[kjoy]

I'm running a Haas SL20 and have a question about the G76 canned cycle. It would be nice if the machine's software supported double block G76, but it doesn't. That being said- I'm running a large thread pitch (metric 4) in 1018 and am getting an ugly finish on the back side of my threads (Major=1.882 inch, typ 300rpm- I've tried slowing it down to as little as 150, it only seems to "rip" at the material). I have tried adjusting my 99 and 98 settings (finish allowance, minimum depth) to allow spring passes and such, with unsatisfactory results. I have tried P1,2,3 and 4 (though I admitt I don't have a complete understanding, aside from the standard definitions, of what these are supposed to do) and they do not seem to make a difference. The best I have been able to do is program two G76 paths, leaving a couple tenths on the minor of the first- and entering a large D value in the second (effectively creating a couple spring passes). Though its better, I'm still not happy with it. I am aware that some materials are just difficult, but given the look of the lead edge, I'm sure it can be better. Any suggestions? Though I've never used G92, I understand it in theory. Is this my only other option? Any help would be greatly appreciated.

[Geof]

In this situation I would use G92 because it is possible to exactly control the cut depth on each pass.

I would also be tempted to go faster rather than slower. I have found 1018 tends to tear badly at slow speeds. However, when thread cutting sometimes you are limited in speed because you exceed the rapid capacity of the machine when the tool is retracting; but I would try faster and see what happens.

Also I would look into getting an angled shim for the toolholder. A large pitch thread has a high helix angle and sometimes this means the tool does not have enough clearance. It needs to be angled so it matches the helix angle better.

[kjoy]

Yes, slower was much worse. I've gone up to 450rpm, but was also concerned about burning up my insert. I will try faster though. As far as the angle... I'm using an insert with a 60deg included angle made specifically for larger threads. I guess I'm not sure what you mean by shimming it for a better angle. Isn't this the purpose of the insert shape?

[txcncman]

Guess everything is based on perception and experience. 1.882" is not a large thread. I have successfully cut 4.500" with 4 TPI on a Haas TL-3 using G76 threading cycle in 4140. 1018 is pretty rough material and sometimes difficult to get a good finish. P2 is usually the best option, but mostly just helps your threading insert wear more evenly, giving longer tool life. As suggested, you probably are not turning enough RPM. I was running about 200 on the 4.500" threads. That is about 235 SFM. For 1.882", that becomes 477 RPM. And, based on past experience with 1018, I suspect you will need to be over 600 RPM to get a decent finish. Put first pass at about 0.012" and minimum at 0.002" or 0.003". Those are my recommendations.

[fordav11]

The 'angle' means the insert is tilted sideways slightly to give it more clearance.
Here is a page containing tips on solving threading problems...... Insert wear
For your problem where there is poor finish/ripping on one side of the thread they suggest changing the in-feed method or changing the angle of the shim.

The bottom of this page shows a diagram of the different shims....
CoroThread 266 - Overview

I've attached a quick snap of the shim angle chart from a large book I got from our Sandvik sales rep. These are handed out on request to big-spending customers
It's called The Sandvik Coromant Metal Cutting Technical Guide (~800 pages). Unfortunately it's not available online as far as I can see.

If you look up your diameter and pitch on this chart (near enough M48x4) you will see that your shim needs to be 2 degrees, and your thread is right on the 1 degrees limit for what your insert can handle with the normal shim and/or normal tip angle. Sandvik threading tools (and possibly others) have interchangeable shims that can tilt the insert to suit your pitch and diameter. It does make a big difference if you are close to the limit on the diameter and pitch that the insert would normally handle.

Having said all that I'm tending to agree with txcncman about your thread being pretty standard. Not big by general turning standards. I routinely cut 4" to 8" diameter threads with pitches ranging from 0.200" to 1" with no major issues. Of course the larger pitches are special threads that are profiled using a single point tool. But my point is your thread is fairly common and relatively easy with the right approach

[kjoy]

Thanks for the tips guys. I'll try it out today and let you know how it works. To clarify one point though- by "larger thread" I didn't mean diameter. A 4tpi pitch is a much deeper thread than a 40tpi. This is what I actually meant, I guess I could have worded it better.

