Metric and Acme threading on SL

HAA_S · Dec 13, 2009

Hi-
New to this forum but had a problem this week/weekend.
Had to cut M5 X.8 and M6 x 1. threads earlier this week and came across the simple fact that the HAAS lathe is not set up for metric threads program wise since G76 threading is based on inches per rev. (G99) So, from what I have read the lead thread will not be correct unless I change the HAAS to metric.

Is this in setting 9 (G21)?
Is there a better way?

Second, when entering an X (thread pitch) value in the G76 code, the machine never reaches the correct X value (always cuts to an X value larger then programmed) and I have to either change the X value in the G76 or subtract it in X in the wear offset to get the correct pitch dia.

Any ideas why?

Third..
Regarding ACME thread cutting on the SL. How???? LOL.
Is there a formula?
(Once again, never needed to cut these threads)

Thanks for the help in advance. Never had an issue prior because I have never had to cut either metric or acme threads on the SL (prior company never used them)

machinist man · Dec 14, 2009

Welcome to the forum!

You could convert the lead of the thread into inch and program that for your feedrate. I think you can use an "E" instead of an "F" to get 5 decimal places in your feed, that'll give you a more accurate lead. For changing the machine to metric, you have to change that setting and program a G21 in your program.

If I remember (I don't do a lot of lathe programming), X is the minor diameter of the thread. The way I've done it, I've set my offset bigger, cut the thread, measured, adjusted, and ran the thread tool again.

For acme threads, change the A in your G76 to the angle of the thread (29), and use an acme thread insert. You're going to make sure that you don't exceed the max feedrate of the machine, with acme threads being so coarse it doesn't always take a lot of spindle speed to exceed it.

Hopefully this helped, good luck!

Haas_Apps · Dec 14, 2009

Metric Threads

For the threads you have mentioned the 1mm would be .03937 and the .8mm would be .03149 feed per revolution. These values are close enough for any standard length thread.

It is normal to have to make some adjustment to the X diameter when threading.

HAA_S said:
Hi-
New to this forum but had a problem this week/weekend.
Had to cut M5 X.8 and M6 x 1. threads earlier this week and came across the simple fact that the HAAS lathe is not set up for metric threads program wise since G76 threading is based on inches per rev. (G99) So, from what I have read the lead thread will not be correct unless I change the HAAS to metric.

Is this in setting 9 (G21)?
Is there a better way?

Second, when entering an X (thread pitch) value in the G76 code, the machine never reaches the correct X value (always cuts to an X value larger then programmed) and I have to either change the X value in the G76 or subtract it in X in the wear offset to get the correct pitch dia.

Any ideas why?

Third..
Regarding ACME thread cutting on the SL. How???? LOL.
Is there a formula?
(Once again, never needed to cut these threads)

Thanks for the help in advance. Never had an issue prior because I have never had to cut either metric or acme threads on the SL (prior company never used them)

SeymourDumore · Dec 14, 2009

I think you've had a mental lock this weekend.
Think of it this way. You have to figure out the IPR feedrate for an inch thread. That is no different for a metric thread.
For inch threads, you're given a value of # of threads per inch.
You need to figure out the pitch, which is 1/TPI.
In metric threads it's even easier, as they're already giving you the pitch, which is in the case of a 1mm thread is exactly 1 mm, or 1/25.4 = .0393"
Same for a 1.2mm pitch thread is 1.2/25.4=.0472"

If your lathe is set in inch mode, then those are the values you need to use in the cycle.
No difference whatsoever between inch and metric threads as far as the cycle is concerned.

Secondly
The G76 X value is not the pitch diameter, rather the min. diameter. The tolerance of this is given in a table for each thread, but the actual X value is dependent on the size of the tip radius and the angle accuracy of the actual insert you're using. Remember, with threads the governing dimension is the pitch diameter and the lead primarily, the major ( or minor with internal thds) dimensions are secondary. With the exception of controlled root radius threads ( and some other special threads ) the minor (ext) or major (int) diameter is given only as a max or min value. You use it as a reference only when programming. Interestingly enough, these loosely controlled dimensions are also the only way for you to adjust the governing pitch dia. when threading on a lathe or threadmilling.
Hence the need to go over or under the initial programmed value.

HAA_S · Dec 14, 2009

SeymourDumore said:
I think you've had a mental lock this weekend.
Think of it this way. You have to figure out the IPR feedrate for an inch thread. That is no different for a metric thread.
For inch threads, you're given a value of # of threads per inch.
You need to figure out the pitch, which is 1/TPI.
In metric threads it's even easier, as they're already giving you the pitch, which is in the case of a 1mm thread is exactly 1 mm, or 1/25.4 = .0393"
Same for a 1.2mm pitch thread is 1.2/25.4=.0472"

If your lathe is set in inch mode, then those are the values you need to use in the cycle.
No difference whatsoever between inch and metric threads as far as the cycle is concerned.

Secondly
The G76 X value is not the pitch diameter, rather the min. diameter. The tolerance of this is given in a table for each thread, but the actual X value is dependent on the size of the tip radius and the angle accuracy of the actual insert you're using. Remember, with threads the governing dimension is the pitch diameter and the lead primarily, the major ( or minor with internal thds) dimensions are secondary. With the exception of controlled root radius threads ( and some other special threads ) the minor (ext) or major (int) diameter is given only as a max or min value. You use it as a reference only when programming. Interestingly enough, these loosely controlled dimensions are also the only way for you to adjust the governing pitch dia. when threading on a lathe or threadmilling.
Hence the need to go over or under the initial programmed value.

Ahhhh.. your right. Very helpful. I always figured it weird that the machine did not reach the given X value but now I understand. As far as the metric threads, ya I used the values given above (converted to inch) and it worked out. Ends up there was a problem with the threads because the mill guy used a worn out tap (and the hole was smaller but still right) and I made the threads to the middle of the tolerances and mine didn't fit. :willy_nilly:

Oh well. Got bigger worries this week... :angry:

Thanks everyone for this info.

Search

Largest Manufacturing Technology Community on the Web

Search

Metric and Acme threading on SL

HAA_S

Plastic

machinist man

Aluminum

Haas_Apps

Plastic

SeymourDumore

Diamond

HAA_S

Plastic

Similar threads