# Hard turning, finishing the part.



## P. Waller (Sep 20, 2018)

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 (Sep 20, 2018)

Looks like fun, how about that keyway?


----------



## P. Waller (Sep 20, 2018)

MrWhoopee said:


> 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 (Sep 21, 2018)

You sure that not a CBN insert. I never seen Cermet coated just CBN. 


Sent from my iPhone using Tapatalk


----------



## P. Waller (Sep 21, 2018)

jdedmon91 said:


> 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 (Sep 21, 2018)

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 (Sep 22, 2018)

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.


----------



## hman (Sep 22, 2018)

That is one very nasty looking snake of a "chip."  Be careful out there! 

[Hill Street Blues]


----------



## P. Waller (Sep 22, 2018)

hman said:


> 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 (Sep 22, 2018)

On the positive side it's a good sign of a really nicely sharpened drill bit.


----------



## dulltool17 (Sep 22, 2018)

RWanke said:


> On the positive side it's a good sign of a really nicely sharpened drill bit.



Not to mention good perfect feed and speed...


----------



## P. Waller (Sep 22, 2018)

dulltool17 said:


> 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 (Sep 22, 2018)

P. Waller said:


> 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 (Sep 24, 2018)

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 (Sep 26, 2018)

Boswell said:


> 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 (Sep 28, 2018)

P. Waller said:


> 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 (Sep 28, 2018)

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 (Sep 28, 2018)

P. Waller said:


> 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 (Sep 29, 2018)

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 (Oct 1, 2018)

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 (-:


----------



## P. Waller (Oct 1, 2018)

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 (Oct 4, 2018)

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.


----------



## Boswell (Oct 4, 2018)

P. Waller said:


> 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 (Oct 4, 2018)

Boswell said:


> 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 (Oct 5, 2018)

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 (Oct 10, 2018)

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 (Oct 11, 2018)

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.


----------



## P. Waller (Oct 11, 2018)

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 (Oct 11, 2018)

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 (Oct 12, 2018)

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.


----------



## P. Waller (Oct 17, 2018)

Had to do some parts today using my second least favorite lathe operation.

Knurling.

3 1/8 Dia. steel tubes, the knurl is 22 5/8" long and 12 TPI. X .015" depth.

Did use a clamp knurling tool. Eaglerock.
Did not skim the OD to achieve some multiple of 12 TPI circumference as many youtube videos recommend.
Did use about as much coolant as I could throw at it, one nozzle per wheel, this is important.
80 Rpm's, .008" feed per revolution.

I used their (Eaglerock) recommended methods for a manual lathe.
Set tool X axis, center of the wheels at the center of the spindle.
Run the tool to center with the spindle stopped, turn the adjustment until the wheels touch the part then crank in the wheels to full depth.
Engage feed then start spindle.
This is not a full depth knurl, the top has a flat per the drawing/sample.
They get hard chromed afterwards.

Worked a charm for the most part, had to do a bit of fussy adjusting on the first part but the following ones ran rather well. 3 more to run tomorrow.


----------



## Boswell (Oct 17, 2018)

P. Waller said:


> Had to do some parts today using my second least favorite lathe operation.



I appreciate seeing your posts about "a day in the life of a working machinist"  keep them coming !


----------



## P. Waller (Oct 17, 2018)

Thank you
It is not fast however, 80 Rpm's X .008" feed is .64" per minute, 22.625" / .64 IPM is 35+ minutes per part just for the spindle time.

I have ran knurls much faster in the past but common knurling tools are HSS wheels running on hardened tool steel pins, I have had them seize together in the past when used to fast, this does not work well as you can imagine.


----------



## P. Waller (Oct 22, 2018)

Dovetail O-ring  groove. A nasty job on a large part in a manual machine.
The dovetail keeps the O-ring from falling out of the groove when the part is inverted. I can understand the rational behind this but they can be a bugger to produce. 11 3/4 OD X .120 deep plunge in 304 SS then decrease the diameter in the groove by about .050" per side to produce the dovetail with a large radius.

How easy do you think this carbide insert would be to break? If your guess is very easy you win.






It looks like this on the drawing minus the radii,depth, width and tolerance dimensions, these are all on a second tabulated data sheet for each O-ring cross section.
I am doing this on a 24" X 100" manual lathe by very gently bumping the carriage wheel for infeed in Z to produce the initial groove to depth, the carriage, compound and toolpost weigh well more then 500 Lbs on this machine including it's own 3 phase motor that will rapid each axis close to where you want it, this is an excellent feature as one will quickly grow weary of hand cranking a large carriage 50 or 60" up and down the bed (-:


----------



## P. Waller (Nov 2, 2018)

Long small diameter parts today, 125 parts in total.
3/8" 1018 CRS round bars.
They finish at 33.75" length with a reduced diameter and a retaining ring groove on each end, the tolerances are rather loose.
+- .030" on the length, +- .005" on the diameters and the groove width is .039" +.000 -.005" with a minor diameter of +-.005"

This was done in a CNC Bridgeport lathe, the parts were a few inches longer then the spindle stop so I made an extension for it that is extremely simple.




The stock was cut about .200" long so I faced one end then turned and grooved, turned with a VCMT insert and grooved with a Kennametal Topnotch .029" wide grooving insert tool. The finish was excellent considering the material.
A very conservative 1000 Rpm's with .020" DOC and .012" feed for roughing, .004" DOC and .004" feed for finishing.
Short end



Long end




Part


----------



## P. Waller (Nov 20, 2018)

Cold rolled 1045 steel, 6 1/2" nominal stock diameter 36 1/4" long.
The part finishes at 36 1/8" +- .030"

We do not have a lathe that is 6 1/2" through the spindle so the steady is employed.
Place part in chuck and push a flat center drilled plate against the end and push it against the chuck with the tail stock, indicate this end and knock in as close as needed.
Turn a band as wide as required for the steady rollers/fingers, set the steady and face the first end and drill a center in it.

