Warning

 

Close

Confirm Action

Are you sure you wish to do this?

Confirm Cancel
BCM
User Panel

Posted: 3/12/2015 9:32:02 PM EDT
My father purchased a used lathe a year ago, and has taught himself how to use it.  I'll give him credit, he went from zero knowledge to threading any barrel he can chuck.

His threads are concentric and functionally perfect, he's quite the perfectionist there, but they are rough.  The threads don't look or feel smooth, you can feel the roughness when you screw on a flash hider as well.

They work fine, but they are just rough.  Any general ideas as to why?

He's using new HSS, 60 degree cutting bit, the lathe is a South Bend, circa 1960.  We've measured and found no excessive run out.
Link Posted: 3/12/2015 10:23:50 PM EDT
[#1]
My guess would be too much slop. Lathe just worn out.
Link Posted: 3/12/2015 11:32:50 PM EDT
[#2]
Link Posted: 3/13/2015 1:55:58 AM EDT
[#3]
A couple things -

1)  Is the HSS cutter exactly at half height?  Not too high or too low?

2)  Cutter may be rough.  Stone the edges with a medium and then fine diamond stick.  I get by OK with 90 degree edges without a rake.
Link Posted: 3/13/2015 9:21:41 AM EDT
[#4]
^^^great advice, especially Dano's. Advancing the tool with the compound cuts the chip loading in half resulting in a smoother cut.
One thing I do after my last pass- I have a small stainless brush with the bristles cut down to about an 1/8" long. I spin the barrel about 300 RPM and "buff" the threads a smidge. A file card works well also. This takes a lot of roughness off of threads, even if they look smooth and clean.
Chip control- is the top of the tool flat or does it have about a 5 degree rake away from your cutting face? It helps the chip curl away from the face instead of piling up.
Using a dark, sulphurated cutting oil?
Gibs nice and snug on the compound and carriage?
I like to advance the tool only about .003 or so per pass.
How much is the tool sticking out from the holder? Keep it as close as you can so the tool doesn't flex excessively.

Kudos to Pop for learning a new skill!
Link Posted: 3/13/2015 12:54:12 PM EDT
[#5]
Do not plunge a 60 degree cutter at 90 degrees for thread cutting.

Angle the cutter in the compound.

Make sure any gibs are tight.

Even relatively worn lathes can cut clean threads if set up correctly.
It just takes repeated smaller cuts.
Link Posted: 3/13/2015 5:06:43 PM EDT
[#6]
all the things mentioned above, but also make sure you have slow speed and feed and are using a decent cutting oil and (i typically thread at 50-80rpm and with a feed rate of .0064") also, he is taking a series of cuts and not hogging the entire thread out in two or three passes, right?
Link Posted: 3/14/2015 10:13:09 AM EDT
[#7]
Link Posted: 3/14/2015 9:09:11 PM EDT
[#8]
All good advice from the previous posters.
May I suggest you buy your dad this HSS threading tool as a gift. I have one and they use disposable HSS inserts and are very well made.
Link Posted: 3/16/2015 5:58:08 PM EDT
[#9]
Excellent responses so far from folks who I can tell know how to cut threads. And congrats to your dad on picking up a new
talent!

If you are wanting perfect threads, it will require going the extra mile. Perfect tool geometry will also be required. Try anywhere
from 3 to 7 degrees side rake clearance angle at the most, with no more than 7 degrees under the nose. As mentioned before,
cutting oil is VERY important. Different metals like different cutting oil. Try Cool Tool #2 from MscDirect for starters. Old burnt
or used motor oil will also work - the thicker weight is best. Try Crisco shortening....it's a miracle cure for tapping holes. For
Aluminum use kerosene or mineral spirits & HSS only.

Now, I am assuming he doesn't have a Hardinge lathe & is using the leadscrew with the half-nut for engagement. If you want
perfect threads, do not disengage the half-nut when you reach the end.....stop the spindle, back the cross-slide out, reverse
the spindle back to a good safe engagement point, stop the spindle, move back to 0 on the cross-slide, advance the compound,
turn spindle on forward & rinse & repeat. It is slower, but it will give you excellent threads.

Let's assume your threadform requires you to advance the compound 0.052" from the start of the thread to the bottom of
the thread. First cut 0.005", second cut is no advancement.......You want to make a dry cut second, so the tool will take
what it couldn't take the first time. We call this "taking the flex out of the tool". Third cut another 0.005", flex pass of 0.0" again.
Now you have removed 0.010" of the theoretical 0.052". Rinse & repeat. At 0.030" deep, back it off to 0.002" per advancement.
Cut, flex pass, cut, flex pass etc etc etc. At 0.040" deep, drop the advancements to 0.001" & go to 2 flex passes in a row.
At 0.048", use 3 flex passes in a row.

