machinist@lists.ibiblio.org
Subject: Machinist
List archive
[machinist] Single point threading on a manual lathe
- From: Lawrence London <lfljvenaura@gmail.com>
- To: machinist@lists.ibiblio.org
- Subject: [machinist] Single point threading on a manual lathe
- Date: Fri, 1 Nov 2013 21:47:35 -0400
http://www.practicalmachinist.com/vb/general/single-point-threading-manual-lathe-273000/
Thread: Single point threading on a manual lathe
-
Single point threading on a manual lathe
A long time ago I read on this forum, I think, an easy way to do single point threading, especially figuring the cut depth, which would get you real close to finish size. I tried it, and it was a pleasure to use. I, of course, forgot how to do it. Must be old age. Anyone know what I'm talking about, or have a "canned" method of single point threading? Thanks guys!
-
10-04-2013, 11:03 AM #2
- Join Date
- Jan 2005
- Location
- Canada
- Posts
- 6,251
Because the flat (or radius) on the tip of the tool could be anything, precalculated depths to go are kind of useless. I'd recommend getting a set of thread measuring wires, and learn how to measure threads in progress.
Visually, the crests of completed threads are not sharp, but are 1/8 of the thread's pitch, so learn to stop and make an initial measurement before you progress too far.James H Clark likes this. -
-
10-04-2013, 11:16 AM #4
- Join Date
- Aug 2008
- Location
- Californeeeah
- Posts
- 1,056
Maybe you're thinking of the "threading to zero" method of setting infeed of the topslide when feeding at 30d? You still need to know the depth though.
-
Here's a "quick and dirty" way to do it:
Put a coat of blueing on the area to be threaded. Cut your threads until the blueing just dissapears. Then check with known threaded part for fit. (A nut or whatever) Usually after the cut that removes the last of the blueing you are pretty much there. (as long as you don't have to hold a critical clearence tollerance) Take small cuts for your last cuts so you don't go past where you want to be.
FrankRoger Williams likes this. -
longer ago than I care to remember, a teacher gave us these formulas:
total infeed = .708 x pitch
7 infeed passes @ 35% of total infeed, 25%, 20%, 10%, 5%, 3%, 2%
as I recall, it worked out pretty nice. now, I find a pitch mic is a lot easier. -
10-04-2013, 12:40 PM #7
- Join Date
- Dec 2000
- Location
- Bremerton WA USA
- Posts
- 8,865
I've been cuting threads on lathes, vertical boring mills, horizontal boring mills etc since the rocks were soft and use only one system:
1. Look up or calculate thread data
2. Make sure the flat on the tool tip suits the standard for that particular pitch
3. check the machine settings and verify the pitch cut using the first tool scatch and a fishtail gage
4. Cut until it looks like a thread, then check with wires, gages, thread mikes
5. If the stop/pull-out drenches your armpits with sweat, set up a dial indicator stop. Get a little practice and you can open the half nut and twirl out the tool hitting the zero to +/-0.002. Your analog eye is way keener than your reaction to a DRO approaching zero.
That's about it. Tool infeed, double depth, etc may be handy but I haven't used them since my apprenticeship in the early '60's. I ran into an old railroad machinist about then and he taught me a ton of crafty shortcuts like simple ways of cutting threads.
Oh, yeah I forgot the most important part: practice. Even at my stage of advanced decrepitude if I haven't cut a thread for a while, I'll grab a remnent and cut a few before I attack the money job. If you think about it, it's really dumb to risk work because your practice isn't current. Airline pilots don't. -
Can't do any better than the suggestions written from experience, but I will add something that I like to do on any thread pitch greater than about 16tpi, or if using a lightweight setup.
That is, after sizing the stock, using the threading dial as reference, on the first threading pass , pick a number. (there are rules for what numbers work for subsequent passes, but that is covered in your lathe info) As suggested above, that first pass can be a big portion of the overall thread depth. At least 25%.
On the SECOND threading pass, Close the half nut on a threading dial indication BETWEEN numbers just before or after your choosen point. The threading tool will make a pass just a step over from the first, and so wasting a good bit of material at the same depth of cut as the first. The rough gouge with look like a W instead of a V.
