Changing Direction of Internal Taper

[dlall]

Hi There,

I am very new to this forum so please forgive me in advance for any newbie mistakes.

I'm using the controller on the TL-1 to make an internal taper. I want to reverse the direction of the taper so that the bigger diameter is nearer to the chuck and the smaller diameter nearer to the toolpost. The tool I'm using as well as the diameters of the taper allow enough clearance to do so. But for some reason I'm having problems reversing it. Any help with respect to the G-code needed will be appreciated.

Thanks

[swain]

Are you using canned cycle to do this?

If so...haas has wierd ways when you want to do non standard
cycles. One way to fix this is to put it into Type II fanuc roughing.
(I think thats what its called...going off of memory here)
If you have manual, look under G71 and it has an explanation
of type I and type II roughing.

G'day

[dlall]

Hi Swain,
Thanks for your help.
I've had a crack at your suggestion but haven't been successful. I'm not quite sure what I'm doing wrong.

I changed to Setting 33 to YASNAC and inserted R1 at the end of my G71 block to allow me to go either way in the x-axis. This is what the book said.

Have you done this before, if so do you have a sample of your G code with particular attention to the G71 block?

Any further help would be greatly appreciated.

Thanks Again.

[swain]

I have never set the machine to Yasnac...

I left my machine as it came from factory and used the Fanuc setting.

From the lathe handbook...

"Type II, when Setting 33 is set to FANUC, must have a reference move, in both the X and Z axis, in the block
specified by P."

What this means....in your first block after the G71 cycle that has an X or Z move...add the other axis to it. For example,

G96 S1000 M03
X1.25 Z.125 M08
G71 P100 Q101 U.04 W.01 D.05 F.008
N100 G00 X-.062
G01 Z0 F.004
X.6125
Z-.25
N101 X1.25

The line that has the N100 is the only line that changes. To make the program do Type II roughing change that line to this....

N100 G00 X-.062 Z0

The rest of the programming can stay the same...and hass will not error when you command it to do the inverse taper move or any other unless programmed to go past the starting location.

Give it a try...!

G'day

[dlall]

Hi Swain,

Just wanted to say thanks for the help. The advice you gave me worked. All the best to you and your family for the Christmas Season.

Thanks Again,

[swain]

Hi Swain,

Just wanted to say thanks for the help. The advice you gave me worked. All the best to you and your family for the Christmas Season.

Thanks Again,

Most welcome...

Merry Xmas to you and yours!!

Swain