info on turning tols

Hi All,
I have a part 125mm long (5")and it requires turning to a shoulder
of 5mm(3/16 ish).Dia is 19mm (3/4" ish)the tolerance is 0.01 (0.0004)total .zero deviation in 304 st st.
We would buy a machine to make the parts. Every machine maker gives us "a no problem"
But I have listened to crap before.

Please can I have your views.

Thanks GTW

The very best machine in the world can have trouble making that part.
Operator skill and quality of holding device are keys to success,. and yes the machine.
Good that at 3/4 x 5 it is a stout part and .0004 is not that chose if +-.
.0004 TiR (total) is considered very close and on some machines may need be done between centers, or have very good holding device.
Parted off would make it easier. Out of a collet or chuck the holder would have to run <.0002 if .0004 TIR.

For close grinding I have clocked a spindle to find perhaps .0001 error and a put a paint spot at the high place..Then with finding the collet .0002(very good for most collets) I match high and low to get closer to zero..

If you can use a center or false center than this part is easy. If not you might check out roller box style tools, though not sure if you can get to a square shoulder with them.

I don't know boo about 304 but a, "long, skinny part with tight OD tolerance" is where sliding headstock (i.e. "Swiss") machines shine. Think Citizen, Tsugami, Star (in that order.). The cutting generally takes place 1mm out in "Z" from the guide bushing support so it is very rigid. It's a heavy cut but a positive insert would help keep the load and tool deflection under control. I regularly turn down 4340 from .875 to .470 and hold +/- .001" with non-ground stock using a DNMG. Good luck!

Nerdlinger said:

I don't know boo about 304 but a, "long, skinny part with tight OD tolerance" is where sliding headstock (i.e. "Swiss") machines shine. Think Citizen, Tsugami, Star (in that order.). The cutting generally takes place 1mm out in "Z" from the guide bushing support so it is very rigid. It's a heavy cut but a positive insert would help keep the load and tool deflection under control. I regularly turn down 4340 from .875 to .470 and hold +/- .001" with non-ground stock using a DNMG. Good luck!

Click to expand...

This. And if it's not an issue for them, ask them to provide you with sample parts and a quote to have the machine dropped on your floor turn key.

Turning tol's

AARONT said:

This. And if it's not an issue for them, ask them to provide you with sample parts and a quote to have the machine dropped on your floor turn key.

Click to expand...

Sliders are great but the tol. is .0004 total. and the oval problems using a guide bush
can put you out of that let alone 120mm + lengths. Roller boxing again is a great thing but
the tol. is to close over the distance (I set them for years).

I agree we would not buy a machine without a trial
run.

Centerless form grinding?

Hi TeachMePlease,
This is an option we would consider. Also a hard turning machine.
We would also do this internally and buy to suit our needs.

I am leaning to this direction for production / quality consistancy

Gerrythewelshman said:

Sliders are great but the tol. is .0004 total. and the oval problems using a guide bush
can put you out of that let alone 120mm + lengths.

Click to expand...

I do not work in the world if +\- .0002” but I know Star and Tsugami (maybe Citizen, too?) offer optional pneumatic guide bushings that always maintain even pressure around the bar. This helps with varying bar diameters and would definitely help with ovality but I do NOT know if +\- .0002” is reasonable. It wouldn’t surprise me, though!

Swiss will be the way to go. Look for something with a second gang tool post or turret so you can pinch-turn. You'll basically have the rougher & finisher engaged in the cut at the same time.

Well, you didn't state what the bar stock size is, so hard to tell how well the Swiss is suited, but I doo agree that if you chose the Swiss, you would want to git the pneumatic guide bushing. (if trying to produce finished part)

While it can be done within reason on either fixed or sliding headstock, if I was planning on making umpteen of them every day - as you seem to be preparing for, I would lean towards roughing out on a lathe and finish plunge grind on centerless to finish. You will hold your tol way better on the grinder and it's a quick opp. Quicker than that final cut on the lathe.

