# Threading - 29.5/30 vs 90



## Susquatch (Jun 10, 2022)

Since the very beginning of my machining experience on a lathe, I have always done 29.5 degree threading. I thought everyone did it this way. But I recently learned from @gerritv that while this practice is mostly common in North America, the rest of the world normally cuts their threads using a 90 degree plunge cut. Apparently the rest of the world handles the increased chip load by reducing the depth of cut as the threading tool is advanced.

This global difference bothers me so much that I have created this new thread to discuss it with my fellow members.

The idea behind the 30 degree cut is to cut on just one face of the 60 degree tool and slide along the other. Cutting on only one face reduces the chip load on the tool by half. Sometimes this leaves a rough chattered surface on the sliding edge. Rarely, it can even leave a bit of a staircase effect. The idea behind the 29.5 degree cut is to cut the normal 30 degree plus a little 1/2 degree shave off of the other surface to clean it up and eliminate the possibility of any staircasing. I have no idea how the 1/2 degree was decided. I do know that it is not critical.

When plunge cutting at 90 degrees, this 1/2 degree difference is not needed because both edges cut all the time. As stated above, the increased cutting load from cutting on both edges is reduced by gradually reducing the depth of cut as the tool is advanced in order to maintain a constant chip/cutting load. I also think it's rather obvious to me that chip loading is not a concern for small fine threads.

At first, I accepted the global difference as just another example of common practice differences. Perhaps even like metric VS imperial.

But I slept on the matter last night and I came to realize that there is another potential difference that "might" be important. And it further occurred to me that there may be other factors at play that I have never considered or perhaps never even heard of. 

Most of us don't have tool room grade or cnc lathes. Many of us have old lathes that are well worn. Some of us have low cost machines that were never intended for high precision use. One of the most common wear items is the leade screws. We learn early on to accommodate leade screw backlash by loading the leade screw in one direction only. Essentially, this keeps the tooling indexed against the pressure/loaded side of the leade screw which greatly reduces the effect of any backlash.

In a plunge cut, the vast majority of the load is radial and there is very little side loading of the leade screws. Most of the tool locating forces are generated by the tool profile - essentially the tool mostly follows the groove.

On the other hand cutting on the side of a tool creates higher side loads which should increase the load on the leade screws and thereby ensure that there is no backlash affecting the path of the tool.

Basically, I am suggesting that another reason for cutting a thread on just one face of the tool (the 30/29.5 practice) might be to improve the geometric precision of the thread by using the cutting forces to reduce the backlash effect. I realize that much of the backlash is taken up purely by the sideways movement of the tool. But I also think this isn't as reliable or as consistent as higher side loading might provide.

For me, perhaps the most compelling argument to the contrary is the Sandvik recommendations wherein they provide a chart of tool advancement settings for each thread settings for cutting at 90 degrees. This clearly supports the practice of plunge cut threading at 90 degrees. But perhaps their recommendations are for professional use with cnc machines or tool room lathes - not potentially well-worn sloppy hobbiest lathes.

I am hoping that some of the other members here have more experience and knowledge on the matter than I do and can help sift through the pros and cons of 30/29.5 degree threading VS 90 degree plunge cut threading. Is it really just a matter of choice or are there compelling reasons why we should prefer one method over the other?

What do you folks think?


----------



## 6.5 Fan (Jun 10, 2022)

I'm in the 29.5 degree camp, it's what i was taught and have used very effectively 35+ years of steel butchering. I'm going to try the 90 degree threading on the new lathe i have to see for myself what all the fuss is about.


----------



## Susquatch (Jun 10, 2022)

For reference, here is a copy of the Sandvik infeed recommendations for imperial external threads cut at 90 degrees as provided by @gerritv in another thread. It shows the variation in cutting depth as the threading progresses.


----------



## thestelster (Jun 10, 2022)

Susquatch said:


> For reference, here is a copy of the Sandvik infeed recommendations for imperial external threads cut at 90 degrees as provided by @gerritv in another thread. It shows the variation in cutting depth as the threading progresses.
> 
> View attachment 24396


Those infeed recommendations are accurate IF you use the corresponding topping threading insert which have the crest and root sections set on that insert.  If you use a non-topping insert, or a HSS tool which you have ground sharp, the final depth recommended will not be deep enough.  You will then have to either go deeper or go axially by a certain amount with the cutter to produce the correct pitch diameter.


----------



## Susquatch (Jun 10, 2022)

thestelster said:


> Those infeed recommendations are accurate IF you use the corresponding topping threading insert which have the crest and root sections set on that insert.  If you use a non-topping insert, or a HSS tool which you have ground sharp, the final depth recommended will not be deep enough.  You will then have to either go deeper or go axially by a certain amount with the cutter to produce the correct pitch diameter.



This is an interesting observation @thestelster. In the other thread, I had speculated that these infeeds and perhaps even the whole 90 degree feed approach might be specific to the Sandvik inserts. You have answered half the question with your discovery. Those in feeds do indeed appear to be specific to the Sandvik threading inserts of that profile. But I doubt this means that the 90 degree method only applies to Sandvik. In fact, @gerritv linked a video demonstrating the 90 degree method using a HSS threading tool by Gotteswinter. I've repeated Gerrit's link here for convenience. Hope you catch the irony - it may be the last YouTube video you will ever see me post...... But then again, it's only a repost! LOL! 

The start of the video shows him making a, custom change gear. I confess that this was actually worth the painful watch.... The actual threading starts at 31:25.


----------



## thestelster (Jun 10, 2022)

thestelster said:


> Those infeed recommendations are accurate IF you use the corresponding topping threading insert which have the crest and root sections set on that insert.  If you use a non-topping insert, or a HSS tool which you have ground sharp, the final depth recommended will not be deep enough.  You will then have to either go deeper or go axially by a certain amount with the cutter to produce the correct pitch diameter.


For properly shaped thread profiles, you are advised to have a separate insert for each thread profile and pitch.  I cannot afford all those inserts, so I use a non-topping insert, which can do many pitches, and set my compound to feed axially, and will do the infeeds with the cross-slide to the Sandvik recommended total infeed, test for fit, or measure pitch diameter.  And if I need to reduce pitch diameter, I feed using the compound until the corresponding component threads nicely, or have reached the proper pitch diameter.

Also, by having the compound set axially; once I have reached the designated in-feed, according to the Sandvik tables, I will use the compound to take a thou or two off the back side of the thread to clean it up, and then move in towards the chuck, 1 thou per pass.


----------



## VicHobbyGuy (Jun 10, 2022)

Susquatch said:


> For reference, here is a copy of the Sandvik infeed recommendations for imperial external threads cut at 90 degrees as provided by @gerritv in another thread. It shows the variation in cutting depth as the threading progresses.


One look at that table tells me that those depth of cut recommendtions are NOT for my 'toy' 7x14 lathe! 

For mini lathe users, there's another 'angle'  to this topic: Which is going to produce a smoother cut with less chatter and inaccuracy - a 29.5 cut using the compound, or a plunge cut with the compound removed from the lathe and replaced by a solid block (a.k.a. plinth) of metal?


----------



## Susquatch (Jun 10, 2022)

thestelster said:


> For properly shaped thread profiles, you are advised to have a separate insert for each thread profile and pitch. I cannot afford all those inserts



For those few times I considered carbide inserts for threading, I've always seen them advertised and specified for a range of TPI. Even my loveable ARWarner HSS Inserts have a range. But I always thought it was for the back angle more than for the root. 

Like you, there is no way I'm going to buy a separate insert for every thread pitch out there.


----------



## YYCHM (Jun 10, 2022)

Good topic!

I've always been skeptical that setting the compound to 29.5/30 accomplishes anything when you still set the tool to 90 with the tool post.   I abandoned 29.5/30 and just left my compound set to 90.  So how does this 29.5/30 thing work?


----------



## thestelster (Jun 10, 2022)

So here is an example of Sandvik Top-Lok inserts.  Using the TLTC 3R Topping insert, to cut a 12tpi thread.  The nose radius is, which will shape the root of the thread, is 0.010".  We would need to in-feed 0.054" into our material to make our 12tpi thread.  But if we use the non-topping insert TLT 3R to cut the same 12tpi thread, the nose radius of that insert is .005-.008".  (Between .002-.005" less).  Therefore, if we feed into our material 0.054", the pitch diameter is off, (too large).  We would need to widen the root of our new thread between .002-.005", by moving either axially, or by going deeper than the 0.054" that was recommended by Sandvik to get the correct pitch diameter.


----------



## 140mower (Jun 10, 2022)

YYCHM said:


> Good topic!
> 
> I've always.  been skeptical that setting the compound to 29.5/30 accomplishes anything when you still set the tool to 90 with the tool post.   I abandoned 29.5/30 and just left my compound set to 90.  So how does this 29.5/30 thing work?


Well........ I guess I am one of those calves the was born against the electric fence and therefore never knew it was wrong.....
I have always set my compound to 29.5, touched off with the crosslide and zeroed that dial. My infeeds are with the compound, but when I reach the end of the thread I quickly retract the compound while releasing the halfnuts. Wind the carriage back to the starting point, wind the cross slide back to zero, and add more cut with the compound. I'm not good with the math to figure out how much infeed is required at that angle to reach the required depth, so I have always just gone until the thread fit..... So far I have been happy with the results. 
For everything we do, someone will come along with a bigger better idea, but so long as what you are doing works well and doesn't cause great frustration, then that's the method for you, or me..... If you can believe it, I have heard that some people actually try and use their left hand when they write..... Sheesh, doesn't anyone care enough to correct them?......
 ......... Rapidly digging fall out bunker......


