Lathe radius comp question G41, G42

[Rich L]

Folks,

Gang lathe, Fanuc 0i Mate TB control, "rear" lathe (+x away from me, +z to the right)

Even though I've been working with this lathe for a couple years now I have never really needed to use radius comp until now. I have no CAM program so I hand code everything. The part is pretty much dead simple - it's a .728 OD, .628 ID ring with an external convex curve and a small internal concave curve at one of the lips. The stock is .750 x .600 tube.

Here's the code section that has given me an error: 041 INTERFERENCE IN NRC ("overcutting will occur ... modify the program" says Mr Fanuc). The red code line gives me the error. The tool tip number is T2 as it is a left hand profiler. I hope I have that right. The tip radius is .008

I have been poring over the Smid book on this subject and evidently I'm not understanding something about the tool tip clearance required, I think. The line in question is just trying to exit the profile and the retract motion in Z after that has more than the Tx2 clearance from what I just cut. I think.

What am I missing?


...
(EXTERNAL PROFILE)
(G41 LEFT OFFSET T2)

S#104 M3
T0101
F .002
G0 X-.770 (CLEARANCE)
G0 Z.030 (CLEARANCE)
G0 G41 Z.020 T0101 (ENGAGE RADIUS COMP)
G1 X-.700 Z0.0
G1 X-.735 Z-.032 (CHAMFER)
G1 Z-.415 (TURN TO CUTOFF LENGTH)
G0 X-.770
G0 Z.020 (BACK OUT FOR FINISH)
G0 X-.676
G1 Z0.0 F.001

G2 X-.718 Z-.046 R.071
G2 X-.709 Z-.350 R1.808
G1 Z-.415 (TURN TO CUTOFF)
G0 X-.770
G0 G40 Z.5 T0100(CANX COMP)
...
_______________

Here's the Offset screen indicating the radii and tool tip numbers.

Thanks for any help on this and I hope I've provided sufficient information. It will be much appreciated.

Cheers,
Rich

 

[angelw]

Hello Rich,
Try the following.
...
(EXTERNAL PROFILE)
(G41 LEFT OFFSET T2)

S#104 M3
T0101
F .002
G0 X-.770 (CLEARANCE)
G0 Z.030 (CLEARANCE)
G0 G41 Z.020 (ENGAGE RADIUS COMP)
G1 X-.700 Z0.0
G1 X-.735 Z-.032 (CHAMFER)
G1 Z-.415 (TURN TO CUTOFF LENGTH)
G40 G0 X-.770
G0 Z.020 (BACK OUT FOR FINISH)
G41 G0 X-.676
G1 Z0.0 F.001

G2 X-.718 Z-.046 R.071
G2 X-.709 Z-.350 R1.808
G1 Z-.415 (TURN TO CUTOFF)
G0 X-.770
G0 G40 Z.5 (CANX COMP)
...


Regards,

Bill

 

[AHC]

You need to cancel G41 before doing the rapid move back to your start point and running the finish profile. Do a G0G40Z.02
also when applying the G41 do it on the G1X-.700Z0 move.

Folks,

Gang lathe, Fanuc 0i Mate TB control, "rear" lathe (+x away from me, +z to the right)

Even though I've been working with this lathe for a couple years now I have never really needed to use radius comp until now. I have no CAM program so I hand code everything. The part is pretty much dead simple - it's a .728 OD, .628 ID ring with an external convex curve and a small internal concave curve at one of the lips. The stock is .750 x .600 tube.

Here's the code section that has given me an error: 041 INTERFERENCE IN NRC ("overcutting will occur ... modify the program" says Mr Fanuc). The red code line gives me the error. The tool tip number is T2 as it is a left hand profiler. I hope I have that right. The tip radius is .008

I have been poring over the Smid book on this subject and evidently I'm not understanding something about the tool tip clearance required, I think. The line in question is just trying to exit the profile and the retract motion in Z after that has more than the Tx2 clearance from what I just cut. I think.

What am I missing?


