What's new
What's new

Single point threading and cnc lathe power

TauRunUm

Aluminum
Joined
Feb 18, 2021
I have problem with easy (in terms of tolerances) steel screw with thread, so look specs from Star KNC-20 swiss on which I am trying to make it (problem is thread) to look is there any hint

and found out:

max. dia. for cutting M10x1.5, max. dia. for thread tapping M10x1.5? I mean you would expect lathe which can do 20mm dia. can cut M14 in steel? Of course slow and with lot of passes?

but in spec they say M10x1.5 and it is same as tapping?!?

Thread which I am doing is M14x1.5 and it is 7.5mm long.

I use G92 cycle because it works perfect on brass screws we made. It is quite similar screw so program isn't problem.

Older collages (sadly we don't have cnc lathe guys) are convince spec isn't true because you on manual lathe you can do any thread you want, just slow speed and many passes.

I tried different speeds (100-500) and many passes (reducing depth of cut as going deeper and do clearing pass in end) but thread looks awful no matter I do, it is more like ploughing then cutting, as machine simple don't have power to cut thread, which is strange to me based on what manual lathe folks say.

Btw tried HSS and Carbide tools. Similar thread.

Steel is probable some junk but it isn't some super hard stuff so I doubt it is problem? Or could it be?
 
I tried different speeds (100-500) and many passes (reducing depth of cut as going deeper and do clearing pass in end) but thread looks awful no matter I do, it is more like ploughing then cutting, as machine simple don't have power to cut thread, which is strange to me based on what manual lathe folks say.

Btw tried HSS and Carbide tools. Similar thread.

Steel is probable some junk but it isn't some super hard stuff so I doubt it is problem? Or could it be?

100 to 500 RPM is way too slow to single point a thread on a CNC machine. Crank it up to 1,000 to 2,000 RPM and the threads should cut much better with carbide tooling and coolant or oil as lubricant. I would run probably 10 to12 passes on the threading cycle.
 
Okay I will try that but in manual of machine they put 500rpm as max for M14 in steel?

Though manual don't even mentioned carbide inserts only HSS and brazed carbide tools so that could be case.

It doesn't cost us to try 1000-2000rpm after all.

I do similar amount of passes.
 
A KNC-20 should be fine single pointing any O.D. thread in it's size range, it is tapping where it will lack power.
Why don't you post some pictures. I agree with kick up the RPMS, at least to 800. I like 12 passes also. Use insert tooling only.
 
The m10 max has to be for tapping and die cutting, which take much more torque. Single pointing takes little torque. Agree with others unless material is hard 500 rpm way to slow for m14. For carbon steel try 2500. Keep overhangs as short as possible. Compounding in at 29 or 30 degrees will sure help on a bigger thread.
 
I think the problem is more likely because of DOC which cannot be properly controlled with G92.
Try G76 with 1000 rpm.
There is enough info about G76 on this forum.
 
QT guythatbrews Keep overhangs as short as possible.

If there is no way to keep the part short perhaps adding a center for tail center support, perhaps make the part 1/16 longer for the tail center, and then snub it off if the part can have no center.

Some inserts are just not very sharp-edged, and sharp is what you need.
Going straight in with cross makes a very long chip considering you are taking from both sides of the V of the thread.

For manual lathe threading like some side cutting edge rake, and I pull the chip off the left edge with having theh compound at 29-30. I don't know if you can accomplish that with your CNC lathe.
 
I think the problem is more likely because of DOC which cannot be properly controlled with G92.
Try G76 with 1000 rpm.
There is enough info about G76 on this forum.

On the contrary with g92 the user can exactly control the DOC, and the infeed angle and the infeed flank. Using G76 the DOC is only user controllable within a few (albeit intelligent) parameter choices.
 
On the contrary with g92 the user can exactly control the DOC, and the infeed angle and the infeed flank. Using G76 the DOC is only user controllable within a few (albeit intelligent) parameter choices.

