position tol of tapped hole 1

matalik · Feb 15, 2007

I have a tapped hole on the end of a precision shaft. The hole is on the center line. What is the best way to apply a postion tolerance so that the threaded hole stays on the centerline? THe shop that makes the part seems to have a hard time with keeping the tap straight and I want to make sure that the drawing is providing enough information to them. thanks.

drawoh · Feb 15, 2007

matalik,

Are they having a hard time locating it in the centre, or is it crooked?

A true position tolerance tells the fabricator how to locate your hole. True position controls parallism to the OD and/or perpendularity to the end face, but not very accurately. You can use a parallel or perpendularity specification, in addition.

Perhaps it is time for a new machine shop?

JHG

Heckler · Feb 15, 2007

You can put all the controls on the drawing but unless the manufacuturing engineer has the process/fixture for that feature contrained you will end up with a "bad part"

Best Regards,

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

(In reference to David Beckham) "He can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. Apart from that, he'

KENAT · Feb 15, 2007

The first question you need to ask is 'how accurate does the hole need to be' then look at how to tolerance it to meet this requirement.

Looking at the use of GD&T as a quick fix without understanding how accurate the feature needs to be causes problems. GD&T should be driven by functional requirements.

Once you've determined what accuracy, you need then look at if just positional to the end face & OD is enough or do you need extra controls to keep it 'concentric' (note that I'm not actually suggesting to use concentricity tolerance)

drawoh

True position controls parallism to the OD and/or perpendularity to the end face, but not very accurately.

Surely how accurately depends on what value you assign to the tolerance?

prohammy · Feb 16, 2007

Matalik,

(KENAT, good advice)

GD&T will not 'solve' this problem, it will only emphasise what is required by you (the engineer) to your manufacturer (assuming he can understand what you send him).

I would suggest one of the following...

1. Get your manufacturer to pilot bore the shaft to one amd quarter times the full thread depth (GD&T this bore perp and par to shaft centre axis). Then GD&T tapped hole to bore (conc)
2. Reject all inferior material back to your manufacturer. May lead to arguments, so make sure your dims (and GD&T's) are correct.
3. Get a new manufacturer, and before you change to him, make sure your prod/manufacturing engineering audit him to make sure he can do what you require.

Kevin Hammond

Mechanical Design Engineer
Derbyshire, UK

matalik · Feb 16, 2007

thanks, I have my answer. The shop is having a hard time keeping the tap straight, so if I GD&T the hole to the axis, then GD&T the tap to the hole as suggested, I should be covered.

KENAT · Feb 16, 2007

I don't think I've ever toleranced the bore and thread separately before. I dont' have access to the standards today but I'll have to look at it when I do.

Also, wouldn't it be better to use a physical datum rather than the theoretical axis? Or are you going to effectively define the axis by making one end A and one B and having the bore reference A-B or something?

If it's a shaft, is parallel really the right tolerance, if positional isn't adequate would runout be better given that you appear to be concerned about 'concentricity'.

I'm getting in above my head now, you know what they say about a little knowledge, sorry. Maybe one of the more experienced posters can comment.

Plus when I said function should drive the tolerancing, obviously you still need to verify that what you think you need can be physically achieved, it just shouldn't be the initial driving factor.

drawoh · Feb 16, 2007

KENAT,

I routinely apply true position tolerances of 0.2mm on drawings. This is accurate enough to locate tapped holes and clearance holes for machine screws, assuming the clearance holes are through thin material.

If the tapped hole is 10mm deep, the fabricator can use up his entire error budget by angling the hole 0.2mm.

0.2mm/10mm = .02 radians.

This is over a degree of error. If you stick a long screw in it, you will see this clearly. If the clearance hole goes through thick material, the screw will not clear, and you will have a non-functioning assembly.

I have seen this done. You can drive a tap crookedly into a good perpendicular hole. It helps to do it when the forman is not watching.

If you have a deep clearance hole, you should consider adding a perpendularity specification to your tapped hole tolerance. I haven't actually checked this, but my gut feeling is that perpendularity of 0.05mm should be manageable by a machinist with a hand tap. Machinists, please feel free to correct me.

JHG

matalik · Feb 16, 2007

Thanks for the additional thought. That's what I am getting confused about. I have been trying to look at examples and don't see one where they GD&T the bore and thread separately.
It seems like there are several ways to do this, so I'll take any other thoughts. I'm looking for expamples of a similar situation, but am having a hard time finding any that have threaded holes.

Initially (I didn't create the part), the bore and thread are called out on the centerline of the shaft with no GD&T. I have limited experience in this area, and when parts started to fail, I have to clean up the mess. I guess its a good time to learn.

What I am seeing in examples, they GD&T using position first then perp, so that the bore will be in the correct position and square to the face of the part.

drawoh · Feb 16, 2007

matalik,

When you say "bore", are you talking about the tap drill?