...
(EXTERNAL PROFILE)
(G41 LEFT OFFSET T2)

S#104 M3
T0101
F .002
G0 X-.770 (CLEARANCE)
G0 Z.030 (CLEARANCE)
G0 G41 Z.020 T0101 (ENGAGE RADIUS COMP)
G1 X-.700 Z0.0
G1 X-.735 Z-.032 (CHAMFER)
G1 Z-.415 (TURN TO CUTOFF LENGTH)
G0 X-.770
G0 Z.020 (BACK OUT FOR FINISH)
G0 X-.676
G1 Z0.0 F.001

G2 X-.718 Z-.046 R.071
G2 X-.709 Z-.350 R1.808
G1 Z-.415 (TURN TO CUTOFF)
G0 X-.770
G0 G40 Z.5 T0100(CANX COMP)
...
_______________

Here's the Offset screen indicating the radii and tool tip numbers.

Thanks for any help on this and I hope I've provided sufficient information. It will be much appreciated.

Cheers,
Rich

 

[Rich L]

OK. Cool! Why don't I just not use any comp until the finish profile? That should work, right?

Bill, you removed the tool callout on my initial G41 line. Did you mean to do that? The reason I ask is because Smid's examples have the tool callout at the end of the tool comp call line. I know I called the offset out twice so perhaps the second call I had is unnecessary.

Thanks, both of you!

Rich

 

[AHC]

Yes, no need to use comp on roughing.

If you look at your code, the tool call and offset are already applied at the beginning. Tool#01 offset # 01
As a general format rule I try to apply the comp codes g42/g41 in the first feed move towards the finish profile ( G1G41Z0F.001 )
That's just me.


...
(EXTERNAL PROFILE)
(G41 LEFT OFFSET T2)

S#104 M3
T0101
F .002
G0 X-.770 (CLEARANCE)
G0 Z.030 (CLEARANCE)
G0 G41 Z.020 T0101 (ENGAGE RADIUS COMP)
G1 X-.700 Z0.0
G1 X-.735 Z-.032 (CHAMFER)
G1 Z-.415 (TURN TO CUTOFF LENGTH)
G0 X-.770
G0 Z.020 (BACK OUT FOR FINISH)
G0 X-.676
G1 Z0.0 F.001

G2 X-.718 Z-.046 R.071
G2 X-.709 Z-.350 R1.808
G1 Z-.415 (TURN TO CUTOFF)
G0 X-.770
G0 G40 Z.5 T0100(CANX COMP)
...

 

[angelw]

OK. Cool! Why don't I just not use any comp until the finish profile? That should work, right?

Bill, you removed the tool callout on my initial G41 line. Did you mean to do that? The reason I ask is because Smid's examples have the tool callout at the end of the tool comp call line. I know I called the offset out twice so perhaps the second call I had is unnecessary.

Thanks, both of you!

Rich

Hello Rich,

If there were any concave features in the part profile, where any part of the trailing side of the Tool Nose Radius is tangent to the tool path, then you would generally need to use Tool Radius Comp in roughing. However, it would depend on the amount of finishing allowance left as to whether over-cutting by the trailing edge occurs. When only the leading edge of the Tool Radius is tangent to the tool path and Tool Radius Comp at the control is not used, a "metal on" condition will always result on chamfers and radii.

The Tool Offset is already active; you don't have to specify the Tool Offset when you start Tool Radius Comp, nor do you have to cancel the offset when you cancel Tool Radius Comp mode.

Regards,

Bill

 

[Rich L]

Thanks, again, guys. The code alterations worked and now I can tune the program. Lessons learned for next time.

Cheers,
Rich

 

[Dave K]

Wait a minute. If this is a turning tool, don't you need to use tool tip 3, and not 2?

 

[AHC]

Gang tool lathe, turning with a left handed tool. X- side of the part

 

[Dave K]

Gang tool lathe, turning with a left handed tool. X- side of the part

Ok. He called it a "rear lathe" in the original post, so I assumed that meant the tools are all towards the rear of the machine like a turret style cnc.

 

[yardbird]

Wait a minute. If this is a turning tool, don't you need to use tool tip 3, and not 2?

Not always I've worked on machines where they were swapped or different altogether. Look at these pictures I posted of this LeBlond up on the corner of the control I have the tips (tip 3&5) marked so I didn't get confused with the other machines.


Brent

http://www.practicalmachinist.com/v...cnc-nc-machine-229166/index5.html#post2236432

 

[Dave K]

Not always I've worked on machines where they were swapped or different altogether. Look at these pictures I posted of this LeBlond up on the corner of the control I have the tips (tip 3&5) marked so I didn't get confused with the other machines.


