What did I do wrong - Steel chip welding on carbide

I'm working on some light fabrications on mild steel 1"x2"x0.065" rectangle tube. I have to cut 2 0.4"x0.6" oval holes, 1 0.375"wide x 0.08" deep slot across the 1" side, and then drill 24 0.312" holes on the other 1" side. Machine is a Tree VMC1060 with a delta 50 control.

I drill a hole in the center of the oval then use a 1/4" end mill to cut the oval using the pocket frame mill cycle on my control. Seems to work fine, makes a little noise, but I figure that comes with the material I'm working on.

Then I cut the slot using the 1/4" end mill to save a tool change. I've tried to run 2 parts, and both times it appears to get chip welding and snaps the end mill. It's a generic ebay 4 flute no coating.

I have 0 experience running steel in this thing, so I went to the internet and found a feed/speed chart and it suggested 350 sfm and 0.0017 ipt. So 5300RPM and 34ipm. I cut the feed down to 10 where it plowed across the part, and that made vibrant blue chips and a nice fireworks show before it snapped. Next go around I shot from the hip and slowed it down to 2000rpm and 8ipm, I didn't see much color in the chips this time, but it still had the flutes filled up.

how fast should I be going?

Also any tips for drilling holes without getting a large burr on the exit side (inside the tube that I need to remove)

bastarddsm said:

It's a generic ebay 4 flute no coating.

Click to expand...

Well thars yer problem...

I dunno, maybe it works for you, but I use quality tooling; mostly Helical and Harvey for long running stuff, Redline if I don't need as much life or I know I going to abuse the cutter and want something cheaper. It's still head and shoulders better than a generic eBay cutter. I always get the coating, even on the cheaper Redlines, unless I'm cutting plastic. Spending a little more on tooling pays dividends every time I don't have to replace the tool.

Are you using coolant or air blast? Carbide with TIALN coating likes to cut steel with air blast, but I'll run thru spindle coolant for deep pockets just to get the chips out better.

What he said.

As for the hanging off-side burr?

No CNC nor toolchangers under my roof, but.. if yah got 'em, use 'em?

Sounds like a bare touch for last-pass, different tool and parameters, might slice-away the burr's "hinge" anchor ... and drop it right off? Puff of air or spritz of coolant do the usual?

Still have a trace of sharpish edge, off-side, but at least no significant stray material to mess-up the next operation(s), even if not much to 'em.

Or so I'd expect and try.. or seek further advice from the grown-ups.. not being a kid overly fond of manual de-burring.

I've had these for longer than I've known better, and since this is just mild steel with a very small amount of material removed they ought to work. Another problem, it's saturday, and I can't just go get something else. So what sort of speed and feed should I be try while plowing though?

No airblast, but I did try coolant.

thermite said:

Sounds like a bare touch for last-pass, different tool and parameters, might slice-away the burr's "hinge" anchor ... and drop it right off? Puff of air or spritz of coolant do the usual?

Click to expand...

I'm not sure what you are suggesting here. Drop down through with a thread mill or the like and chamfer the back side? I was kinda hoping for a drilling technique to minimize the burr. It is as simple as I'm using a junk drill bit?

I believe he means cut leaving maybe .010" on all faces, then switch to a fresh tool and do a finish pass.

bastarddsm said:

I'm not sure what you are suggesting here. Drop down through with a thread mill or the like and chamfer the back side? I was kinda hoping for a drilling technique to minimize the burr. It is as simple as I'm using a junk drill bit?

Click to expand...

Better endmill alone, NO toolchange, MIGHT do it. As said, CNC is not my rice-bowl, but I am more than just "vaguely aware" than not all passes need be identical even if the tool still is.

What you seek is a burr too thin to support itself even against the modest force of clean-up sluice at least "most of the time", and fast and easy to de-burr with only a general hit when it does NOT fully detach. No min-wage kid with Swiss-files, hand-deburr tool, media blast, or the like in the skinney-minney-budget.

SOME materials you might do the opposite. Goal for a thicker section that breaks of in small chunks as you go .. because the HEAVIER cut over-stressed its ability to even sustain a connection to the parent at all as it was pushed aside.

Given that .... Subtractive machining in general consists of repeatedly "work hardening" the target right ahead of the cutting edge beyond its point of failure?

The "hinge" of a(ny) burr as is still anchored to the parent metal is selectively weakened vs the portion as has yielded.... OR the parent metal to which still attached.

"Differentiated" if you will. Already. That's akin to perforated "tear here" paper.

Experienced clever-devils take advantage of both situations to reduce ops, shorten cycle times, improve revenues.

Become one.

Hopefully, one who DOES this s**t.. eg: - routinely cuts more cleanly than the average bear - and in the CURRENT century.. will drop by and assist.

