Linear Pattern G72.2

We have seen how the circular copy of the program is done. Now we will see how the linear of the program is copied. 

Just like a copy of a program circular is done in a linear copy. 

Only a few changes are made in the circular copy, the rest is just like the circular program. So let's see the linear copy of the program.

The programming format is

G72.2...P...L...I...J...R...

L is a no. of program in linear(compulsory)

I is program shift in X direction
J is program shifting in Y direction

Main Program

%

O0001

N1 G0 G90 G54 X0 Y0 M3 S200 (Point A)

N2 Z5

N3 G01 Z0 F300

N4 X10 Y25 (Point B)

N5 G72.2 P0002 L3  I50

N6 G90 G01 X180 Y25 F300

N7 G0 Z100

N8 M30

%

Subprogram

O0002

N1 G91 G01 X20  (Point C)

N2 Y30 (Point D)

N3 X30 (Point E)

N4 Y-30 (Point F) 

N5 M99

%

Read More

Circular Milling Using Macro Variable

All parameter in form of variable while you make a program of circular milling. 

You just have to set only cutter diameter and hole diameter. This program is automatically calculate path of rotation.

Now see step by step what i did.

Hole Milling

%

O0001

N1 #100=12 (Hole Diameter)

N2 #101=8 (Cutter Diameter)

N3 #102=#100 - #101 (Center Distance)

N4 #103=#102/2 (Calculation)

N5 #104=1 (First Depth of cut)

N6 #105=1 (Global Depth of cut)

N7 #106=15 (Total Depth of cut)

N8 G0 G91 G28 Z0

N9 G90 G54 X0 Y0 M03 S2000

N10 Z5

N11 WHILE[#104LE#106]DO1

N12 G1 Z-#104 F200

N13 X-#103

N14 G03 X#103 I#103

N15 X-#103 I-#103

N16 #104=#104+#105

N17 END1

N18 G01 Z5 F200

N19 G0 G91 G28 Z0

N20 M05

N21 M30

%

Here i make only program for hole milling while i using climb milling, but whenever you make a program for boss milling you should change parameter of above program. 

There are only two changes made in program in line no. 3 and line no. 14.

Now we are using G02 for climb boss milling and  equation should be like this  #102=#100+#101 instead of subtraction. 

Read More

Loop: While...Do...

While Do loop is used when a pass in a program is constantly repeat.

There are main three logic are used in this loop.

LT: Less than

LE: Less than or equal to

GT: Greater than

GE: Greater than or equal to

For example

from XOYO (Left Front Corner)to

N01 X200

N02 Y100

N03 X0

N04 Y0

Here shown program is rectangular single planner pass at some height. Now this pass is continuously repet in at some depth. So the conventional program like. If depth of cut is 5 mm(only for understanding) and depth is 15 mm than

%

O0001

N1 G0 G91 G28 Z0

N2 G90 G54 X0 Y0 M03 S2000

N3 Z5

N4 G01 Z-5 F200

N10 X200

N11 Y100

N12 X0

N13 Y0

N14 Z-10

N15 X200

N16 Y100

N17 X0

N18 Y0

N19 Z-15

N20 X200

N21 Y100

N22 X0

N23 Y0

N29 Z5

N30 G0 G91 G28 Z0

N31 M05

N32 M30

%

So now the While...DO... program is done in such a way.

%

O0001

#100=5 (First depth of cut variable)

#101=5 (Global depth of cut variable)

#102=15 (Total Depth)

G0 G91 G28 Z0

G90 G54 X0 X0 M03 S2000

WHILE[#100LE#102]DO1 (Looping below pass until #100 does not get less than or equal to #102)

G1 Z-#100 F200

X200

Y100

X0

Y0

#100=#100+#101 (additional for next cut)

END1 (loop end)

Z5

G0 G91 G28 Z0

M05

M30

%

Simulation

Read More

Simple Calculation for Hole and Boss Milling

During hole and boss milling there are center distance of cutter axis and hole/boss center is very important.

This CD is defined the pitch circle diameter of cutter rotation. One condition is affect on hole milling that the cutter diameter is greater than half of hole diameter and stating point of program must be at center of hole/boss.

Formula of hole milling from the fig.

CD= (Hole Diameter - Cutter Diameter)/2

For Boss milling

CD= ( Boss Diameter + Cutter Diameter)/2

For example

The hole is 12mm of Dia. and cutter Dia. is 8mm than...

• CD = (12-8)/2
• CD = 2

Program:

N01 G01 X2 F200
N02 G03 X-2 R2
N03 X2 R2

And if Boss dia. is 15mm and cutter dia. 10mm than

• CD =(15+10)/2
• CD = 12.5

Program:

N01 G01 X-12.5 F200
N02 G02 X12.5 R12.5
N03 X-12.5 R12.5

Read More