Don't worry! It will all be cut away anywho...
On small threads, subsequent passes revert back to the first threading dial position.
On the big stuff (4tpi etc.) Alternate half nut engagement positions for a couple of passes. You will be able to see when the offset cut is approaching the crest of the first cut. Blueing helps! Don't go overbaord and spoil thge work . (don't ask;-)
The method works very well for easing the load for all cuts, chatter can be eliminated. and it even makes sense once you get the hang of it.
This is NOT a method to use when you are not going to open the half nuts for any reason (metric threads, worn machine, etc. Though is easily simulated by advancing/retracting the compound when set to parallel the thread.
It really works well for internal threads made with an overhanging bar.
As Addy suggested, a little practice makes for confidence. -
these are all good, valid answers, and I agree to all. What I was looking for was a quick and easy way to get real close. This info had to have came from an old timer, just the way it was worded. I wish I can remember how he said to do it, it was SO simple, you didn't even have to think, and it worked on all the different thread sizes I tried it on. Then forgot it. Shame on me!
Forrest, I actually run the chuck backwards and the tool upside down, and thread from the stop point to the outside to avoid the previously mentioned maladies!! -
10-04-2013, 02:55 PM #10
- Join Date
- Sep 2004
- Location
- south SF Bay area, California
- Posts
- 1,261
I'll quote myself, from several years ago:
"The Basic ISO Metric screwthread is proportioned exactly like the Unified screwthread. The flank-to-flank angle is 60 degrees, the flat at the Major Diameter is 1/8 Pitch, and the flat at the Minor Diameter is 1/4 Pitch. As a result of this basic geometry, the length of the flank is 5/8 Pitch, the Single Depth of Thread is 5/8 Pitch x Cosine 30 degrees, and the Double Depth of Thread is 2 x 5/8 Pitch x Cosine 30 degrees = 1 ¼ Pitch x Cosine 30 degrees, twice the Single Depth of Thread.
Assuming 1) that your toolbit has a correct-width flat at its tip, 2) that you've slewed the compound rest / topslide to feed along the flank of the screwthread, 3) that you've zero'd the compound rest /topslide micrometer collar when the flat tip of the toolbit just contacts the OD of the workpiece, and 4) that the workpiece diameter matches the theoretical Major Diameter, the toolbit should theoretically be fed into the workpiece along the flank of the thread 5/8 x Pitch.
In reality, all four of the factors I've listed will be close but not perfect. That means that theoretically-perfect compound rest / topslide infeed won't produce a perfectly-sized screwthread.
What to do?
Make you setup, and cut your screw until it looks ALMOST deep enough. Then make an over-wires measurement before cutting-away the oversize, which is usually done in a short series of shallow cuts.
John -
Now if there were such a direct and easy message for the internal threads ;-)
The "over wires" part is such a bother. And making the go/no go is so fiddly! ;-)
(Yes, I know there are comparative tools for this application) -
For a 60 deg. thread form I grind a flat on the point of the tool equal to 1/8 the thread pitch. Set the compound to 29 1/2 deg. from perpendicular to the axis of shaft. Touch off tool to shaft. Find required depth of thread and divide by cosine of 29 1/2 deg. This will give you amount to feed in at that angle. Cut about half depth on first cut. Then half of remaining. Repeat until flat remaining at crest of thread is close to 1/8 pitch and start measuring with thread wires.
-
10-05-2013, 08:34 PM #13
- Join Date
- Sep 2004
- Location
- south SF Bay area, California
- Posts
- 1,261
Loomis --
The basic standards for both the Unified (which replaced the US Standard threadform in 1949) and ISO Metric (developed by the International Standards Organization in 1959 as a "world standard" proposal) have 1/4 Pitch flats at the Minor Diameter, and 1/8 Pitch flats at the Major Diameter. To properly single-point either of these threadforms with a single-point tool, the toolbit flat needs to be 1/8 Pitch for an internal thread, 1/4 Pitch for an external thread.
