CNC Lathe Single Point ID Threading Help For First Timer

Got my first CNC theading job coming up this week. 60 parts out of 4140 annealed 1 1/4 hex. Roughly 6" long with an ID thread of M22 X 1.5 Left Hand. The customer is looking for at least 2" of usable thread on this ID.

Question 1: What bar to use?

Steel Thru Coolant Bars - (Not enough money in the job to buy a $310 carbide bar.)

Both just make it as far as the 0.81" Minimum Bore requirements go.

1/2" Top Notch insert bar?

5/8" Laydown Insert bar?

Which of these threading bars would you choose? Obviously one has a larger diameter then the other, and a person would think that is the one to use, but I'm unfamiliar with the nature of the two different types of threading inserts and am curious if the nature of the inserts will sway the answer regardless of bar size. My gut tells me the 5/8 lay-down setup, but what do I know?


Question 2: Inserts

Full Profile?

Partial Profile?

No experience with either.


Question 3: Technique:

Thread towards the chuck?

Thread away from the chuck?

I'm kind of liking the threading away from the chuck idea but am wondering if this can be done without a thread relief? This is a 2000 Mori with Fanuc 18i control if that matters. On this ID, can a guy just barge into the stock at the bottom of the bore without a relief cut there? If run in one non stop cycle, will the tool tip start in the same place every time and not inadvertently run a pass into previously uncut stock? Not sure how that plays out.

As an aside - anyone know where to get a M22 X 1.5 Left Hand Spiral Flute Tap at a reasonable price? I'd machine tap this thing if I had half a chance... and could afford it.

Fellow machinists... I beg your wisdom on these matters. Thank you.

Dave

Always use the biggest bar you can fit in the whole so I would go with the 5/8 bar with laydown inserts. And use full profile inserts. Don't mess around.

I may be wrong but I don't think G76 cycle lets you thread away from the chuck. Plus, depending on the lathe, you need to start away from the part (usually 0.2") for the spindle to synchronize better. I would get the correct left hand bar (insert facing up) and not mess around trying different things for just 60 parts.

If you're going to use a left hand bar and thread into the bore, don't forget to run the spindle in reverse.

I like the top-notch myself, just for rigidity's sake.
Unless you're running a LOT of parts or doing that thread again in the near future, go with a partial profile. That way you can use the inserts for say a 1-8 or 1.5-6 thread.

Plunging in like that is probably not recommended but you can get away with it doing light cuts. I do this all the time on OD threads on my old mazak which uses "right side up" tools in the turret and cuts everything CCW rotation. Feeding this way may help keep chips out of the hole.

I like top notch bars, but in this case things are tight and I would taker the bigger bar. Might still be tricky even with a 5/8 bar. Full profile with make things easier.

Usually easier to Tap really deep holes like this, but that might be a tricky one to find.

Fancuku said:

.........I may be wrong but I don't think G76 cycle lets you thread away from the chuck. Plus, depending on the lathe, you need to start away from the part (usually 0.2") for the spindle to synchronize better. ........

Click to expand...

No problem with G76 starting at the chuck and moving Z positive.

The length of imperfect threads due to axis acceleration depends greatly on the spindle speed programmed and the accel parameter the machine uses and the mass of the turret. IME, 1 to 1.5 leads is enough in most cases.

Thank you everyone for your input. I appreciate it, and every little bit helps.

I'm beginning to pay attention to some of the finer details like Minimum Bore.

I'm looking at a 5/8" bar that leaves only 0.022" clearance in the bore at zero cutting depth. Even though there is more clearance around the tool head, that doesn't sound like enough room in a 2" deep hole. I'm wondering if I should forget about using a 5/8" bar and fighting a tight bore situation and just settle on doing the job with a 1/2" bar regardless of insert type.

I guess my question is, just because the tool will fit down the bore doesn't mean it will actually work in practice? Or does it?

My thru coolant is just that, and not High Pressure. I have a 215 PSI unit but it's not plumbed in yet.

So is this tight going to be a fight?

Dave

a .625 bar will not work in a .625 hole, you need room for pull off which can vary depending on machine parameters.
you want the biggest possible for rigitty. laydown full profile is the way to go
as for threading out, just start in the hole and thread out to z positive number

A 5/8" bar, going 2" deep, in a 0.656 hole, is not going to work. (without an internal thread relief to change thread diameters.
The slight clearance will give you chip control problems, even threading Z- to Z+

If you do use a Ø1/2" bar, you may want to think carbide. (not Noob friendly, at all)
Failing that, a steel bar is right at the limit of the 4/1 (length / diameter ratio) used with steel bars.