Tool geometry is crucial...... Put a chipbreaker on the nose. If you have access to a surface grinder, grind your tool on it. It will
make the tool cut like a son of a heathen motherless goat.

Make sure the tool is exactly on the centerline of the spindle, or no more than 0.002" below the centerline.
(Mark 1 eyeball & a loupe method)
Make sure the carriage & tool post are tight.
As stated before, only let the tool bit stick out as much as needed, as well as the part out of the jaws...


Have fun & Good luck! :)
Link Posted: 3/16/2015 6:01:37 PM EDT
[#10]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Do not plunge a 60 degree cutter at 90 degrees for thread cutting.

Angle the cutter in the compound.

Make sure any gibs are tight.

Even relatively worn lathes can cut clean threads if set up correctly.
It just takes repeated smaller cuts.
View Quote


THIS is the biggest mistake most untrained people make when threading.
The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound.
You can't cut with both sides of the cutter at the same time and have it turn out smooth.

ETA: I can cut some pretty good threads  on my old beat up A-trump


Link Posted: 3/16/2015 10:10:14 PM EDT
[#11]
Discussion ForumsJump to Quoted PostQuote History
Quoted:

The compound is there for a reason, set it to 30deg and lock the cross slide,
View Quote

FWIW, the generally recognized number is 29.5 degrees. You CANNOT hit the number exactly, you will always be slightly higher or slightly lower than the target value. Slightly higher than 30 and you've got problems. So most people shoot for 29.5 degrees and that gives them a small buffer zone if they over-shoot. That is enough to relieve the pressure on the non-cutting edge (it will still remove a small amount of material but will mostly just act to burnish the thread-form, yielding a smoother thread.
Link Posted: 3/17/2015 5:37:43 PM EDT
[#12]
Make sure to use a quality cutting oil.

I've been practicing too.

Link Posted: 3/17/2015 7:21:32 PM EDT
[#13]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


THIS is the biggest mistake most untrained people make when threading.
The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound.
You can't cut with both sides of the cutter at the same time and have it turn out smooth.

ETA: I can cut some pretty good threads  on my old beat up A-trump

http://i241.photobucket.com/albums/ff206/devtucker/AR-45/IMG_20150127_244347_929.jpg
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Do not plunge a 60 degree cutter at 90 degrees for thread cutting.

Angle the cutter in the compound.

Make sure any gibs are tight.

Even relatively worn lathes can cut clean threads if set up correctly.
It just takes repeated smaller cuts.


THIS is the biggest mistake most untrained people make when threading.
The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound.
You can't cut with both sides of the cutter at the same time and have it turn out smooth.

ETA: I can cut some pretty good threads  on my old beat up A-trump

http://i241.photobucket.com/albums/ff206/devtucker/AR-45/IMG_20150127_244347_929.jpg



I am running an Atrump as well, good machine.
Link Posted: 3/17/2015 9:26:51 PM EDT
[#14]
Discussion ForumsJump to Quoted PostQuote History
Quoted:



I am running an Atrump as well, good machine.
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Do not plunge a 60 degree cutter at 90 degrees for thread cutting.

Angle the cutter in the compound.

Make sure any gibs are tight.

Even relatively worn lathes can cut clean threads if set up correctly.
It just takes repeated smaller cuts.


THIS is the biggest mistake most untrained people make when threading.
The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound.
You can't cut with both sides of the cutter at the same time and have it turn out smooth.

ETA: I can cut some pretty good threads  on my old beat up A-trump

http://i241.photobucket.com/albums/ff206/devtucker/AR-45/IMG_20150127_244347_929.jpg



I am running an Atrump as well, good machine.


Got it for basically free, our sister plant was replacing it and they were gonna sell it for salvage.
~$150 in parts and some shimming and truing and it runs like new.

Link Posted: 4/14/2015 2:04:48 AM EDT
[#15]
I have noticed that many people run at too low of a SFM. I run 150-250SFM when threading a 1/2-28 in quality barrel steel. I back it off just a bit if running a stainless barrel.


