[DruMor]

I am trying to cut 5/8-18 threads on a SL-20 and not having very good luck. The work piece is a socket head cap screw with the head cut off to make a stud. I am only getting maybe 2 parts before the insert chips the very end of the point off and makes a bad thread. I am running 500RPM with coolant. This is only the 2nd or 3rd time in 8 years I have cut threads on a CNC lathe, so I may be missing something obvious to someone with experience.

Does the G76 cycle feed the tool straight in, or does it feed in at 30* to cut on one edge of the tool? I see in the manual there is an "A" value that can be added to my G76 line for tool nose angle. Does this make the insert feed in at an angle? I currently do not have an A value in the program.

Thanks!

[WallyL7]

I think the Haas feeds in at 90 degrees unless you program otherwise (or it could be a setting...?)

What is the material? You are threading over threads?

If nothing else I'd simply suggest using oil of some kind - Blaser makes some honey-looking oil that is incredible for that type of stuff...but straight coolant may not be enough for you.

Moly dee or other would be better than what you are using.

[DruMor]

Im not threading over threads. It is a socket head cap screw with the head cut off and ground to a specific length. Then I am cutting fine threads on the end opposite of the original course thread of the screw to make a stud.

I do not know the alloy of the screw, but my boss estimates they are 34-36Rc.

I have some Hangsterfer's tapping gel that I can try.

[KenFoulks]

What is the OD of the bolt at the point where you trying to thread?

Besides broken inserts, are there any problems?

Setting 95 determines chamfer size
Setting 96 determines chamfer angle
M23 / 24 turn chamfering on / off.

The tool nose angle for the thread is specified in A. The value can range from 0 to 120 degrees. If A is not used, 0 degrees is assumed.

Four options for G76 Multiple Thread Cutting are available
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
P1 and P3 both allow for single edge threading, but the difference is that with P3 a constant depth cut is done with every pass. Similarly, P2 and P4 options allow for double edge cutting with P4 giving constant depth cut with every pass. Based on industry experience, double edge cutting option P2 may give superior threading results.

[DruMor]

Our machine is a 2001, so I dont have access to the P2-P4 commands.

I measured a handfull of blanks, and the OD was .623/.6235"

I got my coolant concentration up to a refrac. reading of about 10 and put "A59" on the G76 line. I went from 2 parts per edge to averaging about 6. I slowed the RPM down, it sounded better but thread quality and tool life suffered. I got the RPM back up to 500 and have a decent finish.

I am using M24/chamfer off because I am cutting a radiused relief at the end of the threads before the thread op.

I tried the Hangsterfer's gel, the finish may have been a little better, tool life wasnt as good as flood coolant.

I have a D value of .006, is this in the ballpark?

Thanks!

[gizmo_454]

You have a "D" value of 0.006"? How many passes does it take to cut the thread? "D" is the initial depth of cut. Every cut there after is sequentially smaller until you get to the "minimum depth per pass", which is in the settings. I forget the number. For a thread that size, I would be starting on an annealed piece at about D=0.015", so a harder piece maybe 0.010-0.012" would be better. This will lessen the number of passes. Less passes will help the tool life. Also, on a thread that size, I would set the setting for minimum depth per pass to somewhere between 0.003" and 0.004".

The RPM sounds a little slow to me. I might bump that up to 750 or 1000 RPM. Annealed 4140 or 303/304 stainless, I would be running closer to 2000 rpm. If you are running too slow, you will encounter "built up edge" which will break the point off the insert. You did not, however, mention the length of cut on the part, overhang from chuck, etc. If the length of cut is long enough you may encounter chatter problems which will take out the point on the insert.

A little more information might help us help you a little more.

Mike

[DruMor]

It took 19 passes to cut the thread.

After more research, I have been told that the hardness is probably more in the 38-45Rc range.

Length of cut is 1.350, part is about 1.7 out of the chuck. I have an "I" value of I-.0027 to account for the part springing away from the tool. I arrived at that number by feeling how a nut screwed on the part and tweeked it until it felt the same all the way along the thread.

I'll look for the min. depth of cut setting and see if it can help me.

[KenFoulks]

19 passes is way too many, try D.012

Setting 99 - Thread Minimum Cut
Used in G76 canned threading cycle, this setting sets a minimum amount of successive passes of the thread cut. Succeeding passes cannot be less than the value in this setting. Values can range from 0 through .9999 inch. The default value is .0010 inches.

[DruMor]

I thought 19 passes was quite a few.

I finally got all my parts made yesterday afternoon. I kicked the D up to D.012, changed setting 99 from .002 to .0035 and sped up the RPM to 1000 per gizmo's recommendations. Tool life stayed the same, but I think the finish improved. It did squeal some when I increased the RPM, so I sucked the part .200 more into the chuck and it helped.

Another thought my boss and I had was would coated inserts make any difference? I was using uncoated inserts because thats what we had.

The thing that really threw me for a loop was that all but 6 of these parts were 6.5" long, and 6 were 4.25 long. After moving the cut closer to the chuck, the long parts sounded ok. The short parts made a hell of a chatter, but the finish still looked good. BUT they stuck out the chuck the same amount and I was running the same program on them. All I can figure is the length had something to do with harmonics in the part?????

I appreciate all your help guys!!

[WallyL7]

Things like insert grade would have been helpful to know originally. I actually meant to ask you about it yesterday but figured you were done with them.

Your boss is right. A coated - or simply put, "the correct" - insert is most definitely needed when doing parts like that...also, a "J" style thread insert would be way stronger than a sharp point (Not that I have any idea what you were using)

The fact that using a specialized threading oil didn't give you better results told me you probably had the wrong inserts/program/etc.

Bet you are glad to have them done though!lol