2.375in hole in 17-4

[gregormarwick]

I do think if we can get away with just a spade drill to pull some material out that might be the best MRR/$$$ ratio for the few minutes it should take.

Forget about a spade drill, that is an insert drill job.

 

[boosted]

Forget about a spade drill, that is an insert drill job.

I think I'm pretty convinced that's the way to go. See my previous post, how do I hang on to it in this little machine!?

 

[gregormarwick]

Dumb question. If I get a Sandvik 880 at that size, it has as 1.5in shank diameter. What's the best way to hang onto that big ass shank in a mill?

CAT40 1.5in sidelocks seem to be a bit rare, and would require grinding a flat.

I think I'm pretty convinced that's the way to go. See my previous post, how do I hang on to it in this little machine!?

All cylindrical shank insert drills have a flat or a whistle notch. 880 drills have a flat.

60mm 880 is a 40mm shank.

 

[SND]

I was just thinking that although the mill's spindle claims 30hp, it might not really have the torque at 900rpm or so eh? might be tough to break at chip and not stall that thing, and TSC would also be gooder....

For some reason I thought the 880's were available with Cat end looks like it's a Capto or 1.5" straight shank on those 2-3/8".

Helical milling down with an inserted cutter if you got TSC could be pretty fast and at least make small chips and keep the RPM's higher in the happy HP zone.

 

[???]

If you don't have the horsepower you can drill to size with 2 drills, still faster than helical milling.

 

[SND]

If you don't have the horsepower you can drill to size with 2 drills, still faster than helical milling.

Not with an insert drill, have fun stepping with those.... And if it ain't got the power/feed to push an 880 or DS20, forget spades entirely, actually, forget spades always...
Chip management is gonna be an issue with drilling if he can't push hard enough to break a decent ship and even then it's a big chip so don't forget to add time of dealing with that to the process. At least helical milling is sure to break decent chips, just gotta be able to blow them out of the hole. Also less risk of chipping an edge on break through.

 

[???]

10 Reasons Twin Boring is Better for Holemaking than Helical Interpolation

Anyone who’s made holes understands the difficulties that can arise: vibration, wander and even breakage. When it comes to production-level volume, these issues become even more limiting. Many turn to helical interpolation with a mill as a reliable way to rough out holes. We’re here to tell you...

www.bigdaishowa.com

 

[gregormarwick]

10 Reasons Twin Boring is Better for Holemaking than Helical Interpolation

Anyone who’s made holes understands the difficulties that can arise: vibration, wander and even breakage. When it comes to production-level volume, these issues become even more limiting. Many turn to helical interpolation with a mill as a reliable way to rough out holes. We’re here to tell you...

www.bigdaishowa.com

Twin/triple rough boring heads pull much more torque than an insert drill. Especially in a gummy long chipping material like condition A 17-4 when you have to really push the feedrate to break a chip.

They're fantastic when they fit nicely in the torque curve of the spindle, when they don't they are absolutely miserable.

 

[dandrummerman21]

Is it really going to be the spindle power that is limiting? I have a feeling that Z thrust would be the limiting factor here.

I've got a makino A88 with 40hp and dual z ballscrews and the last time i tried drilling a 2.5" hole, it came nowhere close to advertised feeds for z thrust alone. Ended up with a different approach because underfeeding the drill was not an option.

now, a 5 inch feedmill in titanium on the other hand, at 120rpm and 60ipm? no problem for said machine.

Edit: just checked since it has been 10 years on the feedmill. last program we saved from that run was 180rpm at 72ipm (that's .400" per rev. tool has 9 teeth)... .035 stepdown. Could have probably upped it to .045 but we were wimps!

 

[TKassoc]

This part shape and work holding has me wondering if this is one of the few applications where an 1.5" or 2" inserted plunge rougher is the correct tool.

 

[Ox]

12.5in OD slug. In OP1 it goes from ~200lbs to ~40lbs.

This picture of the pocket feature might make it a little more clear why I don't think it's worth the hassle of punching the hole out on the lathe. Total cycle time for that hole is less than 15 minutes. Total roughing time for the whole pocket (including coming back in with the high feed) is about 30 minutes. The same solid carbide that does 90% of the work in that pocket spends about an hour roughing the OD. It has been a very consistent process, relatively drama free, and relatively quick. But I would like to reduce time in cut for the solid carbide, as they are not cheap.

