More threading questions

[gonzo]

As a bewbie, I consulted the u tube videos on how to cut threads. I followed the directions and was totally pleased with the results. However I subsequently forgot the drill over time and the next time I made threads I forgot to advance the cut using the compound adjustment and instead used the cross feed. The results were quite acceptable and I ended up with a beautiful set of threads. Only later did i discover my error but now I am wondering why to use the compound advance in the first place if the result of using the cross feed works so well.
Seeking comments.

 

[Latinrascalrg1]

When you use the compound correctly you are essentially only cutting on 1edge of the tool which helps maintain a cleaner cut for a few different reasons where as plunging straight in with the crossfeed you will be cutting on 2 cutting edges so you have a a bit less control on "Sneeking up" on that correct spec as well as applying more heat through more friction as well as a few others im sure.

Anyway that's the gist of it....hope it helps.

 

[epanzella]

I made the same discovery 20 years ago and haven't used the compound for threading since! Using the xfeed only cuts on both sides of your cutting tool so requires a bit more rigidity. Locking the gib of the compound or better yet eliminating the compound when threading gives you that rigidity. I replaced the compound on my present lathe and my previous lathe with a solid tool block. It also helps with parting off. I only use my compound for tapers.

 

[benmychree]

There is much more chance of the tool hanging up in the cut and bending the part being threaded, especially with long threads and coarse threads, when feeding straight in. A professional machinist would almost never thread like that, we always use the compound for threading. One problem is that with the chip being generated on both sides of the tool, the chips interfere with each other at the point of the tool. Having said all that, sometimes we will feed straight in for the last couple of thousandths to finish a thread, this will cleanup any steps or roughness on the backside of the thread, it can also be done by causing a slight drag on the carriage handwheel with the fingers on the free cut when finishing.

 

[plunger]

Im too lazy to offset my compound. Most of my stuff is in brass.Sometimes I just wind the topslide closer to the headstock if I want to clean it up a bit on tuff steels like stainless.I was taught during my toolmaking aprenticeship to set the compound over to 29 and a bit degrees but honestly in my homeshop environment I get along fine by being lazy.Im now a plumber so I dont have to be exact.

 

[benmychree]

I was told that the custom in Germany was to have the compound at 90 deg. and so much feed in, and so much feed over; this guy, Karl Groneck came into my apprenticeship shop "right off the boat" and had little English, and had a lot to learn about our way of doing things, the compound at 30 deg. was one of them --- and nobody in the shop did the 29 degree thing.

 

[Bi11Hudson]

The one factor that hasn't been covered here is that with the compound set at 30*, feed is a direct factor of 1/2. The Sin of 30* being 1/2. So that each .001 0f feed, you actually feed .0005 in and .00086 forward. In most cases, it only results in a little smoother cut. But there are cases where it would make a difference.

 

[stupoty]

I use a threading stop on the cros slide so my depth is set by that which makes for quick reset after each pass, I do see a lot of people just use the cross slide, as mentioned courser threads require a more rigid set up for that but with fine threads theirs probably very little issue.

It's sort of one of the things that can be done a few different ways and so long as it all works well for you that's the main thing

Stu

 

[mikey]

... but now I am wondering why to use the compound advance in the first place if the result of using the cross feed works so well.
Seeking comments.

You are going to find that in softer materials using smaller diameters to cut smaller thread pitches, 20 tpi or less, feeding straight in with the cross slide is fine. The amount of cutting edge engaged is small, heat generation and chip evacuation is not a major issue and the thread form usually turns out fine. Tool life is also good under these conditions.

In harder materials and larger diameters, especially if you use carbide inserts, then feeding in with the compound is favored. The key reasons this is preferred is that it limits the amount of edge contact sustained by the tool. This reduces cutting forces, heat production and enhances chip clearance. Because of reduced edge contact, deflection is also reduced so accuracy is more easily obtained.

A threading tool is a form tool. On smaller threads, especially in softer materials, cutting forces are easily managed but in larger threads the amount of edge contact does matter. You are essentially cutting with a zero rake form tool so ALL the cutting forces are on the edges. Feeding straight in with a form tool is a recipe for chatter, deflection and poor finishes on a manual lathe cutting deep threads, which is why using the compound for larger threads is favored.

Many of us use inserted carbide threading tools. The geometry of these inserts is fixed, although you can alter that geometry by using different anvils under the insert to match the helix angle of the thread. When using inserts, I have found that feeding with the compound tends to work better because I cannot alter the geometry of the insert so I have to minimize cutting forces by minimizing edge contact.

When using a HSS threading tool I can increase the relief angles to reduce forces so I can cut with either the cross slide or compound without too much trouble. You might not think the relief angles on a tool matters but I have found that a relief angle of 12 degrees may chatter, while 15 degrees will not.

Cutting forces always matters and on a threading tool, the only controls you have are your relief angles, your approach angle and depth of cut; speed and feed is what it is. So, choose your tools well and use them to your advantage.

 

[mksj]

A number of different factors come into play as described above, but a major determent is the cutting tool/insert and the rigidity/weight of the machine. I started out using the compound on my 1340GT, and later switched to the cross slide and reduced the amount of material removed per pass. I prefer the cross slide because the stop position is always the same when using an electronic stopping system, the cutting edge completes in the same grove/place. The difference between the two was an extra pass with the cross slide method. Finish wise it was about the same.

Increase the rigidity of the machine and thread cutting tooling, then the cross slide works well. I find the laydown threading inserts to worked better than the TNMA/TNMC types and are quite durable. I have used the same laydown insert for many months and still on the same cutting edge (it has 3). My current lathe is 2400 lbs and doesn't really care either way. I get very clean cuts with the cross slide, the cuts are w/o chatter. There is always an issue with the chip curl/removal when taking deep cuts with the cross slide. What is also important, in particular with the cross slide threading is to reduce the material removed in the last 2-3 passes. On deeper threads I typically take 0.01" passes x 5-6, then reduce the subsequent passes as I get to my target depth, and then do a spring pass. With an electronic stop, I recently did a bunch of threading and it took about 1 minutes to complete all the passes. These days I have been threading O1 rod at 400-450 RPM for 3/8-5/8" diameter, threads pitch varies typically from 12-24 TPI. Finish of the threads was better than my threading die. On less rigid machines, using the compound is more ideal and then do a finishing pass at a reduced depth with the cross slide gave optimum finish with the least amount of passes.

M16-2.0 using the cross slide.


The attached chart shows an example of tapering the cut depth as you approach the target depth, and then a finishing spring pass at 0.001". There is always some level of deflection and also the ability of the cutter to take off a small amount of material, so even a spring pass can remove a significant amount of material and needs to be factored in when you want minimal clearances. Multiple spring passes often will result in chatter.