Calculated Thread Depths for Metric fine threads

[madman]

Guys I am having a dilemma, Haven't done all that much Threading last few years. I need to make a M12 x 1.125 internal thread in some stainless steel 304 Material. I do NOT have a mating part and am working in a different shop away from all my tools and books ect. Is there a calculated depth of engagement to touch of the 60 degree thread tool and then feed a specific amount for a perfect thread so to speak? I'm wondering how to do this without a mating part which I don't have? Thank-you as always Mike NO I don't have a tap that would be too nice and easy..

[Black Forest]

Do you have a full profile lay down type external theading insert of the right size. You could make your own go no go gauge. Not what you asked but maybe a solution.

[dp]

Metric thread depth is 0.614 x pitch.

As an aside, for imperial threads where the compound is set over 30؛ the advance for the compound is 1/pitch as read on the compound dial.

[madman]

Thanx One More Question

Metric thread depth is 0.614 x pitch.

As an aside, for imperial threads where the compound is set over 30؛ the advance for the compound is 1/pitch as read on the compound dial.

I been reading over \posts on thread depths. \is this constant .614 a straight in dimension or with compound turned 29 degrees or??? Thankyou this helps me immensely . Appreciate you're time . Mike

[TGTool]

For jobs like that I'm always more comfortable making the external thread to check my internal which is otherwise hard to measure. With a male thread I can use thread wires to see that I'm in the right tolerance range, then use that to test fit.

[Yow Ling]

Cant you just buy a 12mm bolt ?

[madman]

No 12 mm by 1.25 is a fine metric perhaps a 12 mm sparkplug would be \ok but where \i am \frozen \tundra) I have no access to anything no bolts or nuts like this. The MOW for this thread is??? Ive never used thread wires as \ive not done hardly any threading like this \job ever . \this is my first one ,should be fun and \i appreciate the assistance and \help \guys \thanx \mike

[Davidhcnc]

Is that a mistake in the 1st post? M12 x 1.125 does not exist in real life.


12 x 1.25 does.

If you could procure a M8 x 1.25 which is a standard metric bolt then you could study the thread depth etc and work out the numbers you need.



'Is there a calculated depth of engagement to touch of the 60 degree thread tool ' yes, look at the drawings in the link

http://en.wikipedia.org/wiki/ISO_metric_screw_thread

[dp]

I been reading over \posts on thread depths. \is this constant .614 a straight in dimension or with compound turned 29 degrees or??? Thankyou this helps me immensely . Appreciate you're time . Mike

That is a straight depth of cut. To get the infeed depth on the 30؛ compound you multiply by cos(30) or 0.866. It is also measured in mm. If your dial is in inches then you need to convert mm to inch.

[Paul Alciatore]

You can calculate the theoretical depth of any thread but there is a real problem in using it to cut as real thread. It is very hard to know the exact amount of the difference between the actual tip of a real cutting tool and the theoretical location of the tip of a sharp vee. And that amount must be subtracted from the theoretical depth based on a sharp vee. Or if you have a thread depth based on some particular amount of reduction from the sharp vee form, then you must verify that your tool has exactly that amount of reduction or you must include that difference in your calculation.

Can you grind a tool with a precise amount of tip reduction due to a flat or a radius? How close can you come? Can you measure the actual position of the tip of your actual tool? If you use a commercial insert, how accurate is the radius or flat on it? Is there a stated tolerance on that figure?

Using a thread depth will get you close, but you still have to measure. Thread gauge, thread mike, three wire, mating part, something; you still have to measure and verify your thread. Perhaps your thread is not a high accuracy one and you can use a loose tolerance. That means that you cut deep enough to ensure that it will fit even if all the tolerances add up in the wrong direction.

Since you are away from your tools, I will offer this with no guarantee:

Based on M12 x 1.125 and Sharp Vee tool:

Since this is an internal thread, you must first determine the bore size you are going to use. Rule of thumb for a 75% thread of any pitch, metric or otherwise, is Diameter - Pitch.

12mm - 1.125mm = 10.875mm

That's going to be a hard drill to find. If you have access to inch size drills, that translates to 0.428". That's around 27/64". Since you are single pointing these threads, you can go with a smaller hole than this. Anything between 10.6 and 10.9 mm will probably be OK. I don't know what drills are available where you are so I will go with 10.75mm which is almost exactly 27/64" (0.0013 larger than 27/64" actually). Since it is important to start at a known ID, I would suggest drilling a bit smaller and boring it out to exactly 10.75mm.

With a 10.75mm bore, you will need to move your SHARP VEE tool out far enough IN A RADIAL DIRECTION to bring the flat of the thread (which does not exist on that sharp vee tool) to the 12mm nominal OD size of the thread. Thus the tip of that sharp vee tool will be at a greater diameter than 12 mm. The metric standard thread has a 1/8 h flat on the tip of the threads where h is the height of a sharp vee thread.

Height of a sharp, 1.125mm pitch thread, h = 1.125mm x cosine(30) = .974mm.

And 1/8 of that is 0.122mm.

So we are going to need to move the tip of our sharp vee tool out to a diameter of

12mm + (2 x 0.122mm) = 12.244mm

We are starting (touching off) at 10.75mm and going to 12.244mm

12.244mm - 10.75mm = 1.494mm

But that is on the diameter and we are moving on the radius so we need only half that amount:

1.494mm / 2 = 0.747mm (0.0294")

You can use that if you are moving out using the cross slide.

