What's new
What's new

16mm Wide Thru Pocket/Slot 2.85" Deep in A36; Reconsidering Tooling

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
We run a part, maybe 200 parts per year, which has 2 deep "slots" that are 16mm wide and 40mm long. Full radius ends.

These are thru slots that break into a bore that is about 4" diameter. The tool must reach about 2.85" deep.

This is on a horizontal machining center.



We currently drill 1/2" holes in 3 places. Then we plunge a 5/8 carbide endmill at the center of either end of the slot, and then at the center of the slot. This removes the majority of the material, and leaves some cusps. We then finish the slot with a 1.5" long .5" endmill and then to follow that a 3" long 1/2" carbide endmill.


I have no problem with the finishing tools, but roughing it out takes a lot longer than I think I could do. Maybe more importantly, the 5/8 carbide endmill that we plunge takes a beating. The corners break down, and I usually take it to the diamond wheel and touch up them to first include a bit of a chamfer, but later "regrinds" to have a radius, and I increase the size of the hand ground radius until it won't reach anymore. Then I replace it and have them reground.

The side wall finish isn't too critical, this is for air to go through, so the walls often have overcutting where the endmill walks or simply cuts oversize. We run the slot a few thou big to compensate but you can usually see the witness marks.


So what I'm wondering is, does someone have a better tool I can use to finish this slot?


We predominantly use Iscar but I didn't see anything that I was confident would work.


We have a multimaster shank that is long enough and a 1/2" feedmill head for it, that I was tempted to use, but I've used that thing in steel before. It did not appreciate trying to break through the bottom of the 2" thick material, and broke really fast. I learned that day that you really shouldn't feedmill thin floors, nor should you break through a floor with a feedmill.


I was wondering if there was a beefier option than that solid carbide .480 diameter shank, too. Maybe a steel body feedmill, 14 or 15mm, long enough to reach. Then stop short of breaking through the bottom? Or are there maybe tools that would allow me to punch through without having to drill the last fractions of an inch?

Does anyone have an idea?
 

TeachMePlease

Diamond
Joined
Feb 11, 2014
Location
FL
This is just a stupid off the wall idea.... Do you have the travel to turn it 90° and rough out some with a big ol saw/keyseat cutter?
 

implmex

Titanium
Joined
Jun 23, 2002
Location
Vancouver BC Canada
Hi dandrummerman 21:
Are you plunge roughing...it kind of sounds like you are.
That's a great strategy, but as you're pointing out it beats the shit out of the corners of the cutter.
Once the corners are gone, the flutes start dragging in the slot and fuck up the rest of the cutter pretty quickly.

I've done better with boring bars or multi flute indexables that have 2 or 3 inserts sticking out so they're naturally relieved, and will still cut when they wear on the corners.
The trick is not to get too greedy with the stepover...smaller faster passes will do better than trying to chew out a great whack of material with each stepover.

A boring bar has done it in a pinch, and they last a surprisingly long time if they don't get buried in chips, but if you are making many parts, you can do better with the indexable.
Attached is a picture of an Iscar that has worked for me in the past for through slots.
These things are super tough and will take a severe beating and still work.
I don't know if you can get one small enough though.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

BTW, if you limit your stepover to something like 0.030" to 0.050" you might be able to avoid the finishing cutters altogether...if this is just an air slot, who cares if the sidewalls have a nice scallop pattern.
At that small stepover, you can feed the shit out of it and do no harm so long as you don't spin so fast that you burn up the cutter.
I made 1/16" slots that way...hundreds of them per part, each 0.100" deep in aluminum, and it was by far the fastest strategy and made the best looking part too.
I was plunging at something like 200 IPM with a 3% stepover and it sounded like a machine gun.
 

Attachments

  • indexable.JPG
    indexable.JPG
    12.3 KB · Views: 32

Bobw

Diamond
Joined
Feb 8, 2005
Location
Hatch, NM Chile capital of the WORLD
Necked back solid carbide. Maritool.

6:1 on a 1/2" endmill that is mostly SOLID shank is pretty damn
rigid. Its not like running 1" of flute choked up onto the holder,
but its pretty impressive.

I've run 1/2" endmills with 3" of flute, and they suck. When
2 of those 3" is solid, its a completely different experience.
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
I think I'd chain drill as you are, but with a 39/64" drill that's spaced out ~.005" to each end to get most of the length. Then use a necked 5/8" endmill rougher to zig-zag (ramp, clear, ramp) to depth at ~.008" INSIDE the extents (i.e. don't take the full cut, just miss touching the drilled full diameter).

Then finish with a smaller necked endmill, get Frank to grind you a few six-flute 14mm or similar "nearly there" cutters. If it turns out that the 5/8" rougher cuts oversize, ask Frank for some .600" or whatever four flute necked for that op.

With custom endmills being so fast and relatively cheap to get, this is an application where I'd take advantage of that.
 

