best process for this tapered cylinder (cone) - taper mill? form tool? ???

Working on an aluminum heating block for pcr-tubes (think genetic sampling machine) It's a rush project.
I made first few using an endmill tilted over while spinning on the rotary of my 5-axis machine.
That works of course, but if this succeeds they'll want first a lot of them and then a WHOLE lot of them, and so doing them one piece at a time on a 5-axis machine isn't ideal.

The key shape is attached - a small tapered bore with a hemispherical end. (There's also a cross hole not shown here, other irrelvent features.)

Hopefully that drawing gets big for you all when you click on it.

Key numbers - only 0.271" wide at the top, 0.519" deep for cone section, and an included angle of 17.3°. (No standard taper mill I've found.)

The material is 6061-T6 aluminum.

Is this a job for a form tool of some kind? Would a pre-drill be required? How to get the form tool to not chatter? (My only attempt to use one years ago did not end well - but I'm older and less stupid now...) Could such a form tool make the hemispherical bottom in the same op? Without choking?

Or is it better to have a custom angle taper-mill made, and circular interpolate to get the side angles?

Other milling process suggestions?

You can have a specific drill ground to this shape, you'll need a good tool grinding Co to make it with Al-specific flute/edge geometry. If you need a very good finish get at least two, one to rough, one to finish at a lower RPM and feed, but when developed you should be able to punch the holes very quickly.

I'm going to guess these are for virus testing purposes. Just a hunch...

yes. and while it's always a really worthwhile idea, well, it's obviously an even better idea right now...

I will look into the drilling idea...

bryan_machine said:

yes. and while it's always a really worthwhile idea, well, it's obviously an even better idea right now...

I will look into the drilling idea...

Click to expand...

Heh, three years at Harvard doing bioengineering support wasn't for naught.

My humble opinion - go with the drilling (and pseudo reaming if needed) method, a good carbide grinder should be able to give you tools that you can use at silly RPM for fast hole generation. And you have a legitimate right to plead "emergency speed" when requesting priority for getting these made.

If it helps, you can get a letter of purpose from the research group that you're working with, but just telling the grinder why you need cutters ASAP should be enough.

Schwanog recently got into the custom solid carbide round tool game, and I've used a couple form tools from them that have performed flawlessly, to the same standard you expect from them (If you're not in the threadwhirling game, Schwanog is TOP of the game for threadwhirling inserts). I'd recommend sending them an RFQ. You can either make a drawing of the tool you want, or just send them your drawing (They'll sign an NDA if necessary) and they'll design and tolerance the tool.

Hi bryan_machine:
If you are motivated to make your own tool for these, you can make a single lip D bit from a split blank you can buy commercially, or alternatively, you can use a piece of drill rod to make your tool and then just harden it.
Turn the shape on the end of the rod, split it on the mill, then harden it and stone relief on it under the microscope.
To get you out of the gate this is not a bad approach, but...
If You have to make a whole lot of these, making the cutters will get old awfully fast and if you need them to be consistently accurate, you will tear out your hair.
Also D bits need to be nursed into the cut...no driving the piss out of them.

For anything more than a few hundred of these, I second the idea of having 2 flute ball end customs ground up and also roughing drills.
I'd make the roughing drills as step drills to break up the tapered surface into a fine pitch staircase because there's a LOT less torque on the cutter so you can push it much harder and get the bulk of the meat out in seconds.
Resist the temptation to do this with one cutter in one pass...you'll likely have a mess of broken cutters littering the insides of your VMC and stuck in your workpiece.
The torque on a tapered cutter pounded into the solid is HUGE because of the large surface area that's engaged with the cutter flutes at the bottom of the stroke, and if it grabs just once...

BTW; I like the idea of tilting over the 5 axis mill, spinning the C axis, and driving in a standard ball cutter to get you going.
That's a cool, clever way to go about it.

Also if you consider doing them on the lathe, you can just peck a standard ball cutter in using it as a drill, then back it out on the angle and it'll make that tapered well in seconds.
.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Hi Marcus,
This is the "one in a million" time that I'll disagree with you. The material is easy to drill, the depth is not that great, and the geometry is inherently strong, all leading me to think that a modified drill design is a better choice than a modded ball endmill.

I would want a tip and core that's oriented towards plunge cutting (drilling), as opposed to a ball endmill design that's usually more optimized for bending stiffness and uniform core geometry. A good cutter grinder should be able to produce a tapered core, split or "S" point drill shape with a helix that gives free flow for the chips.

A "D" drill would only be my emergency (and short term) option, it's not great for Al and would require a coolant channel and TSC to have a chance at decent chip removal.

Hi Milland:
I think we actually agree on most of it.
I fully concur that a D bit is a non starter for production.
I also agree that drilling for roughing the shape is the fastest, safest way forward and I like a multi step drill with many small steps, so you can still feed it like a drill without fear.

Where we maybe differ a bit is in the finishing cutter.
As soon as the sidewall is tapered, the sides of the cutter need relief so the geometry is essentially that of a tapered ball end mill.
The aggressiveness of the relief determines its propensity to chatter and grab, so, much like a countersink, the relief has to be small.
This makes it a good taper reamer but a crappy tapered end mill.
Putting a helix on it is a good idea, but I'd make it a left hand helix like a taper pin or sprue roughing reamer.

I fully agree that if it can be made with through tool coolant that would be a major bonus.
Last, the ball diameter is only 0.11142" so it's still fairly small.
Granted the taper is quite big so it is still pretty robust as taper reamers go, but I'd still be puckering my sphincter pretty good if I tried to plunge it into the solid at any respectable feedrate.
With a step drill I'd have no fear whatsoever.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

You might ask if it would be a good option, because it will be faster, to use a 9 degree per side tapered end mill from Harvey tool or elsewhere. We make thermal cycler blocks and related components quite frequently and this does work. The difference between 17.5 degrees, which seems to be a de-facto standard for skirted PCR plates, and 18 degree is only about .003" per side at .52" up the cone. You also press the PCR plate on the thermal cycler block and take the thing to near 100C for PCR, so the whole polypropylene plate gets pretty soft and I'm sure will conform a bit to the shape of the aluminum. So I'd suggest the 9 degree per side option.

Harvey Tapered End Mills: Harvey Tool - Miniature End Mills – Square Tapered Rib Cutters