PDA

View Full Version : Need Help Drilling Thru Holes in Brass Balls



dharnell
04-08-2009, 09:49 PM
I may have a project that requires me to drill and ream a 0.250" hole through approx 100 0.750" diameter brass balls on a regular basis. I would like to use my lathe and a 5C or ER collet chuck or lever collet to hold the balls and drill them. I don't have a collet chuck for my lathe currently, but may purchase one if this seems feasable. I'm hoping someone may have tried this before and can tell me if it would work before I purchase one.

Would the balls spin in the collet, or pull out when the reamer or drill is retracted? When finished the balls can't have any marks on the surface.

I also thought of using soft jaws on my 3 jaw chuck to hold the balls, but the thought of opening and closing the chuck by hand seems tedious.

Any other ideas?

Thanks,

Dave

fishfrnzy
04-08-2009, 10:28 PM
First off not having tried this, I believe the collet or the chuck will leave marks when you grab with sufficient force to hold while drilling and reaming. I would probably use a 1" collet with a sleeve like a plastic shotgun wad with a groove on the ID to get more contact with the ball. Bore the plastic at say .688 dia, Put a hole in the back to push them out with a dowel and three radial slits to make putting them in easy. Dnt' know much about plastics. I think nylon and delrin would be to slippery but there should be something that would work.

wierdscience
04-08-2009, 10:28 PM
A lever style collet closer in 5C will work fine.A collet stop will help backup the thrust produced by drilling.Done a bunch of PTFE 1/2" balls that way and they were slippery little suckers,brass should clamp much better.

barts
04-08-2009, 10:30 PM
I'd use a soft collet and machine a pocket to hold the ball w/ form cutter, ball turner or ball end mill held in toolpost... drill through collet to form clearance for drill and reamer, of course...

If collet marks up the balls (unlikely), open up the hole and line it w/ babbitt or solder and remachine pocket.

- Bart

jimsehr
04-08-2009, 10:31 PM
I have drilled balls in 5c collets and had no finish problems. I would use a emergency 5c collet and bore it about .450 deep to a shoulder so that the balls have a stop. That will make it easy to load and unload them.
Jim

tony ennis
04-08-2009, 10:32 PM
This reminds of a telescope mount Evan made...

jimsehr
04-08-2009, 10:50 PM
http://i86.photobucket.com/albums/k106/jims_03/IMG_0001-2-1.jpg

1 inch steel Ball, I made with my ball turner then held in a 5c collet to blend the cut off part round. Jim

Mcgyver
04-09-2009, 12:15 AM
for job like this, if you don't need 10ths accuracy of a high end collet, make a cylinder maybe an inch long with the ID = the ball dia (and to a good finish) and the OD maybe 3/16 - 1/4 bigger. stamp the position of jaw 1 in the three jaw when you finish the bore. slit lengthwise with a hacksaw and it will hold the ball in the three jaw. since its to hold a ball you could leave a slight internal shoulder at the bottom of the bore so - this will stop drilling pressure from moving the work in the direction of the lathe's axis

whether you mark it or not depends on how much pressure you apply, but with the drill properly ground for brass (brass takes next to no cutting force) i think you'd be ok. I bet you'd find it didn't need much clamping force if you drilled slowly and used the internal shoulder idea. consider making it of AL to further reduce the chance of marring the ball

oldtiffie
04-09-2009, 02:43 AM
Use aluminium soft jaws in a 3-jaw chuck (needs removable front face of jaws) - drill 7/8", bore 1" x depth to suit as counter-bore. Aluminium will not mar the ball surface.

Have enough space between jaws when closed to hook or flick the ball out.

If I were really "flash" I would bore the hole as a 90 degree "V" (as in a V-block) to suit the ball so as to provide two location surfaces (axial) as well as 6 radial gripping surfaces. Sure, you need to open and close more than a plain bore but there is twice the gripping and a positive location both axially and radially.

I'd drill and bore that hole before I reamed it. If it is going to slip at all it will most likely happen when reaming. Also use zero ("flat") top rake on the drills and boring tool.

DO NOT stop the lathe when reaming; DO NOT stop the reamer when reaming - just straight in and out and NEVER reverse the lathe while the reamer is in the hole.

