Programming an Angle using A on a Fanuc Controller

ljeremy578 · Jul 23, 2019

Can anyone explain to me how to program an angle using A? For example A135.0

Mike1974 · Jul 23, 2019

G0 G90 A135.

?

Program an angle for what? A probe routine, a G68 rotation XYR (R value not A for this), an angle on your 4th axis?

ljeremy578 · Jul 23, 2019

Either an ID or OD angle turning on a lathe.

Mike1974 · Jul 23, 2019

ljeremy578 said:
Either an ID or OD angle turning on a lathe.

You wouldn't use an A, you would do it using X and Z values....

Maybe using conversational it is an A value, I don't know..?

I am thinking longhand in CAM....

ljeremy578 · Jul 23, 2019

I have seen it done just was curious how to do it personally. I know its been done with CAD.

TeachMePlease · Jul 23, 2019

Mike1974 said:
You wouldn't use an A, you would do it using X and Z values....

Maybe using conversational it is an A value, I don't know..?

I am thinking longhand in CAM....

On my Mits, and I believe on the Fanucs that were on Citizens before the Mits, you can make a chamfer or an angle by specifying an A or C value, and the controller does the math.

So you could:

G1 X.240 F.002
Z.500
X.270A60

and the control would calculate the Z endpoint to move X to .270 at a 60 degree angle

G1 X.2 F.002
G1 X.5 E.001, R.015

The control moves to X.5 but automatically puts a .015R on the the .5 diameter. The E value gives the feedrate used during the G2, in case you want to slow down.

You can use C in the same way as R to create a 45 degree chamfer of a specified size, automatically.

pcasanova · Jul 23, 2019

teachme is on it with the a movement, but machine in air first to make sure the angle goes the way you want. 0 on the compass may not be where you would assume.

Vancbiker · Jul 23, 2019

There is an optional function called Direct Drawing Dimension Programming that allows combinations of X,Z,A,R values to be entered to define the profile. Never tried turning it on to see how it works. IIRC, the FAPT version controls output used that function. Seems like it could be handy if ones trig and geometry skills were a bit rusty.

EndlessWaltz · Jul 23, 2019

If I remember I manage to do it with a chamfer.

1/32 chamfer 1" shaft:
Blah blah
G1 X.936 Z0.0
G1 X1.00 A-45.0
blah blah

bradleyk · Jul 24, 2019

On my Nakamura I program using A like this..
G0X1.Z.05
G1Z-.458F.004
X1.21, A105.
Z-1.58

This code is creating a 15° from vertical as the tool moves up in the X direction(0° is on centerline sticking out of the spindle, 90° is perpendicular to centerline, 180° is on centerline going towards the spindle, 235° would be a 45° going back towards centerline, etc...)

It requires the comma after the X or Z command.
I use A commands whenever I can... makes it easier to read the code afterwards.

Dominic Ferland · Nov 20, 2020

I have a Nakamura WT150.
Have a ''Y'' axis on the upper and life tool on upper and lower

Now, I try to figure out how to use that kind of G-Code in my program that I do by hand.

I ran that simple test just to see if my code was good.

For any reason when I run that program I have an error that say ''57 no solution for block end''...
So I don't know if the way I doing the code for the angle is not good or I need to activate something somewhere in the controler of the machine (Fanuc 18i-TB)

Program :

O0011(test with id statements)
(10-12-2020)

(UPPER TURRET PROGRAM)

N1 M41(ROUGH TURN TURN_OD_ROUGH_1)
G54
(PLT-CNMG432-PR GR4315_C4)
(UPPER TURRET)
(MAIN SPINDLE)
G28 U0
G28 V0
G28 W0
M981 (SECURITY CHECK)
G18
G0 G40 G80 T1111
G08 P1
G99
G50 S2500
G96 S450 M3
M07
G0 X.5 Z0.0756
G1 Z0 F.012
Z-1.0,A165.0 F0.001
X3.0
G0 Z0.05
M09
G28 U0
G28 V0
G28 W0
G08 P0
M1

TeachMePlease · Nov 20, 2020

Try changing the angle to something simple like 90, see if it can calculate it then.