Actually, it is not so. The doc must be controlled in such a manner that nearly equal volume is machined in each pass. G76 does internal calculations to ensure this.

Yes, user has direct control over doc in G92, but does he know how to reduce doc in subsequent passes?
 
Ok. Calculate subsequent doc to ensure equal-volume removal in each pass of G92.
It is not impossible. There is a well-known formula which Fanuc uses.
 
Hi TauRunUm:
Others have already covered much relevant ground but there are important things not yet discussed.

The first is material choice.
Which steel they're made from is hugely relevant...a free machining grade like 12L14 or 303 stainless will be much more forgiving than a tougher alloy like 4140 HTSR or equivalent.
A soft steel like 1018 (commonly called "mild steel" in North America) is gummy as Hell and will always make a shitty thread with torn out and smeared areas and will look like the pig's breakfast you're describing.
A few strategies can help but it will ALWAYS look like shyte and it's not the machine or the strategy that is the root cause...it's the material.

Second is the geometry of the tool: a zero rake tool will plough the material away rather than shearing it.
If you are using inserts with this geometry and especially if you are using tools that are not ground to a dead sharp cutting edge in soft steels, you will also have the problems you describe, and a low horsepower machine will make it worse.

Third, as others have alluded to, your infeed direction determines if you remove a chip from one flank of the developing thread vs both sides at the same time.
So infeeding at 60 degrees for a 60 degree Vee thread requires less force than infeeding at 90 degrees for the same thread.
It will also make a single chip that can shear from the leading flank rather than two chips that converge and pile up upon each other, and the free egress of chips from only one side means less force needed to clear the chips.
Also the trailing flank is cut with negative rake unless the top of the insert is ditched to make it positive rake, so any substantial chip taken by the trailing flank side of the insert will not shear but must plough.

Moving on to the coding strategy...others like Sinha or Angelw can explain this far better than I ever could but here's how I prefer to think of it:

G32 will allow me to control the behaviour of a single pass really well, but I must write code for every single pass, so a complete thread involves a LOT of code.

G92 as I understand it is intermediate in behaviour, automating some things but not others.
I have very little experience with G92 so I don't know it well.
From what I understand that crucial infeed direction cannot be controlled with G92...it will always plunge infeed.

G76 is a complete canned cycle in which you can incorporate one of several threading strategies including the infeed direction, all with only two lines of code.
Apparently there is a G76 variant that some controls understand that is only a single line, but I am unfamiliar with it and how it works.

Which strategy to use is entirely up to what you need to accomplish...for the vast majority of threads cut by most machinists, G76 is so convenient it gets used by just about everyone who knows how it works.

There is one other thing you can exploit to make big threads on a little lathe, and that is to rough it in many small nibbles none of which is a full depth or full width pass.
In effect, you program multiple threads with different start points across the whole gullet of the thread you're trying to make, and then do it all again at a smaller diameter, and again, and again until you reach the thread root.
Obviously, for each depth, you have fewer passes as you get down into the root of the thread.

Once it's roughed, you can walk down the trailing flank in multiple successive passes, across the root, and back up the leading flank.
Obviously it takes a LOT of code to do this...typically I have used G32 whenever I've had to do stuff like this, because I can place each pass exactly where I want it, and I don't know how to do that as easily using G92 or G76.

Really good programmers can automate much of this so they don't have to figure out and write all that code longhand.
I'm not that good, so I bite the bitter pill and do it the clumsy, old fashioned way.

I am not aware of any CADCAM software out there that can do this, but who knows...maybe there is.


Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Thanks for advances,

Doing threads for two weeks, it was RPM problem. 1200rpm and G92 works fine M14 in this steel. Steel they got isn't that bad either by opinion of experienced machinist which made same part on cam swiss but without threading.

Thread would be probable look even better if insert isn't some Chinese one for inox but when I look cost and how it work I am super fine with it.

Box of ten inserts cost me 30dollars.

