PDA

View Full Version : Threading



patty boy
01-03-2009, 11:05 AM
I'm having trouble producing good threads when using carbide tools. My threads are only passable with HSS. I've been running the tools dry, but am finding improved results when I use a cutting lubricant. Can someone give me a short tutorial on threading and tools.

Lastly, where can you find HSS threading cutters that are pre-ground? I can sharpen them with little difficulty but for a new one I'd prefer to not start with an HSS blank.

johnl
01-03-2009, 11:36 AM
Try Grizzly
Johnl

S_J_H
01-03-2009, 12:07 PM
Mcmaster sells them preground individually-
Type in 2464 and it'll give you the page.
http://www.mcmaster.com/

Steve

Your Old Dog
01-03-2009, 12:58 PM
PattyBoy, I made set my grinder at 10 degrees and then made a guide to slide in my grinders track of 30 degrees on one end and the same on the other. Now its a snap to grind thread cutting HSS bits from blanks.

A few things that helped me with threading were"


Make sure the tool is sharp.
Make sure the tool is on center with the stock.
Try and use the tail-stock whenever possibles.
Don't extend to much stock out of the chuck, keep it short as possible.
Make sure the compound is set to 29.5 degrees.
Make sure and set the cross feed to zero when it touches the work. Lock the cross feed down.
Make sure to in-feed with the compound and not the cross feed.
Realize these threads are all made in several light passes and not one heavy plow cut.
Be sure to realize that a file plays an important roll when you are finished with the lathe. Most of the perfect threads you see on this site were cleaned up with a file.
There's more to it then what I indicated but that will get you thinking in the right direction. Rigidity and tool placement would be my main concerns if I were you.
If you post some pictures someone will be able to help straighten you out.

Fasttrack
01-03-2009, 01:26 PM
Going along with YOD, remember that most carbide inserts have a certain radius at their tip. That radius prevents you from cutting a fine thread, since the root of the thread is smaller than the radius of the insert. And, obviously, you need to be using triangular inserts with 60* included angle for standard threads :)

mochinist
01-03-2009, 02:12 PM
I don't remember the last time I turned the compound to do a thread, probably when I was turning an acme, and feeding with the crossfeed will work fine also. I'm not saying you wont make a better thread the other way but it isn't as necessary as some people would have you believe. Most of my threading is done on cold rolled steel or 304 ss also just for reference.

Fasttrack
01-03-2009, 03:42 PM
I don't remember the last time I turned the compound to do a thread, probably when I was turning an acme, and feeding with the crossfeed will work fine also. I'm not saying you wont make a better thread the other way but it isn't as necessary as some people would have you believe. Most of my threading is done on cold rolled steel or 304 ss also just for reference.


Do you do that with carbide inserts, too? I've fed with cross-slide and compound, depending upon the job. I've yet to feed with the cross-slide and not chip a carbide insert. Now, I always feed with the compound if I have to use carbide.

mochinist
01-03-2009, 03:54 PM
Do you do that with carbide inserts, too? I've fed with cross-slide and compound, depending upon the job. I've yet to feed with the cross-slide and not chip a carbide insert. Now, I always feed with the compound if I have to use carbide.All carbide, I have one HSS steel thread cutter that I ground in trade school, I dont remember the last time I used it either, I think it may have been on a piece of plastic rod I was threading.

dp
01-03-2009, 03:56 PM
Since the compound has to be there, and since the compound needs to be set at something, why not 29.5? No significant time or steps are saved by not doing it, and the advantages stated endlessly in the literature about using the compound for threading can be easily followed. It isn't worth a religious war defending one way or the other but for the general case I fail to see any advantage while seeing a disadvantage in threading only with the cross feed.