ETA: What about a 15mm bar? (0.590")

The hard part will be keeping chatter from starting. Once it starts, it will not go away....
(caveat: unless you can alter your RPM/ harmonincs when threading single point. IIRC my Okuma control will do that.)

Whoah partners, that 0.022" clearance is at ZERO cutting depth as I said. Meaning that's what's left on the back side of the bar with the insert just touching. The bar specs at 0.787" minimum bore and the hole is 0.81" as was mentioned in the original post. Center of bar to tool tip is 0.472", so actually that's what leaves me the 0.022" on a 5/8 bar. (0.025 corrected) The bar is rounded with flats and does have the typical little bit of undercutting at the head area. I'm beginning to think it's okay, but again... what do I know? Been a long time since I threaded on a lathe, and never on a CNC one.

Sorry for the confusion.

Would it be too much to ask to re-comment knowing the correct criteria?

Please and thank you.

Dave

Bar: R166.0KF-16-1220-11B

Insert: R166.0L-11VM01-001 1020

Right hand bar, thread from headstock to tailstock. Low depth of cut, low spindle speed. It's only 60 parts so another 20 seconds threading won't make or break this job hopefully. I would probably start at .006 depth and spindle speed of 400. It's not an ideal setup but should work okay.

I always try to buy tooling I know I am going to use in the future. Left handed tooling is not one of the higher priority candidates so if I can get away with a suitable RH version I do.

Also don't let the minimum bores be absolute God's word. That .787 you referenced is probably the minimum bore to prevent the heal of the insert rubbing. Drill size is .807, and you have a .625" bar. You have a little under .100" clearance for chip evacuation. Minimum bore diameter has nothing to do with it.

Since you are drilling a Ø20.5mm hole, the 5/8" bar will fit, and leave room for chips to flow towards the tailstock.

PS. I hope you have a gage (or if the customer will allow, a L/H bolt) to check the thread with.

Thanks again all. Yes I think the 5/8 bar will be the way to go. I do like the idea of the bar bigjon61 mentioned where the cutting end is fully relieved. I've been looking at more all one diameter bars but can see how all that relief up at the business end equals much needed chip room.

With laydown inserts moving away from the chuck it looks like a right hand tool with right hand inserts is called for. Though what I've been noticing on these 11 and 16 size insert bars, is there is no option for changing to a minus 1.5 degree shim which seems to be called for. What's a person supposed to do about that? Does it not matter at this size thread?

Been wanting to go with Full Profile inserts, but only if I can buy them one-zy two-zy style. 250-350 bucks for a box of inserts where I'll die with 7 still in the box is not my plan.

I do have a tie rod end from the customer to check the thread with. And now that I have a sample in hand, that 2" depth is deep, but I'm beginning to think it's not THAT deep.

Dave

Fancuku said:

Always use the biggest bar you can fit in the whole so I would go with the 5/8 bar with laydown inserts. And use full profile inserts. Don't mess around.

I may be wrong but I don't think G76 cycle lets you thread away from the chuck. Plus, depending on the lathe, you need to start away from the part (usually 0.2") for the spindle to synchronize better. I would get the correct left hand bar (insert facing up) and not mess around trying different things for just 60 parts.

Click to expand...

Hello Fancuku,
As mentioned by Kevin, no problem with using G76 from the Chuck towards the Tailstock. The only issue will be the tool will be moving at Rapid Traverse speed into the start of the Thread if no Relief Groove is provided.

With regards to the Thread Error experienced at the Start of a Thread, this also occurs at the Finish end of the Thread due to Deceleration. Accordingly, there will be infinitesimal difference at the inboard end of the Thread irrespective of whether the Thread is cut going towards, or away from the Chuck.

@13engines

With regards to cutting away from the Chuck and the Tool moving at Rapid Travers into the cut when a relief groove is not provided, this could be avoided by using G32 to cut the Thread. The control has a function called Continuous Thread Cutting, where a number of G32 Commands are strung together to produce a Threaded surface where change of direction and and Lead is possible. In the example of a Thread starting at the Finish end of the Thread and with no relief groove provided, G32 will provide a synchronized in feed to the cut diameter for each pass. Continuous Thread Cutting also circumvents the Lead Error at the start of the successive Thread elements.

The only negative for using G32, is that the Threading Process has to be coded long hand; no cycle to minimize program code. However, a Macro to Loop the code for one pass, with a new DOC for each pass, would be easy to write.

Regards,

Bill

I often program a slight taper to I.D. threads to counteract any flexing of the thread tool.

