What's new
What's new

Turning 1018 Steel

Circuit 1

Aluminum
Joined
Nov 14, 2015
First off I'm still really new to the lathe. I have a SQT-10M lathe with T-Plus control and all I've turned is Aluminum and Plastics. I have a small job I need to do with 1018 steel. I've read little about feeds and speeds but my main question is about DOC. Everyone says not to baby the cut but what about when boring and you're trying to hit a few tenths. Do you just scrap parts until you get to the number or can you take a few tenths off like with aluminum to get the number you need? And is it better to use coolant or not? Also a little input on some conservative feeds and speeds would be appreciated. I only have a few of these to do.
Thanks!
 
I'm a hobby guy and as such many times deal with less than desirable steels like 1018 and can't really crank DOC, feeds, and speeds on my machine to get good results with a typical carbide setup. But just recently I tried a common hobby trick which was to use sharp aluminum inserts for finishing some mild steel, and it worked wonders and was able to take tiny DOC while leaving a great finish compared to the regular insert I was roughing with. Definitely worth a try compared to scrapping parts.
 
It really depends on the depth of the bore, a rigid stub boring bar compared to a 6+ x D stickout bar will have different processes.

You maybe be better off running it like a manual lathe. Rough it to .03 per side out and take 3 .01" cuts checking in between. If you miss the mark that's on you at that point.

A sharp aluminum insert as mentioned above is another good option for finishing like a CCGT or DCGT.

It will take some serious SFM to get a nice finish out of 1018, I would probably start at 500 SFM and expect to go up. Your roughing will probably look great due to the high DoC.

Roughing 500 sfm, .015 fpr .1 DoC
Finishing 650 sfm, .005-8 fpr .01 DoC should be a decent starting point if your bore is at least Ø3/4"

Use coolant.
 
Typically when I'm trying to hit a bore dimension within a few tenths I will first bump the offset to make the bore .03" small then I measure and adjust the offset to make the bore correct, this makes the very light cuts unnecessary.

Sent from my A577VL using Tapatalk
 
These are basically a wheel. I can't do them on a manual because the OD is radiused with a small corner radius.
The bearing bore is just under .600" and just over .250" deep. I have lots of aluminum inserts for my boring bars so I'll give those a try. There's a small step for the bearing and so after I drill through I'll have about .025" per side to take off. What should I use for speeds and feeds with an aluminum insert?
 
That's a quick cut so no need to push it, if it were me 1200-1500rpm and 0.004"/rev and see what happens, finer feed if you want.
 
I wasn't suggesting to do them on manual equipment but to follow the same process you might follow on manual equipment for taking tool deflection into account.
 
Not certain how others can comment on a finish feedrate on a close tolerance hole. The closer the tolerance on anything, the better the surface finish is supposed to be. Your finish feed/per/rev will be based soley on your insert radius. I'd suggest 1/4-1/3 of your insert radius for your finish feedrate. Not familiar with the lathe you are using, but DOC is related to your setup/grip/and horsepower rating. If you are low quanity, and using a CNMG type insert, you can feed at 1/3 the radius as to break the chip properly. DOC I'd stay conservative at 2X the radius.
 
If you going to take shallow cuts trying to hit tenths it would be best to have a dead sharp tool without a corner radius, use the dead sharp tool to finish and a tool with a corner radius to rough. I have recently used Kennametal grade KCU10 on smaller 1018 parts with good results.
 
I've never used an insert without a corner radius. Can you get a good finish with a sharp corner tool? I always thought the radius was part of what gave a good finish.
 
I commonly adjust cuts by 0.01 mm, down to 0.001 mm, and it works fine.
All work is (tool) steel.
CCMT 21.51 inserts.

An external DTI proves the tool moves in x, by 1 micron, and the surface finish changes indicating material is removed.
The insert tips wear fast, so the finish soon turns fuzzy and not polished.
But the inserts are still fine for normal cuts.

I have a very very good, very rigid 12x lathe retrofit.

It might be the process is power scraping rather than cutting.
Don´t know.
But the workpieces become exactly the size I want, when measuring with external digital 1 micron micrometers.

I don´t care about using 1-2 tips on a sub 2$ insert, to finish a precision piece to a given size.
And the insert is still fine for deeper cuts.
 
Not certain how others can comment on a finish feedrate on a close tolerance hole......

Point taken. I was just trying to give him a starting point, he'd asked twice. For us manual guys this cut is too quick to even bother with autofeed, but it's still possible to get close enough and with a good enough finish to press a bearing into by look and feel. OP doesn't have that choice or the experience on the lathe.