G32 is problem because we write program on old Fanuc control which is PITA, it doesn't have copy and cut for example, and keyboard isn't great either (small one).

G76 tried year ago and didn't like it, and it was brass thread. G92 works fine. Btw I would use G32 if we can connect PC to machine but don't have time to bother with that too, and if something goes wrong I would be blamed, so this is the way :D
 
Okay I will try that but in manual of machine they put 500rpm as max for M14 in steel?

Though manual don't even mentioned carbide inserts only HSS and brazed carbide tools so that could be case.

It doesn't cost us to try 1000-2000rpm after all.

I do similar amount of passes.
Hello TauRunum,
The limit to RPM in screw cutting is the resulting Slide velocity (RMP x Thread Lead) of the machine. If the resulting slide velocity exceeds the max Rapid Travers rate of the machine the spindle and axis slide won't keep in synch. There is normally a maximum feed rate specified for most machines. Exceed this and the same occurs as with exceeding max rapid.

At 500 rpm at diameter 14, the cutting speed is only circa 22metres per minute; that's slow to moderate for HSS. Using carbide inserts at that speed, you will get a crap finish, extreme built up edge of the insert and very poor tool life. As others have said, its the torque of the machine that is the limiter with regards to the diameter you're able to screw cut on your machine and running slow revs on a largish diameter (for the machine), the torque will be at the bottom end of the scale. The rpm only have to change by a small amount during screw cutting; this can happen when not much torque is available and when it does, the start of the Thread will change in synch with the spindle revs, wrecking the Thread and perhaps breaking the Threading Inserts.

100MPM surface speed at diameter 14 is circa 2,300 RPM; accordingly, 2000 rpm would be a reasonable starting point. That would result in a slide velocity of 3 Metres per minute. which would be well below the max Feed Rate or Rapid Traverse rate of your machine.

Regards,

Bill
 
Last edited:
G76 is a complete canned cycle in which you can incorporate one of several threading strategies including the infeed direction, all with only two lines of code.
Apparently there is a G76 variant that some controls understand that is only a single line, but I am unfamiliar with it and how it works.

Which strategy to use is entirely up to what you need to accomplish...for the vast majority of threads cut by most machinists, G76 is so convenient it gets used by just about everyone who knows how it works.

There is one other thing you can exploit to make big threads on a little lathe, and that is to rough it in many small nibbles none of which is a full depth or full width pass.
In effect, you program multiple threads with different start points across the whole gullet of the thread you're trying to make, and then do it all again at a smaller diameter, and again, and again until you reach the thread root.
Obviously, for each depth, you have fewer passes as you get down into the root of the thread.

Once it's roughed, you can walk down the trailing flank in multiple successive passes, across the root, and back up the leading flank.
Obviously it takes a LOT of code to do this...typically I have used G32 whenever I've had to do stuff like this, because I can place each pass exactly where I want it, and I don't know how to do that as easily using G92 or G76.
Hello implmex,
You have covered it pretty well for the OP. With regards to the one and two line G76 cycles, Fanuc refer to it as FS15 and Standard FS16 format respectively; it can be selected via parameter. The first Block of the two Block format is to set parameters. These parameters are retained until changed by using different values in subsequent first Block of the two Block format. Accordingly, if the min DOC, finish allowance etc remains the same over many different threads you may be cutting, the first Block can be omitted.

With the FS15, single Block G76 Format, the values set via the first Block of the two Block version can be set manually in parameters. The advantages of the single Block version is that compound in feed can be specified from 0 to 120degs in 1 degree increments and the index of the start for multi lead threads can be specified with a "Q" address, rather that shift the Z Start location of the Threading Tool. This can be rather helpful when cutting close to a tail-stock, where there may be little or no scope to either moving the tool closer to or further away from the end of the work-piece.

There are also 4 in-feed methods available, selected by a "P" address.

Regards,

Bill
 
Last edited:








 
Back
Top