# thread on outside threading ...



## wquiles (Aug 1, 2008)

I am having some difficulties on outside threading that I wanted to share with the experts here - hopefully you guys can help me correct what I am doing wrong.

What I am trying to do is a project for a forum member in which I am basically duplicating this escrew:







The problem that I have is that when I am done, the peaks of the newly formed threads have been basically "squeezed" out and I end up with a larger OD than the one I started with. I don't know if this is due to the straight cutting of the threads (no 29.5Deg) or because of the actual thread cutting tip (60Deg), or what. I will post photos here in the hopes of trying to learn more 


So I first get the OD to the same outer thread dia (major diameter):






I then make the edge beveled:






While I am threading, I am using a trick I learned here using super magnets holding a dial indicator. I have the parts from Modamag to get my Shumatech going, but this works in the meantime:
















Then I cut and bevel the grove where the threading will end - this also marks the size of the heatsink:






So I am now ready to cut threads - I even have the thread table indicating the total cut depth and how much to cut at each pass (I am doing 20TPI):












So I set up the cutter for the first pass:






here is after the first pass:






second pass:











third pass:











fourth pass:











fifth pass:











sixth pass:











Even though I am suposedly done, when I try the head on the heatsink, it is still too big:






and when I measure the OD, I can see why - I am now at 0.822" !!!:






So I used a diamond file to cut the "tops" of the threads, and did another pass on the threads to clean-up:






and now it fits, although now the fit is a little bit too loose for my taste (looser than the actual escrew):











So what do you guys think is the problem?

Will


----------



## wquiles (Aug 1, 2008)

RESERVED


----------



## Mirage_Man (Aug 1, 2008)

Will, as you know I advocate the use of the 29.5* method over straight infeed. However I would suggest hitting the peaks of the threads lightly with a file with plenty of WD-40 or whatever you use on the next to last pass. Then make your final pass of about .001-.002". Then spin the spindle up to 1000 or so RPM and hit it with a Red and then Gray Scotchbrite again soaked with WD-40.


----------



## precisionworks (Aug 1, 2008)

29.5° is also what I use, as it's easy to set the compound to that angle. Then a fishtail gage is used to set the tool at 90° to the part being threaded.






For almost all lathe ops, carbide tooling is used. The exception is single point threading in aluminum. A carbide insert is never as sharp as a freshly ground HSS tool, and carbide tends to tear most alloys including 6061. It's easy to get the correct point angle, again using the fishtail gage.

I also use mag-back bases for threading. When using 29.5° compound, you make a pass & retract the tool, go back to the start position, advance the tool back to where it last was, zero out the dial, and dial in more depth. Much faster to do it than to write about it:thinking:


----------



## VanIsleDSM (Aug 1, 2008)

I think that threading table is wrong, it doesn't tell you to go deep enough.

This one is much more in depth, in 2 ways 

http://www.walteranderson.us/hobbies/metalworking/microlathe/frog/threading.html

0.28" for a 24TPI thread for example, is wrong, the actual depth is 0.316", which means if you were using 29.5 you'd actually want to go in 0.365". The threading and the depth seems easy now.. it's all about getting the diameters right. I'm debating on just buying some full form 24 TPI inserts or something.. yet I have nothing to insert them into yet.. would be nice to have the bit knock down crest of the thread once you're deep enough.


----------



## gadget_lover (Aug 1, 2008)

At first I thought you were moving the compound to the left, then I noticed the dial indicator in the back. 

That's 60 degree sharp ended tool, right?

What I can not tell from your pictures is wether the tip of the tool is centered at the right height. That makes a difference. It also looks like the threads are different widths in one picture ( mg_5912.jpg ). Other than bumping the compound crank or loose gears, I'm not sure how that happens.

Is there a radius on the tip of your tool , or is it sharp?

Daniel


----------



## PhotonFanatic (Aug 1, 2008)

Hi Will,

If you are going to cut threads, you really should learn the proper technique, especially for the coarser pitches, i.e., 4 to 24 tpi. That means using your compound slide set to 29-30 degrees to the axis of the workpiece. Doing so will place less stress on your cutting bit, resulting in cleaner threads. Sure, for fine threads, where you really aren't removing much material, feeding your cutting bit straight into the piece will be OK, but I suggest you adopt one technique and stick to it. The odds of making a mistake drop significantly once you have the routine down.

