anyone know what g-code is used for cutting acme threads on cnc lathe with fanuc control? g-76 not working. Thanks

Why isn't G76 working. I use G76 all the time for acme and stub-acme threads?

G92 quite good, can stipulate each pass. personal preference I use both

I use G76 but G 92 will work just as well. If it's not working it's probably because your spindle RPM is set to high, and you can't move the Z axis fast enough to keep up, so it will either alarm out or not work. reduce the RPM to keep the Z axis speed under control and it should work fine.

Stu

My spindle speed is fine. The minor diameter is good, the pitch is right, pitch diameter is huge (like .04 big). This is my first attempt at acme threads,Im missing something. The machine cuts "normal" threads perfectly.

no difference mate acme or no acme unless your making a mistake with cam software in geometry. are you using Cam software?

no need to feel challenged by this thread.
you will need to take many passes. and perhaps to go sideways to avoid excess load or chatter with your tooling.

can you paste your program to view, and it should stick out like a sore thumb.

Acme threads are 29 deg inclusive. May I ask what diameter and is it a stub acme.

I love to help

1 3/16"-12 stub. Im not at work so cant paste my program. What do you mean by "go sideways"? Thanks. Im not sure if this will make sense but here goes,lets say i just made a 1"3/16-12 60 degree thread. would i be able to just change the insert,tag the cycle start button and make a correct acme thread? (lets assume the major and minor diameters are correct for the acme thread).

I think so mate.

major and minor diameters are correct.
you have the pitch (12 tpi)
( you have the insert/tool correct geometry )
your speed and feeds are acceptable you say

are you programming in g99 or g98? 95% of the time on lathe you must be in g99 but sure this is the case.

what i mean byt sideways is ok here is an example for the G92 code:

G54G99
T1??M8
G97M3S400
G0X35.Z10.M23
G92 X29.5 Z-120. F2.117
X29.
X28.6
(stay above root)

G0X35.Z9.8
G92 X29.5 Z-120. F2.117
X29.
X28.6
(AND SO ON UNTIL THE ROOT DIAMETER)

Thats all I mean by sideways

Mate, what's the end result of thread and/or alarms your getting, trying to do this. What controller and machine you have?

if you have high spindle speed your exit may look crap.
regards

The threads look perfect, no alarms no chatter. minor dia is right on, pitch dia is about .04"(1.01mm) over size (mic over wires) The thread gage doesnt even want to start. fanuc control, By changing your starting z from z10. to z9.8 are you making the valleys wider? I know almost nothing about acme threads. Are they supposed to be wider than the insert? If I put it on the comparitor, the insert fits the valley perfectly.

yes they will be wider. I wanted to warn that, as a way around chatter. after my last post

what is your thread gauge? Are you looking for a loose fit.

I am running out of ideas. I'm very logical and practical person. If all else fails, perhaps your testing gauge is non standard.

You 100% certain it's an acme, not square/ trapazoid?

there is no mystical thing to this. There is human judgement error or blip in program in my eyes.

regards

scappini

eject let me show you a typical program I have done a few weeks ago for an acme thread

here is one on my programs
I needed to grind a tip on a tool and cutter grinder
hope this helps:

T404 (3 TPI ACME TUNGSTEN BRAISED TIP)
G97 M03 S225
M08
G00 X109. Z6.
M24
G92 X104.2 Z-37.3 F8.467
X104.
X103.8
X103.6
X103.4
X103.2
X103.
X102.9
X102.8
X102.7
X102.6
X102.5
X102.4
X102.6
X102.2
X102.1
X102.
X101.9
X101.8
X101.7
X101.6
X101.5
X101.4
X101.3
X101.2
X101.1
X101.
X100.9
X100.8
X100.7
X100.6
X100.5
X100.4
X100.3
X100.2
X100.1
X100.
X99.9
X99.8
X99.7
X99.6
X99.5
X99.4
X99.3
X99.2
X99.1
X99.
X98.9
X98.8
X98.7
X98.6
X98.5
X98.4
X98.3
X98.2
X98.1
X98.
X97.9
X97.8
X97.7
X97.6
X97.5
X97.4
X97.3
X97.2
X97.1
X97.
X96.9
X96.8
X96.7
X96.6
X96.5
X96.4
X96.3
X96.2
X96.1
X96.
X95.9
X95.8
X95.7
X95.6
X95.5
X95.4
X95.3
X95.3
X95.3
G00 X109. Z5.9
(.1MM TO THE LEFT)
M24
G92 X96.8 Z-37.3 F8.467
X96.7
X96.6
X96.5
X96.4
X96.3
X96.2
X96.1
X96.
X95.9
X95.8
X95.7
X95.6
X95.5
X95.4
X95.3
X95.3
X95.3

