Lathe - G32 - taper into straight thread

[my87csx481]

How can I use MastercamX3 to cut a tapered OD thread into a straight OD thread (1/4-18 NPT into .562 - 18, continuous)? I know I need to use G32 for this, and it posted out ok with just a tapered thread, and just a straight thread, but I need to combine the two toolpaths into one continuous thread.

 

Is there a way to select a chain for the minor diameter instead of just a point (on the thread toolpath thread shape parameters page)?

 

I know I don't offer any help on here but, it's not because I refuse. It's because I'm not exactly formally educated in much of anything.

 

Any help is very much appreciated. Thanks in advance.

 

Machine is a HAAS SL-20 (no C-Axis), X3, generic machine definition that I modified, generic Fanuc post updated from V9 and slightly customized.

[Philcott]

I don't know of a way to create a single cycle to achieve what you want. That doesn't mean it doesn't exist, just that I don't know how to do it.

[my87csx481]

It's quite tedious but, the job was run before in very small quantities by the guy I replaced.

 

Just the final pass was coded by hand with only a few blocks. To run the job, I had to back off the tool using the X wear offset and use the wear to take the depth of cut I wanted....adjust X....re-run....adjust x....re-run. I refuse to do this again for any lot size.

 

I'm trying to re-program it to make it a bit more efficient and easier.

 

I think my workaround is going to be: create two separate threading toolpaths, then merge the two paths by hand in the text editor of choice.

 

Almost as tedious, but hopefully I'll only have to do it once.

[Philcott]

quote:

---

I think my workaround is going to be: create two separate threading toolpaths, then merge the two paths by hand in the text editor of choice.

---

You will also have to syncronize the two paths by adjusting the "Z" approach so that the thread paths are continuous. Or use a different offset number to adjust diameter and starting "Z". Once done it should work every time.

 

Good luck with it.

[cncchuck]

program the taper then manualy input your z move at the end of it

 

ex.

G0 X.95 Z.1

G32 X1. Z-.75 F.062

Z-1.

G0X1.2

 

this is how i do it and it works fine.

[M_CODE1]

We do somthing like this except the threads are straight first, then it tapers

The first operation below works on an Okuma lathe. On our Fanuc controlled swiss lathes our PartMaker software will post it out long hand for each pass simalar to what CNCCHUCK has.

 

 

This is cutting a M16 thread with a taper at the end,

NAT6

( TOOL - 6 OFFSET - 6 )

( LFINISH GD THREADER )

G97 S850 M08

G00 X0.7915 Z0.15 T060606

G88 NAT40 H0.1037 D0.005 U0.001 B60 M23 M22 M73 M32

NAT40 G81

G00 X.5855

G34 X.5855 Z-.4921 F.0787

X.5915 Z-.4921-.3346

X.7915

G80

M09

G00 X37 Z7 T0600

M01

 

This is used on the Fanuc control.

Its cutting a M12 thread with taper in the back

 

N4(FRONT THREAD1ST)

G97S450M13

T1313(QUADTHREADER )

G99G0Z-0.1

X0.5783

X0.4651

G32Z0.1379F0.0689

X.4725Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4535

G32Z0.1379

X.4609Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4435

G32Z0.138

X.451Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4353

G32Z0.138

X.4427Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4287

G32Z0.1381

X.4361Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4229

G32Z0.1381

X.4304Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4173

G32Z0.1381

X.4247Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4118

G32Z0.1381

X.4192Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4063

G32Z0.1382

X.4137Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.4009

G32Z0.1382

X.4084Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.3957

G32Z0.1382

X.4031Z0.3543

X0.5868

G0X0.5783Z-0.1

X0.3957

G32Z0.1382

X.4031Z0.3543

X0.5868

G0X2.28T0

M1

 

 

Hope this helps

[my87csx481]

Thanks everyone for your help.

 

quote:

---

program the taper then

manualy input your z move at the end of it

 

ex.

G0 X.95 Z.1

G32 X1. Z-.75 F.062

Z-1.

G0X1.2

 

this is how i do it and it works fine.

---

That is exactly what I ended up doing.

 

In Mastercam, I actually created 3 tool paths, the taper thread, a 45 degree taper into the straight thread, and then the straight thread. I ended up using a 0.0 degree infeed angle to make it easier to add the 45 degree angle to the mix. (The material is brass, so tool pressure was not a major concern. The 45 degree feature is not on the print but, in order to make the threads to the accepted pitch diameters, and not violate any length dimensions on the print, it was necessary to blend the two threads in this manner.) Anyway, then, in a text editor, I manually added the 45 degree and straight move to the NPT toolpath.

 

For those that are curious: the part is a bulkhead fitting, used in some sort of control panel. Barbed nipple on one end, and the above thread configuration on the other end. I guess they're threading on whatever 1/4-18 NPT fitting, sticking it through the panel, and then using a 9/16-18 nut to lock it in place.

 

Maybe CNC Software can add chain selection functionality to the threading parameters for toolpath creation. Along with the ability to have different feed rates for each individual entity along the chain. I know it's asking a lot, but it's necessary when using G32.

 

Thanks again everyone.

[jhjr]

quote:

---

For those that are curious

---

thanks, you read my mind

 

also

 

quote:

---

McamX3 Lathe Level 1

XP, C2D E6400 @ 2.1, 1024 RAM

Barely enough to check email

It's hard coming from home (i7 920 @ 4200 and 6 gigs of ddr3 1600)

---

I hear you. I wish mastercam would up there minimum requirements. Cheap Employers suck!!! They'll spend the bucks on the software then make you run it on a turd.

[my87csx481]

You're welcome jhjr. I figured somebody probably read through this and asked themselves why a configuration like this would be needed.

It may be a space issue inside the panel. The barb end is pretty long. Also, I think this part was "designed" with the idea of cutting the threads by hand with a die....so, in the past, there was a natural blend from the chamfer on the die.

 

Thanks for the comment on my workstation....I laughed.

[Philcott]

I'll have to try that code and see if it works on our machines. Every day is a learning day.

[my87csx481]

Be careful though.

 

The Inch Per Revolution feedrate is along the G01 line....not along Z axis, unless it's a line parallel with Z....on the HAAS/Fanuc copy I'm using anyway.

 

Here's my re-trace finish pass:

 

G97 G99 S1000 M03

G0 X.7368 Z.25

X.4161

G32 X.468 Z-.5834 F.05559 (NPT thread)

X.4887 Z-.5937 F.07857 (blend at 45 degrees to 9/16-18)

Z-.6875 F.05556 (9/16-18 thread)

G0 X.7368 (retract)

Z.25

 

Also, I think running in single block will scrap the part. Don't know about overrides. Again, be careful.

 

Edit: not trying to brag or anything....I've been programming CNC lathes for 10 years, 8 with various versions of Mastercam....this is the first time I've used G32 to cut a thread....just for some point of reference.

[M_CODE1]

quote:

---

Also, I think running in single block will scrap the part. Don't know about overrides. Again, be careful.

---

All controls are diferent, but our Tsugmai Swiss Lathes will stop after the [G0 X.7368 (retract)] when in single block.

I guess to check just raise you X offset up about a half inch or so and try it.