PDA

View Full Version : Compound Feed for Threading



panchula
01-26-2008, 08:22 PM
Here's the best explanation I've found of how far to feed in the compound for threading (and why).

http://www-personal.umich.edu/~panchula/ToolTravel2.jpg

Assuming the compound is set at 30 degrees, the compound travels along one leg of a triangle. The length of the side is the same as the crest to crest distance of one thread. Next, reduce that travel by 1/8th to allow for the root clearance and again by 1/8 for the crest. That's a total of 1/4 or 25%. The remainder comprises the 75% thread form.

Divide .750 by the TPI, and that's how far to advance the compound.

-Mike

IOWOLF
01-26-2008, 09:36 PM
How many times does it take to get it through you guys heads....

TWENTY-FRICKIN-NINE-AND A GOD DAMN HALF DEGREES.

Or you get lines.

tattoomike68
01-26-2008, 09:51 PM
I dont use the compound at all till I get to 5 TPI or less.

oldtiffie
01-26-2008, 09:52 PM
Here's the best explanation I've found of how far to feed in the compound for threading (and why).

http://www-personal.umich.edu/~panchula/ToolTravel2.jpg
..........................................
.........................................
........................................

Assuming the compound is set at 30 degrees, the compound travels along one leg of a triangle.
-Mike

Hi Mike.

Never mind the "flak".

I will cover that subject and a lot of others on screw-threading shortly on another HSM thread at:
http://bbs.homeshopmachinist.net/showthread.php?t=27274

J.Ramsey
01-26-2008, 09:57 PM
I dont use the compund at all till I get to 5 TPI or less.


Whats a compund? I guess you like chatttttter and rub.:D


Wolfie I always use 29.5 degrees is that ok with you?

tattoomike68
01-26-2008, 10:00 PM
I guess you like chatttttter and rub.:D

Its never been a problem on shallow threads. Also the indexable insert tool I use has the right geometry for plunging strait in.

J.Ramsey
01-26-2008, 10:10 PM
Its never been a problem on shallow threads. Also the indexable insert tool I use has the right geometry for plunging strait in.

I guess you need to share your secret tool with all of us out of date thread chasers.

tattoomike68
01-26-2008, 10:36 PM
http://www1.mscdirect.com/ProductImages/0659214-11.jpg

The price is a bit spendy but they hold up for a long time. You need to go faster but the threads end up with a mirror finnish in 4140.

http://www1.mscdirect.com/CGI/NNSRIT?PMPXNO=16558239&PMT4NO=36659257

panchula
01-26-2008, 11:54 PM
29.5 does give a nicer finish. For illustrating the basic geometry, I thought the excerpt would be helpful for those who have anxiety about single pointing a thread. We're all at different points on the learning (not to mention tooling) curve.

mochinist
01-27-2008, 12:01 AM
I'm with tattoomike on this one

oldtiffie
01-27-2008, 12:23 AM
Here's the best explanation I've found of how far to feed in the compound for threading (and why).

http://www-personal.umich.edu/~panchula/ToolTravel2.jpg
..........................................
.........................................
........................................

Assuming the compound is set at 30 degrees, the compound travels along one leg of a triangle.
-Mike



Hi Mike.

Never mind the "flak".

I will cover that subject and a lot of others on screw-threading shortly on another HSM thread at:
http://bbs.homeshopmachinist.net/showthread.php?t=27274

Hi Mike (panchula).

I have completed my task on screw-threadind on the lathe at:

http://bbs.homeshopmachinist.net/showpost.php?p=329969&postcount=14

JCHannum
01-27-2008, 05:46 AM
Different texts and instructors assign various values for the compound setover. 29, 29-1/2 and 30 degrees are all presented as proper. With the crude graduations on most compounds, setting to 1/2 degree is only an approximation.

29-1/2 degrees can only be described as more than 29 degrees and less than 30 degrees, and keeps you somewhere in the middle of the range, thus it is somewhat "safer", but there is little reason to go to extremes to achieve the setting. A spring pass or two at the final compound setting is appropriate and will clean up most threads.

I have not seen the 0.75 method previously, and it is a handy tip. It will work well enough with either of the three setover values to get you close enough.

Thanks Mike, it is a keeper.

