CNC Woes

[PatMarlin]

The past two (2) weeks I've had problems with the parting cut off tooling on my CNC that has been giving me fits and holding things up.

I would get so many cycles and parts ran, then the cutting insert would just break instead of getting dull, and send my tool holder into the work and destroy it if I was not there to catch it. I'm using ISCAR parting tool that uses the carbide insert that grips and seats in the tool by pressure. Not cheap. So far I've been able to re-file the seat on two of them, but one's totally *****.

Finally, I found a one digit error- one number off I programmed buried in the code that was pushing on the side if the insert bit .006 for a brief second during the program run. This would weaken the bit just enough and over time cause me hours of grief... :groner:

Well now I've been humming along and running the machines 14-16 hours each day to catch up. I like the tool as I can hone the bit with an EZE-lap diamond flat every so often and tune it right up.

Any of you experienced CNC guys still go through this kind of stuff, or is it me?

[dragonrider]

I don't have a cnc but I do have the type of parting tool you discribe and I won't use any other type. I use the 1/8" wide inserts and one day will get a thinner one cause sometimes it is what's needed. Glad you found the problem.

[scb]

Any of you experienced CNC guys still go through this kind of stuff, or is it me?

NO I've never:
put the decimal point in the wrong place.
forgotten the decimal point.
transposed a number.
forgotten the minus sign.
put the right tool offset in the wrong place.
put the wrong tool offset in the right place
called up the wrong work offset.
forgotten the r (or i&j) when calling a g2 or 3
or
forgotten to cancel a canned cycle .
Nope, never happens.:oops: (thankfully after 8 years it doesn't happen very often)

[jhrosier]

I've been an NC programmer for twenty or more years.
I describe programming as "running an NC from a safe distance."

Stuff happens, not often, but it does sometimes happen.

A thousand line NC program is a work of art when it works as intended, and a nightmare when it doesn't.

Jack

[PatMarlin]

Thanks fellas. Now I feel better. After all that was the whole point of the thread... :mrgreen:


Paul-

ISCAR I'm running now has a .118 bit, and your definitely notice more pressure when using it. The one I was using before was .094 which cut real nice, but they are not as strong when you get thinner of course. I do a tiny bit of turning and profiling with it so I need the strength.

[theperfessor]

I still make stupid mistakes, and my students still find all kinds of ways to generate "nonstandard" G & M codes.

On the Haas mill we run simulations on the actual machine first, then we run it without tools in place, then using glued up blocks of HDF with tools in place, then with the actual part. And you still can't catch all the errors the first or even third time. And the parts that we make production runs of, such as tensile test specimens, we're still tweaking the code to cut machine time to a minimum with reasonable tool life.

It's the price you pay for all the advantages of CNC.

[PatMarlin]

I did about 3 horrible crashes at first. I was thinking about making wood fake tooling at one time, then I just tested a move at a time, with the machine moving real slow. This last one was a 6 on the end of 3 digits that was a plaiin typo, and when I finally found it, I thought what in the heck is that doing there? Then I realized what had been happening.

The last crash I had wasn't my falt. 2 bits and a boring tool snapped right off. I couldn't believe it and had no idea how it could have happened with my programing, THEN I realized my X axis was not working. Belt slipped off the servo motor.

Lube was working it's way from the coolant down inside. I replaced the belt and broke an aluminum splash shield to protect the area and stopped that.

[PatMarlin]

And the parts that we make production runs of, such as tensile test specimens, we're still tweaking the code to cut machine time to a minimum with reasonable tool life.



I work on fine tunning that as I go along. People don't realize how time consuming and much work that is. Then you have numerous choices in tools and bits. I'm getting better and better at it every day.

I've got one other limitation that's a challenge and that's only 4.5" of X travel. I've had to use my turret in a fixed position as these year Hardinges where notorious for indexing problems. So I have to figure out how to do things with that much travel and it ain't easy.

Here's a pic of my die housing setup. I've built tool blocks around an Omni-Turn 8 oposition tool block and tied it all into the Hardinge turret plate. Starting from the back is the ISCAR cut off block, then drill, threading tool, and the last bar to face, and turn. I have to do the final bore ID in another operation, as there's not enough X.

I had to mill the shank on the last bar at an offset to give me .120 more reach otherwise there wasn't enough travel to use it. It worked. I need an Omni-turn Accuslide for this machine and that would give 8" in X axis. That would be heaven.

http://www.patmarlins.com/Diehousings.jpg


Another limting factor of the X is I can't get the cut off over back out of the way far as I want so I wind up having to pull the stock out farther, and that creates some finish issues on some parts to deal with.

[JIMinPHX]

Anyone who hasn't crashed a carbide part off tool in an NC machine, hasn't run one very much. Those things are real fussy about how they get applied. They don't like side loads at all. The ones from Manchester seem to have a little more tolerance for it, but not much. I only use them when I really have to.