Fasttrack
01-03-2009, 04:14 PM
Yep - I don't reckon its worth a flame war :)

So whats the trick, Mochinist? Very light DOC, lots of heavy oil, something else entirely? Seems like I always get through the first several passes no problem and right as I near the end, I chip the carbide and bugger it up! :) I use HSS for everything that doesn't strictly need carbide now.

mochinist
01-03-2009, 04:31 PM
Since the compound has to be there, and since the compound needs to be set at something, why not 29.5? No significant time or steps are saved by not doing it, and the advantages stated endlessly in the literature about using the compound for threading can be easily followed. It isn't worth a religious war defending one way or the other but for the general case I fail to see any advantage while seeing a disadvantage in threading only with the cross feed.
Well a compound doesn't need to be there, but that is besides the point:) Literature is great and it usually shows the correct way to do things, and I was also showed the correct way and it has its place, then I was showed how to get things done faster and make money, while the other guys were fussing with angles and every chart the literature told them they needed to have and use to get a good thread, this was by an old machinist that had trained and worked at some armory up in New York



Yep - I don't reckon its worth a flame war :)

So whats the trick, Mochinist? Very light DOC, lots of heavy oil, something else entirely? Seems like I always get through the first several passes no problem and right as I near the end, I chip the carbide and bugger it up! :) I use HSS for everything that doesn't strictly need carbide now.I dont get why it chips it at the end, my last few passes are really light, I take out a majority of the meat on the first few passes, and yes a lot of cutting oil. I don't know if there is really a secret, but I like to thread at higher rpm's than I see posted on here for threading.



and who's flaming? no one mentioned bearings in this thread yet :D

juergenwt
01-03-2009, 05:49 PM
Old dog has all the right points. I prefer HSS hand ground. Here are some trick of the trade:
Use a HSS blank. Set it up at 30 deg from the horizontal plane and grind the 30 deg angle on the left side of the tool bit. Depending on the size of the blank - let's say you use a 5/16 blank - grind the angle to where there is about 1/8 left at the end.
Now move your blank another 30 deg. and grind the 1/8 portion on top to a sharp point with the right side of the tool bit. You now have a nice 60 deg. point at the tip.
Now on a bench grinder back off just the left side of the 60 deg point (right hand threads only).
As for the top rake - depending on the material you want to cut - I like to just use the radius of a 6 inch grinding wheel to come to a sharp edge on top of the 60 deg portion.
For right hand threads there is no need to back off the right side of the 60 deg..
Stone the sharp edges very lightly and stone a very small radius on the tip.
At the start you can take a heavier cut. The closer you come to your finish size you must take less and less. Your final pass should be with the same setting on the compound. Use a good cutting oil except for brass. Check to make sure it is OK to use on Aluminum.

http://i305.photobucket.com/albums/nn219/juergenwt/Toolbit.jpg

This has the advantage of letting you cut real close to a shoulder and keeps your holder away from the chuck.
As to the 29.5 deg compound setting - it's a must. you are feeding in at 29.5 deg., you tool bit is 60 deg. The main cutting action takes place on the left side. There is no chip coming of the right side to interfere with the chip from the left side. By feeding in at 29.5 deg it will leave .5 deg on the right side for a nice clean up. juergen
Follow up:

May be these pictures will explain better what I am trying to say. Look at the extra clearance between the chuck and the tool holder when using a 30-60 deg threading tool.. As far as backing off your cutting edge - a slight back off will change your 60 deg a very insignificant amount.
http://i305.photobucket.com/albums/nn219/juergenwt/DSC01738-1.jpg
http://i305.photobucket.com/albums/nn219/juergenwt/DSC01737.jpg

SDL
01-03-2009, 06:02 PM
Going along with YOD, remember that most carbide inserts have a certain radius at their tip. That radius prevents you from cutting a fine thread, since the root of the thread is smaller than the radius of the insert. And, obviously, you need to be using triangular inserts with 60* included angle for standard threads :)

Not if you are using the full form thread inserts that have the correct profile for the root and crest. Most of the lay down tips are designed to fed in at an angle or cut on alternate flanks if the CNC progame is available.

Steve Larner

Your Old Dog
01-03-2009, 09:28 PM
When you advance the 60 degree cutter into the stock using the cutter set at 29.5 you are only really cutting on the left side of the cutter. This means you will be taking half as much cut and therefore not over stressing the stock or the lathe. This should translate to less vibration. This issue was part of my learning problem and coupled with my bit being a shade to low it was the reason my threads looked so ratty. You gotta move one in anyway so doing the compound instead of the cross slide just makes it easier on the setup and gives you more control. IMIHO

loose nut
01-04-2009, 11:55 AM
Patty boy, for what they are charging for the pre-ground tool bits it would be worth your time to practice grinding them from tool blanks, it's isn't very hard and it's a skill you can use to impress the friends and family.

dp
01-04-2009, 03:02 PM
Patty boy, for what they are charging for the pre-ground tool bits it would be worth your time to practice grinding them from tool blanks, it's isn't very hard and it's a skill you can use to impress the friends and family.