----------



## thestelster (Jun 10, 2022)

140mower said:


> Well........ I guess I am one of those calves the was born against the electric fence and therefore never knew it was wrong.....
> I have always set my compound to 29.5, touched off with the crosslide and zeroed that dial. My infeeds are with the compound, but when I reach the end of the thread I quickly retract the compound while releasing the halfnuts. Wind the carriage back to the starting point, wind the cross slide back to zero, and add more cut with the compound. I'm not good with the math to figure out how much infeed is required at that angle to reach the required depth, so I have always just gone until the thread fit..... So far I have been happy with the results.
> For everything we do, someone will come along with a bigger better idea, but so long as what you are doing works well and doesn't cause great frustration, then that's the method for you, or me..... If you can believe it, I have heard that some people actually try and use their left hand when they write..... Sheesh, doesn't anyone care enough to correct them?......
> ......... Rapidly digging fall out bunker......


Don, you are right on the money.   Many different methods to get the same results.  Use the method which is most comfortable to you that nets the required results.


----------



## Susquatch (Jun 10, 2022)

VicHobbyGuy said:


> One look at that table tells me that those depth of cut recommendtions are NOT for my 'toy' 7x14 lathe!
> 
> For mini lathe users, there's another 'angle'  to this topic: Which is going to produce a smoother cut with less chatter and inaccuracy - a 29.5 cut using the compound, or a plunge cut with the compound removed from the lathe and replaced by a solid block (a.k.a. plinth) of metal?



Hmmm..... I don't think that is really a fair question. Better to ask about 90 vs 30 on your lathe with no plinth. 

Now if what you are saying is that a 30 cut does not permit a plinth, and the 90 approach dies allow you to go to a plinth to achieve better rigidity, it's a fair comment.  But it's not really comparing 90 to 30. It's more like comparing plinth to no plinth.


----------



## Tom Kitta (Jun 10, 2022)

I always cut 90 deg in. simple, fast, easy, no issues. For smaller threads, when possible, I use a die.


----------



## Susquatch (Jun 10, 2022)

YYCHM said:


> Good topic!
> 
> I've always been skeptical that setting the compound to 29.5/30 accomplishes anything when you still set the tool to 90 with the tool post.   I abandoned 29.5/30 and just left my compound set to 90.  So how does this 29.5/30 thing work?



Too funny! Leave it to you to negate the question!

If I were you I'd stick with what works for you. No substitute for doing what you are comfortable with!

Maybe later I'll draw something up for you to demonstrate how the 30 degree cut works. But it will have wait a while. Where is @PeterT when you need him?

In the meantime @140mower s description of the methods is pretty good. And if my memory is working you are already that lefty he was yacking about!


----------



## jcdammeyer (Jun 10, 2022)

Back when I developed the Electronic Lead Screw this discussion came up a number of times.  I wanted an ELS because I didn't want to wait to build the Gingery shaper and mill and rotary indexer just to be able to cut gears for my Gingery lathe.  The ELS solved that problem.

Once I acquired my South Bend, which had gears, threading was less of an issue until I needed some metric ones.  At that point I added a leadscrew drive and an ELS to it too.  Now it doesn't bother powering the cross feed and is 1942 vintage so has lots of backlash everywhere, even with a new cross slide nut.  Haven't installed the new cross slide screw yet.

Anyway, the ELS is set up to let a user choose the angle of entry regardless of whether it's powered on the cross slide or not.  I set 29.5 because once you cut on both flanks you may no longer be running on the driving edge of the carriage leadscrew.  The load of cutting, although small, still means one edge of the tool is cutting, it doesn't have to be flat so it can have some rake and therefore also cuts better.  The ELS takes care of the angle by either instructing me to move the compound in a certain amount on each pass or if I don't have a compound it changes the X and Z positions so it follows the required angle.  (Which can also be set).

If you have a ball screw with virtually zero backlash on carriage and cross slide then cutting straight in is viable.  But there's extra load and if it's a long shaft, then flex.    The tool bit for the 29.5 is still a 30 degree cut and still set with the threading gauge against the work.  If you sketch it out you can see how the method shaves thread while still creating 30 degree thereads.


----------



## Susquatch (Jun 10, 2022)

jcdammeyer said:


> Back when I developed the Electronic Lead Screw this discussion came up a number of times.  I wanted an ELS because I didn't want to wait to build the Gingery shaper and mill and rotary indexer just to be able to cut gears for my Gingery lathe.  The ELS solved that problem.
> 
> Once I acquired my South Bend, which had gears, threading was less of an issue until I needed some metric ones.  At that point I added a leadscrew drive and an ELS to it too.  Now it doesn't bother powering the cross feed and is 1942 vintage so has lots of backlash everywhere, even with a new cross slide nut.  Haven't installed the new cross slide screw yet.
> 
> ...



My take-away from your post is that you believe there is some merit to the advantages of the 30/29.5 cut to load the leade screw a bit...... Is that fair to say?

I hope so, because that is the thought that prompted me to start this thread in the first place. It would be good to think I'm doing more than just stirring the pot here.

It's also good to think our ancestors knew a thing or two that we may be overlooking in the name of progress.

Please note that I am NOT against 90 degree threading here. I am only seeking to understand the history and the pros and cons of the two methods because I don't like the idea of thinking that our predecessors were all clueless and led so many of us astray for nothing.


----------



## VicHobbyGuy (Jun 10, 2022)

Susquatch said:


> Hmmm..... I don't think that is really a fair question. Better to ask about 90 vs 30 on your lathe with no plinth.


I know the answer to that one. 


Susquatch said:


> Now if what you are saying is that a 30 cut does not permit a plinth, and the 90 approach dies allow you to go to a plinth to achieve better rigidity, it's a fair comment.  But it's not really comparing 90 to 30. It's more like comparing plinth to no plinth.


Not really - I guess I wasn't clear.
Two possibilities for me (I would use 30/29.5 if the compound was installed...):
Plinth (greater rigidity) +90 plunge cut (more cutting force and cut area and likelihood of chatter)
VS
Compound (less rigid) + 29.5/30 cut on one side of tool only (less force, less chatter likelihood)

Pick one if you have a flimsy lathe.  

And, cutting away from the chuck/shoulder is MUCH better for a beginner like me....which I realized when the first threads I recently cut on a lathe in 30 years was a LH thread. So now I cut RH threads with the tool upside down.
YMMV, etc...


----------



## VicHobbyGuy (Jun 10, 2022)

Tom Kitta said:


> I always cut 90 deg in. simple, fast, easy, no issues.


One advantage with using 90 deg is that the depth of the cut is obvious from the cross slide dial - no trigonometry needed!


----------



## Susquatch (Jun 10, 2022)

VicHobbyGuy said:


> I know the answer to that one.



OK, I give. What is the answer to that one?


----------



## Susquatch (Jun 10, 2022)

thestelster said:


> Don, you are right on the money.   Many different methods to get the same results.  Use the method which is most comfortable to you that nets the required results.



So what are YOU most comfortable with @thestelster - 90 or 30/29.5? 

More importantly, why?


----------



## Brent H (Jun 10, 2022)

@Susquatch : here is a PDF for you to have a gander at :


----------



## David_R8 (Jun 10, 2022)

I just do what Tony does...


----------



## Susquatch (Jun 10, 2022)

Brent H said:


> @Susquatch : here is a PDF for you to have a gander at :



A comprehensive read of the document you provided included the following statements:

_Donald of  gingery_machines BBS points out:  “The usual argument against this method (i.e. in favor of setting over so you're feeding effectively parallel to one face) is to avoid the cut material from both sides of the tool bit from crowding; this crowding causes an increase in pressure and can lead to chatter or digging the cut off material into the face and pushing the work piece out of alignment, leading to a tapered thread.” 

Russ of atlas_craftsman pointed out that with the cutting force on both sides of the cutter, there is no consistent pressure on the leadscrew and halfnuts. The result is that any backlash will show up as a wandering thread. 

Doc of atlas_craftsman wrote – I believe  the  helix  on the  lead  screw provides  constant  pressure  towards  the  headstock , eliminating  backlash or a drunken thread ...the straight in  bit  has  pressure perpendicular , but there  is pressure  to  the  left   by  the  driving  of  the  lead  screw.... 
So I guess Russ and Doc will have to go outside and settle the matter _



This treatise provides two views on whether or not loading the leade screw by cutting at 30/29.5 degrees is important but makes no attempt to validate either point of view. The author leaves the reader to decide.

I will only say here that I think the choice of view is always the right of the reader. However, it is *my opinion *that the quality of the machine should have an impact on that choice because the level of force required to keep the so called drunken sailor on course depends on how drunken he is...... That is to say that 30/29.5 might be a better choice than 90 for lower quality or well worn machines. The size of the thread might also be important. 

Thanks Brent.


----------



## Susquatch (Jun 10, 2022)

YYCHM said:


> So how does this 29.5/30 thing work?



I was going to draw this up for you but Brent's attachment above has a perfext drawing and description of 90 vs 30/29.5 starting on page 5.


----------



## Susquatch (Jun 10, 2022)

David_R8 said:


> I just do what Tony does...



Who is Tony?


----------



## David_R8 (Jun 10, 2022)

Susquatch said:


> Who is Tony?


This Old Tony... I blame my entire descent onto this bottomless rabbit hole on him...


			https://www.youtube.com/c/ThisOldTony


----------



## Tom O (Jun 10, 2022)

So if you use the 29.5 method cross slide dial on 0 I haven tryed it but shouldn’t you be able to use a one or two thou plunge on the cross slide to address the thread finish not touching the 29.5 feed.


