We have a part that we are making on our CNC lathe (Feeler FTC-200L with a Fanuc Oi-TD controller) that has a 7/16-14 UNC threaded section on one end. I am using the G76 command to cut the threads, but I am getting a burr on the lead in. I tried to increase the size of the chamfer on the part before I thread, but the thread tool pushes material out so the nut won't go one. Is there a way to chamfer with the thread tool in the G76 step to get more of a tapered lead in?
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Chamfering the start of threads on a lathe part
- Thread starter Bigdawg07
- Start date
- Replies 15
- Views 9,156
Booze Daily
Titanium
- Joined
- Sep 18, 2015
- Location
- Ohio
It's just the nature of threading. Some materials are worse than others.
I usually just re-turn the chamfer and re-thread, setting your G76 so it only takes one pass.
On some materials you'll get a better result re-turning the chamfer backwards toward Z0.
Same thing when getting burrs in an undercut at the end of a thread.
I usually just re-turn the chamfer and re-thread, setting your G76 so it only takes one pass.
On some materials you'll get a better result re-turning the chamfer backwards toward Z0.
Same thing when getting burrs in an undercut at the end of a thread.
We had a lathe guy that would blunt start a thread with a grooving tool. He set it up so it would feed in at the pitch and retract after a full thread had formed. I guess the retract would generate a radius. I'm not sure exactly how it did it but it was something along those lines. Maybe somebody else here can shed some light on that.
alphonso
Titanium
- Joined
- Feb 15, 2006
- Location
- Republic of Texas
G
guest
Guest
...Add a spring pass or two, use a full profile insert.
There are two solutions to the "thread start burr" used at my shop:
1) Rerun the finish turning tool, after the threading, then a spring pass with the threading tool.
or
2) Program a 45° (1:1) chamfer from just beneath the minor to the PD, then change to a 30° 'ish (2:1) from the PD to the major.
Option 2 is used mostly, unless the print forbids altering the thread start.
Doug.
1) Rerun the finish turning tool, after the threading, then a spring pass with the threading tool.
or
2) Program a 45° (1:1) chamfer from just beneath the minor to the PD, then change to a 30° 'ish (2:1) from the PD to the major.
Option 2 is used mostly, unless the print forbids altering the thread start.
Doug.
I have read that there is a M23/M24 to turn automatic chamfering on and off on the Funac controls. I'm assuming this is set in the control somewhere as when I put an M23 in my code the machine just stops. I have not been able to find it yet though.
Booze Daily
Titanium
- Joined
- Sep 18, 2015
- Location
- Ohio
The chamfer on/off applies to how the threading tool exits the thread. Chamfer on is used when there is no undercut. The threading tool keeps advancing in Z as the X pulls out. (usually within one pitch)
Chamfer off is used when treading into an under cut. Z stops then X pulls out.
Chamfer off is used when treading into an under cut. Z stops then X pulls out.
Bingo!
Set your depth above (or at) the thread height, on the spring pass.
Everything else should be the same.
Doug.
If I am using a full profile insert most of the time all I do is recut the chamfer but instead of a turning op I face it instead and that helps to roll the burr away from the thread instead of into it. That usually cuts it clean enough I wont have to rerun a threading pass after.
hy bigdawg, just like doug said, try using a combo of c45 + c30 or c40 + c_whatever, so to smooth out the start of the thread
a critical aspect is controlling the infeed pattern + the thread cutting mode; try to avoid negative infeed angles, especially on the last passes, so to reduce the tendency to burr the start
lower cutting specs ( + more coolant ) should reduce the deformation tendency of soft materials
a critical aspect is controlling the infeed pattern + the thread cutting mode; try to avoid negative infeed angles, especially on the last passes, so to reduce the tendency to burr the start
lower cutting specs ( + more coolant ) should reduce the deformation tendency of soft materials
Mydrrin
Hot Rolled
- Joined
- Jan 22, 2012
- Location
- Canada, Edmonton
What I typically do is thread chamfer bad starts, usually required for acme threads.
So you do your normal thread lets say 0.100 out from the part.
Z0.1
G76P010000
G76X0.500Z-1.0P450Q90F0.0625
Then come in with a grooving tool, look up how much it is from the edge to the centre of the threading part of the insert. Seco has it in their book under each of the UN threading inserts, either 0.059 or 0.031 for smaller threads. Plan for the grooving insert will follow in at the bottom of the threading insert.
Z0.131
G76P010500
G76X0.500Z-0.080P450Q90F0.0625
The second number of the P (05) is the chamfer at the end so it raises up over half a thread, you can adjust this if you want a little less or more blunt kind of start. You start it at something like 0.08" deep where it finishes the angled threading and adjust either deeper depending on if it's chamfering the thread or want it less or more.
That's how I do it. There is no wrong way as long as it gets done.
So you do your normal thread lets say 0.100 out from the part.
Z0.1
G76P010000
G76X0.500Z-1.0P450Q90F0.0625
Then come in with a grooving tool, look up how much it is from the edge to the centre of the threading part of the insert. Seco has it in their book under each of the UN threading inserts, either 0.059 or 0.031 for smaller threads. Plan for the grooving insert will follow in at the bottom of the threading insert.
Z0.131
G76P010500
G76X0.500Z-0.080P450Q90F0.0625
The second number of the P (05) is the chamfer at the end so it raises up over half a thread, you can adjust this if you want a little less or more blunt kind of start. You start it at something like 0.08" deep where it finishes the angled threading and adjust either deeper depending on if it's chamfering the thread or want it less or more.
That's how I do it. There is no wrong way as long as it gets done.
I've been threading on stainless and the burr's are a constant , I've generally done the chamfer a little deeper than thread debth , turn the thread , then either rechamfer with the turn tool or do a second G76 only offset .0005" in Z+ . I also use A57,A58 ect.. to minimize the burr if possible .
.
.
I finally finished working on this part and got it working. I did the 2 part chamfer that Doug suggested and added a second finish pass after the threading. Worked out good. Thanks for all the help!