Im using solid carbide full profile inserts, and coming back through and performing a higbee cut on the first thread to cut away the partial thread. If Im being lazy I plunge directly in X or if I have time I will alternate flank infeed.
Link Posted: 4/14/2015 5:45:17 AM EDT
[#16]
Lots of good information above!  The compound probably being one of the biggest pieces that beginners don't know.  It was also said to make sure your gibs are tight.  If you don't know what they are a quick youtube search will show how to adjust them.  They make a huge difference when threading and parting.
Link Posted: 4/14/2015 8:06:54 PM EDT
[#17]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Lots of good information above!  The compound probably being one of the biggest pieces that beginners don't know.  It was also said to make sure your gibs are tight.  If you don't know what they are a quick youtube search will show how to adjust them.  They make a huge difference when threading and parting.
View Quote


If you set a compound at 84 degrees you can do 0.0001 feed
Link Posted: 4/18/2015 10:44:18 PM EDT
[#18]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


If you set a compound at 84 degrees you can do 0.0001 feed
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Lots of good information above!  The compound probably being one of the biggest pieces that beginners don't know.  It was also said to make sure your gibs are tight.  If you don't know what they are a quick youtube search will show how to adjust them.  They make a huge difference when threading and parting.


If you set a compound at 84 degrees you can do 0.0001 feed


Just not while threading.
Link Posted: 4/19/2015 11:09:11 AM EDT
[#19]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


Just not while threading.
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Lots of good information above!  The compound probably being one of the biggest pieces that beginners don't know.  It was also said to make sure your gibs are tight.  If you don't know what they are a quick youtube search will show how to adjust them.  They make a huge difference when threading and parting.


If you set a compound at 84 degrees you can do 0.0001 feed


Just not while threading.

29.5 for threading
The feed is about half the dial, so make sure you measure and watch carefully.
When the off flank starts to form up you are getting close.
I have been known to chase with a die for the last little bit.
Link Posted: 4/19/2015 3:22:45 PM EDT
[#20]
Was just making it clear to anyone that was listening that they weren't going to feed .0001" and get super clean threads that way
Link Posted: 4/19/2015 4:03:40 PM EDT
[#21]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Was just making it clear to anyone that was listening that they weren't going to feed .0001" and get super clean threads that way
View Quote


Even if you could, there's such a thing as taking too little material per pass
Link Posted: 4/20/2015 2:58:07 PM EDT
[#22]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


Even if you could, there's such a thing as taking too little material per pass
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Was just making it clear to anyone that was listening that they weren't going to feed .0001" and get super clean threads that way


Even if you could, there's such a thing as taking too little material per pass


it is one of those hidden tricks on a compound to get surface close enough to polish down to final size for bearings.

Very shallow cuts do put a premium on tool and material rigidity.

Heat buildup can be an issue with small cuts.
The chip carries away significant heat.
Link Posted: 5/6/2015 12:18:11 PM EDT
[#23]
Discussion ForumsJump to Quoted PostQuote History
Quoted:

Now, I am assuming he doesn't have a Hardinge lathe & is using the leadscrew with the half-nut for engagement. If you want
perfect threads, do not disengage the half-nut when you reach the end.....stop the spindle, back the cross-slide out, reverse
the spindle back to a good safe engagement point, stop the spindle, move back to 0 on the cross-slide, advance the compound,
turn spindle on forward & rinse & repeat. It is slower, but it will give you excellent threads.
View Quote



That sounds really hard, depending on the lathe.  That's how my buddy threads on a big lathe with transmission and brake, but on a smaller lathe without a transmission or brake there's no way I could cut power and coast to a stop in the thread relief without crashing into the shoulder.  I'm using a Southbend Fourteen for reference, I don't have a problem using the halfnut and thread dial to get good threads.  


My method is to set the compound to 29 degrees and set the tool square to the work.  

I'll  set the crossfeed to 0 on the dial, run the compound in until the tool tip is touching the barrel, and move to the left until it touches the shoulder, then back off towards the muzzle by half a thread plus a little buffer.  For example, a 5/8x24 thread is .042 per thread, so I'll move back by .021 + .010.  Then I put a dial indicator on the frame of the lathe touching the apron, and set it so that it's exactly one complete turn in.  This is hard to describe, but really simple once you see what I'm doing.  I don't have a good picture, but you can see the dial indicator on the bottom.  



When I'm threading, I wait for the thread dial to line up and then engage the halfnut to start the feed.  Then I watch the dial indicator.  When it gets close the apron will hit the indicator and start turning it; when it has turned one complete revolution I disengage the halfnut and back out the crossfeed.  The half a thread clearance, .021 in the example, gives clearance since the compound will end up moving the tool half a thread towards the shoulder as you cut deeper.  The extra .010 is in case you don't disengage the halfnut exactly on time, although I can hit it within a thousandth or two most of the time.  Sounds complicated, but is really easy once you see it done.  Other people may have better ways, I made this one up myself.