If you blank on a Swiss you don't have the center in the end, nor the time to produce it.
The grinder will take the sub collet marks off too.



edit1:

Also note that you will get 2 less parts per 12' bar on the Swiss (if running a guide bushing) and on big diameter SS - that can add up quickly.
Likely about the same/bar if running a short loader tho.

edit2:

If you went Swiss, you would want to make sure that it is a machine that can pinch turn. (Again - depending on bar size)
That means twin turret usually, so ends up not being a very cheap machine.


edit3:

Also note that 304 has a bad reputation for consistancy.
The grinder will bring consistancy to the table.


Not sure what "zero deviation" means?



-------------------------

Think Snow Eh!
Ox

Some Swiss machines are available with tooling next to the sub spindle, intended to be used for drilling deep holes in the part on the main spindle side, but I bet you could put a boring bar in there and use it to pinch turn. It’s still a $200,000 machine if you need a magazine barfeed.

Nerdlinger said:

Some Swiss machines are available with tooling next to the sub spindle, intended to be used for drilling deep holes in the part on the main spindle side, but I bet you could put a boring bar in there and use it to pinch turn. It’s still a $200,000 machine if you need a magazine barfeed.

Click to expand...

For that, you could use one of these: DS-ACH Toolholders - Unique Tooling - NTK Cutting Tools (The Americas)

The only downside is the 5+" overhang you'd need to clear the finished part.

I'm a big Swiss guy, it's more or less all I do, all day, every day... and given the time and resources, I'm sure I could make this work, reliably...

But if looking for a turnkey solution, with minimal fuss and adjustment, with a dedicated machine... I think centerless grinding is the way to go for these parts/tolerances.

How many do you need? Might be easier to job it out to someone that already knows how to do it.

Maybe I am reading this wrong but asumming the shoulder is on the o.d.
if its an I.d. shoulder Ie step with a 3/16 bore 5" long + or -.0002

Remember the tools dont move on a swiss in the Z direction . The stock does.

I dont think a swiss will work for O.D. shoulder reason being is it goes from a 3/16 dia to shoulder of 3/4 dia. somewhere in 5" or its longer
unless you can take that whole cut in one shot, its going to fall out of the bushing after your 1st cut going for the other cuts.
if you can find a tool to make the entire cut from 3/4" to 3/16 dia, it would be possible if and only if had a sub sindle that could grab the front of the part 3/16 dia and move back while feeding ( TeachMePlease will understand) Typically a bushing is about .5-1" long of actual dia.
The stock would have to be ground to the biggest size in which case is 3/4"

and depending what fillet if required between the shoulder face and the centerless might not be an option, o.d. grinding might be the only option

If the guy had a mark up print it would be easier to tell. I dotn think he understands machining very well, his explanation is very vague.

I think we ain't all picturing the same part. Is it 19mm material being turned to 5mm. Or Bigger material being turned down to 19mm and the shoulder is 5mm thick?

If its turned to a 19mm dia, that's easy enough.

SND said:

I think we ain't all picturing the same part. Is it 19mm material being turned to 5mm. Or Bigger material being turned down to 19mm and the shoulder is 5mm thick?

If its turned to a 19mm dia, that's easy enough.

Click to expand...

yeah thats what I mean I cant figure out what he wants exactly because he says shoulder.

Gerrythewelshman said:

Hi All,
I have a part 125mm long (5")and it requires turning to a shoulder
of 5mm(3/16 ish).Dia is 19mm (3/4" ish)the tolerance is 0.01 (0.0004)total .zero deviation in 304 st st.
We would buy a machine to make the parts. Every machine maker gives us "a no problem"
But I have listened to crap before.
if he is just turning 19mm to 3/16 rough it down and centerless grind it its a simple job then. a screw machine would be out of the question those do to length and bushing like explained above) any lathe would work fine otherwise.


Please can I have your views.

Thanks GTW

Click to expand...