What's new
What's new

Tool nose radius compensation

cuttergrinder

Hot Rolled
Joined
Mar 16, 2007
Location
Salem,Ohio
This is probably a dumb question to most but here goes. Does having a lathe tool upside down or right side up effect whether you use g41 or g42
 
The direction the Spindle is turning, which will dictate which orientation the Tool is, has no effect on TNR comp. BUT if you are changing the orientation of the Tool, (IE back turning) then yes it changes.

R
 
No. Best rule of thumb with lathes is there is no rule of thumb. If you are cutting towards the headstock on the OD it should be G42. If you are boring towards the headstock it would be G41. There are way too many variables running a lathe to haphazardly generalize it like that.
 
No. Best rule of thumb with lathes is there is no rule of thumb. If you are cutting towards the headstock on the OD it should be G42. If you are boring towards the headstock it would be G41. There are way too many variables running a lathe to haphazardly generalize it like that.

Except when the Turret is between you and the workpiece or Lower Turret. Or when the headstock is Right of the Operator. Or.....

R
 
You guys .... back to basics. There's the right-hand rule for axis designations and cutter left, cutter right offset for radius comp.

And then there's the better way, which is to write the damned program from the center of the tool nose radius and skip this radius comp entirely. It's a pain in the butt and doesn't do as good a job.
 
Ok thanks guys. So if i am cutting towards the chuck, its G41 and G42 if cutting towards tailstock

Well... no, that isn't correct...

Typically on a turret type CNC lathe when the turret is beyond the X-center..

1:OD turning - Cutting towards the chuck with TNR = G42
2:OD turning - Cutting away from the chuck with TNR = G41
3:ID turning - Cutting towards the chuck with TNR = G41
4:ID turning - Cutting away from the chuck with TNR = G42
 
You guys .... back to basics. There's the right-hand rule for axis designations and cutter left, cutter right offset for radius comp.

And then there's the better way, which is to write the damned program from the center of the tool nose radius and skip this radius comp entirely. It's a pain in the butt and doesn't do as good a job.


Oh My God Emanuel ( note I did not say OMG ... )
Please, just behave like a fossil to be found in a Millennia or Two, and let us old(er) guys help them youngn's of today!
 
Well... no, that isn't correct...

Typically on a turret type CNC lathe when the turret is beyond the X-center..

1:OD turning - Cutting towards the chuck with TNR = G42
2:OD turning - Cutting away from the chuck with TNR = G41
3:ID turning - Cutting towards the chuck with TNR = G41
4:ID turning - Cutting away from the chuck with TNR = G42

Hello Seymour,
Yes, you're right with 1 trough 4 with the turret being beyond the centre line (back of machine), but its also correct when the turret is at the front of the machine (between the operator and the centre line), if X+ is towards the operator.

Regards,

Bill
 
Please, just behave like a fossil to be found in a Millennia or Two, and let us old(er) guys help them youngn's of today!
Well, if he knew the rules then he wouldn't have to ask these stupid questions. We're talking basics here !

if X+ is towards the operator.
With z+ extending from the chuck towards the tailstock then x+ is always towards the operator. Unless the operator is standing on the back side, which I guess is possible but rare.
 
With z+ extending from the chuck towards the tailstock then x+ is always towards the operator.

Well, no.

Clearly you haven't encountered the most common of CNC lathe configuration where the Turret is at the back of the machine and where X+ is away from the operator and Z+ is towards Tail Stock to the right. Further, there are the odd machines that have an increasing X- traveling away from the machine centre line; whether its towards, or away from the operator.

I don't advocate the use of TNRC on a lathe and I calculate the true location of the tool. Tool Radius Comp on a machining centre is almost mandatory, as its the convenient method of obtaining size of a feature when using the periphery of a cutter such as an End Mill. With a lathe, diameter size is generally achieved using an X Offset, not a TNR Offset. However, it has its place in producing accurate profiles, for example roll forms if high accuracy of the profile is required. And it also allows for Tool Insert with a different TNR to be swapped in with very little inconvenience. To do this if the program didn't use TNRC would require the coordinates for the parts profile to be recalculated.
 
