What's new
What's new

Requesting tips to speed up production of this simple part on manual lathe.

stoneaxe

Stainless
Joined
Mar 2, 2010
Location
pacific northwest
Occasionally we need to make small quantities of these spacers -maybe 10 to 100 per year.
My purpose in asking this is not simply to make parts faster on this job, but to learn - I realize this is bog standard lathe work but you all have a lot of years in- there are likely simple things that would help, that I have no idea about.

Part- spacer,
Aluminum, 6061, 1.00" long, .550" dia.
Step on one end .420" dia. x .135" long.
7/32" hole bored through.
everything +- .005" -not fine work - but I would like to hold it to .001" +- because that is how I will get better.:)
DSCF1518.JPG
1340 Taiwan manual lathe with DRO. 1300 rpm face and turn, 370 rpm cut off. Aluminum specific carbide insets, HHS on the parting tool. 3 jaw chuck.
Sequence
Chuck 9/16" bar, about 1 1/4"extension, face, then zero z axis and set x axis number.
Turn to diameter, then turn reduced dia.
Bore hole with tailstock mounted drill. I use a screw machine short drill. No center drill. Takes a bit as the hole is deep and the chips are hard to clear after half an inch or so. using WD40 as lube.
Drop on the cutoff tool and part off - the part is 1.000", cut off blade is .094", offset from facing tool is .076", so I dial in 1.170 and part off.
Then re-chuck the stock, face and re-zero the z axis and repeat operations.
The X axis stays the same, of course.
After they are all cut, the part is flipped and the cut off end is chamfered slightly.

I would love to use a stop on the reduced diameter length, but do not know how to set one up as it would interfere with the full diameter turning. Some sort of flip stop maybe?

Also, it would be handy to chuck up the stock to a preset length, instead of having to face and re-zero to that face every time. What to butt the stock to? The facing tool set to +.010" on the DRO? Then back to zero and face?

And maybe use a triangle (like a threading insert) to start the cut off , then use the parting tool, so the chamfer would already be cut.

As far as accuracy, the length on these few parts has about .005 variance, due mostly to my initial idea of bumping the parting blade against the face of the stock, re-zeroing and then parting off. I think that .005" was flex in the parting blade when it was run up against the stock. So I switched to calculating the off set between the turning tool and the cut off tool and leaving the DRO zero alone.
The length of the reduced diameter is also more varied than I like, I was hand feeding it with no stop.
Thanks, stoneaxe.
 
You could do toolpost mounted drilling instead of using the tailstock, much faster to clear chips but it is another tool change, rear mounted parting off tool to save a tool change, using spindle reverse if you have to or an upside down tool if you can.

I would use carbide tooling to part off, probably could avoid a speed change that way.
 
Classic job for a British style ratchet indexing 4-way tool post.

If you have enough stations on your QC post look into sorting a ratchet base. +1 on the tool post drill idea but you need some form of cross-slide stop to set the drill to centre. If your lathe has a long enough cross slide to take a rear tool post, fit holes if need be, thats probably the place for the drill.

Chucking stop could go in one of those tailstock turrets doobies. You will soon get used to it pointing up, or up and back whilst doing the job. Mine is professional version good for decently heavy work and big enough to get in the way. Cheap hobby one, in a step up adapter if need be, would fine to carry a stop as no real forces involved.

As you are using carbide tooling and a drill there is no need to worry about height adjustment so why not just make a fixed size four way with an MT socket on one face for the drill and be done with it. Pawl and gear for the ratchet. Will only go one way but one is enough. If your drill is in the tool post remember to lock the compound so it doesn't get off centre. But on a job like this who needs a compound anyway. Just sit your home brew 4 way on the cross slide with aspire to take up teh distance and hold the ratchet.

Clive
 
1300 rpm face and turn, 370 rpm cut off.

Why are you turning the spindle so slow? Why are you changing speed?

What to butt the stock to? The facing tool set to +.010" on the DRO? Then back to zero and face?

A ruler kind of thing with 1 line on it to measure from the nose of the jaws would probably be faster.

And maybe use a triangle (like a threading insert) to start the cut off , then use the parting tool, so the chamfer would already be cut.

Won't save time because you still have the ID chamfer. Use a D-bit to chamfer both ID and OD.

A carriage stop like this might help:
stop.png
 
For quantity 10 at a time, maybe I'm the weirdo, I'd chamfer the first end, cutoff a blank, wait until I had all ten blanks, set up a collet stop, face and turn the end with the reduced diameter, remove collet stop, spot all 10 for ID edge break, then drill all 10 through. I'd rather swap parts than tools for something like this.
 
Don't forget that you can over-drill (1.1") into the bar so the next part already has a bore to follow.

At 100 pieces a year, it's probably not worth a CNC but, a turning center would not only bang those out in no time but, you could chamfer all the edges in one profiling operation and even do the back chamfer with the parting tool. The only edge you wouldn't touch in the first op is the drill hole intersection to the parting plane. You'd have to hand deburr the one hole.
 
Get a collet system much faster as on the second op you can use a collet stop.
Can a ER- be set up with internal stops? Or is a 5-C better for this?
You could do toolpost mounted drilling instead of using the tailstock, much faster to clear chips but it is another tool change, rear mounted parting off tool to save a tool change, using spindle reverse if you have to or an upside down tool if you can.

I would use carbide tooling to part off, probably could avoid a speed change that way.
Why faster to clear chips? They are packing up in the bore, what does a power feed have to do with it? I am concerned about breaking off that little 7/32 bit in a 1" deep hole.
Why are you turning the spindle so slow? Why are you changing speed?
I was getting chatter at higher speeds- probably need more feed?
A ruler kind of thing with 1 line on it to measure from the nose of the jaws would probably be faster.



