How to make 10mm hemispherical cavity?

Hi guys,

I'm looking at this part, in 1018, quantity several hundred. The cavity terminates with a 10mm hemisphere:



Boring bar interferes with the "other side" trying to finish the hemisphere.
Standard face grooving tools do not have a radiused end relief and will interfere (yes, I can hand-grind the relief, but I would prefer a grab-and-go tool).

What else might work? I thought about plunging a 10mm ball endmill .

Thanks for your ideas, and regards.

Mike

Ive used a touch smaller ball end mill as a boring bar. Drill to clear the bulk of material and then to the ball end mill. Id say an 8mm ball end mill for the 10mm radius?

Man thats small to be trying to turn that. If you can get the finish requirements out of a ball that might be the way you have to go? The thing about doing a ball not only do the backside to worry about but the underneath too. Almost need a pointed tool pointed forward at just a slight angle. But you already know this. lol...

I can't say if I've ever saw an off the shelf tool for that. I'll be keeping a close on this thread to see if someone has a idea for a turning tool for this.

The guy in post 2 has a very good idea!

Good luck...

Brent

If you can't do what Wade C suggested a 10mm BE 2 flute will work a treat, - again, I'd drill a 3/8 ''starter hole'' to a few thou short of depth first ;- it's much kinder to the BN / EM.

Purpose-ground form tool? IMO, that's so similar to the ball end mill, I'd just use 3/8".

I might be tempted to forge that...but that's cheating.

Seen these?
ISCAR Cutting Tools - Metal Working Tools - MIFHR : 286 - MIFHR 8SC-8-SRK
ISCAR Cutting Tools - Metal Working Tools - MIFR : 6449 - MIFR 8-1.6-.8

There are off the shelf bars for boring hemispheres (SDXCR/L) but they all seem to start at 10mm shank for a 20mm hemisphere.

I looked through the solid micro bars from sandvik, horn and simtek to no avail.

Looks like off the shelf tools for such a small hemisphere are unavailable unfortunately.

If you plan on profiling the hemi with a ballnose rather than plunging you'll need a straight flute one. Dapra go down to 8mm with their blade type inserts:

It will be easy to make a simple, single lip cutting tool (basically a D bit) that will finish the cavity in one operation after drilling with undersized drill.

The question to ask is "Does the center of the cavity have to make contact with the ball?" A slight counterbore on center, maybe 3 or 4 mm in diameter would make the finish issues go away and....wait for it...it could hold some lubricant!

I'm going to reveal my secret technique for times when they say, "no tool marks at the bottom of the hemisphere." Weld a 10 mm ball bearing to a rod or tube. With the right copper cup, you can spot weld it without damage. Clean out the chips, put the bearing in the hole, support the part and apply a BFH to the end of the rod.

Hi finegrain:
I'm with those who recommend a ball nose endmill, but I'd do two things differently from those who've posted so far.
First, I'd use a significantly smaller ball than the size of the feature; say 1/4" diameter and interpolate the path.
Second I'd run it in a live station and essentially mill it on the lathe, using the spinning ball mill as if it were a single point tool.

Two reasons:
First you need room for the chips and milling it makes nice small ones that are easy to flush out.
The little chips also won't scarf up the finish like turning swarf will.

Second 1018 is shitty gummy material to turn but milling it with a live tool can give you nice finishes without pain once you get your speeds and feeds right.


It'll be no slower than turning it and it'll likely give you a better job with less pain.
Cheers

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

I've used 2 flute ball mills with a pre drill as close as possible to finish detail size
This was on annealed s7 in 1/8 - 1/2" pockets
A very slight dwell at the bottom of the pocket.
Just enough to get a couple revolutions before backing out

1/8 + 3/16 ball mills would last about 30-40 parts before getting dull

I would use a small (less than 5mm min bore) Boring Bar, with greater than 30º lead angle (if using a 118º drill point). I would drill close to diameter and depth. Then go in with the BB, start first pass at X zero, not drill diameter, take small roughing passes .25mm-.5mm. Then it will come out perfect. 4mm Min bore diameter Bar, with 16 or 20mm Max depth.

