What's new
What's new

How to: presize bushing with tiny inner hole concentric with OD

kiriba-ru

Plastic
Joined
Sep 24, 2018
Hi,

I need some steel bushings that should have 11mm lenght, 6mm OD, 1mm ID, OD and ID centers can missmatch not more than 0.03mm.
Which way I will get most close results?
Using lathe and turning from rod in one setup looks most easy way, but:
- tailstock center height is never aligned with spindle center
- even if drill will find center on the face surface, just wonder how far from center it will exit at the back surface.
I can also use manual mill to make hole (after OD is done with lathe). Indicating center with OD will be easy, can use smaller drill first and proper size mill to finish hole. But:
- 1mm mills is probably more rigid than 1mm drill, but anyway it will have reasonable deflection with 11mm length.
So, if making small hole concentric to the OD is so hard, maybe I need to reverse operations?
Drill smaller hole, finish it with reamer, and then use tool grinder with 1mm arbor to finish OD? Does this looks realistic?

Thanks.
 
Chuck the rod in your lathe. Drill and ream the ID to finished size. Remove from the chuck. Place another piece of stock between centres and turn a mandrel to a light press fit, or a sliding fit with super glue. Then put your bushing on the mandrel and turn the ID concentric.

Hope this helps,

Lee

Sent from my SM-N960U using Tapatalk
 
I'd sooner attempt the job on the mill, where at least I've got proven tooling with minimal runout, compared to a lathe tailstock's unknown reliability of position. Also have the rpms available on the mill which are quite beyond most lathes.

Make one first and test it's concentricity. Then worry about improving it. My go to method for accurate holes is to drill first maybe .75mm in this case, then interpolate the top of the hole to 1mm to act as a guide for the reamer. Then ream it and test it.

I guess you could grind it on a mandrel, but that sounds like a PITA to do, so I'd try anything else first.
 
I'm missing something here. OP needs to make an 11mm long bushing with concentric bore that deviates not more than 0.001" end to end. That's not especially close tolerance - why does it need to be ground, and why can't he use the lathe he already has? I don't think he said anything about the lathe's condition, but even a very worn lathe should be able to pull that off with some care?

Sent from my SM-N960U using Tapatalk
 
Im not familiar with watchmakers technologies, when I take 0.7mm drill it seems to deflect after each breath.
Even if there are some ways to setup tailstock (or chuck in toolholder) with this tolerance to the spindle center, I have no ideas how drill will deflect during drilling and how far away from this perfect center it will get out.
I dont see how smaller or more precise lathe can help. Unless you have nano boring bar that is able to bore 1mm hole.
Turning OD hold on 1mm mandrel looks crazy for me. Even if part wont fly away, mandrel will bent and bushing will have cone shape after turning.
So, I suppose that making ID before OD can be more easy (Im not able to bore 1mm with boring bar or boring head), but OD should be finished with lower force operation (grinding).
So, if I have roughed OD and have made 1mm hole (with any technic), I need to use this hole as reference. Mandrel with some threadlocker/glue is one option. 60 degree chamfer (for dead center) is another option. (I can leave extra length and face this chamfers after OD is done). Which way is preferable?
 
My first question would be what method/tools you're using to locate the ID hole before using a drill/end mill. If the lathe tailstock is out of alignment with the headstock then the hole will have to be put in with the mill. You will have to finish the OD on a machine that you feel will hold concentricity and that sounds like your grinder. Rough in the OD on the lathe, leaving .13mm on the OD and maybe 1.5mm on the overall length. A larger hole, for grinding arbor, can be put in on one side (4.5mm?). Put the bushing in the mill and drop the hole in. Starting the hole is critical for location, I've used a spotting drill and then an end mill depth at least 2X the cutter OD so the hole is sized/located and acts as a guide for the full sized drill. All cutting tools must be indicated for run-out in the mill spindle too. If the grinder has a tailstock for a center (dead or live) then perhaps a small chamfer can be put in on the other side to help locate/support the bushing while grinding. When the OD is ground to size and is concentric to the ID you simply toss the bushing back in the lathe and face off the extra length. Yes it's some wasted material and extra steps to go through but the conditions of your available machines and the tolerance you seek often dictate the methods used. You may have to adjust the roughing OD to leave enough material on there for the grinder to clean up. A test piece will show what needs to be done. Hope this helps.
 
