Threads not deep enough

[rronald]

If you cut that long thread, you do need to support the part using the tail stock. If you don't, you will need to cut deeper and the nut will have more play towards the chuck.

The cutting depth depends on the tool. There is a lot of difference if you have a sharp ground HSS tool, a ground HSS tool with a tool nose radius, a half profile insert or a full profile insert.
If the half profile insert has a minimum pitch that is larger than the required pitch, you also need to cut deeper. If the half profile insert has a maximum pitch that is smaller than your pitch, you have to cut a lot deeper.
If the full profile pitch is less than you pitch you have to cut a lot deeper.
If you use a ground tool without a tool nose radius, you have to cut deeper but that is something you can calculate.
If you use a ground tool with a tool nose radius, you can only guess how deep to cut.

Check the thread depth using the 3 wire method. Any 3 wires will do if they have the same diameter and aren't to thin or to thick. The shaft of a drill will do well. Glue them on the thread using some thick grease and measure the diameter using a micrometer. There are web sites where you can find the requested diameter like this one. More info about 3 wire thread measuring.

If you can read the thread charts, know the tool nose radius of the threading tool and are comfortable using CAD, you can draw the thread and the tool in CAD to find out how deep to cut the thread.

Last year I start skipping the cleanup (spring) passes that you really need to do and cut the threads 0.02 mm deeper (adjusted the tool length). Now the threads fit without cleanup (spring) passes. So I do not have to worry about work hardening any more.

I did drill a hole for a center, but changed my mind and did w/o it. And the cut seems consistent along the length, But, I wouldn't go any longer w/o support and I wouldn't have done it this time if I'd noticed the lack of support impacting the amount of cut. I could be dead wrong too!

I'm using a 11ER insert 60 degree thread cutter in a SER holder. There's a visible radius. It's a "partial profile" type.:

 

[rronald]

Yes .

If the minor diameter is unimportant...perhaps the insert requires making the minor diameter smaller than spec to hit the proper pitch diameter?

That would be a satisfying answer for me since it would explain why I have to cut more than expected.

 

[mmcmdl]

That is an awful big nose radius for a threading tool for an 18 pitch thread . Better off with a dead sharp tool . Look up double depth for lathe threads , it'll help you out .

Information On Double Depth As On A Fishtail Gauge

Can someone explain to me how to use the numbers that are printed on a fishtail gauge used for single point threading? From what I can understand, the double depth is listed. Are these numbers used to determine how much you would need to turn in the compound at 30 degrees? Are these numbers...

www.hobby-machinist.com

 

[GT-6 Racer]

Drove myself nuts with this one on the CNC lathe when swapping threading tools to sharp points from partial profiles to full profiles. On the manuals I just do like mmcmdl suggested get it close and run a good Little Giant die down it. But when running many parts on CNC you need to get it right. Machinery Handbook is the source. You will need to do the math. Make sure you account for the angle of the compound on manuals. My CNC canned cycles for threading have some expectations for profile. Just measure the nose radius and make sure you fit the cycle expectations and it gets within a few thou…. Then tweak, On the manuals, if doing multiples sneak up on the first one. Once you get it, note the compound dial reading and just repeat. One can also use a dial indicator to repeat the zero.

It gets easier the more you do ! Have fun

 

[Ischgl99]

That is an awful big nose radius for a threading tool for an 18 pitch thread . Better off with a dead sharp tool . Look up double depth for lathe threads , it'll help you out .

that looks like a stock photo, so probably not the insert he is actually using.

If the minor diameter is unimportant...perhaps the insert requires making the minor diameter smaller than spec to hit the proper pitch diameter?

That would be a satisfying answer for me since it would explain why I have to cut more than expected.

The minor diameter is not unimportant, but it only is part of the thread specs to make sure it fits. You need to make sure it is correct so that the internal thread will fit, but you can’t use it to determine if you are at the right depth. I use the minor diameter to determine when to start measuring the pitch diameter. I know with my tools that I will need to go a bit past that due to the cutting tool/insert point, so if I measure once I advance to the maximum minor diameter, I will still be good and can see how much further to reach the upper end of the pitch diameter, measure again and then make passes to reach my PD goal.