So then I just back up, reset the crossfeed to 0, advance the compound .003, and take the next cut.  I take a spring cut before measuring, and slow down to around .001 when I'm close to full depth.
Link Posted: 5/6/2015 12:22:18 PM EDT
[#24]
My engagement is a little wonky, so I stop, retract and reverse.
My A-trump has a good, tight foot brake that kills the motor, so I don't need a massive thread relief.
Link Posted: 5/16/2015 8:08:19 PM EDT
[#25]
Discussion ForumsJump to Quoted PostQuote History
Quoted:

29.5 for threading
The feed is about half the dial, so make sure you measure and watch carefully.
When the off flank starts to form up you are getting close.
I have been known to chase with a die for the last little bit.
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Quoted:
Lots of good information above!  The compound probably being one of the biggest pieces that beginners don't know.  It was also said to make sure your gibs are tight.  If you don't know what they are a quick youtube search will show how to adjust them.  They make a huge difference when threading and parting.


If you set a compound at 84 degrees you can do 0.0001 feed


Just not while threading.

29.5 for threading
The feed is about half the dial, so make sure you measure and watch carefully.
When the off flank starts to form up you are getting close.
I have been known to chase with a die for the last little bit.

Chasing the threads with a sharp, quality, properly adjusted die is a great way to finish them. Many machinists do not like doing this, but it is a great method. This is assuming the threads are very close to finish size before the die gets involved.

This is my favorite method, by far. It takes a lot of the tedious spring and finish passes out of the equation if things are done right. Let the die do the hard work. It will also correct the pitch and thread form to a certain degree. The die will also help with the deburring process. It can help to remove the rubber cratex from the process, if done right.
Link Posted: 5/20/2015 1:32:06 PM EDT
[#26]
Discussion ForumsJump to Quoted PostQuote History
Quoted:

Chasing the threads with a sharp, quality, properly adjusted die is a great way to finish them. Many machinists do not like doing this, but it is a great method. This is assuming the threads are very close to finish size before the die gets involved.

This is my favorite method, by far. It takes a lot of the tedious spring and finish passes out of the equation if things are done right. Let the die do the hard work. It will also correct the pitch and thread form to a certain degree. The die will also help with the deburring process. It can help to remove the rubber cratex from the process, if done right.
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Quoted:
Quoted:
Lots of good information above!  The compound probably being one of the biggest pieces that beginners don't know.  It was also said to make sure your gibs are tight.  If you don't know what they are a quick youtube search will show how to adjust them.  They make a huge difference when threading and parting.


If you set a compound at 84 degrees you can do 0.0001 feed


Just not while threading.

29.5 for threading
The feed is about half the dial, so make sure you measure and watch carefully.
When the off flank starts to form up you are getting close.
I have been known to chase with a die for the last little bit.

Chasing the threads with a sharp, quality, properly adjusted die is a great way to finish them. Many machinists do not like doing this, but it is a great method. This is assuming the threads are very close to finish size before the die gets involved.

This is my favorite method, by far. It takes a lot of the tedious spring and finish passes out of the equation if things are done right. Let the die do the hard work. It will also correct the pitch and thread form to a certain degree. The die will also help with the deburring process. It can help to remove the rubber cratex from the process, if done right.

I tend to chase with a die when I am doing stainless...it really help to remove some of the micro galling that can form...
Link Posted: 5/20/2015 2:13:22 PM EDT
[#27]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
That's how my buddy threads on a big lathe with transmission and brake, but on a smaller lathe without a transmission or brake there's no way I could cut power and coast to a stop in the thread relief without crashing into the shoulder.  I'm using a Southbend Fourteen for reference, I don't have a problem using the halfnut and thread dial to get good threads.  
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
That's how my buddy threads on a big lathe with transmission and brake, but on a smaller lathe without a transmission or brake there's no way I could cut power and coast to a stop in the thread relief without crashing into the shoulder.  I'm using a Southbend Fourteen for reference, I don't have a problem using the halfnut and thread dial to get good threads.  

I thread with NO thread relief; stopping & reversing, threading away from the shoulder is the most reliable way I've found of doing this. Doing it this way makes the thread job look factory, like it was done on a CNC lathe at the same time the barrel profile was being turned. How many factory threaded barrels have you seen with a thread relief? I have seen NONE.