[Geof]

......I guess I could have worded it better.

Gotta watch it with those words or all those guys cleverer than you are going to jump all over you.

I guess your query about what I meant by "angled shim" has been answered. I probably could have worded it better. Actually you were (are) fighting three awkward issues, all related: 1018 tends to be 'gummy' and the chips flow better at a higher surface speed. I have often found going up to or above 400SFM can give an improved finish. With a large (high) lead thread (See below for more words about this.) this can be problematic because sometimes the feed cannot keep up with the rpm needed on a smallish diameter. To cap things off a high lead thread on a smallish diameter gives a larger pitch angle so, unless the tool is tilted slightly so the top surface is closer to perpendicular to the helix angle, the lack of clearance can lead to the tool rubbing on the leading flank.

More Words:

Pitch is the distance between adjacent thread profiles.
Lead is the distance the thread travels in one revolution.
On a single start thread pitch and lead are the same.
On a multi-start thread lead is a multiple of pitch.
Lead is what should be used to calculate helix angle; pitch is only correct for a single start thread.

On a final note: Welcome to CNCzone.

P.S.: See if your customer can accept leaded, 12L14, almost identical tensile to 1018 and far easier to machine.

[kjoy]

Geof- Thanks for the advice... all of it.

I'll keep all these things in mind next time I'm programming a similar part and try something new. As for this part: I upped the speed, but it did little to improve the finish. Being that they were production parts that needed to get out the door, I decided to stop being such a perfectionist.

Thanks for all the help guys.

[g-codeguy]

As already stated, in your case faster is better. I think it would be a pretty poor lathe that couldn't do at least 120 IPM. That would be about 760 RPM for a 4mm pitch thread. Insert grade is going to be another factor in determining what surface feet to run. If it is a grade designed for toughness, then SFM will be slower. KC5025 minimum SFM is 150 for this material while KC5010 minimum is 300 SFM. I definitely wouldn't be running on the low end unless you had to for various reason(s). I typically thread 316 SS at about 365 SFM using Seco CP500 inserts, but will drop down to the 150 SFM area for KC5025.

Besides G92 you should have an option such as G32 which allows infeed angles to be programmed. G92 doesn't, at least not in a Fanuc control. G92 is easier to program.

A good job was done explaining shim angle. You should always be aware of this when programming.

Another option would be to try a Cerment threading insert in this material. Cerments give better finishes at a wider range of SFM than carbide inserts.

[angelw]

Besides G92 you should have an option such as G32 which allows infeed angles to be programmed. G92 doesn't, at least not in a Fanuc control. G92 is easier to program.

If by infeed angles you mean the ability to have the threading tool advance down the flank of the thread, as is programmable via an “A” address in the G76 cycle, it should be qualified that this ability with a G32 address is not an inherent programmable feature as with the G76 cycle. It can however be contrived by calculating a new start point in Z based on the incremental difference in X of each successive cut, or by using the Q address, normally used to index for multi start threads, to achieve a similar result. Both methods require considerable input by the programmer. The same can be done with a G92 cycle.


Regards,

Bill

[g-codeguy]

If by infeed angles you mean the ability to have the threading tool advance down the flank of the thread, as is programmable via an “A” address in the G76 cycle, it should be qualified that this ability with a G32 address is not an inherent programmable feature as with the G76 cycle. It can however be contrived by calculating a new start point in Z based on the incremental difference in X of each successive cut, or by using the Q address, normally used to index for multi start threads, to achieve a similar result. Both methods require considerable input by the programmer. The same can be done with a G92 cycle.


Regards,

Bill

I was referring to compound infeed, and I realize the programmer has to do all the 'work' in figuring out the infeed with a G32. I can't recall ever seeing a Q address used with a G32 cycle in any manual. How is it used?

As for the G92, I have only seen it (and used it) in this method:

X1.04Z.3
G92X.987Z-.75F.03125
X.9736
X.9684
ETC.

