irregular cut when turning

This forum is dedicated to those hobbyists with the 3-in-1 metalworking machines. Mill-Drill-Lathes. Tips, techniques, modification and use of these machines is topical.

Moderator: Harold_V

driveslayer
Posts: 8
Joined: Mon Jan 29, 2007 8:50 pm
Location: Florida, USA

irregular cut when turning

Post by driveslayer »

Hello, I have a WT 3014-0015 - model hq800. It appears to be the same as the HF 44142 and the Grizzly model. The problem i have is when i am turning it is never smooth. I use either brazed carbide bits, indexable tool holders with replaceable tool inserts. I guess the point i am making is i am not relying on my tool sharpening skills in most cases. in the length of a cut, size doesn't seem to matter, it appears i get ridges in the cut. if i had to guess it is almost like the tool holder is moving away from the work. i have tightened or adjusted the gibs to a snug fit with no apparent change in symptom. They are not so bad i cannot take them out with some medium emry cloth, but if i can figure out how to stop this, or at least reduce it that would be great.
Thanks for any feedback you can give.
Mac
Posts: 9
Joined: Sun Jan 28, 2007 11:55 am
Location: Carrollton, Georgia

Post by Mac »

Make sure the leadscrew does not have a bow in it.
driveslayer
Posts: 8
Joined: Mon Jan 29, 2007 8:50 pm
Location: Florida, USA

Post by driveslayer »

Hadn't considered a bow in the LS ... it will be a few days before i get back to it but i will check that first.

Thanks
User avatar
Harold_V
Posts: 20231
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Post by Harold_V »

You didn't mention the material you're machining, nor have you stated the amount of experience you have.

If you're machining mild steel (low carbon), you should expect the surface to be ragged----it doesn't cut well, not unless you run it very fast (using carbide, not HSS) with the proper depth of cut. Light cuts will tear, and there's little you can do about it. Its the nature of the material.

I may be wrong, but I think you're kidding yourself by using carbide. The machine you have is borderline able to warrant its use----regardless of being brazed or insert type-----but if you're using negative rake, it most likely isn't capable. I strongly encourage you to not use carbide to avoid the learning curve of grinding HSS toolbits. Do yourself a favor and get familiar with tool configurations and grinding. It's a skill you'll use to great advantage.

Harold
driveslayer
Posts: 8
Joined: Mon Jan 29, 2007 8:50 pm
Location: Florida, USA

Post by driveslayer »

Thanks for the input.

I do consider myself a begginer. i have tinkered for a few years on this machine off and on as i feel like 'playing'. Never had any official training so it is learn as i go.

I mostly cut 304 stainless . usually 900rpm -
occasionally aluminum - not sure what type - just whatever i can find.

I have ground many a hss tool, not gonna claim always right, but i will claim not always wrong =). But when trying to determine the cut issue i figured best not to leave anything to chance.
The irregular cut bothers me because it is not a constistent roughness or smoothness on the same pass - just spots seem rougher than others.
User avatar
Harold_V
Posts: 20231
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Post by Harold_V »

304 is one of the materials that will cut cleanly. It's tough, but not hard, so it responds fairly well to positive rake, but with light feed. I've yet to find a tool that will stand up to heavy feed in 304. Edge life is generally short, with inserts broken when not changed in a timely fashion.

If you're using carbide, and it's not a C2, that could very well be part of your trouble. A C5 grade will not usually hold up well at all when machining series 300 stainless, nor is it the recommended grade. If you intend to stick with carbide, make sure you explore the C2 grade if you haven't already.

The 900 rpm doesn't mean much without a diameter attached. It might be too slow for ¼", but woefully too fast for 1" diameter, depending on your choice of tools.

A sure sign of tip failure when machining 304 is the generation of roughness, often accompanied by tiny spines that protrude from the machined surface. If you're having any of these symptoms, your tool geometry may be off, and you may be running too fast, destroying the fine edge prematurely. You haven't provided enough information to form a solid opinion.

If you aren't faced with a real need for 304, you might consider changing to 303 S or Se. The difference in machining is staggering. It doesn't cut with as bright a surface, but it otherwise machines beautifully. It tends to cut with a slightly frosty surface, but smooth, and tools last much longer. Chemically, it's almost identical to 304, but slightly less corrosion resistant, a result of the sulfur or selenium added for free machining.

Harold
driveslayer
Posts: 8
Joined: Mon Jan 29, 2007 8:50 pm
Location: Florida, USA

Post by driveslayer »

