PDA

View Full Version : Threading Question



Steve Middleton
05-22-2013, 04:55 PM
Have some 1/4" brass rod I'd like to thread to 1/4" x 20. I turned it down to about .220 and the threads look good but nut does not turn smoothly. Is there a "rule of thumb" or table to guide me? Have looked on line and in a couple reference books but have not found anything relevant so far. Thanks in advance for the help.

Errol Groff
05-22-2013, 05:19 PM
.220 is pretty small for 1/4-20 but not unheard of. Try running a tap through the nut, often hardware store nuts can be rough inside and running a tap through helps a lot.

danlb
05-22-2013, 05:38 PM
Are you single point threading or using a die? The formula for an UN thread is very straight forward. You only need the pitch and the major diameter to use it. The example at http://www.tanj.com/cgi-bin/tpi.cgi walks you through the calculations. That page is oriented towards using a lathe tool with a sharp, V shaped tip.

The .220 is way too small. The major diameter should be only .010 smaller than the nominal size.


Dan

john11668
05-22-2013, 05:54 PM
Could your nut be 1/4 BSW
Same pitch but 55 deg included angle
A tap will sort it !

Rich Carlstedt
05-22-2013, 07:08 PM
I think Steve meant that he ran the thread tool down to a .220 " diameter ( Root Diameter !)
For his thread.
Steve what you want is called the double depth of thread ( DDT)
You normally find it on "center gauges", the small arrowhead looking gauges that tell you the threading tooling is perpendicular to the stock when you set up the lathe ..
The "V" DDT for 20 threads is .0866
http://shopswarf.orconhosting.net.nz/thread2d.html

So a .250 OD means .250 x .0866= .2165 as a root diameter
Your root is too tight.
It is also acceptable to run a file or other abrasive over the crests of the thread to smooth is out after single pointing.
Rich

Juergenwt
05-23-2013, 12:28 AM
Steve - if you are using a die to cut it - just put a chamfer in front and run your die over it. No need to cut it undersize.
If you are single pointing it - it's ok to turn it down by .002 0r .003 and than cut it until the mating part fits.
If you need it to be precise - turn it down by .002 to .003, than single point the thread to either a thread gage or 3-wire measurement.
Rich Carlstedt gave you some good advise.

iMisspell
05-23-2013, 12:59 AM
Yea... it sounds like he is talking about the root.
At work, prints normal call out .002 under the OD size and give a -.007 tolerance from there (all in house/production parts)...


It is also acceptable to run a file or other abrasive over the crests of the thread to smooth is out after single pointing Personally, at home, i hit them with a fine file (sometimes emery after the file) and then take a zero pass after that.... if the thread is long enough i'll file as i cut. At work, on the CNC's i'll add a clean up pass over the threads and then take two threading passes after that, first .001 bigger then finish and the last .0005. Most of the time the threads come out nice.

JoeEM
05-23-2013, 08:58 AM
Steve what you want is called the double depth of thread ( DDT)
You normally find it on "center gauges", the small arrowhead looking gauges that tell you the threading tooling is perpendicular to the stock when you set up the lathe ..
The "V" DDT for 20 threads is .0866
http://shopswarf.orconhosting.net.nz/thread2d.html

So a .250 OD means .250 x .0866= .2165 as a root diameter
Your root is too tight.

Thanks Rich! I'm a newb to threading myself and that's the kind of info I wish I had at the start. Everyone kept telling me to just cut it close and then try a nut or finish with a die. I suspected there was more info on those arrowheads!

J Tiers
05-23-2013, 07:45 PM
There is a "trap" in threading......

if you don't strictly go by angle and pitch diameter, you may get caught by the burrs that Rich Carlstedt mentioned. Those are on the crests, and can make the thread *seem* to be still too big, by dragging on the nut.

But if you continue to cut until you get them small enough to fit, the threads will be way undersized.