now this was only designed for a loose fitting Giuberson hose fitting but this is only in respect to Tolerance.

If your tolerance is within limits, and lower limit is correct (assuming tool is not buggered)
I would definately look at your thread gauge.

regards

scappini

i use gibbs cam also at work so I'll look and see if gibbs have a program for 1-3/6" stub acme in the morning.

you might need to look at an alternative stub acme thread which is the standard tolerances at major diameters and thread thickness at the pitchline (.5P). The basic heiht of thread form 1, height is 0.375P as compared to 0.250P for form 2.

The width of flat in form 1 internal is 0.4030P and for form 2 is 0.4353.


So perhaps you need to look at this perhaps you meant to be machining an alternative stub acme thread.

Hope this helps.

form 1 being standard and form 2 being alternative... sorry!

Its a customer supplied thread gage,(doesn't mean it isn't damaged) But the reading over the wires seem to back it up. I'm out of ideas as well. I think it just became the day-shifts problem.Iwill let you know when we do figure it out, Thanks very much for your help,

Some threads I have done in acme style have been double start threads and I have used the (from memory) G32 cycle. I would do one z position then the other at a particular diameter and then repeat the pair at the next diameter and so on and so on. The G32 cycle is typed out in longhand. I mean all four points for each and every pass. It enables you to enter or exit a pass at an angle which helps if the thread is not at the end of a part or to do a left hand thread from chuck to tailstock direction. Lots of code but lots of control.

PS...Where I work has two Fanuc controller lathes but one is a 21i and the other is 21(some other letter!). The G code designations for the various thread cycles vary from one machine to the other. Eg G92 versus G84 (from memory) etc. And one lathe has no deep hole drilling canned cycle!

How did this end up? Did it ever get resolved?

anyone know what g-code is used for cutting acme threads on cnc lathe with fanuc control? g-76 not working. Thanks
Check your insert. Acme and Stub Acme are not the same.
Also I have ran into problems with insert grinders that make Standup (triangle)Acme Inserts that work fine on the OD but not the ID.

I run mostly Acme Threads and have not incountered any problems using
either G76 or G92 code. I prefer G92 code becuase of more control.
My threads are chatterless and shiny not dull.

In reply to Kmacke.
The company I work for bought two CNC Lathes in quick succession around the year 2000 from the same dealer. The first was a Harrison Alpha 400s with a Fanuc 21 controller. The second was a Colchester Tornado A90 with a Fanuc 21iT controller. The controllers are almost identical but with a few annoying changes in the names of some of the G codes.

On the Alpha Lathe you can thread with G32, G76 and G92. Spindle speed is limited by the G50 command, mm per rev is G99 and there is no deep hole drilling cycle. There is only a pecking cycle for drilling.

On the Tornado Lathe you can thread with G32(possibly), G76 and G78 (I said incorrectly in my previous post it was G84). Spindle speed is limited by the G92 command, mm per rev is G95. There is a deep hole drilling cycle. G78 is the same cycle as G92 but a different designation is used.

We have found that the dealers we bought the Lathes from are not so interested in helping with any problems, after they get their money!

Sencinia, you are right, It turns out we had purchased the wrong inserts for stub acme threads. G92 worked fine, we ran them as normal,shifted in .006" with a seperate offset and re- ran the G92 path. Worked as a quick fix, we will get the right inserts before we turn anymore stub acme threads. Thanks guys!