Anyone have thread cutting experience using lathe?

CuriousOne

Hello.

Recently I've purchased littlemachineshop's mini lathe. While I know how to do basic tasks with lathe, I never tried to cut threads with it.

I need to cut M42X1 thread on aluminum. I've set the gears so pitch is correct, but I don't know, which thread cutting tool (head size) I have to use for such fine threads.

Any ideas?

Thanks in advance!

garyg

I'm not sure if this will help you, but I found this link http://mdmetric.com/tech/M-thead%20600.htm
It shows diameters, angles and such.
I have not done any metal lathe things in quite a few years.
Threading always gave me much trouble.
I usually ended up using the technical skills of a local machine shop for things like you are describing.

I hope this helps you in some manner

pedward

When cutting threads, you can use a few methods.

a) Full form carbide inserts
b) simple pointed carbide inserts
c) brazed carbide
d) Ground HSS tool bit

In the above examples, a) are sold per the thread pitch you are cutting, because they have a follower that cleans up the crest when you are cutting the thread, these are typically used for production work on single point threading.

For b) some inserts may not have sufficient clearance for very coarse threads, so they may be sold in 1-4, 5-40, and 42-120 pitch increments. Often times you can simply find a do-all insert in this genre.

For c) and d) you have nothing more than a simple 60 degree point that cuts the thread in successive passes. These are often the simplest and cheapest to use and setup.

Genetix

How many parts do you need to make, how long is the thread, and is this an internal or external thread?
I've cut threads on a CNC which a lot easier than on a manual lathe.
If your lathe has gearing for the thread pitch then you only need to worry about the Major and Minor diameter of the threads.
For an external thread, the major diameter is the Outer Diameter (OD) and the minor diameter is the Inner Diameter (ID).
For an internal thread, it's reversed since the Major Diameter is always bigger than the Minor Diameter.
The thread depth is the difference between the major and minor diameter.

For turning and facing you can use HSS (high speed steel) tool bits but for threading you should consider getting a threading tool-holder for carbide (tungsten carbide or TC) inserts.
Place a notch deeper than the thread depth in front of the thread so you have a place to adjust the depth before you start cutting.
Aluminum is easy to cut but if the thread is long then it's best to use coolant to keep the tool cool.

Mark Mara

Good information so far. Practice on delrin or some other soft material. Lots of light cuts. Run your machine at very low speed until you get a rhythm going.

PropGuy2

Practice, practice, and more practice.. For what its worth, soft metals like aluminum are very difficult to machine, to get the accuracy and finish (smoothness) for threads VS harder metals like steel. I would use an insert if at all possible.

CuriousOne

Thanks a lot.

I need to cut both inner and outer threads. I'm volunteriing at local university and we're building telescopes from old camera lenses.

Regarding the cutter type, I know there are different types, but exactly which pitch (model) of cutter I need for this thread ? this is the question

Genetix

If you have access to taps and dies then use those but if you have to buy them they can be expensive.

External Thead - Class 6g
Major Dia: 41.79 - 41.97
Minor Dia: 40.583 - 40.891
Pitch Dia: 41.2 - 41.32

Internal Thread - Class 6H
Minor: 40.917 - 41.153
Major: 42 - 42.314
Pitch: 41.35 - 41.52

The pitch is determined by the feed rate and it can be measured using a Pitch Micrometer
On an external thread, turn to the Major diameter and the Minor diameter is determined by how deep your theading tool cuts.
On an internal thread, turn to the Minor diameter and then cut until the Major diameter is reached.

It's probably best to aim for the middle of the Major and Minor diameters.
The internal thread is trickier because you can't see what you are doing.
Also, on the internal thread the tool needs to be pointed TOWARDS you and you will cut into the surface in front of you.
(The part spins CW looking INTO the Head Stock and you want the part to move INTO the tool)
A thread is 60-degrees so used a tool or insert with a 60-degree INCLUDED angle.

Practice on some scrap stock before cutting your parts.

CuriousOne

No, I have lathe, so I'd like to cut with lathe,not with taps and dies.

M42 tap or die costs around $400

Irone

Hello,
I am an old machinist. I have cut many threads on a lathe. According to your last post you need forward and backward threads to accompany the focal length needed to adjust the correct space to clearly see distant objects. This will need correct pitch diameters which can easily be accomplished with wire gauges and a micrometer.
First you need to make the male part according to the wire gauges and then fit your female part to the male part. Your camera lenses will probably have no reverse threads in them so you will have to make this a two sections arrangement with the camera lenses tied together with a bar. I would definitely use a single HS tool ground to sixty degrees and alighted with what we machinists call a fishtail. (It lines the sixty degrees with the diameter)

CuriousOne

Great!

