g76 threading

[wwenter]

Hello
I am run Oak with Dyn4 servos. When cutting threads G76 it doe's not retract all the way out at the end of thread and leaves a groove before it retracts and returns to the start point for next cut. I have play with spindle speed slow or fast makes no difference and used different chamfer amounts from 3 to .025 and still leave that groove at end of thread other than that it threads great up to 1000 rpm have not try to go faster yet. Are there some parameters I need to change.
Thanks for any help

[DannyB]

Hello
I am run Oak with Dyn4 servos. When cutting threads G76 it doe's not retract all the way out at the end of thread and leaves a groove before it retracts and returns to the start point for next cut. I have play with spindle speed slow or fast makes no difference and used different chamfer amounts from 3 to .025 and still leave that groove at end of thread other than that it threads great up to 1000 rpm have not try to go faster yet. Are there some parameters I need to change.
Thanks for any help

Hey,
it's really hard to help here without a proper report attached, which has info on how your setup is configured, etc.

See viewtopic.php?f=20&t=383 and viewtopic.php?f=60&t=943

[cnc_smith]

Besides the report please send the Intercon program if you used that to create the program or if third party send the g-code program.

[tblough]

The chamfer amount controls how many turns the spindle makes at the ending Z position to withdraw the tool. If it is set to 1, the spindle will make one full turn while withdrawing the tool to the major diameter leaving a single turn helix starting at the minor diameter wrapping around 360 degrees to end at the major diameter. The amount the tool backs away past the major diameter is controlled by the F9 SETUP Clearance amount.

If you set the chamfer amount to 0, the tool will retract from the part at the machine rapid speed. This will generate the shortest "groove" possible. If the groove length is still to long for your liking then you will need to do something to increase the rapid speed of your X axis, or decrease the spindle speed.

[wwenter]

Here is a report and the Intercon thread program I used. I can cut nice threads just a the end of the thread it seems to stop before it retracts out of thread and leaves a grove at the end kind a like a relief cut.

[cncsnw]

Try increasing Machine Parameter 242 to 60 degrees.

[cnc_smith]

A note: you sent the g-code program not the Intercon program for "Threading Test". The Intercon file is found in the "icn_lath" directory.

For the chamfer it pulls out at a 45 degree angle so for a value of 1 it will be way high above the material. I have found a discrepancy in the manual. Page 178 of the manual for the G76 has the correct calculation for the chamfer. This number should be less then 1. and closer to .5 or less For the chanfer calculation it is 1/10 of the thread lead (pitch).

For parameters 240-242 there are recommendations for setting on Page 239 of the manual. Parameter 240 I have found works best with this value set to 1/2 to 2 times the pitch. With will be a value less then .100. With higher spindle speeds this value will need to be increased if banging is heard or lost of position. You do not have to change this parameter every time you change the pitch. If you change your RPM to a lot higher value then you may have to change parameter 240.

[wwenter]

Thanks cncsnw
parameter 242 bumped it up to 60. Cuts threads at 1100 rpm with no grove at the end.

[frijoli]

Thanks cncsnw
parameter 242 bumped it up to 60. Cuts threads at 1100 rpm with no grove at the end.

Outstanding! Thanks for the update. And as always thanks everyone for explaining this!