# Great Saunders Youtube on aluminum feeds and speeds ref. lathe inserts



## Alan H. (May 31, 2017)

John Saunders put out a new Youtube today on feeds and speeds for turning aluminum with inserts.  It is 40+ minutes long but worth the watch.


----------



## wildo (May 31, 2017)

I watched it and, once again, I'm thinking that as a hobbiest with a small lathe- I really have no business using carbide. I'm trying to make small spinning tops- about 1" in diameter. To be at a SFM of 785 like in the video, I need to be spinning at 2998rpm. No wonder I keep burning up my inserts (spinning closer to 650rpm for aluminum and 400 for titanium). So I went out to ebay looking for some REX 95 or REX aaa tooling- and it's just as expensive as inserts. Why do I always pick such expensive hobbies!?


----------



## mikey (Jun 1, 2017)

Will, I see no reason not to use carbide for aluminum if you use inserts intended for aluminum. Granted, you won't be able to run it at the recommended speeds and you are limited in the depth of cut you can take but I assure you that a CCGT-AK insert will do a decent job on aluminum, even on a small lathe. Each insert has a minimum depth of cut to make the chipbreaker work as intended and on a positive rake insert like an AK, that is about 0.020" deep. Your lathe can easily handle that. If you use a CCGT 25.51 AK insert that has a 0.016" nose radius, just add at least 0.005" to that and you will reduce tangential forces enough to avoid chatter. For finishing, a 0.005 - 0.008" deep cut will be fine. This insert will cut consistently provided your feed is consistent.

The insert in the video is an AK insert. Contrary to what the guy in the video said, an AK insert is not coated but it is ground and polished and is very sharp. If you own an SCLCR tool holder and have CCGT AK inserts, go for it and it will be fine. You may have long stringers if you take shallower cuts so if roughing, increase your feed rate to reduce this. If you're really roughing, increase depth of cut to do the same thing. Or live with stringers, especially if you're working with 6061 or 7075.  I'm not just saying this. I own an SCLCR tool with AK inserts and I know what they can do. They're good tools; just not as good as a good HSS in my hands. If you use these inserts, use coolant to reduce a built up edge. 

With that said, a HSS tool ground for aluminum will outperform the insert on a small lathe and probably on a big lathe, too.  If you use adequate side and back rake the tool will rough and finish really well, even with small depths of cut at lower speeds. Plain old cheap M2 HSS is fine for aluminum. You don't need Rex AAA (8% cobalt).

Rigidity and power make a big difference when taking big cuts and that's important in a job shop like on the video. On a small lathe in a hobby shop, a properly ground HSS tool will allow the lathe to make cuts that are much heavier than you would think, at speeds and feeds that are achievable even when feeding manually. The biggest cut I've taken in 6061 with a HSS tool on my little Sherline was 0.125" (0.250" off the diameter) and it cut it with no problem. Your SB will do much better with the right tool. On my Emco lathe, the same tool I use on my Sherline will easily take a 0.25" deep cut in aluminum without breathing hard and will leave a mirror finish to boot.

I guess I'm saying to use what you have and when you can, learn to grind a HSS tool for aluminum. You'll be glad you did.


----------



## Alan H. (Jun 1, 2017)

Mike, thanks for the feedback and comments to encourage folks a bit.  I do not think it was John's intent at all to discourage any of us and your comments and clarification help him avoid that.

For those that may not have seen it, late last year Mike posted a fine guide here on "_how to grind a HSS Turning Tool_".


----------



## wildo (Jun 1, 2017)

Yes, indeed- thanks Mike for the explanation. I suppose the biggest thing that stood out to me is the "designed" minimum depth of cut. It really stood out to me and made me realize I have SO much left to learn (as if I didn't already know that). But for me, I am regularly trying to sneak up on a size- taking .001" or sometimes .000x" depths of cut. The insert tools are so frustrating to me because, I assume, the tool pressure isn't right. It's like they'll just rub the surface and not cut anything. I advance the cross slide and still nothing happens. I advance some more and then- bam, I've taken a .005 cut. For this small work that I'm trying to do (and especially because I have considerable wear in my lathe) I think that a properly ground HSS bit is exactly what I'm looking for.

Now the reason I was looking for REX stuff is because I do a fair amount of cast iron stuff in my tops. I've heard that REX tooling is superior when cutting stuff like stainless or cast iron. Now, it's unclear to me if I need REX aaa or REX 95, but my take on it is that the 95 version is the harder of the two, and therefore perhaps the better option.

