[cutshaw]

Can someone here please tell where I can go or tell me what the formula on speeds and feeds for single point threading is for mori seiki turning centers,,I know what the g code is,,I think it is G74,,but I dont know how to figure out the speeds and feeds for a preticular thread,,,please help,,,thx eric cutshaw

[the thrill]

Last I checked it was G76... but either way.

there isn't really a formula aside from (SFM*3.82)/Dia = RPM and 1/TPI = pitch.

when you program your thread cycle, use constant RPM (G97) and IPR programming (G99). Use the above formula to calculate the proper RPM for the material at the diameter you're cutting and when you program you cycle, your feedrate (F) should be your pitch number... (example: 1/4-20 thread = 1/20 = .05 so F0.05)

[cutshaw]

your right,,the g code is G76,sorry about that,thx for the reply,whats throwing me off is ,I use to run okuma,,but now it mori seiki,,and the threading cycle for mori right now is example ,,G76 A60 E.08333 K.05891 X1.5071 D20 Z-.65;...I can program the machine on any other thing including can cycles for turning,,but I never did do much in the way of single point threading,now the company is getting into a lot of threading single point parts,,and I didnt know if there was a formula to go by to figure any diameter any thread,,you mentioned G99,,if you noticed above I didnt have a G99 in the program line.It didnt cause a problem,but if you think it should be required ,I can give it a shot,,the thing with okuma it would program the cycle for you ,,it was a new captain series machine,,and im still not sure what the E.08333 AND THE K.05891 are for,,Im I green on threading cycles ,,sure I am,,thats why im posting here Im pretty flueunt on programming everything else,,but my stumbling block is the threading thats now coming into play,is there a site I can visit that lays it out better that you can suggest,,but anything you offer is much appreciated,,,thx again ERIC

[the thrill]

G99 is the default when you start the machine up so unless you switch it it stays modal. Looks like you're using single line canned cycles. The K should be total thread depth and the E should be your pitch (feed rate).

Coming from all the years of the mori CAPS conversational, my knowledge of canned cycles off the top of my head is somewhat hazy. .08333 would be the decimal equivalent of 1/12 or 12 tpi calculated into pitch.

When all else fails, read the book

[JohnnyTurn]

What series control are you using? Everyone is making a very simple thing sound way to complicated.

If you want to thread a simple straight everyday thread like:

1/4-20 UN 2A

Fanuc control G92 prepatory

EX.

N5
G97S500M03
M08
M98P16969(SAFE INDEX POS.)
T0505X-.300(CALL TOOL 5 OFFSET 5 MOVE TO X-.300, THIS WILL ALSO BE YOUR RETURN CLEARANCE IN THE X WHEN RETURNING TO Z START POINT)
Z.250(ZSTART POINT, MAKE THIS .250 OR 4x THE LEAD WHICH EVER IS GREATER. 1/20 = .050, .050 x 4 =.200
G92X-.240Z-.500F.050
X-.235
X-.230
X-.225
X-.220(ETC. ETC. UNTIL YOU REACH YOUR ROOT DIAMETER)
G0Z1.0(CANCELS G92 THREAD CYCLE)
M98P16969(RETURN TO SAFE INDEX POS.
M1

So here it is cleaner, with no notes:

N5
G97S500M03
M08
M98P16969
T0505X-.300
Z.250
G92X.240Z-.500F.050
X-.235
X-.230
X-.225
X-.220
G0Z1.0
M98P16969
M1

That's it. G92 works on all Funuc & Yasnac controls. The G76 cycle is an option. This cycle enables you to use compound infeed to use more of the threading insert than just the front leading edge. Believe it of not, stay away from 60 Deg. Use 29 Deg for the best looking threads. This angle has nothing to do with the threadform. Many novices believe it does.

"If-a you-a gott-a sixty degree-a tool, you-a gonn-a cutt-a sixty degree-a thread form!

The angle is just for compound in-feed. Trust me 29 is the best. You really only need to use the G76 with compound infeed when threading tough materials like 316sst, super alloys etc. Mild steel, Alum., Brass etc use G92 all day. Best way.

If you want the skinny on how to use G76 send me you controls G76 parameters. Every maker, Mori, Hardinge, Nakamura, etc uses different address's for the same funtion.

Hope this helps.

JT

[the thrill]

I was going to suggest G92. If your mori lathe has a MAPPS control (MSG or MSX series control), you could use CAPS to program the thread and post it out with a variety of flank options and such. It'll output G92 as standard.

