Largest Manufacturing Technology Community on the Web
Stay Connected:
Another turning challenge...ridiculously small parts
- Thread starter implmex
- Start date
- Replies 27
- Views 4,333
plastikdreams
Diamond
- Joined
- May 31, 2011
- Location
- upstate nj
I think with something like this, holding it rigid enough for thread milling is the main issue...and/or getting clearance for the damn tool as well. But I'm just speculating.
implmex
Diamond
- Joined
- Jun 23, 2002
- Location
- Vancouver BC Canada
Hi DanielG:
You wrote:
"What's the relative difficulty of tapping vs thread milling when you get down to the really small sizes? It seems like thread milling would be more reliable once dialed in."
Well, it depends.
I know how unsatisfactory that kind of Smartass answer is, but in this case the Devil is truly in the details, so let me explain what little I know of the subject.
Tapping will always allow a bigger stiffer tool than threadmilling, and as soon as you contemplate the kinds of cutters you need to stuff down your hole for each process it becomes obvious that this is so.
At small sizes and deep holes that matters a lot because the stiffness of the cutter and its resistance to breakage becomes increasingly limiting.
A key factor is the material the cutter is made of.
For example, carbide is wonderful stuff, but it is an agglomeration of tungsten carbide grains in a pudding of cobalt binder, and the fewer the grains the weaker the material.
The relationship is non linear, so long skinny carbide things are not just weaker than short stout carbide things...they are much weaker.
It's still pretty amazing stuff as a 0.005" diameter carbide endmill shows, but there are practical limits that you will not see in the same way with a 1/2" endmill as with a 0.005" endmill.
So among other things, tiny carbide cantilevered beams (cutters) become increasingly intolerant to rapidly changing loads such as you'd impose say if you recut a chip in a confined space as is inevitable when threadmilling a small bore.
The smallest I have tried to threadmill was 2:56 in 303 stainless to a depth of 0.075" and I soiled a few panties in the attempt even though I did it successfully.
The other thing that mattes of course, is the thread pitch.
Two things to consider here:
1) As the pitch coarsens, the cutter has to get smaller since it is is a planar saw trying to cut on a helical path, and the bigger the cutter and steeper the helix, the more it clips the outer edges of the profile and distorts it.
2) As the pitch coarsens the root diameter gets smaller and needs a smaller cutter to get into the hole and a smaller shanked cutter to avoid rubbing at the thread root.
So threadmilling at small diameters is problematic in ways that tapping at small diameters is not.
Tapping at small diameters has its own problems, like you have to take the whole chip in one bite unless you can get a series of successively larger taps down the hole.
The third thing that increasingly matters is the precision of everything; with small stuff,a discrepancy of 0.001" is very different than with big stuff, because it is the proportion that matters.
Going back to that 0.005" endmill vs that 0.500" endmill example: an unexpected extra 0.001" of material is a fifth of the cutter diameter to have to accommodate for the 0.005" endmill but only 1/100th of that for the half inch endmill.
The 5 thou endmill breaks and the 1/2" endmill doesn't even notice.
So that's it...hope it didn't bore everyone to death.
Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
You wrote:
"What's the relative difficulty of tapping vs thread milling when you get down to the really small sizes? It seems like thread milling would be more reliable once dialed in."
Well, it depends.
I know how unsatisfactory that kind of Smartass answer is, but in this case the Devil is truly in the details, so let me explain what little I know of the subject.
Tapping will always allow a bigger stiffer tool than threadmilling, and as soon as you contemplate the kinds of cutters you need to stuff down your hole for each process it becomes obvious that this is so.
At small sizes and deep holes that matters a lot because the stiffness of the cutter and its resistance to breakage becomes increasingly limiting.
A key factor is the material the cutter is made of.
For example, carbide is wonderful stuff, but it is an agglomeration of tungsten carbide grains in a pudding of cobalt binder, and the fewer the grains the weaker the material.
The relationship is non linear, so long skinny carbide things are not just weaker than short stout carbide things...they are much weaker.
It's still pretty amazing stuff as a 0.005" diameter carbide endmill shows, but there are practical limits that you will not see in the same way with a 1/2" endmill as with a 0.005" endmill.
So among other things, tiny carbide cantilevered beams (cutters) become increasingly intolerant to rapidly changing loads such as you'd impose say if you recut a chip in a confined space as is inevitable when threadmilling a small bore.
The smallest I have tried to threadmill was 2:56 in 303 stainless to a depth of 0.075" and I soiled a few panties in the attempt even though I did it successfully.
The other thing that mattes of course, is the thread pitch.
