Lathe roughing cycles (G71 vs G72)

[jhov]

I'm learning lathe programming and from what I can see most people seem to use rough turning (G71) instead of rough facing (G72) to rough out a part. I'd imagine that rough turning would increase time in the cut and minimize rapid moves, but at the same time it seems it would be less rigid, as you're machining away your support material at each pass. Rough facing would preserve the supporting material until the end, but it'd give your spindle a workout if using constant surface speed. Is there some reason why G72 isn't used to rough profiles?

 

[angelw]

Is there some reason why G72 isn't used to rough profiles?

It is used; often.
It comes down to which method for the part profile is going to be the most efficient. Clearly a short, large diameter piece is more suited to being rough faced with G72.

If you have a workpiece of a length that will suffer by its rigidity being diminished via longitudinal cuts being made, to the extent that it causes problems, then its likely that it should be supported by a centre. If the part is going to be a problem roughing it longitudinally, its also likely to be a problem when taking a finish cut.

So, with your plan, you've roughed this longish part using a G72 Cycle, how do you propose to finish it now that its less rigid?

Regards,
Bill

 

[gcodeguy]

I use whichever method keeps the insert in the cut for the longest....most of the time. We have a few barfeed lathes where if making more than one cut to a shoulder, it will push the material back unless making shallow cuts. Normally I will just make the lighter cuts (increase feedrate) and stick with G71 because a lot of our jobs are smaller diameters.

However, there are times because of a parts larger diameter I will switch to a G72 so I can make heavier cuts at decent feedrates and not have to worry about the part pushing back. Especially on what are longer parts (for us). In those cases I often rough and finish turn in sections as long as the part isn't the same diameter for the full length. Not that there hasn't been a few times where I did have to rough and finish turn a diameter in sections because of how small it was and how long the part was. Always a fun job then. NOT! Those type of jobs are best done on a Swiss lathe....which I may have to program, but don't have to set up and run. Lucky me.

 

[jhov]

It is used; often.
It comes down to which method for the part profile is going to be the most efficient. Clearly a short, large diameter piece is more suited to being rough faced with G72.

If you have a workpiece of a length that will suffer by its rigidity being diminished via longitudinal cuts being made, to the extent that it causes problems, then its likely that it should be supported by a centre. If the part is going to be a problem roughing it longitudinally, its also likely to be a problem when taking a finish cut.

So, with your plan, you've roughed this longish part using a G72 Cycle, how do you propose to finish it now that its less rigid?

Regards,
Bill

I'm new to lathes, so I don't speak from any experience (hence my question); but I would think that a finishing pass would be a much lighter cut exerting less tool pressure, no?

 

[angelw]

I'm new to lathes, so I don't speak from any experience (hence my question); but I would think that a finishing pass would be a much lighter cut exerting less tool pressure, no?

Occasionally chatter will occur on a finishing cut when it hasn't during roughing. This happens mostly on parts that are of a length that's borderline requiring tailstock centre support. In the roughing cut there is sufficient pressure that stops the parts bouncing, but in finishing, not so. This phenomenon is common in thread cutting, where the thread cutting is chatter free right up to the last finish passes. However, there is no hard and fast rule and all jobs have to be approached according to their own merits.

However, a rule of thumb for a finishing DOC, is that it should be at least equal to the tool nose radius of the insert. Using your logic of lighter cut less tool pressure doesn't apply. There is actually more push away with a finish cut that is considerably less that the Insert's TNR, than when its equal to or greater than.

Regards,

Bill

 

[DouglasJRizzo]

I used G72 a lot when I had to rough out a part that had a small diameter hub projection on a large diameter gear blank.

 

[sinha]

G94 would have been simpler in this case.

 

[DouglasJRizzo]

G94 would have been simpler in this case.

Sometimes. However if there are contours to be roughed, G72 would be more accommodating.

 

[sinha]

G94 can only do straight or taper facing. No circles.