Need Help!- Tool Tip Direction on TL series machines?

[Donkey Hotey]

What a weekend. I've scrapped $75 worth of brass bar trying to make some very simple parts. I thought I had a handle on this but I guess not.

The part is a very simple shape. It's a 0.5" shank, going into a 0.75" ball on the end (right side of the bar). I start by using a G71 to rough the ball from zero to 90 degrees on the end of the bar.

It's a standard right-turn, inserted tool. I'm using Tool Nose Compensation (TNC) so the ball will end up being true.

The cutter radius is in the offsets page (0.032") and I'm using Tip direction 3. From all I see in the manual, I treat this machine as if I'm using an SL type lathe and that all of the tip directions are from the back of the part (backward from what we see on a Toolroom Lathe).

That end turns just fine.

Then I do a G75 with the parting tool to cut a clearance valley on the other end of the bar (closer to the chuck). After the clearance is cut, I go after the 0.5" shank and completing the ball shape.

This is a standard, LH turning tool, also with 0.032" radius. I specified Tip Direction 4 in the offsets.

The problem is that it cuts just fine through the roughing phase of G71 but when it gets to the final pass, it seems that the TNC kicks in but does it in the wrong direction (cutting waaaayyy into the part--ruining it).

I thought it was I,K values or something else but this shows up in Graphics as well. If I turn the Tip Direction to zero (in Offsets), it looks fine.

What am I doing wrong? I thought that for outside turning, RH-turn=tip direction 3 and LH-turn= tip direction 4. Am I missing something?

Help?

[Geof]

Post your program.

[Donkey Hotey]

Thanks Geof. Forgive my verbose code. While I'm learning, I script what I want to do, the add the operations afterward.

The highlighted portion is where it goes bad. From what I'm seeing in Graphics, TNC doesn't take effect until after the roughing is done, then it makes the final passes in G70/71 with TNC.

It completely digs into the part...double the radius is my guess (about 0.064") and it does it on the final passes. I can see this in graphics. It's as if the TNC is offsetting to the wrong quadrant. I was using TNC 4.

I exaggerated the radius in offsets, then I tried each of the TNC settings to try to identify what it should be using (by the generated path). TNC 6 seems to look right in simulation and on the final part--at least as best as I can tell until I get a radius gauge.

The only thing I can think of is the W-0.005 in that G71 line. My understanding from past posts is that W is an offset allowance in Z. And a negative offset in that left facing operation would leave 0.005" of material on the left side (negative Z) of any programmed faces. Did that negative W mess up the TNC?

% O00200 (Ball socket) (Revision zero) (Stock Diameter: 7/8" Brass) (Chuck 2.2-2.5" from jaws) (Cycle ends with Parting tool) (at set point for next part) (pull bar to face of parting tool) (before resuming) (Tools) (T1 Right Facing tool) (T10 Parting Tool) (T4 Left Facing tool w/0.75 clearance) (****************************************) (PREP STATEMENTS) T10 (Load Parting Tool) G00 X-0.02 Z0.05 (Loading Position) M00 (Ensure Bar is against Parting Face) G00 X1. Z1. (Safe Clearance) T1 (Load Aloris CXA-16N Turning tool) G54 (work offset) G50 S1200 (Spindle Max RPM) G96 S600 M03 (CSS on, 800 SFM, spindle on) (****************************************) (CUT RIGHT HALF OF BALL PROFILE) G00 X1. Z0.15 (Return Point) M08 G71 P3 Q4 D0.04 F0.008 U0.005 W0.005 (roughing cycle) N3 (describe right ball half) G42 (Establish Cutter Comp) G00 X-0.04 Z0.1 (cutter comp move) G01 Z0. F0.006 X0. G03 X0.748 Z-0.374 R0.374 G01 Z-0.5 G40 X1. (Cancel Cutter Comp) N4 (end right ball half) G70 P3 Q4 (Finish Pass) M05 (spindle stop) G00 X2. Z1. (safe location) (****************************************) (TURNING CLEARANCE RELIEF: LEFT SIDE OF PART) (Width to clear right parting tool) T10 (LOAD PARTING TOOL) M03 (spindle on) G00 X1. Z-0.8 (rapid to safe dia n part distance) G75 X0.52 Z-2.1 I0.05 K0.1 F0.005 G00 X1. Z1. M05 (spindle off) (****************************************) (BACK FACE: LEFT SIDE OF PART) (LEFT FACING TOOL) T4 (LOAD DTM H90-2A Dorian LH Facing Tool) M03 (spindle on) G00 X1. Z-1.23 (Return Position) G71 P5 Q6 D0.03 F0.008 U0.004 W-0.01 (roughing cycle) N5 (describe outside profile) G42 G01 X0.5 F0.004 (Establish Cutter Comp) Z-0.652 (Base corner of ball) G02 X0.748 Z-0.374 R0.374 (Cut ball) G01 Z-0.25 (overcut tangent point) G40 X0.75 (Cancel Cutter Comp) N6 (end outside profile) G70 P5 Q6 (Finish Pass) G00 X2. Z5. (safe location) M05 (****************************************) (FINAL PARTING OPERATION) T10 (LOAD PARTING TOOL) M03 (Spindle On) G00 Z-1.35 (0.023" extra for later finish) X0.6 G75 X-0.02 I0.05 F0.006 (cutoff the part) G00 X1. Z-2. X0.6 G75 X-0.02 I0.05 F0.006 (cleanup face) M09 G00 Z0.05 X0. (Reload Bar Position) M05 (spindle off) (Unchuck Bar, Pull to Parting Bar Face) M30 (End Program) %

[Geof]

I feel a bit foolish...I was going to run it through my Simulator; the Simulator that is getting a software glitch fixed. And I was going to compare it with some programs on my TL2...the one that developed the same error as my Simulator; ref. my post on the 250, 251 alarms. So I am not able to do anything.

Obviously short term memory is going.

[Donkey Hotey]

Never mind. I'm an idiot. Whenever faced with a problem like this, put it down, walk away, get something to eat.

I went out to get something to eat, sat down with the programming manual and figgered' I would take it from the top. There it was:

The tool is feeding from left to right. It's tool-left (G41) not tool-right (G42). Everything else I've ever programmed has been from the right so in my mind: outside=G42, inside=G41. How could I be so dumb? I guess that's why they call it 'learning'.

[speeeeed]

Hi,
I thought you had to tell it an offset # when you call the tool. I am really glad you brought that to my attention though because I am trying to get comfortable programming a TL-4 and I can learn from your mistakes.
Thanlks a Bunch
Chris

[alain aleman]

I think that your problem is the tool offset,

T0101
.
.
.

Regards,

Alain

[Geof]

Originally Posted by speeeeed Hi, I thought you had to tell it an offset # when you call the tool. I am really glad you brought that to my attention though because I am trying to get comfortable programming a TL-4 and I can learn from your mistakes. Thanlks a Bunch Chris

As you can see the offset number is included in the tool call as the final two digits. You can actually have more than one offset per tool. T101 selects tool 1 and uses the offset in line 1 of the offset table; T111 selects tool 1 and uses the offset in line 11 of the offset table.

I why would you want to do that? You can gang tools at a single tool number on the tool changer and then assign a different offset for each tool in the gang.

[speeeeed]

Thanks Geoff
Chris

[speeeeed]

But actually I don't see

[Geof]

Originally Posted by speeeeed But actually I don't see

Don't see what?

The idea of gang tooling and multiple tool offsets?

Tool offsets in general?

[Wiseco]

deleted