----------



## YYCHM (Jun 10, 2022)

Susquatch said:


> I was going to draw this up for you but Brent's attachment above has a perfext drawing and description of 90 vs 30/29.5 starting on page 5.



Never mind..... @140mower twigged it for me.  If using 29.5/30 you infeed with the compound Doh.

Rereading the threading section of "BASIC LATHEWORK FOR HOME MACHINISTS" by Stan Bray.  No where is that detail stated.


----------



## Susquatch (Jun 10, 2022)

YYCHM said:


> Never mind..... @140mower twigged it for me.  If using 29.5/30 you infeed with the compound Doh.
> 
> Rereading the threading section of "BASIC LATHEWORK FOR HOME MACHINISTS" by Stan Bray.  No where is that detail stated.



I don't have a copy so I can't help with that Craig. 

But that reminds me that I should look to see what I do have though.....


----------



## 140mower (Jun 10, 2022)

Tom O said:


> So if you use the 29.5 method cross slide dial on 0 I haven tryed it but shouldn’t you be able to use a one or two thou plunge on the cross slide to address the thread finish not touching the 29.5 feed.


If you are going to use the cross slide, it makes no difference where your compound faces, but unless I am missing something important, once committed to a method you need to stay the course.... Ie... If you are facing the trailing edge of the thread with the point of the cutter and the leading edge of the thread with the forward face of the cutter as in the 29.5 method, but try finishing up with a 90 plunge, you are going to remove the backside of the thread you just cut.....
 I'm having a bit of a day, so I apologize if that description made things worse..... I think I know what I am trying to say.  Lol


----------



## Degen (Jun 10, 2022)

I learned 29.5 (or there abouts as long as its not 30) to prevent stepping.  I think the rest of the world uses 30 as the number as long as its a shade less.

The 90 method I definitely agree is from insert tooling (CNC) influence and is beginning to become popular as it now better documented.

Now which to use becomes the question based on you machine and tooling.


----------



## Susquatch (Jun 10, 2022)

Tom O said:


> So if you use the 29.5 method cross slide dial on 0 I haven tryed it but shouldn’t you be able to use a one or two thou plunge on the cross slide to address the thread finish not touching the 29.5 feed.



Theoretically, that should not be required using the 29.5 degree method. But it will be necessary virtually every time if you mistakenly use 30.5 instead of 29.5. It's a very easy mistake. Page 6 (or shortly therafter) in the paper that Brent provided assesses the reasons for this quite well. It repeats what I did many many years ago when I was trying to use a compound that didn't have 29.5 on it so I needed to go back to basics to work it out. I wish I had @Brent H s paper back then.

That said, yes, a straight plunge using the compound will clean up all the faces. I have done this many times so I can vouch for it. Once the trench (plank might be a better word) is laid there are no worries about drunken sailors anymore. They just fall in where they are supposed to.....

I confess I also do this when I have to pick up a thread to take a few more thou off or cleanup an old existing thread. It probably isn't the best practice but it has worked for me.

PS - we should all get @140mower drunk so he is happier. He might make more sense then. I have no idea what he was trying to say! LOL!


----------



## VicHobbyGuy (Jun 10, 2022)

Susquatch said:


> OK, I give. What is the answer to that one?


On my 7x lathe, smaller cutting 'working faces' produce less chatter. So plunging cutting both sides of the 'V' in a thread is not as easy as cutting one side using the  cross slide at 30 degrees.
Similarly a thin parting tool works better than a thicker one, chamfering cuts using the side of the tool are difficult etc...
Back to our regularly scheduled program....


----------



## Susquatch (Jun 10, 2022)

VicHobbyGuy said:


> On my 7x lathe, smaller cutting 'working faces' produce less chatter. So plunging cutting both sides of the 'V' in a thread is not as easy as cutting one side using the  cross slide at 30 degrees.
> Similarly a thin parting tool works better than a thicker one, chamfering cuts using the side of the tool are difficult etc...
> Back to our regularly scheduled program....



I think that's a perfectly fine post for the topic. And it's my thread so it's my call! 

But ya, according to sandvik, you are supposed to just cut less each pass as the going gets tougher. I dunno - I think sometimes a less rigid machine has trouble with that. 

Also, as @gerritv pointed out earlier, the size of the thread matters. A little 32 TPI cut is easy to cut no matter how you do it or what machine you have (unless it's really sloppy). But 4 TPI might be impossible on a small lathe no matter which way you cut it. If I had to do it with a small lathe, I'd prolly make a special hss tool that would allow me to cut the thread from both sides in stages - maybe make a double sided staircase that I clean up afterward.


----------



## Susquatch (Jun 10, 2022)

Just another followup to my reply to @VicHobbyGuy .

This thread is about 29.5/30 vs 90 degree threading. It isn't about a particular size or class of lathe. 

I invite opinions about the problems, solutions, disadvantages, advantages, pros and cons, for each from everyone. I'm also interested in what others might know about the history no matter what size or class of lathe they have. It might well be that size matters, but that will be ok!  It may well be that this might be the last chance for many of us to know the history of this matter before it is lost in the complexities of today.


----------



## Dabbler (Jun 10, 2022)

I missed this thread somehow, but @Susquatch pointed me to it, so blame @Susquatch ...

I have zero skin in this game, and have zero intention to comvert any of you to "my way of thinking", so this is what I do, for reference, with a update that happened 3 years ago.

I was taught by a toolmaker to set up things a particular way, and it has worked for me, despite the fact that 80% of machinists do it another way:

I set my compound to 30 degrees.  as precise as a tenths indicator can make it.  It takes me about 5 minutes, and then I lock it down.  For years.  Only when I loosen it to cut a custom taper, then I spend that 5 minutes again to get it to 30.  I cut threads with no discernible rubbing or laddering even under a 20X loupe.

But that was 42 years ago, and 3 years ago (was it longer?) I watched a video by Stefan Gotteswinter that made me question reality.  It was on his old lathe, a 9" very light lathe that he made extensive tailstock mods to.  Even on this sub-600 lb lathe he cut his threads straight in.  On a solid toolpost - the compound was stored in a drawer somewhere.

I'm always up for something new, so I tried it - on my sub-700 lb 12X36 lathe.  Worked like a charm.  Clean threads, and much more straightforward.  (well at least to me).  Now that I have bigger lathes, I can't wait until I have the next threading job...

@Susquatch I have to disagree with  the opinion about parting tool method in @Brent H PDF -- the movement in the carriage is enough to keep backlash at bay, regardless of single side cutting or double cutting, as in the European method.


----------



## Susquatch (Jun 10, 2022)

Dabbler said:


> I missed this thread somehow, but @Susquatch pointed me to it, so blame @Susquatch ...
> I have to disagree with  the opinion about parting tool method in @Brent H PDF -- the movement in the carriage is enough to keep backlash at bay, regardless of single side cutting or double cutting, as in the European method.



Good stuff @Dabbler ! 

Perhaps you didn't notice that the paper Brent provided presented two views. One being the same as yours and one suggesting that it needed a bit more.

Your comments about two smaller lathes are quite compelling. I had thought perhaps the size and quality of the lathe might dictate a preference in method. But perhaps not.

I assume you are quite happy with the quality of your threads using the 90 degree plunge cut. Do you also reduce the amount of infeed as the depth of cut increases?

I can't help but wonder if your view of plunge cutting is influenced by the amount of effort you took to setup your compound for a very precise 30 degree cut. If it were me, I'd abandon your previous method in a heart beat if I found something so much easier. 

But my practice (at least till now) has been to cut at 29.5 degrees with virtually no precision in the angle. I just eye-ball it and start cutting. I have never found the angle to be critical. It always worked just fine as long as it was slightly less than 30.

Unlike your experience, I found 30 to produce poorer results. But I confess that I didn't set the angle with any precision so perhaps I was not really set to 30 but maybe 30.x instead. That would explain a lot.

I may yet go @gerritv and your way on this. We will see.


----------



## Dabbler (Jun 11, 2022)

Susquatch said:


> Do you also reduce the amount of infeed as the depth of cut increases?


Yes. even on a larger lathe.



Susquatch said:


> I can't help but wonder if your view of plunge cutting is influenced by the amount of effort you took to setup your compound for a very precise 30 degree cut.


Not at all.  I set up the compound only once every year or 2.  No big deal, and it keeps me in practice.



Susquatch said:


> so perhaps I was not really set to 30 but maybe 30.x


That could be one problem.  The other might be chip clearance.  I was taught to use LOTS of lube oil when cutting threads, to stop chips from crowding and jamming on the trailing edge.  As the cut  gets deeper it is harder to clear the chips without good lube.

For me, the attraction wasn't anything more complicated than having only one dial to worry about.  I dislike jumping from the cross slide for extraction, back to zero, then jumping to the compound for next depth of cut. I prefer to extract, then dial to the next increment.  One thing to remember, and one thing to calculate, all on one dial.  Just my preference.  They both make nice threads.  I was taught the compound method, but now prefer the straight in method.  The bonus round is the possibility of removing the compound until it is really necessary, which is very rare.


----------



## gerritv (Jun 11, 2022)

@Susquatch re size of lathe, I use the plunge method on Unimat and Taig (with thread followers to act as leadscrew), and now a used King 1022. None I would call excellent condition or stiffness. I do keep the tool overhang to a minimum, and use fresh inserts/honed HSS esp as the pitch gets coarser.

As confirmed by a few videos I watched last night (in Dutch and Flemish), plunge is used when pitch is small (as in less than 1.5mm/14tpi), after that they use A) the 29 or so method or B) set the compound parallel to axis and  dial in 2, across 1 on each pass. (as in .002 infeed, .001 toward spindle). The B method has the same result as offsetting the compound. Of course A and B don't work without modification for 55 or 47.5 or other thread angles, but the plunge method does 
The big advantage on the non-29 method is that you read your depth off the dial, no real need to keep measuring. You can see that in Stefan's video, no measuring.

