Please help me reverse my threading tool path!

[TheFunk]

I am currently in the process of learning G-code and have ran into a snag with a program. Basically my employer wants me to use a program that the old machinist (No longer here and not on good terms) wrote to produce some parts. After figuring out his setup i hit a snag. The threading cycle starts by the chuck and drags backwards, producing left handed threads. Is there a way to correct this without rewriting from scratch And could you please explain the why of it (if this isnt asking too much)

Thanks again ( section of code below)

(OD THREAD CYCLE)
( SAFETY LINE BELOW )
G00 G54 G18 G40 G80 G97 G99 M31
(TOOL = 3 / OFFSET = 3)
(WORK OFFSET = 54)
(SPINDLE RPM = 1157)
(THREADS PER INCH = 24.)
(THREAD MAJOR DIAMETER = .375)
(THREAD MINOR DIAMETER = 0.33)
(THREAD HEIGHT PER SIDE = 0.026042)
(OPTIMIZED "A" VALUE FOR 60 DEGREE THREADS)
(SEE SETTINGS 95, 96, 99 AND 289 ON THE CONTROL)
T303
G54
G97 S1157 M03
G00 Y0.
G00 Z0.125
G00 X0.775
M08
(**WATCH FOR LIVE CENTER INTERFERENCE**)
(RECOMMENDED Z-AXIS START IS 3 THREADS FROM START POINT)
G00 X0.775 Z-0.163 M24
G76 X0.33 Z0.125 K0.026 D0.0065 F0.0417 A59
G00 Z0.125
M09
G00 G53 X0.
G00 G53 Z0.
G00 Y0.
M05
( END OD THREAD CYCLE )
M01

 

[angelw]

I am currently in the process of learning G-code and have ran into a snag with a program. Basically my employer wants me to use a program that the old machinist (No longer here and not on good terms) wrote to produce some parts. After figuring out his setup i hit a snag. The threading cycle starts by the chuck and drags backwards, producing left handed threads. Is there a way to correct this without rewriting from scratch And could you please explain the why of it (if this isnt asking too much)

Thanks again ( section of code below)

(OD THREAD CYCLE)
( SAFETY LINE BELOW )
G00 G54 G18 G40 G80 G97 G99 M31
(TOOL = 3 / OFFSET = 3)
(WORK OFFSET = 54)
(SPINDLE RPM = 1157)
(THREADS PER INCH = 24.)
(THREAD MAJOR DIAMETER = .375)
(THREAD MINOR DIAMETER = 0.33)
(THREAD HEIGHT PER SIDE = 0.026042)
(OPTIMIZED "A" VALUE FOR 60 DEGREE THREADS)
(SEE SETTINGS 95, 96, 99 AND 289 ON THE CONTROL)
T303
G54
G97 S1157 M03
G00 Y0.
G00 Z0.125
G00 X0.775
M08
(**WATCH FOR LIVE CENTER INTERFERENCE**)
(RECOMMENDED Z-AXIS START IS 3 THREADS FROM START POINT)
G00 X0.775 Z-0.163 M24
G76 X0.33 Z0.125 K0.026 D0.0065 F0.0417 A59
G00 Z0.125
M09
G00 G53 X0.
G00 G53 Z0.
G00 Y0.
M05
( END OD THREAD CYCLE )
M01

Hello TheFunk
Programs don't just change themselves and this program will clearly cut a LH Thread. Is it for sure that its supposed to be a RH Thread?

To make the program cut a RH Thread, change the Z coordinates of the Blocks shown in Red above, to the following. Reason? It simply changes the Start and End Z points of the Thread.

G00 X0.775 Z0.125 M24
G76 X0.33 Z-0.163 K0.026 D0.0065 F0.0417 A59

Not that it will cause any issue for you, but clearly math wasn't the previous guy's strong point.

(THREAD MAJOR DIAMETER = .375)
(THREAD MINOR DIAMETER = 0.33)
(THREAD HEIGHT PER SIDE = 0.026042)

Thread Height = (0.375 - 0.33) / 2
= 0.0225

or

Thread Minor Diameter = 0.375 - 0.026042 x 2
= 0.322916

Regards,

Bill

 

[FredC]

Without trying to look at the program (the format is different than my machine would use) Did you get good looking left hand threads? If so, reverse the spindle direction and flip and reset the tool? Not knowing the machine and if this is possible but this is the first thing that came to my mind.

 

[TheFunk]

Thank you Angelw for the swift response. Thank you for the explanation. I will be changing this up and running a sim, and with any luck get some correct parts. I am positive they need to be right handed threads, as the blueprint doesn't say otherwise. Once again thank you so much!