File off or remove some other way before trying ANY sort of gauge on the threads. Or use a "topping" insert.

DATo
05-23-2013, 08:07 PM
Just repeating what others have said : could be a burr on the crest of the thread. A good rule of thumb is to take a light file stroke or two over the crests of the threads and then take one more pass with the threading tool without feeding anything on the compound.

The burr problem we are talking about is particularly bad with copper. If you are cutting 360 brass I doubt that this would be the case, but and a leaded brass or marine brass might also raise burrs which would significantly increase your O.D. much the same as it does with copper.

gizmo2
05-23-2013, 08:09 PM
I cheat, if the application isn't critical. Single point until the o.d. grows by a thou, then knock it back with a file (it will end up 5 to 7 under). You can feel it too, but the micrometer feels it quicker. Now if you're talking barrel tenon threads or a higher class of fit, this is too quick and dirty.

darryl
05-24-2013, 01:35 AM
I wonder about the threading tool. Is the angle correct, is it high/low, does it have the correct helix angle-

Threading is a fairly simple math problem- root diameter, crest diameter, shape of the tip. Mechanically it's clearance angles around the cutting tip, proper tip shape and sharpness, proper height, the method of advancing the tip into the work, and the ability of the lathe to take the cutting tip through the right path. All I mean by this last point is that the threading mechanism has to be in good working order, and the carriage/top slide/compound have to be capable of maintaining the cutting tip in position without slop, flex, or other anomalous shifting. If you're producing a drunken thread for instance, it's not going to work right. You need to be assured that the lathe can do all this properly- then start looking at the rest of it.

danlb
05-24-2013, 04:14 AM
Am I the only one who is having no problems single point cutting threads on a lathe? I don't need to follow my work with a die. I don't need emery paper or a file to clean it up. I do a test fit only to ensure that I had measured it properly. :)

All you need do is understand that the thread "height" is not the same as the thread depth. Under the unified thread standard, the male and female threads are subtly different in that the male thread crest should be narrower than the female crest and the male thread root should be wider than the female root.

Here's the secret; You get the right thread profile if you turn the screw to the proper major diameter (minus .005) and then cut the threads to the specified depth (measured from the major diameter) . The same thing if you bore (or drill) the nut to the proper minor (plus .005) before cutting the threads to the specified depth (measured from the minor diameter).

Now I will admit that I'm not trying to match a class 3 fit. I'm just making parts that screw together smoothly with little play. I can match a thread from a store bought part just about every time. It's MUCH less nerve wracking than the cut and try method.

Dan
p.s. Please forgive any typos or arrogance. Jose Cuervo and I have been relaxing together this evening.

big job
05-24-2013, 05:58 AM
Thats it Dan, and then there is the golden rule, "if you are in a hurry in a machine
shop, you dont belong there". After you have done a zillion threadings, >no math
no looking back, for that perfect fit. There is no shame in doing several spring
cuts. No shame in using a thread stop, best thing ever especially with old eyes.

Hopper
05-24-2013, 07:20 AM
... the golden rule, "if you are in a hurry in a machine
shop, you dont belong there".

Words that I never ever heard come out of a foreman's mouth though.

J Tiers
05-24-2013, 08:22 AM
Dan: You must never have to thread anything that tends to throw a burr. Otherwise you would be quite aware of the need to clean up the OD.

I don't know that I would call that a "threading problem", more like a "fact of life".

Forestgnome
05-25-2013, 10:15 AM
The other thing that can cause a problem is that the depth of the thread is dependent on the type of root profile you're cutting. A sharp vee depth is different than a flat or radius at the root. A mistake here can cause the thread to be too wide to engage properly. The easiest way to get it right is to use a manufactured cutter with the correct profile. I use a threading cutter that has a tip radius ground to the smallest root I want to cut, then when cutting larger threads I move the cutter along the axis of the work after cutting to depth to narrow the threads until they engage.