How do I.... accurately measure a tilted hole?

[AdeV]

Problem: I am making a new "valley plate" for my Jaguar V12. I want to use the distributor drive to give me an accurate engine position reference for the ECU. I can't easily use the original valley plate, because I'm also mounting 12 coils onto it, and headroom is an issue.

Here's the original distributor mounting plate:



The inner hole is 40mm (maybe a shiver less), the recess takes a rubber seal, and the rest of the plate is a reference surface for the bottom of the distributor to sit on.

What's not obvious from the photo is, the plate is at an angle with respect to the mounting face, of 6 degrees. Fortunately it's only off-horizontal in one plane... otherwise I'd be in serious doo-doo... Anyway, this is the underside in case it's useful:



The flat bits are my horizontal reference.

So... what I need to do, is accurately locate the hole in my replacement valley plate, at the same angle, but I'm not sure how to do it...

My thought so far is: Turn a bar to a sliver under 40mm (the original dizzy drive is 39.80mm by the digi calipers, I've not broken out the micrometer yet). Turn a point on the bar, so effectively a fat dead centre.

Next, mark up the plate with some micrometer blue, and clamp to a piece of cardboard. Smear a little micrometer blue on the point of my "dead centre", and push it through the hole, until it contacts the cardboard (leaving, one hopes, a tiny blue dot). Remove & unclamp. Measure from blue dot to edge of casting using a digivern. That should give me the exact centre point of the circle at the base line of the valley plate. When it comes to milling out, I should be able to centre-punch the bottom of the plate, set my angle plate up to 6 degrees, use a pointy centre finder to align the spinde, then using a fat end mill, mill a flat, then centre-drill, twist-drill out to as big as I can get with a twist drill, and finish off with a boring head to give me the final 40mm dimension.

Am I on the right lines there, or is there a better way? Thanks in advance!

[efrench]

Does it look like A or B or neither?

[Lew_Merrick_PE]

Ade,

Such things have traditionally been accomplished using (old name) Tooling Balls that are now called shoulder construction balls -- here in the U.S., such things are most commonly acquired from Carr-Lane (http://www.carrlane.com/catalog/index.cfm/27825071F0B221118070C1C513E111D081B0006280B1713050245221E0107070F1A3C3B285356425D)

Does this help?

[sparky961]

I'm interpreting your question as: "how do I get a hole in exactly the same spot with the same angle regardless of what that angle actually is".  The "measuring" part may not actually be required if I understand correctly what you're trying to do.

This suggestion assumes you have access to a mill with a tilting head.  If not the same can be accomplished with a bit more difficulty by shimming up the work piece as has been discussed in other recent threads.  You'll be using your existing part as a setup fixture.  You need to have some references that are identical between the two (mounting holes, edges, or the like).  Set up some locating pins or stops so that you can positively remove/replace the old and new while maintaining the same position each time.

Mount the old part on the table and set the head at the correct angle to drill/bore the hole.  Make sure there's enough travel in the quill to do all of your operations without moving the knee once you begin!  Take the crank off or lock it to prevent yourself from doing something you'll regret.

Use a DTI in the spindle (or coaxial indicator) to get yourself centered on the hole in question.  The bore is pretty shallow but you should be able to verify the angle by moving the quill up and down as you sweep the indicator around the inside of the bore.  If the mounting flange is on the same axis that makes it much easier because any error will be more obvious when sweeping the indicator on it.  Get yourself as close to "0" as you're happy with - meaning the quill and your hole are on the same axis.

Replace the old part with your new part using the established references and go nuts.

Now that will get you your hole same as the original but it doesn't tell you where it actually "is".  If you need this information (which I suspect you probably don't) then you might be able to expand on the above advice to figure out the actual location too.

[AdeV]

Hi efrench - it looks like your diagram A. i.e. the dizzy mounting face is at 6 degrees, and the bore is perpendicular to that.

Lew, unfortunately, not so much in this case, but thanks for the thought! I'm not quite sure how I'd use a tooling ball in this instance...

Sparky - That's the one, that's the method I'm going to use (to make it at least). I actually started to think along the same lines when I read Jeff's answer to the question over on the XJS thread, but your write up cemented it. I'll use an angle plate rather than tilt the head (I hate having to tram it back in afterwards...), and the dizzy mounting flange is nice & big (~95mm dia), so I can put quite a large sweep on it, which should get me accurate enough.

OK, that doesn't give me an accurate position for drawing it on the old CAD package.... but as it will be a mixture of CNC & manual, that's not a problem

I would still be interested (academically) on how one goes about accurately locating angled holes, as it's something any of us might need to do in the future...

[efrench]

Won't ball bearings give you an accurate location? 

