Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Min. Full Thread 7
- Thread starter JAS1994
- Start date
-
2
- #2
Not sure there's a text book that covers it, I don't recall seeing it in 14.5.
However, the definition of MIN is given in ASME Y14.5M-1994 at section 2.5, essentially it means minimum and there is no explicit maximum, this is determined by "other elements of the design".
FULL THREAD is an abbreviation of 'FULLY FORMED THREAD FORM' or something like that.
Essentially the thread must be of fully form with not taper or 'run out' etc for the length stated.
I many situations I use the term "MIN FULL THREAD, DO NOT BREAK THRU"
This was discussed to some extent in thread1103-217231
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
However, the definition of MIN is given in ASME Y14.5M-1994 at section 2.5, essentially it means minimum and there is no explicit maximum, this is determined by "other elements of the design".
FULL THREAD is an abbreviation of 'FULLY FORMED THREAD FORM' or something like that.
Essentially the thread must be of fully form with not taper or 'run out' etc for the length stated.
I many situations I use the term "MIN FULL THREAD, DO NOT BREAK THRU"
This was discussed to some extent in thread1103-217231
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
-
1
- #3
CheckerRon
Mechanical
I like KENAT's explanation of MIN FULL THD.
Many companies, including where I am now, specify calling out thread depth on blind holes this way in company standards in order to assure the minimum full thread form required for the design without specifying a plus / minus tolerance for the thread depth. It gives manufacturing some dimensional leeway and avoids overly tight tolerances on the tapping process.
Many companies, including where I am now, specify calling out thread depth on blind holes this way in company standards in order to assure the minimum full thread form required for the design without specifying a plus / minus tolerance for the thread depth. It gives manufacturing some dimensional leeway and avoids overly tight tolerances on the tapping process.
-
2
- #4
I had to look at that a minute as the nomenclature struck me as back to front initially.
I always used the rule of thumb of needing 3 extra thread pitches for the tap hole.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
I always used the rule of thumb of needing 3 extra thread pitches for the tap hole.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
Cool stuff...good chart
Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group
Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group
-
1
- #7
Folks-
"MIN FULL THREAD" is sloppy and unnecessary because the thread depth callout fully defines acceptable limits for the threads. For example, if I call out a .112-40 UNC-2A blind tapped hole that is .20+/-.03 deep then the full thread depth must be more than .17 but less than .23. Technically, if you call out no maximum depth for the thread then the machinist can tap all the way through the part while still meeting the drawing!
Tunalover
"MIN FULL THREAD" is sloppy and unnecessary because the thread depth callout fully defines acceptable limits for the threads. For example, if I call out a .112-40 UNC-2A blind tapped hole that is .20+/-.03 deep then the full thread depth must be more than .17 but less than .23. Technically, if you call out no maximum depth for the thread then the machinist can tap all the way through the part while still meeting the drawing!
Tunalover
Tunalover I disagree.
Specifying Min Full Thread simplifies inspection in many situations.
Functionally for many threaded holes the important thing is that there is enougth thread that the mating fastener doesn't bottom out.
This allows a simple gauge of the minimum required depth to be used, rather than having to have both go & no go gauges.
If you actually read my post you'd have seen I brought up the addition of "DO NOT BREAK THRU" to resolve the situation you mention in your last sentance.
Do you seriously double the inspection when there is no functional requirement?
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:
Specifying Min Full Thread simplifies inspection in many situations.
Functionally for many threaded holes the important thing is that there is enougth thread that the mating fastener doesn't bottom out.
This allows a simple gauge of the minimum required depth to be used, rather than having to have both go & no go gauges.
If you actually read my post you'd have seen I brought up the addition of "DO NOT BREAK THRU" to resolve the situation you mention in your last sentance.
Do you seriously double the inspection when there is no functional requirement?
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:
If you say "DO NOT BREAK THRU" then the very real possibility exists that the pilot hold drill point can go so close to breaking through then a less than paper thin thickness can develope that can eventually break through and expel conductive debris into your assembly. That's just one bad thing that can happen with inadequate (read: sloppy) control is brought forth.
I honestly don't know why people seem to think that ASME Y14.5M-1994 is inadequate for dimensional control; you won't find such notes in there because there is simply no need for them.