@FredC That was actually the first thing i tried. Issue is there was no way for me to turn our CenterPoint around and be on center. Also it was just a piece of the program as for the format im not sure. Im running a Haas ST25Y

 

[angelw]

(OD THREAD CYCLE)
( SAFETY LINE BELOW )
G00 G54 G18 G40 G80 G97 G99 M31
(TOOL = 3 / OFFSET = 3)
(WORK OFFSET = 54)
(SPINDLE RPM = 1157)
(THREADS PER INCH = 24.)
(THREAD MAJOR DIAMETER = .375)
(THREAD MINOR DIAMETER = 0.33)
(THREAD HEIGHT PER SIDE = 0.026042)
(OPTIMIZED "A" VALUE FOR 60 DEGREE THREADS)
(SEE SETTINGS 95, 96, 99 AND 289 ON THE CONTROL)
T303
G54
G97 S1157 M03
G00 Y0.
G00 Z0.125
G00 X0.775
M08
(**WATCH FOR LIVE CENTER INTERFERENCE**)
(RECOMMENDED Z-AXIS START IS 3 THREADS FROM START POINT)
G00 X0.775 Z-0.163 M24
G76 X0.33 Z0.125 K0.026 D0.0065 F0.0417 A59
G00 Z0.125
M09
G00 G53 X0.
G00 G53 Z0.
G00 Y0.
M05
( END OD THREAD CYCLE )
M01

Hello TheFunk,
Irrespective of the configuration of your machine, Spindle in M03 Mode and Threading from Left to Right (away from the chuck) will always result in a LH Thread. As mentioned in my first reply, programs just don't change themselves, so either this program was always for cutting a LH Thread, or the program has been changed since the last time it was successfully used to cut a RH Thread.

Either, as suggested by FredC, the tool is used inverted to how you now have it and run the spindle in M04, or the Z coordinates have to be changed as per my first Post. In either case, a program change has to be made and the program in it's current form didn't get that way by itself.

Reference is made in comments in the program to "WATCH FOR LIVE CENTER INTERFERENCE". Using a RH Tool inverted to what you have now and running the program in M04 Mode, will give you much greater clearance with the Tail Stock Centre, but if the Thread ends close to the chuck, you may get interference there with the back of the tool. In my opinion, the previous guy was probably referring to interference with the back of the tool with the Tail Stock Centre, which is a usual issue with most Threading Tools when cutting small diameter Threads.

Regards,

Bill

 

[TheFunk]

Not sure if my last reply went through. i did change the spindle rotation to m03 as that is the only way i could get the single point to line up with center, otherwise turning it around would have crashed it onto the part. As i am unsure of his exact setup, I am left guessing and trying to figure it out. On that note that fix did work. Thanks a million!

I wish i could share the rest of the code as there are some questions about some of the code, however it is not mine to share out to the web.

 

[metalmadness]

I just did a LH thread on the lathe using M04 threading right to left. The key here being the insert is flipped upside down. An ID threading bar running upside down makes in a LH OD threading bar. Then run reverse spindle and thread normally.

It sounds like you want a RH thread? To do that you need to run M03 and your should be running positive Z to negative Z (right to left).

If I were you, learning Gcode...I would throw this entire part program out in the garbage. Start a new program from scratch (use this program for reference if needed) and create your own program. There are many ways to write a program and this is just one way. If you just go in and modify a few codes or values, you won't really be learning as much as if you write a whole program.

Good luck, I confess I am not a lathe master. Mill FTW

 

[angelw]

Not sure if my last reply went through. i did change the spindle rotation to m03 as that is the only way i could get the single point to line up with center, otherwise turning it around would have crashed it onto the part. As i am unsure of his exact setup, I am left guessing and trying to figure it out. On that note that fix did work. Thanks a million!

I wish i could share the rest of the code as there are some questions about some of the code, however it is not mine to share out to the web.

Hello TheFunk,
If the program originally ran in M04 Mode and it was to cut a RH Thread, then the setup would be as suggested by FredC. A RH Threading Tool Holder would be set in the turret with the cutting insert uppermost. Most machines will accommodate OD Tools being held in the turret either way up and have the facility to locate the cutting insert on centre line. It would help if you were to Post a picture of the turret set up for further advice.

As mentioned in my earlier Post, using a RH Threading Tool inverted to what you have now and running the spindle in M04 Mode will give you a lot more clearance between the cutting tool and the Tail Stock Centre, but you would have to be careful that you have clearance between the back of the tool holder and the chuck.

Given the Start and End Z Coordinates in your program, ie. cutting from Z-0.163 to Z0.125, and the fact that you changed the spindle rotation direction form M04, its extremely probable that the previous programmer/operator, designed the program to run that way, with a RH Tool with the cutting insert uppermost. Probably to give more clearance with the tail stock centre.

Regards,

Bill