I'm going to be threading the tenon of a rifle barrel and am practicing
on a 1" dia piece of scrap crs. The thread is 16tpi, standard 60 deg. With
the compound at 30 deg., 60 deg. threading tool square/centered to the stock
I keep getting an uneven finished thread. The left side of the "V" is about
20 deg. and the right side about 40 deg. If I advance the cutter using only
the cross feed, and not the compound, I get a perfect thread.
I've tried setting the compound at 29.5deg, 30deg, etc. with no
improvement. I've checked the set-up with a protractor, dial indicators,
etc. and can find nothing wrong with the lathe or my set-ups. Obviously
something is wrong but at this point I don't have a clue. Any suggestions?
I was having a similar problem. It turned out that
I actually had the compound set to 60 deg. rather than
30. I was following the marks on the compound and
they were either wrong or misleading....
You need to be set at 30 degrees relative to the
plane defined by the faceplate or 60 degrees relative
to the spinning axis.
Yep, ignore the degree numbers. Put the compound so it feeds
inward along the same axis as the crossfeed. Then count off
30 degrees as you move the compound handle to the left.
Then go back a degree or two.
IOW you want to be mostly advancing the cutter into the face of the V
that you're going toward, yet cut ever so lightly into the 'back' of the V.
Since thread finishes should be fine make lots of really light cuts, and
make sure that tool is sharper than sharp.
There's a much simpler method; one which makes it impossible (!) to
make the error highlighted by Jim Stewart whilst at the same time it
keeps track of the depth of thread by direct reading of the cross-slide
dial - not possible if you angle the compound slide. I use it; by
coincidence I used it this afternoon to cut a half inch BSP internal
thread to a shoulder. The method was described in a letter to Model
Engineer magazine (M.E.) by Duncan Webster of Cheshire, UK as follows:
"In Mr. Ellis' article "Letter to a Grandson" about screwcutting (M.E.
4128, 8th September 2000) he describes two options for incremental tool
feed between cuts: straight in and angled top-slide. As he rightly
points out, the straight-in method requires the tool to cut on both
flanks causing the chips to collide and jam and, incidentally making it
impossible to have any top rake on the tool. The so-called half-angle
method is fine except that you can't use it on the Myford ML7 lathe as
the top-slide won't go round that far; also you no longer have a dial
that tells you how deep you have cut.
The following method is not new, it was shown to me by an old chap who
had been apprenticed in a Merseyside shipyard in the 1920s and it has
been described in M.E. before but seems not to have caught on.
Set the top-slide (compound slide) parallel to the job, its usual
position for plain turning. Wind in the cross-slide until the tool
just touches the job. If the cross-slide index dial can be zeroed,
then do so, otherwise wind the top-slide forward until its dial reads
half the reading on the cross-slide. Ideally, zero both if they are
Move the saddle to the right, clear of the workpiece; wind in the
cross-slide say ten thou(thousanths of an inch) and wind in the
top-slide half of this distance. Engage the leadscrew half-nuts and
take the first cut. Move the saddle back to the start point, wind the
cross-slide in a further cut (say ten thou) and the top-slide forward
by half of this amount and take another cut. You will note that the
top-slide keeps a record of how you are going so there's no need to
remember the cross-slide reading and the total depth of cut is
indicated on the cross-slide dial.
Almost all of the cut is on the left of the tool; the right flank has
only a minute shaving cut. You can therefore have top rake on the tool
which makes life a lot easier when cutting steel. Using this method on
my ancient Myford, I quite happily take 20 thou cuts for the first two
or three, reducing thereafter, but only getting down to fiddly little
ones as I approach final size.
Yes, you do need to have a decent dial on the top-slide; a useful
exercise in turning and dividing if you haven't."
Duncan A. Webster
According to Ian :
Well ... you can keep track of your thread depth using the
compound (presuming that it has a dial, of course), if you calculate the
angular infeed needed from the direct infeed. You divide the depth by
the cosine of the infeed angle.
Here are the cosines of several half thread angle infeeds, and the ones
just slightly less as well:
If you have a scientific calculator, you can calculate the
cosine and perform the division quite easily.
If not, I wrote a computer program (in C) which accepts the
thread pitch (both metric and inch) from the command line, and prints
out the following table:
For a thread of: 10.0000 TPI
the pitch is: 0.1000"/thread
| Thread Style
Format | Sharp-V | Trunc | Formed
Single depth: | 0.0866" | 0.0758" | 0.0541"
Double depth: | 0.1732" | 0.1516" | 0.1083"
29.5 deg. angle feed: | 0.0995" | 0.0871" | 0.0622"
Note: Sharp-V is top and bottom sharp. (Not often the best choice.)
"Trunc" is top truncated only.
"Formed" is both top and bottom truncated or rounded.
Select whichever suits your needs and available tooling.
Note that it provides both single depth (workpiece radius) and
double depth (workpiece diameter), in case your lathe crossfeed dial is
calibrated in radius or diameter. It also has different depth values
for sharp V threads (almost always wrong for normal threading),
truncated (reasonable for most work, including with normal multi-pitch
inserts) or formed threads (for single-thread-pitch carbide inserts
which produce both rounded crests and roots.
I've no experience with the Myford. Most of my thread cutting
is on the 12x24" Clausing (angled infeed for thread cutting), and the
Emco Maier Compact-5/CNC, which does its own choice of infeed with the
CNC. I have no idea for sure, though I suspect that it does the
equivalent of angled feed, based on the chips which it forms as it cuts.
But -- presuming that the compound has a dial, it can still tell
you how close you are to finish depth, as long as you calculate the
infeed depth by whichever means is available.
O.K. This is a 30 degree effective angular infeed. Good enough
for imperial and metric threads, but perhaps not quite right if you are
cutting Whitworth threads (55 degree). But the mention of a Merseyside
shipyard would suggest that the common threads at that time would have
And -- you have to remember to feed both the proper amounts --
one more thing to remember.