My reco, try it out on a few threads. Too much theoretical chatter is not good for making progress.


----------



## gerritv (Jun 11, 2022)

Re: insert profiles, as in tip radius/root width, the A60/A55/AG60/AG55 inserts support a range of pitches, but are not really great at the low or high end of their range. Esp at the low end the tip is too fat, and at the high end too narrow. If that is critical, then I grind the insert into submission (easy to verify on an optical comparator or USB microscope) or grind one out of 6 or 8mm round HSS on my d-bit grinder. And then plunge in incrementally to the correct depth. I might eventually buy some pitch specific inserts to save that hassle for common ones.

One critical thing hinted at earlier is to turn the outside diameter to correct dimension first. Generally that is .125*pitch less radius than nominal. (on the mtric videos I watched they do the math in head, using .1*pitch because, well things are simpler to do in metric) Any thread shape diagram has those factors drawn on them.


----------



## Susquatch (Jun 11, 2022)

gerritv said:


> My reco, try it out on a few threads. Too much theoretical chatter is not good for making progress.



Great stuff Gerrit - right till the very end. You clearly don't know me very well. Curiosity and the pursuit of new knowledge are my basic Raison D'etre.

I didn't begin this thread with any intent to actually change what I do. I began it to understand why 29 is common practice in NA and 90 is common elsewhere. To do that meant understanding details and challenging assumptions. Of course, I may also change my own practice, but only because continuous improvement is always a worthy goal. 

Unfortunately, I am not really significantly closer to understanding why the regional difference exists....... 

And yes, I fully read your entire note. I don't speak Dutch or Flemish.


----------



## Mcgyver (Jun 11, 2022)

6 TPI internal in bronze is going different that 24 tpi external in 12L14.  Obviously 29/29.5 (for a 60 degree thread) has a reduced chip width which I think is advantageous.   Now I'm double thinking it....hmmm.  if the chip is twice as wide but the removal rate the same....is there a difference in the forces?  The other argument for it is the chips don't clear as well coming into the V from both sides.  Does that matter?  Maybe with heavy cuts, not sure.

There are lots of factors pitch, rigidity of machine, rigidity of set up, material and so on.   I've viewed 29.5 as it should let you rough a little more aggressively, all things being equal.  larger pitches (smaller leads) I sometimes won't bother, but always do on larger leads.  For a really coarse thread, at the same DOC, you are imposing less force cutting at 29.   I usually cut with the compound at an angle for most of the job, but the final few finishing cuts to take it dead on to size are done by feeding in the crossfeed, but by quite small amounts, probably thats textbook SOP


----------



## Susquatch (Jun 11, 2022)

Dabbler said:


> The bonus round is the possibility of removing the compound until it is really necessary, which is very rare.



All great stuff Dabbler. I use my compound constantly, for many things other than threading. I like to lock the carriage and use the compound for more precise control of feed position. The carriage is way too course for many of my needs. So that bonus wouldn't really be there for me. But thank you so much for helping me see where you are and how you got there. I do love how you explain things.

See my reply to Gerrit a few moments ago. Anything you can do to answer that basic question will be appreciated - even speculation. Your experience may bridge time better than many.


----------



## Susquatch (Jun 11, 2022)

Mcgyver said:


> 6 TPI internal in bronze is going different that 24 tpi external in 12L14.  Obviously 29/29.5 (for a 60 degree thread) has a reduced chip width which I think is advantageous.   Now I'm double thinking it....hmmm.  if the chip is twice as wide but the removal rate the same....is there a difference in the forces?  The other argument for it is the chips don't clear as well coming into the V from both sides.  Does that matter?  Maybe with heavy cuts, not sure.
> 
> There are lots of factors pitch, rigidity of machine, rigidity of set up, material and so on.   I've viewed 29.5 as it should let you rough a little more aggressively, all things being equal.  larger pitches (smaller leads) I sometimes won't bother, but always do on larger leads.  For a really course, the same DOC, you are imposing less force cutting at 29.   I usually cut with the compound at an angle for most of the job, but the final few finishing cuts to take it dead on to size are done by feeding in the crossfeed, but by quite small amounts, probably thats textbook SOP



I think you are right on all counts. Both methods work with different modifications required to accomplish different goals. From an operational standpoint, I will probably start doing plunge threading more often. One more tool in my tool chest if you will. 

Any idea how or why the two approaches evolved to be different common practice geographically?


----------



## Susquatch (Jun 11, 2022)

gerritv said:


> Re: insert profiles, as in tip radius/root width, the A60/A55/AG60/AG55 inserts support a range of pitches, but are not really great at the low or high end of their range. Esp at the low end the tip is too fat, and at the high end too narrow. If that is critical, then I grind the insert into submission (easy to verify on an optical comparator or USB microscope) or grind one out of 6 or 8mm round HSS on my d-bit grinder. And then plunge in incrementally to the correct depth. I might eventually buy some pitch specific inserts to save that hassle for common ones.
> 
> One critical thing hinted at earlier is to turn the outside diameter to correct dimension first. Generally that is .125*pitch less radius than nominal. (on the mtric videos I watched they do the math in head, using .1*pitch because, well things are simpler to do in metric) Any thread shape diagram has those factors drawn on them.



The initial OD is something most hobbiests probably forget and then wonder why the thread doesn't fit. How many times have I taken a lathe file to an OD to watch someone's face light up with "huh"........ 

This thread profile thing is just another vote for HSS...... (Ducking for cover...  LOL)


----------



## Mcgyver (Jun 11, 2022)

Susquatch said:


> Any idea how or why the two approaches evolved to be different common practice geographically?



I'm not convinced they are, or at least that its so black and white.  I'd think it a safe bet there are machinist here that have figured out it doesn't much matter at 32 tpi and that there's some guy in Germany who's figured out cutting a 10mm thread with the compound slewed over is easier.  There may more here that default to one and vise versa there, but its shades of grey imo.

I also have two European publications, one British and one Austrian and both recommend slewing the compound over.

 "The Amateurs Lathe" (great beginner book if you dont have one).  It's a British publication from 1948 and recommends setting over the "topslide".  I don't have German texts (and could not read them if I did) but did find this in an Emco manual I have (Austrian)






So yeah, things are different there...but they are also the same


----------



## Susquatch (Jun 11, 2022)

Mcgyver said:


> I'm not convinced they are, or at least that its so black and white.  I'd think it a safe bet there are machinist here that have figured out it doesn't much matter at 32 tpi and that there's some guy in Germany who's figured out cutting a 10mm thread with the compound slewed over is easier.  There may more here that default to one and vise versa there, but its shades of grey imo.
> 
> I also have two European publications, one British and one Austrian and both recommend slewing the compound over.
> 
> ...



That's a very good point. 

I have assumed that the difference was some shade of grey already. But it does seem like there is a significant shade difference. 

It seems clear that the North American bias is toward skewing the compound. But even that sense might be a sample error. Regardless, it ought to be more obvious why. Unfortunately, all the really old machinists are long gone so I am left to mostly speculate based on discussions like this one with experienced machinists like you. 

What intrigues me is my observation that skewing the compound is not an intuitive solution. I would have thought that SOP would naturally be the more intuitive approach with alternatives like skewing only arising when faced with challenging situations. 

So what is it that drove the popularity of this old well established, non-intuitive practice? 

I suspect the answer might be found in the old machines. With the old timers all gone, the only thing we have left is old machines and old text books to tell us their history. 

How old is that Austrian  EMCO manual? It's interesting that the manufacturer says "most machinists". This suggests that perhaps the rest of the world had the same bias as here in North America, but perhaps the old world was faster to change.


----------



## Brent H (Jun 11, 2022)

@Susquatch:  Please refer to the attachments for your reading pleasure.  There are "preferences" for how you set up and make threads, and indeed there are many different threads that are cut and the profile of the thread required will possibly dictate what set up is required.  clearance for the tool, load, chip removal etc etc will typically dictate what is necessary for proper threading.


----------



## Dabbler (Jun 11, 2022)

Susquatch said:


> Anything you can do to answer that basic question



@Susquatch  I don't know European things except from contemporary Youtube.  However at least 2 machinists in Canada have independently shown me the plunge method of threading as a 'secret worth knowing'.  Neither explained *why*, so I left it in consideration queue until Gotteswinter properly explained it.

So in summary, plunge is used here.  29.5/30 is used in Europe.  Both sides have all kinds of weapons in the armoury.


----------



## Susquatch (Jun 11, 2022)

Brent H said:


> @Susquatch:  Please refer to the attachments for your reading pleasure.  There are "preferences" for how you set up and make threads, and indeed there are many different threads that are cut and the profile of the thread required will possibly dictate what set up is required.  clearance for the tool, load, chip removal etc etc will typically dictate what is necessary for proper threading.



This was worth its weight in gold to me @Brent H.

I found two things of great significance to my quest in your documents.

In the first document, the author describes how we arrived at 29 vs 30. Basically he confirms what I had surmised earlier. On the earliest lathes it was not practical to set a precise angle of 30 degrees to cut perfect threads. But it was soon discovered that 29 degrees didn't need to be precise. 29 degrees solved the problem of precision by cutting the majority of the work on the leading face of the cutter and cleaning up the remainder on the right face with a very light 1 degree progressively deeper cleanup pass on the right face.

As @Dabbler said, a precise 30 works just fine. But 30.2 would not. In the absence of an easy way to set angles, machinists just fell into the practice of using 29.5 (or at least some slight angle less than 30).

