G42-G43 on lathes...Why?

[g-codeguy]

I can see why one would use tool radius compensation on mills, but what circumstances would require it on a lathe? I tried it on .007R seats when I first started programming, but it didn't work for me. Probably because I didn't have a long enough move when I called up the G42 code.

Anyhoo...since then I haven't felt a need to use these codes in over 22 years of programming lathes. Is it because most of my parts are relatively simple?

Love to hear from some of the experts on here.

[Geof]

I don't claim to be expert in Tool Compensation on lathes but I have found when turning spheres it is much easier to control size with compensation active.

EDIT

Here is some discussion of Tool Comp on lathes including some links that give an explanation of its value.

http://www.cnczone.com/forums/showthread.php?t=40256

[Jorge-D-Fuentes]

I'm FAR from an expert, but...

I've opted not to use the TNC codes in my programs for two reasons:

1. we always seem to use the same tool nose radius (we don't switch inserts) so I just program my toolpaths so that they're offset from the surface of the part by the amount of the nose. As such, we get the accuracy we need (although we're not making precision parts).

2. I don't quite grasp how to adjust the TNC as one makes the other side of a Radius. I can see how to use it if all the parts were tapering upwards of if I were making rectangular profiles... but I make Ring-like pieces with a radius on top... so I can TNC as I make half of the radius, but don't quite get what to do as I come back around, since what it's doing is offsetting the tool 'left' or 'right' (for profiling I guess it's moving it up by the value of the Radius in the offsets, as well as to the right when doing OD turning with the chuck on the left and the tools on the right).

The drawbacks of (not using) TNC is that you need to calculate your offset toollpaths yourself if you want accuracy, and heavens forbid your company decides to change Inserts and you need precision, since you'd have to rewrite all your programs to match that new insert nose radius otherwise your parts will have little imperfections in the parts that are rounded.

I'd love to use TNC, just in case my company decides to do that. My three current tools are tip 3, 2, 3 (OD Turning, ID Turning, Part-Off (though that last one shouldn't really use a 'tip' really), gang table on the right, chuck on left), which tells the the control how they're oriented so that it can offset them for you.

Using TNC simplifies the profiling process, since you're drawing the surface of the profile, not drawing the intended toolpath, and depending on what your offset parameters are for the Radius, the control would calculate your toolpath for you, and if you change inserts for a tool, it'll adjust your program to match after you input the new Radius into the Offsets.

[M-man]

You need radiuscomp on lathe to easy produce correct profiles when cutting arcs, tapers, chamfers etc. Otherwise you must adjust the toolpath for to achive the correct toolpath.

[Andre' B]

So the guy on the floor can switch to a 0.015 rad insert when he runs out of the 0.030 rad inserts without having to edit all the chamfers and radius cuts in the program.

If all you are doing is straight turning and facing cuts, with no corner radius or angled cuts it does not matter. But if you program for an 0.030 external corner radius on your part without comp. using a 0.030 radius tool and just switch to a 0.015 radius tool you will get a 0.045 radius on your part. Any cuts that are not parallel to the X or Z axes will also be wrong by an amount depending on the angle 45's will be off the most.

Been a long time since I did much programming for lathes, I do mostly mills. So when I did program for a lathe I used tool tip type 0, center of the radius because the resulting G code makes sense (most like a mill). Setup guys don't like it because they have to remember to add the tip rad when they touch off a tool.

[adamant]

It takes some getting use to but it is worth it.

I started on second shift and ran the programs that another fellow wrote, so I had to fix all the comp errors.

TRC is all about precision. If it does not have to be a precise radius that you want to hit the first time, first part, then it is not needed.

[g-codeguy]

Adamant: I do not understand your statement, "If it does not have to be a precise radius that you want to hit the first time, first part, then it is not needed." How can you check a radius on the machine? We have to take the part to QC to do it. Forget the fact that most of our machines are barfeed. Trying to put a part back in the chuck could be a PITA depending on whether is is a sawed slug or not, 1st or 2nd end. Even a casting requires indicating back in. Sorry you had to work with a careless (or unknowing) programmer.