Tunalover
I honestly don't know why people seem to think that ASME Y14.5M-1994 is inadequate for dimensional control; you won't find such notes in there because there is simply no need for them.
Tunalover
Both great arguments. I have experienced myself what Tunalover indicates. I needed a very flat external bottom surface. The drill point touched the internal surface and created a slight bulge externally.
The "Do not break thru" note did not help us.
The only way we could avoid this was to dim the depth from the thd/drill starting surface with a "max" dim, and "min full thd".
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion
The "Do not break thru" note did not help us.
The only way we could avoid this was to dim the depth from the thd/drill starting surface with a "max" dim, and "min full thd".
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion
CheckerRon
Mechanical
I think the control of the tap drill depth is being ignored here.
Tap drill depth (1) should be specified, and (2) will limit the thread depth max without imposing a full thread depth tolerance that will need to be inspected and possibly rejected though the fastener design may not be compromised.
The whole reason for MIN FULL THD is to avoid this.
At our place, we control this by specifying the tap drill depth as:
"MINOR Ø (depth symbol) .XX ± .03"
and make it the first line of the thread callout.
Moreover, MIN FULL THD should always be: "MIN FULL THD (depth symbol) .XXX" for blind holes.
Tap drill depth (1) should be specified, and (2) will limit the thread depth max without imposing a full thread depth tolerance that will need to be inspected and possibly rejected though the fastener design may not be compromised.
The whole reason for MIN FULL THD is to avoid this.
At our place, we control this by specifying the tap drill depth as:
"MINOR Ø (depth symbol) .XX ± .03"
and make it the first line of the thread callout.
Moreover, MIN FULL THD should always be: "MIN FULL THD (depth symbol) .XXX" for blind holes.
-
1
- #12
The situation that tunalover mentions is a prime example of one where a detail is called for. If a certain material thickness must be maintained below the tapped hole, then spell it out, or use a ± depth dimension to control it. There is no legitimate reason to risk "a less than paper thin thickness" condition other than laziness. It is the same as blindly choosing your tolerances without regard to function. The majority of cases can still be defined by MIN FULL THD.
I'm with KENAT on this one.
The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]
I'm with KENAT on this one.
The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]
I don't have the Machinery Handbook in front of me, but doesn't it specify what the drill depth should be per the thread size? (I don't remember)
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion
ewh has it.
I'm not saying you never put a +- depth tol on the thread, or potentially on the 'tap drill' or even show a section explicitly detailing it, however, I am saying you do it based on function.
In Ctophers example perhaps an alternative would be a flatness control or equivalent on the far side.
While it may vary by situation, for the majority of holes I see "MIN FULL THREAD DO NOT BREAK THRU" is totally adequate and relaxes inspection & tolerance requirements.
MIN is in ASME Y14.5M-1994 at section 2.5 and it specifically lists depths of holes as a potential application. As such while my complete phrase may not be in there I believe it's compliant with 14.5. Section 1.1.4 states that the absence of a figure illustrating an application is neither reason for to assume inapplicability, no basis for drawing rejection.
Anyway, the OP only asked what "MIN FULL THREAD" meant, he didn't ask for a debate about whether it was 'sloppy'.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:
I'm not saying you never put a +- depth tol on the thread, or potentially on the 'tap drill' or even show a section explicitly detailing it, however, I am saying you do it based on function.
In Ctophers example perhaps an alternative would be a flatness control or equivalent on the far side.
While it may vary by situation, for the majority of holes I see "MIN FULL THREAD DO NOT BREAK THRU" is totally adequate and relaxes inspection & tolerance requirements.
MIN is in ASME Y14.5M-1994 at section 2.5 and it specifically lists depths of holes as a potential application. As such while my complete phrase may not be in there I believe it's compliant with 14.5. Section 1.1.4 states that the absence of a figure illustrating an application is neither reason for to assume inapplicability, no basis for drawing rejection.
Anyway, the OP only asked what "MIN FULL THREAD" meant, he didn't ask for a debate about whether it was 'sloppy'.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:
- Status
Similar threads
- Locked
- Question
- Locked
- Question