The second source contains a reference section with information in it that I have never seen before. I "believe" it points to the reason for doing the 30 degree compound cut.

It is buried in the attached screen shot and discussed in the text.






Note the top rake on the cutting tool used for 30 degree method vs 90 degree in the top right drawing. The author claims that a single point tool that cuts on both faces must be flat with no rake and this results in chip clogging in many cases. A double rake tool is not possible with conventional grinding methods of that time. However, a tool with a top edge ground to cut primarily on the left edge never does this.

It is worth remembering the old lantern style threading tools of the day.






One can, easily imagine the process of cutting even moderate threads with a lantern post tool like that on an old lathe like my 1800s FE Reed.

At this point I can only speculate about a few things. Having done business in other parts of the world, I can say with certainty that there are many industrial practices in the old world and the new that were driven by the two world wars and especially the second world war.

I have almost no difficulty imagining that machine Shop practices on North America would survive the wars virtually intact. Old school (old lathes) machinists would teach the new machinists in the old school ways and that craftsmanship would stay engrained in machining practices regardless of changes in the machines and tools. Where once there was a reason for 30 degrees, the practice would continue even as the reason itself disappeared.

In the old world which had to be largely rebuilt from the ground up after the war ended, new machines, new tooling, and new practices would easily take hold.

Imagine then the arrival of carbide and multi-point threading tooling with none of the limitations of lantern style thread tooling and it is relatively easy for me to speculate about @Mcgyver s different shade of grey in the old world vs the new.

I don't personally believe that we are likely to find clear evidence to support or refute the speculation above. So I am ready to let it go (for now).

Nonetheless, there are some good outcomes from this exercise.

There are times and situations where both processes are advantageous. And while small modern machines are not as robust as new industrial machines, they are certainly orders of magnitude better than the old lantern style lathes that predominated before and after the wars. I believe in my heart of hearts that there is lots of room for both methods in any hobbiest workshop. Furthermore, I believe that learning from history is the best way to avoid repeating its negatives.

I am looking forward to learning to plunge thread and may even go buy some inserts to further facilitate that!

Although I will always be open to alternative explanations with or without evidence, I wish to extend a big huge thank you to everyone for ringing in and especially to @Brent H and his library for helping me bring this to a good comfortable conclusion in my own mind.


----------



## Susquatch (Jun 11, 2022)

Dabbler said:


> @Susquatch  I don't know European things except from contemporary Youtube.  However at least 2 machinists in Canada have independently shown me the plunge method of threading as a 'secret worth knowing'.  Neither explained *why*, so I left it in consideration queue until Gotteswinter properly explained it.
> 
> So in summary, plunge is used here.  29.5/30 is used in Europe.  Both sides have all kinds of weapons in the armoury.



See my reply to Brent. I'm pretty sure it puts everything to bed for me.


----------



## PeterT (Jun 11, 2022)

When I was looking for inexpensive threading carbide inserts a while back I studied Carmex catalog literature. Mostly because that is one of the popular formats which are 'replicated'. From what I recall of documentation, straight-in feed is also prescribed. I recall another competitor system I looked at being the same. So my gut feel is its probably not a Sandvik thing or a European thing, its probably a more modern (current) tooling thing. This tooling relates to industrial/CNC machines which I would think is 99% of their target customer base. Now historically if hobbyists on one continent vs another had earlier exposure to these systems & adapted them earlier as a rub-off factor, hard to say. Back when an insert was $25 and a HSS blank was $5, the hobbyist decision probably favored the cheaper HSS solution that did the job to the standards required. But the tides have shifted. Currently, insert tooling is cheap & affordable for hobbyists either as typically Asian supplier/knockoffs or inventory sell-offs of otherwise more expensive systems. There is no disputing many fine examples of HSS threading both historically & current. I don't think its an either/or issue, its an overlap issue & what fits one (hobbyist) person may not fit another.

How adapting this insert tooling or setup methodology relates to a hobby lathe is a very open question with too many overriding variables IMO: machine condition, material choice, thread type, operator skill, operator bias... just to name a few. As a singular data point FWIW, so far I'm happy with Carmex clones & matching offshore toolholders on a typical manual mode Taiwan 14x40 lathe '98 vintage. Most of threading has been sub 12 TPI in materials like 1018, 12L14, O1, SS, aluminum alloys. I am hopelessly off the recommended charts, meaning lower speeds & feeds. But my takeaway point is thus far the world did not explode, no shattered carbide edges. But getting better threads than what I was achieving with my own grinds (or bad quality braze-on carbide tools which was another matter). So a lot of the insert handwringing I read about fortunately did not come into play, at least in my own experience. For personal R&D I did try straight in vs 29.5 & found no discernable difference to finish or accuracy. I have not done coarse thread lead screw like threading yet though. So on the basis of convenience & time I have become a straight-in guy.

Relating to geometry of tooling & setup, I can makes some guesses as to why hobbyists might have variable different results. The way I learned was hand grinding a HSS blank with relief angle set on grinder table, compare included angle to a fish tail template, set up to work piece... the classic method. Actually at school we put both the tool tip & thread on the big toolroom magnification projection device & that was quite revealing.

The 29.5 vs 30.0 compound discussion is interesting because it relates to cutting forces but also relates to implied theoretically perfect 60-deg pitch angle. Is a hand grind to a fish tail template really within 0.5 deg time after time? I'm not saying it cant be done, but its another variable that might explain different results. Similarly if the left/right relief angle is ground just a bit different or tool is presented to work just a bit different, then straight-in will see this difference & likely cut different. So if that is when chatter is observed the operator concludes straight in is bad. But correlation is not causation. The issue could be related to other factors outside of what can be easily identified. A molded carbide insert hopefully eliminates or at least reduces some of these variables. In addition, 'just because they can', molded carbide inserts can actually have different relief angles per side depending on the thread.

Lastly I have found that DOC passes are another thing to pay attention to, but I'm still learning there & is outside the scope of post.


----------



## Susquatch (Jun 11, 2022)

PeterT said:


> When I was looking for inexpensive threading carbide inserts a while back I studied Carmex catalog literature. Mostly because that is one of the popular formats which are 'replicated'. From what I recall of documentation, straight-in feed is also prescribed. I recall another competitor system I looked at being the same. So my gut feel is its probably not a Sandvik thing or a European thing, its probably a more modern (current) tooling thing. This tooling relates to industrial/CNC machines which I would think is 99% of their target customer base. Now historically if hobbyists on one continent vs another had earlier exposure to these systems & adapted them earlier as a rub-off factor, hard to say. Back when an insert was $25 and a HSS blank was $5, the hobbyist decision probably favored the cheaper HSS solution that did the job to the standards required. But the tides have shifted. Currently, insert tooling is cheap & affordable for hobbyists either as typically Asian supplier/knockoffs or inventory sell-offs of otherwise more expensive systems. There is no disputing many fine examples of HSS threading both historically & current. I don't think its an either/or issue, its an overlap issue & what fits one (hobbyist) person may not fit another.
> 
> How adapting this insert tooling or setup methodology relates to a hobby lathe is a very open question with too many overriding variables IMO: machine condition, material choice, thread type, operator skill, operator bias... just to name a few. As a singular data point FWIW, so far I'm happy with Carmex clones & matching offshore toolholders on a typical manual mode Taiwan 14x40 lathe '98 vintage. Most of threading has been sub 12 TPI in materials like 1018, 12L14, O1, SS, aluminum alloys. I am hopelessly off the recommended charts, meaning lower speeds & feeds. But my takeaway point is thus far the world did not explode, no shattered carbide edges. But getting better threads than what I was achieving with my own grinds (or bad quality braze-on carbide tools which was another matter). So a lot of the insert handwringing I read about fortunately did not come into play, at least in my own experience. For personal R&D I did try straight in vs 29.5 & found no discernable difference to finish or accuracy. I have not done coarse thread lead screw like threading yet though. So on the basis of convenience & time I have become a straight-in guy.
> 
> ...



All good stuff Peter. 

I'm am actually quite happy with the way everything has unfolded. It's complicated but also quite simple. The history and the geographic differences all make sense to me now and I like that. I don't like things that don't make sense. 

I had previously more or less settled on HSS and 29.5 degree threading as a way of life. In my humble opinion, my threading was excellent - although I accept that others might not agree. 

Nonetheless, I am actually quite eager now to plow new ground and add inserts and plunge threading to my Toolbox of threading alternatives. I wish there fewer choices though so some of your recommendations are probably a good place to start. 

I think it's time for me to move on to other areas of interest now and complete a few projects too. Way too much fun for an old man! 

Your interest in indicators, measurements, and spindle alignment seems to have dropped off the planet. I've been waiting for you to reframe your question. But perhaps you got your answers or lost interest. That happens and it's ok. 

I'm still waiting for the spindle test bar to arrive so I can qualify it and then go about the business of comparing the available alignment methodologies.


----------



## thestelster (Jun 11, 2022)

Susquatch said:


> So what are YOU most comfortable with @thestelster - 90 or 30/29.5?
> 
> More importantly, why?


I'm a straight in kinda guy! I started all askew in my early life, but I've straightened up and fly right now.