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
How'bout if you drill the ends through with say a 15.5mm drill instead and forget about the 5/8 altogether.
Then take a long shank 1/2" necked down just a little bit as to avoid rubbing, and then haul ass between the end-holes with a small stepover.
Even better, like Marcus suggested there should be some high-feed inserted cutters ( like the Mitsubishi AJX ) and you won't even need to pre-drill.

Though Mitsubishi's website sucks monkeyballs, but look up the AJXU06R102SA10L part number.
Carbide depot list them for $221.86 and is available. AJXU06R102SA10L
It is a 5/8 dia, 2.75 LOC 2 insert cutter, max stepdown is .039, but trust me, it hauls.
 

Job Shopper TN

Cast Iron
Joined
May 17, 2015
Location
Southeast TN
5/8 high feed mill, zigzag ramp It would be pretty wild. YG1 HF4 would be a good place to start if they go that small. In A36, I could see feeds of 250-300 IPM, .020 or so stepdown each way. Thru spindle coolant would be needed to get chips out, or still drill each end was you are. Then finish with a necked 1/2” if need be. High feed mills are insane for the right applications.
 

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
In A36, I could see feeds of 250-300 IPM, .020 or so stepdown each way. Thru spindle coolant would be needed to get chips out, or still drill each end was you are. Then finish with a necked 1/2” if need be. High feed mills are insane for the right applications.


That Mits I linked to did 400SFM @ 225IPM dry on 304SS.
My features were open so a light "airblow" was enough to get the chips out of the way.
For his slots an air-blast would be mandatory, and in A36 prolly still stay dry....
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Thank you for the suggestions. I'll try to address everything real quick, sorry if i miss something.

The slot is too short (only 1.5" approximate length) to benefit from a keycutter from the far side.

I am plunge roughing the holes basically. What I mean is, I have 1/2" holes because that's about as big as I can get without the holes touching each other. Drilling larger means they break into each other and the drill walks more, and has broken. We used to drill them bigger, perhaps .590, in the past, but sometimes the drill would die when doing the middle of 3 holes, as it is an interrupted cut (breaks into the 2 end holes). Now, I drill near the ends, then plunge the ends with 5/8, then I plunge the center with the 5/8. I do not plunge more than 3 places per slot. I actually go pretty damn slow for carbide. only about 700rpm and 5ipm. I'm sure we'd tried faster in the past and this ended up being the sweet spot.

The idea of some indexable, whether its a 5/8 drill or 5/8 extended endmill to plunge this, sounds like a great idea. The 3" long 5/8" endmills we use aren't cheap (maybe 100$?). I do probably get 100parts per tool, but this is with me touching it up a couple times by hand before swapping it.

Machine does have thru spindle coolant and air available, although this tool does not.

My drills for this are also HSS so there's a fair amount of time that could be saved if I could avoid the drilling entirely.


I could also do drill the corners bigger and do high speed milling with a necked 1/2" tool, in 3 or 4 steps.


I think the most intriguing is the high feed mill. So will a 2.75" reach feedmill appreciate breaking through the bottom? Because that is my biggest worry. (Leaving the bore solid and slotting before the bore is done is not possible because this bore is turned on the lathe before this op and can't be done after.)

I worry that the skin at the bottom will catch the tool and snap off an insert. Does anyone else slot through reliably with a long 5/8 or similar size feedmill? I also wonder how much the tool will walk. if the whole slot was .640 I'd be okay, but I'd be leery if it cut any bigger than that.


While the slot is for air and the customer has never complained about the plunge marks on the slot, I wouldn't say that it doesn't need to look good. At the very least, it needs to not look terrible. They are a larger customer of ours, and this is only one of many parts we run year after year.
 

gregormarwick

Diamond
Joined
Feb 7, 2007
Location
Aberdeen, UK
High feed is the answer. If the wall finish is not that important, single pass helical from solid with a 0.5mm stepdown. It will still leave a better finish that you are getting now, I'd put money on.

Breaking through will be no problem if the thin piece that punches out the bottom stays in one piece.

Solid carbide shank with screw on head, Horn DGH works really well. I have a 16mm one that would probably handle ramping end to end in that slot, but it's not the ideal way to do it.

eShop - Paul Horn GmbH
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Breaking through will be no problem if the thin piece that punches out the bottom stays in one piece.

Obviously it is my worry that it somehow won't, or it will get lodged. Not sure if you've considered it, but since I'm breaking through the wall of a 4" bore, there's a Z difference of about .160" (4mm) between the top of the bore to the end of the slot. So I worry that it will break through in "1 piece" but might be weird and flexy and somehow get bent upwards and pinched, blowing up the insert.