I'm running a SouthBend 10" and I don't have any problems "coasting" to where want. You can't cut power when you get where you want to be, you cut power before you get there. Your lathe should coast to a stop at a fairly repeatable point. I can often hit a .050" window of where I intend to be simply by cutting power.2-.3" before I want to (on a 28 tpi) stop. I then turn the chuck by hand (half-nuts still engage and dragging the carriage along) until it's at the point I want it. If you're worried about running into the shoulder and you're threading away from the shoulder then your "return" should be a on pass where you aren't cutting; retract the cross-slide all the way back so even if you overshoot the shoulder it won't crash.


I just did a barrel shorten/thread job for a guy. This is what he emailed me this morning,
From Customer on another forum:
I can't tell you how pleased I am with the work you did on my upper and barrel.
The rifle is finally starting to take shape, and now I need to start thinking about the insides of this thing so I can actually shoot it.

I found an article on one of the forums about cutting a BCG for a Glock magazine.  Let me know if this is something you'd be interested in working on.
http://www.ar15.com/archive/topic.html?b=3&f=15&t=604491


Customer satisfaction is a testament: the entire time he was there picking up his upper/barrel he kept commenting at how professional and "factory like" the thread job looked.

To each his own, whatever you prefer will most likely function the same no matter what. Just trying to point out that there are ways to skin the cat that you may have not thought of.
Link Posted: 5/20/2015 2:21:26 PM EDT
[#28]
I'm just a noob with a 7x14 mini lathe, but I'm able to cut decent threads if I do the following:

1) stiffest HSS cutter I can fit.
2) Gibbs tight. Otherwise tool will chatter and give rough threads
3) Tool on-center or a hair below center. Above-center it will dig-in as it flexes (I actually part upside-down/reverse because of tool/post flex)
4) 29.5 degree compound. Straight-in is no bueno.
5) Keep the half nut engaged the entire time. Back out and reverse with each pass. I took my threading dial off and thew it in a junk box. This method is slow but is most accurate
6) Check half-nut engagement constantly

Failure of any item #1-4 would give me rough surface.
If I don't do #5-6 and instead disengage the feed and use the threading dial I get very inconsistent passes.

I can almost always trace rough surface finish to flex of some sort: Tool flex, Tool-post flex, loose gibbs flex, unsupported work flex, etc.
Link Posted: 5/27/2015 10:04:39 PM EDT
[#29]
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:

That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the
zero mark on the compound angle, at the *wrong* place!

And they never put this 'minor' fact in their manuals, and nobody ever
talks about it. You need to put the compound at 30 degrees. So you
put the mark on the 60 number!! Just plain nuts.
View Quote


Since I've made this change my threads are perfect and super clean.
Link Posted: 5/28/2015 12:48:12 PM EDT
[#30]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:



Since I've made this change my threads are perfect and super clean.
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:

That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the
zero mark on the compound angle, at the *wrong* place!

And they never put this 'minor' fact in their manuals, and nobody ever
talks about it. You need to put the compound at 30 degrees. So you
put the mark on the 60 number!! Just plain nuts.


Since I've made this change my threads are perfect and super clean.

I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a scale that reads backwards.
Link Posted: 5/28/2015 1:11:16 PM EDT
[#31]
Discussion ForumsJump to Quoted PostQuote History
Quoted:

I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage.
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:

That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the
zero mark on the compound angle, at the *wrong* place!

And they never put this 'minor' fact in their manuals, and nobody ever
talks about it. You need to put the compound at 30 degrees. So you
put the mark on the 60 number!! Just plain nuts.


Since I've made this change my threads are perfect and super clean.

I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage.


I think that he thinks that the scale is double-angle, not reverse angle (90deg off)
Link Posted: 5/28/2015 1:50:44 PM EDT
[#32]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


I think that he thinks that the scale is double-angle, not reverse angle (90deg off)
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:

That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the
zero mark on the compound angle, at the *wrong* place!

And they never put this 'minor' fact in their manuals, and nobody ever
talks about it. You need to put the compound at 30 degrees. So you
put the mark on the 60 number!! Just plain nuts.


Since I've made this change my threads are perfect and super clean.

I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage.


I think that he thinks that the scale is double-angle, not reverse angle (90deg off)


First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are.

Link Posted: 5/28/2015 2:11:13 PM EDT
[#33]
tap a tap double tap
Link Posted: 5/28/2015 2:11:39 PM EDT
[#34]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are.

http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:

That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the
zero mark on the compound angle, at the *wrong* place!

