Machined shafts Drawing Inside

Looking to have some small shafts machined. Quantities for pricing will be 50/100/250 sets. Like I've stated in a few earlier posts, I'm pretty new to mechanical drawings so bare with me on tolerances and details. Feel free to ask any questions.

a little drawing help....

Nick,
looking at the bottom shaft first....you've got plenty of paper there,
move those 2 parts away from each other, maybe side by side.

You've got rather tight tolerance on drilled holes (.003 location) ruling
out using a simple drill jig (try .012 r) for location unless you really need
this, then the locating dimension is .1 taken to one place ?

the chamfers on the end, call out 15 degree x .031 as a lead in for the
bearings (if the are a slight or tigh press fit) others call out maybe .031 x 45 deg.
or "break sharp corner .005 max"

Hardened steel ? get off your chair and make a decision.....now.

What is the application ? lets start off with a simple 4140-ht
is available in tonnage qty's, is already heat treated up to Rc 28-30
can still machine and drill it, no distortion from heat treating afterward.

And a big one.....what is the o.d. on these parts, and their tolerances ?
And finish as well, torch cut o.k. or hydraulic lifter smooth ?

Those holes, any relation to each other?.....angular or lengthwise, looks like from
your +-.003 location on those holes your trying to hold a bearing in properly,
try dimensioning one hole from the end of the shaft, and then the other hole
from the first hole. What is the diameter tolerance on those holes ?

Or re-design so the holes are not so critical, locate a bearing on a shoulder,
that is easier to hold to a tight tolerance (lengthwise) setting bearing clearance.

Like I said I'm not a mechanical engineer. Just someone with a basic understand of CAD which is why I posted this publicly. Appreciate the drawing help.

I'm not quit following you on the tolerance for the holes? What do you mean .012 r?

These shafts are to fit inside a 5mm bearing. Bearing should slide on and be able to be removed easily.

Holes on the ends of the shafts are for a drive cup to be attached. Drive cup slides on the shaft and a pin goes through the shaft and drive cup. Holes in the center of the shafts are for a pin, a gear slides over the shaft and the pin through the shaft locks the gear to the shaft.

The holes are not that critical. I just thought that was a pretty normal tolerance and figured if I didn't dimensions a tolerance someone would ask.

Angular dimension doesn't matter for hole location

What is a normal tolerance for the holes of that size? it's a thru-pin that goes through them. The larger the hole the more slop that pin will have when the shaft is turned.

01 steel ok?

Nick,
Treat this as a red pencil markup of your drawing, nothing more, no
bad feelings.

the 5mm dia. stock is just that, the stock dia. not the finished dia.
you want, place that on the part.

All these words you sent me do not get conveyed on the drawing
(were they are needed) in fact less time is spent in properly dimensioning
a drawing then typing the paragraph explaining what is wanted.

The drawing IS the contract, it should convey all the info.

"These shafts are to fit inside a 5mm bearing. Bearing should slide on and be able to be removed easily"

what kind of bearing ? the tolerance of the bearing is important for the next
question... fit, loose,slip, or press.You said slide on, assume slip not loose.

I'm not harping on you because I want to, it's just when you ask for a quote,
give these guys a fully toleranced drawing, or they will pick and hunt you with
all these questions and more.

.003 hole location on drilled holes is tight ,.012r is our standard and it means
this:

Draw on cad, the cross hairs where you want the hole, in the
ether world of perfection (the cad screen) now draw a circle around
that cross hair with a radius of .012". The actual hole centerline
is allowed to deviate anywhere in that area.

other people have other tolerances, and ways of expressing it.


So if I can take a little license here, what you really want is someone
to take some 5mm (don't mix units metric/english BTW) P&G (polished
and ground) stock (something hard). Cut this off, and drill some cross
holes in it.

As I tell people, the devil is in the details.

I can see where the rings might work out nicely be I'm trying to work with an existing set of gears and the gears are setup for the pin.

DD, no hard feelings at all. I would have kept all the consultation private if I didn't take criticism well

I am revising the drawing but was wanting to clarify what I didn't understand first before revising the drawing that was revised incorrectly.

I knew the metric/standard on the same drawing was a no-no..... Why did I did I do it? Because I'm using metric bearings? What is a safe dimension to call out for 5mm then? How close of a tolerance? .197"? Or should I make the whole drawing metric?

Nick,
On the "mating up to a metric bearing" use the english measurement
.197 and in parenthesis I would put (5mm ref.)

What would be the Finished OD tolerance on something like that? I don't really know what to spec for the bearing other than I have 500 of them sitting in my shop?

Hopefully the updates are correct. I attached a revised drawing.

Would I be correct in assuming that .012r locatio means +/- .012...location?
Also, is it necessary to have .082 holes??? and .06...???

why not #45 drill and 1/16 or #53 drill???
What tolerance on hole sizes??? I thought you had originally posted +/-.003

Yes two different size holes are required. The pins that are used to lock on each part use different size pins. The #45 would be ok for the .082", I don't know if the .0595" would work or not. I would imagine so.

It's my understanding that the .12r tolerance relates to any direction and not just horizontal placement.

Nick,
the drawing is looking better, but the .012r is used (or drawn) using
the "feature control symbol" command, so there is a box with a cross hairs
(and a bullseye circle) and then in the next box is the .012 r. note

tapped holes go to .018 r.

"Would I be correct in assuming that .012r locatio means +/- .012...location?"

pretty much, but adding this little note eliminates adding +/- .012 on each dim.

see some others are comming in and asking questions ?
granted some are for a cost reduction (same size drilled hole
at both ends, is it o.k.) but others are because things are not
completely sewed up.

I had a vendor call me on one of my drawings I had done years ago,
it was a fully detailed production part drawing, and this vendor wanted
to know "what can I slide on, and what do I have to hold ?"

I told the vendor, he has to hold everything,.... to it's dimensions.
It was a motor shaft, and the bearing fits were clearly dimensioned
to tight tolerances, (as well as concentricity and to each other and
perpendicularity to a mounting face)
and the other diameters and lengths were dimensioned
to correspondingly looser tolerances (2-place and the like).

Note, NOWHERE on that drawing was the word "bearing". The vendor really
doesn't need to know what your putting on the shaft IF, if you dimension
and tolerance the part fully.

In your case, you don't know what the bearings and gears have as far
as tolerances, and what fit you want (loose,slip,press) so indicating
on the print (to fit 5mm bearing s.f.) will ussually get you a part
that is workable.

Especially from these guys around here (machine shops), they know
what they are doing and will work with a small guy like yourself.

tnx
Doug

Sent a P M

Brian
Brian's Machine & Powdercoat

Nick:

did you make a decision on the grills?

snocat_trf said:

Nick:

did you make a decision on the grills?

Click to expand...

Doesn't look like they'll be getting done anytime soon. A few other projects have taken priority.

I'm no longer taking quotes on these parts. I'm pretty sure I've found someone to make them.

Nick, sent PM

If you can help it, do not dimension from both ends of a part. Pick an end or hole and use it as the primary datum. If it doesn't add any information, end views on round stock are often not needed.
Look up True position tolerance. for more info on specing out locations.(Y14.5M or any drafting textbooks you may have.)
Also look into an area Tech school for classes on Geometric Dimensioning and Tolerancing. This will really help you in the long run.