[stuby]

I am just starting to mess around with G70 and G71 on my CNC; a Leadwell LTC-15 with a Fanuc-OT controller. I have the machine moving in the right paths, however it is generating an extra shoulder that I am not sure where its coming from. Here is my Code :

G50 S800
G0 T0202
G96 S500 M3
G99 Z0.1 X2.1
M08
G71 U0.015 R 0.05
G71 P1 Q2 U0.02 W0.02 F0.014 S500
N1 G42 G01 X0.5
Z -0.5
G02 X 0.750 Z-0.75 I 0.125 K0 F.006
G01 X1.0
Z-1.25
G02 X1.25 Z-1.5 I0.125 K0
G01 X1.5
Z-2.0
N2 G70 P1 Q2
G0 T0200
G28 X0
G28 Z0
M09
M05
M30

The machine creates the first diameter correct. Then it moves into the radius, also correct. But then, instead of moving straight up in the X-axis, it feeds in .125 on the Z and cuts a different shoulder. It does the same thing right after the next radius. Im not sure if I have my cutter comp correct either. Any input on the situation?


Edit : I fixed one of my problems but another one has arisen. I was indeed making a .125 radius, when really I was trying to program a .250 radius. BUT, I still seem to have a little shoulder extra. Its about .080 big. I attached a print of what it is making, and what I am trying to make. Thanks alot for the help.

[CNCRim]

I'm not sure what you want to program but it seem to me that you trying to cut 2 quadrant of circle that is why the tool..... cut .125 deeper. Change your Z if .... you only want to cut 1 quadrant circle.

[dcoupar]

I think both of your Z values at the start of the arcs are 0.125 short. I assume you're cutting a 0.125 radius? Change the Z-0.5 to Z-0.625 and Z-1.25 to Z-1.375

[jackson]

can you show us a print.

[cnc-king]

i am not quite that familiar with the I & K on the lathes but it seems that your problem is your K value, you are moving the Z .25 but your K is zero, does your machine use R instead of I and K's.

[stuby]

I fixed one of my problems but another one has arisen. I was indeed making a .125 radius, when really I was trying to program a .250 radius. BUT, I still seem to have a little shoulder extra. Its about .080 big. I attached a print of what it is making, and what I am trying to make above. Thanks alot for the help.

[cnc-king]

I fixed one of my problems but another one has arisen. I was indeed making a .125 radius, when really I was trying to program a .250 radius. BUT, I still seem to have a little shoulder extra. Its about .080 big. I attached a print of what it is making, and what I am trying to make above. Thanks alot for the help.

make sure the T value in your offset page is set to 3
and your TNR is correct
your program profile should look some what like this with R's instead of I's & K's

Z-.5
G2 X1. Z-.75 R.25
G1 X1.5
Z-1.33
G2 X2. Z-1.58 R.25
G1 X2.5
Z-2.175
X2.75

[Tcooper571]

I think you are going to find that cutter comp doesnt work, or at least work well in a canned cycle, especially the way you are turning cutter comp on. When it finishes the G71, then loops back up and does the G70 you are double compensating by re-activating comp. Maybe try the finish pass not in G70, or use G71 without comp, then use comp only for finishing.

[stuby]

What exactly does the T do in the tool offset menu? I know they are all 0 right now, but Im not sure exactly what they do, Ill try turning it to 3. Also with the cutter comp; I was reading in my book and it says that if the cutter comp is turned on in inside the specified start and stop blocks that it would only be turned on during finishing. Im not sure exactly how it knows when to turn it on and off. But thanks for the help, Ill try both of these and post a little later today. Thanks again.

[Tcooper571]

The T is the imaginary tool tip location. It allows comp to get an idea were the tip of the tool is. If you are doing O.D. turning most T values should be set to the 3 you where going to try. That may help.

[stuby]

I have eliminated the extra shoulder. The problem with that was the I,K instead of R. BUT as usual another problem has come up. It seems like when I cut the radius, it moves in about .010 before actually cutting the radius. It does the half inch shoulder fine, and then it dips in 10 grand before actually doing the radius, so I have not only a lip that you can feel, but you can see it from just looking at it. I have tried many combinations of Cutter comp, and changing the T in my tool offsets, and I am stuck. Any help at all with this?

[DryRun]

This Is how i would program this:

G50 S800
N2 G0 T0202
G96 S500 M3
G99 X2.1 Z0.1 M08
G71 U0.1 R 0.025
G71 P100 Q101 U0.03 W0.002 F0.014
N100 G0 X0.460
G42 G01 Z0.0
X0.5 Z-0.02
Z -0.5
G02 X1.0 Z-0.75 R0.25
G01 Z-1.25
G02 X1.5 Z-1.5 R0.25
G01 Z-2.0
X2.0
N101 G40X2.1Z-1.4
N22 G70 P100 Q101 F0.006
G0 T0200
G28 U0W0M9
M05
M30
Note cutter comp will only work on finish pass

USE A T3 FOR TURNING
USE A T2 FOR BORING
MAKE SURE YOU SET THE TOOL RADIUS IN THE OFFSET PAGE RADIUS

[stuby]

Im not at the shop today, but I will try that code first thing in the morning; it was a little different then mine and it seems to make more sense. Thanks for the help with the T, one quick clarification though. These are only need to be input when using a G70, or G71? Or should I always use these? Also, mine are all currently on T0, does it do anything like that? How about T1? Thanks again for all the help.

[DryRun]

you only need the t code when using cutter comp

g41 boring t2
g42 turning t3

[stuby]

I have corrected several problems. Thanks agian for the help; but heres another one. I was using the same tool for both roughing and finishing before, so I didnt have this problem. I have T0303 for roughing, and T0202 for finishing now. T3 is used in beginning of program, leading up to my G71 block. Where exactly do I want to put the T0202 block? In between the 2 blocks I specify with G71, or does it go in between the end of the sequence and the G70? Also, Im assuming I should return to home before I tool change, correct? Im sure its a pretty simple fix, but I need some help. Thanks in advance.

[Tcooper571]

Now what you need to do is start another block specifically for the finish tool just like you did for the rougher. Have the finish rapid to the same start point that your rougher did, then instert your G70 lines there. The program will go back up and look for the line numbers on the G70 line and then execute that. Below I copied what you first started this thread with (you may have changed it a bit but concept is same).

(rought tool)
G50 S800
G0 T0303
G96 S500 M3
G99 Z0.1 X2.1
M08
G71 U0.015 R 0.05
G71 P1 Q2 U0.02 W0.02 F0.014 S500
N1 G42 G01 X0.5
Z -0.5
G02 X 0.750 Z-0.75 I 0.125 K0 F.006
G01 X1.0
Z-1.25
G02 X1.25 Z-1.5 I0.125 K0
N2G01 X1.5
Z-2.0
G0 T0200
G28 X0
G28 Z0
M09
M05
M01

(Finish tool)
G50 S800
G0 T0202
G96 S500 M3
G99 Z0.1 X2.1
M08
G70 P1 Q2
G0 T0200
G28 X0
G28 Z0
M09
M05
M30

[stuby]

more problems. I Originally had my Finish tool within the P and Q blocks, after reading that, I took those out. Now, for some reason, it isnt actually roughing the part. Instead of starting to rough from its current position, it reads the G71 and tries to cut that profile exactly, no roughing involved. This never happened to me before, and I cant find any reasonable explanation about it. Any help would be appreciated.

P.S. This is the exact same program I was roughing with yesterday, I didnt change anything except add the finish tool to the end, and remove it from the G71 block.