• This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn more.
  • PLEASE: Read the FORUM RULES BEFORE registering!

4

Using the Cross Slide for Threading

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

ddickey

H-M Supporter - Premium Member
H-M Supporter-Premium Member
Joined
Apr 21, 2016
Messages
1,005
Likes
505
#1
I need to cut 1/2-20.
If I just used the cross slide what would the outcome look like?
I've read it's okay to use the cross slide on some fine threads.
Does 20tpi qualify?
 

benmychree

John York
H-M Supporter-Premium Member
Joined
Jun 7, 2013
Messages
998
Likes
565
#2
Why would you want to use only the cross slide, if in fact you have a compound rest; the result of using only the cross slide is that the tool cuts on both sides using this plunge cut method; what happens is that the two chip streams converge at the point, interfering with each other and causing galling in the cut and a very unpleasant looking finish on the flanks of the thread. An advantage to using the compound for feeding is that you zero the cross slide on every cut and do your successive cuts by feeding the compound in, with no numbers to memorize for each new cut. Some folks like to compute the distance the compound is fed in to size the thread, or use the figures on the "fish tail" thread gage; this may work in an perfect universe and with sharp vee threads, but if you use a flat on your threading tools, it does not. Best is a thread mike, and the tables published in machinist's handbooks, but for me, a thread ring gage or a nut that has had a tap run through it is all that is necessary to insure a good thread fit for most purposes.
Lastly, I think, no, 20tpi is not fine enough to plunge in straight, and personally, I would not recommend it for any threading.
 

shooter123456

Active Member
Active Member
Joined
Jan 20, 2016
Messages
218
Likes
238
#3
It will probably depend a lot on your lathe, the material you are cutting, and the tool you are using. If you are using a 2000 lb lathe with a razor sharp HSS tool to cut aluminum, you will probably get good results. If you have a 7x12 with a poorly ground HSS or the wrong kind of carbide trying to cut 4140 or 304 stainless, it will not go well.

I have gotten by just locking the compound and using the cross slide, but it tends to go better using the compound.
 

mikey

Active User
H-M Supporter-Premium Member
Joined
Dec 20, 2012
Messages
3,037
Likes
2,956
#4
Both ways work, in my experience. I cut clean threads on my Sherline lathe for years, including 20 tpi, with a straight in feed with the cross slide (it has no compound). I can do the same with the compound on my larger lathe; I agree with Benmychree but I do know that both ways work. I use sharp, accurately ground HSS tools and cut much finer threads than 20 tpi with no real issues. You do need to take very small cuts as you progress but you'll do that anyway.

This is an M8-1.25 thread in 1144 steel cut with the cross slide on a Sherline lathe. Other than wire brushing the debris off, it is just as it comes off the lathe.

IMG_4830.jpg
 

ddickey

H-M Supporter - Premium Member
H-M Supporter-Premium Member
Joined
Apr 21, 2016
Messages
1,005
Likes
505
#5
Nice looking thread there Mike.
I use a solid tool post and don't feel like setting it back up, that is really the only reason.
If I can get threads to like that only using the cross slide I'm tempted.
 

george wilson

Global Moderator
Staff member
H-M Supporter-Premium Member
Joined
Jul 26, 2011
Messages
3,486
Likes
749
#7
You can make nice threads. Just take small cuts. A really good old machinist I used to know applied the top surface of his threading tools to the round,front edge of a bench grinder,making the whole top surface of his threading tools give the chips someplace to go,rather than just possibly bunching up on the threading cutter. The grind was flat all the way across the threading tool,and concave as seen from the side view.
 

mikey

Active User
H-M Supporter-Premium Member
Joined
Dec 20, 2012
Messages
3,037
Likes
2,956
#9
Nice looking thread there Mike.
I use a solid tool post and don't feel like setting it back up, that is really the only reason.
If I can get threads to like that only using the cross slide I'm tempted.
As long as your tool is accurately ground and you can confirm that the tool is perpendicular to the work and on center then you should be fine.
 

uncle harry

Active User
Active Member
Joined
Aug 19, 2013
Messages
651
Likes
353
#10
Kieth Fenner of YOUTUBE fame has a video showing compound-only thread cutting. He uses a dial indicator to determine calculated or "look it up" thread depth. It worked very well for him and the video describes the method very well. I'll try to find it & if successful I'll post it on this thread.

Edit: Cross feed only, locked compound

I searched for about 15 min with no success. K. Fenner
 
Last edited:

Bob Korves

H-M Supporter - Premium Member
H-M Supporter-Premium Member
Joined
Jul 2, 2014
Messages
4,032
Likes
4,182
#12
If you try to cut threads using the cross slide considerably coarser than 20 TPI, you will run into more problems. When cutting 20 TPI on one of our hobby lathes it is pretty easy to get decent results using the cross slide only. Benmychree is correct, however. Doing it with the compound is the correct way to cut threads and will give excellent results with a tool ground correctly. My own soft rule is to cut threads using the compound for any pitch coarser than 20 TPI.
 