CalG --
The "simple trick" for single-pointing an internal thread is a combination of a properly-flatted toolbit and a short counterbore 0.002 inch or so over the theoretical Major Diameter of the thread you're trying to cut. For my own work -- and nobody has ever knowingly paid me to machine anything -- I do what an old-timer taught me, and generally make the counterbore 1 to 2 Pitches deep, and if visibility is poor, a touch of Magic Marker ink or layout dye inside the counterbore can be a help. Set the toolbit to the bore to be threaded, and cut the thread. When the toolbit tip just grazes the counterbore, your internal thread is done.
John -
10-05-2013, 09:53 PM #14
- Join Date
- Jun 2010
- Location
- milton freewater oregon
- Posts
- 1,644
Myself I horse a lathe hard when threading, it should not take long or very many passes. No less than .010" on a Finnish pass if possible.
Practice is huge, as you get better you can speed up the RPM's and take bigger bites given the capabilities of your particular lathe.
My main trick Lots of oil, saves on the tool and helps on surface Finnish. -
John--
The two books I have been using for reference are a American Machinists' Handbook and Machinery Handbook both of which give the width of flat as P/8 at both root and crest of the thread. I have been using this method for 45 years with no problem.
Lou -
10-05-2013, 11:25 PM #16
- Join Date
- Sep 2004
- Location
- south SF Bay area, California
- Posts
- 1,261
Loomis --
The 60-degree-V threadform having 1/8 Pitch flats at both the Major and Minor Diameters is the Sellers, which is also known as the Franklin Institute, US Standard, and American National threadform. William Sellers introduced the Sellers threadform and its Major Diameter and Pitch combinations as a proposed standard in a presentation at the Franklin Institute in Philadelphia in 1864, and it was, over time, widely accepted and eventually adapted as the United States' national-standard threadform in the early 1900s.
Even before that, in England, Joseph Whitworth had proposed a different threadform, one having a 55-degree-V and full radii at both the Major and Minor Diameters, that became the British Standard.
Both nations prospered with their own national standard screwthreads, but during World War II the non-interchangeability of the two screwthreads created massive logistic headaches. After WWII was finished, the US and British authorities -- and the Canadians, who had more-or-less-commonly used both threadforms for most of a century -- made a conscious decision to replace their differing standard screwthreads with one common standard. The new threadform, dubbed the "Unified" form, became the new national standard of Canada, Great Britain, and the United States in 1959.
The Unified threadform differed slightly from the Sellers, but was designed to be practically interchangeable with existing Sellers-threaded hardware, and hexes of bolts heads and nuts were sized to fit Sellers-sized wrenches. The changes -- increasing the theoretical Minor Diameter, and the length of the flat at the Minor Diameter without changing the Major Diameter and its flat -- even allows Sellers-form taps to be used to cut Unified-form internal threads as long as the Major Diameter and Pitch match, which they generally do. To this day, the majority of "American size" taps sold are still made to Sellers form, and marked either NC, NF, or NS designators that hark back to the "American National" alternative name of the Sellers threadform.
Be that as it may, the Sellers threadform has been obsolescent for more than 60 years now.
JohnMrSleepy and Trboatworks like this. -
10-06-2013, 10:48 AM #17
- Join Date
- Nov 2008
- Location
- Chicago, IL
- Posts
- 1,368
-
10-06-2013, 11:02 AM #18
- Join Date
- Feb 2009
- Location
- Wisconsin
- Posts
- 1,103
Grind a 60 degree threading tool (HSS) with a flat equal to one-eighth the pitch, multiply the single depth of the thread by 1.143 to get the amount to feed the compound set at 29 1/2 degrees. This has worked for me for 60 years.
Lord ByronJoe Miranda likes this. -
Hm,
I will explain my method which has probably already been mentioned.
For example, 3/8-24 thread.
1. Turn OD (~.370) and undercut (~.325)
2. Set compound angle, zero compound.
3. Touch off on OD with cross slide, leaving compound set at zero.
4. Back your compound out for clearance, and go in your thread depth on the cross slide. Refer to double depth chart. For 24 TPI, double depth is .051. Go in this amount and zero your cross slide.
5. Now with your cross slide at the thread depth, you can start threading into your undercut, advancing the compound little by little until the desired depth is achieved and your thread is good.
