What's new
What's new

What causing this "galling"?

FlyinChip

Aluminum
Joined
Dec 20, 2017
Hi all, I was slowly cutting threads using HSS and had this what i call galling issue. Then I bought a Carbide 60 degree cutter and had similar issues. I went a little deeper and the tip broke off, so scratch one brand new bit. Slow speed. Not sure why this happening but I'm not very experienced.

Somehow it seems like maybe the 1018 steel part metal quality may be an issue?

Stumped!

threads galling by Chris P, on Flickr
 
Could be lots of things. We need to know what speed you're threading at, it could be possible its TO SLOW, tearing the metal instead of cutting it. Also did you grind your HSS cutter by hand? Clearances my be off. It also looks like you're cutting on both side of the thread, do you have the compound set to 30 degrees, or 29? 1018 can be hard to work with as well. Poor finishes especially with carbide are common at low speeds. Carbide needs to run very fast as opposed to HSS
 
Very typical problem for something like 1018 steel.
Try smaller DOC and occasional "spring pass" between cuts. Good thread cutting oil is also helpful.

Something like 4140 prehard is lot easier to get nice threads.
 
Thanks for the reply guys. Lot of good leads to follow.

Like I said I am new. It's a 60 degree tool so I assumed threads are fully cut going in 5-10 thousanths per pass and didnt think the compound angle made a difference since the tool would be going straight in about 5 thiousanths or so per pass.

No oil was used I will try that, have 766 on hand.

Yes was turning very slow. This is 3/4" diameter 10TPI

Using thus piece 1018 for practice run before I get into the 304 for the actual part. It's a,long piece so I can try until I get this right.

Made the HSS tool myself (actually modified one to fit into an example thread) but bought the 60 degree carbide tipped tool when that didnt work, assumed I made it wrong and the store bought would work.

when u say carbide likes fast, what rpm/sfm would be correct for this job?
 
1018 is hard to thread smoothly. You absolutely need a cutting oil. Try some dark pipe threading oil from the hardware store. IMO, the speed thing is overrated. I can thread with properly sharpened carbide at any speed, though it does work better faster. That can also be coating dependent, as some need heat to work right.

Many times you can get away with plunging the tool straight in, but the proper way is to use the compound so the cutter mostly cuts one side of the thread and just skims the other. Thus the 29.5 or similar angles they tell you to set the compound to. They aren't all marked the same, so I tell people to point the handle at their belly button, then rotate it CCW by 29.5 degrees. In that position the tool still have to be properly aligned to the part- use a fishtail gauge.

I've got some (hopefully) useful stuff at the bottom of this page- Metric Threading
 
Assuming this is on a manual lathe its very difficult to get above the speed range that causes tearing. For 3/4” diameter you probably won’t see much improvement from speed alone until 2000-3000rpm.

One thing I forgot to mention is really sharp and mirror polished tool.

I would drop the depth of cut to 0.04mm or even just 0.02mm for the finishing cuts. And if the surface is already torn like that you need lots of finishing passes.
 
That's ugly. Even the thread relieve and shoulder are having a problem.

1018 usually plays a bit better than that, though it can still be ugly.
Are you sure its not A36?

In my experience, there are three ways to get good finishes on a low carbon
steel, and even annealed 4xxx to some extent. Either SPEED, bigger Depth of Cut,
or really fricken sharp.

Or some combination of those 3 things.

One thing I have noticed with low carbon steels, sometimes you will get a better
finish if you are running wet, and sometimes you're better off running dry. I guess
there is a sweet spot for everything.
 
and... I thought this course thread on mild steel would be easy !

good point I bought 1018, who knows if was accidentally mixed up though? more likely it's my technique and lack of experience. will keep trying but will have to switch back to HSS and learn to make my own bits.

Confused though about coming in at 29.5 degrees or whatever. The tool is 60 degrees and going into a straight surface. It's gonna cut both sides of the point anyway, no?
 
