2 flute or 4 flute

[phaxtris]

Working on a project to add secondary plugs to vw cylinder heads, im trying to figure out the best way to cut through the cooling fins in order to make a spark plug seating surface, and clearance for the plug socket. The simplest way i have been able to figure is the biggest endmill i can run, 22mm, plunge through the path of the drill bit to make the seat, and clearance all in 1.

Question is, 2 or 4 flute endmill ? i know the normal answer is 2 for aluminum, but im wondering if thats the best choice here, given the size of endmill there is lots of room for chips, and the interrupted cut through the fins might be problematic with 2 flutes. Thoughts ?

I have found 22mm in 2 and 4 flute for 26$ ea (HSS), i could buy both, but i would rather not, what the heck am i going to use a 22mm hss endmill for beyond this

 

[RobinHood]

Use a boring head and work your way out to 22mm?

If the geometry is right, the face can cut clearance for the side of the cutter to follow. That way it would be possible to use a 1/2” or even 3/4” tool in the BH for extra rigidity.

 

[Proxule]

3 flute ?

 

[PeterT]

I like these high relief angle EM's for aluminum. I don't let them taste steel.

There are some funky new styles now I may have to try just for the heck of it

But back to your project, I think an annular cutter would be better. It has proper clearance for plunging deep. Radial teeth vs a cross diameter cutting surface, so more efficient cutting & should also help with irregular breakthrough of the fins, especially at an angle. They make pretty good finished cuts but better yet do a pilot bore followed by boring head.
BTW I just received a 2" long (50mm) annular cutter with carbide teeth for about same price or lower as the cobalt/HSS. It fits my tooling shanks perfectly. I haven't tried it yet but its razor sharp.

I think VW cases are a magnesium alloy but I'm not sure if that's a gummer or harder than typical structural aluminum. A shop I worked in as a teenager always drilled out the threads for cylinder hold down studs & replaced with something stronger, but maybe that was a thread specific thing.

 

[phaxtris]

There are a few clearance and reach issues that may not have been apparent, ill post some more photos. I also need a flat sealing surface at the bottom of the bore for the spark plug washer. The cylinder heads are cast aluminum, only the cases are magnesium.

I did think of the boring head, but I dont have a tool long enough for the reach, and i think i would have to set the bore multiple times ? i dont have one of those facing boring heads, just the regular china special, grinding the cutter square to make the seat would i assume chatter like crazy ?

I also thought about an annular cutter, but i would need to break the fins off, and then i still need that flat sealing surface, either i would need to buy a plug seat cutter, or a long reach endmill, or do something with the boring head

The endmills i have found are 141 long, I haven't come across a 3 flute cutter that long with a 22mm diameter yet, however the search is not over

My reasoning behind the big endmill was that it would cut the seat and bore the clearance all in 1 operation, 1 tool, rigid, not overly expensive. there was also a thought to use that annular cutter idea with some sort of home made facing fly cutter....but im unsure if that would be worth the effort, probably chatter city, and 2 operations over 1

 

[Mike R]

I think you'll find out that the 22mm cutter won't make a nice 22mm seat. Its going to move all around on you and wallow out the seat to something other than 22mm and round, especially at that distance.

 

[phaxtris]

It doesn't have to be perfectly 22mm, or even round, just flat and perpendicular to the plug bore

The only reason for 22mm is for socket clearance

Another thought if the seat is garbage that way would be a piloted counterbore bit

Or maybe bore the majority out with a 3/4 drill bit, then finish the rest up with ? Annular cutter? big endmill?

 

[PeterT]

Ah, I get it now. I thought it was just making a big through hole with a challenging path. Maybe more like a piloted counterbore but probably a longer shank? I doubt these would be long enough in stock form, but maybe some kind of extension could be fabricated as long as it had proper clearance. (BTW you probably know but end mills are not necessarily square cutting or square corners depending on the style).

I've seen another style of tool where it has a cutting head that slipped over a center shaft & fixed with set screws or something like that. Kind of like a valve seat tool but more aggressive cutting & chip clearance. Maybe used carbide insert(s)? Cant seem to find a picture. Maybe it had some tradename.

 

[phaxtris]

Yea I realize the face of an endmill is not perfectly flat, there is some relief angle, I don't know if that will be a problem or not. I had intended on using plugs that have a hollow crush washer so it may be fine, but I may also need to run a counterbore bit, I assume those are square, but I don't know for sure

The only bonus is with the counterbore it doesn't need to be 22mm, 18mm would be plenty, if I do need to go that route the question rises again, 2, 3, 4 flute ?

And with the larger diameter does the 2 flute rule of thumb still work ? The chip relief on a 2f 10mm cutter is x, but when you step up to say 20mm yours chip relief or distance between cutting edges triples, so should you then step up to 4f, I something I have never had to think about before

 

[PeterT]

If I had to guess, 2 flute EM might be marginally better based on deeper & wider gullets vs 4F from a swarf clearance perspective. More cutting surfaces might help a bit when you get to the interrupted break throughs but maybe not enough to warrant it. Just a gut feel, nothing more.