[cutshaw]

thx for the reply johnny,,,the machine is a mori seki sl-35,,,I understand the process you explained here,,except for the m98 P16969 ,What is the 16969,,and to you what is the easiest way to figure out the feed rate on any thread that you chose,,like 3/4-16 and so on,,I dont understand the process you came up with on the 1/4-20,,sorry to be a rookie on that part,,but help if you dont mind,,,but the threading process you have posted seems much ,,much,,simpler to use,,and I will give this a shot when the time is needed,,again thx very much for your input on this

[JohnnyTurn]

Cutshaw,

Thanks for the machine model, but what control do you have? Fanuc, Yasnac? and what series 18-T, etc.

M98 is the Fanuc subroutine/macro call command. It say: Hello control, subroutine/macro #6969 calling. Control says: Hello 6969, how many times repeat? One time says M98P16969

Where: M98 = Subroutine/ Macro call command

Where: P1 = Repeat one time

Where: 6969 = program/subroutine/macro number 6969

Lets give you a bit of history:

Hardinge came up with the best way to program fanuc controls. It's called the Hardinge safe indexing programing format. All it is, is a safety. It forces the machine to be in a safe indexing position no matter where you start the program from. I have seen many machinists not use this format and have crashed their machines because they do not use this safety.

What you do is to write a "SAFE INDEXING POSITION SUBPROGRAM"

This will include a return to a safe indexing position (every machine can do this differently G28, G30, #501=X12.0 #502=Z12.0)
You will have to find what works best for your machine.
It will include a G40, TNRC OFF, T0, Tool Offset Cancel, G90, Absolute programming, G00, Rapid traverse and any other safety you wish to include.

What this does, is always puts the control into a safe position for indexing, cancels all unwanted modal codes, and gives you a fresh start for subsequent tools.

I learned under a pervert who used 6969 as his subroutine number. It stuck and my safe indexing program has always been 6969.

Now, to use it correctly you must place M98P16969 BEFORE the T word AND AFTER the tool has cleared the workpiece. When my X has cleared I go out to G00Z1.0 then call M98P16969 to go to my safe indexing position.

Don't forget, YOU MUST WRITE YOUR OWN O6969 PROGRAM AND STORE IT IN THE PROGRAM LIBRIARY.

I remember the troubles of learning haw to machine good threads. So as Bubba says: "I feel your pain"

Any Unified Thread you want to cut, (A thread that has a TPI) all you have to do to solve F is to divide 1 by the TPI.

So, you said, 3/4-16 right? So go, 1/16 and that equals .0625, F = .0625

Now as far as speed in concerend. Forget the SFPM formula. Threads are a tricky thing. And there is no perfect formula that works across the board to make all the different threads and their respective diameters.

Thats why mechanical engineers can't machine. They think in absolutes. machining is a sort of black art. Data, is important, but does not always solve the problem.

If you are cutting harder to machine materials like 316sst or super alloys, Inconel etc, you need to run your tool around 100 SFPM. Take a max of .005 per pass and you will get results. Softer materials you can try to go as fast as you think. There is a limit on how fast you can single point thread though.

The formula for figuring MAX spindle speed on any given thread is: 120/lead

So, 3/4-16 thread, 1/16 = .0625, 120/.0625 = 1920 max spindle speed.

If you go any faster than this you will get lead error. The thread may look OK but it will not gage.

1920 RPM is very fast. Don't use fast speeds like this. I normaly don't go any faster than 1000 RPM.

For softer materials use between 500 RPM and 1000 RPM
Harder materials use the 100 SFPM formula.

That's the real trick isn't it? Speeds & Feeds! These are good starting points, but many things can alter the results.

Long overhang i.e. diameter to length ratio. Makes for bad rigidity. Coarse threads are tougher to make that fine. Apt to chatter. etc etc. That's what the machinist's job is, make it come out right. You have to fool with it a bit.

There is no perfect formula across the board. But with this data I have given here, you should be able to do it.

Good luck,

JT

[cutshaw]

scan.pdf

[g-codeguy]

Cutshaw, JohnnyTurn has given you some excellent information tho I don't agree with everything he said. Will get to the disagreement part in a bit.

