[Blackknight]

Hi guys,

I am looking for information on how to manually program a multi start thread using G76 cycle and and angle index instead of the Pitch mode, everyone is familiar with. The reason for that is , I do not have enough room in the machine to use the second aproach. I will be cutting 6 square grooves on a 4.5in I/d. major dia. is 4-3/4in. the pitch is 6in.. The part's lenght is 10in. The machine is a Mori Seiki nl-2500 with C-axis.
Any help would be gratly appreciated.

Thank you.
xknight.

[txcncman]

To my knowledge, Fanuc does not have this option.

[ChrisW]

Try shifting coordinates without moving the tool just position on screen.
That should give you the room you need.

Shift in beginning of program and shift it back at the end

I used G50 Z

Be careful it is a nasty approach g code programming could crash if not done right.

[Waynno]

I have tricked my older yasnacs very easy on this,

simple as doubling the pitch, cut 12 pitch thread first thread .1666 Pitch

Back off start point .083

Cut second thread .1666

That will give you a 12 pitch double thread

Not sure if this trick works on newer models, But test on some aluminum stock
and fiddle with it, Once ya figgure it out, not too complicated at all

[Blackknight]

This is not a Fanuc Control, It is a propietary Mori Seiki control. It does fully support G- code. I has a very powerfull conversational part, Called MAPPs. It is posible to program multi start thread with an angular index in the conversational part of it. I just would like to know the sintax for doing it in G-code.

Thanks
xknight

[Blackknight]

The pitch aproached method is not an option since the part is too large or the machine too small. No room for doing so. Part=10.0 inches. boring bar 10.5 inches . turret ~6 inches = pitch method +5-inches, just not enough room. Moreover, The pitch of the grooves is 6-inches, even If I was able to do so, I would hate to have to machine so much air.

Thanks
xknight

[Waynno]

Sorry, Did not read into your original post, That is one crazy pitch

Maybe a second op on 4th axis? The control you describe is way above
my 25 year old controlled machines

[txcncman]

You only need 5" of additional clearance. You need to consult your machine manual for proprietary codes to accomplish this. I still do not think Fanuc does this. It will have to be a machine tool builder special add on if it is available.

If you have C axis capability, you might can index the start angle with a C axis shift. You might also have to revert to G92 or G33/G33 threading cycles.

[Blackknight]

I am afraid that I do not have those aditional 5-inches. However, even If I did I would hate having to cut that much air. I have seen it done in the past. Once in a very old Mori Seiki, over 15 years ago, and also in an Okuma cnc lathe .

Thanks
xknight

[fordav11]

you could use G54-G59. one for each of the starts and pre-set your workshifts to the correct amount then position the tool at an offset of the 12-pitch (1/12 * start number)
the positional change is done by the workshift and your tool position is also set in the Z. not entirely sure if it will work and you may need to adjust the Z start position to a multiple of the pitch to get it to work. test it on a scrap piece of material :-)
G54
G0 X Z-0.0833
G76 (etc)
G55
G0 X Z-0.1666
G76 (etc)
G56
G0 X Z-0.25
G76 (etc)
G57
(etc)

[txcncman]

I am afraid that I do not have those aditional 5-inches. However, even If I did I would hate having to cut that much air. I have seen it done in the past. Once in a very old Mori Seiki, over 15 years ago, and also in an Okuma cnc lathe .

Thanks
xknight

At 6" per revolution, do you know how much time it takes to "cut air" for 5"? Let's say you are running 10 RPM. That is 6 revolutions per second. Your machine will need to be able to feed 180 IPM to keep up. Each pass will take less than 4 seconds.

There is the option to reposition the part every 60 degrees in the chuck.

[fordav11]

I recall doing multi-start threads an easier way years ago.
After some research I found it. If your machine accepts the changes and the new G76 format it will work.

Set parameter 0001 bit 1 to 1 (FCV).

This sets it to Fanuc Series 15 format for fixed cycles so it will accept a one-line cycle for G76.

Now the interesting part (quoted from Series 15 manual)....

The threading start angle can be shifted by specifying address Q. This enables multi-start thread cutting to be easily performed. When Q is not specified Q0 is assumed. An integer from 0 to 360 (degrees) can be specified for Q.
Example:
G76X-Z-I-K-D-F-A-P-Q0;
G76X-Z-I-K-D-F-A-P-Q90000;
The threading start angle is shifted 90 degrees from the angle specified by Q0 at the spindle.


So to do 6 starts you would program it like this....

G76 X Z I K D F A P Q0
G76 X Z I K D F A P Q60000
G76 X Z I K D F A P Q120000
G76 X Z I K D F A P Q180000
G76 X Z I K D F A P Q240000
G76 X Z I K D F A P Q300000

[Blackknight]

Thanks you very much , that's what I was looking for. I knew about the Q, But not how to implement it. I will try it at the control and experiment with it.

Thanks again.
xknight

[Buckshott00]

@Blackknight

The controller is a Mits MSX850III fordav11 is right that should give you what you want, It's page 312 of the programming manual, just be careful how you enter the Q value especially if you change a parameter to run in the F15 format. Otherwise Q will specify the depth of cut for the first path.

[Blackknight]

Thanks I'll keep that in mind.

[Blackknight]

At 6" per revolution, do you know how much time it takes to "cut air" for 5"? Let's say you are running 10 RPM. That is 6 revolutions per second. Your machine will need to be able to feed 180 IPM to keep up. Each pass will take less than 4 seconds.

There is the option to reposition the part every 60 degrees in the chuck.

10 RPM = 10 revolution per minute, not 6 revolutions per second.
at that speed and it would take 4.8 seconds of cutting air.
if we remove .005 per pass, it would take 25 passes to cut one groove.
25 passes times 4.8 seconds times 6 grooves equals 12 minutes of cutting air.

Repositioning the part is out of question due to acuracy issues.

[txcncman]

10 RPM = 10 revolution per minute, not 6 revolutions per second.
at that speed and it would take 4.8 seconds of cutting air.
if we remove .005 per pass, it would take 25 passes to cut one groove.
25 passes times 4.8 seconds times 6 grooves equals 12 minutes of cutting air.

Repositioning the part is out of question due to acuracy issues.

Bah ha ha ha ha ha! Yeah. You caught my typo/bad math. You win! And I bet you still have not completed your part either after 7 days. Lets see, which is longer? 12 minutes or 7 days? The cutting air time is nothing compared to the talk time. Bah ha ha ha ha ha!

[fordav11]

so did the G76 multi-start method I mentioned above work on your machine?

[Blackknight]

To fordav11

Yes we have done those parts numerous times in and old Daewoo Machine using the pitch method. I was asked about an easier way to make them. Since we have the Mori machine I figured I'd ask in this forum. We will definitly try your suggestion next time we make them. I no longer deal with turning centers , I am 100% milling guy now. I was just helping a coworker.


Thank you very much for your help
xknight