Thread cutting (lathe) help!

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?
Thanks...Jon.
Reply to
Jon Eiserling
Loading thread data ...
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.
Reply to
Jim Stewart
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.
Jim
Reply to
jim rozen
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.
Reply to
Tim Wescott
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 adjustable. 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 Cheshire. Regards, Ian
Reply to
Ian
Got it!...Works perfectly. Thanks Jim & Jim
Jon
Reply to
Jon Eiserling
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:
Angle cosine ==================== Unified/UNC/UNF 30.0 0.8660 29.5 0.8704 Whitworth 27.5 0.8870 27.0 0.8910
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 been Whitworth.
And -- you have to remember to feed both the proper amounts -- one more thing to remember.
Enjoy, DoN.
Reply to
DoN. Nichols
Sounds like your lathe compound is marked "the other way around" . Try setting the compound to 60 deg. That is the way our Clausing/Metosas are. ...lew...
Reply to
Lew Hartswick
That's great.
I think the compound graduations on my 10L southbend work backwards that way. Makes a fella have to look twice.
Jim
Reply to
jim rozen

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.