So if you are going to make threads using the 30-degree compound slide setting, here is an explanation as to how and why to determine the depth of cut:

The Theoretical Single Depth of Thread for either the Unified or ISO Metric threadform -- which are both 60-degree threads with a 1/8 Pitch flat at the Major Diameter and a 1/4 Pitch flat at the Minor Diameter -- can be calculated easily from the Thread Pitch:

Theoretical Single Depth = (5/8) x Pitch x Cos (30 degrees)

Working a numerical example for a Unified threadform of 1/20 inch Pitch:

Theoretical Single Depth = (5/8) x 1/20 inch x Cos (30 degrees)

= 0.625 x 0.05 inch x 0.866

= 0.0270 inch

Working a numerical example for an ISO Metric threadform of 1.25 millimeter Pitch:

Theoretical Single Depth = (5/8) x 1.25 millimeter x Cos (30 degrees)

= 0.625 x 1.25 millimeter x 0.866

= 0.677 millimeter

The Unified and ISO Metric threadforms are modified (truncated) V screwthreads with a 60-degree included angle between the flanks. In a 60-degree Sharp-V screwthread, the measured-along-the-flank length would be exactly equal to the Pitch. The flats at the Major and Minor Diameters on the Unified and ISO Metric threadforms result in a reduction of the measured-along-flank length to 5/8 that of a same-pitch Sharp-V screwthread. [This means that the Theoretical Along-Flank Infeed of a compound / top slide set at 30 degrees to feed along the flank can be calculated as (5/8) x Pitch, which for a Unified threadform is exactly equal to (5/8) / Number of Threads per Inch.]

The Single Depth of the screwthread is the measured-along-flank length of the screwthread times the Cosine of one-half of the V angle, i.e., 30 degrees.

I would suggest sitting down at your computer and making a spreadsheet for every possible TPI, or metric pitch, that you may be expected to cut, using the formula(s) above. Then when you are ready to cut some threads, you only need to know the nominal diameter and can look up the suggested diameters in Machinery's Handbook for the class of fit that you want.

++++

As an aside, if you cutting your threads properly, you don't need to file anything down, nor do you need to use Scotch-Brite on them, either.


----------



## wquiles (Aug 1, 2008)

Mirage_Man said:


> Will, as you know I advocate the use of the 29.5* method over straight infeed. However I would suggest hitting the peaks of the threads lightly with a file with plenty of WD-40 or whatever you use on the next to last pass. Then make your final pass of about .001-.002". Then spin the spindle up to 1000 or so RPM and hit it with a Red and then Gray Scotchbrite again soaked with WD-40.


OK, I will try the Scotchbrite pads - supermarket stuff?




precisionworks said:


> 29.5° is also what I use, as it's easy to set the compound to that angle. Then a fishtail gage is used to set the tool at 90° to the part being threaded.
> 
> 
> 
> ...


Yep, I used that tool to line-up the bit - alignment of the cutting tool is not the problem this time.

As to the actual process:
1) engage cariage at #1 on the thread dial
2) set cutter depth
3) turn on motor
4) stop motor on the cut groove
5) turn motor in reverse
6) once cutter is back past the piece, proceed to #2 
7) once final depth is achieved, do a couple of pases
8) clean cuts with a metal brush

Note that the carriage is always engaged and I use the reverse on the motor to go back and forth.


----------



## jhanko (Aug 1, 2008)

Your problem is caused by your reverse procedure. There is too much backlash in the change gears, lead screw, half nut, etc. to expect the cutter to be in the same position in reverse as it was in forward. Before you reverse the machine, back off the cutter to slightly clear the O.D. of the work. The cutter is rubbing the side of the thread in reverse, distorting the material. I learned this the hard way also..