J.Ramsey
01-27-2008, 07:11 AM
http://www1.mscdirect.com/ProductImages/0659214-11.jpg

The price is a bit spendy but they hold up for a long time. You need to go faster but the threads end up with a mirror finnish in 4140.

http://www1.mscdirect.com/CGI/NNSRIT?PMPXNO=16558239&PMT4NO=36659257

Whats the finish like on softer materials say 1010-1045 cold rolled?
I've been using TNMC inserts for years with excellent results and I will always set the compound at 29.5 and use it.

John Stevenson
01-27-2008, 07:36 AM
Most of my threading is done with inserts out of Coventry die heads.
You only need one insert to do any threads of that pitch.

The holder is on the left.

http://homepage.ntlworld.com/stevenson.engineers/lsteve/hidden/threading_holders.jpg


The lathe I do most of my threading on has no top slide fitted so I can't feed in at an angle. It does have a top slide but it's in the lathe cupboard and has been replaced by a large block of steel machined to hold the toolpost and miss the tailstock when close.

The idea of this is you need rigidity 100% of the time and a top slide 10% of the time.

Given that a Coventry die head can't feed in at 29 degrees but still works I just plunge in and cut as if I was using a normal single point tool and it works for me with no problems.

The only time I do set over at an angle is on large pitch Acme thread when I have to rely on a single point tool with large cutting areas.

IOWOLF
01-27-2008, 11:15 AM
All that I know is that it has been this way for longer than all of us have been doing this,This is how I was taught and this is what I teach to My students or anyone who will listen.

I also use Mikes and Sir Johns methods, They to are good , But I still set the Compound slide to 29.5*,Just Habit I guess.

As a side note, on some lathes the compass is 90* off so you must set up accordingly.

J Tiers
01-27-2008, 11:47 AM
I've got another reason for using the compound, besides the chatter issue. If you have a large machine with a 200 lb carriage, you can ignore it.

If you feed straight in, you get approximately equal cuts on both sides of the bit.

IF your machine isn't perfect, if it has some slop in the half-nuts, or some slop in the leadscrew, etc, then the carriage can move relative to the bed even if the half-nuts are engaged, and the leadscrew is not turning.

So......... if there is some irregularity in the steel, or if one side of the cutter is a little sharper, etc, it is possible for the work to "take charge" and PUSH the cutter ahead of the leadscrew instead of being cut evenly.

Pushing will advance the cutter past the point it should be, distorting the thread form. You have no control over the cutter movement at that time, the leadscrew is not in control of the movement, the half-nuts are "un-loaded".

Then there is an irregular thread, not a proper helix, there is a "knuckle" in the thread at the point that the pushing occurred. If the half-nuts 'catch up" later and regain control of the cutter movement, there is another "knuckle" where the proper helix begins again. Successive passes may not straighten it out.

If, however, you do the 29 deg deal, then the cutting force always is pushing back AGAINST the half-nuts, and a "knuckle" is a lot less likely, even with considerable slop in the half-nuts etc.

A heavy lathe may avoid this. The carriage may be heavy enough and have friction enough that the half-nuts are always "pre-loaded" and the work can't push hard enough to unload them.

smiller6912
01-27-2008, 12:24 PM
Just a few links to some single point threading info tat I found interesting and, hopefully, useful......

http://www.mmsonline.com/articles/010302.html

http://www.manufacturingcenter.com/tooling/archives/0304/0304tooling_around.asp

http://www.manufacturingcenter.com/tooling/archives/0504/0504tooling.asp

http://findarticles.com/p/articles/mi_m3101/is_n8_v63/ai_9339164

Lew Hartswick
01-27-2008, 12:34 PM
How many times does it take to get it through you guys heads....

TWENTY-FRICKIN-NINE-AND A GOD DAMN HALF DEGREES.

Or you get lines.

NOT IF YOUR LATHE COMPOUND IS CALIBRATED IN DEGREES FROM
PALALLEL TO THE SPINDLE. ( SO THERE QUIT SHOUTING)

I'm sure there are more than the Clausing /Metosas that are so
calibrated. In that case it should be 60 and 1/2 degrees.

Now behave. :-)
...lew...