I assume to use a compound infeed with a G92 would require the programmer to change the Z-starting position for every pass, but does that also mean the G92 block would have to be re-written? Or is there another method I am unaware of?

[Geof]

Haas lathes allow a 'Q Start Thread Angle' in the G92 command.

[angelw]

I was referring to compound infeed, and I realize the programmer has to do all the 'work' in figuring out the infeed with a G32. I can't recall ever seeing a Q address used with a G32 cycle in any manual. How is it used?

As for the G92, I have only seen it (and used it) in this method:

X1.04Z.3
G92X.987Z-.75F.03125
X.9736
X.9684
ETC.

I assume to use a compound infeed with a G92 would require the programmer to change the Z-starting position for every pass, but does that also mean the G92 block would have to be re-written? Or is there another method I am unaware of?

It doesn’t apply with early Fanuc controls, but an R address is used with the G92 cycle to specify a Taper amount.

A “Q” argument is available with both G32 and G92 for the purpose of machining a multi start thread. The index angle between the first start and all subsequent starts is specified by the “Q” argument, in increments of 0.001 degrees. However, the Q argument in this instance can’t be programmed with a period. A two start thread will have a Q argument of 180 degrees (Q180000), and is non modal. Omit the Q address and Zero degree is assumed.

Yes it would mean that the a new G92 cycle be started on each block, but the cycle would at least get the tool back to the start point with fewer blocks than when using G32. If the OP's machine has the User Maco option available, it would be better to write a custom cycle than program using G32 or G92 if the the G76 cycle is being avoided.

Regards,

Bill

[camsys]

There's been a great deal of excellent advice posted related to the subject
problem. It seems all of then responses centered on application methodolgy
and tooling/material conditions. I thought I'd throw another possibility out there:

Can you perhaps be experiencing electro-mechanical tuning problems?

The decription of the orginal problem included chatter etc on the thread, which
can be an indicator of ill-tuned servos. Clearly if the same type of finish
problems occur in other materials that machine more freely, then I'd
consider looking into the drive settings, and machine error comp parameters.

Because threading requires a high degree of synch between the spindle and axes
chatter and tearing can result when things arent tuned properly. If it's a new
machine it may not have been commissioned entirely. If it's an older machine
there may be backlash, friction etc. that's changed and needs to be updated.

Other physical indicators of servo tuning issues include abnormal noise, or
vibration when cutting threads.

Just some random thoughts.

threads are cut,

[g-codeguy]

Bill, thanks for clarifying. I checked a couple Fanuc manuals, but couldn't find a reference to Q with either the G32 or G92. However, I did find the Q in a 10T-11T-12T manual in the G33 threading cycle with a reference to G32 in case of G code system A. The only reference I could find to G92 in this manual was in regards to setting the Work Coordinate System. Course I could have missed it.

I know you have mentioned the 2 different systems before. We do have one lathe with a 10T control, but all lathes in my area are OT, 16TT, 18T or 21i-T although I do on occasion program the others as well. I don't understand why Fanuc would omit the Q definition in later manuals. It leads me to wonder what else is available that I have no idea about.

[angelw]

Bill, thanks for clarifying. I checked a couple Fanuc manuals, but couldn't find a reference to Q with either the G32 or G92. However, I did find the Q in a 10T-11T-12T manual in the G33 threading cycle with a reference to G32 in case of G code system A. The only reference I could find to G92 in this manual was in regards to setting the Work Coordinate System. Course I could have missed it.

I know you have mentioned the 2 different systems before. We do have one lathe with a 10T control, but all lathes in my area are OT, 16TT, 18T or 21i-T although I do on occasion program the others as well. I don't understand why Fanuc would omit the Q definition in later manuals. It leads me to wonder what else is available that I have no idea about.

The "Q" argument used with the G76 cycle is not avaiolable with the two block G76 version, referred to as Standard Series 16 Format. The single block version is available by parameter setting to select Series 10/11 Format. Fanuc actually advise in a number of their manulas to use this format if multi start threads are to be machined.