[EDIT]- I would add that my Tormach Super Fly with the SEHT1204AFFN-X83 inserts do an exceptional job on my mill. So yes, I agree that inserts absolutely can work! I just found it interesting when they started talking nose radius and minimum depths of cut.


----------



## mikey (Jun 1, 2017)

Alan H said:


> Mike, thanks for the feedback and comments to encourage folks a bit.  I do not think it was John's intent at all to discourage any of us and your comments and clarification help him avoid that.
> 
> For those that may not have seen it, late last year Mike posted a fine guide here on "_how to grind a HSS Turning Tool_".



I agree that the point of the video seemed to be to make folks aware that the geometry and nose radius of the insert is important, and that the user has to know how to use it to best advantage. I liked the video and I really like that Saunders guy. His enthusiasm reminds me of our own Justin, the student machinist who recently made a thread jack. Both exude excitement with learning and machining - very nice to see.

I'm waiting to see your HSS tools, Alan!


----------



## mikey (Jun 1, 2017)

wildo said:


> Yes, indeed- thanks Mike for the explanation. I suppose the biggest thing that stood out to me is the "designed" minimum depth of cut. It really stood out to me and made me realize I have SO much left to learn (as if I didn't already know that). But for me, I am regularly trying to sneak up on a size- taking .001" or sometimes .000x" depths of cut. The insert tools are so frustrating to me because, I assume, the tool pressure isn't right. It's like they'll just rub the surface and not cut anything. I advance the cross slide and still nothing happens. I advance some more and then- bam, I've taken a .005 cut. For this small work that I'm trying to do (and especially because I have considerable wear in my lathe) I think that a properly ground HSS bit is exactly what I'm looking for.
> 
> Now the reason I was looking for REX stuff is because I do a fair amount of cast iron stuff in my tops. I've heard that REX tooling is superior when cutting stuff like stainless or cast iron. Now, it's unclear to me if I need REX aaa or REX 95, but my take on it is that the 95 version is the harder of the two, and therefore perhaps the better option.
> 
> [EDIT]- I would add that my Tormach Super Fly with the SEHT1204AFFN-X83 inserts do an exceptional job on my mill. So yes, I agree that inserts absolutely can work! I just found it interesting when they started talking nose radius and minimum depths of cut.



The key reason you're having trouble with light cuts is because an inserted tool does not like to take light cuts. The reason for that is because radial cutting forces are very high with light cuts and the tip is being pushed out of the cut. At minimum, the lightest finishing cut an insert can take is about 1/3 - 1/2 the nose radius of the cutter, while roughing cuts need to be at least 0.005 - 0.010" larger than the nose radius at minimum if you want to avoid chatter. So, you need the right nose radius on the insert. Complicating this is the fact that in order for the chip breaker to work as intended, you need to take a deep enough cut. This is typically around 0.020" deep or more for it to work as intended for most inserts.

You need to know how your tool/insert like to cut in the material you're working with. For example, a SCLCR tool with a CCGT 25.51 AK insert (this has a nose radius of 0.016") in 6061 has a minimum roughing depth of cut of about 0.02 - 0.03", and a minimum finishing depth of cut of about 0.005 - 0.008". If you try to finish with a shallower depth of cut, the insert won't cut properly. If you can find a depth of cut that works well, that insert will consistently cut that depth pass after pass after pass. Knowing what your finishing depth of cut must be, you can rough until you get to, say, 0.016" from final diameter and dial in the finish pass. You will need to slow your feed rate to about 1/2 the nose radius in inches per minute but it will take that cut with a decent finish.

This is not as complicated as it sounds. Once you figure out how your roughing and finishing pass requirements, you just dial it in and make your cuts. The insert will cut consistently if all your cutting conditions are dialed in.

On the other hand, HSS is much less fussy but your tool geometry makes a big difference. I won't go into that here but in my experience, you will have far fewer issues with HSS.

I was wrong. Rex AAA is also 5% cobalt, not 8%. I think you're on the right track going with cobalt for cast iron. It is a superior cutting tool. I prefer Cleveland Mo-Max cobalt (5%) and Super-Mo-Max (8%) for this. I normally turn cast iron with a brazed carbide tool, actually, and finish with a cobalt tool. If turning a rough piece, use an old HSS tool to break through the cast surface, then switch to a very sharp brazed carbide tool with a small nose radius on it to continue roughing it in. Then change to a sharp HSS to finish it. Keep your speeds low - back gear if you have it - and it will go well.