The bigger issue is EM's are mostly designed to cut chips with OD traversing laterally into/across metal. They are less efficient at axially plunging or at least at high Depth : Bore ratios in one go. I've found it beneficial (often necessary) to pre-drill a decent sized pilot hole say 50-75% of the EM diameter. The more pre-removal the better if the part allows, because the EM corner is doing 90% of the cutting work; the helical edges are more or less going along for the ride. If chip packing occurs, bad things can happen. So even so best to peck or withdraw often. Long depth drills actually have tricks in the grind to reduce friction & rubbing in the cutting surface behind the cutting tip whereas EM's are designed to be cylindrical body diameter. Sounds like you will have a pilot hole, so fingers crossed it will be sufficient if the diameter is dimensionally constrained by plug. If your bigger bore ID & bottom shape is a bit more tolerant, EM might work just fine. I've seen some people grind the shanks down so the cutting surface is relatively short (thus looking like those counterbore tools in #8 just no pilot stub) but that's getting into specialized grinding.

 

[Dan Dubeau]

TBH either would work fine for what you're doing (if you drill it first). If you can, I would drill out the majority, then plunge out the rest, running slow rpm with the EM as if you're running a boring head, not a drill. Traditional wisdom says the 2flutes are better for slotting/plunging, and especially with aluminum. But in practice you can pretty much run either if you feed accordingly (and they're both center cutting end mills). Especially if you first drill out the center. If a one and done is required, I'd go 2fl.

As stated above, both will leave a 1-3* taper on the seat, so that might be something to look out for. You could always sharpen one to a flat bottom too.

You could always make your own cutter here. A piece of hss (old tap/drill) held crossways through a hole in a suitable bar stock, and sharpened to the correct geometry would bore that hole to size (after drilled to clear the bar first). Alternatively, brazing a chunk of HSS or carbide onto bar would work too. Many way to make a cutting edge to do the job, but spending $26 is an easy way to buy time too. Also, a 7/8" dia S&D drill sharpened to a flat bottom would probably do the job just fine as well. Just spin it slow and keep the cutting edge loaded up and lubricated.

 

[phaxtris]

i tried with a 7/8 SD bit to hog the majority out, that worked ok, had to put it in a collet, and i think next time i might try stepping it up, maybe pilot to 1/2, to 3/4 then to 7/8, and maybe with a 135 deg bit. Followed that up with one of those BAP300 style indexable endmills to at least confirm how long of a bit i need to do the face, the relief on the inserts is to great for the sealing surface IMO, but at least i know how it will behave and how long of a bit i need, and show me what length of plug i need.

I think what may be the ticket is upsize to a 12mm plug, the standard available counter bore bits that have a big enough counter bore size require a 10.3mm pilot, so that knocks out the use of a 10mm plug, i could pilot the 10.3 from the combustion chamber side, flip the head, bore out with the SD bits and then either go in with a BAP endmill to clean up the bulk (i believe i have a big enough one for the counterbore) and follow up with the counterbore, and tap, or straight in with the counter bore and then tap. I may have to drill a second time, as a 12x1.25 should use a 10.75 hole....but im willing to bet i could run the tap through that slight undersize in aluminum

the only thing with that plan is i will need to make an extension, i dont see any counterbore bits the right size with enough of a shank (from face i would need at least 120mm to use without an extension). Possibly make it out of cold rolled with an interference fit and a couple set screws for good measure ? ive never made an extension for an endmill

 

[jorogi]

So I know what would end up biting me in the ass so I just have to say it. Your 22mm diameter is clearance for the plug socket not the plug, right. OK I'll shut up now and go back to my room.

 

[phaxtris]

So I know what would end up biting me in the ass so I just have to say it. Your 22mm diameter is clearance for the plug socket not the plug, right. OK I'll shut up now and go back to my room.

yea plug socket, i think the thinnest socket i could find on the net was 20.4mm, 22mm seemed to be the next size endmill after 20, the plug and sealing surface really needs to be 16mm. The counter bore bits i can find are 17mm, so that gives a little extra (1.5mm ish depending on manufacturing tolerance of the plug body)

 

[PeterT]

This is what I was trying to remember - Spade Drill (aka Violence Drill lol). Expensive in N-Am but not too bad on Ali. I thought they were longer depth but I also didn't search too hard. This 22mm dia is 66mm DOC. Might be able to forego the Weldon style holder with R8 collet. Some stores offer packages of inserts as a bundle deal. That doesn't solve the flat bottoming operation, but some good ideas were mentioned.

 

[David]

A person has to ask what a Violence Drill is... and pray my dentist never gets one!