Jeff


----------



## gadget_lover (Aug 1, 2008)

JHanko said:


> Your problem is caused by your reverse procedure. There is too much backlash in the change gears, lead screw, half nut, etc. to expect the cutter to be in the same position in reverse as it was in forward. Before you reverse the machine, back off the cutter to slightly clear the O.D. of the work. The cutter is rubbing the side of the thread in reverse, distorting the material. I learned this the hard way also..
> 
> Jeff




This makes perfect sense, as in reverse you are not cutting, but are instead rubbing. That , combined with the backlash as Jhanko pointed out, could easily deform the threads.


Good call!

Daniel


----------



## DUQ (Aug 1, 2008)

wquiles said:


> OK, I will try the Scotchbrite pads - supermarket stuff?



MM meant 3M hand pads. They come in different colors (grade)

http://www.3mestore.com/hand-pads.html


----------



## ICUDoc (Aug 1, 2008)

Will I am often nervous cutting threads at 29.5 degrees as the carbide cutter I use seems to remove a tiny bit of the newly formed thread all the way from its base ( at the forming minor diameter) to its tip ( all the way to the major diameter) and have wondered whether it is actually making the MajDia smaller with the last few passes. it always seems to fit OK. Maybe this will prevent the "upsizing" you are seeing???
I am an amateur at this but I offer it FWIW...


----------



## Mirage_Man (Aug 1, 2008)

DUQ said:


> MM meant 3M hand pads. They come in different colors (grade)
> 
> http://www.3mestore.com/hand-pads.html



Yup, Scotch-Brite Hand Pads.

Enco has them...

Red/Maroon Very Fine
Gray Ultra Fine


----------



## PEU (Aug 2, 2008)

http://video.google.com/videoplay?docid=5557473837334990194 

Yeterday I adapted one of my toolholders to accept my new threading tool, I dont believe how nice the thread resulted, best thread I did ever! It uses TPMC 16 inserts.


Pablo


----------



## Mirage_Man (Aug 2, 2008)

PEU said:


> http://video.google.com/videoplay?docid=5557473837334990194
> 
> Yeterday I adapted one of my toolholders to accept my new threading tool, I dont believe how nice the thread resulted, best thread I did ever! It uses TPMC 16 inserts.
> 
> ...



That's sweet! Wish I had a CNC machine.


----------



## greenlight (Aug 2, 2008)

I love watching your demonstration videos.


----------



## Anglepoise (Aug 2, 2008)

Will,
If you intend to make parts that have to fit other parts you have never seen or measured, I would take Fred's advise.

Also I don't see from your detailed post if you are reversing with the cutting tool still engaged with the workpiece. If you are doing this, the slack in the gears will completely screw up the thread (as posted by member JHanko). Always disengage the tool from the workpiece when winding back. Knurling and threading are a pain but your threads have to be perfect if the items is to fit an unseen piece as you can not trial fit.


----------



## jhanko (Aug 2, 2008)

Looking at your pictures, I just noticed something else that will definitely cause problems although it has nothing to do with your increase in diameter problem. I noticed that as you are making each cut, you are cutting the feed in half. That is correct if your goal is reducing diameter as the amount you cut will result in a double that amount in diameter reduction. When cutting threads, The depth of feed is just that, not halved. The first cut you made should have been .008", but you did .004". When you were all done, you were at .019". A little more than half as deep as it should have been. To get a great thread on your mini-lathe, try this:

Follow that chart you have excactly. Don't cut the feeds in half. When you get to the last pass, keep repeating it until the cutter isn't removing anything anymore. This will vary depending on how loose the lathe is.
Example for 20 TPI: .008", .007", .006", .005", .004", .003", .000", .000", .000", .000". You will notice that even though you make 4 or more passes with the feed set at .033", it is still removing material, less and less each time. I usually make 4 passes at my final depth. When finished, all you'll need to do is wipe off with a terry cloth towel and admire the mirror like finish. As PhotonFanatic stated, when finished cutting the threads, you shouldn't have to touch them with anything (file, sandpaper, scotchbrite pad).

Most importantly, never let the cutter touch the work while reversing.