I really like the Hardinge Safe Index programs, and use them on every machine I can. What Johnny didn't mention was that Hardinge uses two of them. One at the beginning of the program (I will use it at the end of an operation if my tool is in front of the part), and one at the end of an operation. Scares the he$$ out of an operator that can read a program, but is not familiar with the Safe Index programs. Say you are drilling. The end of my op. would look like this:

G1Z-.75F.008
M92
M1

M92 is a M-code program call that I use to call the Hardinge Safe Index subprogram for end of operation. First block in it is G0G97Z.5. So when boring, grooving, etc., clear X then call up the sub. I put my safe index subprograms in protected 9000 numbers to keep operators from accidentally deleting them, or trying to modify them. I use the M-code call instead of M98P9002 because I am lazy. Less typing.

Part of the Hardinge Safe Index programs is another very short sub that contains the safe Z-axis position. After the set-up person finishes touching off the tools, he checks the Z-GEOM for the longest tool, then puts this number plus another inch in the 3rd Hardinge sub. Now the turret will always index one inch in front of the part. I don't have this program in a protected number, but could, and then use a macro for the Z dimension.

This is what my safe index programs look like.


:9001 (MAIN SAFE START & O.D. END)
G0G40G97G99M42
M98P999
M99

:9002 (MAIN SAFE I.D. END)
G0G97Z.5
G40
M98P999
M99

:999 (MAIN SAFE INDEX)
T0
X4.Z4.
M99

I use another set for subspindle work. You may have to modify these for the control you are using.

Here's where I disagree with Johnny. I thread 15/16-26 & 3/4-28 UNF threads at S1350 in 303 SS. Would go faster, but threads have to be within a certain distance of a shoulder. The higher the RPM the sooner the insert starts to withdraw from the thread. Just asked the operator how many parts per corner. His best estimate is around 3000 parts per corner. He runs one or the other thread day after day, year after year. DOC of first pass is .006 because of the thread height.

I run a 7/8-20 UNF at S1600 in 316 SS and a 1-5/8-20 UNF in 316 SS at S850. No problem. I use G76 cycles for all. Am threading 15/16-26 UNF at S1800 in 430F because there is only a .055 thread relief before a shoulder. Otherwise I would be threading faster.

Inserts are designed to run within a certain SFM range. Go too fast and they burn up. Go too slow and they can chip. What happens going too slow is material builds up on the cutting edge. Then at withdrawal from or entering another cut, the insert can chip. Even if it doesn't chip, the built up material on the cutting edge gives a poor finish to the threads. Can even leave grooves on the flank of the thread if big enough build up. Having said this I must tell you that some grades are better than others at running below the suggested SFM. Some will chip within 3-4 pieces while others will do a fair number of parts before causing problems. Sandvik makes one of the better grades for this of the companies I have experimented with. Problem with Sandvik inserts is that you have to use their tool holders. Their insert is .015 thicker than the standard everyone else uses.

I also use 120 SFM for thread RPM maximum speed. Got it from a Hardinge manual. They were the first lathes I programmed. However this isn't written in stone. Had chatter problems on an external thread one time. Small part. Wound up threading at 70% over the 120 SFM limit with a cermet threading insert on a Hardinge T42 Conquest. Good thread, but you do have to start further away to give the machine time to accelerate to the correct feed. Can't recall the RPM used, but know it was over S3000.

I have threaded at S3000 on other parts with no thread lead problems. Just remember what I said about starting further away from the actual thread.

Nor do I agree with Johnny about not taking more than .005 DOC per pass. Depending on thread height I may use anywere from .006 to .015 or more for the first pass. Of course material type also has some bearing on my DOCs. We all know that some materials work harden easily. For these I try to use .003 for a minimum DOC. Sometimes it isn't possible to follow this rule, and I have even made spring passes on hardening materials. Not good for tool life, but you do what is necessary to get good threads.

I haven't used the G92 threading cycle in a good many years. Can't use compound infeed with it. This creates the toughest possible chip as the chip is the same thickness on both sides of the insert. (Maybe why Johnny uses .005 for maximum DOC?) If I need a manually programmed thread, I will use G32 so I can do compound infeed.

However, I am not hard-headed. Next time I am having problems with a G76 cycle, I will try Johnny's suggestion and give the G92 cycle another shot.

[JohnnyTurn]

G-code Guy,

I like the name by the way. Too many posers out there now-a-days with zero G code knowledge.

Anyway, I can see you are up to speed on programming and tooling. Let me inform you about some of your comments directed towards me.

