What's new
What's new

Cuttin' threads away from the chuck to a shoulder...................

david n

Diamond
Joined
Apr 13, 2007
Location
Pillager, MN
I have a part I'm looking to do in one OP...............I need to cut a thread away from the chuck to a shoulder and quite frankly I don't ever remember doing such a thing:scratchchin:.............I can't use a lay down style insert due to the shoulder, a top notch style insert should work. My quandary is do I need a LH toolholder and need to run in M04? G code? The Lynx has Fanuc Oi control.......................This should be easy, but my brain is tired and drawing a blank...................TIA
 
Flip your tool upside down and go left to right? I've done that many times on the lathe, but it's been YEARS.
 
It's been a while, but I think if you run your "normal" tool orientation from left to right you get a LH thread, so maybe flipping the tool and running reverse will do it...??
 
For a right hand thread starting at chuck and feeding towards tail stock you need a Left hand tool (insert facing up) and spindle rotation CCW.
 
If you run you "normal" tool from the undercut toward the chuck you will get a right hand thread.
Upside down, M04 from chuck toward undercut will also give a right hand thread.
 
Not sure how close you need to get to the shoulder, but check out Carmex slim throat holders. The part number is SER1000M16VS, but it's kinda hard to find a website that has a picture.
 

Attachments

  • SERVS_729202b4-1d7c-43a1-8c2f-af137a5c8436_2048x2048.jpg
    SERVS_729202b4-1d7c-43a1-8c2f-af137a5c8436_2048x2048.jpg
    68.6 KB · Views: 165
Not knowing what the part looks like... Can you run the thread like normal, then use a groove/turn tool behind the thread or whatever?

https://www.iscar.com/ita/MainPage.aspx?sid=1

I'm with Mike on threading toward the shoulder and then making a relief cut.

Program up just shy of the shoulder and make your fade-out as short as absolutely possible. Keep the RPM down so the X axis can pull out in time.

Make a pass or two and then program it to go .05 farther in Z. Once it just barely kisses the shoulder you back off a touch.......;)
 
A trick to measure threads behind a shoulder is to measure the approximate pitch diameter with the thin points of calipers.

I use a reference thread to find what “measurement” the calipers give, then look for this same measurement on your back threads.

(Easier and quicker than thread wires and mics!)

Of course as with any measurement with calipers, you gotta have a consistent feel for the correct measuring pressure....a little wiggle and easy thumb pressure works for me.

ToolCat
 
Here's what I got goin' on....................I wanna cut RHT away from the chuck to the 1.220"Ø shoulder................

IMG_0546.jpg
 
Ass_u_ming you are holding on to the shoulder or behind it, who sez you have to make life hard on yourself? ;)

I would thread toward the shoulder, you have a nice relief there already......:confused:

Shoulder/relief is not of concern.................original question is threading a RHT away from the chuck..................sounds like a LH toolholder running CCW......................
 
Shoulder/relief is not of concern.................original question is threading a RHT away from the chuck..................sounds like a LH toolholder running CCW......................

Not to challenge you, but I'm wondering why?

Your shoulder isn't that large in relation to the thread..........why doesn't it work to thread it toward the chuck? :confused:

I'm prolly missing something really obvious.....:dunce:
 
Not to challenge you, but I'm wondering why?

Your shoulder isn't that large in relation to the thread..........why doesn't it work to thread it toward the chuck? :confused:

I'm prolly missing something really obvious.....:dunce:

Could do it I guess, acceleration distance could come into play, and you could
get some wonky threads at the end.

The diameter in that relief could also pose a problem with the nose of your threading tool
slamming into it. (thread pal time). Looks like if you had the max nose radius allowed,
you could clear it.
 
Not to challenge you, but I'm wondering why?

Your shoulder isn't that large in relation to the thread..........why doesn't it work to thread it toward the chuck? :confused:

I'm prolly missing something really obvious.....:dunce:

You're missing the OP. He wants to build the part in a single operation.

If you can run a M3 and Turn away from the Chuck, it will generate a Left Hand Thread.
 
Here's what I got goin' on....................I wanna cut RHT away from the chuck to the 1.220"Ø shoulder................

View attachment 292657

I have ran a lot of parts this way from barstock.

To "back thread" I use the cut-off tool to make a groove at the end of the part, where it cuts off later. This groove's width/depth is sized to allow room for a narrow threading tool to start. I chamfer the thread diameter using the cut-off tool as well.

For the threading tools, I like to use Iscar stuff for this, the long-narrow double-ended carbide threading inserts...either 3, 4, or 5mm wide.

After threading, I use the cut-off tool again to clip the corner of the thread before cutting off - getting rid of the little sharp starting thread burr.

If my thread-start groove had to be wider that the cut-off tool, I would just face off the waste at the next part after bar pullout. In this case, you're lucky, you can make the thread-start groove as wide as you need!

On edit: added info, and why are they specifying a rather close tolerance for the thread relief at the shoulder??

ToolCat
 
Last edited:
On edit: added info, and why are they specifying a rather close tolerance for the thread relief at the shoulder??

ToolCat

Don't you know that only really good engineers specify really tight tolerances?

"Bad" engineers specify loose tolerances.

Probably a piece of ground support equipment. I'm working on one nows. Stupid
thread relief dimensions on the nuts on each end, angles, radii (I want to type radiuses),
diameters. Just retarded, but there are a bunch of other places on the shaft that need
a corner relief. One is just a simple groove. Some are .007 radiuses (take that Radii!!!)
to a square corner, and some others are 13 degree reliefs going into a .015±.003R corner and
a moderate tolerance on the diameter. And then there are places the shaft is necked down
for no reason and the tolerances on the R's in and out of that are really tight, for no
F'n reason.

Somebody's nephew needed a job. And they can't trust them to do critical work, so they put them
on ground support. And they "OVER" engineer it.

I've done ag processing shafts that do more, and have more features, and "the print" sketch, had 10% of
the dimensions on it. This bearing has to go to the shoulder. This plate has to go to that shoulder,
this nut has to tighten on this other thing. This sprocket has to go to this shoulder, this gear has
to go to the other shoulder.

Thread(shoulder) reliefs are the most over toleranced bunch of shit I've ever seen in my life.

To be a "Good" engineer, how do you make the print look like you are earning your money on a simple
shaft. You add a ton of dimensions and a ton of detail and section views, and the only place you
can really do that is in the corners.

I'm looking at this print, and I just want to puke, I hate these F'n things. I'm not doing these
anymore, its just not worth it. I tried to price myself out of it, I really did, and its still
not worth it.
 








 
Back
Top