Carld
01-27-2008, 12:51 PM
It's my understanding that all CNC lathes plunge cut threads. The threads look good but I sure wouldn't try it on a manual lathe at those speeds and feeds.

If you check the compound deg. marks on lathes you will find they may be off 1 or 2 deg +/- so don't count on accuracy unless you check and remark your lathe.

I have been cutting threads using 30 deg since 1962 and turn out some mighty fine looking threads and class fit threads as well. I always stay just short of the 30 deg line so I suppose I am using maybe 29 deg, 55 min. but reallistically it's 30 deg.

I seldom use the plunge method but I have seen many fellow machinists do it on threads up to 10 or 12 tpi and get decent looking threads but not clean finishes that I like to see.

There is almost always more than one way to do a job. Some ways may turn out better fit and fnish than others but the job gets done.

djc
01-27-2008, 01:04 PM
No one has yet pointed out the error in the original diagram viz: the root is shown as H/8. Mr Oldtiffie's post shows the correct forms.

John Stevenson
01-27-2008, 01:07 PM
Here's a couple of pics of just plunge cutting in using an insert from a die head.

http://homepage.ntlworld.com/stevenson.engineers/lsteve/files/thread1.jpg

The thread is a 14mm x 2mm pitch so in English that's about 9/16" x 13 tpi or so.

The material is silver steel, what you call drill rod and as many know this isn't the best material for getting a good finish as it loves to rip and tear.

This is the same thread after 2 roughing passes and requires one more roughing pass, one finish pass and one spring pass.
The quality of the thread is claer on this shot.

http://homepage.ntlworld.com/stevenson.engineers/lsteve/files/thread2.jpg

This isn't a staged shot, it was part of a stub shaft for a motor and didn't even require a centre or end support.

.

Lew Hartswick
01-27-2008, 01:17 PM
John, Using one of those how can you get a complete thread up to
a fairly narrow stop groove?. It looks like the tapered start pitches
would never be able to do it.
...lew...

JCHannum
01-27-2008, 01:19 PM
All that I know is that it has been this way for longer than all of us have been doing this,This is how I was taught and this is what I teach to My students or anyone who will listen.

Burghardt "Machine Tool Operation" First Edition, 1919 gives 30 degrees.
Atlas Lathe "Manual of Lathe Operation", early 40's gives 29 degrees.
South Bend "How to Run a Lathe" 1934 Edition says "Some mechanics set the compound rest at an angle of 30 degrees...........but it is not recommended for the apprentice as it requires skill in grinding and setting the thread cutting tool."

Three pretty good sources, all older than most of us, none recommending 29-1/2 degrees. The compound should be set at either 90 degrees or something between 29 & 30 degrees. In the overall scheme of things it doesn't make a great difference as the thread is being cut with a form tool. It merely adds to the mystique of thread cutting and makes a simple lathe operation seem more difficult to the beginner than it really needs to be.

mochinist
01-27-2008, 01:20 PM
It's my understanding that all CNC lathes plunge cut threads. The threads look good but I sure wouldn't try it on a manual lathe at those speeds and feeds.http://img.photobucket.com/albums/v471/mochinist/fanucG76.jpg

IOWOLF
01-27-2008, 01:34 PM
Lew Did you read the unedited Post 15, or just post so quickly after reading my first post, Just to look like an A$$.

J.Ramsey
01-27-2008, 01:40 PM
I was taught that using the compound at 29-29.5 for a 60 degree thread the back side of the tool burnishes the back side of the thread.

When using the crossfeed only it cuts on both sides and the chips collide and results in a rough finish, at least in my experience with single point tooling.

cybor462
01-27-2008, 07:47 PM
First I am sorry these are not very good pics. My old camera like me is not working up to par any more.
I have been interested in this thread as I needed to single point and I have not done it in quite some time. I enjoy it but I have not done many fun things for me in ages. All the other work I do is for pay and I am slow enough as it is. I have to find ways to get er done quicker. I use dies and taps mainly for time and also since I run many more than 1zies I just can't afford to sp thread.
Ok so I needed to do it and I tossed off the rust (mental rust that is) and had at it. This is CR 1018 which we know can be a bugger to get a decent finish. Half my problem is it may be a decent thread but if it does not look nice I am not satisfied.
The first pic is both parts. who can tell me which is sp and which is die?
http://mywebpages.comcast.net/cybor462/thread.jpg
Both threads are quite decent in fit and operation but one looks like sh*t and the other much better.
http://mywebpages.comcast.net/cybor462/threads.jpg

