Romi M27 - Fanuc 21i-TB

[cappy]

Hello,

 

Can someone post any examples of NC code G76 canned cycle threading for this machine.

 

Just installed machine and I am beginning on getting some post edits together for our reseller.

 

I have started with MPLFAN.pst and it gives me this for a 1.967-18 rh thread.

 

O0001

(PROGRAM NAME - TEST)

(DATE - 02-23-11)

(TIME - 4:54 PM)

N10 G20

(TOOL - 4 OFFSET - 4)

(NT3R THREADER INSERT - NT3R(18))

N15 G28 U0. W0.

N20 G50 X10. Z15.34

N25 G0 T0404

N30 M8

N35 G97 S200 M03

N40 G0 X2.167 Z12.8564

N45 Z3.2425

N50 G76 P010029 Q0. R0.

N55 G76 X1.8988 Z2.5395 P341 Q54 R0. E.05556

N60 M09

N65 G28 U0. W0. M05

N70 T0400

N75 M30

 

Thanks in advance.

Greg.

[cappy]

Hello,

 

Found this on the web. I thought I would post it if anyone else is looking for this info.

 

Tooling & Production June 2003

"Shop Talk with Steve Rose"

 

 

 

Threading Methods

 

There are three programming methods available for programming on Fanuc based controls. We’ll look at the benefits of each method in the next few articles of Shop Talk.

The production of an external or internal thread requires several passes with a single-point threading tool. The deeper the thread, the greater the number of passes required to produce that thread.

The traditional threading method uses G32/G33 codes. These commands require four lines of program code for each thread pass. For example, machining a 3/4 - 10 external thread could require 10 - 14 threading passes resulting in 40 - 56 lines of code.

Typically in a single pass threading routine the depth is reduced in each pass as the diameter gets smaller. Reducing the depth in this manner is necessary to balance the load on the insert. As the insert goes deeper into the material the area of contact between the tool and the part increases. To minimize this contact area, smaller pass depths are programmed as the insert approaches its final depth. Your insert supplier’s catalog has information regarding the number of passes needed for a specific thread.

There are two alternative programming methods to reduce the programming effort. Today we’ll review G76; this canned cycle method is very popular and suitable for many threading applications. Only 1-2 lines of information must be programmed, depending upon the type of control.

A Fanuc 0/18/21 control is often programmed with 2 lines of code as follows. Let’s use a 7/8 - 9 TPI thread in a modal program as an example. First, use the Machinist Handbook to determine the major (outside) and minor (root) diameter of the thread. Then, calculate the thread depth as follows.

 

thread depth = (major ø - minor ø ) ÷ 2

 

1111 (thread 7/8 - 9 TPI) ;

N10 G00 G40 G99 ;

N20 G97 S1090 M13 ; (spindle direction & coolant)

N30 T0303 ; (tool & offset)

N40 X0.955 Z0.444 ; (start position)

N50 G76 P010060 Q0050 R0.0005 ;

N60 G76 X0.7387 Z-1.50 P0.06815 Q0060;

N70 G00 X1. Z1. M09 ; (clearance position) In this 7 line program, 2 lines of code produce the 7/8-9 thread. Let’s review each segment of these codes, we’ll start with program line N50.

 

Program Explanation

N50 = program line identification

 

G76 = canned cycle routine

 

P010060

 

The first two digits (P010060) represent the number of spring (finish) passes. In this example, there is one finish pass.

The second two digits (P010060) represent the chamfer amount pull out. The 00 in this example program a straight pull out.

To calculate the chamfer pull out, multiplying the two-digit value by the thread pitch. Ex: P010560 = 05 x 0.111 = 0.0556 chamfer length.

The final two digits (P010060) represent the thread angle. This value can be changed to suit the thread angle required. A 00 would represent a plunge (straight) in-feed angle.

Q0050 = minimum pass depth

Note, this value is programmed without a decimal point.

R0.0005 = depth of last threading pass

N60 = program line identification

G76 = canned cycle routine

X0.7387 = minor diameter from machinist handbook

Z-1.500 = ending Z axis position

P0.06815 = total thread depth (amount per side)

Q0080 = maximum pass depth

This value programmed without a decimal point.

F0.1111 = lead of thread pitch = 1 ÷ 9

 

The Z start position (shown in line N40) is recommended as Z0.300 or a minimum of 4 multiplied by the pitch dimension. Ex: 7/8 - 9 TPI thread = 4 x 0.111 = Z0.444 dimension. This approach allows the machine to accelerate to the correct axis velocity before the insert enters the material.