Won't save time because you still have the ID chamfer. Use a D-bit to chamfer both ID and OD.
THe stock was parting off with a burr around the hole, so I was using a center dril to get rid of the burr and chamfer the ID.
A carriage stop like this might help:
View attachment 440636
I like the idea, but how does one get the longest stop out of the way, so the shorter ones can be used?
Don't forget that you can over-drill (1.1") into the bar so the next part already has a bore to follow.
I tried this once on a series of parts and found over a few of them the drill drift compounded so the hole was off center.
At 100 pieces a year, it's probably not worth a CNC but, a turning center would not only bang those out in no time but, you could chamfer all the edges in one profiling operation and even do the back chamfer with the parting tool. The only edge you wouldn't touch in the first op is the drill hole intersection to the parting plane. You'd have to hand deburr the one hole.
There is a beat up old enco turret lathe near me for sale, one of those little Taiwan ones- maybe I should grab it.....
 
In the PM spirit of offering up useless information, these'd be perfect for a DSM-59.

If he came across one cheap, grab it. Here ...

Ahhh yes, super productive, makes my shoulder hurt just seeing a video of one :D
 
Can a ER- be set up with internal stops? Or is a 5-C better for this?

- 5C would be my pick - probably the easiest to find.
Why faster to clear chips? They are packing up in the bore, what does a power feed have to do with it? I am concerned about breaking off that little 7/32 bit in a 1" deep hole.

- It's way faster to crank the carriage handwheel left and right to clear chips than to crank the tailstock or to unlock-and-relock the tailstock. Powerfeed is a bonus for consistent cuts, though!

*on edit...drilling 7/32" an inch deep in 6061 is a piece of cake. You'd be more likely to make the drill wander from packed chips vs. breaking it off

I was getting chatter at higher speeds- probably need more feed?
- Might need more feed, or a sharper tool, or less stickout from the chuck (soon to be collet ;)). You can also run faster rippums with a collet chuck (less imbalance)
I tried this once on a series of parts and found over a few of them the drill drift compounded so the hole was off center.

- Yeah...you'll have that on these big jobs. I'd center-drill every part, then re-chuck them and drill through like Teach said
 
Don't forget that you can over-drill (1.1") into the bar so the next part already has a bore to follow.

<snippo>
I'd try that too, but be wary that a slightly bad drill grind could easily wander.
For the parting if you are using hss, change to cardide insert bar and push through at full speed.
Kerosine is cheaper than wd40 and gives a beautiful finish on alu.
 
A carriage stop like this might help:
View attachment 440636
I like the idea, but how does one get the longest stop out of the way, so the shorter ones can be used?


I'd say that one is on upside down. On mine the active stop is right at the bottom so the longer ones project over the saddle.
My pal Mike-the-Pilot has a Colchester with a factory stop arrangement on the tailstock side of the saddle. Basically a long tube with many tapped holes to fit blocks carrying short screws to act as the stops working against another block fixed to the bed. Only one I've ever seen but it works well.

Bed turret style capstans are nice but a lathe with a ratchet four way, cut-off tool carrier and a tailstock turret can give them a decent run for their money. Especially on jobs needing longitudinal turning.

Clive
 
  • Like
Reactions: pcd
In the PM spirit of offering up useless information, these'd be perfect for a DSM-59.

If he came across one cheap, grab it. Here ...

Or at least he could study the features and adapt some to the 1340.

Quick change tail stock tooling, turret tool post, indexable or flip stops, etc. Maybe even make a box turning tool for the OD features.

However, for repetitive manual jobs nothing beats a speed lathe which is what we used to call them.
 
I've not read the entire thread to see if this has been suggested but I'd look at the DRO and see it has the ability to store tool offsets. On mine you set the diameter using your first tool (T001) then all other tools are set relative to that one. I usually set the offsets as I go on the first part then after that it's just swapping out the tools in my quick change tool post and tabbing to the next offset on the DRO. If you can't do this then you may be able to use stored positions. It's not quite as good on the lathe but works in a similar way.

I run jobs like this in the manual from time to time when the CNC is busy and I'm standing around not doing anything productive. A part like this in the manual would be a single op - sequence would be:

Using OD turning tool, T001, face and turn OD to size. If you're not using some form of workstop for the stock set your Z0 on the DRO. If you are using a stop then you should only need to set it once then in future return to Z0 then face. There's a ruler type stop that's perfect for first op work - I can't remember what they're called so hopefully someone else can chime in. I couldn't get my hands on one over here in the UK so 3D printed one - it uses a 3D printed carriage that runs along a piece of stock aluminium angle.
Drill using tailstock (flood coolant preferable but due to high RPM's with alu usually just go in dry or with a bit of WD-40 as it's always on hand).
Switch to your parting / grooving tool and cut a groove at the back of the part close to the drill diameter but leaving a little material so you don't part it off. Use your DRO offset T002 (or whatever) to get the Z position right but leave a little facing allowance, maybe .2 mm or so to clean up later.
Switch to a 90 degree square insert in a 45 degree holder. Put chamfers on all OD edges - I usually just use the graduations on the hand wheels for this as only takes a few seconds.
Return back to your parting tool and set to finished Z. Feed in slowly and this will clean up the back side of the part and leave a much better finish than a typical part off finish. Part through all the way.

For the internal chamfers on simple jobs like this I'll use a single flute countersink tool mounted in a cordless drill set to slow and it should give nice consistent chamfer - just don't use too much force or it could dig in and when that happens it's hard to get it even.
 








 
Back
Top