Don Wojtaszek
04-09-2009, 03:55 AM
Dave,

I had to drill and tap holes in aluminum balls in a lathe, and was afraid to scratch them up using a 3 jaw or collets. What I did was get a ball mill and cut out a pocket in some vinyl rod I had, then use that in the 3 jaw to hold them while I drilled. The ball mill gave me a curved pocket to better grip the balls with, and I did not get any slippage. Depending on the thickness of the vinyl or whatever you use, three cuts in it may be needed to get the 3 jaw chuck to give you enough force to hold the balls.

Good luck!

Don

oldtiffie
04-09-2009, 06:35 AM
If chucking and un-chucking the ball in the head-stock is tedious, then centre-drilling, drilling, boring and reaming is going to bore you $hitless.

As you have the chance of more of this, then I suggest that you get a 4-stage/step/indexing accurate relocating quick change tool post. Make/get four adaptors, at a single set position (locked) on the cross-slide, drill/bore/ream and incorporate a clamp as required in each in turn for:
- centre-drill;
- 15/64" or 7/32" drill;
- boring bar - or "D" bit (set for pre-reaming -say 0.240"); and
- 1/4" (0.250") machine reamer.

Combine this with the "V"-ed soft jaws as previously and using one chucking operation, and without stopping the lathe spindle (other than perhaps for reaming) , and the lathe carriage hand and power feeds (with the cross-slide and top-slide locked/clamped) centre-drill; index; drill; index; bore or "D" bit; index; ream; index to start (centre-drill position); stop lathe; un-chuck finished ball; chuck new ball; re-commence cycle again etc.

In other words, use your lathe as a turret/capstan lathe - and forget about the tail-stock.

If the centre-drill cuts a hole just larger than 1/4" there will be no need to de-burr that end of the hole.

To de-bur the other end, put a short length (1/2">5/8") of 1/4" rod in your pedestal drill vise, centre it under your drill quill, clamp the vise to the table, put an old centre-drill (without the guide spigot) - note: the centre-drill has zero rake as required - hold the ball by hand or with soft-jaw pliers/"multi-grips" - or other to suit, place ball on spigot, non-de-burred end of hole upward, start drill and use centre-drill to de-burr second end - no need to stop the drill.

Job done.

And then you will be bored $hitless again - wondering how to fill in all the time you saved.

If it were me and I had more to do, I'd buy a new tool-post and set it up as previously, remove it when finished for other work and then just re-mount it and re-set it to centre as previously - and away you go.

If things are really going well, do the same with a new chuck wit soft-jaws mounted 0 just for that job.

Then more money, more time, more boredom.

What a worry!!

Evan
04-09-2009, 07:15 AM
I recently ordered some high quality 1/8" solid carbide drill bits that were on clearance from Thomas Skinner. The other day I needed to enlarge a dremel style brass collet from 1/16 to 1/8. I tried chucking one up with the split jaws held in the chuck jaws and drilling it with a new, regular HSS bit. This did not work as it tore off the jaws on the collet. I decided to try one of the new carbide drill bits as they are the sharpest drill bits I have ever seen in my life.

I was able to cleanly drill through a brass collet with no support for the collet jaws at all. The bit is so sharp that there is almost no cutting force imparted to the work. These same drill bits will, in a hand drill, drill through 1/2" mild steel in 9 seconds.

Using such a drill bit will minimize the holding force required. It also reduces the tendency for the bit to grab and screw it's way into the brass. It also cuts very close to size because of the low cutting forces and the precision of the tool. You didn't specify any tolerance but a good quality carbide bit will drill a hole to within .001 of nominal size. Since a 1/4" bit is normally sized at 0.249" it will be nearly dead on 0.250 and may eliminate the need to ream.

For holding I would make a collet from Delrin or acetal or Nylon that fits in the three jaw. If the balls are polished then any metal contact will probably leave some visible mark. It will also depend a lot on whether the brass is hard or not.

loose nut
04-09-2009, 06:59 PM
Do you drill them before or after you get them off the monkey!!!

dharnell
04-09-2009, 07:10 PM
Thanks, for all the replies. After reading the replies I think this is a doable job with a 5C collet closer on my lathe. I been doing some research and if I get the job, I think I'll try a pneumatic 5C collet closer and some combination of a collet or pot collet. For tooling I think I'll try the turret tool post, would work well I think.
The quantity of balls to drill has increased also, they now plan 6000 pcs a year.

