02/G03 arcs. G02 becomes

counterclockwise and G03 becomes clockwise

activates a reverse of programmed G41/G42 cutter compensation. G41

becomes tool right and G42 becomes tool left

Manual Mirror Image

In addition to the programmable mirror image feature, the control can also

be equipped with an optional mirror image switch, installed by your

system installer that activates the manual mirror image feature. This

feature can also be activated by using the {FRONT PANEL} softkey.

The manual mirror image feature differs from the programmable mirror

image feature. When you use manual mirror image, the location of the

mirrored plane is fixed along the selected axis in the current work

coordinate system. This means that the mirror plane is parallel to the

selected axis. It passes through the zero point of the currently active work

coordinate system.

The mirrored plane is fixed and cannot be moved from along the selected

axis. This mirrored plane is the equivalent of programming a

programmable mirror image and using all zero values for the axis words.

14-21

Chapter

15

Using QuickPath Plus‰

15.0

The QuickPath Plus feature offers a convenient programming method to

simplify programming with the 9/Series control.

Chapter Overview

We discuss some QuickPath Plus features in this chapter. Major topics

include:

Topic:

On page:

Programming

15-2

Linear QuickPath

15-3

Circular QuickPath

15-7

This method of programming can prove useful in simplifying the

programming of a part directly from a part drawing.

The most significant advantage to the QuickPath Plus feature is the

programmer no longer has the need to calculate the endpoint of every

block or every point of intersection. QuickPath Plus determines these

points from angles and lengths.

QuickPath Plus uses these addresses:

,A

Angle

This word is used to define the angle of a tool path. This manual

assumes that the ,A-word is used. The angle is always measured

counterclockwise from the first axis defining the currently active

plane. The angle is in units of degrees.

L

Length

This word is used to define the length of a linear tool path, the

direction of which is determined by the angle (,A). It is always

interpreted as an incremental value.

The 9/Series control offers a variety of sample patterns with prompting to

aid in the programming of QuickPath Plus. These are found under the

QuickView feature described in chapter 5.

15-1

Chapter 15

Using QuickPath Plus

If an angle is programmed in a circular QuickPath Plus block, an error is

generated.

If an L-word is programmed in a G13, or G13.1 block an error is

generated.

15.2

One End Coordinate

Linear QuickPath Plus

Many times part drawings give a programmer only one axis dimension for

a tool path and require that the other axis dimension be calculated by the

angle. This QuickPath Plus feature eliminates the need for this calculation.

This must be a linear block. See section 15.3 for circular block.

The format for this block is:

,A__

X__

;

Z__

Where :

Is :

,A

Angle

This word is used to define the angle of a tool path. This manual

assumes that the ,A-word is used. The angle is a positive value when

measured counterclockwise from the first axis defining the currently active

plane and a negative value when measured clockwise. The angle is in

units of degrees.

X,Z End Point

This word is used to program one of the coordinates of the end point of a

linear path. The control calculates the other end point automatically. This

can be any axis word that is in the current plane.

Only one axes word from the current plane can be programmed in this

block. Any axis word that is not in the current plane is executed as a

normal linear move to that coordinate and combined with the QuickPath

Plus generated tool path. If both axis words from the current plane are

entered in the block, the angle is ignored and the control moves to the

coordinate position programmed with the axis words. All examples in this

section assume that the ZX plane is active.

Important: If the programmed tool path is going to be parallel to an axis

in the current plane, the axis word for the end point in the block should be

for the axis in the current plane that is not parallel to the tool path. This

means if the value of the angle (,A-word) is 0°or 180°, the second axis in

the plane must be programmed in the block. If the value of the angle is

90°or 270°, the first axis in the plane must be programmed in the block.

15-3

Chapter 15

Using QuickPath Plus

Example 15.1

Angle Designation:

N10 GO1 X0.0 Z25.0 F.1.;

N20 X15. ,A90;

N30 Z5.,A165;

Figure 15.1

Results of Angle Designation, Example 15.1

X

165°

15

10

5

Z

0

5

10

15

20

25

Important: Circular QuickPath Plus can also use an angle (,A) in a

program block. This is described in section 15.3.

