Dimensioning on drawing with gauge/gage bar/ball 2

[KENAT]

I have a drawing for checking that has a dimension scheme similar to the attachment (it’s a channel/slot not a c’bore hole).

I have concerns about the way it’s been done but it’s not a type of scheme I’ve really used much before. I looked in ASME Y14.5M-1994 and don’t see dimensioning in this way addressed.

So I’m wondering if I should re-dimension it using surface profile (similar to discussed in thread1103-205200) or try and keep the same basic scheme but correct it.

If the basic scheme is OK then what needs correcting? I’m thinking the gauge diameter probably needs to be basic, but in that case do I really need to use a surface profile and make the angle basic too (I’m thinking it should be the included 90 not 45 to CL)? Would it be better to dimension to the top of the gage bar rather than the theoretical center? Anyone have any examples?

FYI the function is that it’s used to clamp a cylindrical item in a fixture while it’s glued to a perpendicular component. Basically 2 parts have a similar groove, one of them also has a surface perpendicular to the channel, and the parts being glued in are clamped between them (& pushed onto the perpendicular surface). Clear as mud right?

KENAT, probably the least qualified checker you'll ever meet...

 

[BARM]

I've done it that way before and got no flack back. See attached.

I consdier this a "conventional" dimensioning method. if you want to control the feature using GD&T well... then you'll need to have the confidence in your shop that they can understand it. In my case they couldn't.

---SW 2008 SP1.1---

 

[drawoh]

KENAT,

Definitely, I would show basic dimensions to the slot edges and the angle, and then apply geometric tolerances. As the inspector, I would select the inspection bar. Perhaps it would not be 1" in diameter. Perhaps I would repeat the test with several sizes of bar!

As shown, you do not have tolerances on the drawing. I do not see a way to apply tolerance that were not ambiguous.

I would use some combination of profile tolerances, angular tolerances and perhaps even a positional tolerance. It depends on what you are doing with it.

You could apply a tolerance on the round bar, and then a positional tolerance, effectively specifying the inspection tools. I do not know how this stacks up against the standard. This might be a good functional specification, but I would prefer the GD&T, above.

JHG

 

[BARM]

Here's the attched. 2nd attempt.

---SW 2008 SP1.1---

 

[KENAT]

Thanks BARM, out of interest what is the tolerance info on your sketch, espeically on the 1.125? I assume this has some kind of special control as it's labelled Critical, or is this an inspection issue? Also where you 1.175 says PART SIZE is this meant to imply it's a perfect diameter or does it still have some tolerance on it.

On the drawing I have it has block tols +-.005 for 3 DP, +-.010 for 2 DP and +- 1/2 degree. As drawn I'm assuming this applies to the height and the diameter. This leads to quite a bit of tolerance build up. The diameter represents the diameter of the part being clamped although the part is actuall +-.002.

I'm inclined to agree with you drawoh about probably using profile tolerance , a bit like either 6-23 or 6-24 but obviously linear not conical.

KENAT, probably the least qualified checker you'll ever meet...

 

[BARM]

KENAT,

Going by memory cause I don't have the completed drawing anymore.

Tolerances from drawing tittle block may have been.
XX = +/-.010
XXX = +/-.005
ANGLES = +/- 1/2 DEG.

This is a 1/4" thick plate used to clamp/locate a part. The part is a forged valve. The valve needed to be clamped prior to being machined.

So.... my toolmakers didn't need to have the drawing "hold their hand" by me over tolerancing/dimensioning the drawing. I did want to highlite to them the importance of comtroling the center of the 1.175 dia. This dia represented the nominal size of the valve.

The toolmakers may have machined up a 1.175 dia rod, set it into the "v-plate" and measured to it's top side to calculate the center "critial" dimension.

Again, our engineering department likes to use GD&T but if the toolmakers aren't comfortable using it then we used the conventional method.

Note. If we were dimensioning gauges used to check production parts then we almost always used GD&T. It's way more precise. The toolmakers would then need to rely on our inspection department to ensure comformance to the drawing.
Brent



---SW 2008 SP1.1---

 

[KENAT]

Thanks BARM, while the parts I'm working on are for tooling fixtures they're used to align a critical component of our product. Also they'll be machined externally as we don't have a machine shop so...

I think I'll go with surface profile.

Thanks to both of you.

Ken

KENAT, probably the least qualified checker you'll ever meet...