Jeff


----------



## wquiles (Aug 2, 2008)

Too hard to thank each one individually - thanks so very much for the many replies/suggestions. :thumbsup:

I will be trying again tomorrow morning (garage is now at 101F here in Texas!!!) and will update post #2 with my results as it is obvious I am doing not one, but several things wrong :shakehead

Now, I do seem to have some different goals for thread depth: Fred's equations state a thread depth of 0.0270", but JHanko/thread table states a depth of 0.0330". I think I will try 0.027" first and see how it works out 

Again, you guys are awesome - thanks much for the help :twothumbs

Will


----------



## PhotonFanatic (Aug 2, 2008)

Will,

You will need to re-read what I posted--if you are like me, you might need to re-read it about five times. 

The .027" is the depth of thread for a straight infeed of the cutting bit into the material, i.e., at a right angle to the axis of the workpiece.

But, if you do switch to cutting using the flank infeed method, i.e., set the compound slide to 30-degrees, then the distance of infeed along the path that the tool bit will follow when using the compound slide is, in fact, .0312".

This graphic should make it a bit easier to visualize:






Hope that helps.

BTW, different depths of cut are to be expected from different sources--one thing we aren't delving into here is the class of fit, or the % of thread engagement. But I believe that if you use that basic formula for depth of cut using the 30-degree setting, i.e., 5/8 / TPI, you will have at least 75% thread engagement and that will be sufficient for most flashlight pieces.


----------



## wquiles (Aug 3, 2008)

Fred - you are certainly right - I missed that point on my first pass. Thanks much for the clarification


----------



## will (Aug 3, 2008)

This is for what it is worth 

If you have a diameter that is increasing as you are cutting, you really are not cutting material, you are 'shoving' it around or pushing it. 

I do a lot of woodworking. I have read a great deal about using scrapers instead of sanding wood. In a nut shell - you file a square edge on the scraper, this actually will leave a burr on the edge, it is too fine to be removed with the file, it just bends over. This has the same effect as making the edge some what thicker, In this instance it is a good thing. 

You are having the same result with threading, the peaks are too fine to be cut and are left over. Scotch bright pads, 600 grit wet or dry will fix this, this is similar to stropping a razor after it has been sharpened, it removes the 'burr on the edge'


----------



## jhanko (Aug 3, 2008)

wquiles said:


> I will be trying again tomorrow morning (garage is now at 101F here in Texas!!!)



Wow, that is exactly the reason I hauled my lathe down in the basement. And let me tell you, it's no fun moving a 300 lb. piece of cast iron down stairs. Although we don't get that hot up here in Chicagoland, we do get in the 90's occasionally and even that is way too hot for me. Now I have a nice little work area that's 70 degrees year round.:thumbsup:


----------



## VanIsleDSM (Aug 3, 2008)

This thread has got me to thinking now about the way I do internal threads.

I use these tools that I cut myself on the grinder:







I made the internal tool to work with the lathe in reverse, threading away from the headstock, so I wouldn't have to worry about bottoming out in a blind hole. I like it very much, and it works well.. though I'd like to make a stiffer one out of a larger tool bit. Now, on to what I got to thinking about; I use the 29.5 degree method, but when internal threading, I'm pushing the bit into the work, @29.5 degrees towards the headstock, like the diagram above, and then pulling it out of the hole with the leadscrew to make the threads. Is this defeating the purpose? it still cuts on the one side, and it works pretty well.. but maybe it would be better to set the angle the other way, so I'm pulling out with the compound into the work, and then the leadscrew also pulls out of the work to form the thread.. ? Would this make a difference? I suppose I should just try.. but I'd like to see what the machinists around here have to say.

I also cut my boring bar on the grinder to work the same way.. with the lathe in reverse, easier to see what you're doing as you don't have to torque your head around to look inside the hole where the cutting is going on.

On another note, does anyone know why the 2 charts conflict with each other on depth of cut?


----------



## jhanko (Aug 3, 2008)

VanIsleDSM said:


> On another note, does anyone know why the 2 charts conflict with each other on depth of cut?