This link shows the thread geometry, you can see the point of a sharp tool vs the minor diameter and what the thread width is at that point. The inserts you are using don’t come to a sharp point, but are for a range of thread sizes, so might be right for the smallest pitch, but too sharp for anything bigger, requiring you to go deeper.

ANSI External Screw Threads Size Tolerances Chart

ANSI/ ASME EXTERNAL Screw Thread Size Chart. All units are in inches. Unified Screw Threads per. ANSI/ASME B1.1-1989 (R2001), R2001) Nomenclature, are used. Acceptability criteria are described in ANSI/ASME B1.3M-1992 (R2001).

www.engineersedge.com

 

[mmcmdl]

The minor diameter is not unimportant, but it only is part of the thread specs to make sure it fits.

I'll reword that . As long as the minor D is under the max spec , it isn't important . Using a sharp v tool , you do go under the minimum spec often . If you use the minimum minor diameter as an undercut groove , a sharp v tool will cut into that groove before reaching pitch diameter occasionally . We used Kennemetal Top Knotch inserts without radii , maybe .002 max . But as I said , the minor diameter is only clearance for the internal thread . In 48 years , I've never had a QC inspector even look at the minor diameter , and this was DoD work .

 

[mmcmdl]

Drove myself nuts with this one on the CNC lathe when swapping threading tools to sharp points from partial profiles to full profiles.

What I loved about the G76 cycle was on these parts where L over D was too much but could program a nice little taper into cycle .

 

[Ischgl99]

I'll reword that . As long as the minor D is under the max spec , it isn't important . Using a sharp v tool , you do go under the minimum spec often . If you use the minimum minor diameter as an undercut groove , a sharp v tool will cut into that groove before reaching pitch diameter occasionally . We used Kennemetal Top Knotch inserts without radii , maybe .002 max . But as I said , the minor diameter is only clearance for the internal thread . In 48 years , I've never had a QC inspector even look at the minor diameter , and this was DoD work .

I don’t think anyone really cares about the minimum minor diameter, even with sharp v tools, it has a limit to how deep it can go and still hit the PD tolerance. Except maybe the Germans, they have a spec for everything

 

[ChazzC]

Also remember to take a (or several) spring passes after your final cut: the DRO indicates where the tools is, but can’t account for deflection.

 

[rronald]

Amazon brought me some thread wires today. It still amazes me that I can buy something that is incredibly specialized (like thread wires) and get them in a day (or even less if I were willing to pay $3.99 to get it by 8AM).

So, I used one of the online calculators for the three wire method and it said to use the ,032" wires and that the measured thickness of bolt and wires should be .5743".

I measured .5732 (the last digit is definitely a guess). I call being just over a thousandth off as a great victory. Especially given that my only measuring tool was a nut. And that nut happened to be the one holding down the QCTP....so each time I trial fitted it, I had to remove it from the QCTP, attempt to spin it onto the bolt I was cutting, and then return it to the QCTP without changing the position of the tool-post.

I had a lot of trouble the first time I measured with the wires. The bolt being measured was handheld, so I had to hold the bolt, the wires, and the micrometer.

I repeated the measurement a second time and (IMHO) made several improvements.

1. Don't be a knucklehead and hold the threaded part being tested in your hands! I stuck it back into the collet on the lathe.
2. All the pics I see for the three wire method show the two wires under the thread being measured and the single wire on top. Seems silly to me. You can see the harder side of the problem if the double wires are on top of the thread.
3. found it far easier to install the two wires on top and close the micrometer on them w/o worrying about the third wire. Don't even pick that one up until the two side-by-side wires are (lightly) clamped in place by the micrometer.
4. It's then easy to loosen the micrometer a tiny bit-just enough to slide in the single wire.

Thanks to all for the help! While I was able to cut a thread before, it was mostly due to luck and lot's of trial and occasional error. Now, I think that I'm armed with enough information to cut external threads reliably.