Assuming this is a Turning project, I didn't see anything to say different, except Marcus' post made me think this may be a Milling job??

R

Hi litlerob1:
Yep, this is a turning project judging by Finegrain mentioning a face grooving tool in his first post.
I just offered a weirdass alternative that I occasionally pull out when I've got oddball stuff to do that gives me fits if i try to tackle it conventionally.

I recommended it because 1018 is so shitty to turn; I find it almost impossible to get a nice finish especially when the surface speed gets really low like at the center of the hemisphere.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

litlerob1 said:

Assuming this is a Turning project, I didn't see anything to say different, except Marcus' post made me think this may be a Milling job??

Click to expand...

Yes, turning, so I can barfeed.

Regards.

Mike

implmex said:

Hi litlerob1:

I recommended it because 1018 is so shitty to turn; I find it almost impossible to get a nice finish especially when the surface speed gets really low like at the center of the hemisphere.

Click to expand...

True, True at max spindle speed it still isn't fast enough is it. @ 10mm I would be way past maximum already. But what I described is what I do when I need to be right at the bottom of a tricky hole, that doesn't allow a drill point. Anyway, you may proceed.

R

I made similar parts in 304 on a manual lathe. I plunged a ball endmill and it worked really good. Better than I expected. I pre-drilled the first one then I tried it without a hole. It worked better without a pilot- having the center buried seemed to stabilize the endmill. This was with a 7/8 carbide 2 flute at about 300 RPM.

Finegrain said:

quantity several hundred. The cavity terminates with a 10mm hemisphere

Click to expand...

hello finegrain

tool 3 :
... desired radius + z>=2
... good to have : a bit of conicity + short as posible + maybe coolant through
... short straight flutes ( cheaper )
tool 2 :
... tool 3 scaled down, so to make life easier for tool 3
... longer flutes
tool 1 : normal drill, so make life easier for tool 2

tool 3 should never cut more than 0.2 - 0.5 mm
tool 3 should last for long time, delivering nice finish surface, at high specs

tool 2 is doing the dirty work this tool may have the profile not exactly a full radius, but a bit changed, so to handle cutting forces better; it is roughing less than tool 1, but it should cost more than tool 1, so it is necessary to make it last much longer than tool 1

tools 3&2 should rotate (live holder), so to deliver a smoother cutting and avoid main spindle stress because of high rpm

it may be possible to eliminate tool 2; in this case, tool 3 will cut more, so a bit of profile deviation from the full radius may help

if tool3 is not coaxial with the spindle, or if coaxiality can not be maintained, than is no longer possible to finish the part; this makes it hard to get setup stability using only Z axis + tools with active diameter = nominal diameter; alternatives :

1) reduce tool3 diameter and :
... it should work just like that on the M axis, or
... interpolate, or
... use it as a turning tool
... use it with a 2nd tool that will finish the center, etc

2) reduce tool 3 diameter and compensate for coaxial errors using an excentrical adjustement holder inside a live holder ( attached ) :
http://www.ews-tools.de/upload/pdf/flyer/ews_flyer_flexicenter_en.pdf
EWS.Centerpoint und EWS.Flexicenter - YouTube
* that girl is the boss daughter or something, and the music ( kind of new era theme ) from the video is way too much only for this

3) turning should be considered for finishing, because turning is less coaxiality demanding ( kyocera tool attached ); however, on small tools, especially for those that must deliver bottom radius, Y excentricity may be tricky; Y excentricity fine adjustments on lathes without Y, may be an interesting discussion but such small tools are not cheap, so Y exc. adjustemnt can wait

ps : i guess these are normal : tolerances, rugozity, control method / have a good day

Wade C said:

Ive used a touch smaller ball end mill as a boring bar. Drill to clear the bulk of material and then to the ball end mill. Id say an 8mm ball end mill for the 10mm radius?

Click to expand...

I have done this on a few occasions successfully on a manual machine. It worked for me.