How would they machine a socket driver? When I look at a socket on the back side the square socket side, the angles are very sharp with maybe a very slight radius, whats the standard procedure to machine this? I see some radius on these look to be less than 2mm even, how can they get that deep with such a narrow bit? I am designing something similar but I am not 100% sure on the bit size or depth etc, is there an ASME standard or machining drawing to cover radius etc. maybe a radius to length of flat ratio or something?
Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
MACHINING A SOCKET DRIVER 1
- Thread starter valmeidan
- Start date
- Thread starter
- #2
here is a better picture showing the angles and features I am talking about. Also whats the depth to bit size ratio or is there such a thing? I designed the part in solidworks using a 2mm radius and on an 11mm x 11mm square part about 15mm deep and solidworks said my depth is to deep because of the depth to hole ration when i check it, but I look at a regular socket and its easily 15mm deep... not sure
They aren't "machined".. typically cold formed or similar
but could be machined.. broaching/milling/turning for one offs.
but could be machined.. broaching/milling/turning for one offs.
Or, push comes to shove you drill out the corners before machining the pockets.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
- Thread starter
- #5
MikeHalloran
Mechanical
You probably can't machine the square socket recess to look like the picture, because of the sharp-ish internal corners.
The part was probably made by driving a machined square into a soft bar, i.e. cold forming, and then heat treating after the shape was pretty much complete.
You can get the appearance pretty close with EDM.
Perhaps it would help if we knew what you are trying to do, and how many tons of such parts you need.
Mike Halloran
Pembroke Pines, FL, USA
The part was probably made by driving a machined square into a soft bar, i.e. cold forming, and then heat treating after the shape was pretty much complete.
You can get the appearance pretty close with EDM.
Perhaps it would help if we knew what you are trying to do, and how many tons of such parts you need.
Mike Halloran
Pembroke Pines, FL, USA
btrueblood
Mechanical
You could rotary broach a blind pocket like that, or drill the corners and mill it like Kenat suggested. Cold heading (or even hot forging) is likely the method for high volume tools, as Mike suggested. I'd avoid EDM if the tool is going to be used for high torque levels or on an impact driver. You might think of cutting a disc from flat sheet and having the hole water-jet cut through, then welding the part on its o.d. to the tool bit and hardening the whole thing. We've made some "special" tools this way, and they hold up ok.
- Thread starter
- #8
ornerynorsk
Industrial
Offering some additional details on your application, material properties requirements, and volume of parts that you will need will yield much better suggestions from the forum. The socket as pictured in your first posts are almost exclusively made from a forged blank and then precision broached before heat treating and plating.
It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.
It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.
valmeidan - are you ok using a ~ 2 mm mill bit to finish machine that pocket? Looks a little deep for that to me but what do I know I'm not by any stretch a machinist.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
MikeHalloran
Mechanical
KENAT, some tricks are possible, like:
Drill 4 holes at the corners, first.
Then plunge a big endmill right down the center to remove most of the mass.
Then change to a somewhat smaller endmill, mill a square around the round hole,
then change to progressively smaller endmills and mill progressively larger endmills,
and maybe finish by pushing a one-step broach down the hole to smooth the square.
OR, plunge an array of circular holes,
then plunge another array of smaller circular holes in the interstices,
and recurse until you can knock out the remaining stuff with a chisel or a small endmill.
In really old toolsets, you will find a drilled hole slightly larger than the square, right down the center of the square, straight broached sides, and tightly curled chips left behind by the broach, still packed into the bottom of the hole, fifty or more years later.
It's probably best to just specify a minimum depth of the square hole, a maximum corner radius or a note about a maximum relief, and a minimum solid thickness of the web beyond the end of the square cavity.
I tend to get sucked into super- detailing a solid model, making believe I actually know the best way to make what I want, until some old machinist sees my print, spits on it, and then shows me a better way. ... or doesn't show me, but just asks what features I really need, and goes ahead and makes a better part for less investment than I could ever imagine.
Mike Halloran
Pembroke Pines, FL, USA
Drill 4 holes at the corners, first.
Then plunge a big endmill right down the center to remove most of the mass.
Then change to a somewhat smaller endmill, mill a square around the round hole,
then change to progressively smaller endmills and mill progressively larger endmills,
and maybe finish by pushing a one-step broach down the hole to smooth the square.
OR, plunge an array of circular holes,
then plunge another array of smaller circular holes in the interstices,
and recurse until you can knock out the remaining stuff with a chisel or a small endmill.