G92 used as a threading cycle is also G Code System A specific, as is the case, as you have found, with G32. G92 in G Code System B and C is used in the same way it is for a machining center for setting the coordinate system. Overwhelmingly, Fanuc lath controls are generally set to use G Code System A

Regards,

Bill

[kjoy]

Wow, lots of new information... which leads to more questions. So where to start?

To Camsys: Interesting threory, but this was a problem specifically with this part. It is an older machine with (unfortunately) little in the way of maintenance, however, I've run many other threads on this machine in various material without issue.

g-code guy: I did bump up to a tougher insert to help with tool wear and ran it at 600rpm. It was effective, though not entirely "pretty".

...along this line though... In reading up on this problem, I've seen some examples where people were programing with an "A" of 58 or 59 instead of 60. Apparently this causes the insert to cut on both edges creating a cleaner finish on the back side? Any thoughts on this?

Another question is in regards to what I've read here about a "Q" variable. Is this available in single block G76? If so, does it calculate the multiple passes based on the value? For example: Q180 would give 2 threads because that's how many fit within 360? Or are there multiple G76 lines required for each start point? (I've programmed multiple start helix grooves before, but calculated out different Z start points to do it. If what I understand about Q is true, that would be much more convenient.)

My last question: How many other programable variables are available for single block G76? I know: Z,X,A,D,K,I,E, and (if I understand it correctly) Q. E is what I use for feed rate. Some people use F... not sure if there is a difference.

Thanks again all! Very helpful.

[angelw]

In reading up on this problem, I've seen some examples where people were programing with an "A" of 58 or 59 instead of 60. Apparently this causes the insert to cut on both edges creating a cleaner finish on the back side? Any thoughts on this?

This is my preferred procedure. Particularly on large threads having a considerable thread depth, steps are often visible on the trailing thread flank when the angle specified equals the included angle of the thread form (threading tool tip angle). Only a specific few angles are available with the two block G76 cycle (Fanuc), while the angles available with the single block version are in the range of 0 to 120 degrees in 1 degree increments.

Another question is in regards to what I've read here about a "Q" variable. Is this available in single block G76? If so, does it calculate the multiple passes based on the value? For example: Q180 would give 2 threads because that's how many fit within 360? Or are there multiple G76 lines required for each start point? (I've programmed multiple start helix grooves before, but calculated out different Z start points to do it. If what I understand about Q is true, that would be much more convenient.)

The use of the "Q" address when cutting multiple starts threads, requires a separate G76 cycle for each thread starts. Accordingly, for a two start thread, one G76 cycle will be used with the "Q" address either omitted, or included with a Zero value, and a second G76 cycle will be executed with a "Q" value of 180 degrees.

I don't particularly like machining multiple start thread in this manner, as each successive thread start is being machined with a threading insert that has progressively more wear than those preceding. After cutting a thread where each individual start is machined until finished, if the thread is then checked with a screw on type Go gauge and it doesn't fit, which start is incorrect?

As a consequence of my dislike of this method, I've written a Custom Macro threading cycle that will take one pass on each and every start until finished. If the gauge doesn't fit, then I know that all starts are oversize. This cycle is still called with G76 and has all the functionality of the standard version, with the addition of the better Multiple Start function, and of course, only one execution of the threading cycle is required to complete all the thread starts.

How many other programable variables are available for single block G76? I know: Z,X,A,D,K,I,E, and (if I understand it correctly) Q. E is what I use for feed rate. Some people use F... not sure if there is a difference.

A "P" address is also available to specify the method of cutting:
P1: Single edge cutting, cutting amount constant
P2: Double edge cutting, cutting amount constant
P3: Single edge cutting, cutting depth constant
P4: Double edge cutting, cutting depth constant

I'm not 100% sure with the Haas control, but with the Fanuc control, E was used to gain added precision in the feed argument. For example when cutting an Imperial lead thread with the machine configured in Metric mode, or the inverse of this.


Regards,

Bill