I only use carbide inserts.  Hopefully I can show my methodology properly in these pictures.  I set up the compound so it will advance the cutter in the Z-axis when the time comes, dial set to zero, and backlash taken up. I have to cut 16tpi thread.  According to the Sandvik chart my infeed (@90°) is 0.041".  So I go ahead and thread that part to a depth of 0.041".  Doing so does raise some burrs and the thread flanks are a little rough.  I will use a file to remove the burrs and bring that part to the original OD.  I try to screw the action in, and it starts, but stops within 1 rotation.  I now use the compound, it was at zero, I back it up a fair bit and then advance it(taking up the backlash) to 99 (.001" before the zero).  I move the cross-slide to 0.041", and make a cut.  This cleans up the trailing flank of the thread.  I test fit the part, it now screw is two rotations before it stops.  I advance the compound towards the chuck +Z .001, move the crosslide to 0.041", and make a pass.  This cuts on the leading flank of the thread. Test, and repeat moving the compound in 0.001" increments.  I had to remove a total of 0.004" of material from the flanks of the thread for the action to fit perfectly.

On those cards:  the one on the left shows how many passes, and depth of cut in the X-axis.
The card on the right:
According to Sandvik, a topping insert of 16tpi, has a nose radius of 0.008".  The threading insert I use is non-topping, and has a nose radius of between. 002"-.004".  So, when I cut the thread (before I used the compound), the root radius was between. 002-.004, and probably closer to the larger value since its been used many times.  And the action wouldn't fit, because it was too tight, but by moving the compound in the Zaxis by 0.004, it now matches up with the topping value would be, and lo and behold, it fits.


----------



## PeterT (Jun 11, 2022)

My AliExpress Carmex 'style' insert & toolholder on 303 stainless. One nice setup aspect of this style of insert is you can pre-align quite quickly & accurately a few different ways because the pocket is already aligned within toolholder. Bring long edge of the insert up to end of work piece & daylight gap. Or daylight gap front of toolholder to side of work. Or set up an indicator on insert edge or toolholder shank side surface & advance cross travel.


----------



## PeterT (Jun 11, 2022)

Susquatch said:


> Your interest in indicators, measurements, and spindle alignment seems to have dropped off the planet. I've been waiting for you to reframe your question. But perhaps you got your answers or lost interest. That happens and it's ok.


Mostly a function of time. Our weekend weather looks crappy so I'll probably pick up on it again.


----------



## Susquatch (Jun 11, 2022)

PeterT said:


> My AliExpress Carmex 'style' insert & toolholder on 303 stainless. One nice setup aspect of this style of insert is you can pre-align quite quickly & accurately a few different ways because the pocket is already aligned within toolholder. Bring long edge of the insert up to end of work piece & daylight gap. Or daylight gap front of toolholder to side of work. Or set up an indicator on insert edge or toolholder shank side surface & advance cross travel.



I have several insert type tools that also provide convenient alignment so I get the idea.

What store did you get your inserts and holder on Ali?


----------



## thestelster (Jun 11, 2022)

PeterT said:


> My AliExpress Carmex 'style' insert & toolholder on 303 stainless. One nice setup aspect of this style of insert is you can pre-align quite quickly & accurately a few different ways because the pocket is already aligned within toolholder. Bring long edge of the insert up to end of work piece & daylight gap. Or daylight gap front of toolholder to side of work. Or set up an indicator on insert edge or toolholder shank side surface & advance cross travel.


Or take a precision square placed on the tool holder with the blade against the side of the chuck.  Perfect alignment. Snap off the tip, no problem rotate or replace the insert.  I have threaded many, many,  many parts with a single insert without having to dress it, or touch it up, or sharpen it (does that look like 60° or 58°?)


----------



## VicHobbyGuy (Jun 11, 2022)

PeterT said:


> My AliExpress Carmex 'style' insert & toolholder on 303 stainless. I have several insert type tools that also provide convenient alignment so I get the idea.





Susquatch said:


> What store did you get your inserts and holder on Ali?


I'm interested in gettng some carbide insert tooling for threading, but 'can't make head or tail' of all the choices. So I would really appreiate specific recommendations - not just the store, but the actual insert and insert holder/tool. Thanks in advance!


----------



## thestelster (Jun 11, 2022)

VicHobbyGuy said:


> I'm interested in gettng some carbide insert tooling for threading, but 'can't make head or tail' of all the choices. So I would really appreiate specific recommendations - not just the store, but the actual insert and insert holder/tool. Thanks in advance!


What size tool holders or tool bits is your lathe capable of using?


----------



## VicHobbyGuy (Jun 11, 2022)

thestelster said:


> What size tool holders or tool bits is your lathe capable of using?


It's a 7x14 lathe with OXA tool post and holders. To align to spindle center, it's easiest for me to use 8mm tools; 10mm usually can work also. I have some insert holders and inserts for turning, just nothing for cutting threads. I'm using a home ground HSS 60 deg thread tool and it works OK but I find it tricky to get the 60 deg. angle and nose radius exactly correct.


----------



## PeterT (Jun 11, 2022)

Susquatch said:


> What store did you get your inserts and holder on Ali?


I might not be all that helpful but I'll try. I went back to my notes & looks like I got my external toolholders & inserts from 2 stores: Leader & Beyond. I pasted the store home page below. But this is going back 3-4 years ago likely dated information. Seems like some Ali stores are a bit nomadic & searching for stuff can be a PITA. Just now I typed in one of the common shanks SER1212H11 & got many hits (attached screen grab), but most of the stores I don't recognize (mostly because I haven't bought any recently). But seems like the same stuff, holders 8-12$, pack of 10 inserts 30-40$. Sometimes the same sellers can be found on Ebay, but pays to check prices & shipping etc.

Leader




__





						Buy Products Online from China Wholesalers at Aliexpress.com
					





					leadercutting.aliexpress.com
				




Beyond (now Oyyu?)




__





						Buy Products Online from China Wholesalers at Aliexpress.com
					





					oyyuchampions.aliexpress.com
				




Ebay random hit








						SER1616H16 Lathe Turning Tool Holder+10Pcs 16ER AG60 Threading Carbide Insert BE  | eBay
					

Find many great new & used options and get the best deals for SER1616H16 Lathe Turning Tool Holder+10Pcs 16ER AG60 Threading Carbide Insert BE at the best online prices at eBay! Free shipping for many products!



					www.ebay.ca


----------



## PeterT (Jun 11, 2022)

Its slowly coming back to me. I stayed within the (10,12,16mm) shank sizes because those fit my tool holder & do not require anvil (green shade on matrix). This system is consistent with Carmex where bigger or different inserts can benefit from anvils to alter the effective angle. It gets confusing but generally those were outside my application. 

I had to chuckle looking for the Oh-so-convenient tool shank cross reference table buried way down the Oyyo/Beyond link. Like don't bother us with your questions. Just waste your own time reading our crappy website & just click buy already. Sheesh.

Also internal inserts are different than external! (personally I think there are better options like Ali 60-deg carbide bars to accomplish threading but maybe that's biased to my own work)


----------



## Susquatch (Jun 11, 2022)

thestelster said:


> I'm a straight in kinda guy! I started all askew in my early life, but I've straightened up and fly right now.
> 
> I only use carbide inserts.  Hopefully I can show my methodology properly in these pictures.  I set up the compound so it will advance the cutter in the Z-axis when the time comes, dial set to zero, and backlash taken up. I have to cut 16tpi thread.  According to the Sandvik chart my infeed (@90°) is 0.041".  So I go ahead and thread that part to a depth of 0.041".  Doing so does raise some burrs and the thread flanks are a little rough.  I will use a file to remove the burrs and bring that part to the original OD.  I try to screw the action in, and it starts, but stops within 1 rotation.  I now use the compound, it was at zero, I back it up a fair bit and then advance it(taking up the backlash) to 99 (.001" before the zero).  I move the cross-slide to 0.041", and make a cut.  This cleans up the trailing flank of the thread.  I test fit the part, it now screw is two rotations before it stops.  I advance the compound towards the chuck +Z .001, move the crosslide to 0.041", and make a pass.  This cuts on the leading flank of the thread. Test, and repeat moving the compound in 0.001" increments.  I had to remove a total of 0.004" of material from the flanks of the thread for the action to fit perfectly.
> 
> ...



Sorry, I somehow missed your post. 

So you used to do 29 but now do a 90 plunge with inserts.

Was there a reason that you switched? 

That's a nice clean thread. Nothing wrong with that. I like your approach to making the thread fit too. 

Did you order threading mics yet? If not, wanna borrow mine to try them first?


----------



## thestelster (Jun 12, 2022)

Susquatch said:


> Sorry, I somehow missed your post.
> 
> So you used to do 29 but now do a 90 plunge with inserts.
> 
> ...


@Susquatch 
I used the 29° infeed when I was taught in high-school.  My most difficult aspect in the process was shaping the HSS tool bits for threading.  For turning you have a lot of leeway, but for threading they have to be precise since they are form tools.  I switched to carbide inserts when I saw a Sandvik catalogue.  The information in those catalogues is amazing.   Inserts are simple, no mess, no fuss, convenient, exact dimensions, last longer, cut turn at much higher speeds, cut harder steels, return to zero repeatability, no need to adjust tool height/no shims required, (I don't have a QCTP), resists built-up edge, can give a mirror finish at correct speed/feed, different inserts for optimizing finish in different materials,  and using the same tool.

I have not ordered those mikes yet. Thank you so much for the offer.  I probably will eventually, but because I do mostly one-of's, where the thread is matched to it's mate, I have no immediate need.  If I was making fasteners in bulk, then yes, definitely.


----------



## thestelster (Jun 12, 2022)

VicHobbyGuy said:


> It's a 7x14 lathe with OXA tool post and holders. To align to spindle center, it's easiest for me to use 8mm tools; 10mm usually can work also. I have some insert holders and inserts for turning, just nothing for cutting threads. I'm using a home ground HSS 60 deg thread tool and it works OK but I find it tricky to get the 60 deg. angle and nose radius exactly correct.