The M92 function was not taught or shown or available when I visited Hardinge in 2001.(Nor do I agree with you on how you use it. A subroutine for clearance when your inside a hole, bad idea)
I had been successfully programming and machining CNC Mills since 1994 and when I attended Hardinge training in 2001 I used it as a sort of finishing school (We had bought a new 6/42). 2-3 weeks before class started I wrote down all the little questions one develops through the years. Since I was somewhat new to CNC turning at the time (started CNC turning in 1998 on CHNC3's) I had questions on how to machine better threads with more pieces per insert. When the Applications Engineer (Gary Blackwell) saw that I was an advanced CNC Machinist, I was offered to leave the class and take a semi-private coarse with two other Hardinge Machinists. I accepted eagerly, those green horns I was with the first day didn't know how to turn on a machine let alone use it.

With that being said, I learned so much that week that when I returned to my shop, one of the machinists who I had worked with for 8 years could just see it in me that I had come back more powerful. I also had learned CAP 2 programming. I Figured the 18T had it, why not learn it. I Never use it though. Some guys, it's all they know. Without it, they can't machine anything.

Every part I make here, is to spec. or better. 99.9% of the time my parts exceed all requirements. That .1% of the time, I just meet them.
I machine tough to machine materials here. It's hard to compare with anyone that just does general machine work. You were speaking of 303 SST before. Please, that's like cheese. And I can tell you are one of those guys that holds 316 SST as some kind of major feat. That's our bread and butter here. And some other everyday materials are Inconel 22, Monel 400, Kovar, 17-4PH, Waspaloy, Nickel 200, just to name a few. So I may not know about your 3000 rpm Brass threads but I do know that you try that nonsense in real materials like I have mentioned, and your toast. I am a Precision Machinist. There is a difference!

I don't care if the job runs 5 minutes longer. I care about how many parts per insert/end mill and what is the part to part consistency. Also, My setups don't need constant attention and constant fiddling and tooling replacement. When you machine in High Temp Alloys, you better know how to get every last work piece from your tooling or you will just be making MSC/J&L rich. Rip through 20 3/8 SC Emills for a job, let me know how ya boss likes it!

So I do not agree with you at all about high RPM and high stock removal when threading. .005 works for all materials. I know you can cut more per pass, but I find this to be the best. Every machinist that sees my threads comment on the beauty. In fact, a hard as nails Raytheon Inspector said, and I quote, "I'm lovin' your threads!" So, be a cowboy, ramp it up, index your tooling every 15 min. and push the spindle and the drives at their fullest. We shall see who wins in the end when parts come back with shiny red stickers on the box.
But then again you are talking about Brass, 6061, 303, 1018, cookie cutting. And I believe I mentioned to use .005 DOC in TOUGH materials. Not soft!

Getting back to your M92 idea. I do not agree with your laziness. It's better practice to rapid out to Z1.0 on a drill then call your safe index. On a BB, clear your X by .010 rapid out to Z1.0 call Safe Index Subroutine. Never assume, I don't like it and I would NEVER use your sequence on any of my equipment.

Another thing, you mention operators touching programs. Any operator touching programs in my shop will have a all expense paid trip over to the vertical band saw for a quick hand removal. LOL
No one is to touch programs except qualified Machinists!

Why use G32 for single pointing when you need compound in feed????
G76 has it automatically. Why waste your time with all the cumbersome Z start point formulas. G32 is really for a floating tapping head. There it works well. Also, you can use it for a poor mans spindle orient.

G76 already has compound in feed in it.
PARAMETER ENTRY LINE: G76P010029Q0050R0030

Where 01= 1 spring pass, 00= No pull off (most of the time called chamfer)
29= degrees of compound in-feed, Q= Min. depth cut, R= Fin. pass amount.

Guess where I learned about the 29 deg. trick for best 60 Deg. threads?
H-A-R-D-I-N-G-E training! It's not my fancy little idea, it's the nuts.

Another thing you are wrong about is your comment about: "The higher the RPM the sooner the thread pulls out." WRONG. That is controlled by a parameter in the control and by the pull off distance
(better known as chamfer). You can set that parameter to Zero so the X axis will jump off hard as hell at the end of the pass. That is the only reason it's really there. So the machine doesn't jolt hard at the end. Also, it's nice to chamfer out the thread on a shaft with no undercut. But when going into a shoulder, (Esp. when a damn engineer had specified a .040 wide undercut) it's nice to know you can shut the chamfer off all together.
But again.....
ALL THE MORE REASON WHY HARDINGE TELLS YOU NOT TO THREAD AT COO-COO COWBOY FEEDRATES WHEN THREADING!!!!!!!!