6" long 4140 Hex parts, I bet material is pricey. Seems like the price of 4140 hex has quadrupled over the last 10 years and then some.

Dualkit said:

Seems like the price of 4140 hex has quadrupled over the last 10 years and then some.

Click to expand...

Hex? Oh yeah, that is not a cheap bit of material.
It seems most materials have gone up in price; though, the price of scrap [anything] is lower than I have seen in the last 10 years.

Dualkit said:

I often program a slight taper to I.D. threads to counteract any flexing of the thread tool.

Click to expand...

Depending on the workpiece and set up, some Taper in the Thread Program may be required, but usually, taper in a Thread is caused by the Workpiece flexing, not the Tool. It would be a fair presumption that the flexing of the Threading Bar will remain constant (except for the very first Thread Form), given that its diameter and stick-out doesn't change during the path of the tool along the length of the Thread.

Regards,

Bill

13engines said:

1) Been wanting to go with Full Profile inserts, but only if I can buy them one-zy two-zy style. 250-350 bucks for a box of inserts where I'll die with 7 still in the box is not my plan.

2) I do have a tie rod end from the customer to check the thread with. And now that I have a sample in hand, that 2" depth is deep, but I'm beginning to think it's not THAT deep.

Dave

Click to expand...

Dave,

1) I remember well, the days when I first started, there never seemed to be enough money on parts, to buy all the tooling you need to do the job. (Truthfully, that is still the case at times.)
Don't undersell your service, just because you are the new guy on the block. You have a lifetime of tools you will need ahead of you, and hopefully many years to accomplish all the new toys.

2) I am glad they provided you an easy means of gaging [their] thread.

Sometimes a job looks easy, but "Doh! I didn't foresee this actually being a PITA"
other times, it is the opposite.

Doug.

angelw said:

@13engines

With regards to cutting away from the Chuck and the Tool moving at Rapid Travers into the cut when a relief groove is not provided, this could be avoided by using G32 to cut the Thread. The control has a function called Continuous Thread Cutting, where a number of G32 Commands are strung together to produce a Threaded surface where change of direction and and Lead is possible. In the example of a Thread starting at the Finish end of the Thread and with no relief groove provided, G32 will provide a synchronized in feed to the cut diameter for each pass. Continuous Thread Cutting also circumvents the Lead Error at the start of the successive Thread elements...

Regards,

Bill

Click to expand...

I was sure the entry into the cut without thread relief was going to be iffy, and honestly unilt you mentioned it and I then peeked at the thread cycle diagram, I hadn't realized it was going to be at the Rapid Rate. Even if at feed, I'm thinking threading feeds are a moderate version of Rapid to begin with.

angelw said:

Depending on the workpiece and set up, some Taper in the Thread Program may be required, but usually, taper in a Thread is caused by the Workpiece flexing, not the Tool. It would be a fair presumption that the flexing of the Threading Bar will remain constant (except for the very first Thread Form), given that its diameter and stick-out doesn't change during the path of the tool along the length of the Thread.

Regards,

Bill

Click to expand...

Don't you just hate it when a guy has all the answers, and correct and reasonable ones at that? I don't! :-) It's hard to grow tired of knowledge much greater then your own. Thank you Sir.

doug925 said:

Dave,

1) I remember well, the days when I first started, there never seemed to be enough money on parts, to buy all the tooling you need to do the job. (Truthfully, that is still the case at times.)
Don't undersell your service, just because you are the new guy on the block. You have a lifetime of tools you will need ahead of you, and hopefully many years to accomplish all the new toys.

Sometimes a job looks easy, but "Doh! I didn't foresee this actually being a PITA"
other times, it is the opposite.
Doug.

Click to expand...

Thanks Doug for the inspiration and understanding. When they said "the devil is in the details," I'm pretty sure they were talking about small-ish bore left hand ID blind hole threading.

My customer texted about an hour ago asking how things were going. I called back with the bad news that so far I got nothin as I'm still researching. I then come to find out he's done this thread in the past with a straight flute hand tap on his manual lathe. All the way in and out without a problem or chip breaking. What the? I'd have never thought. Must be because it's fine threads. That particular type of tap is the only kind you can find on the shelf for this thread. I even have an RFQ out to a tool maker for a left hand spiral flute tap, which was beginning to look like the most cost effective way to get through this job. Won't be needing that. There's still a 7/8-14 RH OD thread to deal with which is not as troubling.

Thanks everyone for your help. I've still learned a lot! A straight flute LH hand tap has thrown the life preserver my way.

And really... customer's waiting.

Dave