G71 cycle Haas tl 2

[maxsic]

Hey guys, my first post on here. I have a Haas tl 2 from 2005 at work, im trying to get them to let me do some machining as i got certified back in highschool. This lathe is giving me a bunch of problems, first is that if you are doing a taper or circular interpolation you need to put the z before the x or it sends your toolpath everywhere but where it needs to be. Second is my contour works fine by itself or under the g70 cycle but in graphics on the g71 it turns into a nightmare my code is this
T101
M06 s2000
G00 z.01 x1.5
G71 p1 q2 d.1 u.05 w.05 f.01
N1 G00 w0 x1.5
G01 z0 x0
G03 z-.25 x.5 r.25
G01 z-.875
G02 z1 x.625 r.125
G01 z-1.75 x.75
G01 z-2 x1
N2 G01 z-3
It has been a while and it ran almost perfectly until it hit the first rough cut on the .25 radius then the toolpatb got sent through the part every which way. Any help would be much appreciated, I've heard a lot of people say that Haas is very picky about codes. This code also worked completely fine in a Cnc simulator program.

 

[angelw]

Hey guys, my first post on here. I have a Haas tl 2 from 2005 at work, im trying to get them to let me do some machining as i got certified back in highschool. This lathe is giving me a bunch of problems, first is that if you are doing a taper or circular interpolation you need to put the z before the x or it sends your toolpath everywhere but where it needs to be. Second is my contour works fine by itself or under the g70 cycle but in graphics on the g71 it turns into a nightmare my code is this
T101
M06 s2000
G00 z.01 x1.5
G71 p1 q2 d.1 u.05 w.05 f.01
N1 G00 w0 x1.5
G01 z0 x0
G03 z-.25 x.5 r.25
G01 z-.875
G02 z1 x.625 r.125
G01 z-1.75 x.75
G01 z-2 x1
N2 G01 z-3
It has been a while and it ran almost perfectly until it hit the first rough cut on the .25 radius then the toolpatb got sent through the part every which way. Any help would be much appreciated, I've heard a lot of people say that Haas is very picky about codes. This code also worked completely fine in a Cnc simulator program.

I've not seen a HAAS machine, Lathe or Machining Centre, where the order of X,Y and Z made any difference.

Your N1 line is incorrect; this line should specify the Start Coordinate for your profile description, not the Start Position in X in fresh air. Try the following:

G00 Z.01 X1.5
G71 P1 Q2 D.1 U.05 W.05 F.01
N1 G00 W0.0 X0.0
G01 Z0.0
G03 Z-.25 X0.5 R.25
G01 Z-.875
G02 Z-1. X.625 R.125
G01 Z-1.75 X.75
G01 Z-2.0 X1.0
N2 G01 Z-3.0

The control is only picky when your program is incorrect.

Regards,

Bill

 

[maxsic]

So the code works and stopped throwing alarms but same as last time i got it to work, when it comes to the 2 radius it sends the toolpath through the part right in the middle of the radius

 

[maxsic]

I wish i could attach a picture but it says the file is too large.

 

[angelw]

So the code works and stopped throwing alarms but same as last time i got it to work, when it comes to the 2 radius it sends the toolpath through the part right in the middle of the radius

It depends on whether you're using your example or mine. In your program example the following Block:

G02 z1 x.625 r.125

has a positive Z value; it should be Z-1.0. With the lower case alpha characters, I suspected it was a typo, but if you have that Z value in your program, the program is incorrect.

Regards,

Bill

 

[maxsic]

I just got the profile i wanted, for some reason the finish allowance in z was causing it, i dropped it down to .01 and it works fine, maybe because those first cuts would have been out of range of the z starting point. Thank you for your help, definitely helped me with the contour start.

 

[sinha]

I just got the profile i wanted, for some reason the finish allowance in z was causing it, i dropped it down to .01 and it works fine, maybe because those first cuts would have been out of range of the z starting point. Thank you for your help, definitely helped me with the contour start.

This problem seems to be unique to Haas. On a Fanuc, if you have W0 in the N1 block, the cycle works for any value of Z-finishing allowance.
Possibly, there is a parameter, limiting the value of Z-finishing allowance.

 

[angelw]

This problem seems to be unique to Haas. On a Fanuc, if you have W0 in the N1 block, the cycle works for any value of Z-finishing allowance.
Possibly, there is a parameter, limiting the value of Z-finishing allowance.

