[HELP] First thread turning.

[EdK]

Here's a link to the metric thread version of the one Russ linked to.

http://www.shender4.com/metric_thread_chart.htm

Ed

[TomG]

Your question is actually rather timely. I was just planning a YouTube video of my own on single point threading because the techniques I see on YouTube are generally overly complex and confusing. I tend to be contrary and do it a bit differently. I’ve been bouncing ideas around in my head for a few weeks and now seems to be as good a time as any to put them to “paper”. Here’s a basic rundown of what I plan to pattern the video after. It's a work in progress, so ignore any typos and be patient because my typing sucks. I'll post it as I it develops, starting with the tool:

The first step if you haven’t cut a single point thread before is to grind the tool. A threading tool is actually easier to grind than a turning or facing tool, but care must be taken to get the 60º angle as close as possible since you are making a form tool and the thread form will only be as accurate as the form of the tool. Since you are making a form tool, the top of the tool must be flat, no back rake is allowed. Therefore, if you are using a lantern type tool holder, the top of the tool must be angle so when it is held in the holder, the top is flat, not angled back. If you use a quick change tool post, just ignore this step. I usually start by grinding the left flank 30º to the side of the tool, adding about 12º of clearance so the cutting edge doesn’t rub, a few degrees more for aluminum or brass. When you grind tools with flat sides, use the entire face of the grinding wheel, moving the tool back and forth to generate the straight edge. And don’t forget to dress the wheel before starting.

Something that needs to be addressed with a threading tool is the helix angle of the thread. If you look at the side of a thread, you’ll see that the thread angles, to the left for a right hand thread and to the right for a left hand thread. This is the helix angle and it must be accounted for in the clearance angles of the tool. In other words, the leading edge of the tool requires slightly more clearance than the trailing edge. This helix angle business is not that important when cutting a 60º V thread, but is critical when cutting an Acme or square thread, so it’s good to understand the concept now. I’ll go into more detail on how to calculate the helix angle for various threads in the video.

Once the left flank of the tool is ground, it’s time to grind the right flank. This angle forms the V shape of the thread and as already mentioned, needs to be as close to 60º as possible. Use an arrow head thread gauge to dial this angle in, holding it up to the light to see. This side of the tool, the trailing side requires slightly less clearance than the leading side to allow for the helix of the thread, about three degrees for common threads.

Now that the right side is complete, it’s time to add the flat. A flat is not a necessity for 60º V threads, but it makes a nicer looking thread and one that is slightly stronger than a sharp V. The flat is ground or stoned (it’s very small) square to the shank and the width should be 1/8 the pitch of the thread, or less. For instance, the flat for a thread that is 16 threads per inch is (1/16)8=.008”.

[Sunset Machine]

Just to add a bit about feeding in at an angle. You mentioned the helix angle; feeding straight in results in a negative rake on the right flank which will probably cause problems with surface finish on lighter machines turning coarser threads in poor materials. It's reduced by feeding in at slightly less than 30 degrees. Unfortunately, there seems to be a discrepancy between lathe manufacturers as to what that actually means on the compound, but the object is to feed nearly parallel to the trailing flank of the toolbit.

Also, it seems to me a back rake in the tool bit can be compensated for with a greater than 60 degree form. The math required escapes me, but I would expect an improved finish from a shearing effect although I've never attempted it.

[TomG]

Sunset,

The text that follows should clear up point number one.

Any back rake on a form tool will affect the shape of the form. Yes, you could adjust (increase) the 60º angle to compensate, but it would only be an approximation and the straight flanks of the thread would start to curve since all of the form tool is not the centerline of the work. Certainly a few degrees wouldn't hurt, but I would recommend any more. I've never had any problem getting good surface finishes with a flat top form tool so it's probably not worth worrying about.

Ok, on to part II. A lot of this stuff will be much easier to visualize with the video so hang in there and I'll get it cranked out as soon as possible.

Tom



Now that the tool is ground, let’s set up the lathe.
Set the compound rest angle to 30º. Let me repeat: Set the compound angle to 30º. Not 29º, not 29 ½º, set it to 30º. When the tool is held to the work, the right side of the compound should be parallel to the right side of the tool. I mention this because on some lathes this setting is called 60º, not 30º. Now I know this statement is going to ruffle a few feathers because “they” always tell you to set the compound to 29º when threading, or that’s what it says in the book, or that’s the way I was taught in school. My response is that you wouldn’t have been taught that way if you had me for an instructor because setting the compound to anything other than 30º is confusing, unnecessary and inefficient. I’ll explain why later.

Next, mount the part to be threaded and align the tool to the part. The top surface of the tool needs to be on the centerline of the part, not above or below, it should be on dead center. This is easily accomplished by lining it up to the point of a dead center. The tool also needs to be perpendicular to the part. This is accomplished with the arrow head thread gauge. To make the alignment process easier to see, place a piece of white paper under the part and move the machine light down so it illuminates the paper, but not the top of the part. This creates a nice silhouette of the tool and parts and makes it very easy to see when all is aligned. Place the arrowhead gauge against the part and align one edge of the tool to the gauge. Don’t jam the tool into the gauge, because that will damage the gauge. Once the tool is aligned, run it in with the compound and cross slide until it just touches the surface of the part and set the dials to zero, making sure all backlash is removed from the screws.