Well, no.

Clearly you haven't encountered the most common of CNC lathe configuration where the Turret is at the back of the machine and where X+ is away from the operator and Z+ is towards Tail Stock to the right.
Clearly I have owned four ... no, make that five lathes with this exact configuration except x plus is not supposed to be away from the operator. X plus is towards the operator, x minus is away from center, towards the rear, with the turret moving farther in x minus the farther it gets from center.

This is an international standard. When z plus is towards the tailstock (never seen one that wasn't but that doesn't mean they don't exist), then x plus is toward the operator. X 0 would conventionally be the center. Turret on the back should program in x minus.

The Japs often do not follow the standards, but at least if you know what the standard is, you can wrap your brain around how it is supposed to be.

(It gets a little confusing when you have one turret on the front and one on the rear. I just used separate G92's for each turret.)

The exception I can think of that makes some sense in a Japanesey sort of way is a Mori that cuts upside-down. In that case you have to think of it as the entire machine is rolled over, and the operator should be on the other side of the turret standing on his head. They rotated a normal setup through 180* around the z axis. The Japs like that kind of thing, you'd think the place was in the southern hemisphere or something :)

Further, there are the odd machines that have an increasing X- traveling away from the machine centre line; whether its towards, or away from the operator.
This is not correct, period. Those builders should be shot.

I don't advocate the use of TNRC on a lathe and I calculate the true location of the tool. Tool Radius Comp on a machining centre is almost mandatory, as its the convenient method of obtaining size of a feature when using the periphery of a cutter such as an End Mill. With a lathe, diameter size is generally achieved using an X Offset, not a TNR Offset.
Holy shit, put a mark on the calendar, we agree on something :)

However, it has its place in producing accurate profiles, for example roll forms if high accuracy of the profile is required.
You can achieve the same thing writing centerline ... used to be a bit more work but with cad nowadays it's pretty simple. You're dependent on the insert being correct tho ... which they seem to be.

And it also allows for Tool Insert with a different TNR to be swapped in with very little inconvenience.
I used to be concerned about this. But since I may have changed nose radius twice in twenty years, I quit thinking this was an advantage.

Back to the op question, if he had the basics down this would not even be a question : think of yourself riding the tool. From the tailstock towards the headstock, tool in front, then you want to offset yourself to the left of the programmed dimension. Cutting backwards, towards the tailstock, then offset to the right.

Unless you are a boring bar, then the opposite applies.

Tools on the back side will be the opposite.

If you have a Jap machine that cuts upside-down, then I have to put my ass on a chair and head on the ground and look up, to visualize which direction we are going :)

But if you can keep plus and minus correct in your head, then left-right while riding the tool is easy to remember. Working from principles is much easier than memorizing a table (imo). It is certainly more versatile.
 
The qualification in my comment is "the most common of CNC lathe configuration where the Turret is at the back of the machine and where X+ is away from the operator and Z+ is towards Tail Stock to the right." And that is the most common configuration. I understand the Right Hand rule, but you saying that X+ away from centre line, with the one and only turret at the back is not the norm, is just making yourself out to be..., let see, ah yes, Johnny Larue.

Poll this very Forum on the subject and see what result you get.
 
I agree with just not using TNR comp (instead using X/Z comps/wear/geometry for diameter and length), but I also despise programming at the control, which seems like it would get the most use. As Bill said, handy to switch different rad inserts, but other than that (and making really tight forms/rads) just seems to complicate things IMO.

It's like programming control comp on a mill with cam. It has a use for sure, but it is oh so much nicer (again opinions and all :)) to program computer or wear comp *knowing* you are using a 1/2" or 1/4" endmill... no lead in / lead out problems, 3 flute endmills are hard to check without proper mics, don't have to rely on operator to mic the tools and enter correct values....
 