It all depends on the type of cutter being used. If you are using a cutter that is sharpened to a point, you will have to feed the tool in farther than you would with a carbide insert that has a radiused tip to get the same width of the root, and that is what's most important. I notice that the older publications usually quote larger infeeds. I imagine that's because back then, all that was ever used was sharply pointed tools. The chart that Will has shown is for modern carbide inserts that aren't pointed. If you fed a 60 degree pointed tool and a 60 degree radiused tool in the same amount, the width of the roots would be different. The thread cut with the pointed tool would fit tighter.

Jeff

EDIT: One thing I forgot to mention is that in your case you can do things one of two ways. You can continue using your sharply pointed tools (which you have done an excellent job on, BTW) and use the chart that you have been using or you can grind ~.004" off the tip of your tools and use the chart that Will has shown. You will end up with the same thread. The big downside of using the pointed tool is that you are unnecessarily removing material with the sharp point. That wouldn't matter on solid material like a bolt or shaft, but on a thin wall piece like a compact flashlight, it could be the difference between success and disaster.


----------



## gadget_lover (Aug 4, 2008)

JHanko said:


> If you fed a 60 degree pointed tool and a 60 degree radiused tool in the same amount, the width of the roots would be different. The thread cut with the pointed tool would fit tighter.
> 
> Jeff



I may be wrong, but as I envision it the thread profile will be different if you advance both tools the same amount. Which one is messed up depends on the chart you are using. 

The "thread height" is theoretical, not physical, and is defined earlier in the thread. (1/TPI) * .86603. The thread height is NOT the depth that you will cut.

The general rule for unified threads is that the properly radiused tool cut will be 5/8 the height of the thread. An internal cutter should have a smaller radius than an external cutter.

If you advance a radiused tool the full thread depth you end up cutting too deep and the crests will be too narrow, even to the point where they are sharp.

If you advance the sharp tool only 5/8 the thread height, you are cutting too shallow and the crests will be too wide.

The rule for the sharp tool cutting depth is :
external thread = 7/8 the thread height.
Intrenal thread = 6/8 the thread height.

Daniel


----------



## jhanko (Aug 4, 2008)

gadget_lover said:


> I may be wrong, but as I envision it the thread profile will be different if you advance both tools the same amount. Which one is messed up depends on the chart you are using.



Exactly true. If you fed a pointed tool into the material a distance that is recommended for a tool with a radiused tip, you would end up with a thread that has the roots too close together and would result in a tight fit or no fit at all.



gadget_lover said:


> The "thread height" is theoretical, not physical, and is defined earlier in the thread. (1/TPI) * .86603. The thread height is NOT the depth that you will cut.



True again. The thread height is simply a result of the depth you cut. If the thread height and depth of cut are the same, you have cut way too deep. The main goals of cutting a thread are cutting the correct angle (the easy part), and having the correct width between the roots (the hard part). The depth of cut is just the means to get there. The only way to be certain that the thread is exact is to measure the distance between the roots with thread measuring wires as seen here. I feel this is certainly overkill for flashlight threads though. If the threads engage smoothly without slop or interference, call it a day...

Jeff


----------



## precisionworks (Aug 4, 2008)

> The only way to be certain that the thread is exact is to measure the distance between the roots with thread measuring wires


Wires are an accurate way to measure ... pretty funny the first time you watch someone try to get all three wires in the threads & get the mic around the wires

Probably less funny if you are that person, which is why the thread mic is an alternative to measuring over wires. The most versatile thread mics have interchangeable anvils & will work with a wide tpi range. Less expensive mics have fixed anvils & cover only a limited range of threads.


----------



## gadget_lover (Aug 4, 2008)

JHanko said:


> True again. The thread height is simply a result of the depth you cut. If the thread height and depth of cut are the same, you have cut way too deep.
> Jeff



One of the problems with discussing threads is that the term "thread height" sounds like it would be the same as "the height of the thread".

As Jeff said, the height of the groove you cut is simply a result of the depth of the cut. The "thread height" will always be the same based on the number of threads per inch.