I have several feet of 3/8" square stock CRS. One day I decided I needed to practice grinding cutters so I cut up some of this stock into cutter-length sizes and went at it on the grinder. The stuff is dirt cheap compared to HSS and you end up with a great looking piece of metal that is useless for cutting but what a great experience it was. The setups for grinding CRS "cutters" is the same for grinding HSS and that is what I was after. It was good practice done on the cheap. It was also a good exercise for my radial arm saw-turned-grinder :eek:.

I will add that once I started grinding HSS it was pretty slow sledding :D

tdmidget
01-04-2009, 03:45 PM
I'm pretty much with Mochinist here. I worked for a German machinist and he caught me threading with the compound and had a fit, said that was BS. I thereafter did all my threading in that shop with the cross slide and no problem. I have cut many 32 pitch this way and have seen him cut a 40. I have used this technique on threads as coarse as 8tpi and it works. Use light cuts, remember you are cutting with both side of the the tool. Use a fairly heavy oil and take a spring cut at the end. All we ever used was carbide, usually insert tools but some hand ground.

bob ward
01-04-2009, 06:02 PM
I get good looking threads by cutting 90% of the thread on the lathe with a carbide threading insert, plunge or 29.5 cutting as the mood takes me, and finishing off with a die.

This works better for me at my current level of expertise than 100% on the lathe or 100% with a tailstock die.

If I'm don't have the right die, then of course it is fingers crossed and 100% on the lathe.

Mark Hockett
01-04-2009, 07:28 PM
I'm pretty much with Mochinist here. I worked for a German machinist and he caught me threading with the compound and had a fit, said that was BS. I thereafter did all my threading in that shop with the cross slide and no problem. I have cut many 32 pitch this way and have seen him cut a 40. I have used this technique on threads as coarse as 8tpi and it works. Use light cuts, remember you are cutting with both side of the the tool. Use a fairly heavy oil and take a spring cut at the end. All we ever used was carbide, usually insert tools but some hand ground.

That German machinist didn't have a clue. In-feed angle plays a huge role on tool wear and productivity. When the tool enters the work on a perpendicular path, radial in-feed, the tool cuts on the nose and both flanks so you are wearing the tool because you have more surface area in the cut. Along with that chip control can be a problem as the radial in-feed creates a V-shaped, undirected chip. Chip flow is more directed with a flank in-feed which will also give you longer tool life and better surface finish. It has also been well documented that the thread surface finish is much better with a flank in-feed. There is a good article in the December issue of Cutting Tool Engineering magazine that goes into detail about threading in-feed. It spells out the problems with radial in-feed.

Here is a FAQ from the Vardex site,

Q: What is the recommended in-feed method ?

A: Flank in-feed has a better chip control and surface finish in most raw materials and applications.

Here is a quote from Peter Smid out of the CNC programing handbook,
"The result of a radial in-feed motion is that both insert edges of the threading tool are removing material at the same time. Since the edges are opposite to each other, the curling of the chips will also be opposite to each other. In many applications, this will cause high temperature and tool wear problems related to the heat. Even decreasing depth for each in-feed may not eliminate the problem. If the radial in-feed does not produce a high quality thread, a compound in-feed approach will generally do a much better job."

He also recommends radial in-feed only for soft materials such as brass and some aluminum and states that it could damage threads cut in harder materials.

As I said it is well documented in the machining industry what the proper threading approach should be.



Use light cuts
How is that helping get the job done faster if you are taking more light cuts, I use a flank in-feed and take some serious cuts and get long tool life as it takes less passes.



I have used this technique on threads as coarse as 8tpi and it works

One of my contract jobs is making spindles for wood turning machines, I make hundreds of spindles a year for them. They are all 1"X 8tpi. I have done extensive testing on different in-feeds as it is a simple A code to change the in-feed angle on my CNC lathe. Radial in-feed will cut the threads but they look like crap under a magnifying glass. Flank in-feed on my lathe produces a thread that looks like it was ground.
One other item that is not so much of an issue on a CNC lathe but can be on a manual lathe is maintaining pressure against the lead screw. using a flank in-feed puts more pressure on the lead screw which helps fight chatter.