Lathe thread

[AMCNitro]

How do I program a thread end like in the pic? I've never had to do it before. I'm on X8

[crazy^millman]

Like any other thread. You can pick from the chart. Funny you put this up. I am about to post a topic about how tools are defined in Mastercam for lathe threading.

[AMCNitro]

The problem I'm having is with the end if the thread, I'm not sure how to explain. I'll post another pic later.

Thanks.

[crazy^millman]

It is called a gradual lead out. You want the thread to transition out at the end of the cut verses dwell in place at the end. To do this Mastercam you make a over cut and/or Anticipated pulloff setting to 1 rev. Some machines have a specific thread cycle that will do this also. Would need to reference the book to see which one is the bets one for your machine.

[SlaveCam]

If it's a Fanuc control (16i-T or newer), use continuous threading (G32). You can chain G32 commands, first line for the cylinderical part and the second line for the lead-out taper.

Dunno how to do it on Mastercam, likely need a custom post.

[Orvie]

You can also use the MPLMASTER_THREADC post.

You can create geometry for the exact lead out that you are looking for.

[Newbeeee™]

You just select a tab on Siemens Shopturn...

[AMCNitro]

Its a Haas SL10(doesnt matter where I work, can seem to get away from Haas lol).  Ron gave the answer I needed.  Ill go try it on monday.

Thanks everyone.

[Mike@Lustre]

On the HAAS TL series you can use a M code to change the end of the thread from  angle out to  no angle out for threading into a run out undercut at the end of the thread .

 

M23 command angles the thread out at the end , and M24 command will not angle it out . 

[AMCNitro]

I tried it today and it didnt do anything, it was still dewling...

Perhaps  its not on the post?

[AMCNitro]

On the HAAS TL series you can use a M code to change the end of the thread from  angle out to  no angle out for threading into a run out undercut at the end of the thread .

 

M23 command angles the thread out at the end , and M24 command will not angle it out . 

What would the program look like?  I work in mold shop and Im the only CNC lathe guy, Im going to need to be doing threads like that a lot, so I need to figure it out.

[Mick]

It is called a gradual lead out. You want the thread to transition out at the end of the cut verses dwell in place at the end. To do this Mastercam you make a over cut and/or Anticipated pulloff setting to 1 rev. Some machines have a specific thread cycle that will do this also. Would need to reference the book to see which one is the bets one for your machine.

 

Mastercam Lathe Threading. Quick and Simple. I always liked how in a few mouse clicks, you can have a threading toolpath generated on the screen, and typically without requiring any geometry.

[crazy^millman]

What would the program look like?  I work in mold shop and Im the only CNC lathe guy, Im going to need to be doing threads like that a lot, so I need to figure it out.

 

I would get on the phone to HAAS Applications tomorrow and see why you are getting this issue. Short of drawing the thread shape like the others have mentioned it should be pretty straight forward.

[civiceg]

Haas threading retract

 

 

M23 commands the control to execute a chamfer at the end of a thread executed by G76 orG92. M24 commands the control not to perform chamfering at the end of the threading cycles (G76 or G92). An M23 remains in effect until changed by M24, likewise for M24. Refer to Settings 95 and 96 to control the chamfer size and angle. M23 is the default at power-up and when the control is reset.

 

95 - Thread Chamfer Size

This setting is used in G76 and G92 threading cycles when an M23 is commanded. When command M23 is active, threading strokes end with an angled retraction, as opposed to pulling straight out. The value in Setting 95 is equal to the number of turns (chamfered threads) desired.

Note: Settings 95 and 96 interact with each other. Valid range: 0 to 29.999 (Multiple of current thread lead, F or E).

Setting 95 - Thread Chamfer Size, G76 or G92 threading stroke with M23 active: [1] Setting 96 = 45, [2] Setting 95 x Lead, [3] Tool path, [4] Programmed thread endpoint, [5] Actual stroke endpoint, [6] Lead.

 

96 - Thread Chamfer Angle

See Setting 95. Valid range: 0 to 89 degrees (No decimal point allowed)

[mmack]

What would the program look like?  I work in mold shop and Im the only CNC lathe guy, Im going to need to be doing threads like that a lot, so I need to figure it out.

Logged in from home ,

 

it,s a G76 cycle with the M23/M24 in the line above

 

, you may need the parameter turned on

 

setting 95/96  are for the Thread chamfer size , and Thread chamfer angle

 

does your machine have the intuitive package ?

 

 

also you mentioned you will be doing a lot of threads , if it's a course pitch look into thread clipping as well ,

 

I have never used it but my partner at work has used it . it is a tool path that removes the rag edge on the 1st few threads

 

, basically from what I gather you use a grooving tool and crest the tops of the 1st few threads on a taper and it deburrs the thread and provides a nice lead in

[Mike-T]

  Higbee thread.