If you are using the compound set to 29.5 degrees then that amount would be increased to

0.747mm / cos(30) = 0.863mm or 0.034".

That would be a theoretical thread size. Since you have no way of testing it, I would recommend that you cut just a bit further to ensure a fit. Perhaps another 0.025 or 0.050mm or one or two thousandths more.

I would greatly appreciate it if someone else here would check my math on this.

[Juergenwt]

This is a tough one. Not much experience, in the middle of nowhere, no thread wires. Do you have a 60 deg. threading insert? If not - you will have to grind a HSS bit to 60 deg. Put (stone) a very small radius on the tip. Turn your material down to 11.9mm. Forget about feeding in on a 29 1/2 deg angle and feed in straight. 1.25 is a fine pitch and should not give you a problem.
Your pitch dia is 11.188. Your root dia is 10.466mm. Since you have nothing to go by - I would just tough the 11.9 mm outer dia and slowly start feeding in and cutting 0.1mm at a time untill you are 0.767 deep/side. Run the last cut at least 2x. Caution: your dial will most likely show the total stock removal on the dia. In that case you need to dial in 2 x .767 = 1.534mm
Good luck.

12mm minus 10.466 = 1.534 double depth
1.534mm div. by 2 = 0.767

The extra 0.1mm you removed from the outer dia should give you enough clearance for your screw to fit.

[John Garner]

madman --

A backwoods approach to single-pointing an internal screwthread: First drill your hole for threading. In the absence of a drawing requiring a specific hole size, I'd use the "Tap Drill Diameter = Major Diameter - Pitch" rule of thumb. Then counterbore the hole to (Major Diameter + 0.05 millimeter) x 1 Pitch deep. Using a toolbit with a correctly-sized flat tip (1/8 x Pitch for an internal thread), start threading the inside of the drilled hole, and stop feeding when the toolbit tip just starts to scratch the ID of the counterbore.

John

[danlb]

Single point threading with a sharp V is relatively easy. If the tool has a sharp tip you can use the formula to determine exactly what depth to make it. If you stone the tip to put a radius on it, you lose that reference point.

Paul A did a good writeup. In the future, you can also use use the threading calculator at http://www.tanj.com/cgi-bin/tpi.cgi to find out what the major and minor dimensions are, as well as how deep the threads are.


Dan

[oldtiffie]

Never mind the depth of cut as calculated for an internal thread.

Drill/bore the root diameter and start cutting the thread until the "flat" (on the bore) is 1/4 x pitch ( ie 0.25 x pitch).

Do it "by eye" - you might be surprised at how accurate (for practical purposes) it is.

http://upload.wikimedia.org/wikipedia/commons/thumb/4/4b/ISO_and_UTS_Thread_Dimensions.svg/2000px-ISO_and_UTS_Thread_Dimensions.svg.png

https://www.google.com.au/search?q=metric+thread+form&biw=1536&bih=732&tbm=isch&tbo=u&source=univ&sa=X&ei=p63aVJ_oOOLemAWRwYKIBw&ved=0CCMQsAQ&dpr=1.25

https://www.google.com.au/?gws_rd=ssl#q=metric+thread+form

[dp]

You can calculate the theoretical depth of any thread but there is a real problem in using it to cut as real thread. It is very hard to know the exact amount of the difference between the actual tip of a real cutting tool and the theoretical location of the tip of a sharp vee. And that amount must be subtracted from the theoretical depth based on a sharp vee. Or if you have a thread depth based on some particular amount of reduction from the sharp vee form, then you must verify that your tool has exactly that amount of reduction or you must include that difference in your calculation.

The width of the flats of the internal and external threads is precisely described. For an external thread the flat for the minor diameter is P/4 and the flat for the major diameter is P/8. This is inverted for internal threads. Everything is derived from the pitch. Note too the asymmetry in the flat widths. This is because the thread is not cut symmetric about the pitch diameter. This defines the form of the cutters needed to cut internal and external threads. A sharp vee cutter is not used nor defined in the standard. That hasn't stopped anyone from doing so.

The height of the thread is defined as the distance between the points when the thread is drawn and the specification requires H = cos(30) * P and is yet another dimension derived from pitch. The points are imaginary and are located outside the actual thread. The thread depth is precisely described in the standards and is Dmaj - Dmin. Dmaj is given in the designation of the part eg, M8x1.25 defines Dmaj as 8mm. Dmin = Dmaj - 2 * 5/8 * H = depth of thread.

So we have the major diameter and the pitch as starting points. We quickly calculate H and Dmin and we're ready to cut. Except the thread cutting tool is a form tool and we have to address that. There's one more problem to solve and that is the clearance at the thread root. Some clearance is required outside the dimensions of the thread. This clearance area is not part of the thread itself. From reading above we see that for an external thread the thread width at Dmin is P/4. Using a sample M8x1.25 thread the minor diameter flat will be 1.25/4 == 0.313mm. So we grind our perfect 60؛ cutter to a fine point then grind the tip off until it is 0.313mm in width. Except that leaves nothing for the clearance. So we use our optical comparator to locate the P/4 line on the cutter tip and grind a slight radius that fits the P/4 line.

Nothing left but to cut the thread.

Edit: Forgot to add this - including the clearance, the depth of cut will be 0.614 * P which means you can ignore everything else in this thread if you use threading inserts.