Put a live center in the end and turn the OD as close to the steady as possible, in this photo the first half is finished and I am facing and center drilling the other end using the band for the steady, the finish OD is 6.437 +.000 -.005.




I have flipped the part and will now turn the second 1/2, this will require a cats head for the steady because running the rollers on the finished surface will damage it, I have also placed aluminum flats between the chuck jaws and finished surface. Steel banding is used under the set screws inside the catshead to protect the surface. This requires much set up time.
The finish is excellent considering the material, turned the OD at 400 sfm at .008" IPR feedrate using a TPG 321 triangular TIN coated insert.
6 7/16" diameter cut at 400 SFM is 237 RPMs.
The C-Clamps and sheetmetal are a movable guard to keep the chips away from the rollers on the steady, nothing will ruin your day faster then rolling a large chip in a steady, a steady with non rolling elements does not have this problem, score 1 for 1850 era technology


----------



## P. Waller (Nov 21, 2018)

Indicate the part after flipping it, I use 2 indicators for this 1 for the axial runout of the cats head and one for the radial runout of the part.
This is a very time consuming process.




The finish turning looks like so. This method will not likely work for many hobbyists because it will leave a visible line at the center when turning from both ends, in this case it is well within the +.000 -.005" on the drawing.
A 1 tenth difference in diameter will leave a visible artifact on the part.

I am beginning to like this enormous noga indicator holder that I bought several months ago.


----------



## P. Waller (Dec 20, 2018)

Just made it, 25" diameter X 1" thick disk in 304 SS, the ID and OD were first milled to size because the 25 1/2" diameter rough burnout would not clear the ways with the gap in place. Removing the gap causes all manner of tooling problems on this machine.
It cleared by a healthy 1/4"

I believe that way oil stained this machine (-:



Now to face it to 3/4" thick with a 250 surface finish on both sides then cut an extremely annoying dovetail O-ring groove at 13 3/16" minor diameter in one face, for anyone that has never done a face dovetail groove in a large machine it is tedious at best, it looks like so. Feeding such a small carbide insert form tool with a 500+ Lb carriage machine is difficult, I have broken many inserts doing this operation, fortunately the inserts are so easily broken that they do not ruin the part.



Using one of these toolshttp://www.thinbit.com/products/face-grooving/index.php


----------



## Boswell (Dec 20, 2018)

those face-grooving bits do look fragile. out of curiosity. to get the underhang, I guess you plunge into the face to the required depth then move in to create the underhang?


----------



## P. Waller (Dec 20, 2018)

Boswell said:


> those face-grooving bits do look fragile. out of curiosity. to get the underhang, I guess you plunge into the face to the required depth then move in to create the underhang?


Exactly.
This is my least favorite lathe operation on a large machine using a very small tool. I will take some pictures tomorrow morning.
If the first part goes well of course, if not no pictures means that it did not happen.
Successfully


----------



## MarkM (Dec 21, 2018)

Thanks for posting.  Enjoy seeing shop operations performed.


----------



## P. Waller (Dec 22, 2018)

The facing went as as well as expected, the face grooving not so well. This 25" X 100" lathe will not power feed slow enough for this tool so it must be done by hand. It is difficult to keep the tool loaded enough that it will not chatter at the bottom.


----------



## Tozguy (Dec 22, 2018)

P. Waller said:


> I believe that way oil stained this machine (-:



Are you referring to the rust coloured stain on the ways?
If you would elaborate on this I would appreciate it. Seems like the last thing I would expect to happen.


----------



## P. Waller (Dec 22, 2018)

Tozguy said:


> Are you referring to the rust coloured stain on the ways?
> If you would elaborate on this I would appreciate it. Seems like the last thing I would expect to happen.


This is a joke, several weeks ago someone posted a thread on this forum about waylube staining their machine ways, I advised him that the best way to avoid this is to have 2 machines.
One to use and one to admire, I got mail for that comment.
To answer your question lubrication products and use will discolor the metal surfaces over time, this is inevetable, the machine pictured above is nearly 20 years old and has been in a working job shop since new, rode hard and put away wet so to speak.

Also the facing operations went well, the face grooving took forever.
Faced the second part today, reasonable finish with just a wee bit of chatter marks between the jaws as so often happens.
40 RPMs(260 FPM) at the OD, .050" DOC, .008" Feed rate using a CNMT insert for roughing.
Used a TPG 431 insert for finishing at 28 RPMs, .015" DOC and .006" feed for finishing.

.006" Feed Per Minute X 28 RPMs is .168" per minute X 6" length of cut = 1 hour of spindle time for the finish pass alone.




This sort of thing will drive a hobbyist chasing tenths absolutely bonkers, you will never get a 25" part that has had its OD milled by circular interpolation to have 0 run out. The mill used for this part did an excellent job of it however considering that it was done in halfs, a 24" travel Y axis machine will not mill a 25" circle (-:


----------



## e189552 (Dec 22, 2018)

Back in the day, we cut similar parts for the oilfield.
Supported the part with bolts and t-nuts.
Parts had to be flat within .005”
Looked somewhat like what you have there.
Toughest part was the sealing faces, full radius about .500”
Think that your part had a thicker ring around the OD.
Usually started out as torch/plasma cut plate, it was a bear to get through.


----------



## P. Waller (Dec 22, 2018)

They were to be water jet cut, this did not happen unless a water jet can turn the edges of 1" stainless plate blue.


----------

