[4]

Hard turning, finishing the part.

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#1
A month ago a 2" + dia. bar of D2 turned up, I faced it to 110 1/4" long and drilled and tapped the ends 5/8-11, the threaded end is for hanging it in a vacuum furnace for hardening I am told.
It was then straightened and centerless ground to 1.999 +-.0005, the grinder nailed it. It is now 62C Rockwell scale hardness as well.


My job is to turn one end to 1.437" +-.001" diameter X 7" long and the other end to 1.500 +- .001" diameter X 5" long. The company that hardened it earned their money as it is every bit of 60 Rc

Due to length I had to turn it in a steady rest over a cats head and a live tail stock center, one of the advantages of having a tapped hole in each end is that one may screw a common hex head bolt in it and create a new center.

I chose a 135 Deg. insert shape to clear the center using a Sumitomo hard turning insert that I believe is cermet, unless parting to center I set the tool height with a ruler, this will probably cause many hobbyists a good deal of chagrin, this lathe is 11 7/16 from the ways to the center of the spindle.

Made a spindle guide to keep the part from flailing around at the back of the machine from nylon, this does the job of what many call a "spider".

It looks like this in use

Hard turning leaves a beautiful finish even when roughing, tomorrow morning the finishing cut will be completed and I will have to nearly double the spindle speed for this as the diameter is now smaller.
Roughed at 200 SFM, .020" DOC and .008 IPR, this is conservative, will spin it at 300 FPM, .005" DOC and a .004" IPR feed which should work nicely, this would be about 700 RPM
 

MrWhoopee

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Jan 20, 2018
Messages
387
Likes
248
#2
Looks like fun, how about that keyway?
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#3
Looks like fun, how about that keyway?
You have a completely different definition of "fun" then I have (-:
The keyway is not my problem.
 

jdedmon91

Active Member
Registered
Joined
Dec 29, 2017
Messages
286
Likes
574
#4
You sure that not a CBN insert. I never seen Cermet coated just CBN.


Sent from my iPhone using Tapatalk
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#5
You sure that not a CBN insert. I never seen Cermet coated just CBN.


Sent from my iPhone using Tapatalk
I believe it is CBN, it has about 1/4 the mass of carbide.
Worked a charm and the turning was finished this morning. As mentioned the key way is SEP (Someone Elses Problem)

Turning looked like so, I would have kept the camera on it longer but the hot chips were out to get me so only a 2 second video.
https://photos.smugmug.com/My-First-Gallery/i-5R5q99h/0/1b738faa/640/21video[1]-640.mp4
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#6
Had a cnc lathe running a lengthy program unattended so I drilled rough holes in the parts for the next job.
I made a How To video, I dislike the constant chatter prevalent in most How To ytube videos so this has no narration.

How to a Drill 1 5/16" hole through 3" of Mild Steel

1 Buy a used 60 year old WS turret lathe with a 25 HP spindle motor (-:
2 Place drill in turret position
3 Place saw cut blanks in chuck, the chuck must have serrated hard jaws and be very tight or it will push the part through the chuck
4 Turn spindle on
5 Engage turret feed and coolant
6 Sit down for 5 minutes or go and do something else, repeat 32 times
No spot drill, no pilot hole and no pecking required, drill straight through.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#7
Finished just in time today, the chips wanted revenge and were leaving the machine.
Many look forward to "making chips" I look forward to the day when I never make another chip. I loathe them in every possible way.


For anyone that has never used such a machine, the blue frame and tube is part of it.
The round unpainted part is a back rest, a "spider" chuck with its own bearings and 4 set screws to hold the stock bars. The entire tube and back rest will slide along the round bar ways and advance the stock for the next part using a hydraulic cylinder.
One may load 20 Ft. lengths of 5" diameter rounds and advance them against a stop held in a turret position.
 
Last edited:

hman

Active User
H-M Platinum Supporter ($50)
Joined
Feb 17, 2013
Messages
1,749
Likes
1,364
#8
That is one very nasty looking snake of a "chip." Be careful out there!

[Hill Street Blues]
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#9
That is one very nasty looking snake of a "chip." Be careful out there!

[Hill Street Blues]
They were out to get me today, after 30 years of killing metals Chipnet has become sentient and is fighting back, the outcome is uncertain.
 

RWanke

Active Member
Registered
Joined
Aug 23, 2017
Messages
107
Likes
118
#10
On the positive side it's a good sign of a really nicely sharpened drill bit. :clapping:
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#12
Not to mention good perfect feed and speed...
Thanks
No magic here, began at a conservative 35 SFM and a .004" per revolution feed rate then bumped it up to 50 SFM at .008 IPR, it seemed happy there.
The consistent chip is a result of the constant feed rate which would be difficult to achieve from a lathe tail stock by hand, if not impossible, I am pretty good at watching chip development when drilling by hand but can never duplicate a power feed.