So that's my rant for today! Isn't this machining stuff fun!!!!

JT

[g-codeguy]

Johnny Johnny. A little testy are we? I feel a rebuttal coming on. First let me say that I don't think you read my post very carefully based on a couple of remarks you made.

G-code Guy,

I like the name by the way. Too many posers out there now-a-days with zero G code knowledge.

Thanks. I've always preferred manual programming to using a CAD/Cam software. However, I now do most of my programming in Mastercam because that is what the boss wants...IF I HAVE TIME. Takes longer. Especially since I take the extra time to get the output as close as possible to my manual programs. The other lathe programmer doesn't care as long as the part runs without crashing.

The M92 function was not taught or shown or available when I visited Hardinge in 2001.(Nor do I agree with you on how you use it. A subroutine for clearance when your inside a hole, bad idea)

M92 wasn't taught to me nor is it a function. It was available when you took the Hardinge class. Look in the Fanuc Operator's Manual under Custom Macro. Check out the page describing how to use a "Macro call using an M code." See below for further comments on this.

Every part I make here, is to spec. or better. 99.9% of the time my parts exceed all requirements. That .1% of the time, I just meet them.

I think we are a lot alike here. A part may have +/-.005 tolerance, but if it is consistently running a tenth off the mean I will make the offset change to bring it dead on. A little anal, but I take pride in my work.

I machine tough to machine materials here. It's hard to compare with anyone that just does general machine work. You were speaking of 303 SST before. Please, that's like cheese. And I can tell you are one of those guys that holds 316 SST as some kind of major feat. That's our bread and butter here. And some other everyday materials are Inconel 22, Monel 400, Kovar, 17-4PH, Waspaloy, Nickel 200, just to name a few. So I may not know about your 3000 rpm Brass threads but I do know that you try that nonsense in real materials like I have mentioned, and your toast. I am a Precision Machinist. There is a difference!

I know 303 SS cuts like cheese. 430F cuts like butter. I used them as examples of threading over 1000 RPM. I also mentioned the RPM used on a couple 316 SS jobs. Remember? Who said anything about Brass? Our 51 Conquest is set up with a 2-jaw check. Can't remember the last time it ran a job that wasn't a 316 SS casting. About 3 years ago we switched our Hitachi to a 2-jaw chuck and I trained a mill operator to run it so he could finish machine two jobs coming off his mill. Both are 316 SS castings...as is the only other job to run on this lathe since then. The Mori SL-25 runs with either a 2 or 3-jaw chuck. Guess what material it is machining when the 2-jaw chuck is on. It is currently set up with a 3-jaw chuck running, yup you guessed it, a 316 SS casting job. Almost all these programs were modified from the 51 Conquest programs that ran these parts previously. All the Conquest programs were written by me. The Daewoo next to it runs a lot of 316 SS castings and slug jobs with the occasional Hast. C job. Most of the lathes I program are barfeed machines. These lathes also run 316 SS round or hex bar stock jobs on occasion. So I think I know a little bit about machining 316 SS.

Been a long time since we've had any kind of Inconnel to run. We do run 17-4PH, 420, 420F, 304, 440C, BG-42, XD15NW, X30, Pyrowear 675, Schedule 40, Carpenter 20, Hastelloy C and Waspaloy to name a few. Ever machine Stellite? Pretty tough stuff.

Regarding the 3000 rpm brass thread comment you made. We mostly use Seco threading inserts. The suggested starting SFM for 316 SS type of material was 365 for a CP50 grade insert. I still use this value for the CP500 grade that replaced the CP50. Don't know what size material you run, but most of my jobs are small. Using this SFM and .312 to figure the rpm for a 5/16 whatever pitch thread results in a value over 4400. And you thought 3000 was high!! No I don't thread at this speed. The maximum rpm for a 24 pitch thread using the 120 fpm formula would be S2880.

When I first started I use to run a job with .0002 total tolerance on the bore and with two faces that had to be parallel within .0002. We still run many jobs with a total of .0005 tolerance and sometimes a tenth or two less. Does this qualify me as a Precision Machinist?

I don't care if the job runs 5 minutes longer. I care about how many parts per insert/end mill and what is the part to part consistency.

