Machine collision from drilling

We're drilling 1" holes in SS 304L, with 1/2" (140°) solid carbide, TiAlN coated.

The initial plunges sounded heavy, like they were pushing into the stock.

A few pecks through, the machine gave a collision warning.

We went through 2 tools, one of them had a tooth break off.



We increased the rpm by 40%, and right after it crashed again.
Any ideas why this happened?

Just where are you pulling your speeds and feeds from? Fusion defaults?

60 SFM and .004 IPR for 304 with a 1/2" carbide hi-perf drill.....

For starters:

-Don't peck. It's a carbide drill. You don't have to.
-Run more like 200 SFM and .01 IPR.* (1500 RPM and 15 IPM)



*(In 1018 you can run 400 SFM and .018 IPR with a Kennametal.)

ChipSplitter said:

Just where are you pulling your speeds and feeds from? Fusion defaults?

60 SFM and .004 IPR for 304 with a 1/2" carbide hi-perf drill.....

For starters:

-Don't peck. It's a carbide drill. You don't have to.
-Run more like 200 SFM and .01 IPR.* (1500 RPM and 15 IPM)



*(In 1018 you can run 400 SFM and .018 IPR with a Kennametal.)

Click to expand...

GWizard recommendations. 50% between aggressive/conservative.
Doesn't really explain why it crashed and broke a tooth.

teachme said:

GWizard recommendations. 50% between aggressive/conservative.
Doesn't really explain why it crashed and broke a tooth.

Click to expand...

Gwizard is garbage, that's why it's "crashing". Are you spotting your holes? If so that can cause chatter with carbide drills and will rapidly destroy the cutting edges. I'd run 1000-1500 rpm and somewhere around 10ipm and 8ncrease from there, no peck.


Or get a good .375 endmill and interpolate it.

teachme said:

GWizard recommendations. 50% between aggressive/conservative.
Doesn't really explain why it crashed and broke a tooth.

Click to expand...

I don't trust GWizard. Made by a hobbyist....

Try what I posted above.
My WAG is you were feeding too slow and work-hardened.
At .004 IPR with a 1/2" drill you will need to peck to break chips. You need more like .01 IPR.

Without more details it's hard to say for sure, though.

You guys are going about this all wrong. No need to change feeds and speeds. Just switch to a cobalt twist drill and everything should be about spot on

Sometimes when pecking chips will be left in the hole, then if the code makes the drill return directly to the last cut point, the tip will crash into those chips. This can definitely fracture carbide drills, so I agree with those saying "no pecks", especially if only drilling an inch deep.

As for S/F, I'd like to know how the tool and part are held. If things aren't rigid enough then a softer feed makes sense, but you're better off being aggressive if the tooling will allow it.

I've used HSM advisor with a 1/2" machine length cobalt drill with no issues in 304. Don't remember the settings, but HSM advisor hasn't failed me yet.

Wsurfer said:

I've used HSM advisor with a 1/2" machine length cobalt drill with no issues in 304. Don't remember the settings, but HSM advisor hasn't failed me yet.

Click to expand...

There's no replacement for experience...no program can beat that or replicate it's results.

plastikdreams said:

There's no replacement for experience...no program can beat that or replicate it's results.

Click to expand...

I also prefer to fly by the seat of my pants

Hardplates said:

I also prefer to fly by the seat of my pants

Click to expand...

I'm just glad my pants have a fly...

Hardplates said:

I also prefer to fly by the seat of my pants

Click to expand...

Sometimes that green button can cause some exhilaration and some adrenaline...mmm it's fun

TSC on the drill? L x D ratio? If it is a jobber length drill with flood coolant it may also be an issue. Stainless loves TSC, no spot drill, nothing extra unless your drill is over 8xD in which case a stub length carbide drill should be used initially, most manufacturers have pilot drills specifically.

Here is a basic TSC drill with speeds/feeds for reference.
Solid Carbide Coolant Thru Drill 294A Series .5000 Diameter MariTool
If you click the feeds and speeds image a very good starting parameters chart is listed.

