Results 1 to 6 of 6
Thread: thread programming on lathe
07-21-2013, 10:01 AM #1
thread programming on lathe
I was looking through a tooling catalog for threading tools. In the catalog they said something about the canned threading cycles on a lathe doesnt make real good threads sometimes because of the depth of cut isn't deep enough or something. It said that it is better to write a custom program for threading? Now im new to this stuff so I do not know what they are talking about. Anyone know what they are talking about and if you do can you give me an example of a custom threading program. Thanks again.
07-21-2013, 10:20 AM #2
Explore the Haas programming manual, paying attention to the G76 and G92 cycles.
Both are threading cycles that will likely work well for you.
07-21-2013, 10:42 AM #3
07-21-2013, 11:32 AM #4
G92 will give you custom threading.
example...2''-12 thread...numbers may not be accurate but it's just for show.
G92 X1.980 Z-3.00 F.0833 DEPTH OF FIRST CUT CAN BE AS HEAVY OR LIGHT AS YOU NEED
\X1.960 CAN MAKE CUT DEPTH WHAT EVER I WANT IN EACH X MOVE...THE \ IS THERE FOR THE FIRST PASSES TO ALLOW ME TO SKIP THEM IF I RERUN PART TO HIT SIZE,NOT NEEDED BUT HELPS ON DEEP THREADS
X1.895 be careful on taking light cuts in a thread.sometimes you need a couple light passes for spring back.Other times it will cause chatter or shitty thread..you just have to give it a go and adjust from there.
G00 X10. Z.03
G76 can be custom to an extent.In the settings there are factors you can change to control how much it leaves for last pass and a few others,sorry I forget now because I have mine set and never muck with it much.
G76 is like using the compound and slide to move the tool in at an angle and only cut on one side.G92 just goes straight in and cuts on both sides of tool.
G76 A59 K.054 D.02 X1.892 Z-2. F.0833 that's it,same thread as above just less punching of the buttons.On HAAS control every thing is needed in this sample to cut.The settings in the control cover all the other stuff.
A59 this is the angle of the thread.It is not 60 degree so it gives you just a lil clearance on the tool as it works its way down the profile of the thread
K value is simple take depth of thread and devide by two,if book says thread total depth is .100 I add a few then devide that number
X is the major thread diameter minus total thread depth
D is what it will take on first pass...try to take a decent size cut here
Z of course is how long the thread is
F 1 / number of threads 12threads = 1 / 12=.0833" for F
The way I do it may not be up to par with those that have much more knowledge than I do but it works and we make money and customers are happy.
07-25-2013, 09:20 PM #5
thread programming on lathe
I use canned threading cycles all day long with no issues. On my Hass "ST" series lathes you can go into your setting and change depth of cut per threading pass if need be. This has worked very well for me when I clip Acme and Stub Acme threads by putting grooving insert and running threading canned cycle .010-.015" doc instead of .003-.005" doc
07-29-2013, 07:34 AM #6
The vast majority of threads cut on CNC equipment, and that's the vast majority of threads cut at all these days, comes off of canned thread cycles. I can't feature where a tool catalog would get off telling you right off the bat that canned cycles won't make a decent thread.