GK1918

Active User
Active Member
Joined
Nov 21, 2010
Messages
1,589
Likes
107
#13
Old school just ramblin again. Although both methods work But for perfect threads: In my 50yrs threading i use the compound. My secret which is no secret' first you need a crosslide stop, thats one more thing not to worry about. In
my case one of my So.Bend long bed is the dedicated threading lathe. I use no wires no mic.(which I never use) I put the lathe in back gear and the belt on high speed. End of cut back out compound return to start wind in crosslide (to its stop)
feed compound .005 or so by the time thats done and my number comes up, hit the half nut & away we go.. About the
number or line on the dial. Forget it. On the setup after the TPI is set on the gear box = start it up and hit the half nut
now backlass is gone -- shut the power - now is reset the thread dial and MARK it with a sharpie. (got it) release 1/2 nut
return carriage to the begging then move cross slide to its thread stop turn lathe on move coumpoud until you touch off
on the part.....stop and zero the coumpound -- now dial a scrach pass turning counpound .004 or so when the sharpie
comes up hit the lever. thread age says OK. end of cut hit the lever !/2 nut: now if you did not cut a reliefe , end of cut,
don't worry at that point , end of thread you hit the half nut-- let it run right there then retract the cross slide.
When I see a peak at the top of the thread I stop and try a nut what ever then a no go a couple spring passes the usually
little better so feed compound 2 or 3 check it another spring pass. then try the nut is going on but a little stiff. Old
trick paint on valve grinding compond and I run the nut or female back and forth using a vise grip or something
use gloves and a wood on the bed. Bear with me ain't a writer but I give you sir 15 minutes using my method ..
Ok people new to this Please ya don't have to be policically correct or machine correct no wires no nothing. You
need look listen and feel. Rule one after all is said as you get deeper you gotta take litghter coumpond cuts cause the tool is getting deeper. sam got F's in writing in school 60 yrs ago
 

Wreck™Wreck

Active User
H-M Supporter-Premium Member
Joined
Sep 29, 2014
Messages
1,918
Likes
1,463
#15
This is a screen shot from a canned threading cycle on a late 90's CNC lathe, eight parts that I ran this morning, 1 1/2"-12 internal thread 2 1/2" deep in 1018 steel.

You will notice the "Approach Angle" field is 29 1/2 Degrees as if threading from a compound. This is the default setting, I have found that this means little when making 1 or just a few parts per day, however it may help tool life when making 1000's of parts per day.

Many modern lathes have multiple options for approach angles when threading including alternating between the Z+ and Z- sides of the thread each pass.

A useful method of manually threading repetitive parts that I employ is to use the compound for controlling the diameter, advance it and leave it then retract the cross slide to clear when returning to the start. Return the CS to zero then advance the the compound for the next pass, this works very well on machines with an X axis DRO. One quickly grows weary of backing off the compound by the 50th part (-:


When threading on manual machines I use the cross slide only and have never had a problem in the last 30 years doing so. Having never used a hobby type machine I may be entirely wrong however.

Also very few manual lathes have a 3rd axis DRO for the compound, I dislike using hand dials.

 
Last edited:

Ulma Doctor

Infinitely Curious
Active Member
Joined
Feb 2, 2013
Messages
4,297
Likes
3,495
#16
i have never cut threads with the crosslide.
i was taught to use the compound @29.5*.
i should try some crosslide threading to see the differences for myself.

i'm a little reticent before starting the process, that the method may not be ideal for 304 stainless steel, which galls terribly.
but i'll give it a go!
 

benmychree

John York
H-M Supporter-Premium Member
Joined
Jun 7, 2013
Messages
998
Likes
565
#17
For one piece why not use a die to cut the thread.
The common sort of threading dies seldom start correctly and result in A "drunken thread", one that wobbles. An automatic die, like a Geometric die does not do this, but if one wants a concentric , non wobbly thread, single pointing is the way to get it.
 

mikey

Active User
H-M Supporter-Premium Member
Joined
Dec 20, 2012
Messages
3,037
Likes
2,956
#18
i have never cut threads with the crosslide.
i was taught to use the compound @29.5*.
i should try some crosslide threading to see the differences for myself.

i'm a little reticent before starting the process, that the method may not be ideal for 304 stainless steel, which galls terribly.
but i'll give it a go!
Mike, if you thread with a HSS tool, try using a 15 degree side relief for stainless. It should cut fine.
 

Bob Korves

H-M Supporter - Premium Member
H-M Supporter-Premium Member
Joined
Jul 2, 2014
Messages
4,032
Likes
4,182
#21
What has gone unsaid in this thread is that the cross slide versus compound question is really all about keeping track of the depth of cut. When using the cross slide, what you see on the dial is the depth of cut. When using the compound, it is the cosine of the actual compound angle from the cross slide axis times the travel on the compound dial. It is easier to just use the cross slide, sometimes better to use the compound, best to know how to do both, and important to understand grinding threading tools that will work properly with the chosen method.
 

Ulma Doctor

Infinitely Curious
Active Member
Joined
Feb 2, 2013
Messages
4,297
Likes
3,495
#22
i read somewhere that, at a compound angle of 30*, each .001" of travel on the compound is equivalent to .0005" of tool movement towards the work.
so in essence you are moving the dial on the compound at half of indicated movement at a 30* compound angle
 

Bamban

Active User
H-M Supporter-Premium Member
Joined
Jul 13, 2014
Messages
604
Likes
428
#25
My Jet 1024 has been set up to chamber AR 223 barrels, meaning the compound has been set to bore the barrel to the same taper as the case/reamer before running the finishing reamer, and I don't want to reset compound back and forth. With that set up I thread with the cross slide. So far life is good, I thread with half nuts closed the whole time and use the full feature of the VFD and the proximity sensor, threading close to the shoulder with no thread relief.

The threads come out with nice finish. This picture of a thread adapter was the maiden run with cross slide, did not want to push to the shoulder, just enough for the internal thread relief in the muzzle break to clear.

Using this special order Thin Bit carbide threading insert I can thread real close the shoulder.

20170413_201656.jpg
 

Attachments

Last edited:

bfd

H-M Supporter - Premium Member
H-M Supporter-Premium Member
Joined
Sep 9, 2016
Messages
351
Likes
190
#26
there is a thread that I have cut that requires using the cross slide the compound is set at 90 degrees so you can advance the tool bit 1/3 of the way around the thread I was cutting was a triple lead thread that I was cutting for an apprentice project so you had only the cross slide to advance the toolbit bill
 
6
5 7