An alternative method of thread programming is to use the G92/G76 commands. Check back next month when we discuss use of these codes and programming tapered pipe threads.

[cappy]

Hello,

 

Found this on the web. I thought I would post it if anyone else is looking for this info.

 

Tooling & Production June 2003

"Shop Talk with Steve Rose"

 

 

 

Threading Methods

 

There are three programming methods available for programming on Fanuc based controls. We’ll look at the benefits of each method in the next few articles of Shop Talk.

The production of an external or internal thread requires several passes with a single-point threading tool. The deeper the thread, the greater the number of passes required to produce that thread.

The traditional threading method uses G32/G33 codes. These commands require four lines of program code for each thread pass. For example, machining a 3/4 - 10 external thread could require 10 - 14 threading passes resulting in 40 - 56 lines of code.

Typically in a single pass threading routine the depth is reduced in each pass as the diameter gets smaller. Reducing the depth in this manner is necessary to balance the load on the insert. As the insert goes deeper into the material the area of contact between the tool and the part increases. To minimize this contact area, smaller pass depths are programmed as the insert approaches its final depth. Your insert supplier’s catalog has information regarding the number of passes needed for a specific thread.

There are two alternative programming methods to reduce the programming effort. Today we’ll review G76; this canned cycle method is very popular and suitable for many threading applications. Only 1-2 lines of information must be programmed, depending upon the type of control.

A Fanuc 0/18/21 control is often programmed with 2 lines of code as follows. Let’s use a 7/8 - 9 TPI thread in a modal program as an example. First, use the Machinist Handbook to determine the major (outside) and minor (root) diameter of the thread. Then, calculate the thread depth as follows.

 

thread depth = (major ø - minor ø ) ÷ 2

 

1111 (thread 7/8 - 9 TPI) ;

N10 G00 G40 G99 ;

N20 G97 S1090 M13 ; (spindle direction & coolant)

N30 T0303 ; (tool & offset)

N40 X0.955 Z0.444 ; (start position)

N50 G76 P010060 Q0050 R0.0005 ;

N60 G76 X0.7387 Z-1.50 P0.06815 Q0060;

N70 G00 X1. Z1. M09 ; (clearance position) In this 7 line program, 2 lines of code produce the 7/8-9 thread. Let’s review each segment of these codes, we’ll start with program line N50.

 

Program Explanation

N50 = program line identification

 

G76 = canned cycle routine

 

P010060

 

The first two digits (P010060) represent the number of spring (finish) passes. In this example, there is one finish pass.

The second two digits (P010060) represent the chamfer amount pull out. The 00 in this example program a straight pull out.

To calculate the chamfer pull out, multiplying the two-digit value by the thread pitch. Ex: P010560 = 05 x 0.111 = 0.0556 chamfer length.

The final two digits (P010060) represent the thread angle. This value can be changed to suit the thread angle required. A 00 would represent a plunge (straight) in-feed angle.

Q0050 = minimum pass depth

Note, this value is programmed without a decimal point.

R0.0005 = depth of last threading pass

N60 = program line identification

G76 = canned cycle routine

X0.7387 = minor diameter from machinist handbook

Z-1.500 = ending Z axis position

P0.06815 = total thread depth (amount per side)

Q0080 = maximum pass depth

This value programmed without a decimal point.

F0.1111 = lead of thread pitch = 1 ÷ 9

 

The Z start position (shown in line N40) is recommended as Z0.300 or a minimum of 4 multiplied by the pitch dimension. Ex: 7/8 - 9 TPI thread = 4 x 0.111 = Z0.444 dimension. This approach allows the machine to accelerate to the correct axis velocity before the insert enters the material.

An alternative method of thread programming is to use the G92/G76 commands. Check back next month when we discuss use of these codes and programming tapered pipe threads.

[dougm]

cappy

we have a M-27

Doug

[Thoob]

cappy

we have a M-27

Doug

 

We have one as well. I have the codes all figured out. PM me if you need any assistance.

[Thoob]

This is a sample code that works on my M27.

Its a 2.5-12 thread.

 

G76 P010060 Q0050 R.001

G76 X2.392 Z-1.9125 P0540 Q0100 R0 F.08333

[marcodintino]

We have one as well. I have the codes all figured out. PM me if you need any assistance.

We purchased a romi m27 wondering if you can help me find a post for masterm x6