That is good information, i do see most of those symptoms. Truth be told i am not sure what information is needed and what is not to provide a good base to form an opinion. I do believe i am using mostly the c5 carbide. The diameters vary from .5" - 2" - i try not to cut too deep with each pass. how deep of cut should i be turning?
304 just seems more readly available. I make parts for my motorcycles with the stainless ... handle bar risers, highway peg mounts, other misc spacers and such . i think my largest part was a new lightbar to support the turning signals and passing lamps.
User avatar
Harold_V
Posts: 20231
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Post by Harold_V »

driveslayer wrote:I do believe i am using mostly the c5 carbide.
That be the case, you should be able to see the problem when you inspect the tool. It will be rounded, or otherwise eroded at the point of contact. Looking at the front relief area, you often see a shiny band that runs vertically along the cutting edge, where the tool has failed and is making contact in an area wider than the intended edge. C5 is not suited to that kind of material ----but, being steel based, it's a common mistake folks make. The carbide of choice for stainless and cast iron is always C2----which has superior edge wearing characteristics, although more brittle. The difference in tool life as compared to C5 is staggering under normal conditions.
The diameters vary from .5" - 2" - i try not to cut too deep with each pass. how deep of cut should i be turning?
That's a tough one to answer, dependant on so many variables that only experience will help you know the answer. The power and rigidity available at your spindle will be a factor, as well as the tool configuration. The chief thing to remember is that 304 stainless isn't fond of heavy feeds, nor negative rake. You can take a generous depth of cut (.05"/.150") with light feed (.002"/.004") with positive rake and move a fair amount of metal, assuming you have the speed right and you can keep the tool cool and lubricated. That is best accomplished with HSS and a proper chip breaker. It could prove challenging without coolant. The best thing I can offer is for you to record what you do each time you machine the material, and make changes towards those I've recommended. What ever you discover works for you is good, even if it goes against everything I've said. You may find the only way you'll move past where you are is to experiment. What works for one guy doesn't necessarily work for another.

Do slow down your spindle speed. I'd suggest that you should be running no faster than 75 sfpm using hss, or slightly faster if you use C2 carbide. With carbide, watch the chip as it comes off the tool. If you see any signs of sparks, or the chip comes off a purple color, you're running way too fast. The chip shouldn't shift color by much. At worst, a slight yellowing of the chip. If it does, you're running too fast and can expect premature edge failure. If the surface cuts without being shiny, the tool is buggered. That happens very fast when using the wrong grade of carbide, especially when running too fast.
304 just seems more readly available. I make parts for my motorcycles with the stainless ... handle bar risers, highway peg mounts, other misc spacers and such . i think my largest part was a new lightbar to support the turning signals and passing lamps.
Nothing wrong with your choice, aside from its machinability. It's not fun to machine, but it's far better for corrosion resistance.

If you find you get some minor rusting of the things you make (very common), they should be passivated. That removes all the free iron from the surface and prevents the hint of rust you often see on stainless.

Harold
Jose Rivera
Posts: 3803
Joined: Wed Feb 21, 2007 9:21 pm
Location: Vallejo California

Re: irregular cut when turning

Post by Jose Rivera »

Humm, this one I would almost have to see the finish to comment.
Finish is controlled by several issues.
One is the speed of the spindle, the faster the speed assuming you don't burn your tool the shinier the finish.
If the tool has a sharp point can cause a bad finish, tools must have some sort of radii or at the least a small flat at the nose.
Incorrect rake angles (clearance) also can contribute to a crappy finish.
Some materials, specially aluminum can by gummy and almost impossible to get a good clean cut.
Feed rate or a dull tool. I can mention lots more, that why I said that I would have to see what you're doing to give a better suggestion.

I have a Grizzly G4000 that consider to be the worst quality built lathe that I've have ever put my hands on.
I just bought a Maximat V10 Mentor and there is no fair comparison. In a scale of 10, the G4000 I'll give about a .5 (point five) next to this Austrian made machine.

One thing that I experience with the G4000 regarding finish is that I could never get a clean finish because no matter what I did, there where always a light spiral created along the cut.
This happens when the spindle bearing rest areas are out of concentricity and this causes the spindle to wobble.
Even an error as small as .0001" can cause this.

In my opinion, is so sad that there are no new European or American made lathes for the home machinist (affordable) that I know of.
Though there may be some Chinese made lathes of better quality, I consider Grizzly to fit exactly YOU GET WHAT PAY FOR, even less !
User avatar
Harold_V
Posts: 20231
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: irregular cut when turning

Post by Harold_V »

Jose Rivera wrote: Incorrect rake angles (clearance) also can contribute to a crappy finish.
Rake angles are not clearance. Rake is the angle at which the top of a cutting tool addresses the cut. Clearance (relief) is the angle that allows for the balance of the tool to not make contact with the cut. The names (and features) are not interchangeable, and are each equally important for a cutting tool to function as intended.

Harold
Jose Rivera
Posts: 3803
Joined: Wed Feb 21, 2007 9:21 pm
Location: Vallejo California

Re: irregular cut when turning

Post by Jose Rivera »

I stand corrected !
driveslayer
Posts: 8
Joined: Mon Jan 29, 2007 8:50 pm
Location: Florida, USA

Post by driveslayer »

Thanks for all the great replies.

Since my last post i have been reading and cutting ... i have moved to using HHS bits that i am grinding myself and what i have found is 1) i need to get a better stone on my grinder .. ordering one from WT tomorrow =), 2) if i grind my tool on my bench grinder then follow-up the grind on a disc sander, 5" disc 120grit (it is a little 1" belt and 5" disc craftsman), to round the point i am getting a pretty good cut, in fact much better than any carbide i have ever used. What i cannot do it make an effective chip breaker in the tool and i always end up with long strands of Stainless razor wire. I have read Harlolds Post on grinding HSS tools - thanks H., but i can't see any of the pictures .. maybe they've been pulled off after all this time... Anyway things are getting much better now...
Post Reply