Minimizing cutting tool burrs in general are a really OLD part of a(ny) job well run. They get no love. NO one wants them.

Burrs are a reduceable pain in the a**. And NOT just in the manufacture of sex toys for the adventurous! Or so one reads about in the funny-papers..

So JF Reduce them.

350 SFM and 140 SFM.
Not a believer in small steps here I guess.
You have gone off both ends. Some advice Dad gave me a while back with uncoated carbide.
"Chips should come off silver and at least half of them should turn blue as they hit the floor."
Air blow and your load per tooth a tad high for full width slotting. Profile at 60% yes, slot no.
You are most likely using a C-2 grade endmill and these face weld if not enough speed.
Fireworks are very bad and too much speed.
Full width slots can be a pain as there is no climb or conventional cutting.
The chip starts thin (bad), goes way up and then back down and the tooth has to carry and make room for the chip until the exit point where hopefully it exits.
Do not recut chips, the tool must unload on the back side of the slot and it has very little time to do that.
Bob

Seeing as your holes are all on one side, it'd be worth a tool change to install a 1/4" DA (or SA) cutter with a short neck to do your back de-burring.

Program your de-burr path in Incremental Mode with it starting and stopping at the center of a 5/16 hole, and make that a subroutine. Then copy and paste your drill cycle, drop the drilling parameters, and stick a Subroutine call after each hole location. Your troubles will be over soon enough. Well... that is if you have a cutter in house.

For your slots, the small finish pass mentioned is not a bad idea, or the DA tool will clean those slots up too, plus leave a chamfer to boot. On both sides if you're willing.

Agree with Bob ^. Surface speed 350 & cut the feed by half. The steel used in tubing is very low in carbon and tends to be the gummiest stuff you’ll ever run into…

Good luck,
Matt

13engines said:

Seeing as your holes are all on one side, it'd be worth a tool change to install a 1/4" DA (or SA) cutter with a short neck to do your back de-burring.

Program your de-burr path in Incremental Mode with it starting and stopping at the center of a 5/16 hole, and make that a subroutine. Then copy and paste your drill cycle, drop the drilling parameters, and stick a Subroutine call after each hole location. Your troubles will be over soon enough. Well... that is if you have a cutter in house.

For your slots, the small finish pass mentioned is not a bad idea, or the DA tool will clean those slots up too, plus leave a chamfer to boot. On both sides if you're willing.

Click to expand...

"Eligible for hire".

I don't actually OWN much nicer language.
Didn't much need it. Not that you are alone, either, BTW.

Cats get skint, Invoices gets paid. Ever' body eats for one more day and counting.

Matt_Maguire said:

..steel used in tubing is very low in carbon and tends to be the gummiest stuff you’ll ever run into…

Click to expand...

LOL! Ain't life a b***h?

Interviewed as Plant Mangler for a DOM outfit onct.. 'bout half a century ago?.

It dam' near HAS to be "gummy" if you want to make yer tube throughput numbers cheaply!

thermite said:

Better endmill alone, NO toolchange, MIGHT do it. As said, CNC is not my rice-bowl, but I am more than just "vaguely aware" than not all passes need be identical even if the tool still is.

Click to expand...

I don't know how to make this not sound backhanded, but thanks I appreciate being made to think about it, instead of being spoon fed. I think the gist of what you are saying is take a finish cut. The burrs I'm worried about are from drilling, not milling though. I suppose tomorrow I'll go out and drill it with a 19/64 first, then second pass with a 5/16" and see how that does. 

Matt_Maguire said:

Agree with Bob ^. Surface speed 350 & cut the feed by half. The steel used in tubing is very low in carbon and tends to be the gummiest stuff you’ll ever run into…

Good luck,
Matt

Click to expand...

So like .0008ipt? Doesn't too slow of feed get into rubbing instead of cutting?

CarbideBob said:

350 SFM and 140 SFM.
Not a believer in small steps here I guess.
You have gone off both ends. Some advice Dad gave me a while back with uncoated carbide.
"Chips should come off silver and at least half of them should turn blue as the
Air blow and your load per tooth a tad high for full width slotting. Profile at 60% yes, slot no.
You are most likely using a C-2 grade endmill and these face weld if not enough speed.
Fireworks are very bad and too much speed.
Full width slots can be a pain as there is no climb or conventional cutting.
The chip starts thin (bad), goes way up and then back down and the tooth has to carry and make room for the chip until the exit point where hopefully it exits.
Do not recut chips, the tool must unload on the back side of the slot and it has very little time to do that.
Bob

Click to expand...