Brent

http://www.practicalmachinist.com/v...cnc-nc-machine-229166/index5.html#post2236432

So, an OD turning tool on that was not tool tip three? That would go against any standards I've seen anywhere.

 

[yardbird]

So, an OD turning tool on that was not tool tip three? That would go against any standards I've seen anywhere.

Yeah it was tip 3 for OD but ID was tip 5 not 2 like normally would be. I've ran othe machines where OD was tip 2 and ID was tip 3. Actually I believe its up to the MTB as to what the tip are


Brent

 

[yardbird]

To the OP.. I would use extreme caution canceling comp on a G0 rapid move. Depending on how the tool is positioned what the situation is you do not need to cancel comp but need to switch it. Ask me how I found this out. The hard way obviously.

 

[angelw]

Yeah it was tip 3 for OD but ID was tip 5 not 2 like normally would be. I've ran othe machines where OD was tip 2 and ID was tip 3. Actually I believe its up to the MTB as to what the tip are


Brent

Hi Brent,
Its not a MTB thing, the control calculates the true position of the tool based on the Tool Nose Radius, and the position of the TNR centre in relation to the setting points used in setting the tool. The MTB has no control over this.

Its convention for Imaginary Tool Type 3 to be used for OD turning on the positive X side of the centre line and from a plus Z to minus Z direction. On machines where two tool turrets share the same fixed slideway; one on the X+ and the other X- side of centre line, such as a Mazak M5, then the Imaginary Tool Types are reversed for the turret on the X- side of centre.

If Imaginary Tool Type 3 is being used for OD turning on your LeBlond, it would be extraordinary for Tool Type 2 not to be used of a Boring tool with the tool set on the leading edge of the insert in Z and on the point of the insert radius closest to the centre line. Any Imaginary Tool Type number can be used for any operation, if the tool is set in accordance with the Tool Type number being used. Obviously its not recommended, and its more difficult.

In the case of a Gang Tooled machine, a tool used to OD turn on the X- side of centre will be set in the same way as a boring bar used on the X+ side of centre, and hence the Tool Type 2 usage.

Regards,

Bill

 

[ZachN]

Bill, I just learned so much from your post! Thanks! I have a gang lathe and comp and tool tip types has always screwed me up! Thanks

 

[Rich L]

Ok. He called it a "rear lathe" in the original post, so I assumed that meant the tools are all towards the rear of the machine like a turret style cnc.

On the "rear lathe" thing, I got this from Smid's Programming Handbook p. 275 3rd edition:

..."standard tool tip numbering for rear orientation CNC lathes - those with X+ up and Z+ to the right of origin." The figures on the next page showing tool tip orientation bear out the T2 and T3 numbers I used. Fortunately, my lathe is consistent with this.

_________

I have another question, though. There are two "offset" displays/pages: one for geometry and one for wear and I had entries on the wear page for "R" as well as entries for "R" on the geometry page. I must have entered them both in my naïveté at the outset. The radii I entered on the wear page are identical to the ones I entered on the geometry page. That is, tool tip 2 had wear radius = .008 and geometry radius = .008

I'm not sure I even understand what wear on a radius would mean given that geometry could/should/might be able to accommodate. According to the Fanuc Operators Manual the wear radius gets added to the geometry radius. Given that's true, for tool tip compensation my radii were double what I had intended.

I'm fixin' to remove the wear entries but I'm wondering if that was a contributor to the initial problem with the 041 error code I got for interference.

Cheers,
Rich

 

[AHC]

wear offsets are to compensate for insert tip wear. If you add a value to the Geo and Wear pages together you may well overcompensate for the tool and get an alarm.
I generally haven't needed to wear comp for a tool tip unless the part is very fussy about radiuses (radii? ) or tapers. And then I would just check the tip on a comparator and enter the actual value into Geo.

 

[706jim]

I was initially confused about those two radius values (on the geometry and wear screens).

Eventually, I figured out that the "wear" screen values would be the change required as the insert wears, that is, starts with "0" value and would change only slightly. So, yes, don't put TNR in both of these screens; practically just on the geometry screen.

When working with lathe inserts, the compensation is minimal compared to milling, so if you screwed those values up, they wouldn't be immediately noticeable.

 

[Dave K]

The geometry page should show the radius value of the tool point radius. The wear page should be 0. Otherwise you're comping the radius twice. The radius value in the wear should only be used to fine tune the radius on your part, should it be just a tad off from what you programmed it to be.