hi all i am cutting a 4tpi acme thread using sandviks inserts.
The thread runs for about 8" long and i am getting major problems with cuttings wrapping around the part and inserts breaking.

It is being done on a puma250 700L controller as far as i can see using the g76 line there in no way of doing a modified infeed so it cuts either side of the thread. Does any one have any suggestions to this as i have loads more to do and am eating chims and inserts like there going out of fashion.

Thanks

I have tried the messing with surface speed but this seems to do nothing. and depths of cut but again nothing seems to be doing anything.

You can do this by cycling through threading cycles that have different Z start positions. The first cycle might only take one cut then the next two have the Z moved very slightly positive then negative and take a couple of cuts then back to a centered cut, etc, etc. You will probably still get long chips but they are not as thick and strong. Tedious to program but it can work.

Another option is to go through a threading cycle with a 60 degree threading tool down to the acme depth then come in with the acme tool to take out the flanks. Again it is possible to offset the Z to take out each side separately.

looking at the second method there but cycle time is an issue so this would have a bad affect on it.

I am going to try and change the infeed angle on the first G76 line it is set to 29deg so the back of the thread would be rubbing all the time.
If i change this to 32 then the front would be cutting and not the back just not sure on the Puma on the fanucs we have this is okay as the last two finishing passes are plunged so it brings back to the correct angle, again not sure if the pumas do this.

I do not believe the G76 cycle is ideal for Acme thread forms. I like Geof's suggestion, which would involve writing the cycle out longhand using G32 or G33, whichever is suitable for your controller.

Its best that carbide not drag along the surface. Make both sides cut, or have only one cut, but dragging the insert will damage it. IMO.

....I have tried the messing with surface speed but this seems to do nothing. and depths of cut but again nothing seems to be doing anything.

You mention cycle time issues.

Depending on how rigid your machine is, the motor size and how much nerve you have, you might try being really aggresive on speed and feed. Sometimes it is possible to force the chip to curl nicely just by brute force. Of course when something does go sideways you not only wipe out the insert but the holder probably goes too.

thanks all i have just written the program using G32. I was just trying to make it easy for the operator and use G76.

Not sure on brute force to chip the swarf pushed it quite hard and you get a long blue string that is no where near curling or chipping.

Just got to go type the two pages of G32 now :O(

thanks all i have just written the program using G32. I was just trying to make it easy for the operator and use G76.

Not sure on brute force to chip the swarf pushed it quite hard and you get a long blue string that is no where near curling or chipping.

Just got to go type the two pages of G32 now :O(

If you are using a standar grove tool holder.
Try setting the tool holder to the hilex angle of the tread. You will have to modifie the holder forthis and then use a shim to keep it at the centerline. When we first tarted roughing threads either Ball threads or Acmes we would have the same problem. When you set the cutter to the corect hilex it will break the chip. You will also get a better thread finish.


Bluesman

not sure if i get what your saying there. I am using a standard screw cutting tool not toplock style one a lie down insert style.
are you saying rotate the angle of the tool holder so it sits at a angle ie mill a flat along the bottom to get the a helix angle of 0.6513. Long time since i messed with helix angles think it was about 15 years ago when i used a matrix chaser for screw cutting.

The G32 method works for giving a better thread but the swarf is still a major major concern

not sure if i get what your saying there. I am using a standard screw cutting tool not toplock style one a lie down insert style.
are you saying rotate the angle of the tool holder so it sits at a angle ie mill a flat along the bottom to get the a helix angle of 0.6513. Long time since i messed with helix angles think it was about 15 years ago when i used a matrix chaser for screw cutting.

The G32 method works for giving a better thread but the swarf is still a major major concern

You need to match the helix of the thread at the dia and lead of the part. exsample a 2in dia screw with a .250 lead has a helix of 7deg and a 4in dia screw with the same .250 lead has 4deg helix. What is breaking the insert is that the deeper you cut you are starting to cut more with the side of the insert ande not the top cutting edge. When you set the tool to the helix you get a nice even cut to full depth.

Bluesman

I dont really get what your saying still sorry.
I understand the helix angle of a 3 acme on a 7" dia is 0.6513. What im having trouble understanding is what you want done with the tool.
1 mill the bottom of the tool so it drops 0.6513 deg but then the bottom of the insert on the back stide would rub.
2 tap the tool out the toolpost 0.6513 deg this would change the thread angle.

I think what Bluesman is getting at is that the material is not passing the tool in a direction perpendicular to the top face of the tool. I haven't looked at his .doc attachment because I can't open it. There is a sideways component to the motion due to the tool advancing along the work. This means that the chip does not come out parallel to the centerline of the tool it tends toward the side and runs into the thread flank on the trailing side. Leaning the tool into the thread at the helix angle means the chip comes out centered and the cut is more symmetric.

Several of the laydown type thread tools have carbide shims available with various angles ground in, to tilt the insert to the proper angle for the pitch of thread being cut. Might be worth consulting the tool catalogue. Page C75 in my Sandvik Turning tools and inserts, catalogue is LIT-CAT 00T that I am looking in (older book year 2000).

I think what Bluesman is getting at is that the material is not passing the tool in a direction perpendicular to the top face of the tool. I haven't looked at his .doc attachment because I can't open it. There is a sideways component to the motion due to the tool advancing along the work. This means that the chip does not come out parallel to the centerline of the tool it tends toward the side and runs into the thread flank on the trailing side. Leaning the tool into the thread at the helix angle means the chip comes out centered and the cut is more symmetric.

Thank you Geof for exsplaining better that is excactly what I am talking abiut, And yes Hu Flung is right also some manufactures of lay down inserts make the shimes all ready.
But Geof has done what I and my lack of vocabular talents could not. The tool must match the helix of the thread it can not run perpendicular to the workpiece.
I spent ten years at Tompson Saginaw making Ball Screws and some Acme also and while we use very few laydown stile for roughing these threads. What we would do is take a 1.5 in holder lay it on a sign plate mill the helix into it then flip it over and mill it paralel to the bottom side. So when you mounted it in the lathe the the tool matched the helix on the thread grove. It works exstreamly well.
Thanks guys for helping me exsplain it so well

Bluesman

Several of the laydown type thread tools have carbide shims available with various angles ground in, to tilt the insert to the proper angle for the pitch of thread being cut. Might be worth consulting the tool catalogue. Page C75 in my Sandvik Turning tools and inserts, catalogue is LIT-CAT 00T that I am looking in (older book year 2000).

I am going to scrutinise my Iscar catalogue with an intense scrute (the old english guys will get that allusion). I have not noticed mention of these angled shims but I could use them. Thank yu Hu

right i get it thanks for the information on that, now i understand what you are saying the insert is at the correct angle i have used the shim supplied for cutting a 4 acme. I think its just down to material is to soft so no matter how hard i hit it or soft it just comes of in a string.
Im hopping when the new machine comes which is a lot lot bigger there will be room for the swarf to flow away.
We have also noticed that the insert does not sit in the tool correct and it rocks on slightly but still does rock from left to right, which i am sure is not helping the situation.