Dave

Spin Doctor
04-09-2009, 07:22 PM
For that many I'd think really hard about one of these

http://cgi.ebay.com/SuperTec-Model-STL-59-Quick-Acting-Turret-Lathe-1984_W0QQitemZ170317691604QQcmdZViewItemQQptZBI_La thes?hash=item170317691604&_trksid=p3286.c0.m14&_trkparms=72%3A1205%7C66%3A2%7C65%3A12%7C39%3A1%7C 240%3A1318%7C301%3A1%7C293%3A1%7C294%3A50

Liger Zero
04-09-2009, 08:01 PM
. Dnt' know much about plastics. I think nylon and delrin would be to slippery but there should be something that would work.

I visualized something similar to your setup but replace the plastic with a piece of rubber.

Liger Zero
04-09-2009, 08:05 PM
Do you drill them before or after you get them off the monkey!!!

And what pray tell do you do with that many monkeys after?!:eek: :D

lane
04-09-2009, 08:41 PM
The fast way to drill and ream is in a mill. Make 2 soft jaws for your vise . close jaws with a shim about 1/4 thick in them and drill a hole 1/2 in both jaws and deep enough so 1/4 of the ball sticks up above jaws. insert ball close vise jaw . Indicate spindle over center of ball ,indicating the top radius sticking up above vise .Lock table in all axis . now drill and ream ,open jaw take ball out drop in another and go again . Nothing faster. Twice as fast as in the lathe.

wierdscience
04-09-2009, 09:04 PM
Lane has a point,a quill is faster than a tailstock barrel.

Consider too that those Eagle air 5-C collet fixtures are on sale regular.

http://www1.mscdirect.com/CGI/NNSRIT?PMPXNO=1796282&PMT4NO=0

Evan
04-09-2009, 09:11 PM
I agree with Lane except for one point. Since these are presumably round balls then the orientation for drilling doesn't matter. All you need is a slightly tapered cone with some sort of ejector at the bottom, perhaps lever operated. The pressure of the tool will sieze the ball in the cone which can be made of plastic or perhaps even better a really hard wood, say for instance Jatoba. :D Make the cone about twice a deep as the ball requires so it will wear gracefully.


Still thinking about this. A pair of flat rectangular plates placed at maybe a 5 degree angle to each other with vee grooves appropriately spaced will do the same thing, will be easier to eject and can hold a group of parts at a convenient spacing to drill in sequence before reloading. Make the spacing an even number of turns of the crank.

oldtiffie
04-09-2009, 09:48 PM
I may have a project that requires me to drill and ream a 0.250" hole through approx 100 0.750" diameter brass balls on a regular basis. I would like to use my lathe and a 5C or ER collet chuck or lever collet to hold the balls and drill them. I don't have a collet chuck for my lathe currently, but may purchase one if this seems feasable. I'm hoping someone may have tried this before and can tell me if it would work before I purchase one.

Would the balls spin in the collet, or pull out when the reamer or drill is retracted? When finished the balls can't have any marks on the surface.

I also thought of using soft jaws on my 3 jaw chuck to hold the balls, but the thought of opening and closing the chuck by hand seems tedious.

Any other ideas?

Thanks,

Dave

The OP (Dave) said he preferred to use his lathe. He did not mention a mill.

While I generally agree with Lane, I would say that tool changes are needed. Hooking the ball out of the vise may not be all that easy either.

I made no mention of using the lathe tail-stock, in fact I suggested ignoring and not using it.

A quick-change 4-station rapid accurate turret tool post requires no tool changes nor does it require the lathe to be stopped - other than perhaps for reaming.

Soft jaws are about as good a grip and location as you can get.

The ball needs to be at least half its diameter into the collets if used and that may be a problem to extract the the ball - a magnet is no help as the ball is brass. The ball has to be held in place as the collets are tightened whereas the ball will self-locate in the "V"-groove in the soft jaws.

It is the OP's choice after all.

lane
04-09-2009, 09:59 PM
I for got to say . the reason for boring the hole with the shim in the vise is so when tight on the ball their is a gap between both jaws. Slide a thin piece of stock are a scale under ball and pop out . the drill point will give you the cone Evan was talking about . And as far as tool change only 2 required . 35 drill point self centering and drill quick change chuck insert reamer .Albrecht type.
I figured he did not know he could do that in a mill.