No End Coordinate Known (L)

This feature of QuickPath Plus allows the programmer to define a tool path

using only the start point angle and length of a tool path. This must be a

linear block.

The format for this block is:

,A__ L__;

Where :

Is :

,A

Angle

This word is used to define the angle of a tool path. This manual assumes that

the ,A-word is used. The angle is a positive value when measured

counterclockwise from the first axis defining the currently active plane and a

negative value when measured clockwise. The angle is in units of degrees.

L Length

This word determines the length of the tool path. It is measured from the start

point to the end point of the move along a linear path. No coordinate points are

necessary.

15-4

Chapter 15

Using QuickPath Plus

Important: If any axis word from the current plane is designated in the

block, the L-word is ignored and the control calculates the end point from

the angle and the axis word. If an angle (,A) or a length (L) is

programmed in a block that also contains both axis words in the current

plane, then QuickPath Plus is not performed and the control ignores the ,A-

and the L-words in the block.

Example 15.2

Angle with Length Designation:

N10 GO1 X0. Z25. F.1.;

N20 ,A90 L15;

N30 ,A165 L20.7;

Figure 15.2

Results of Angle With Length Designation, Example 15.2

X

165°

15

10

5

Z

0

5

10

15

20

25

No Intersection Known

This feature of QuickPath Plus allows the programmer to define two

intersecting, consecutive, linear tool paths without knowing the point

where the actual intersection takes place. Both of these blocks must be

linear blocks and programmed in absolute mode. The angle of both of

these lines must be known.

This is done with a sequence of two linear blocks (in the current plane) in

which QPP is used to calculated the end point of the first block. The start

point of the first block is the current tool position.

Important: The second block of these two blocks must be programmed in

absolute mode. Any attempt to program the second block in incremental

generates an error.

15-5

Chapter 15

Using QuickPath Plus

The format for these blocks is:

N1 ,A__;

N2 ,A__Z__X__;

Where :

Is :

,A

Angle

This word is used to define the angle of a tool path. This manual

assumes that the ,A-word is used. The angle is a positive value when

measured counterclockwise from the first axis defining the currently

active plane and a negative value when measured clockwise. The

angle is in units of degrees.

ZX End Point of

These represent the actual coordinate location of the end point of the

second block

second block. They must be programmed as absolute values and

must be axes in the current plane.

Important: There may be up to four program blocks between the two

blocks in the above format. The only requirement being that these blocks

may not generate axis motion in the current plane.

Both of these blocks must be programmed in the same plane. If the current

plane is changed between these two blocks execution, the control generates

an error.

Example 15.3

QuickPath Plus When An Intersection is Unknown

N10 GO1 X0. Z25. F.1;

N20 ,A90;

N30 ,A165 X20.Z5.;

Figure 15.3

Results of Unknown Intersection, Example 15.3

X

165°

15

10

5

Z

0

5

10

15

20

25

If the control cannot determine an intersection point for the two linear

paths (for example, if the paths are parallel), an error occurs.

15-6

Chapter 15

Using QuickPath Plus

15.3

The programmer uses the Circular QuickPath when a drawing does not call

out the actual intersection of two consecutive tool paths and at least one of

Circular QuickPath Plus

the tool paths is circular. This prevents the programmer from having to do

(G13, G13.1)

any complex calculations to determine end points and start points when an

arc is involved.

For most cases of circular QuickPath Plus there may be two possible

intersection points for the two defined blocks. Define which intersection is

desired using either G13 or G13.1 in the first of the two blocks.

Programming:

Defines:

G13

the first intersection that occurs when the tool path of the first block

intersects with the second block

G13.1

the second intersection that occurs when the tool path of the first block

intersects with the second block.