I do think if we can get away with just a spade drill to pull some material out that might be the best MRR/$$$ ratio for the few minutes it should take.

View attachment 434479

,,, and you're dooing that in a vertical?


------------

I am Ox and I approve this here post!

 

[boosted]

\

,,, and you're dooing that in a vertical?


------------

I am Ox and I approve this here post!

Besides the hole in the center, it's all mill work. I've found that if you can get the chips out of the way, the part doesn't really care if it's sitting vertical or horizontal.

But yes. 5.5 hrs each on the vertical, then 2.5 hours each on the 5 axis. We run 2 at a time so we can get one load in the morning and another at night so it runs almost continuously. At this point I'm just looking to optimize a little bit, and the cost of that solid carbide which does most of the roughing is near top of my list.

Parts are sitting right now while I wait for a 2.375in Sandvik 880 to test next week. Fingers crossed. Will definitely give the machine a workout.

 

[Ox]

You must run a very high volume of coolant to keep that bowl flushed?
Does your coolant not get too warm?
Not overly tight size tols?


--------------------

I am Ox and I approve this here post!

 

[dandrummerman21]

I'd be more concerned with getting the chips spraying towards and into the conveyor, than simply out of that pocket. Who likes shoveling chips?

 

[Orange Vise]

but getting all the way to the bottom of the pocket is a chore, and the endmills are expensive.

What's the size and geometry of these endmills?

 

[boosted]

I'd be more concerned with getting the chips spraying towards and into the conveyor, than simply out of that pocket. Who likes shoveling chips?

Not me!

We're good. Chip evacuation on that machine (M560V) leaves something to be desired, but we hose it out at the end of a 11 hour run with pretty minimal drama.

What's the size and geometry of these endmills?

We have Kennametal HARVI IV. 5/8 diameter. It's an 8 flute with a chipbreaker. 3XD LOC. In a shrink so we can really squeeze into the hole and get the most material possible out before rest machining with a high feed. Not normally a fan of Kennametal, but they work really well for this. The ISCAR and Mits 2in and 2.5in high feed that we use with some frequency are not even close to the same MRR, and a lot of insert wear issues.

 

[boosted]

You must run a very high volume of coolant to keep that bowl flushed?
Does your coolant not get too warm?
Not overly tight size tols?


--------------------

I am Ox and I approve this here post!

With a nice chipbreaker, a 1inch through hole to start, and through holder coolant flushing, it's pretty easy to keep the pocket clear. Coolant stays room temperature. It does atomize like crazy though. We are adding 5 - 10 gallons a day to make up for mist evaporation. Don't get me wrong, I'd probably put in on a horizontal if we had one, but I don't find the vertical to be much of a liability for this particular part.

Nothing crazy tight on OP1. Just +/- .001in on the o-ring depth and width. The Okuma has pretty decent spindle growth comp. Doesn't tend to drift much. We drag it over to the 5 axis for OP2 and put it all the critical stuff at the same time.

 

[Ox]

I am just surprised that you are able to doo that much werk - AND flush all those chips - and still keep your coolant that cool.

You are able to flush all the chips out the bottom then?

I was expecting that your coolant would be getting quite warm, and that bowl looks like a stickler for following temperature growth.


----------------------

Think Snow Eh!
Ox

 

[Orange Vise]

We have Kennametal HARVI IV. 5/8 diameter. It's an 8 flute with a chipbreaker. 3XD LOC. In a shrink so we can really squeeze into the hole and get the most material possible out before rest machining with a high feed. Not normally a fan of Kennametal, but they work really well for this. The ISCAR and Mits 2in and 2.5in high feed that we use with some frequency are not even close to the same MRR, and a lot of insert wear issues.

Hmm I think you might already be optimized for this process.

What you're doing with the shrink holder and 3xD tool to avoid using more expensive, slower-running, long reach tools for roughing was a smart move.

 

[boosted]

Well, the Sandvik 880 worked fantastic. I am using a 1.000in ISCAR Chamdrill to pilot, then coming in with the 2.250in Sandvik.

The machine has just enough power to push the drill hard enough that it settles down. 4.14IPM @ 1036RPM. Unfortunately I am pecking every .100in to break the chips. Not the fastest at ~ 4min per hole, but not too bad considering how cheap inserts are!

Thanks for the help. It was worth it just to see the looks on faces as I came sauntering across the shop with that 12lb drill in a sidelock where the tool interface is bigger than the CAT40 end.