Now I know that there are going to be some people on the board that are going to want to flame me for what I'm about to say, but I actually prefer to use HSS part off tools for most applications in common materials up to & including medium carbon alloys. They aren't as prone to chip or shatter. They tolerate side loads better. And they are a whole lot cheaper to run.

Sure you need to sharpen them up a little more often, & then you need to re-qualify your tool tip position, but that seems like a small price to pay for what you get. I even find that I can get away with sticking them out further than the books tell you to with good results as long as I have a good rigid holder.

The standard style Aloris holders don't count as rigid in my book. The pictures below show what I'm using these days. The reason that it doesn't have a height adjustment screw on it is because I cut the body of the holder so that it sits at the perfect center height when it bottoms out on the tool post.

[PatMarlin]

Well- that's interesting that you say that Jim because I have found HSS to cut off better as well.

I've got an HSS blade mounted on my manual Hardinge Chucker- at 90 dgrs, and it cuts through cold roll like butter. I've only used it on up to 1/2" diameter as yet. I've tried it on the CNC and it parts well, but will not turn well, but that is mainly due to it being a bout' .080 wide and it's sitting in one of those adapter 1/2" block mounts, then in the Hardinge (1/2") tool block.

The ISCAR I'm using has an 8drg tip radius, and a 4 dgr lead angle which does the little turning I need to do. What I was going to do next- right before I found my program error is grind my own part off tool out of 1/2" HSS, with the nose radius and lead angle. In fact I still should. Heck- I have to hone the ISCAR bit every 10 or so cycles, and set my tool offset .001 closer every so often anyway on cutting 7/8" cold roll. No big deal.

Wish you could use an aloris tool post on a chucker sometimes, but no luck there.

And one thing my old 1955 Hardinge HC chucker- I picked up for $500, cleaned and did a motor swap on it in 3 days, puts a mirror finish on parts with my hand ground HSS bits. I can take sizable feeds as well. It has that old motor clutch auto feed and it just works beautifully.

[JIMinPHX]

Hand ground multi-purpose tools for combination shallow part-off/turning applications can be really handy on small diameter work. You've got a good idea there. I would stick with it. On a tool like that, I would grind it like a narrow AL style tool & turn from the headstock out with it. Leaving your clearances in that direction will allow you to part off with a clean face on the back of the part.

I don't know which Iscar holder you have, but the way that most of them are set up, the holder is not designed to give the chip any side support. That little V under the chip on most of them doesn't hold worth Jack & the dainty little top clamp (if you can even call it that) only holds if the stresses on it come from the intended direction. It's not just that tiny little chip that isn't up to the task of making a turning cut, it's the whole tool holder.

I've managed to make some chamfers with one of Manchester's part off tools, but I did it super gently. I grooved to half depth first, then I backed off & came back in at a .0005"/rev feed rate on a SMALL radial cut to get my chamfer. Even being that gentle, I still had to keep an eye on that thing. That style of tool is generally rated for ZERO side load. You are lucky to get anything at all with one of them.

I've used that rig you see in my pictures to part off 3" cold roll & aluminum that was even bigger than that on a crummy little 10" lathe. I find that I can part off about 5 times faster than I can make a cut with a band saw & the finish is better.

Hardinge makes a beautiful machine. Years ago, I often used to run one in a shop that I worked at. I don't have one myself. That machine even made my Clausing Colechester look like a rough machine. I've never seen a Hardinge sell for $500 before. You did great on that deal. I keep hoping to bump into a HLV-H for reasonable money, but they never seem to sell for less than the down payment on a small house.

When it comes to getting a good finish, always remember the 3 "R's" of machining - Rigidity, Rigidity & Rigidity. A sharp tool & proper tool tip geometry can sometimes help too.

[PatMarlin]

THe thiner ISCAR tool I have accepts up to a .094 wide insert, and there is the "V" groove on the bottom and top,. Like you say it's not made for side load.

The next size up is .118 and it has a "V" on the bottom and the top, plus one on the nose face which gives it some strength to handle some side load. Not a lot, but is working for me and so far has held up. I'm still not 100% happy with it.

Some tools I have made a final decision on after much experimentation are working like gang busters. Several parts ran, and not a sign of wearing down, no built up edge, and reasonable cost. Needless to say I like that combination.

[Marvin S]

NO I've never:
put the decimal point in the wrong place.
forgotten the decimal point.
transposed a number.
forgotten the minus sign.
put the right tool offset in the wrong place.
put the wrong tool offset in the right place
called up the wrong work offset.
forgotten the r (or i&j) when calling a g2 or 3
or
forgotten to cancel a canned cycle .
Nope, never happens.:oops: (thankfully after 8 years it doesn't happen very often)

Yea that pretty much sums it up, they mostly do exactly what they are told to do. I been lucky enough so far to escape with a few broke inserts and a coolant snake or two. Not bad for here's your new CNC machine uncrate it hook it up and good luck. The HAAS set up guy hardly knew how to turn it on and set home, so he wernt no help.