You must own the shop. Otherwise consider yourself lucky. Time is money where I work. Minutes??? Try seconds. Nothing gets said to the mill guys about cycle times, but us lathe guys have to put up with BS all the time. (You are obviously a mill guy. LOL.) Most of my jobs run in 2.5 or less. Almost all end washers run in less than one minute. These are mostly made from 52100, but some 420 and 440C. I had one brass job that the work order specified it had to run at a maximum of 45 seconds. Took some doing, but I did it. The other lathe programmer has the bigger lathes so his cycle times may run 5 minutes or higher at times. An old timer here said he remembers hearing a statement made one time that the lathe department paid every ones wages in the company.

Also, My setups don't need constant attention and constant fiddling and tooling replacement. When you machine in High Temp Alloys, you better know how to get every last work piece from your tooling or you will just be making MSC/J&L rich. Rip through 20 3/8 SC Emills for a job, let me know how ya boss likes it!

My guys don't have to change inserts every 15 minutes either. I try to balance cycle time with tool life. Sometimes I am forced to cut say 10 seconds off a cycle time even tho it results in fewer parts being made at the end of the day. Owner is only concerned with the cycle time. Upsets me, but he signs my checks. 3000 parts per corner ain’t bad even if it is in 303 SS and don’t forget they run over your S1000 limit.

I program lathes only. Wouldn't think to correct you on any mill work.

So I do not agree with you at all about high RPM and high stock removal when threading. .005 works for all materials. I know you can cut more per pass, but I find this to be the best. Every machinist that sees my threads comment on the beauty. In fact, a hard as nails Raytheon Inspector said, and I quote, "I'm lovin' your threads!" So, be a cowboy, ramp it up, index your tooling every 15 min. and push the spindle and the drives at their fullest. We shall see who wins in the end when parts come back with shiny red stickers on the box.
But then again you are talking about Brass, 6061, 303, 1018, cookie cutting. And I believe I mentioned to use .005 DOC in TOUGH materials. Not soft!

Too bad. See my previous comments on high RPM, materials and tool life. Never had anyone say "I'm lovin' your threads!". However, never in 100s and 100s of thousands of parts shipped have any come back because they weren't "pretty enough". Had some come back because operators didn't hold threads to size, but that has nothing to do with how they were programmed. With the exception of 303 SS we do run some jobs in all of the materials you just mentioned. We run a lot of 303 SS.

Getting back to your M92 idea. I do not agree with your laziness. It's better practice to rapid out to Z1.0 on a drill then call your safe index. On a BB, clear your X by .010 rapid out to Z1.0 call Safe Index Subroutine. Never assume, I don't like it and I would NEVER use your sequence on any of my equipment.

My remark about laziness was a tongue-in-cheek comment. Assume??? Assume what? I know what the first block is in the subprogram. The program is in a protected number. How do you know that your subprogram is going to send the tool home after you manually program that Z1.0 instead of making a rapid move back into the part? Couldn't start to estimate how many programs I have written this way, but you can bet the farm that 10,000 is way too low a guess. Never had a crash from using M98P1, M98P9001 or M92 and never will. These are all the same subprogram, just how my programming progressed. The results of our methods of programming are the same. The only difference is you have to type an extra block of information at the end of every operation.

Many times I have given a tooling list to a set-up person, and then programmed the job while he was getting the tools put in the machine. Usually I finish first. That is another reason I use M92...faster and less chance of making a typing error. Did it yesterday.

Another thing, you mention operators touching programs. Any operator touching programs in my shop will have a all expense paid trip over to the vertical band saw for a quick hand removal. LOL
No one is to touch programs except qualified Machinists!

From this statement it’s obvious that you go out to the machine to modify the Z clearance after the set up person finishes touching off the tools on every job that gets set up on machines using the Hardinge safe index subprograms. Seems like a waste of your time. Definitely wouldn't call all our set up people excellent machinists, but they all know how to add 1.0 to the longest tool, and modify the Z to that dimension (usually rounding up to the nearest half or quarter inch). And I thought we had some slow people!

I don't like others modifying my programs either even tho this only involves slowing RPM, max rpm in G50 blocks or feedrates. I want to know why the changes were necessary.

Why use G32 for single pointing when you need compound in feed????
G76 has it automatically. Why waste your time with all the cumbersome Z start point formulas. G32 is really for a floating tapping head. There it works well. Also, you can use it for a poor mans spindle orient.

Another example of not reading my post carefully. A direct quote from my post above. "I use G76 cycles for all." Another quote. "If I need a manually programmed thread, I will use G32..." I've used G32 instead of G92 for years because of the information given in the technical section of carbide distributor catalogs in their threading sections. I am not too lazy to take the time to figure the math.