Mcgyver
04-09-2009, 10:29 PM
I I figured he did not know he could do that in a mill.

i didn't know he had a mill :)

first reaction was yeah the mill would be quick, and it would be for the part changing so part would be power down/up for the tool change....with a tailstock cheapo turret, or even just swapping in the drill chuck, you're finishing each part without a tool change requiring the spindle to wind do/up - as all ops need doing in one set up as you won't be able to reorient it. hmmm, is it quicker buttoning the shirt up or down :D

japcas
04-10-2009, 08:42 AM
I agree with the tailstock turret. You don't have to wait on the spindle to start and stop for each tool change. Just stop the spindle when changing parts. Drill, ream, and then change the part out. Repeat. Better hire some cheap help to deburr the holes when your done.

Evan
04-10-2009, 08:54 AM
Tool change??? What tool change? No way you can make money if you have to change tooling each part.

Regardless of what machine is used this job calls for a combination drill bit/reamer.




MSC #: 02535169
Price: $31.45 ea
In stock: 52
Mfr: Made in USA

Description: HSS 118 Combination Drill-Reamers Size: 1/4 Reamer Diameter: 0.2500 In. Flute Length: 2-15/16 Overall Length: 4-1/8 Material: HSS


Or, use a carbide bit as I described.

dharnell
04-10-2009, 10:48 AM
Hi, thanks again for all the replies. A lot of ideas have been posted, have to sit down and do some thinking about this some more. I guess some background on the potential project would clarify the situation.

I've been asked by my employer as he knows I do machining on the side, if I could machine a small part that is comprised of a few simple components. If I get the job it would mean my shop would actually start paying for itself, that would be a change! I have a First 9"x42" vertical mill, a DS&G 13"x42" lathe, as well as a surface grinder and other ancillary tools. I was hoping to be doing other operations in my mill while my assistant(wife) ran the lathe.

That's why I thought a pneumatic collet closer and an indexable tool holder would work well. I was hoping that I would be ale to mount a bar tipped with nylon and left in the head stock to pop the balls out(possibly driven by a small air cylinder?). Would be fairly simply to operate.

I may have to rethink this whole thing out. I like the idea of the combination drill/reamer, it would eliminate one step.

Thanks again for the help!

Dave

jimsehr
04-10-2009, 04:54 PM
This is on a Logan .


http://s86.photobucket.com/albums/k106/jims_03/?action=view&current=33a2fec1.flv

dharnell
04-10-2009, 09:42 PM
Jimsher, was that done on your lathe? If so, how were you getting the balls to drop out of the collet?

Thanks,

Dave

oldtiffie
04-10-2009, 10:07 PM
Back to the OP:


Originally Posted by dharnell
I may have a project that requires me to drill and ream a 0.250" hole through approx 100 0.750" diameter brass balls on a regular basis. I would like to use my lathe and a 5C or ER collet chuck or lever collet to hold the balls and drill them. I don't have a collet chuck for my lathe currently, but may purchase one if this seems feasible. I'm hoping someone may have tried this before and can tell me if it would work before I purchase one.

Would the balls spin in the collet, or pull out when the reamer or drill is retracted? When finished the balls can't have any marks on the surface.

I also thought of using soft jaws on my 3 jaw chuck to hold the balls, but the thought of opening and closing the chuck by hand seems tedious.

Any other ideas?

Thanks,

Dave

In the OP (re-posted above with my emphasis), the OP clearly says that:
When finished the balls can't have any marks on the surface.

This rather suggests that as it is more than likely that what-ever holding method is used, that there will be some cuttings/swarf/residue left in what-ever the holding medium is (chuck, collet, vise etc.).

This being the case, prudence would require that the holding medium be cleaned out by hand - cloth/rag or air-blast? - at the end of each cycle so that following cycles did not mark the balls that follow.

The "no-marking" criteria also applies to there being no marking by the clamping medium as well - chuck, collet, vise etc.

I would guess that the balls as supplied will not only have a good finish when they arrive but will need to have it maintained until they are taken delivery of by the client.

Damaging/marking the balls before or after machining might be problem as well. I can't see that requirement being met if the balls are just dropped into the machine well or a bucket etc.