1. If you are grinding your own HSS tool, be sure you understand how to properly do the rake and relief angles. And understand that those angles should be different for different work materials. The threading tool for steel will have side rake, so it only cuts on the left side of the tool. That means it has to be fed into the work at a 29 to 30 degree angle so it does not try to remove metal with the right side of the tool. I think the South Bend How to Run a Lathe book has a section with explanations of tool grinding. There is also a section on threading. The book is free online somewhere. Altas Press Co. also published a good book on lathe operating. Here is a short explanation of grinding tool bits: https://littlemachineshop.com/images/gallery/instructions/grindingtoolbits.pdf

2. Get some 12L14 steel bar for practicing lathe work. You will be amazed at the difference between that and 1018. It will make it much easier to get good results, even when cutting dry, but only if you get the tool geometry right.

3. If that 60 degree carbide tool you used is a style E brazed carbide bit, then it is not suited for threading steel or stainless. The top is flat and has no back or side relief, which is fine for turning brass, but really bad for turning steel.

4. Cutting oil will help when turning steel. The smelly dark pipe threading oil is good for 1018. There are some fluids specially advertised for tapping, and they will work fine for single point threading in a lathe. Some of those tapping fluids are advertised as being good for stainless.

5. Learn about machinability of metals. That is a scoring system that predicts how difficult it is to machine various metals. Note the numbers for 1018, 304 and 12L14 and take warning.

Metals Machinability

Larry
 
Confused though about coming in at 29.5 degrees or whatever. The tool is 60 degrees and going into a straight surface. It's gonna cut both sides of the point anyway, no?

If you come in at half the 60 degrees you are only cutting on one side. 29.5 degrees in theory does almost all the cutting on one side and just a very light skim on the other to not leave step marks.

Even when programing a turning center I alternate flanks. Less chance of chatter and so on.
 
Speed and lots of top rake plus lube.
That is a great picture. One can see the tool loading and unloading and the re-welding process.
Is it okay with you that I copy this picture and use it to help others? (Blatant up front, can I use your photo for my own commercial gain)
Bob
 
and... I thought this course thread on mild steel would be easy !

good point I bought 1018, who knows if was accidentally mixed up though? more likely it's my technique and lack of experience. will keep trying but will have to switch back to HSS and learn to make my own bits.

Confused though about coming in at 29.5 degrees or whatever. The tool is 60 degrees and going into a straight surface. It's gonna cut both sides of the point anyway, no?

If you are coming straight in, that would contribute to your problems. Try setting your compound at 29.5
degrees and only cutting on one side. Oh, one other thing, that is not galling, it is tearing.

JH
 
Some test shots that I took in similar situation: (material is european S355 structural steel, close to US 1018)

KcU4zIDh.jpg


Same hss tool and speed but smaller DOC and LOTS of finishing passes:

6gOgwi5h.jpg


edit: forgot to mention, I have had slightly better luck with coated carbide(Mitsubishi VP15TF) than HSS despite what some old farts might tell you. Chip is less prone to friction weld to the coated carbide than HSS.
 
Thats from the side of tool. I had this smooth and only the threads got tearing.

I finally understand about the 30 degree compound, pushes tool off to one side a little. I'll look for some technique video when I get home...
 
I see where some guys are recommending top rake on your tool but personally I always make my threading tools flat on top. I grind them out of a new high speed tool and just leave the factory finish on the top of the tool. The smoother the top is the better. This will prevent the chips from welding to the top. That's what usually causes a nasty finish like this. The cutting oil and feeding the compound it at 29 1/2 degrees will both help. Carbide tools are great in a cnc or in a manual for a really experienced operator where you can run some high rpms but for a newby I feel a high speed tool is the way to go. The tool needs to be sharp and have the proper clearances though.
 
Reminds me of some of my first threads I cut over 50 years ago. Mobilmet 766 you mentioned should give you good results and good finish. As others have said, it's in the grinding and honing the edges of your threading tool that count. 10 tpi should not be a problem cutting at around 100-125 RPM. Maybe even a little higher if you are brave like me. Usually for me, I'll run at about 250 RPM. But you have to be fast at the half nuts.

It takes practice, practice, practice to get good at single point threading. For the stainless steel you're talking about, you will have to cut your speed down to around 50 RPM and lots of cutting oil! But, get your practice on that piece of 1018, and the SS will be almost a breeze!!!

Post pictures of your cutting tool, that may help us help you in getting it right. Ken
 
Looks like a plunge cut straight in. Finish on both flanks is identical. Op needs to use the compound and come in at 29 degrees.
 








 
Back
Top