I also agree with Circuit, the sharp aluminum inserts with a 1/64" radius will take a really light pass so I'm not sure I follow the recommendation to finish with a no-radius tool.
 
Got to remember on my boring bar I'm using an aluminum insert (only because that's all I have). It has an .016" radius and so I ended up using .004 on the feed and .020 on the DOC. I hate to change anything because it's coming out to size. I'm still waiting for a grooving tool to put the snap ring in. So I actually won't make these for a few days. I appreciate everyone giving somewhere to at least start.
 
I've never used an insert without a corner radius. Can you get a good finish with a sharp corner tool? I always thought the radius was part of what gave a good finish.

I do it all the time, grinding the radius off on a diamond wheel. The problem is tool life can be short as the corner can chip off so unless you are cutting plastic, brass or aluminum it is best to just use them as shallow finishing tools. What kind of tool geometries do you think were used before inserts? We aren't talking cave man days, inserts did not become popular and used wide spread until the 90's. Before that dead sharp brazed carbide tools were all the rage. The radius is actually a detriment to a good finish on a shallow cut and I believe the OP wanted to take a shallow finishing cut. If your DOC is less than the radius, you can have all kinds of problems.
 
The radius is actually a detriment to a good finish on a shallow cut and I believe the OP wanted to take a shallow finishing cut. If your DOC is less than the radius, you can have all kinds of problems.

I think you may be mixing two different things here. Every source I've ever seen says use a larger radius for better (theoretical) surface finishes at the same feed. A sharp tool will basically leave a very fine thread and require a super fine feed rate to achieve the same finish as a tool with a radius. The fragility of the tip is another issue. Before inserts when folks uses HSS you'd still grind or hone in an appropriate radius.

Larger radii do have more contact in the cut and are more likely to cause chatter. As you state if you don't take at least the radius DOC (some sources say at least 2/3) you can run into issues as radial force takes over axial, and a lot of inserts make this worse because they're not truly sharp (not WRT radius, but with respect to the land between the cutting edge and chipbreaker).

In the real world there's a balance between these two factors, but I maintain you need a little radius on that tool.
 
I think you may be mixing two different things here. Every source I've ever seen says use a larger radius for better (theoretical) surface finishes at the same feed. A sharp tool will basically leave a very fine thread and require a super fine feed rate to achieve the same finish as a tool with a radius. The fragility of the tip is another issue. Before inserts when folks uses HSS you'd still grind or hone in an appropriate radius.

Larger radii do have more contact in the cut and are more likely to cause chatter. As you state if you don't take at least the radius DOC (some sources say at least 2/3) you can run into issues as radial force takes over axial, and a lot of inserts make this worse because they're not truly sharp (not WRT radius, but with respect to the land between the cutting edge and chipbreaker).

In the real world there's a balance between these two factors, but I maintain you need a little radius on that tool.

I know what I have done with success and what has failed, I don't exist on theories. Let me guess, since you have been machining insert tooling was always readily available.
 
I know what I have done with success and what has failed, I don't exist on theories. Let me guess, since you have been machining insert tooling was always readily available.

I've only been machining a handful of years so yeah inserts have been around, kind of irrelevant. I know how to grind HSS, self taught from books and forums, never seen one recommendation for a no-radius tool. Inserts are hard to find like that too. Like you said, the tip wear is poor, but also, so is the surface finish. Don't mistake my use of the word theoretical, this is proven science, and I know you understand it because you're absolutely right about the DOC vs radius. I mean you nailed almost all of it, but a radius is not a detriment to surface finish:

Insert nose radius and depth of cut

I mean if we want to get really deep in theory we can talk about whether or not your sharp tool actually has a radius, albeit a very small one, maybe microscopic.
 
I've only been machining a handful of years so yeah inserts have been around, kind of irrelevant. I know how to grind HSS, self taught from books and forums, never seen one recommendation for a no-radius tool. Inserts are hard to find like that too. Like you said, the tip wear is poor, but also, so is the surface finish. Don't mistake my use of the word theoretical, this is proven science, and I know you understand it because you're absolutely right about the DOC vs radius. I mean you nailed almost all of it, but a radius is not a detriment to surface finish:

Insert nose radius and depth of cut

I mean if we want to get really deep in theory we can talk about whether or not your sharp tool actually has a radius, albeit a very small one, maybe microscopic.

I was talking about grinding carbide, not HSS, no one back in the day used HSS tools for production runs of any quantity except for drilling. A radius is a detriment if it is too big for the application.
 








 
Back
Top