G76 already has compound in feed in it.
PARAMETER ENTRY LINE: G76P010029Q0050R0030

Where 01= 1 spring pass, 00= No pull off (most of the time called chamfer)
29= degrees of compound in-feed, Q= Min. depth cut, R= Fin. pass amount.

Sorry, but you can't tell me anything about how a G76 thread cycle works that I didn't already know long before you wrote your first lathe program. Don't forget that R can't be used in this block when machining tapered threads.

Guess where I learned about the 29 deg. trick for best 60 Deg. threads?
H-A-R-D-I-N-G-E training! It's not my fancy little idea, it's the nuts.

You got me there. Never had any Hardinge training, but I learned that Hardinge settled on 29 thru experimentation from talking with a Hardinge tech rep. I learned machining by writing the program, setting the job up, running it, then figuring out what to do to solve any problems I might be having with that job. I increased my knowledge my reading the technical information in carbide catalogs, and occasionally talking with one of their reps about a problem I would be having. Taught myself to macro program reading the Fanuc operator’s manual.

Another thing you are wrong about is your comment about: "The higher the RPM the sooner the thread pulls out." WRONG.

I've already proved my statement to be true through actual machining at higher rpms. Several times. That's a fact. Believe it or not. You've never seen this phenomenon since you don't thread any faster than S1000. That's another fact.

That is controlled by a parameter in the control and by the pull off distance
(better known as chamfer). You can set that parameter to Zero so the X axis will jump off hard as hell at the end of the pass. That is the only reason it's really there. So the machine doesn't jolt hard at the end. Also, it's nice to chamfer out the thread on a shaft with no undercut. But when going into a shoulder, (Esp. when a damn engineer had specified a .040 wide undercut) it's nice to know you can shut the chamfer off all together.
But again.....

Don't know anything about the parameters controlling the G76 cycle as I've always been able to accomplish what I wanted without making any changes to them. However, I will look into them. Pulling out quicker would be a benefit to me. You do realize that you can use the 00 in your above example to control the thread pull out chamfer. You do know how to use it, right? Save you the trouble of changing the parameter back and forth to achieve the same results.

ALL THE MORE REASON WHY HARDINGE TELLS YOU NOT TO THREAD AT COO-COO COWBOY FEEDRATES WHEN THREADING!!!!!!!!

Obviously you've never talked to a carbide tech rep. Otherwise you wouldn't consider anything over S1000 to be 'COO-COO'. This is the second time you have referred to me as a 'COWBOY' Only wish I were. Country hick, yes. I like to think I am a pretty decent programmer for the jobs we run. Others seem to think so also. Put me in a different shop running different types of jobs, and no doubt I would have to learn new things. I like learning.

So that's my rant for today! Isn't this machining stuff fun!!!!

Yeah, it's fun. I really enjoy my job most of the time. Seems you do too.

EDIT: Maybe you shouldn't arbitrarily dismiss others opinions. You might learn something new. I know I do.
EDIT2: Meant to tell you that the 3/4-28 and 15/16-26 threads were running at S500 to S800 and making 19-21 passes when I first started. We had chatter problems and the inserts wouldn't hold up. I did a little research, and increased rpm to 1300-1400 and decreased passes to 5 or 6. No more chatter. I already mentioned how many parts we now get per corner. I figured it out, and the cycle time from this one change made to one machine (the Hitachi was running those bodies at that time) paid for my yearly salary if based on $50 hr. lathe rate. These changes were made to all the other lathes. Doesn't take into account the savings in the cost of inserts or time saved while changing the insert and getting back on size.

[cutshaw]

GOOD GOSH GUYS PLEASE,,WE ARE ALL FRIENDS HERE,,LOL...JOHNNY DID YOU GET THE PRIVATE MESSAGE ,,TO SEE IF I WAS CORRECT IN MY FIGURING,,IM LATHE GUY TO,,AND CYCLE TIME SEEMS TO BE THE BIG BURR UP THE BOSSES @%*,,IF YOU GET WHAT I MEAN. HOPE TO HEAR FROM YOU ALL,,AGAIN THX FOR ALL YOUR GUYS HELP AND EXAMPLES HERE

[g-codeguy]

GOOD GOSH GUYS PLEASE,,WE ARE ALL FRIENDS HERE,,LOL...JOHNNY DID YOU GET THE PRIVATE MESSAGE ,,TO SEE IF I WAS CORRECT IN MY FIGURING,,IM LATHE GUY TO,,AND CYCLE TIME SEEMS TO BE THE BIG BURR UP THE BOSSES @%*,,IF YOU GET WHAT I MEAN. HOPE TO HEAR FROM YOU ALL,,AGAIN THX FOR ALL YOUR GUYS HELP AND EXAMPLES HERE

What? You thought Johnny and I were fighting? No. No. Just having a spirited discussion! You know how it is between the elderly and the young. Sometimes we have trouble communicating.