 

[CheckerRon]

One correction I would suggest on the attached sketches, and that is dimensioning to the top of the gage ball (direct measurement, not to its' centerline.

 

[KENAT]

Thanks Ron, that's what I was thinking.

However, I think I'm going to progress with surface profile.

KENAT, probably the least qualified checker you'll ever meet...

 

[BARM]

Yes, I agree with that or provide it as a reference dimension.

---SW 2008 SP1.1---

 

[BARM]

KENAT,

I have just one final option that I'd consider in the future. See attached.

The gauge pin can be any standard size approx. to the dia. called out on the drawing. All other dimensions carry a +/-.010" tol. Therefore the center of the gauge pin being the tighter controled feature get the necessary attention. The positional callout has a 3D control applied which in my opinion is suffice for the application.

Brent

---SW 2008 SP1.1---

 

[Xplicator]

You may or may not have control over this and this is my opinion, but if the cylindrical part is your product than the spec information belongs on it. If the result you are looking for is in the form of a sub-assy or "gluement" than generate a drawing of it specifying what is desired using functional GD&T, absent of piece part detail specs unless necessary and not redundant. If you employ datum targets you may find that fixture drawings are not necessary at all. Take a look at para 4.6.6 for use of equalizing datum targets for a v-block feature. Remember, that with proper use of GD&T, most all tooling can be envisioned solely from the spec alone, plus this allows for the machinist to better utilize their creativity and tacit knowledge of toolmaking and you are not dictating to them how to do this.

If for whatever reason those involved are confused, take the opportunity to teach them now, rather than later. Again, this is just my opinion.


Vance
--If you lead them, they are likely to follow, tell them and you will likely be alone!--

 

[KENAT]

Thanks for the responses.

Xplicator, I'm actually looking at this for our manufacturing guys. It's part of a gluing fixture that is used to assemble a critical part of our product. They want to be able to make several fixtures to increase thruput and yet get consistent results.

The entire pack is on my list to review as ther've been a few problems and I'm working my way through it but the priority right now is just getting the fixture drawn up in a way that we can get several make. We don't have our own machine shop, so all parts are made externally so we have to be a bit more careful with part definition even for fixtures etc.

KENAT, probably the least qualified checker you'll ever meet...

 

[drawoh]

BARM,

Your drawing precisely describes one of the suggestions I made, above. You need a tolerance on the gauge pin. The gauge pin diameter affects the profiles of the v-slot.

The comments I made above about this, still apply. I would only consider a drawing like this if the sole purpose of the v-slot was to locate a round bar or shaft.

JHG

 

[BARM]

Hi drawoh,

Assuming "sole purpose of the v-slot is to locate a round bar or shaft."

1) The gauge pin would have a very tight tolerance therefore you would adjust for that in your positional call-out tolerance. Right?

2) Supposing the inspector does not have the gauge pin size called out on the drawing (Actual sized called out not the best selection). Calculations could be made to adjust for new center. Right?

BARM

---SW 2008 SP1.1---

 

[drawoh]

BARM,

[ol]
[li]Yes, the pin would have a much more accurate diameter than the intended shaft, and I would think carefully about the implications of this. Perhaps I would call up two pins fabricated to the maximum and minimum shaft sizes. [/li]
[li]If the inspector does not have the gauge pin size specified on the drawing, he has to purchase or fabricate one. If I specify the manufacturing or inspection procedure, I mean it to be followed.[/li]
[/ol]

If a shaft is being located by a v-slot, the shaft diameter affects the final location. An inspector can calculate the true positon of an alternate size pin, however, there are all sorts of slot forms that will correctly locate the alternate pin, but will not correctly locate the correct pin.

JHG

 

[BARM]

drawoh,

1)Got it.

2)Got that too.

"there are all sorts of slot forms that will correctly locate the alternate pin, but will not correctly locate the correct pin."

For that to happen you'd want an inspection report that verifies the inspector followed the intention of the drawing. Right?

Thanks,
BARM

---SW 2008 SP1.1---

 

[drawoh]

For that to happen you'd want an inspection report that verifies the inspector followed the intention of the drawing. Right?

BARM,

It all depends on how badly you want an inspection report.

If the specification is called up on the drawing and the drawing is called on the purchase order, then the specififed performance is mandatory. If I repeat the inspection with my own correctly size pin(s), either the part passes or it is returned to the fabricator.

This is not good drafting practise. If I were serious enough to be demanding inspection reports, I would be much less likely to prepare drawings this way.

JHG