Chuck the rod in your lathe. Drill and ream the ID to finished size. Remove from the chuck. Place another piece of stock between centres and turn a mandrel to a light press fit, or a sliding fit with super glue. Then put your bushing on the mandrel and turn the ID concentric.

Hope this helps,

Lee

Sent from my SM-N960U using Tapatalk

On a 1 mm (0.040'') diameter UNSUPPORTED mandrel / peg?
 
On a 1 mm (0.040'') diameter UNSUPPORTED mandrel / peg?
Yes, I realized after I posted that the mandrel would be tiny.

Could the piece be turned in the chuck, and the bore created with an center cutting endmill held in the toolpost?

Sent from my SM-N960U using Tapatalk
 
Yes, I realized after I posted that the mandrel would be tiny.

Could the piece be turned in the chuck, and the bore created with an center cutting endmill held in the toolpost?

Sent from my SM-N960U using Tapatalk

1mm dia @ 11 x d long? ………...I'm not saying it can't be done, but I wouldn't like to try it.
 
I have found that on a lathe to face and then tool bit nick the bore/hole location makes the best hold to center. Tail location and even poor drill point locating can mess up a spot-on center need. The tool bit nick will run true to the spindle, even with holding part in a poor chuck. ..the a part-off will make the other end good.

Facing,OD,Id and parting-off in one chucking make everything run true.

Carbide reamer might make /finish the bore..
https://drillsandcutters.com/1-00mm...ica/?msclkid=7e9f473a3cf31782e1111ab94f877d46

Q: [ and then use tool grinder with 1mm arbor to finish OD? Does this looks realistic?}
A very short arbor so less wheel pressure deflection.
I have set such parts between centers to skim OD for .001 and less run out with just using the part bore... with using a point center lap to make a small center in the part.
A AO Center Lap Mounted Point | Norton Abrasives
 
I need to mention that I have made bushings ("somehow") and it seems that none of the ways discussed here can guarantee a great result.
Feeding tiny drill or reamer with relatively giant quill without special attachment was not a good idea. Ended by broking some rare reamers.
Regular 2-flute centre drills and 4-flute countersink bits didn't want to follow center hole. Had to use a single lip carbide cutter.
Centers that seemed to have great shape don't look so anymore when you need sharp 1mm ends.
Probably next time I will pay for EDM services.
 
Turn OD finished accurately, drill under size, wire EDM a fixture to hold the OD and wire EDM the ID. Simple and accurate. I don't think a 1mm arbor is feasible , and any method of spot drilling, drilling and or reaming will need a bit of luck to hold tolerances consistently. ,
 
1mm dia @ 11 x d long? ………...I'm not saying it can't be done, but I wouldn't like to try it.

We regularly run carbide circuit board drills .028" diam x .40 LOC. 6061 mat'l in a vmc, not sure bout steel in a lathe (wouldn't want to use a lathe tailstock to drill that though..)
 
I'm missing something here. OP needs to make an 11mm long bushing with concentric bore that deviates not more than 0.001" end to end. That's not especially close tolerance - why does it need to be ground, and why can't he use the lathe he already has? I don't think he said anything about the lathe's condition, but even a very worn lathe should be able to pull that off with some care?

Sent from my SM-N960U using Tapatalk

cause machining is all so easy I can just do it in my sleep
 
I must be missing something here, if so I apologize.

Turn the OD, don't use the Tailstock, use a Drill holder (of whatever flavour) on the Tool post. Dial it all in, drill the hole.....done.

R
 
Spend a little time preparing the lathe. Get the tailstock aligned with the spindle. Check that the tailstock quill is at the same height as the spindle. Shim it if necessary.