Figure 15.4

G13 vs G13.1 Intersections

Second block if G13.1 programmed

Second block if G13 programmed

1st block

1st block

When programming circular QuickPath Plus, remember:

When there is only one intersection involved with the tool paths, you

can program the G13 and G13.1 codes interchangeably. One of these

G-codes must be programmed however.

The G13 or G13.1 code must be programmed in the first of the two

blocks defining the two tool paths.

If the arc is programmed with an R-word, the two tool paths must be

tangent. The sign (+ or -) of the R-word determines the arc center

location as described in section 14.1.3.

The angle word (,A) cannot be programmed in a circular block.

Both absolute coordinate values in the current plane must be

programmed for the second block. Both must be programmed

regardless of whether the final coordinates change or not.

15-7

Chapter 15

Using QuickPath Plus

Linear to Circular blocks

When the coordinates of the intersection of a linear path into a circular

path are unknown, use the following format. G13 or G13.1 must be

programmed. These blocks must be programmed in absolute.

Format:

G13G01 ,A__;

or

G13G01 ,A__;

G02 Z__X__K__I__;

G02 Z__X__R__;

Important: If the second block is an arc and it is programmed by using I,

and K integrand, the values programmed with I, and K are not measured

from the start point of the arc as normally done. This is because the start

point of the arc is normally unknown when using this format. The

integrands specify the distance from the end point of the arc to the center

point.

Example 15.4

Line Into Arc Without Programming Intersection

G00Z25.X0.;

G01G13.1,A90;

G03Z7.X15.K9.21I-2.;

Figure 15.5

Results Of Line into Arc Without Intersection, Example 15.4

X

135°

20

R 10.0

15

I

K

10

5

90°

Z

5

10

15

20

25

Important: You cannot program R to specify the arc radius for

linear-to-circular block combinations unless the two tool paths are tangent.

15-8

Chapter 15

Using QuickPath Plus

Circular to Linear blocks

When the coordinates of the intersection of a circular path into a linear

path are unknown, use the following format. G13 or G13.1 must be

programmed in the first of the two blocks. These blocks must be

programmed in absolute.

Format:

G13G02I__K_;

or

G13G02R__;

G01,A__Z__X__;

G01,A__Z__X__;

Important: K values are the normal integrand values when you use this

format (measured from start point of arc to arc center).

Example 15.5

Arc Into Line Without Programming Intersection Point

G0X0Z0.;

G13G03K4I10F.1;

G01,A0X10Z20;

Figure 15.6

Results of Arc Into Line Without Intersection, Example 15.5

X

Control generates

intersection

10

8

6

4

2

Z

8

10

12

14

16

18

20

2

6

4

Important: R cannot be programmed to specify the arc radius for linear to

circular block combinations unless the two tool paths are tangent.

15-9

Chapter 15

Using QuickPath Plus

Circular to Circular blocks

When the coordinates of the point of intersection of a circular path into a

circular path are unknown, use the following format. G13 or G13.1 must

be programmed. If using this format, the R-word cannot be used to

specify the radius of an arc in either of the circular blocks. These blocks

must be programmed in absolute.

Format:

G13G02K__I__;

G02 Z__X__K__I__;

Important: The I, K integrand vectors are not necessarily the same values

as discussed for normal circular interpolation when you use this QuickPath

Plus format. The integrands of the first circular block specify the distance

from the START point to the center of the circle. The integrands of the

second circular block specify the distance from the END point to the center

of the circle (this is the reverse of normal). At least one of these integrand

words must be programmed in each of the two circular blocks.

Neither circular block can contain an angle word (,A) when you use this

format.

Example 15.6

Arc Into Arc Without Programming Intersection

G0X0.Z0.;

G13.G03I5F.1;

G02X12Z5I-2.75K2;

Figure 15.7

Results Arc Into Arc Without Intersection, Example 15.6

X

12

10

+

8

Control generates

6

intersection

4

2

Z

2

4

6

8

10

END OF CHAPTER

15-10

Content      ..     11      12      13      14     ..