Need Help!- infeed angle

[jmichaud1]

I am very new to swiss programming and would like some advice on what angle to use for feeding a thread tool while doing a segmented thread. I wrote a really cool macro that will turn-thread-turn but my inserts are just not lasting. They aren't burning up but just chipping a little at the tip of the insert after just a few parts, so I'm thinking it might be in my approach.

If anyone has had successs with segmenting threads, could you please let me know what angle you are sending the thread tool into the part to pick up the next segment.

Also, what speeds are good for threading on the Swiss. I am programming on a Citizen A20 and trying to cut an 8-32 thread 1.625 inches long in 304 SS. I started with 1000 RPM and tried dropping it down to 800. I am more experienced on mills so this Swiss and turning is all pretty new to me.

[danrudolph]

I haven't done any segmented threading, but I would think you could use G92 with a straight infeed on the X. If chamfer angle was a problem, I would expect the inserts to chip on every cycle.

Sounds like your core for the threading tool is may not be set correctly? I had some inserts chipping and an adjustment of a few thou on the core took care of it.

[jmichaud1]

I am using a G32 threading cylcle with a custom macro I wrote. I just don't know the best angle to come into the next segment to pick it up the thread correctly.

[cogsman1]

You need to enter at the trailing angle of the thread and pull out at the leading angle to be able to hide the blend points.

[chet470]

Threading in sections can be difficult to get used too. I actually do it on a regular basis and almost always feed in at a 45. If #7 equals thread pitch......G32U[#7*2]W#7 or G32U[#7+#7]W#7 if you prefer.

[chet470]

That would obviously be a 45 lead-out but I think you get the idea

[kwmkoester]

I believe the infeed angle argument in Citizen/Mits programming pertains to the way the threading tools' position(in relation to the center of the thread) within the thread during the roughing passes, your approach angle is established with your position before starting the thread. If you have Win-CNC, there is a little wizard that will help you establish a good foundation for turn-thread-turn-thread processes. If not, just make sure that you are positioning in Z at a factor of the thread on each subsequent thread, and always start at the same X value. If your pitch is .05 and you start your thread at -.05 in Z, then say you threaded to .500 in the first pass, make sure you start your second pass at .500-.05=.450 or .500-(2x.05)=.400. Always a factor of the thread pitch. Hope this is clear and that it helps.

[chet470]

Well obviously the start point of each subsequent thread section has to be in proper relation to the previous thread section and the difference between start points must be divisible by the thread pitch. I believe the question though was in regard to custom thread macros programming and what to program the infeed angle to and not how to "snyc" one thread section to another.

[kwmkoester]

Originally Posted by chet470 Well obviously the start point of each subsequent thread section has to be in proper relation to the previous thread section and the difference between start points must be divisible by the thread pitch. I believe the question though was in regard to custom thread macros programming and what to program the infeed angle to and not how to "snyc" one thread section to another.

Obvious? Without seeing his macro and only knowing that he is chipping the tip of his insert, I don't assume anything. In a diplomatic way, I was trying to make sure he wasn't missing a piece of the puzzle, you may, or not, be surprised how often, even good programmers, don't "get" how to segment threads properly, often chipping threading inserts. Also, people often, mistakenly, think that infeed angle means the angle at which the tool approaches the thread, when it is actually how tool roughs the thread(flank default, modified flank if argued). I probably could have been more clear but I was in a hurry and just wanted to get the info into the discussion. Best of luck.