The qualification in my comment is "the most common of CNC lathe configuration where the Turret is at the back of the machine and where X+ is away from the operator and Z+ is towards Tail Stock to the right." And that is the most common configuration. I understand the Right Hand rule, but you saying that X+ away from centre line, with the one and only turret at the back is not the norm, is just making yourself out to be..., let see, ah yes, Johnny Larue.
Well, it is correct if it the tools are cutting upside-down. In that case it is a rolled-over configuration, where the operator really should be standing on his head on the other side. Or you could consider it a front-turret machine that fell over backwards.

Otherwise, common or not, it is wrong.

Poll this very Forum on the subject and see what result you get.
Poll the whole damned world for all I care, look at the international standard and see what is correct.

We have all agreed to a standard where green is the color of the ground wire. If some twat in China decides to make ground red and +12 green, then floods the market so it's the most "common", that still doesn't make it correct.
 
Otherwise, common or not, it is wrong.

I think that lots of things are "wrong", but it doesn't change that they are what they are. Your argument is null, if OP is using what is most common configuration for the Machine. The configuration you're referring to is NOT the Industry standard, if it were-----they would be common, but they aren't. Machine configuration doesn't need to follow the Cartesian system, it's not the law.

R
 
Well, it is correct if it the tools are cutting upside-down. In that case it is a rolled-over configuration, where the operator really should be standing on his head on the other side. Or you could consider it a front-turret machine that fell over backwards.

Wrong again. Whether the tool is upside down or not (the original question put by the OP) is totally irrelevant with regards to TRN Compensation. Use all LH OD Turning tools on the Back Turret (insert facing up) and feeding towards the Spindle to the Left, its still G42. That's already been covered in this Thread by others, but I guess you missed that.
 
Wrong again. Whether the tool is upside down or not (the original question put by the OP) is totally irrelevant with regards to TRN Compensation. Use all LH OD Turning tools on the Back Turret (insert facing up) and feeding towards the Spindle to the Left, its still G42. That's already been covered in this Thread by others, but I guess you missed that.

It's amazing that someone is arguing with you. You're one of the most knowledgeable people on this forum in my time here.
 
Machine configuration doesn't need to follow the Cartesian system, it's not the law.
Oh for sure, for sure ! My inch, your inch, Jorge's inch, why make them the same ? Let's go farther ! Pounds, kilograms, feet, miles, who cares what the standard is ? We can each have our own ! I'm going to go outside and drive on the left side now, and stop at green lights because standards are meaningless ! Whoopee !

Wrong again. Whether the tool is upside down or not (the original question put by the OP) is totally irrelevant with regards to TRN Compensation.
The discussion (as it developed) was right hand rule. G41-G42 is dependent on tool-right and tool-left, according to the path it is taking. Upside-down and rightside up are supplemental to the left-right question.

Mtndew said:
It's amazing that someone is arguing with you. You're one of the most knowledgeable people on this forum in my time here.
Angel knows Fanuc very well but that is not the entire world. There are dangers in a monoculture. If you want to be a sheep, have at it. Stick your nose up the wooly ass in front of you and follow along ...


It's like this : in the seventies, Monarch and American Tool both had programming manuals. The Monarch approach was like Fanuc - "just do this, and this, and here's a chart of the four quadrants, when in I do this, when in II do that ..."

The American Tool manual explained the theory. If you understand the theory, you can do anything. If all you know is charts and directions, then when something comes along that is not in the book, you're screwed.

This question would never come up if the op had learned what G41 and G42 really mean.

Incidentally, one reason I think tnr is not as good as writing from tool centerline is that you are giving up control of the tool path. When you write the program complete, the tool will go exactly where you want. When you use cutter comp, the control makes decisions about how to fill in the blanks where you go around corners. I came from a machining background, not a click-the-button background, so I trust myself more than a computer to make these decisions. Other people can feel differently.

I still like machining. Some people thing computering is more fun. Different strokes ... but then you read questions from people who don't have a clue asking "why can't I plunge 2" deep with a four-flute 4" long 1/4" endmill then drive it into this corner, let it sit there between direction changes and get a good finish ?" That was a real question just a week ago.

I mean shit, this is supposed to be about machining, not drawing pretty pictures on the screen.

And css sucks dead donkey dicks for roughing on a lathe. So there :D
 








 
Back
Top