But the more suggestions I see about the high feed mill, the more I want to try it. I actually now just found iscar does have a 5/8 feedmill with 3" of length, which I already have inserts for. (we used to have a 5/8" feedmill about 1" long that died spectacularly on another job a while ago, that we never replaced)
 

Rick Finsta

Stainless
Joined
Sep 27, 2017
What happens is the high feed pushes the material down until the actual OD of the tool contacts the very bottom of the slot, then the floor drops out. It sounds like shit (seriously it is an awful racket) and beats up inserts but solid carbide high feeds don't seem too bothered by it. I do this when I make steel torque plates for customers - usually 4140 or A36 - and I get these 0.050" thick pucks dropping out the bottom that have been obviously distorted by the downwards tool pressure.

However, if you are really worried about it, then drill one end and plunge mill with a high feed. You can plunge mill stupid fast with them at relatively insane stepovers.

I would absolutely use air through tool for this application. If you recut with a high feed you are asking a LOT of the tool and that is about the only way I've ever blown an insert or chipped a solid carbide high feed.

I would use a 1/2" or 12mm high feed and ramp contour it. 1200-1500SFM (start at 600-800 and adjust upwards until your chips are turning blue), 1-1.5deg ramp (limit depth of cut to the tool's maximum, say around 0.015-0.020" for a 1/2" tool), 0.015-0.020" feed per tooth with a Seco/Niagara tool.

Hope that helps.
 

lastrada

Aluminum
Joined
Aug 23, 2014
Location
Indiana
But the more suggestions I see about the high feed mill, the more I want to try it.

I would go for it and I think it would solve a lot of your issues. I used to mill out large injection molds that required really long reach tooling, a high feed screw on head on a carbide bar works wonders.
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
As far as chain drilling with a larger drill, if you use a straight (constant, not S/D) split point stub you should have no walking. I drill like this for a lot of deep features without a problem.

.6094" 39/64" PREMIUM STEEL STUB LENGTH DRILL 135 DEGREE SPLIT POINT | North Bay Cutting Tools ["Premium HHS steel @ $23]

.6094" 39/64" COBALT SCREW MACHINE LENGTH DRILL | North Bay Cutting Tools [Cobalt @ $30]

Of amusing note: I'd not heard of the (Swedish) company that made the second drill, so I checked it out. Turns out they're almost 500 years old (yes, one 5 and two 0), listed on a tax role in 1538. I guess that gives them a little more gravitas than a fly-by-night like Westinghouse.
 

tonymor

Aluminum
Joined
Feb 9, 2017
Location
Chambersburg PA USA
We use this tool to plunge mill out a 20mm wide slot 70mm deep about 80mm long in 1045.

R217.21-1225.RE-LO06.4A | Secotools.com

Tips are double sided so have 4 cutting faces per tip. We run batches 100 at a time and flip the tips at 50 just to be safe.

We're doing this on a smallish lathe with live tooling so I know the tool could be pushed harder than we do.
Seco have a nice ER32-Combimaster adapter that works well on the lathe. It's the main reason we ended up doing it this way.

They do seem to have a 16mm & 12mm version also.

Seco plunge mill.JPG
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
I would avoid drilling entirely and take a standard 1/2" dia variable helix end mill with 1-1/4" flute length and hog out the slot as deep as you can, finish it also.
Then grab a necked end mill and continue on taking lighter cuts breaking thru.

Or use a high feed mill.
Either of these 2 ways will save you a ton of time.
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Alright so I went to my handy "fucked up tools drawer" to see what the deal was with the 5/8" feedmill we had was.

So the inserts were chewed up, screws bent, and the pockets are semi-wasted. BUT with a loving touch, I was able to break out the rest of the carbide, drill the screws out from the back, and some fine touches with the dremel tool, and the tool is back in service!

Now, its only 2" long (I thought it was shorter) but it appears to be long enough that I can neck it back further and grind a flat near the end of the shank.

There is about .0015" difference in the height of the inserts (That does not concern me) and one insert sticks out about .002" further (also not a concern) so it is wounded but I'm sure it will be fine. And if I lose it, it didn't cost anything. It measures .621 across the inserts.

Now I need to find the time to stick it in the machine and play with the program. Maybe this weekend or monday. Currently the parts are running and we've got maybe 50 more of this batch to go. But I'd like to get this changed over on this batch so I can plan for the next one.

I'm still unsure if am going to drill one end and plunge mill, or just ramp down back and forth. I'll see what I come up with and try to report back in a timely manner. I'll still be reading if any other tool suggestions or methods come out. I appreciate the feedback so far.
 

Rick Finsta

Stainless
Joined
Sep 27, 2017
I use the same inserted Seco high feed series as tony posted above.

Here is dialing in a 1.25" diameter unit in A36. I ended up at 1550SFM and 430ipm and the chips were still dark straw so I probably have another few hundred rpm left to go.

Login • Instagram

I've got a 2" deep bore video somewhere at the final speed and feed but evidently never uploaded it on IG.
 








 
Top