Daniel


----------



## VanIsleDSM (Aug 5, 2008)

Thanks, that makes sense about the thread cutting depth, I understand now.. the chart posted by Will is for his specific radiused carbide tools, the one I posted is for pointy tools. Any info about how I'm cutting internal threads? or did I not explain that very well? Maybe I'll take a little video if I get around to cleaning up my work area to a non embarrassing state.


----------



## jhanko (Aug 5, 2008)

VanIsleDSM said:


> Any info about how I'm cutting internal threads? or did I not explain that very well?



No, you explained very well. I personally didn't reply because I don't have any experience with boring and right hand threading in reverse, but I think it's a better idea and much safer. I caught myself getting my shirt very close to the chuck jaws a couple of times while leaning in to see where the cutter was at while boring and threading. I didn't figure out the advantages of left hand internal tools until after I invested in right hand boring bars and threading tool. I really don't see why it would make any difference which direction the cutter comes in from or which side of the thread you remove material from. You could try feeding in from the left and let us know if you see any difference, but I doubt there will be any. Oh, and don't worry about your messy work area. We all love watching videos of lathes in action. It's a great way for some people to be able to help and for others to learn.

Jeff


----------



## Anglepoise (Aug 5, 2008)

VanIsleDSM said:


> Any info about how I'm cutting internal threads? .



When I cut internal threads, I set the topslide over as depicted by the white dots in the pic below. ( Crank handle would be off screen top right of pic)






Now this makes sure all slack is taken up the right way and I am cutting on the correct flank of the tool. I only thread towards the headstock so in your case it might be worth experimenting and see what works best for you.


----------



## wquiles (Aug 5, 2008)

Anglepoise said:


> When I cut internal threads, I set the topslide over as depicted by the white dots in the pic below. ( Crank handle would be off screen top right of pic)
> 
> 
> 
> ...



David - besides all of the great help/advice you provide, I am also always very impressed how clean/neat your lathe always is in the pics :twothumbs


----------



## Anglepoise (Aug 6, 2008)

wquiles said:


> David - besides all of the great help/advice you provide, I am also always very impressed how clean/neat your lathe always is in the pics :twothumbs


I must admit your post gave me a good chuckle as you are not the only one on the site that has noticed that and given me a hard time about it ( in a kind and most friendly sort of way )

I did my apprenticeship in England working for Alcan Aluminiun in 1962 and the foreman was a tough old war horse from WW II. If our lathes were not kept spotless, we were not given any overtime and after this training it sort of stuck. 

Still today I clean up after every job....habit I suppose, .....<gg>


----------



## wquiles (Aug 9, 2008)

OK, here is my full second attempt at perfect threads 

I setup the compound for approx. 29-1/2 deg:











I of course used this little tool to align things before starting (and by the way, I am using the other new side of this 60deg carbide insert as well):






First pass:











Second pass (I am now backing away the cutter before turning the motor in reverse - carriage always stays engaged to the screw):











Third pass:
Second pass:











Fourth pass:











Fifth pass (and last pass according to the table):











Now I do a final pass straight "in" of 0.001":
















But the threads do not look "quite" symmetrical yet, so I do another 0.001" pass:











The threads are still not perfectly symmetric, but look better!


So then I go and try the piece. It fits first time, with just little play, and no deburring or anything!






and the outer diameter has not changed!






As I mentioned, the threads are not "perfect" yet. Here is a closeup after cleaning and then a cropped version (larger size):











What do you guys think? I feel that I am making lots of progress, but I am not "quite" there yet 

Seems I can still improve some. Additional suggestions?

EDIT: The only thing I can think about right now, looking at the magnified picture, is that I am almost cutting too much on the right side, and not enough on the left side - maybe the 29 1/2 degree is not market accurately in my lathe? Maybe I should try an even 30deg instead?


----------



## Mirage_Man (Aug 9, 2008)

Will,

Looking good but your compound is not really set at 29.5 degrees. That's why your threads don't look quite right. You can't go by the marking on the compound to set the angle. Make a reference mark on the cross slide then add up the numbers until you get a true 29.5 degrees. I'm not quite sure of the math but you're actually at around 60 degrees.