DouglasJRizzo · Nov 20, 2020

On Okuma OSP giving an "X" or "Z" target point and an "A" - the control will generate an angle. It's called "Auto Any-Angle" and it's standard on OSP. "0" degrees is 3: O'Clock, and it goes CCW from there.

On Fanuc it's an option called something like "Direct Drawing Input" and I believe it works the same.

LockNut · Nov 20, 2020

On some Fanucs, it is an option, but a lot of MTB provided it standard. But on some models a parameter controls how it is programmed. I remember needing a comma before the letter address. Like,C or ,R. I found the below graphic a Fanuc manual.

EnginCycles · Nov 20, 2020

DouglasJRizzo said:
On Okuma OSP giving an "X" or "Z" target point and an "A" - the control will generate an angle. It's called "Auto Any-Angle" and it's standard on OSP. "0" degrees is 3: O'Clock, and it goes CCW from there.

On Fanuc it's an option called something like "Direct Drawing Input" and I believe it works the same.

Is this working in minutes or degrees? I have an Okuma and this would be kind of slick. Wish I had known it. So going in the negative Z direction on a face if I wanted a 45 chamfer and I doing A 225 or 37.5 if we are going in minutes? (only asking because you said 3 o'clock as the start so I figured maybe we are using minutes.

Vancbiker · Nov 20, 2020

It is in degrees and CCW is positive from 0 at 3 o'clock.

70olds · Nov 23, 2020

EnginCycles said:
Is this working in minutes or degrees? I have an Okuma and this would be kind of slick. Wish I had known it. So going in the negative Z direction on a face if I wanted a 45 chamfer and I doing A 225 or 37.5 if we are going in minutes? (only asking because you said 3 o'clock as the start so I figured maybe we are using minutes.

It's all done in degrees.
If you want a 45 on the face to OD in the Z minus and X positive direction you would say A135.
.....
X.9 Z0.0
Z-.1 A135 (from Z0 to Z-.1 (X is automatically calculated) you go at 135 degrees from straight out of the spindle being 0, vertical towards your upper turret being 90)
Z-1
.....

Neil101 · Dec 12, 2022

70olds said:
It's all done in degrees.
If you want a 45 on the face to OD in the Z minus and X positive direction you would say A135.
.....
X.9 Z0.0
Z-.1 A135 (from Z0 to Z-.1 (X is automatically calculated) you go at 135 degrees from straight out of the spindle being 0, vertical towards your upper turret being 90)
Z-1
.....

Hey @70olds how do I figure out the A value for the angle I want to make?

For example, if I want to make a 10 degree angle or 35 degree how do I find the A value.

Thanks

guythatbrews · Dec 13, 2022

On okuma controls the auto any angle feature also allows radius. For example

G1 X1. Z0
X2. A135. R.1

will radius the chamfer corner. This is really handy.

70olds · Dec 14, 2022

guythatbrews said:
On okuma controls the auto any angle feature also allows radius. For example

G1 X1. Z0
X2. A135. R.1

will radius the chamfer corner. This is really handy.

Are you sure about that? On Okuma lathes radii are expressed using the letter L. I can't say that I've expressly tried to not use it, but there's a G76 command for automatically radiusing the end of a line into the next one. Using your example it would be:

G1 X1 Z0 (Okumas don't need the decimal point FWIW)
G76 X2 A135 L.1

That will END that line with a .1" radius going into the next programmed line. It won't radius anything before the angle.

Programming an Angle using A on a Fanuc Controller

Plastic

Diamond

Plastic

Diamond

Plastic

Diamond

Hot Rolled

Diamond

Cast Iron

Cast Iron

Plastic

Diamond

Titanium

Stainless

Aluminum

Diamond

Aluminum

Aluminum

Titanium

Aluminum

Similar threads