[flyingmike]

I have a small cnc lathe (denford starturn 4) in my home workshop and have converted it to run on mach3 and so far quite happy with the accuracy the machine offers on small aero modelling parts.

However, when facing off I have noticed very subtle equally spaced rings in the surface when facing off mild steel (1000rpm and 10mm/min feed) using a HSS tool. They tend to be more visible when the surface is polished with a bit of wet and dry.

Originally I thought it was the tool not allowing good chip removal but I have more recently come to the conclusion that the preloaded ball nut (which does provide some resistance) is causing the top slide to 'rock' causing this pattern in the surface (that appears to roughly match the pitch of the screw). Is this something that anyone has come across before?
There is very little play in the mechanics and a rub with some Emory cloth removes the pattern but I was intrigued to here if anyone has come across this problem before...

I plan to use a clock gauge and try and see any 'rocking' when travelling along the X axis....

[fizzissist]

You're beating a dead horse.

Leave .01-.03" length on the back end, flip the part and face off the back.

A cutoff blade isn't going to give you jewelry quality on the back end when the part isn't supported. Unless you've got a sub-spindle and the tool is ground accordingly.

There's a myriad of reasons for your rings... chips building up and exerting forces on the part, coolant intermittently hitting the part as chips get in the way or hit the cutting zone, vibrations in the system, you're on your period, .... etc...

CNC or manual, the butt end won't be pretty. Lord knows I've spent enough hours trying.

[flyingmike]

Hi, Thanks for the reply!

I think I confused matters a little....I`m not parting off the workpiece I`m just facing the surface of some 30mm diameter bar. Taking cuts of about 0.05mm

[Geof]

..... very subtle equally spaced rings in the surface when facing off mild steel (1000rpm and 10mm/min feed) using a HSS tool.....

The rings could be caused by the cross slide wobbling but a more likely cause is a small build up of material on the tip of the tool which periodically breaks off. HSS is very prone to do on mild steel this especially with a light cut at a low feed rate. The steel adheres to the HSS and builds forward actually extending the tip of the tool until it has built out so far it breaks off and then repeats the process. It can be quite regular particularly if the feed is constant. And of course the size of the build up is measured in small fractions of a thousandth of an inch so it creates a visible ring that is really very very shallow and easily polished away.

To check for actual wobble in the cross slide face off a piece of brass. If you get rings with the same spacing as on the steel it is probably wobble.

[fizzissist]

As Geoff points out, there could be "wobble" on your cross slide,,,, correctable to some extent by cleaning, properly lubing, and adjust the gib.

There's also some tendency of the cutoff blade to jump side to side as it's cutting, which can be minimized by a shallow angle on the tip (for mild steel vs. HSS blades I usually use about a 10-15deg tip angle, 10deg relief), on center to .001 above, hollow ground blade, and DEAD SQUARE to the spindle. The blade also needs to be chucked up in the holder absolutely back into the holder as far as you can get it with just enough clearance so the holder doesn't hit the bar as the part drops off.

If your blade is vibrating at the tip too much during cutoff, then go to the next wider size. Use a good quality blade too. I have a stash of old Empire P-1N, P2, and P3 blades that are golden. I've found the cheap ones are different, and I have more problems with them.

You may find that for your machine, running slower, with a heavier feed may help. There's no substitute for experimenting with a manual lathe to get the feel for what's best if you can. Nice thing about CNC is the ability to program constant surface speed, retract, and a change up for just before the part drops.
Still, don't be disappointed at lousy finishes on the back end. It's life. I've cut a lot of 1018, B1113, and C12L14 on screw machines up to 1.5"dia w/ HSS, and saving a back-facing operation was very cost efficient... Sometimes you just can't avoid it.

[neilw20]

As was noted, it is not using a cutoff blade but a facing operation.
If tool is picking up material then that will do it. A more aggressive final cut often is better.
Measure twice, cut once.
How far apart are the concentric circles? Always the same place?
Could it be that you are seeing the variability of steps in the stepper motor? Is it direct drive? Belts are springy things.
Does using cutting oil - the stuff for doing threading... If this helps it is pickup on the tool.
Examine the tool with a powerful magnifying glass. Any flats rubbed on the front face will not help.
If the top of thee tool is highly polished it will help stopping sticking.
Is the tool height correct?

Is it crappy material?
Hmmm. lots of things to consider...

[flyingmike]

I put in a little more time on the lathe tonight. I figured I would check my mechanics better before going any further. putting a dial gauge on the tool holder I was getting movement when I rocked the cross slide. I estimated about +/- 15microns on the gauge. So I took the slide off and cleaned it up and rebuilt it all and tightened the gib up so it was quite tight. Tighter than I would do a manual lathe but still able to move. I couldn’t read any movement on the dial gauge so I tried another cut.

The photos show a much better cut and when polished a little I just got normal scratches that I would expect rather than the thick bands I was getting before.

You can see the tool I have been trying. My aim was to make a tool for both turning and facing. Its getting a little thin now following a lot of trial and error grinding but seems to cut well so I`ll make a new one. I havnt really got a good cutter for facing off so its back on the grinder. learning lots!

[flyingmike]

The drive is a toothed belt to the ballscrew and the pitch of the ballscrew is 2.5mm. I`m microstepping so I dont think I would see the steps in the surface finish. I just squirt on the coolant with a bottle so no flooding.

[Shane1234]

have you tried using a g96 instead of g97 on your mach3 machine? f.001 or .0015 on a .005" pass would be nice..... g96 s400 or s450.....

[neilw20]

That's if it has variable speed.

[Shane1234]

That's if it has variable speed.

ah yes, my bad. i forgot that it is a converted manual lathe so most likely he doesnt have that function as the gearing is lever driven, not cnc control driven.

[flyingmike]

Hi, The starturn is a CNC lathe from the 1980`s just converted to run on modern electronics. There is a belt drive from the motor to the spindle with no additional gearing. During the conversion I never added any spindle control for constant surface speed but I could do it in the future if neccessary. I have got an optical sensor on the spindle as I use the maching for thread cutting.

[fizzissist]

That tool in the pic is serious old-school. Serious positive rake, which you don't need... what's the face and side relief, and back relief?
(so we're on the same page on geometry nomenclature, I'll use the terms of this link)
http://upload.wikimedia.org/wikipedi...t_Geometry.JPG

For HSS you can use 0deg Back Rake Angle & Side Rake Angle and do just fine on mild steel, aluminum, and brass.

For Front Clearance Angle I've used 10-12deg for years with no problems. Side Clearance Angle 3-5deg, same for End Cutting Edge Angle. For Side Cutting Edge Angle, I leave the angle alone and just kick the tool over a few degrees to give a few degrees of clearance for facing.
If you're going to use the tool for both turning (to shoulders & straight facing), just increase the End Cutting Edge Angle so you still have clearance with the tool kicked over in the holder.

Grind a nice .03 rad on the nose then stone it for a uniform radius... (do it accurately and it'll program nicely into your tool nose radius compensation)

Setting the angles as I've described will allow easy honing of the cutting edges with a hand stone ( I use an India... 'cause I've had it for years and it works), and results in perfectly acceptable surface finishes. Leaving the Back Rake Angle at 0deg also allows for easy regrinding... flop the tool on the surface grinder, a few quick passes, and you're ready to go. Just readjust the height in your toolholder. Voila!!

(Screw machine guys know this approach.... it leaves form tool geometry on square tools essentially intact!)

You're on the right track, just save yourself some time, and go easy on the angles. Ya don't need radical except on special jobs... and plastics.