Now I need someone who will tell me that I need to buy this particular part number cutter.

Irone

Hello,

I should have underlined the old in my last thread. Every thread I have cut on a standard lathe has been made from a HS tool bit blank that has been taken to a pedestal grinder and modified with 60 degree angles to form the thread. I drew up a diagram which shows a tool that can be used for outside and inside threads. I have found out if you groove the inside to the major diameter and run the lathe in reverse inside threads are easier to cut. Also if you take a flat stone and radius the 60 degree point around .003 to .008 (don't be fussy, just a few swipes) will keep the end from cracking at the top. If your inside threads are longer you must put a modified tool bit in a boring bar.

Attachment not found.

Mark Mara

Running a lathe in reverse can be very exciting if you have a screw on chuck. No problems if your chuck is a cam lock type, but the cutting forces can cause a threaded chuck to unscrew running in reverse. Tight chuck and light cuts should be OK, but be warned.

tranger

Thread chasing can be tricky. It has been a long time since I've done it, but used to a lot of external threads. Not sure how familiar you are with the process, sorry if it is obvious.

You have to set the compound slide up to 30 deg (or 29.5) and use this to advance the tool. The tool will then cut only on one side. The cross slide is used to quickly move the tool out to a clearance position and then back in to the cutting position. You always return the cross slide to the same place before cutting. The tool is not fed by the normal feed, but by engaging the half-nut with the lead screw. There is an indicating dial that is used to time the engagement of the half-nut. Engaging with the dial at the same number every time ensures that the tool is "in-time" with previous cuts. Depending on the pitch and the lathe, there are some rules about what other numbers can be used so you don't have to wait a long time for your number to come around.

If you have a thru hole or a simple diameter, then the timing of releasing the nut and backing out the tool is forgiving. And that is the sequence - release the nut and then back out the tool. If you are threading to a shoulder, then the timing can be fast. Running as slow as practical is best. It is also worthwhile to try to start the cut in a relief if there is a shoulder and then feed the tool away from the shoulder. You can flip the tool upside down and reverse the spindle to do this.

McMaster Carr has HSS lathe tools ground for od work and Carbide tools for ID work. http://www.mcmaster.com/#3364a36/=r30iun http://www.mcmaster.com/#3369a26/=r30jan
Which tool you buy depends on the thread and what toolholders you have.

edit: this is interesting http://www.aliexpress.com/store/product/Free-ship-Lot-1pcs-Metric-Right-Hand-Die-M42X1-Dies-Threading-Tools-42mmX1mm-pitch/827733_959751255.html

Good Luck.

-Russ

CuriousOne

Thanks a lot, at least some p/n's!

The question is, how from this data:



Minimum Hole Diameter
0.23"


Maximum Hole Depth
0.75"


Offset (A)
0.055"


Shank Diameter
5/16"


Overall Length
2 1/2"




You've figured out that this can be used to cut 1mm pitch metric thread? as I guess, the first two parameters are key to that, 0.23" and 0.75", right?

tranger

I wasn't intending to select that specific tool for you, but wanted to give you a place to go to pick one out. Since you are working with a 42mm diameter, the Minimum Hole Diameter isn't really important. The Maximum Hole Depth of 0.75" tells you how far the tool can reach into the part before the the shank interferes- this would be very important. The offset (A) dimension tells you how deep of a thread you can cut. 1mm pitch, 60 degree threads are 0.867mm deep (to sharp corners) or 0.034". The A dimension needs to be larger than that. The Shank Diameter and Overall Length are relevant with respect to the tool holders you have available to make sure you can clamp it up.

Here is a list of this style of tools available at McMaster Carr: http://www.mcmaster.com/#internal-threading-tools/=r3j2r9

I noticed that the maximum thread depth available from these tools is 1.00". If you need to reach further into a part, these tools won't do the job.

edit: Ebay also has a pretty good listing of tools: http://www.ebay.com/sch/i.html?_trksid=p2050601.m570.l1313.TR0.TRC0.H0.Xinternal+thread+toolholder&_nkw=internal+thread+toolholder&_sacat=0&_from=R40

The indexable insert style has the advantage that if you bugger up the tool you can just rotate the insert and get a fresh edge (as long as you don't really wreck it...) It looks like they are pricer and of course you have to buy inserts in addition to the holder.


-Russ