----------



## PhotonFanatic (Aug 9, 2008)

Will,

Mirage Man has told you of your major problem--improper setting of the compound slide angle. 

I will presume that your Zero mark on the compound slide would set that to be parallel to the Z axis, i.e., parallel to the ways.

If you look at this photo, where I placed a YELLOW line, that would be where your 29.5 degree mark (GREEN arrow) needs to be set. That yellow line would correspond to a 90 degree difference from the scratch mark that is visible on your slide--bottom right in the photo.






To help visualize the correct set-up, let me post some additional photos of my lathe and the various angles that we are discussing. First, here's the compound slide as I normally use it--parallel to the Z axis:






With that set-up, one could only feed the cutting tool into the workpiece by advancing the Cross Slide, which would be perpendicular to the workpiece. As you know that means that both sides of the cutting tool would be engaged and cutting into the workpiece--not the ideal set-up, especially with deep threads.

And here's a close-up of the degree scale with the Compound Slide parallel to the Z axis:






And if you then were to go clockwise around that degree scale some 90 degrees, i.e., moving closer to the spindle, you will see the 90-degree reading:






So, my Compound Slide has two marks on it, bascially at the 6 O'clock and 9 O'clock positions.

To properly set the 29.5 degrees, I need to rotate my compound slide clockwise until the 29.5 mark is at the line where the 90-degree mark was before.






And backing away from the lathe, this is what it all looks like once in the right position:






As you can see, it is a much smaller angle that what you had set your compound slide to.

Now regarding some other things that you mentioned: You fit the head to the threads that you had cut, but that doesn't mean much--it only means that you cut the threads deep enough in some sort of shape that allowed the head to screw on. But, in fact, you haven't cut the threads to spec. As you mentioned the threads were lopsided and there is no visible flat on the crest of the threads.

Also, while lots of folks like to use that fishtail to set the cutting tool tip so that it is perpendicular to the workpiece, I find that holding it properly, at the right height, with no tilt to it, can be problematic. Instead, I like to face the workpiece end first, and then place the lefthand edge of the cutting tool against the end of the workpiece. I can clearly see if it is in full contact along the length of the cutting tool. If it is, then I tighten down my toolholder to the Compound Slide. 






Finally, when I'm cutting threads, I usually like to try fitting the internally threaded piece to the exterior threaded piece as the scales indicate that I am almost done with the compound slide infeeds. That sometimes give me a better feel as to how much infeed I will need on the cross slide to complete the threads.

Hope there's something in this rambling post that will help.


----------



## wquiles (Aug 9, 2008)

PhotonFanatic said:


> Hope there's something in this rambling post that will help.



Fred,

I knew by just looking at the ending thread that something was not "right", but I did not quite know why. I get it now. I will definitely try it again until I get it right. Thanks so much for taking the time to explain it so well :bow:


Another follow-on question: Although I am cutting a relieve are on both sides of the thread (where it begins and ends, the very ends are "very" thin and sharp and deform easily. How do you handle/fix/correct those thin edges?


----------



## jhanko (Aug 9, 2008)

Will,
You're definitely getting there. You've got a nice, defined thread but as others have said, the feed angle is wrong. While I agree it is best to learn cuttting threads at 29.5 degree feed as it will be required when you start threading harder materials, it won't make a difference with aluminum. Just for the hell of it, try cutting that thread again with a straight feed. You are SO close to getting a perfect thread, the suspense is killing me...

Jeff



wquiles said:


> Another follow-on question: Although I am cutting a relieve are on both sides of the thread (where it begins and ends, the very ends are "very" thin and sharp and deform easily. How do you handle/fix/correct those thin edges?



It sounds like you are cutting the reliefs at the same angle as the thread. That will result in a razor thin start and finish. You are threading with a 60 degree tool. Try cutting the reliefs at 45 degrees so the thread has a "ramp" to climb up and fall off.


----------



## fludunlimited (Aug 9, 2008)

1+ 
I need pics to understand this stuff.

thanks





wquiles said:


> Fred,
> 
> I knew by just looking at the ending thread that something was not "right", but I did not quite know why. I get it now. I will definitely try it again until I get it right. Thanks so much for taking the time to explain it so well :bow:
> 
> ...