@VicHobbyGuy I use mostly Sandvik tools and inserts, but their small threading tool is 1/2" shank.  I do have a Tool-Flo tool and inserts, which are just as nice.  And they do make an external thread tool in 10mm.  FLO-LOCK FLSR-1010M2, and using their insert FLTF-2R which is non-topping and will do threads from 14-44tpi.  But there are tons of others.  Just go into their catalogues.


----------



## VicHobbyGuy (Jun 12, 2022)

thestelster said:


> @VicHobbyGuy I use mostly Sandvik tools and inserts, but their small threading tool is 1/2" shank.  I do have a Tool-Flo tool and inserts, which are just as nice.  And they do make an external thread tool in 10mm.  FLO-LOCK FLSR-1010M2, and using their insert FLTF-2R which is non-topping and will do threads from 14-44tpi.  But there are tons of others.  Just go into their catalogues.


Thanks, @thestelster . I appreciate the suggestions. The "tons of others" is the problem!  I ordered a SER1010H11 holder and some inserts from AliExpress- with cheap stuff I can afford "buying the wrong one" mistakes. Finding a supplier for 'name-brand' high quality stuff is a challenge, and when I do, the prices (and shippng costs) often tend to be breathtaking.


----------



## VicHobbyGuy (Jun 12, 2022)

thestelster said:


> @Susquatch
> My most difficult aspect in the process was shaping the HSS tool bits for threading.


+1 on that.


----------



## Susquatch (Jun 12, 2022)

thestelster said:


> @Susquatch
> I used the 29° infeed when I was taught in high-school.  My most difficult aspect in the process was shaping the HSS tool bits for threading.  For turning you have a lot of leeway, but for threading they have to be precise since they are form tools.  I switched to carbide inserts when I saw a Sandvik catalogue.  The information in those catalogues is amazing.   Inserts are simple, no mess, no fuss, convenient, exact dimensions, last longer, cut turn at much higher speeds, cut harder steels, return to zero repeatability, no need to adjust tool height/no shims required, (I don't have a QCTP), resists built-up edge, can give a mirror finish at correct speed/feed, different inserts for optimizing finish in different materials,  and using the same tool.
> 
> I have not ordered those mikes yet. Thank you so much for the offer.  I probably will eventually, but because I do mostly one-of's, where the thread is matched to it's mate, I have no immediate need.  If I was making fasteners in bulk, then yes, definitely.



OK, I follow you. 

Many of the reasons you provide are the same as my reason for liking hss inserts. Especially the ARWarner ones. They have a perfect grind. 

They would probably work fine with 90 degree plunge threading too. But the main advantage of HSS is interrupted cuts and much lower cutting speeds.


----------



## thestelster (Jun 12, 2022)

Susquatch said:


> OK, I follow you.
> 
> Many of the reasons you provide are the same as my reason for liking hss inserts. Especially the ARWarner ones. They have a perfect grind.
> 
> They would probably work fine with 90 degree plunge threading too. But the main advantage of HSS is interrupted cuts and much lower cutting speeds.


I wanted to try those inserts, but I sent 2 emails to them with no response, and phoned twice.  Once leaving a message and the other time actually speaking to someone.  Gave him my order, and he said he would get back to me with total cost.  Never did.  I gave up.


----------



## PeterT (Jun 12, 2022)

Susquatch said:


> But the main advantage of HSS is interrupted cuts and much lower cutting speeds.



Has this been your own personal experience? If so what kinds of problems were you having with carbide threading inserts in the past that HSS proved better? Like carbide fracturing or surface finish or....? 

As I mentioned in my post with the stainless steel examples, I was on the slowest rpm my lathe will allow, completely off the minimum manufacturers recommended RPM range (presumably prescribed for CNC setups). But I didn't see any adverse issues whatsoever & actually never have. I don't mean this to be an all encompassing statement or pushing an agenda, just saying it thankfully didn't materialize in my particular case.

What do you mean my interrupted cuts (specific to threading)? Like entering & exiting a thread or threading across a slot or something?


----------



## Susquatch (Jun 12, 2022)

PeterT said:


> Has this been your own personal experience? If so what kinds of problems were you having with carbide threading inserts in the past that HSS proved better? Like carbide fracturing or surface finish or....?
> 
> As I mentioned in my post with the stainless steel examples, I was on the slowest rpm my lathe will allow, completely off the minimum manufacturers recommended RPM range (presumably prescribed for CNC setups). But I didn't see any adverse issues whatsoever & actually never have. I don't mean this to be an all encompassing statement or pushing an agenda, just saying it thankfully didn't materialize in my particular case.
> 
> What do you mean my interrupted cuts (specific to threading)? Like entering & exiting a thread or threading across a slot or something?



These are good questions Peter.....

I tend not to let my personal experience guide my views. It's simply too likely to be one-off or exceptions to the rule. I don't like anecdotal either as there is no rigor to establishing the facts.

But in this case, I confess that it's just my personal experience - which could be all wrong.

To answer your questions with the qualifications above, my experience with carbide is not threading based. That's because I ALWAYS thread with HSS. I did try a carbide threading tool a few times and didn't like it. But that wasn't a good hss vs carbide test. It was a cheapo carbide tool that came as part of a kit. I have never owned or tried one like yours. The bottom line here is that I always use HSS for threading and it has never disappointed me. Like you, I generally thread at very low speeds. I don't like threading at high speeds - I'm too old for that and my hand eye coordination sucks. I do SOME precision threading on stainless steel and Chromemoly but most of my threading is just plain old threading on random steel that just happened to be the right size for whatever farm repair job I'm doing.  HSS has never failed me. It is entirely possible that good quality carbide inserts in good tools would work just as well as my hss. I simply don't know. So ya, good question.

My experience with regular turning is quite different. It's kinda the reverse of threading. For regular turning, I use mostly carbide inserts and only rarely use HSS.

I've totally lost count of how many carbide tools I ruined (usually chipped the tip off) with interrupted cuts and I have not had good experience with surface finish cutting at low speed either. For interrupted cuts, I usually switch to HSS. For better surface finish on regular lathe work, I turn up the speed or take a bigger cut or faster feed or switch to round inserts or at least inserts with a bigger nose radius. Sometimes I will grind a special HSS bit for the job. I also like using a HSS shear tool for really stubborn surfaces.

To be honest, I only stick with carbide inserts because I like the convenience of inserts. On the other hand, I only stick with hss for threading because it works great at low speeds. But they are still inserts - expensive inserts at that!

Someday soon I will try better carbide inserts for threading than the crap I used previously.

So ya, you are right to question my statements. They are hardly rigorous. They should be considered as "my experience only" along with all the baggage and erroneous conclusions that go along with any small scale individual experience. They are what they are - your mileage may vary!


----------



## PeterT (Jun 12, 2022)

All good. Quite a few years ago now I had blah experience with cheapo brazed carbide threading tools. The included angle checked out (kinda) the relief angle seemed fine, my setup was at least consistent, but the results were  just not pretty. Even on 12L14 which should cut like butter. I pulled out a HSS blank from school, it worked fine. Ground my own HSS tool, worked fine. Whatever the difference, it seemed subtle to the naked eye. Under magnification some of story became clear. The factory grind had striations & the cutting edge had kind of a sawtooth appearance. It didn't seem chipped though. I tried cleaning up with a fine diamond stone but not sure I improved it much. The HSS grind didn't look pretty either but I could see a band on the edge where it saw some oil stone action. One does need to define the material. I had a batch of local 1018 that cut like sh*t in every respect (turning, facing, drilling & threading) but I didn't know that at the time. The exact same tooling & setup in 12L14 was perfectly fine.

Later on I bought a different carbide insert holder system which stood upright & offered 3 points. That seemed to cut better but I just wasn't doing much threading then. I only had a couple inserts to try because they were spendy, managed to lose one & the whole system became obsolete. So the more recent Ali purchase was yet another experiment for which I had reservations. I wasn't keen on dropping a wad on name brand. I think the Carmex toolholders alone are over $100 at Travers & inserts maybe $10 a pop. (The Ali were about $10 per holder & 3$/insert).

Anyways, so far so good. I'm not into it for very much cash outlay & results are meeting my objectives. If all I ever do is this kind of threading I should be OK. If I have to break out the odd HSS for special situation that's fine too. I don't know if my particular are knock-offs with potential quality issues, or if they are the real thing & just cutting out the N-Am distributer middlemen. I've seen both sides of this coin but its very hard if not impossible to distinguish. The Ali toolholders I'm sure are plain jane 4140 vs maybe something better on a cnc tool. But that doesn't seem to be adversely affecting my hobbyist setup. The trouble with Ali is it can be hard to find things to begin with & equally hard to re-order things once you land on something that is actually OK. Its like going to a fish market. Last years catch of the day may not resemble current offerings.


----------



## VicHobbyGuy (Jun 12, 2022)

PeterT said:


> The trouble with Ali is it can be hard to find things to begin with & equally hard to re-order things once you land on something that is actually OK. Its like going to a fish market. Last years catch of the day may not resemble current offerings.


Yup!


----------



## Dabbler (Jun 12, 2022)

For those with smallish lathes (or perhaps any lathe)  Clough42 on Youtube just found out why his 400 lb lathe didn't like form tools much, and fixed it.  Since threading tools are form tools no matter how you use them, this video might be appropriate form some people. 

It highlights the idea that the whole system contributes to chatter, and some times it is fixable...


----------



## PeterT (Jun 12, 2022)

Good video. Classic example where the initial perceived problem ended up being related to a completely different problem. And most people, or at least novice owners, may not think to check something like this presumed to be fitted properly at the factory.