Well, the fireworks and breaking the first one right away kinda scared me so I figured I ought to really slow it down. I get what you are saying about slotting, I'm guessing that this problem gets exponentially worse with smaller end mills? I could likely use a 3/8" in one pass with a better chance of sucsess, but some day I'm gonna have to make narrow slots, on a part that matters. 

I'm sort of confused on some of your statements. Fireworks say I'm going too fast, but also welding is too slow.

Air and oil go a long way to prevent welding

Sent from my SM-G955U using Tapatalk

bastarddsm said:

I don't know how to make this not sound backhanded, but thanks I appreciate being made to think about it, instead of being spoon fed. I think the gist of what you are saying is take a finish cut. The burrs I'm worried about are from drilling, not milling though. I suppose tomorrow I'll go out and drill it with a 19/64 first, then second pass with a 5/16" and see how that does. 

Click to expand...

Most of us CAN "spoon feed". But "direct" is waay faster... so long as dealing with another who realizes none among has yet learnt it ALL.. Quite often because we were off doing some OTHER thing and there just didn't happen to be "the" or "a" time (we had different JOBS, after all) - or a priority NEED to do "whatever" in any one, single person's working lifetime. Our "work" decides what we see. Then again, too many among us cheat and go off-shit to eat, sleep, or "formulate".

Not many put in 25 hours to the day any longer!



That's why we find it valuable to share.

Some have just dealt with more "slots", "holes", and "burrs" than others?
In the metal... or otherwise.



Helps to experiment, test a concept or tool choice, and prove it-out on scrap, BTW. Same-alloy and even shape best of all.

Generally cheaper and less em-bare-assing than adding to the scrap.
No scrap to-hand? Steel is cheap. Tooling less-so. And time is scarce.

The more alert to events a "seeker", the more inputs researched, and rapidly, the more observant to effects when put to the test?

The less time wasted. We all get but the ONE ration - however lean or generous. So make it COUNT. It matters.

Put a bit more "intensity" into it than just "I suppose".

'Coz there ain't "NFW" you can ever BUY "new" time, "recycle" wasted time, nor hunt cheap leftovers of "New, Old Stock" time to stash as "emergency spare" for future needs.

They call it "RDD" (Required Delivery Date) and "DDD" (Drop Dead Date) from more than a hundred years of "formalizing" the mere Management of ....... a reality .... that began with "Big Bang".

Who knows? "Big Bang" that began our whole dam' universe ...may have been over-budget, delivered late, and might not have met spec ... for excessive burrs?

You'd have to know eBay and shiddy endmills?

D'yah suppose even GOD gets cut a break for half-vast work?

Oh, yeah?

From whom?

Just read the funny papers.

Sure as Hell ain't his customers!

bastarddsm said:

So like .0008ipt? Doesn't too slow of feed get into rubbing instead of cutting?

Click to expand...

My bad! Actually went back & looked at Metcut&Associates(1967) & their starting parameters for C-2 carbide endmill (profiling) and a 1/4"EM would be 400SFPM, .0025"IPT & .050"DOC for 1008-1028 steel. They didn't do a lot of slotting with endmills in those days and when they did the EM had straight sides or 7-10 degree helix on the flutes (noisy but they didn't make crooked slots LOL).

Your slotting through the narrow side of the tube so if it's up out of the jaws very far that could cause some misery also with .065" wall tube.

Good luck,
Matt

Just to make it even more confusing on the slot my starting place in uncoated carbide would be 275-300 SFM and .0010/.0012 per tooth with air blow and then work the feed up from there and adjust the RPM by chip color.
I think .0025 per tooth rather heavy for a quarter inch in full width slotting in poopy steel.
Buy endmills with the least amount of standard flute length you can use and grip up as short as possible. This makes a big difference.
Rubbing is when you get down in the .0001/.0003 chipload although people with .025 diameter endmills make chips at this level.
Above all you must not recut chips so some method of making them go away is critical and you only have that back 180 to get them the heck out of Dodge when in a slot.
Bob

CarbideBob said:

Just to make it even more confusing on the slot my starting place in uncoated carbide would be 275-300 SFM and .0010/.0012 per tooth with air blow and then work the feed up from there and adjust the RPM by chip color.

Bob

Click to expand...

hmm. Yeah at that sfm it looked like I had a grinder in there. My chip load was low at 0.0005 though.

Hindsight these are not ebay cheapies, they are probably worse, they came from the guy that was selling a bucket load of used ones at $1ea. I've had them long enough I forgot where they came from. I'm guessing maybe they are just dull.

Old man I used work for liked to say "it's hard to make a living working with junk"

I didn't see it above but I like to move in "z" when cutting steel tube, for instance if I am making a 1" cut along the x axis I will cut through then as I make the 1" in x I may deop 1/4" in z then back up in the next cut so I use the entire tool fairly evenly. You can't always do this but when you can I think I ger more life