----------



## ICUDoc (Aug 10, 2008)

wquiles you need (90 -29.5) = 60.5 degrees as you are looking for 29.5 degrees to the long axis of the lathe. On my lathe this is an estimate as the marks only go up to 60 degrees. So the extra .5 degrees is a guess, but an easy one to get close on my lathe.Your lathe might need a protractor to do this, or make a mark at 90 degrees then subtract the 29.5???


----------



## wquiles (Aug 10, 2008)

Third time is a charm? 


Get the part to the right height:







Bevel the edges at 45deg (I did a little bit too much the right side):











Align the compound at 29.5deg (mark spot for future operations):











Align cutter using straight edge machinist "L" and zero both dials:











First pass:






Second pass:






Third pass:






Fourth pass:






Fifth pass (final pass on compound):






Final "final" pass with 0.001" straight "IN". By the way, I got this from this great tutorial by TB here [ https://www.candlepowerforums.com/threads/118257 ]:
















last picture magnified and cropped. Note that I have done no de-burring, nor touched up on the threads at all - simply "as is":






Mating head fits perfectly with little play:






Final piece (dark is original escrew):





















A few more pics:
















last picture magnified/cropped:







I still need lots more practice, but the threads are getting better


----------



## jhanko (Aug 10, 2008)

Now you got it. Very nice looking threads...:thumbsup:

Jeff


----------



## Mirage_Man (Aug 10, 2008)

:twothumbs


----------



## PhotonFanatic (Aug 10, 2008)

That's some quick learning--well done!


----------



## cmacclel (Aug 11, 2008)

The compound slide issue 

Thats how it all started with me. My threads all looked skewed when I had the compound set to 29.5 degrees. It really needed to be at 60.5 degrees as previous mentioned. 

I still use the straight infeed method and have been for years. I probably have cut over a thousands threads into *aluminum* this way. My threads are very smooth and look perfect. Though I doubt this method will work well in harder materials but for aluminum it works for me. Internal or external all my threading happens in 3 passes then a 0.002 finish pass. All my threads get cleaned up with maroon scotchbrite.

If you think about it a CNC cuts straight threads......right?

Mac


----------



## wquiles (Aug 11, 2008)

Thank you guys


----------



## Mirage_Man (Aug 11, 2008)

cmacclel said:


> If you think about it a CNC cuts straight threads......right?
> 
> Mac



I don't know for sure but I think not.


----------



## cmacclel (Aug 11, 2008)

Mirage_Man said:


> I don't know for sure but I think not.


 
Your using 3 axis's to cut threads. All the CNC lathes I have seen only have X & Z so unless I'm missing something I don't see how they could cut threads like a manual machine. Also the last cut even using a manual machine should be a straight cut from everything I read and have been taught by 40 year veterans 

Mac


----------



## Mirage_Man (Aug 11, 2008)

cmacclel said:


> Your using 3 axis's to cut threads. All the CNC lathes I have seen only have X & Z so unless I'm missing something I don't see how they could cut threads like a manual machine. Also the last cut even using a manual machine should be a straight cut from everything I read and have been taught by 40 year veterans
> 
> Mac



Mac, I see what you're saying. I'm not all that familiar with CNC machines. Maybe one of our resident CNC guys can tell us the skinny? 

Edit: After thinking about it for a few minutes I have to say that can't the in-feed angle of a compound be simulated with the X & Z axis?

BTW I use the flank infeed method for cutting threads and always feed in a thou or two for the final pass with the cross slide.


----------



## Anglepoise (Aug 11, 2008)

I know Sandvik recommend 'modified flank infeed' for their inserts with CNC and manual lathes. Also ,interesting, they recommend adjusting the infeed angle from 3 > 5° smaller than the angle of the thread. They recomend this angle adjustment to 'steer the chip' so it gets out of the way.

Most people get fooled once in their life with setting the compound angle.
I certainly have. Now I just remember that the compound must be parellel with one side (flank ?) of the 60° cutting insert. Easy to see and use as a quick check.


----------