Another consideration when using such a powerful machine is that if you make a mistake and the tool fails the machine will not stop, it will easily explode a 2" diameter twist drill, you do not want to be close when this happens. With any luck it will spin the part or push it through the chuck first.
Or shear the tang off of a 6 MT drill and let it spin, do not do this.
3" drill
 

Boswell

Hobby Machinist since 2010
H-M Platinum Supporter ($50)
Joined
Feb 27, 2014
Messages
619
Likes
278
#13
it will easily explode a 2" diameter twist drill,
Yikes. I thought the chip/snakes looks dangerous but thinking about a tool failure like that is down right scary.

Thanks for the pics
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#14
Bad luck, the second operation machine filled up with chips after 20 parts.


1/4" keyway broaching begins tomorrow, as much as I dislike keyseater machines it is preferable to pumping a push broach in a manual hydraulic press through 30 parts.
This is what they are for after all. 2 hours of set up for one key way is not cost effective unless it can't be pushed.
2 hours of set up for 30 holes is far better.

Did I mention that I hate chips in every possible way?
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#15
Yikes. I thought the chip/snakes looks dangerous but thinking about a tool failure like that is down right scary.

Thanks for the pics
This is a machine built in the 50's or earlier, safety was not a major concern at the time.
How big of a tool would it take to stop a 25 hp spindle drive from spinning (-:
 

MrWhoopee

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Jan 20, 2018
Messages
387
Likes
248
#16
Did I mention that I hate chips in every possible way?
Hatred of chips is what motivates us to dedicate our lives to their removal from the usable parts they are concealing.

Too bad the turret feed can't provide for momentary pauses to break the chip.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#17
Drill chips are easy to handle just annoying to clean up.
The chips generated in a lathe turning/boring operation are a different animal especially if a blind bore. These can break tools and damage parts if they will not break, this is one of the reasons why there are so many different chip breaking designs on insert tooling.

1950 era machines do not peck drill, in the 60's tape machines began to appear so I assume that this sort of control began then, I would not know this because I am only 60 years old and it was well before my time.
 

jdedmon91

Active Member
Registered
Joined
Dec 29, 2017
Messages
286
Likes
574
#18
Drill chips are easy to handle just annoying to clean up.
The chips generated in a lathe turning/boring operation are a different animal especially if a blind bore. These can break tools and damage parts if they will not break, this is one of the reasons why there are so many different chip breaking designs on insert tooling.

1950 era machines do not peck drill, in the 60's tape machines began to appear so I assume that this sort of control began then, I would not know this because I am only 60 years old and it was well before my time.
Well I’m older than you and to peck drill in the early days of CNC tool lots of lines of program. Because you program a depth back it out then start again.

I ran a job for a while we had a 5 inch long by 1 inch bore. We used insert drills and drilled half way the drilled the other half in the second operation. Of course you had to change the inserts on a regular intervals or you would have a drill failure an expense proposition


Sent from my iPhone using Tapatalk
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#19
Today's lovely part, an off the shelf shaft coupling supplied by the customer which means that you only get one shot at doing it correctly, if you bore it wrong you will have to supply another on your own dime, I suspect that this half costs several hundred dollars.

It is a tapered bore with a 3/4" keyway (not shown) the stock part has a 1 3/4" rough hole through it.
A 6 Deg. included taper 2.925/2.937" long. I had no drawings only a sample part, it is difficult to easily measure a tapered bore accurately so I first made a plug gauge that fit the sample.

Once you know the diameter of either end and the length simple math will yield the diameter of the other end, in this case 3.250" start diameter.
The tangent of 6 Deg. is .1051"
.1051" X the length of 2.930 is .307
The large diameter of 3.25" - .307" = 2.943" over a length of 2.930"

I am doing this in a 30 year old CNC lathe so only have to input a start diameter at a known position and an end diameter at a known distance from the start.

If you need to generate a taper that is not dead nuts accurate in a manual lathe a dial indicator in the toolpost moved a fixed distance with the compound slide will get you in the ballpark. Do not do so if generating machine spindle tapers.

Part drawing


Part
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#20
Small parts for the next few days, 3/8 seamless SS pipe turned to .625 +-.005, a 9/16-32 thread on one end .500 long.
A .518 diameter .375 long non threaded feature on the other end reamed .478 thru the 1.625 length, the OD, threading, rough drilling and parting to length will be done in a small NC lathe, the reaming will be done in a Hardinge turret lathe because it is much faster.
105 parts, or at this point 110 parts after tweaking the program today, pipe is an inexpensive material and I only require 17 feet, we have 20 feet of material, I can make many bad parts while working up to maximum speed.