As the designer, drafter and inspector, you have no interest whatsoever in the tap drill. Don't specify it. Don't apply tolerances to it. Don't inspect it.

Machinists know, probably much better than you do, what size drill to use prior to tapping. If your machinists need you to tell them this, this might be the source of your problem.

For a tapped hole, specify the size, the pitch or TPI, the tolerance class, the depth, and the positional tolerance. Add a perpedularity specification to the tolerance box if you need it. Buy thread gauges to inspect it.

If your bore has some functionality other than allowing you to tap a hole, then you apply the tolerances needed to meet that functionality.

JHG

dingy2 · Feb 16, 2007

I would place a positional tolerance on the threaded hole relative to the axis created by the OD.

This would be fine at the end surface but it still does not control parallelism.

Since this is a blind hole, I would also place a projected tolerance of at least the depth of the hole in the feature control frame.

How to check this - there would be a small checking fixture that threads all the way down in the hole. Protruding up from the hole on this checking fixture would be a cylindrical shaft the length would be the projected tolerance length.

Once installed in the threaded hole, check the position at the end face of the shaft and also at the end of the checking fixture cylinder which controls the parallelism.

That should do it.

Dave D.

http://www.qmsi.ca

ctopher · Feb 16, 2007

After you apply GD&T to the tapped hole on the dwg, add "MINOR Ø" under the FCF.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 02-10-07)

dingy2 · Feb 16, 2007

Chris:

If one was using the thought that I have, I would not use "MINOR DIA" since the feature control frame defaults to its pitch diameter. I would need pitch diameter so that I can thread the checking fixture into the hole.

Dave D.

http://www.qmsi.ca

ctopher · Feb 16, 2007

Is OK, but can cost more $$ to check pitch vs minor.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 02-10-07)

drawoh · Feb 16, 2007

dingy2 and ctopher,

On my big adventure with crooked tapped holes, I was able to observe the angle of the thread gauge. I was inspecting the angle of the threads at the pitch diameter, which I believe was a good idea. The pilot holes were drilled by a CNC machine, and probably, were perpendicular. I am guessing the holes were tapped out by hand.

JHG

Tunalover · Feb 17, 2007

What is the diameter of the shaft? The length?

What size is the threaded hole and how deep? These are all pertinent questions that no one has asked.

Tunalover

rigarc00 · Mar 7, 2007

I agree with what most posters have suggested. Use a true position on the top of the surface and then a perpendicularity for the depth.

My gut feeling is that the problem is going to be with determining a good reliable process in manufacturing. Has the machine shop tried to adjust their drill feeds to get the best results? there are techniques such as peck drilling (drill with smaller size prior to finilizing the hole) that improves the perpendicularity of the hole. This however can add cost depending on the amount of holes you need. Also, make sure the tapping is done in a controlled manner, hand tapping is an art and not a very repeatable procress from a quality point of view.

My last suggestion is to look into heli-coil or threaded inserts that might improve the procress and perhaps remove some of the procress that are currently hard to control.

powerhound · Mar 13, 2007

I don't believe a perp callout would be necessary in this case unless it is tighter than what the positional callout would allow with respect to the depth of the hole. In the ASME standard 1.4(m) it states that all geometric tolerances apply for the full depth, length, and width of the feature. If the hole is 10mm deep, the entire axis of the hole would have to comply with the positional tolerance provided the end face of the shaft was a datum and it was specified in the FCF. I think this is what drawoh was saying

Powerhound
Production Supervisor
Inventor 11
Mastercam X
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

matalik · Mar 13, 2007

Thanks for pointing out this fundemental rule, which I wasn't aware of. I guess it would help to know the basic rules. But what you say makes sense that the position of the hole feature shall remain the same of the entire depth, making a perp callout meaningless. Lots of good reply's on this question and I was a little overwhelmed being a beginner to GD&T.

KENAT · Mar 13, 2007

Perp isn't meaningless if you make it tighter than what you get from the positional. For instance if your pos is dia .2 and your perp is .1 then your perpendicularity is tighter. i.e. you're more concerned about perpendicularity than position.

However in your application I doubt you really care about perpendicular to the end face.

You say you want to keep the hole on the centerline, effectively you want to keep it concentric.

Now I'd think twice about using a concentric tolerance as it's based on the 'theoretical' centerline but there are ways to achieve basically the same thing with tolerances that actually apply to measurable features.

As per my first post though before you begin to GD&T it you need to know how accurate it needs to be, function must be the driving factor.

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

position tol of tapped hole 1

Mechanical

Recommended for you

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

Mechanical

New member

Mechanical

Mechanical

Mechanical

Similar threads

Log in

Part and Inventory Search

Sponsor