[peterthevet]

I wonder if a deep grooving insert or possibly a profiling insert may be able to achieve what you are after....get a couple on insert catalogues (Kennametal/Sumitomo etc) and have a peruse.....just a few thoughts from left field....don't laugh if I'm wrong (just trying to help)!!!! I'm interested in machining but have little practical experience as yet!! Final thought - maybe a modified top notch insert........lots of cheap inserts on evilbay to try/play with. Cheers Peter

[mellonhead]

NO I've never:
put the decimal point in the wrong place.
forgotten the decimal point.
transposed a number.
forgotten the minus sign.
put the right tool offset in the wrong place.
put the wrong tool offset in the right place
called up the wrong work offset.
forgotten the r (or i&j) when calling a g2 or 3
or
forgotten to cancel a canned cycle .
Nope, never happens.:oops: (thankfully after 8 years it doesn't happen very often)



I just laughed when I read that. I'm glad I'm not the only one.

Toby

[JIMinPHX]

If you're having problems with edge build up, you might try a slightly more aggressive feed rate & a slower spindle speed, within reason of course. You also might try a slightly richer coolant mix. From the picture that you posted, it looks like you probably have enough coolant volume already.

Edit: or you could try a different grade of insert.

[JIMinPHX]

I should have mentioned this before, but I always just did it automatically, so It didn't occur to me right off that others may not do it. Those tools often work best when you peck with them. Go in about .020"or .030", then back out about .005", then go in another .020" or .030" & keep doing that until you reach the desired depth. Interrupted pecks like that prevent edge build up, allow for better lubrication & also give you better chip control.

[PatMarlin]

Well I got one problem solved with my drill chuck shaft.

But today- I'm back to cut off tooling hell. Now I only have the .118 wide ISCAR running and parting 01 drill rod, it just puts to much flex and pressure in the tool. It gives me inconsistant dimensions, but I seem to have it stalbized after all day of tweeking somewhat. The .087 ISCAR cuts way nicer. Unfortunately, I messed the seat up on that tool to far.

Talked to ISCAR and the tech suggested I try a "DuoGrip" type tool of theirs with the .087 width, and a 6drg lead angle. This bit is double ended. Twice as much money, but has 2 edges. Supposed to be much stronger, with side load as well so I ordered one.

It's good to see we have a group of CNC guys here at CB.

One thing that dawned on me this evening. Should I be running constant surface speed on cut off? Because I'm not and I think I big duh! is in order.

I'm running G95 -feed per revolution IPR on my Fagor control, as it's the only one I know right now. The tool cuts better as it nears the center.

Looking in the manual it calls for a G96 for CSS mode:




http://www.patmarlins.com/css.jpg


Now I've got to figure out how this works and wit the G22.

[JIMinPHX]

When you get done talking to the guys at Israeli Carbide (Iscar), you might want to give the boys over at Manchester a Jingle & see what they think. The guys at Iscar make a lot of nice stuff, but for cut off tools, I haven't seen anything that beats a Manchester.

& Yes, CSS can make a big difference if you are parting off through a large diameter or all the way to center. On the small diameter stuff, or going through thin wall sections, it doesn't really matter as much.

[PatMarlin]

Manchester. Have to check that out.

Bout' 1/2" all the way through.

[JIMinPHX]

1/2" is pretty small. If you take the parting tool all the way to center, that still beats on them. If you can drill a hole in the part first, even something small like 3/16", it makes a huge difference in the life expectancy of the part off tool. Even a little 1/8" hole will help, but then trying to push a 1/8" drill bit 6 or 8 diameters deep into tool steel can present issues of its own. 3/16" is much easier to drill with. If you get bits with good geometry, they should play ball with you, even in that material. Small drill bits tend to be cheaper than carbide inserts. ...just food for thought.

[PatMarlin]

Yep this one is all the way through hard steel. Can't use a drill.

[JIMinPHX]

I thought that you said you were working with O-1 drill rod. Whenever I buy that stuff, I get it in an annealed state. It drills fine with HSS bits as long as you keep the feeds & speeds where they belong & keep plenty of coolant on it. I make drill bushings out of that stuff all the time. I get 1/8" bits 3/4" deep without too much trouble. I get 3/32" bits through it more times than not without a catastrophe, although that's not always a sure thing. 3/16" bits are a walk in the park. Stick with 135 degree split point bits from a reputable manufacturer like Cleveland, Triumph, or Chicago Latrobe & you should be able to get 30 or more inch-deep holes out of a $2 bit.

By the way, Ghurring spot bits are on sale at MSC this month. They ain't $2, but they are offered at a reasonable discount off the going rate. Keo center drills are on sale at a pretty attractive price too.