180 sfpm converted to rpm
3.82 x 180 / .500 = 1,375rpm

.0065 ipr converted to ipm
IPM = RPM * IPR
1,375 x .0065 = 9ipm

These are starting parameters, feedrate may double or triple to force a chip to break with TSC, and actually make the drill last longer.

With longer drills or flood coolant 1.000" deep you may want to program something by hand to enter at 50% feed until the point is buried then ramp up to 9ipm. Any pecking greater increases the chance of chipping the carbide, 1.000" is very shallow.

Hardplates said:

I also prefer to fly by the seat of my pants

Click to expand...

Kinda something how that werks.......

I judge speed/feed advisors by my internal calculator a.k.a. gut feeling. Rarely lets me down, either.

G-Wizard has been feeding my feeds and speeds needs for nearly two decades without trouble or any great sense of lacking. For those of you bashing it, I"d have to imagine that you haven't actually used it or used it enough to get a handle on it.

In general I do think it runs HSS drill feeds on the slow-ish side. Not terribly so, but a little. That has improved here in the last few years. My favorite drill feed info is still in the back pages of an old Precision Twist Drill catalog. I'll turn to that when GW strikes me as balking on feed. I always leave the slider at 100%, especially for drills.

Honestly if I'm running a 100 dollar carbide drill I'll go to the manufacturers literature and start from there and not GW. Same with any specialty cutter like you might find from Harvey. And I wouldn't be running carbide on this job unless I was doing a lot of holes and was using TSC. The cobalt and no peck suggestions stated earlier make about the most sense.

G-Wizard milling feeds are heavily weighted by tool stick out, which by extension controls the maximum feed rate before chatter is expected. The software has a setup page to take into account the machine used. Like with any F&S software, secure and proper tool holding has to be a given, and is up to the operator to make that as good as reasonable or possible for the task at hand. I've seen very little discussion of tool stick out as a factor weighing into other F&S Calculators out there. (Not that I've studied many) I'd be curious to hear how many other calculators ask you for tool stick out as part of any tools setup criteria. If you ask me, it is very high up on the important factor list. And honestly, GW's chatter point predictions are pretty darn good.

Anyway... I've got my broken tool graveyard like anybody else, but little of that is G-Wizards fault. And I can assure you, the last thing I'm going to do is allow my machines to lolly-gag through the material while machining a part. G-Wizard does not make those types of suggestions. And if by chance it does, there is always experience to modify suggestions as deemed fitting.

FWIW, I've used a Kennametal Universal drill, which is their basic carbide drill with a Dynapoint and TiAlN coating.

I had a job using a 13 mm (.512") 3xD drilling holes in long tubing so I wanted to run it dry.
I ran 150 sfm to keep the heat down and .02 ipr feedrate. Chips were crazy thick, but it was dead quiet and never chipped.
The OSG rep was scared stiff to watch it run. He didn't give me a chance to try his drill....

The owner of a company I worked at touted gwizard as the next coming pretty much...I tried it and every time I was able to double or triple process times over what I got with gwizard. It was really good at burning cutters in 17-4 though lol.

plastikdreams said:

The owner of a company I worked at touted gwizard as the next coming pretty much...I tried it and every time I was able to double or triple process times over what I got with gwizard. It was really good at burning cutters in 17-4 though lol.

Click to expand...

There is no way a computer program can take all the variables into consideration and give you the best numbers.
There are recommendations and starting points but they are tweaked endlessly for optimum performance.


You learn from experience. Period.

ChipSplitter said:

There is no way a computer program can take all the variables into consideration and give you the best numbers.
There are recommendations and starting points but they are tweaked endlessly for optimum performance.


You learn from experience. Period.

Click to expand...

Exactly.

Or "Like," in other words. : - )

The best collection of machining information I can recommend is on the Sandvik website. Just click on the knowledge page for all topics, but here is a link to drilling in particular.

Drilling

I am not in any way affiliated with Sandvik, but this collection is excellent.