I guess I gave it away.
http://mywebpages.comcast.net/cybor462/thread1.jpg

I used a HSS commercially ground tool as these threads are 3/8 40 and are quite fine. I normally use carbide tools but I do not have any that have a thin/fine point. I ran these on my Chicom lathe at 70 rpms using sulfur based oil. Compound set at 29.5 * and took .005 each pass until the final and then also took a free pass.

http://mywebpages.comcast.net/cybor462/thread2.jpg
As you can see this part the threads has snags and I am not pleased at all with finish. The fit is fine. These are for my project, yes the MLA 17 diesel engine.

Spin Doctor
01-27-2008, 08:03 PM
For myself it depends on the lathe and the part being threaded. Let's suppose it is three years ago before I retired. And I had a small diameter threading job that I was going to do on a Hardinge HLV-H. The thread was up to a shoulder with a minimal undercut on the back side. I would set the compound anywhere from 10 to 25 degrees and feed with the cross slide. Plus the tool would be set up with a chip breaker on both sides of the cutting edge. That is because I would have the threading dis-engaging trip dog set to kick it out of gear when I hit the groove. The compound is simply used to retact the tool via the quick retract lever. Feeding with the compound would place the tool progressively farther into the groove and I might hit the should. On a LeBlond or Harrison the compound would be set at 1/2 degree sort of the thread form and I would feed with the compound. On a Trak LXII the job would be done using the menu option that best fit the situation. But most likely 1/2 degree short of the included angle with progessively smaller feed steps.

GadgetBuilder
01-27-2008, 09:04 PM
An area not mentioned above is that threading tools have a tip radius that is larger for coarse threads. To get the thread right using the methods above it seems one would (theoretically) need a threading tool with a different tip radius for each pitch.

"Screwcutting in the Lathe" suggests using the compound parallel to the work axis, advancing the compound 1/2 the amount the cross slide is advanced. This moves the tool down the thread flank at about 26 degrees so it cuts mostly on one flank and shaves the other flank. Cleeve says this angle works well for 55 or 60 degree flank angles (29 degree flanks - Acme, etc. - use a compound advance of 1/4).

When the desired thread depth is reached, as read directly from the cross slide, then additional passes can be made at depth, advancing the compound to thin the thread until the gauge fits - this widens the base of the thread much as a tool with a larger nose radius would. Thus, one can use a single threading tool for all pitches with the nose radius set for the finest thread normally used.

I've been using Cleeve's method for a while now and prefer it to the plunge method and the 29 degree compound method because it is simple, works well, and I only need one threading bit for all the pitches I cut.

John

J Tiers
01-27-2008, 10:08 PM
I might mention also, that if you use the thread stop for threading, you are almost certainly feeding using the compound, presumably at 29+ deg.

A number of machines have a built-in threading stop, like the 2+turn ball type, or a standard option like clamp and thumbscrew.

S-B for one use the clamp and thumbscrew. I had to tell the dad-in-law what his was, obviously he doesn't use it.

Lew Hartswick
01-28-2008, 09:56 AM
Lew Did you read the unedited Post 15, or just post so quickly after reading my first post, Just to look like an A$$.
I just quoted your post #2 and was pointing that not all lathes
have the compound marked the same way.
Post 15 has nothing to do with it.
You were the one shouting and I just wanted you to notice. :-)
...lew...

IOWOLF
01-28-2008, 11:11 AM
Then You didn't read post 15,obviously.

BTW, What do you teach your students to set it at 30,29,29.5,or 60.5?

3jaw
01-28-2008, 05:40 PM
JCHannum said it best:


The compound should be set at either 90 degrees or something between 29 & 30 degrees. In the overall scheme of things it doesn't make a great difference as the thread is being cut with a form tool. It merely adds to the mystique of thread cutting and makes a simple lathe operation seem more difficult to the beginner than it really needs to be.

Now, the answer to the real question:
Exactly 32,478,935,521 angels can dance on the head of a pin. Look it up if you don't believe me!!! :D