I'd imaging that de-burring will be a requirement as well.

jimsehr
04-10-2009, 10:28 PM
I used a stop in the collet and if you listen to the sound on the vid you will hear a tapping sound every time I opened the collet and pulled the handle to
the front that tap is enought to pop the ball out. I did not stop the machine
as I loaded them and I don't think the finish will be harmed by loading them while running spindle. If so then you would have to stop spindle to unload
parts. If you use an emergency 5c collet I would drill a 3/8 hole thru and chamfer edge about .100 where ball stops to protect finish.
To break edges on front and back of ball I would goggle Cogsdill or ezburr.com and get a special deburr tool that will do that.
And you might try a high performance parabolic screw machine drill with a split point. Guhring drills can penetrate up to 15 times the drill dia without flute
clogging . They almost throw the brass chips out of the hole.
Jim

dharnell
04-11-2009, 09:56 AM
Oldtiffie is correct. The part being machinied is part of a custom ball valve assembly. Thus the requirements for no marks on the ball surface. Jimsehr, it looks like you were using a lever actuated collet closer. Are you saying that when you actuated the lever, the collet stop popped the ball out, or was it simple the act of opening the collet closer?

I'm going to have to make 5 prototypes this week. I'm thinking that for the 5 I'll drill on the mill and try some of the different drill bits members have been talking about.

Thanks again everyone.

Dave

Evan
04-11-2009, 10:51 AM
If it is for a ball valve then the requirement is really that there be no marks in the seal seating area, not necessarily the entire ball. You should negotiate with the customer and his engineering department to see if you can modify the requirement to a more detailed specification of what zone must remain pristine and what zone may have minor scuffing, if any. It might save you a lot of time and you can offer him the same carrot by lowering your quote if they are willing and able to relax the requirement in that regard. It will depend on the type of ball valve.

JCHannum
04-11-2009, 11:21 AM
Generally, a ball valve seal will encompass a large part of the ball's surface area. In this case, it is a 3/4" ball with a 1/4" thru hole, which leaves little room.

Questioning or asking for relaxed standards can cause a potential customer to believe you have qualms about meeting them and can lead to them looking elsewhere for a suppiler. It is best to make every attempt to meet their requirements. In this case, it should not be too difficult using the suggestions posted. The potential quantities warrant purchasing and/or making the tooling to do the job properly.

Evan
04-11-2009, 12:18 PM
There are many type of ball valves including ones with limited motion. Offering the customer the possibility of a discount for more detailed specifications is hardly an admission of incompetence. The customer should be providing a detailed drawing indicating what areas must be free of marks, including the entire surface if that is the actual requirement. A good engineer will recognize that is a more expensive requirement than restricting the condition to the zones that matter, if possible. You can't "make it like the print" if you don't have one.

jimsehr
04-11-2009, 01:10 PM
I have not used one but MSC has 5c emergency nylon collets.
# 09744277 $13.95
Jim
I think a regular emergency will work. I am tempted to go out to the garage and make a brass ball just to try it out.

dharnell
I was using a lever actuated closer and the balls popped out when I opened the closer. You have to kind of tap the
handle to get parts out. I used to run thousands of parts in collets that I made ejecter stops for that would shoot the
parts out 4 to 6 inches when the collet was opened. It is simple to do with a 5c collet. If you want I will make a sketch
of how I did it.

dharnell
04-11-2009, 03:17 PM
Jim, a sketch would be really appreciated.

Dave

jimsehr
04-11-2009, 11:50 PM
I made a guick spring stop . I found that 3/4 inch pvc pipe just fit in my collet
tube and it can be threaded to fit the thread inside the collet. I then used a3/4 nylon tube for the ejector stop. I did not thread the pvc as I have no leadscrew on my lathe . So I just turned it about .01 larger then the thread minor and force screwed it in by hand. If I had a leadscrew I would have cut the thread. I found a spring that went over 3/4 dia but needed a stop for the spring so I bored a washer to .730 and turned the 3/4 tube to .730 part way so I could have a shoulder for spring to push . I used a nylon tube so that
after drilling the tube could be cleared of chips with a shot of air. Then I drilled and tapped a 1/4 20 hole thru pvc pipe and put a 5/16 slot in nylon tube to stop it from springing too far out of collet. If dharnell wants the stop
he can have it for the asking.
Jim



http://s86.photobucket.com/albums/k106/jims_03/?action=view&current=27f0340e.flv

jimsehr
04-12-2009, 12:07 AM
http://i86.photobucket.com/albums/k106/jims_03/P1050454.jpg

Sketch of spring stop