In really old toolsets, you will find a drilled hole slightly larger than the square, right down the center of the square, straight broached sides, and tightly curled chips left behind by the broach, still packed into the bottom of the hole, fifty or more years later.
It's probably best to just specify a minimum depth of the square hole, a maximum corner radius or a note about a maximum relief, and a minimum solid thickness of the web beyond the end of the square cavity.
I tend to get sucked into super- detailing a solid model, making believe I actually know the best way to make what I want, until some old machinist sees my print, spits on it, and then shows me a better way. ... or doesn't show me, but just asks what features I really need, and goes ahead and makes a better part for less investment than I could ever imagine.
Mike Halloran
Pembroke Pines, FL, USA
Valmeidan, here is a sketch showing some corner relief options I've used before to maximize cutter size while allowing for a 'square' mating part.
They don't allow for tolerance etc. but illustrate the point hopefully, in each case let's assume the corner was pre drilled by 2 mm bit before machining the pocket - only location varies.
Now there is no free lunch, the more of the 'square' wall material you remove the less you have to resist the Brinelling from your square drive etc.
They don't allow for tolerance etc. but illustrate the point hopefully, in each case let's assume the corner was pre drilled by 2 mm bit before machining the pocket - only location varies.
Now there is no free lunch, the more of the 'square' wall material you remove the less you have to resist the Brinelling from your square drive etc.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
Oops posting at the same time Mike. I didn't mean to imply you have to remove all the material with the 2 mm bit, just that you're left with finishing up the machining with a bit of that size.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
I have seen special sockets being made. Drill the center. Change to a end mill and flat bottom the drilled hole. Put the socket on a Bridgeport with a shaper head and shape the square in one corner. Index the part and repeat the shaping.
Bill
Bill
- Thread starter
- #15
thanks guys, I think the relief 2mm holes is a good start then plunging a larger diameter bit to clear out most then form the square maybe. Also, as far as material cost goes, I noticed alof these are made from heat treated alloy steel, but like was mentioned earlier these are probably forged so maybe the steel is different than machining. The purpose of this is to be used as an adapter to connect an actuator to a 3way valve, would it be best to machine from stainless 304 or another steel and then finish with nickel plate or something?
Why finish stainless with Nickel plate unless you're in a fairly aggressive environment? Or do you mean make from steel and then nickel plate? Ni may work, might want to check hard chrome too.
Is 303 'strong' enough to resist the Brinelling from your applied load?
Will this part be removed often etc. or one shot deal? Think of the impact of the actuation and insertion etc. on the plating.
Is your primary load in one direction, or is torque similar both directions? The corner relief I showed bottom right can work OK in unidirectional applications.
Is 303 'strong' enough to resist the Brinelling from your applied load?
Will this part be removed often etc. or one shot deal? Think of the impact of the actuation and insertion etc. on the plating.
Is your primary load in one direction, or is torque similar both directions? The corner relief I showed bottom right can work OK in unidirectional applications.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
-
1
- Thread starter
- #17
KENAT said:
304 stainless should be strong enough, essentially it will be fitted into place then wont be taken off, nots sure of exact torque, the handle that came with the valve is pretty tough to turn. The load is rotational 90 degrees on y axis clockwise or counterclockwise depending on the flow direction. So your saying 2mm not corner relief just a radius is better then the relief in the top right which is what I am using now? in your bottomr right pic the hole is tangent with the bottom edge but offest right
You're making both the male and female components of this adapter?
This is a one-off?
Is there something holding you to a square socket shape? Could you just choose a different geometry that is much more practical/profitable for a limited production run, and not hold you to geometry typically reserved for processes that are only practical for high-quantity runs?
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
This is a one-off?
Is there something holding you to a square socket shape? Could you just choose a different geometry that is much more practical/profitable for a limited production run, and not hold you to geometry typically reserved for processes that are only practical for high-quantity runs?
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
racookpe1978
Nuclear
Now, when I need a "one-of" 36 or 42 inch long socket "adapter extension" to reach into a difficult spot, I weld a standard (hardware store) female socket head on to one end of a 1/2 x 1/2 square rod, then weld the needed male socket adapter on to the other end.
Looks a bit ugly, but gets the job done with less than 5.00 in tooling, and another 2.00 dollars for the steel rod.
Looks a bit ugly, but gets the job done with less than 5.00 in tooling, and another 2.00 dollars for the steel rod.
"So your saying 2mm not corner relief just a radius is better then the relief " - no, your other bottom right.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
- Status
Similar threads
- Locked
- Question
- Locked
- Question