Now go ahead and set the lathe to cut the required number of threads per inch. I won’t go into detail on this because every lathe is different and you’ll just need to figure out how to do that on your own. Since we are going to be cutting a right hand external thread, the tool must feed toward the headstock, with the spindle turning counter-clockwise. If you wanted to cut a left hand thread, the tool would feed toward the tailstock, so set the feed direction lever accordingly. Also set the rpm to about half the speed you would normally turn or less depending on your confidence level at operating the lathe. A faster speed will create a better finish but a slower speed will be easier to start and stop the tool in the right place.

It’s time to make chips, albeit small ones. Before actually starting to cut the threads, it’s always good to take a trial cut to be sure that everything is set up properly. Position the tool to the right of the part and advance the compound a few thousandths. But before we get rolling let’s talk about the half nut and chasing dial. The half nut is used to engage and disengage the lead screw and the dial gives you control over where the tool starts and stops feeding. The numbers on the dial tell you where to engage the half nuts to start the feed so you don’t end up cutting a thread on top of a thread (bad). The basic rule is as follows:

1) For an even number of threads, the half nuts can be engaged on any mark or number.
2) For an odd number of threads, they must be engaged on any number.
3) For a half thread, they must be engaged on any opposite number, 1 and 3 or 2 and 4.
4) For quarter threads they must be engaged on the same number.
5) If the thread being cut is a multiple of the pitch of the lead screw, the half nuts can be engaged at any position.

Start the spindle and engage the half nuts on the proper line of the chasing dial as required by the thread you are cutting. When the tool reaches the end of the thread, disengage the half nuts, retract the tool with the cross slide and return it to the starting position. Now check the lines the tool created to be sure they are the proper spacing for the thread you are cutting. The distance between the lines is the lead of the thread, which is simply one divided by the number of threads per inch.

Continue taking progressively deeper cuts using the compound, with the cross slide re-set to zero, until the V thread form starts to become visible. The upside of feeding with the compound is that only the left side of the tool cuts, the right side just slides parallel to the right flank of the thread. This puts less of a load on the tool while roughing out the thread than if it was being fed with the cross slide. The downside is that the compound does not directly read the diameter of the thread, so it must be calculated, which is why I only use the compound for roughing, this is where my technique differs from the traditional method.

When the thread starts looking like a thread it’s time to take a measurement. The width of the flat or crest on and external 60º V thread is ¼ the lead of the thread, or double the width of the flat on the tool. Watching this flat develop gives you an idea of how far along the thread is and when it’s time to measure. A thread is measured by checking its pitch diameter, which is midway between the theoretical crest and root of the thread. The pitch diameter is readily available for whatever class of thread you are cutting in thread charts such as those found in the Machinery’s Handbook. Common methods of measuring this diameter are the three wire method, or better yet using a thread micrometer. Once you determine how much oversize the thread is, it’s time to switch to feeding the tool with the cross slide instead of the compound. This has several benefits; since the cross slide dial reads diameter directly, there is no guesswork or calculation required to determine how much material to remove as there is with the compound. A second benefit is that by moving the tool straight in, the tool cuts on both flanks, thereby copying the shape of the tool and cleaning up the right flank of the thread.

Move the cross slide in, stopping a few thousandths shy of the finish diameter and make a few passes without changing its position. This removes any spring in the set-up and allows a final reading of the pitch diameter to be made. Move the tool in the final amount with the cross slide and make a few finish passes to complete the thread. If you are confident in your ability, the spindle speed can be increased for a better finish.

This method eliminates any confusion about how to set the angle of the compound, makes it much easier to measure the pitch diameter of the thread without having to make calculations and produces a very accurate thread form, or at least as accurate as the tool used to cut it.

That’s all there is to it single point thread cutting.

[marfaguy]

ieezitin,
Thanks. I've enjoyed his whole series on machining, in fact watching him and Myfordboy's videos is what got me
interested in the first place.

Russ,
Thanks for the links, much appreciated.

Tom,
I really look forward to your upcoming tutorial.

All,
I went ahead and gave it a shot Sunday. Here's the results.
I took Tom's advise (I had seen this done in numerous video's but had forgotten about it) and did a scratch run first just to
check the TPI count. It was dead on at 16.
I also took ieezitin's advice and once I got close but the nut wouldn't quite fit, I ran a die down it to bring it to final size.
Cheating maybe but I wanted this first try to succeed.

Anyway as the saying goes, pics or it didn't happen.

[wrustle]

Congrats pal! You are no longer a single point threading virgin!!

[Mayhem]

[stevec]

See what a snore it is? Congrats!

[TomG]

By the looks of that thread you don't need no stinking tutorial.

Tom

[DaveH]

Well done, nice looking thread

DaveH