They look like so


I snuck up on the Pitch diameter, I measured it over wires. The PD over .024 wires should be .584", this one is .582, thus a bit small, in the scrap it goes
The next several were spot on after subtracting .001 from the thread depth. Another 100 parts and I am done.
This should be on Thursday (-:
 
Last edited:

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#21
Excellent finish on the part aside from the threads,

this is what often happens when the threading tool crests when the PD is too small, it creates a sharp edge at the crest of the V, this often leaves a nasty burr, do not do this with a single point threading tool.
A full form insert will reduce this but it is unlikely that many hobbyists will buy or grind a full form tool.
The thread PD on this one is way too small, the following part threads look excellent, almost like I know what I am doing.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#22
Bloody hell, I just bought a new mag base indicator holder, I was looking for a long reach holder with a very strong magnet base as I will use it on a 24 X 100 lathe.

It arrived today, it is WAY larger then I had anticipated. This is with a 3" dial drop indicator. I bought the arm and base without an indicator as I have several.
This is a commonly available sized base in the foreground as a size reference.
It looked way smaller in the pictures, one of the advantages of an actual physical store is that one may see it in scale. It is reasonably well made so I am keeping it.
 
Last edited:

Boswell

Hobby Machinist since 2010
H-M Platinum Supporter ($50)
Joined
Feb 27, 2014
Messages
619
Likes
278
#23
It looked way smaller in the pictures, one of the advantages
I have struggled with learning this lesson of online purchasing. "Don't trust pictures for scale, always check the measurements" One of these days, I'll get it. (I hope sooner than later).
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#24
I have struggled with learning this lesson of online purchasing. "Don't trust pictures for scale, always check the measurements" One of these days, I'll get it. (I hope sooner than later).
Fortunately it is exactly what I was looking for but far more robust then I was expecting for $170.00 https://www.amazon.com/gp/product/B002NEPEXO/ref=oh_aui_detailpage_o01_s00?ie=UTF8&psc=1
We shall see how it holds up after a year of use in a busy job shop, it appears very well made however. The fussy little indicator holder on the end is not likely to live through the next year I suspect, there are indicator holders that I prefer over this type that are easily added via a threaded hole on the end.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#25
Interesting problem that had me scratching the old head for a few hours on this part.

The first order of operations was leave just enough out of the chuck in order to turn the large diameter past the un-threaded end, face then turn the OD's including the thread undercut.

Thread 9/16-32 then drill 15/32" (.469") from the nominal .420" ID of 3/8 NPT pipe. I measured the thread PD over wires.
Finished part, the wall thickness is .025" under the thread.




This worked well for 40 parts or so then the PD began to grow, this was caused by the drill becoming dull and deforming the tube. Normally I will do every roughing operation before any finish operations but figured that drilling .024" per side is almost finishing, but I was wrong.

Drilled first then did everything else and the next 65 parts ran flawlessly, live and learn.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#26
My venerable Mitutoyo indicator failed after 23 years of use, I bought a new B&S Interapid last week.
This will last beyond my limited life span I suspect.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#27
One easy job today, 6061 aluminum ring water jet cut from 1 3/8" plate stock, the flange OD is 14 1/2" X 1/4" long, the smaller OD is 13 1/2" X 1" long, the bore is 13" leaving a 1/4" wall.

This became a problem once the part became thin, the part was held in a 3-Jaw chuck with soft jaws, there is considerable unsupported distance between the jaws, it began to chatter in the area between the jaws. I suspect that a few here have experienced this with thin parts.

Until it became a game of cat and mouse between speed and chatter I could have at it.
14"+ diameter, 450 SFM cut speed (125 RPM's), .008 IPR feed and a .050" DOC using a CCMT negative rake insert with a positive rake chip breaker geometry.

Roughing aluminum with stable work holding should look like this, chips not coils, springy coiled chips will drive you mad over time.
This is a manual lathe.



I did produce some annoying stringy chips when finishing due the reduced speed and feeds required to stop the chatter.
Turned out well however, with set up included about 5 hours.
 
Last edited:

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#28
Tomorrow morning I have to do something that I have never done before.
Pick up an existing 1 1/4-7 thread on a CNC lathe, have not the faintest clue how to do so on this machine.
Anyone with hints (-:
Jim Dawson?
 

e189552

Newbie
Registered
Joined
Feb 25, 2017
Messages
12
Likes
18
#29
We would use the tool offsets.
Back the tool up in X a comfortable amount and run the thread routine.
We would carefully “eyeball” the Z position relative to the thread flank and adjust the Z tool offset.
Apply dykem layout fluid or even a permanent marker when you get really close to see which thread flank you contact first.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
489
Likes
317
#30
It went very well adjusting the Z offset and eyeballing the tool when it got close but it kept moving to the right. I then remembered that this control has an approach angle parameter in the thread cycle and someone had set the default value to 29 Deg. Once I set it to 0 it was quite easy to pick up the thread, it just scraped off some of the dykem then finished the additional 1/2" of thread on gauge.

I use a 0 Deg. approach angle when threading on a manual lathe so didn't consider this until doing a bit of head scratching.
 
[6]
[5] [7]
Top