Daewoo Puma lathe and Fanuc 18T thread start orientation

------- What kind of holding fixture are you using? Does this index the part in the chuck to the same radial position every time? If not, can you add a pin or something to do so?

Unka' George [George McDuffee]

------------------------------------------- He that will not apply new remedies, must expect new evils: for Time is the greatest innovator: and if Time, of course, alter things to the worse, and wisdom and counsel shall not alter them to the better, what shall be the end?

Francis Bacon (1561-1626), English philosopher, essayist, statesman. Essays, "Of Innovations" (1597-1625).

The part is run out of bar stock and is complete after cut off. I guess I should have mentioned that.

Does the machine naturally always start the thread cycle from the same angle, given the same program? I didn't want to assume that the machine would exhibit this type of behavour, but I suppose it makes sense to some degree.

Regards,

Robin

Is the thread and all of these related drilled features being machined on the lathe in one chucking?

What is the tolerance and how are you inspecting it?

==================

Assuming all features are being machined in one chucking and not knowing your machine and controller I suggest;

1) Thread milling is the easiest and most precise method to control a thread start, IMO.

2) (G76/G92 thread cycle) If thread start position is not too tight run a sacrificial setup part and adjust thread tool start position Z accordingly.

3) (G76/G92) If start position is not too tight you might run a sacrificial setup part and rotate the positions for the drilled features accordingly.

+++++++

If the related features are machined in a different machine or a different setup then you need a fixture/Stop/Pin to orientate your part.

-- Tom

Yes. The part starts as bar stock and is cut off as a complete part in one setup.

I should have mentioned that. Approx. +/-5=BA (pretty loose, given the process). Inspection happens during assembly. Misalignment is obvious during assembly as some holes on a mating part have to (roughly) match.

That's not a bad suggestion at all actually, and it hadn't occured to me at all. The thread is 1.0mm pitch and only about four or five threads long (about 1.3" diameter - I know inch AND metric thread dimensions!). Maybe faster to threadmill than to take multiple passes with a single point tool.

I do have some clearance to change the Z position of the start. Would a Fanuc 18T always start the thread in the same angular location given the same program? I wasn't sure if the control did this, or just started the first feed "whenever".

I'd likely just change the C offset using G50 or something as I don't want to reprogram all the drilled angles. This again begs the question as to whether the machine will always start the thread at the same position.

Thanks for your help Tom. Great suggestions.

Regards,

Robin

Sounds like your solution as long as it's within your work envelope.

All I can say is it has worked for me where thread milling was not an available option. If it is the same program, same machine it should repeat. If it is the same program, different machine then Z start may need adjustment on setup part but all subsequent parts should repeat.

I suggest you run a couple test parts on scrap or inexpensive material to verify it works on your machine.

You can thread a part using G76 then run a deburring routine to break the thread burrs using another tool and return with same threading tool using G92 as a single spring pass to make sure you didn't push the burr back into the thread. As long as the Z start is exactly the same in both threading cycles the tool will pick up the same lead so it is not random ("whenever").

It should but verify by testing it out on scrap or inexpensive material.

Good luck, Tom

"Robin S." wrote in news:bbdc35b8-7723-453d- snipped-for-privacy@q11g2000yqi.googlegroups.com:

Too bad it's not a 31i control. With it you can specify an angular relation to the start of the thread.

But you can hold the angular relationship in any case. The zero pulse marker for threading is the same zero for the C-axis plus or minus any grid shift value set in a parameter.

The easiest way to do this is to adjust you Z-axis start point for the thread. You didn't say what the thread lead is, but lets take a 16 pitch thread as an example. 1/16=.0625 So every 0.0625 movement in Z=360 degrees rotation on the spindle. So every 0.00017" is equal to one degree on the spindle.

The easiest way to adjust your start point in Z without editing the program is to use a macro variable. Just add it to the Z-value on your positioning move.

G00 Z[0.125+#513];

Or something like that.

As far as getting the first part to come out right, that would be difficult using this method. If possible cut a test part, measure and adjust the variable.

In a situation where you have an expensive part that needs to be right the first time, I would cut the thread first, then engage the C-axis and shift it using a coordinate setting command. If possible have a screw on gage made up beforehand that can be indicated after the thread is cut. Indicate it to zero then set the C-axis coordinate to zero or the appropriate dimension to be in relation to your milling.

You could also thread mill if you have a live holder available and the part lends itself to being thread milled.

Ran some parts today. Seems that changing the Z start position is the most straight forward way to adjust where the thread starts. (Z linear offset = pitch(angle/360)) The thread does indeed always start at the same angle, given the same program.

Thanks very much for the suggestions guys. Worked out very well.

Regards,

Robin