PDA

View Full Version : Those numbers on a fishtail gauge



mklotz
05-19-2006, 12:32 PM
On my fishtail (center?) gauge are printed some numbers labeled "double depth
of sharp thread" for various thread pitches.

I did some math and verified that these numbers are indeed twice the thread
depth, measured perpendicular to the thread axis, for the indicated pitches.

My question is...

What use are these numbers? Since most machinists angle the compound when
cutting threads a number related to feeding straight in seems less useful than
say the compound infeed for some standard compound angle (e.g. 29 deg).

I've never seen a fishtail gauge without these numbers so I have to presume
that they're there for a good reason and 'real' machinists have some use for
them. Perhaps some 'real' machinist can explain?

lynnl
05-19-2006, 12:48 PM
Well Marv, I'm no "real machinist", and won't presume to have an authoritative answer. But I've always assumed they were included on the guage simply to save me from having to do the calculation or consult a table.
But in practice I've usually already done the calculation before I ever get around to picking up that gauge, or even thought about those numbers being there.

ps ...as I think more about it, I guess I have found the info handy, to use as a doublecheck against my calculations.

J Tiers
05-19-2006, 12:57 PM
The double depth is what you would read on the crosslide dial at proper depth........ if you plunge cut as many apparently still do and more probably used to do.

But as for use, now that sharp threads are a dim memory as far as standards are concerned, the number isn't likely that much use.

Forrest Addy
05-19-2006, 01:35 PM
I'm a real machinist but I never use the "double depth to sharp point" for the reason there's no such animal as a sharp point thread and few machinists chase threads by plunging straight in. The Unified Thread and the ISO thread we all use since WW II both have a rounded root not interfering with the creat of the mating thread as the standard thread root form.

I became a student of Unified Screw Threads in early 1973 when a local crisis developed in the shop where I worked. I was appointed to teach a series of classes on the topic. Since then always truncated the tool point for external threads to p/5 (and for internal p/10) as a personally selected hedge to comply with H28 intent to avoid root and crest interferance.

I was taught as an apprentice to "cut it til it looks like a thread", then try the gage, thread mike, wires, what ever.

I did make up a little chart, back in the old days, that showed the compound infeed at 30 degrees for p/5 (external) P/10 (internal) and the tool tip width for external and internal threads for common TPI 32 to 8. The old guys always sharpened their threading tools to a point and stoned it "just a little" across the tip so it would hold up. That "little bit" was seldom enough as the optical comparator showed time and again.

I taught my apprentices and later my students to follow the standards using my self-selected tool tip rules. They made good threads in compliance with the standards.

mklotz
05-19-2006, 01:45 PM
Ok, that's four (three plus mine) votes for the fact that those numbers are
pretty much worthless in the world of modern threadcutting.

We've had angled compounds and truncated root/tip threads since at least WWII,
maybe earlier. So why do the makers of fishtail gauges keep putting those
numbers on there? Are they some sort of secret sign of the Ancient Order of
Freemachinists?

John Stevenson
05-19-2006, 01:52 PM
It's because the Chinese just copy everything without query :o

And Forrest, if you had a problem with Unified threads back in '73 you should have got them to revert back to the Whitworth thread.
Funny how the first Standard employed turned out to be the one with the strongest thread all those years ago and still is.
Marvellous bloke that Mr Whitworth.

.

JCHannum
05-19-2006, 02:01 PM
Just to add to the fun, I have a Starrett fishtail that gives double depth of American National thread and a Lufkin that has double depth of Sharp Thread. The numbers are different of course.

Next question is why are they called Center Gages?

John Foster
05-19-2006, 02:58 PM
Jim, because they can be used to check the 60° point on a lathe center. John

IOWOLF
05-19-2006, 03:04 PM
Because you can put it between work and thread tool to see if you are on center,like a 6" scale.

Getting my flame retardant clothes on now.;)

japcas
05-19-2006, 03:16 PM
I use the numbers on the center finder quite frequently. When I'm running a cnc lathe and programming the part where a thread is at, I can simply look at the center finder, find the double depth of thread that I am programming for, divide it by 2 and then I'll add .010 to .020 to it for the chamfer at the start of the thread. Maybe not the best or only use for it, but it's a quick reference.

lane
05-19-2006, 11:25 PM
I use the Double depth to subtract from the max dia. for thread relif groves

wierdscience
05-19-2006, 11:43 PM
-Since I know that the table on the gauge is used for determining the the size of tap drills for American or US standard threads.

It gives in thousandths the double depth of tap and screw in the pitches most commonly used.