And they never put this 'minor' fact in their manuals, and nobody ever
talks about it. You need to put the compound at 30 degrees. So you
put the mark on the 60 number!! Just plain nuts.


Since I've made this change my threads are perfect and super clean.

I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage.


I think that he thinks that the scale is double-angle, not reverse angle (90deg off)


First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are.

http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg

when I thread with the exception of plastic...

I never take a larger than .004" depth of cut and finish with .001" and "Clear" passes
Link Posted: 5/28/2015 2:14:06 PM EDT
[#35]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
when I thread with the exception of plastic...

I never take a larger than .004" depth of cut
View Quote


Yeah, if this was an actual piece of work, like a barrel, I wouldn't take a cut over 0.005". Also, I meant that to say 0.01", not 0.10" in my original post.
Link Posted: 5/28/2015 5:02:34 PM EDT
[#36]
Discussion ForumsJump to Quoted PostQuote History
Quoted:


First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are.

http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg
View Quote View All Quotes
View All Quotes
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Quoted:
Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:

That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the
zero mark on the compound angle, at the *wrong* place!

And they never put this 'minor' fact in their manuals, and nobody ever
talks about it. You need to put the compound at 30 degrees. So you
put the mark on the 60 number!! Just plain nuts.


Since I've made this change my threads are perfect and super clean.

I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage.


I think that he thinks that the scale is double-angle, not reverse angle (90deg off)


First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are.

http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg


Take a thread pitch gage and put against those threads.  You might be using a 60deg cutter, but those aren't 60deg threads, they look closer to 80deg.

Link Posted: 5/28/2015 5:27:02 PM EDT
[#37]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
Take a thread pitch gage and put against those threads.  You might be using a 60deg cutter, but those aren't 60deg threads, they look closer to 80deg.

http://www.roymech.co.uk/images/Iso_thread.gif
View Quote


I couldn't get it to focus using my phone but the pitch gauge fits well. I did get a little aggressive filing the tops of the thread:

Link Posted: 5/29/2015 8:21:03 PM EDT
[#38]
You can also trig it out with an indicator.

Multiply 29.5 tan x 1.000". The result is the length of the Opposite (short) leg of the triangle.
If you travel exactly 1.000" with the cross-slide, that result should be what you shoot for.
In other words, zero your Z axis & move it in X axis 1.000" & touch the same point on the indicator.
When the Z axis travel amount is the same as the result you are good to go.

You do not have to be exactly on 29.5 degrees. CNC lathes can cut at 90 degrees & have flawless
threads. Manual machines are less rigid & it works better for them if they feed in on an angle.

Link Posted: 6/1/2015 9:18:24 PM EDT
[#39]
Link Posted: 6/9/2015 11:54:40 AM EDT
[#40]
Discussion ForumsJump to Quoted PostQuote History
Quoted:
I thread with NO thread relief; stopping & reversing, threading away from the shoulder is the most reliable way I've found of doing this. Doing it this way makes the thread job look factory, like it was done on a CNC lathe at the same time the barrel profile was being turned. How many factory threaded barrels have you seen with a thread relief? I have seen NONE.

I'm running a SouthBend 10" and I don't have any problems "coasting" to where want. You can't cut power when you get where you want to be, you cut power before you get there. Your lathe should coast to a stop at a fairly repeatable point. I can often hit a .050" window of where I intend to be simply by cutting power.2-.3" before I want to (on a 28 tpi) stop. I then turn the chuck by hand (half-nuts still engage and dragging the carriage along) until it's at the point I want it. If you're worried about running into the shoulder and you're threading away from the shoulder then your "return" should be a on pass where you aren't cutting; retract the cross-slide all the way back so even if you overshoot the shoulder it won't crash.

.
View Quote


Ah, you're turning the last part by hand.  That's the part I couldn't figure out.  

I frequently do it without a relief as well, here's one I did for myself a couple weeks ago.  It's for the barrel extension on a large frame AR.

Close Join Our Mail List to Stay Up To Date! Win a FREE Membership!

Sign up for the ARFCOM weekly newsletter and be entered to win a free ARFCOM membership. One new winner* is announced every week!

You will receive an email every Friday morning featuring the latest chatter from the hottest topics, breaking news surrounding legislation, as well as exclusive deals only available to ARFCOM email subscribers.


By signing up you agree to our User Agreement. *Must have a registered ARFCOM account to win.
Top Top