Fadal subroutine question

K

Kevinstj

Cast Iron

Joined

Feb 17, 2011

Location

USA

• Dec 7, 2018

• #1

I am trying to do a mill out a 1.750 slot with a 1.00" 2 insert indexable endmill ,3.250 deep( stock is 3" square , 6 1/8 tall) . I think the best way to do this is a subroutine. I understand that the first lines designate the subroutine movement. How do I go about feeding the Z down after every pass is that called out in the subroutine.
Thanks for your help

 

G

guest

Guest

• Dec 7, 2018

• #2

Kevinstj said:

...How do I go about feeding the Z down after every pass is that called out in the subroutine.
Thanks for your help

Click to expand...

Write your sub in incremental and position Z down at the end, Repeat L times until you are at depth.

 

K

Kevinstj

Cast Iron

Joined

Feb 17, 2011

Location

USA

• Dec 7, 2018

• #3

Ok, Can you give me an example of what this would look like?

 

G

guest

Guest

• Dec 7, 2018

• #4

This would be the fanuc version- don't know about fadal specific codes...

main prog:

O1000
N1 G90 G40 G49 G80
T1 M6
S3500 M3
G0 G54 X0.6 Y0.375
G43 Z1.0 H1
Z.1
G1 Z0 F35.0
M98 P1001 L20
G91 G28 Z0
G28 Y0
M30

Sub:

O1001
G91
G1 Z-.1625
G1 X-4.200 F35.0
Y-.750
X4.200
Y.750
M99

X0 is right EOP, Y0 is centerline of slot

Edit: changed Z down move to beginning of sub to eliminate unneeded Z move at end of program.

 

Bobw

Diamond

Joined

Feb 8, 2005

Location

Hatch, NM Chile capital of the WORLD

• Dec 7, 2018

• #5

Personally I prefer to do all my X-Y's in absolute and only use incremental for the Z move.

A little bit of a pain in the ass if you need to ramp, but not too bad. Not a big deal with a helix.

 

G

guest

Guest

• Dec 7, 2018

• #6

Bobw said:

Personally I prefer to do all my X-Y's in absolute and only use incremental for the Z move.

Click to expand...

That works too. IIRC Fadal uses E1 instead of G54, yes?

@OP- Programming absolute except for the Z move, the sub would look like this:

Sub:

O1001
G91
G1 Z-.1625
G90
G1 X-3.6 F35.0
Y-.375
X0.6
Y.375
M99

 

Bobw

Diamond

Joined

Feb 8, 2005

Location

Hatch, NM Chile capital of the WORLD

• Dec 7, 2018

• #7

That works too. IIRC Fadal uses E1 instead of G54, yes?

Click to expand...

Take your pick.. At least in format 2, a Fadal doesn't care... It'll take
straight up Fanuc code. If a G43 is there it doesn't care.. It knows how
to deal with a G28..

when I had a Fanuc machine I accidentally posted Fanuc and sent it to a Fadal,
and I didn't even realize it until the machine didn't come home at the end of the
program.

And I much prefer the 'E's... Fixture offset '1' is E1... Fixture offset '43' is E43 not
G59.2 or some stupid thing. And it would make more sense if it was an 'F' not an 'E', but
'F' is already spoken for, as is 'O'.

 

K

Kevinstj

Cast Iron

Joined

Feb 17, 2011

Location

USA

• Dec 9, 2018

• #8

So this is what I have come up with for my program. I’m sure there is a mistake in there somewhere.
Thanks

N1 O1234
N2 L100
N3 G91
N4 G1 Z-.125 F20.0
N5 G90 X1.125 Y+.750
N6 Y-3.500
N7 X1.875
N8 Y+.750
N9 X1.125
N10 M17
N11 M30
N12 M6 T1
N13 M3 S2500
N14 G0 G90 G54 X0.0 Y+1.00
N15 G43 H1 D1 Z 0.0 M7
N16 L126
N17 G0 Z0 M5 M9
N18 G28 Z0
N19 X0 Y1.00
N20 M30

 

K

Kevinstj

Cast Iron

Joined

Feb 17, 2011

Location

USA

• Dec 10, 2018

• #9

Well, the subroutine worked great. I had to change the depth of cut down to reduce tool chatter due to the length of the end mill.
Thanks for everybody’s help.

 

Cole2534

Diamond

Joined

Sep 10, 2010

Location

Oklahoma City, OK

• May 7, 2019

• #10

Kevinstj said:

So this is what I have come up with for my program. I’m sure there is a mistake in there somewhere.
Thanks

N1 O1234
N2 L100
N3 G91
N4 G1 Z-.125 F20.0
N5 G90 X1.125 Y+.750
N6 Y-3.500
N7 X1.875
N8 Y+.750
N9 X1.125
N10 M17
N11 M30
N12 M6 T1
N13 M3 S2500
N14 G0 G90 G54 X0.0 Y+1.00
N15 G43 H1 D1 Z 0.0 M7
N16 L126
N17 G0 Z0 M5 M9
N18 G28 Z0
N19 X0 Y1.00
N20 M30

Click to expand...

I'm having a little trouble with subs and was hoping someone could answer a few Q's using this example.

Where was the subroutine defined? I see it called as L100, is it only the bold portion?

If so, was it executed at the 3 spots I underlined, then canceled by the M17?

Noobie Questions, I know.