Two things to consider here:
1) As the pitch coarsens, the cutter has to get smaller since it is is a planar saw trying to cut on a helical path, and the bigger the cutter and steeper the helix, the more it clips the outer edges of the profile and distorts it.
2) As the pitch coarsens the root diameter gets smaller and needs a smaller cutter to get into the hole and a smaller shanked cutter to avoid rubbing at the thread root.
So threadmilling at small diameters is problematic in ways that tapping at small diameters is not.
Tapping at small diameters has its own problems, like you have to take the whole chip in one bite unless you can get a series of successively larger taps down the hole.
The third thing that increasingly matters is the precision of everything; with small stuff,a discrepancy of 0.001" is very different than with big stuff, because it is the proportion that matters.
Going back to that 0.005" endmill vs that 0.500" endmill example: an unexpected extra 0.001" of material is a fifth of the cutter diameter to have to accommodate for the 0.005" endmill but only 1/100th of that for the half inch endmill.
The 5 thou endmill breaks and the 1/2" endmill doesn't even notice.
So that's it...hope it didn't bore everyone to death.
Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
implmex
Diamond
- Joined
- Jun 23, 2002
- Location
- Vancouver BC Canada
Hi boslab:
I forgot to address your question, in post #20, so here it is now.
Yes it's "sort of" a hemispherical chamber lap, basically I put a chamfered hole a bit smaller than the ball diameter into the end of the lap and then I rotate the part in the lathe and the lap in a slow speed dental surgi-motor (used for installing dental implants and runs at as slow as 60 RPM).
I then press the lap against the ball I'm lapping while both are rotating, and move the lap around the circumference of the ball freehand while both are rotating.
The mechanics make for a perfect sphere...kind of like how you can make a spherical shape with a rotary table and a boring head on a Bridgeport.
It's intrinsically very accurate...you can make a spherical shape within millionths without any sophisticated gear.
Unlike a lap that has the exact shape you want to make on it, this relies of the lapping compound at the edge of the hole in the lap to describe a circular path, and so long as it remains circular and smaller than the workpiece diameter, it will lap a sphere if it is moved in such a way that some part of the edge intersects the axis of workpiece rotation from time to time.
Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
I forgot to address your question, in post #20, so here it is now.
Yes it's "sort of" a hemispherical chamber lap, basically I put a chamfered hole a bit smaller than the ball diameter into the end of the lap and then I rotate the part in the lathe and the lap in a slow speed dental surgi-motor (used for installing dental implants and runs at as slow as 60 RPM).
I then press the lap against the ball I'm lapping while both are rotating, and move the lap around the circumference of the ball freehand while both are rotating.
The mechanics make for a perfect sphere...kind of like how you can make a spherical shape with a rotary table and a boring head on a Bridgeport.
It's intrinsically very accurate...you can make a spherical shape within millionths without any sophisticated gear.
Unlike a lap that has the exact shape you want to make on it, this relies of the lapping compound at the edge of the hole in the lap to describe a circular path, and so long as it remains circular and smaller than the workpiece diameter, it will lap a sphere if it is moved in such a way that some part of the edge intersects the axis of workpiece rotation from time to time.
Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
Fascinating, thanks M, I remember an old machinist showing me how to make a split ball lap years ago, using a steel ball bearing, 2 copper pads and a hydraulic press, the pads were held with a length of signode steel banding, clever guy
Mark
Mark
Bill D
Diamond
- Joined
- Apr 1, 2004
- Location
- Modesto, CA USA
Seems like making the socket would be harder since the tool has to go down inside the socket.
Bill D
Bill D
implmex
Diamond
- Joined
- Jun 23, 2002
- Location
- Vancouver BC Canada
Hi Bill D:
You are exactly right the socket is indeed the weak link in the need to get the assembly right.
It's easy to make the male part within very close limits and it's also easy to measure when you get there.
It's very hard to do the same for the female socket, even though turning "a socket" is not very hard once you've made a tool for it.
Consider how it was done:
I ground and wire EDM cut a lollipop shaped boring bar, and I made it as accurate as the EDM conveniently allows but I measured it with a shadowgraph and a micrometer, neither of which is particularly accurate for this application.
I mounted it into the machine and brought the cutting edge as close to the axis as I could, using a drop gauge.
I programmed it in a conventional way, telling the CAM program to follow the nominal modeled contour to 5 decimal places
I touched the tool off in the conventional way with a gauge block against the faced end of the stock for Z and by turning and miking a test diameter with the edge of the tool in X
I turned a split block, took it apart and inspected a socket half under the toolmakers microscope and again with the shadowgraph.