Hello Sinha,
Its not the case with only W0.0, but also with an Absolute coordinate for the Z axis. With a Fanuc control, had the OP's first definition Block of the profile, N1 G00 W0.0 X0.0 been modified to the following Block to give the same result as using W0.0

N1 G00 Z0.01 X0.0

any Z finishing allowance could have been used without error.

Regards,

Bill

 

[angelw]

I just got the profile i wanted, for some reason the finish allowance in z was causing it, i dropped it down to .01 and it works fine, maybe because those first cuts would have been out of range of the z starting point. Thank you for your help, definitely helped me with the contour start.

You say that you "got the profile I wanted". Are you ware that the Tool Nose Radius of the cutting insert affects Radii and Taper features? The coordinates used in your roughing cycle appear not to have TNR Compensation incorporated and unless you used Tool Nose Radius Comp by the control (G42), or incorporated Tool Nose Radius Comp in the part program finishing coordinates, then the part profile wont be correct.

Regards,

Bill

 

[sinha]

Yes
As long as the axial location of the start position of the tool lies to the right or at the axial location of the first point on the profile (in the P block), there will be no issues.

Hello Sinha,
Its not the case with only W0.0, but also with an Absolute coordinate for the Z axis. With a Fanuc control, had the OP's first definition Block of the profile, N1 G00 W0.0 X0.0 been modified to the following Block to give the same result as using W0.0

N1 G00 Z0.01 X0.0

any Z finishing allowance could have been used without error.

Regards,

Bill

 

[sinha]

Yes
As long as the axial location of the start position of the tool lies to the right or at the axial location of the first point on the profile (in the P block), there will be no issues.

This condition applies to machining from right to left.

If G71 is being used for machining from left to right, the start Z of the tool must lie to the left of the start Z of the profile, or it can be at the start Z of the profile. The Z finishing allowance must be negative in this case.

The best is to use W0 in the P block. It always works.

In type 1 G71, W or Z is not mentioned. The control assumes W0 for the start Z of the profile.

All this as well as many other things are discussed in quite detail in my book on G71/G72. Quite a few of you have downloaded it. Please read it also.

 

[angelw]

This condition applies to machining from right to left.

If G71 is being used for machining from left to right, the start Z of the tool must lie to the left of the start Z of the profile, or it can be at the start Z of the profile. The Z finishing allowance must be negative in this case.

The best is to use W0 in the P block. It always works.

In type 1 G71, W or Z is not mentioned. The control assumes W0 for the start Z of the profile.

All this as well as many other things are discussed in quite detail in my book on G71/G72. Quite a few of you have downloaded it. Please read it also.

The sole purpose of a Z or W being included in the P reference Block of the G71 cycle or X or U in the G72 cycle, is to initiate the Type 2 version of those two cycles, to allow machining of a profile with concave features.

Using W0 and U0 in the P reference block of G71 and G72 cycles respectively, is just a convenient method of turning the Type 2 version of these cycles on without having to take care that the Z and X used in the P reference block of G71 and G72, are the same as the Start Position of the tool in the respective axes, if no movement in Z (G71) or X(G72) from the Tool Start Position to the Profile Start Position..

The control makes no assumption with regards to the addresses to turn Type 2 Multi-repetitive cycles, when they are omitted; the Type 2 version of the cycle just isn't used. In the G71 Cycle for example, the last Z address executed before launching the Cycle, will be to position the Tool at the Z Start Position. The Z coordinate will be Modal and therefore, omitting a Z address in the P reference block will result in an X Move only after the Finish Allowance has been taken up, the same as the following two examples outside of a Roughing Cycle will result in the same Tool movement:

G00 X50.0 Z2.0
G01 Z0.15 F1.0
N1 G01 X0.0 Z0.15 F0.25 (Z included)

G00 X50.0 Z2.0
G01 Z0.15 F1.0
N1 G01 X0.0 F0.25 (Z omitted)

In the above case, W0 is not assumed, Z0.15 is Modal and therefore, the two N1 Blocks above are equal.

Regards,

Bill.

 

[sinha]

I was not very clear.
When I said that W0 is assumed, I only meant this for the purpose of defining the start point of the profile (because Z is modal). It is not that type 2 will start!