Hope this helps, good luck. -
10-07-2013, 07:49 AM #20
- Join Date
- Jun 2012
- Location
- Michigan
- Posts
- 866
*For "canned" or easy to remember old school..
http://team358.org/files/mechanical/...ingThreads.pdf see page-4
I think one old trade school short cut rule for 60* thread was SA7585 (basically a ballpark)
Saturday afternoon 7585 (memory helper) With this pitch means number of threads
Straight in: .75/p-r
Angle in: .85/p-r (come in at 29 1/2 degrees)
R is the tool bit radius (flat)
For 14 TPI: .75 / 14= .053 (Book says .0541) Then take away the radius
.85/14=.061 for come in at 29 1/2
Seems to work OK.
*That was to get ball park near and when getting close finish test with wires or a good (G-8) nut.
-Or test with Gordon's thread check calipers.-
http://littlemachineshop.com/instruc...WireMethod.pdf
http://www.f-m-s.dk/FMS%20Thread%20Measurement.htm
Malzo's .708 x p (.708 x .0714 = .050) that works. (.0714 is 1 divided by 14 TPI or pitch.)
Another quick thought is at 60* three sides are equal,so the pitch (1 / #thds) will be ball park close feed in at 29 1/2* *1/14 = .071 for angle in. That is a bit deep perhaps for 100% thread. Don't try to to make 100% thds.
Seems there was a 115 Ball Park rule ? It may have been: Straight in amount x 1.15 is angle in amount. I will have to see if that works. *for 14TPI: .053 x 1.15 = .061 seems to work
A trick I used for threading and turning was to just touch work with tool bit, feed straight in to mark half way around part and set that as zero. That was like indicating with the tool bit for run out to get spindle center for beginning a job.
>From South Bend book: How to Cut Screw Threads: Depth = P x .64952
(Straight in for 14TPI ) 1/14=.0714 x .64952= .046
Flat =P/8 (.0714/8= .009)
*Best to trig out numbers or use a good book reference but out in the field improvise may be only choice.
Single point HHS tool bits have a cutting edge angle going one way off the cutting edge so should only cut one way (right or left) with coming in at 29 1/2 or so to the cut.
Many carbide insert tool bits have a combination rake to both sides and to the front so they can cut at angle to right, to left or straight in.
BuckLast edited by michiganbuck; 10-07-2013 at 12:33 PM.
Reply
(which aren't cheap). Still, I like the observation about chip direction. It's a keen observation by the poster.
http://www.practicalmachinist.com/vb/general/single-point-threading-manual-lathe-273000/index2.html
- Join Date
- Feb 2009
- Location
- Wisconsin
- Posts
- 1,103
Grind a 60 degree threading tool (HSS) with a flat equal to one-eighth the pitch, multiply the single depth of the thread by 1.143 to get the amount to feed the compound set at 29 1/2 degrees. This has worked for me for 60 years. I forgot to mention that the single depth of the thread is .649519 x pitch.
Lord Byron
michiganbuck and Joe Miranda like this.
10-08-2013, 09:11 AM
#22
- Join Date
- Jun 2012
- Location
- Michigan
- Posts
- 866
For straight in 1/ TPI x .866 = 100% thread
Example for 14 TPI
1 / 14 = .0714285 x .866 = .06185 for 100% thread
.06185 x.75 = .04639 straight in feed for a common 75% thread.
Canned number:
Re calculating 70 may be better than 75. For a canned straight in feed number.
10TPI: .70/10=.070 act = .065
13TPI:.70/13=.053 act =.050
20TPI .70/20=.035 act=.032
24TPI .70/24=.029 act=027
48TPI .70/48=.0145 act=.013
That is not bad because the science of perfect numbers don't always exist when single point turning threads .
One must take in to account part run out, the perfection or not of the tool bit, error in carriage ect.
With these possible issues one should check and measure with coming to around the last .005 or when the thread looks to be near coming to a point.
Last edited by michiganbuck; 10-08-2013 at 09:18 PM.
- [machinist] Single point threading on a manual lathe, Lawrence London, 11/01/2013
Archive powered by MHonArc 2.6.24.