So, after all those error prone steps...in plastic with only an airgun to cool it, just how close to nominal do you think I got?
Probably not very...certainly not within tenths.
So I made a male ball, lapped it in to nominal size (measured with a mike) and blued it into my socket half,
I reprogrammed my socket a twitch bigger and did it again.
When I was happy with the blueing pattern I turned a full socket and pressed in my nominal ball.
I wiggled it around to see if it felt right.
I made slightly bigger and slightly smaller sockets varying my offset by tenths until I got a socket that I thought was right.
I ran production on the parts; praying that my lathe was as consistent as I pretend.
Every fifth part got the test ball pressed into it to verify it still felt right and I called it good enough for this job.
Then I lapped all the male balls to be the same diameter as the test ball, and that of course is easy to interrogate within a tenth.
So claiming the sockets are spherical within a tenth is bullshit.
Claiming they're all the same within a tenth is more supportable but still bullshit.
Claiming they will all do the same job for the customer is quite reasonable.
Interestingly, those male balls I had lapped a tenth undersize by accident: you could notice how different they feel when snapped into a socket.
Making a ball 2 tenths undersize and it went from just right to pretty loose.
Make one half a thou undersize and it felt like a mile.
We won't even talk about a thou undersize.
So if I had to certify a surface fidelity tolerance for the sockets I couldn't do it.
If I had a fancy CMM maybe I could probe them to an adequate standard...I can't tell because I've never run a CMM.
So yeah, they are what they are...pretty good for a prototype, but not much more than that.
It's instructive to remember these things when a vendor is asked to make a thousand of them in a week for 25 cents apiece.
Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
You are exactly right the socket is indeed the weak link in the need to get the assembly right.
It's easy to make the male part within very close limits and it's also easy to measure when you get there.
It's very hard to do the same for the female socket, even though turning "a socket" is not very hard once you've made a tool for it.
Consider how it was done:
I ground and wire EDM cut a lollipop shaped boring bar, and I made it as accurate as the EDM conveniently allows but I measured it with a shadowgraph and a micrometer, neither of which is particularly accurate for this application.
I mounted it into the machine and brought the cutting edge as close to the axis as I could, using a drop gauge.
I programmed it in a conventional way, telling the CAM program to follow the nominal modeled contour to 5 decimal places
I touched the tool off in the conventional way with a gauge block against the faced end of the stock for Z and by turning and miking a test diameter with the edge of the tool in X
I turned a split block, took it apart and inspected a socket half under the toolmakers microscope and again with the shadowgraph.
So, after all those error prone steps...in plastic with only an airgun to cool it, just how close to nominal do you think I got?
Probably not very...certainly not within tenths.
So I made a male ball, lapped it in to nominal size (measured with a mike) and blued it into my socket half,
I reprogrammed my socket a twitch bigger and did it again.
When I was happy with the blueing pattern I turned a full socket and pressed in my nominal ball.
I wiggled it around to see if it felt right.
I made slightly bigger and slightly smaller sockets varying my offset by tenths until I got a socket that I thought was right.
I ran production on the parts; praying that my lathe was as consistent as I pretend.
Every fifth part got the test ball pressed into it to verify it still felt right and I called it good enough for this job.
Then I lapped all the male balls to be the same diameter as the test ball, and that of course is easy to interrogate within a tenth.
So claiming the sockets are spherical within a tenth is bullshit.
Claiming they're all the same within a tenth is more supportable but still bullshit.
Claiming they will all do the same job for the customer is quite reasonable.
Interestingly, those male balls I had lapped a tenth undersize by accident: you could notice how different they feel when snapped into a socket.
Making a ball 2 tenths undersize and it went from just right to pretty loose.
Make one half a thou undersize and it felt like a mile.
We won't even talk about a thou undersize.
So if I had to certify a surface fidelity tolerance for the sockets I couldn't do it.
If I had a fancy CMM maybe I could probe them to an adequate standard...I can't tell because I've never run a CMM.
So yeah, they are what they are...pretty good for a prototype, but not much more than that.
It's instructive to remember these things when a vendor is asked to make a thousand of them in a week for 25 cents apiece.
Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
Bill D
Diamond
- Joined
- Apr 1, 2004
- Location
- Modesto, CA USA
My mom at around age 95 fell out of bed and broke her hip joint. At that age rather then use a big cast and let it grow back, slowly, the doctor decided to replace her natural hip. Went fine healing nicely until one week later she snapped off the ball. No one knows how. they had to go in again and replace at least the ball portion. I assume it matched the already installed socket. This was not the improperly cleaned ones that the bones rejected.
Bill D
Bill D