I hope our spirited discussion was of some benefit to you.

[the thrill]

wow... this conversation sure got a little heated, eh?... all this over some threading cycles...

nickel 200 is just gummy... it's nowhere near as ugly as 45Rc heat treated inconel 718...

I had a guy bring in a piece of vascomax and thought it was kryptonite (considering it's got 9.25% cobalt in it)... I ran his ugly 1" rougher end mill 3/4" deep full slotting on a 15hp machine. He was wondering why the machine left a step on the bottom of the floor (I did the slot then went back on both sidewalls and you could see a dish/step). Turns out the end mill was working so hard it was twisting to the left LoL.

17-4ph isn't really that nasty... machine it dry at about 475sfm, .004-.007ipt on insertable end mills and they'll last for a good long time . I love when people make all these quibbles about machining Ti6Al4V and how you can't go over 175-180sfm yadda yadda yadda... i've run that stuff at 250sfm with good results using Hanita Varimills

sorry, i'm just rambling... I love metal talk

[g-codeguy]

wow... this conversation sure got a little heated, eh?... all this over some threading cycles...

nickel 200 is just gummy... it's nowhere near as ugly as 45Rc heat treated inconel 718...

I had a guy bring in a piece of vascomax and thought it was kryptonite (considering it's got 9.25% cobalt in it)... I ran his ugly 1" rougher end mill 3/4" deep full slotting on a 15hp machine. He was wondering why the machine left a step on the bottom of the floor (I did the slot then went back on both sidewalls and you could see a dish/step). Turns out the end mill was working so hard it was twisting to the left LoL.

17-4ph isn't really that nasty... machine it dry at about 475sfm, .004-.007ipt on insertable end mills and they'll last for a good long time . I love when people make all these quibbles about machining Ti6Al4V and how you can't go over 175-180sfm yadda yadda yadda... i've run that stuff at 250sfm with good results using Hanita Varimills

sorry, i'm just rambling... I love metal talk

Ramble all you want. I don't mind. Can even learn something from it. Don't program mills, but would like the opportunity. It will never happen where I work even though I was promised 3 years ago that I could. Like I said, the lathe department is the one making the most money, and we have enough machines and work to keep us two lathe programmers busy. Course we both set up too.

Well, statements were made without having the slightest idea of my experience. Some I resented. More statements were made about rpms and DOCs that I know to be BS from years of running lathes. Probably while he was still in grade school! Haven't run Inconel in years and don't think any of the jobs we did run required threading. So I can't make any comments about threading in that material.

Actually think we would get along if working for the same shop. It is apparent that he takes pride in his work, and likes learning. Kind of guy I prefer working with.

[the thrill]

mills, lathes, mill/turns, 4, 9, 12 axis lathes... it all turns into a mush after a while. It all comes down to the fundamentals. On lathes it's chip control, workholding a tool life, on mills it's the same but different. The chip control is more of a "how do we get the chips into the pan?" rather than "how do we keep this damn material from strining so bad?!?!" Talk to enough tooling guys, read the backs of the packages, follow the recommendations, adjust for machine life/rigidity and have a blast. If you want to learn a lot about everything, try to get a job with your local CNC machine distributor or OEM. The travel is extensive and if you're a family man you'll hate the job but the knowledge it brings about the latest products and life are well worth the delayed flights, the angry customers and the stupid alarms stemming from faulty ladders in prototype machines. All in all you gain knowledge you really can't pick up in a shop due to empty promises or people saying "we can't change this, we've done it like this for 30 years". The day I milled a piece of 55Rc steel at 240ipm with a high feed facemill was great. The day I cut inco at 3600sfm was great, the day I got a first article on the landing gear valvebody for the airbus A380 was great... The day that valvebody won the Mori Seiki "innovation of the americas" contest at IMTS 2008 was great (all I got was a lousy handshake... the customer got $2000!!!!!).

Too bad the management sucks at Mori Seiki USA or else I'd still be there. I'm glad to be out of that place, though... it's run by a bunch of salesmen and idiots... and idiot salesmen.