I have to agree that machining a sphere could benefit from tool nose radius comp. We have a couple jobs that have a sphere, and I will try it next time we run one of them.

Andre' B: Never heard of running out of .031R inserts. Might run out of the grade being used, but change grade and modify SFM if necessary. If I can't trust the guy on the floor to use the correct radius insert, how can I trust him to change the R-value?

M-man: Yes, I have had to fudge a program to get the taper I wanted, or even to make a straight cut. Usually it is caused by tool pressure. (We run a lot of small parts.) Don't see how tool comp would help.

Jorge: We have parts with .007R or .008R seats. We use a special seating tool that cuts on both sides of the tool. This is the part I tried MANY years ago to run with TNRC. I could try it again and get back to you with my findings.

Goef: Thanks for the link, and the links within that link! I know how to figure tool nose compensation. I did manual programming for several years. I think you are correct that sphere size could be held better with TRC.

I was interested in what kind of parts would benefit from tool nose radius compensation. So far spheres, and a close tolerance angle are about the only reasons I see for using it.

[Geof]

Originally Posted by g-codeguy .....I was interested in what kind of parts would benefit from tool nose radius compensation. So far spheres, and a close tolerance angle are about the only reasons I see for using it.

In my experience this sums it up quite well.

[M-man]

To get the position of a taper right it is a must to use comp, or to adjust toolpath, meaning that the values of your nc prg is nothing like them on the drawing if you dont uses comp... Look at pic to se what direct drawing dimensions does without comp...

[PatM]

with a good cam post it's not. It is pertty much a left over from the old day's, back when I started there were no computers the way most think NC ran on tape PAPER tape
OMG I'm that old? Well I could give you the whole lesson on cutter comp but why?

[tobyaxis]

Originally Posted by g-codeguy I can see why one would use tool radius compensation on mills, but what circumstances would require it on a lathe? I tried it on .007R seats when I first started programming, but it didn't work for me. Probably because I didn't have a long enough move when I called up the G42 code. Anyhoo...since then I haven't felt a need to use these codes in over 22 years of programming lathes. Is it because most of my parts are relatively simple? Love to hear from some of the experts on here.

TNR comes in handy for parts like these. Because of the angles and radii it makes it easier to program to the print rather than extra trig.

I always use G41/G42 to avoid miscalculating geometry. Why do extra work when you don't have too?? Use the functions of the machine and above all make things simple.

I was always told to work smarter, not harder.

Cheers!!!!

[Jorge-D-Fuentes]

Thanks for the pictures there, awesomeness.

I developed an offsetting parametric draft/model using a combination of Excel and SolidEdge in order to calculate my geometry for me. What it does is basically offset my model's radii and draft contrours/lines by the nose radius, essentially calculating my toolpath for me.

It works... but I fear the day when my company decides to use another tool for OD Turning, for it would render all those 10,000 or so programs useless. It's a standard tool, so I don't see it being discontinued any time soon (it's a 35 degree diamond-shaped insert with what I believe to be a 0.017-0.020" tool nose radius... or so I was told. Hah hah! I could be making the parts wrong all along if misinformed... but no one has complained yet; in fact, they're rather pleased with the results!).

Then again, their margin of error seems to be pretty high, as the pieces I make get treated to a number of steps before they ever make it to the general public.

But yes, working smarter, not harder, is good, heh.

If I used TNC in my programs instead, then I could just go to the Offsets page and enter the new tool's Nose Radius, as well as specify its orientation, and the control would calculate the toolpaths for me...

...but I didn't know that when I started, and I was given the 'promise' of a Cad/Cam package, that only arrived three months ago, when I was already nearly done with the whole thing. I've been in this project for over a year now. Talk about late, heh.

Now I've to learn Mastercam for "Future purposes", although we basically are machining little doughnuts and washers... seems like Overkill to me. Oh well, it's always good to learn something new.

I make similar things to the ones in the picture, only imagine them being only a few millimeters in width, rather than large objects... so our tooling is for small parts.