----------



## VicHobbyGuy (Jun 12, 2022)

Dabbler said:


> For those with smallish lathes (or perhaps any lathe)  Clough42 on Youtube just found out why his 400 lb lathe didn't like form tools much, and fixed it.


Thanks for that link. I watched that video yesterday, and checked my two 7x14 lathes this morning. One of them- the one I use most for turning- actually did have the cross slide lifted off the saddle on one side. I can't blame the Sieg factory for that one, though - it was my replacement ("improved") bronze gib that was a bit too tall. So that was a pretty easy fix.  I have no idea whether it will make the cutting tool more stable or not but it eliminates one possibility. I take pretty light cuts when threading so chatter isn't usually an issue, and if/when it is, I find that a quick touch on the HSS tool with a diamond hone solves the problem.


----------



## VicHobbyGuy (Jun 12, 2022)

PeterT said:


> And most people, or at least novice owners, may not think to check something like this presumed to be fitted properly at the factory.


Perhaps not the case for novice owners of 'big'  lathes like the Grizzly 0602, but few owners of 7x lathes presume anything is fitted properly at the factory!  I am joking; you are correct that most beginners like me wouldn't think to check that the cross slide wasn't touching the top of the dovetails.


----------



## PeterT (Jun 12, 2022)

Some parting tool issues I've heard about that subsequently became resolved ended up being machine issues, not tool issues. Same general idea, if the machine components are not fully supported as they should be or have the ability for undesirable play, those factors can result in similar issues or even cause kind of a feedback loop.


----------



## VicHobbyGuy (Jun 12, 2022)

PeterT said:


> Some parting tool issues I've heard about that subsequently became resolved ended up being machine issues, not tool issues. Same general idea, if the machine components are not fully supported as they should be or have the ability for undesirable play, those factors can result in similar issues or even cause kind of a feedback loop.


Exactly - Parting became a lot quieter and less 'exciting' for me after I replaced the compound with a solid block (a.k.a. plinth) and at about the same time switched to a better quality (Warner) thin (P1N .040") tool. So, probably machine+tool solution - I didn't 'go back' to figure out which; I was just happy that parting was easier.


----------



## DPittman (Jun 12, 2022)

Susquatch said:


> Someday soon I will try better carbide inserts for threading than the crap I used previousl


I believe you had mentioned at one time you have/had a Mesa threading and grooving tool holder....did you not get any threading inserts to go with that?  If not, you should.  They are expensive, but they are sharp and really work nice with that tool holder, you can flip them end to end and then there are also lefthand ones that make upside down threading easier.  Yes they can still chip the point off like most carbide (and probably even easier because of the sharp tip.


----------



## Susquatch (Jun 12, 2022)

Dabbler said:


> For those with smallish lathes (or perhaps any lathe)  Clough42 on Youtube just found out why his 400 lb lathe didn't like form tools much, and fixed it.  Since threading tools are form tools no matter how you use them, this video might be appropriate form some people.
> 
> It highlights the idea that the whole system contributes to chatter, and some times it is fixable...



I have had problems parting............ I will look. You never know.


----------



## Susquatch (Jun 13, 2022)

DPittman said:


> I believe you had mentioned at one time you have/had a Mesa threading and grooving tool holder....did you not get any threading inserts to go with that?  If not, you should.  They are expensive, but they are sharp and really work nice with that tool holder, you can flip them end to end and then there are also lefthand ones that make upside down threading easier.  Yes they can still chip the point off like most carbide (and probably even easier because of the sharp tip.



You have a GREAT memory. 

Yes, I have the Mesa threading tool and I like it. The point on the bits I have are all chipped though. I should buy replacements. $$$ Ugh.  Perhaps I will get enough so I can try grinding the point a bit on one.


----------



## Johnwa (Jun 13, 2022)

If it weren’t for having to grind tools I would almost always stick witH HSS.  With HSS you can shave off a thousandths with a sharp too.  I can’t do that with carbide.  With my Southbend it either does’t cut or takes off 5 to 10 thou. On my SM it will consistently take off about 5 thou but won’t shave off much less than that.  This is all with regular inserts.


----------



## Susquatch (Jun 13, 2022)

DPittman said:


> I believe you had mentioned at one time you have/had a Mesa threading and grooving tool holder....did you not get any threading inserts to go with that?  If not, you should.  They are expensive, but they are sharp and really work nice with that tool holder, you can flip them end to end and then there are also lefthand ones that make upside down threading easier.  Yes they can still chip the point off like most carbide (and probably even easier because of the sharp tip.



@DPittman & @PeterT - Here are photos of my existing Mesa Carbide tool inserts. It's easy to see how they failed.












And here is a photo of a cheap kit insert. Basically the same type of failure.






Now compare that with the ARWarner HSS Inserts with maybe 20 or 30 times the number of jobs under their belt. The flat below the tip is original and intentional. 












For regular non-precision threading, I just grind some regular HSS tooling. As soon as I get some of the regular carbide threading inserts like Peter recommended, I will try them and post again.


----------



## DPittman (Jun 13, 2022)

Yes I learned that the inserts did not like to be bumped up against the work surface when fiddling around centering the height or just being uncareful.  I would imagine they would not handle interrupted cuts very well either.  However i have been pleased with them when I handle them appropriately.  I doubt you would be able to regrind an edge on those as sharp and fine as the original. 
I've only tried the triangle hss inserts from AR Warner but like them also.


----------



## PeterT (Jun 13, 2022)

@Susquatch that is classic carbide fracture. I would share your reluctance to use inserts too if that was a consistent outcome. The key question is, how is it happening? Typically its alignment, chatter, interrupted cut, flex, slide or play anywhere in the supporting components from the holder through to the ways. Easy to type, maybe not so easy to diagnose. My gut feel is its a feedback loop. Initial alignment is good, speed & feed are acceptable. But something is allowing it to move in & out of the cut & brittle materials like carbide just don't like that. The HSS may be the identical form & sharpness & subjected to the forces, but just more tolerant. I think if you fix the problem, even the HSS will look better that they were or at least cut more efficiently.

I'm not familiar with the Warner system but I suspect its good. For $20 of disposable R&D & would try an Ali lay down threading tool. Ease into it with fine threads & something nice like 12L14. If it starts chipping & degrading too, then my assumption would be some kind of other machine/setup issue going on. If its good initially but issues arise at certain DOC or material types, then the focus turns back to insert tooling. Not knowing your machine, but if the leadscrew is wearing & locking isn't done, that can have a big impact on threading & parting which are kind of devious cousins.

A an aside I have been tricked before aligning regular carbides on vertical center in what I call lazy man way - lightly trap a ruler between cutter & work, it should hand vertical. This is actually a bad habit taught to me in school that should be removed from cranial RAM IMO. Many inserts have rake geometry where this actually can land you in the wrong vertical position & adversely affect cutting. Secondly, trapping a steel rule, typically pretty hard material, cant be good for carbide. I've chipped them kissing off a chuck jaw for zeroing so I don't do that anymore, or use an aluminum shim as buffer. Its better to take a micro skim off the end of bar until the nub is gone right through center & lock the toolholder there. Remove the tool & repeat, it should be identical & repeatable. I had a toolholder where the stud started floating & rotating which meant the toolholder was going along for the ride even though the stop & nit were tight.


----------



## Susquatch (Jun 13, 2022)

PeterT said:


> @Susquatch that is classic carbide fracture. I would share your reluctance to use inserts too if that was a consistent outcome. The key question is, how is it happening? Typically its alignment, chatter, interrupted cut, flex, slide or play anywhere in the supporting components from the holder through to the ways. Easy to type, maybe not so easy to diagnose. My gut feel is its a feedback loop. Initial alignment is good, speed & feed are acceptable. But something is allowing it to move in & out of the cut & brittle materials like carbide just don't like that. The HSS may be the identical form & sharpness & subjected to the forces, but just more tolerant. I think if you fix the problem, even the HSS will look better that they were or at least cut more efficiently.
> 
> I'm not familiar with the Warner system but I suspect its good. For $20 of disposable R&D & would try an Ali lay down threading tool. Ease into it with fine threads & something nice like 12L14. If it starts chipping & degrading too, then my assumption would be some kind of other machine/setup issue going on. If its good initially but issues arise at certain DOC or material types, then the focus turns back to insert tooling. Not knowing your machine, but if the leadscrew is wearing & locking isn't done, that can have a big impact on threading & parting which are kind of devious cousins.
> 
> A an aside I have been tricked before aligning regular carbides on vertical center in what I call lazy man way - lightly trap a ruler between cutter & work, it should hand vertical. This is actually a bad habit taught to me in school that should be removed from cranial RAM IMO. Many inserts have rake geometry where this actually can land you in the wrong vertical position & adversely affect cutting. Secondly, trapping a steel rule, typically pretty hard material, cant be good for carbide. I've chipped them kissing off a chuck jaw for zeroing so I don't do that anymore, or use an aluminum shim as buffer. Its better to take a micro skim off the end of bar until the nub is gone right through center & lock the toolholder there. Remove the tool & repeat, it should be identical & repeatable. I had a toolholder where the stud started floating & rotating which meant the toolholder was going along for the ride even though the stop & nit were tight.



These are good questions to ask. Since my experience lined up with what I've read elsewhere, I just assumed it is a hss vs carbide thing. But maybe not. I do have a few things that have bothered me at the back of my mind. 

Eg, how repeatable is my piston style BXA Tool Holder? 

I don't use a ruler to set height. Never did. Made myself a tool height standard when I got my 2nd lathe 10 years ago. I use that to set and check tool heights. 

I have not ordered a carbide insert threading tool yet, but when it arrives I'll try what you suggest. I'm still researching alternatives. The kbc discount is calling me.


----------