Also works in calculating the minor diameter of a hole to be single pointed in the lathe,it's what you do when you need the minor for a 6-5/8"-24 thread:D

Forrest Addy
05-20-2006, 04:24 AM
Sir John. Read what Charles Porter had to say about Mr Whitworth's organization in the 1860's in his "Engineering Reminiscences" Chapter 11 thru 13. It's an interesting contemporary account of the later years of one of the giants of the Industrial Revolution written by someone knowledgeable if a bit biased.

I wonder what Bill Gates' peers will have to say in years to come.

John Stevenson
05-20-2006, 05:48 AM
Forrest,
Believe it or not that's yet another book I have to buy <sigh>

I am a bit wary though about peoples views of Whitworth though given the age in which he lived. In those day to get anywhere with Government backing and support you had to be sponsered, a bit like your lobbiest.
Just who you had as a sponsor and just who the opposion had meant a great deal.
Whitworth was a hands on dragged up by his boots guy who felt that sucess and results meant more.

Others had already worked out that political clout mean more.

This led to the fiasco over the Armstrong guns verus the Whitworths when results spoke volumes but they addopted the very inferior Armstong pattern due to political pressure.

As regards the threads I do remember reading a wartime standard where it stated that the original Whitworth thread FORM was still something like 23% stronger that any of the current thread forms.

Many forms were modified from initial introduction but the Whitworth has stayed as it was first designed.

LES A W HARRIS
05-20-2006, 06:23 AM
Can not recall the numbering, (use it or lose it), worked things out ahead of time, However I used a different type origanaly, as we learned Whitworth, BA, & Unified.
http://i37.photobucket.com/albums/e97/CURVIC9/LATHEWORK/SCWCTNG0003.jpg


But did use the fishtail on taper threads, The apprentice school made lots of basic stuff for the main works, taper threaded mandrels for buffing machines, being the taper thread exercise.
http://i37.photobucket.com/albums/e97/CURVIC9/LATHEWORK/SCWCTNG0002.jpg


Cheers,

Mosey
12-12-2009, 08:22 PM
I use em too because you don't need any books, you just read it off the little fishtail gage for the thread pitch you are making, and that is the depth of the bottom of the thread. Since I'm a baby, I run a flat at both ends of the thread that is the depth of the bottom.
I am looking for the impossible... a center gage with finer threads double-depth numbers on it. Exists???

websterz
12-12-2009, 09:31 PM
It's because the Chinese just copy everything without query :o
...

You got a set of those #@*^'ed up 1-2-3 blocks too? :rolleyes:

Your Old Dog
12-12-2009, 09:49 PM
This thread was interesting 3 1/2 years ago when Marv first brought it up!! Should hold some interest for new members as well.

tdmidget
12-12-2009, 11:43 PM
Les as an apprentice I was taught that those are arbors, not mandrels. Arbors hold tools, mandrels hold work.
This was a mandatory question, miss it , fail the test.

dp
12-13-2009, 01:30 AM
It is an interesting old thread and is answered rather well here:

http://www.schsm.org/html/fishtail_gauge.html

oldtiffie
12-13-2009, 02:26 AM
I never use a "fish-tail" or threading guage.

https://www.machineryhouse.com.au/Products?stockCode=Q612

Getting the angle set on a small section of the tool is a "big ask" as is getting the "fish" parallel to the job or the tail-stock quill as regards accuracy.

I use vernier or digital protractors and/or bevel guages to grind the tool angles as well as setting the tool edge to the face of my lathe chuck or face-plate etc. as well as the top-slide angular off-set (1/2 tool angle less 1/2>1 degree etc.) as it is very quick and accurate:

http://i200.photobucket.com/albums/aa294/oldtiffie/Lathe_setting/Lathe_angle_set6.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Lathe_setting/Lathe_angle_set9.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Lathe_setting/Lathe_angle_set10.jpg

Depth of thread and root diameters are available on readily accessible tables everywhere.

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form1.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form2.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form3.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form4.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form5.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form6.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Screw_threads/Screw-thread_form7.jpg

woodey
04-18-2010, 06:55 PM
The numbers on the center gage are the depth of the run out grove & chanfer if your going to cut a chanfer on the leading edge. Or at least that is what I have been taught. If you were cutting 1" stock w/12TPI you would infeed 1/2 the double depth or .054 and would wind up with .108 double depth. 1" - .108=.892" thats what your mic should read & that would be your run out grove. I was also taught to add .005 to the infeed on the run out grove, when you start to scratch cut in the run out you are at your thread depth.:D