Drill from both sides to limit drift of the hole.
 
Probably few readers here are familiar with Levin lathes, made in the USA since around 1938. One of their products is a special tailstock with a live spindle and adjustments for perfect alignment with the headstock. It is designed specifically for accurate drilling of tiny holes in small parts. The headstock can be ordered with a 3C collet (1/2" or 13 mm round capacity) spindle or with a 10 mm collet (5/16" or 8 mm round capacity) spindle. The drilling tailstock spindle takes 8 mm collets with 3/16" or 5 mm round capacity. Both the headstock and the drilling tailstock can run 0 to 5000 RPM, so the combined drilling speed can be as high as 10,000 RPM.

LevinLathe.com: MICRO-DRILLING MACHINE

LevinLathe.com: MICRO-DRILLING ATTACHMENT

They have lots of really nice stuff in their catalog. I use one of their 10 mm lathes and have a few more waiting for enough shop space to put in use.

Larry
 
A lathe like this is called for:

boley.jpg
 
Hi All:
I have made many many parts with these sorts of criteria, and I've tried all sorts of ways to get there.
The way RJT talks about with a wire EDM is a great way...but only if you just happen to have a wire EDM you can pull out of your back pocket.
A nice Levin or Schaublin would be nice too, but again, only if you can just magically step up to one whenever you come up against a challenge like this one.

The real art is how to do this project with a Southbend or a Sherline, and believe it or not, it's possible there too, because I used to do stuff like this long before I had the cash to get a really good lathe.
Many of the posters have described methods that are pretty good, but I used to use one that has been bomb proof for me and has enabled me to make weird stuff like this on pretty simple equipment.

So here's how I tackled something like this just on the lathe (Yes I have a Monarch 10EE, and it's very nice but it's just a lathe and it will drill a hole about like any other lathe will too).

First I start with oversized stock.
I drill a start hole with a center drill and an undersized drill that I poke in only a short way and then bore it as far as I can conveniently reach with a tiny home ground boring bar. (you can buy bars like this from Harvey Tool and others if you can't conveniently make them).
I bore so my pre-ream drill size will just go in, and then I drill to my pre ream size all the way through, using that first bored hole as a drill bushing to center the start of the drill as accurately as the lathe is capable of.
Now I bore a step so my reamer will just go in, then ream using that new bore again as a drill bushing.
With a decently gentle touch,this gives me the best, straightest hole the drill and reamer are capable of; irrespective of whether I have a Cadillac lathe or a Chevy.

While I still have it chucked, I turn two steps on the outside at the outboard end; one to clamp with the chuck, and one to set up a clock against.

I take it out of the chuck and then turn up a tiny little stub shaft with a tiny little 60 degree center in it but I back turn the stub shaft so I can get it concentric to the center drilled hole. (I kiss the 60 degree face of the center drilled hole with a mini boring bar if I need it close to perfect)
The stub shaft needs to just go in the finished reamed hole, and of course it's going to be a center plug to accept a live center.

Now I can chuck up my blanks on the tiny step I turned on the outboard end and clock them in on the second step.
I can push in my tailstock center plug and run my tailstock up against it.
Because I only have a tiny bit in the chuck to drive the part and can clock that end in perfectly, my hole will run concentrically around it's axis and coaxially with the spindle axis if I've taken the care to set up the tailstock properly
Turning them to diameter is a doddle, and turning them to length afterward is too.

If, by chance I need the holes to be super uber holy crap accurate holes I hone or lap them after reaming and get them dead nuts before I make the plug and turn them down.

Actually, what I usually do now that I have a wire, is just what RJT does...I make a quickie chuck for the wire, and then wirecut them in place.
Typically they will run within a tenth and I can control the size within a tenth too, and I can get there without all the farting about.

But BEFORE I had my wire, this was the way to make accurate concentric bushings that were too small to just bore or grind to ID.

Cheers

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








 
Back
Top