----------



## sanddan (Jun 2, 2017)

I think Mike might have mentioned it but when using inserts you need to take a bigger cut. I had the same issues you are having when I first got started (I'm still a beginner) and found that you can "hit the number" by measuring when you are close and then "going for it" on the last finish cut. After awhile you will find that you can get very close even when taking .015" to .020" final cuts.


----------



## Alan H. (Jun 2, 2017)

@mikey, you referred to the insert in the video as being an "AK".   Is that a manufacturer specific code or is it a standard?


----------



## Doubleeboy (Jun 2, 2017)

For decades I have been using TPG inserts when I want to take light cuts,especially finishing cuts.   I can consistently take cuts of 1 or 2 thou in aluminum with a fresh  321 or 320.5 TPG uncoated.  Old school insert, has its issues with chip breaking but is dirt cheap and works well at low speeds, low feeds and light cuts.   Granted I have two pretty stout lathes that can run more modern inserts with big feeds and depths of cut but if I want to sneak up on a final dimension and hit a tolerance of a few tenths, I frequently use TPG for last 2 cuts.  For the frugal, they are a bargain and very easy to touch up with diamond hone.


----------



## mikey (Jun 2, 2017)

Alan H said:


> @mikey, you referred to the insert in the video as being an "AK".   Is that a manufacturer specific code or is it a standard?



As far as I know, AK is a style of insert with a very positive rake and a parallel pattern chip breaker. Most have a radius just before the insert screw hole to direct chips upward, presumably to curl and break the chip. All AK inserts are for non-ferrous turning, are polished and ground and the ones I am familiar with are uncoated. They come in different grades but H-01 is the one I use. The grade designation varies with the maker but the AK style is pretty standard.


----------



## mikey (Jun 3, 2017)

Alan, I should clarify that there are all sorts of AK insert. There are diamond AK's in 80 degree and 55 degree, round and maybe even other shapes. The CCGT that I and many others use, including the one in the video, looks like this:




You can see that it has only two usable points when using the SCLCR tool holder and the entire upper edge of this thing is sharp enough to slice flesh. You cannot see it but it has a very positive rake and a raised ring near the hole - this gets the chips moving in a hurry, carrying heat out of the cut with the chips - but you have to get past the nose radius before cutting takes place. Given that the nose radius of an insert has a significant impact on all your cutting conditions, choose wisely.


----------



## jbolt (Jun 11, 2017)

sanddan said:


> I think Mike might have mentioned it but when using inserts you need to take a bigger cut. I had the same issues you are having when I first got started (I'm still a beginner) and found that you can "hit the number" by measuring when you are close and then "going for it" on the last finish cut. After awhile you will find that you can get very close even when taking .015" to .020" final cuts.



Just to expand on this a bit. 

When I am turning to a precise dimension all I am really concerned about is the final finish pass. I find the RPM,  depth of cut and feed rate that achieves the desired finish and then set my tool zero to that. 

Lets say 700 RPM, .015" DOC and .005" feed rate, for the tool used, gets me the results I'm looking for. I will take a couple of finish passes at this setting and measure. If I'm hitting the number I'm expecting. based on my zero. then I'm confident that when I take that cut as my finish pass I will hit my number. If I am removing a lot of material I may wait until I am close to the finished diameter before fine tuning my tool zero but I always fine tune with the cutting parameters that get me the finish I need.

For roughing, depending on the tool geometry, DOC and feed rate, the roughing cut may be slightly larger or smaller than the input value due to spring, rigidity, lash, tool grab etc. As long as I know how the tool will behave at the finishing cut, I can rough to within a few thou of the finish cut depth and then take my finish cut without having to sneak up on it.


----------



## Alan H. (Jun 16, 2017)

mikey said:


> . . . . . . . .
> 
> I'm waiting to see your HSS tools, Alan!


Okay Mike, finally got 'round to it.  So here's one with geometry that you may recognize.   I ground this bad boy to see if it will peel .002" off some aluminum.   It is a 1/2" Rex 95 bit in a BXA holder.  If it works well I will grind a left handed one to match.


----------



## mikey (Jun 16, 2017)

Nice! Bet that tool will cut aluminum nicely - let us know how it works. For someone who is new to tool grinding, that is a great job, Alan!!


----------