[Lew_Merrick_PE]

Lew, unfortunately, not so much in this case, but thanks for the thought! I'm not quite sure how I'd use a tooling ball in this instance...

There is a relatively simple solution to your problem if the countersinks are consistent and accurate.  Place (3 equal sized) ball bearings into the countersinks and lay a piece of (flat & true) plate on top.  You can then adjust (tilting head or table) until an indicator sweep is reasonably close to true -- and your head's axis will be perpendicular to the hole set.  The rest is just trig!

[Joules]

For my own jobs I make a plug with a central dowel on the lathe.  If need be the plug can have a shoulder, then a DTI is used to reference off the dowel.  3 Balls great as long as the screw holes aren't damaged or chewed up.  If I understand what you are wanting to achieve, correctly.

[awemawson]

Lew,

The fly in the ointment of your method is that it entirely relies on those counter sinks being exactly the same. I'd have though sweeping the face that they are drilled in is more likely to give an accurate result 

[BillTodd]

know any one with a cmm?

measuring the angle requires ony a surface plate and a sine bar.

locating the hole is tricky, but if you have a mill big enough to make one, then could you not make measurements with the mill and a touch sensor? (poor man's cmm)

[seadog]

Joules, a dowel with a centre pip is fine for hole which are perpendicular. However, if you try and use that technique here to spot through the existing plate onto the new one, you'll end up with a centre mark that's out of position. That said, you could then use simple trig. to work back from the position to find the correct point.

[sparky961]

I think it's ironic how more than a few people have mentioned "trig" to figure out the actual measurement, but no one has described the method.  That's like saying "Oh, that's easy - just use calculus".  Well, ok... not quite the same scale of obfuscation.

Crap.  Now you've got me thinking about how to figure out how to measure your part. 

What comes to mind is this:

Set up as I've already described so that you're aligned with the axis of the hole.  Set up your indicator for minimal travel when you drop it in the hole so that you know where "0" is (eg. less than one full rotation).  Establish your datum by zeroing the DRO.  Now you raise the indicator clear of the hole using the quill or knee. The knee can be used only if you're tilting the part not the head.  The advantage being that you may be able to use a scale or dial to measure the vertical offset as well as the horizontal offset I'm about to describe.

Move the long axis close to another well-defined feature.  Touch off the indicator by carefully sweeping it back and forth until you get the same reading you had in the hole.  By the looks of it the raised threaded mounting bosses might be a good candidate.  You can get an accurate measurement of the height, diameter of the top edge, and location. 

You'll want to be right on the corner with the maximum diameter of the indicator tip for the most accurate results.  Move up and down, closer and farther until you're happy you've found the right spot.  Your DRO will now read the distance between the edge of the hole and the edge of your chosen feature.  Now you use this dimension in your CAD program using a line coincident with the edge of the feature and parallel to the axis of the hole.

Here's a quick little mock-up that may help with any confusion in my description.  I've exaggerated the angle for the sake of clarity.



You might be able to come up with something that's easier to pick up with the indicator than what I've suggested.  Something mounted on the table or bolted into a hole perhaps.  Maybe even something set at the same angle as the hole so that it's vertical.  You'll probably have to do this separately for the X and Y axis.

If you can do all of the above, your accuracy is limited only to how well you can measure the rest of the features.

.... not that it matters anyway. ;)  Who knows... maybe there's a much easier way but I can get my head around this one.  Unlike calculus.

[seadog]

Maybe I'm missing something but I think it is a very easy calculation to make provided you can measure the angle and the thickness of the existing cover accurately.

If the angle is 6 degrees and the thickness is, say, T, then the offset is T x tan6

[sparky961]

Maybe I'm missing something but I think it is a very easy calculation to make provided you can measure the angle and the thickness of the existing cover accurately.

If the angle is 6 degrees and the thickness is, say, T, then the offset is T x tan6

I certainly can appreciate a simple solution over one that's complex... but offset from what?  Looking at the pictures, there's no edge of the hole that's on the same plane as the top or bottom of the cover.  This makes an accurate measurement to the edge of the hole very difficult.  You could extend the surface of the hole with something but you're introducing a lot of measurement error to an already tricky task.

There's been no discussion of accuracy required but I'm assuming that if the hole needs to be in line for a shaft and gear to line up with it's mate then you'd need to be closer than a degree or two and a 32nd or so.  That's about all the accuracy you could expect to get using simple handheld measuring tools in this situation.

Besides, it's much more important mechanically to get the hole on the same axis as the original.  Who cares where that hole really is until you start sending out your drawing for quantity pricing quotes.

Apologies if this sounds a bit confrontational.... I'm late for supper and perhaps getting a bit hangry.

[seadog]

I admit my reply omitted certain bits of information which were in my head 
Using the transfer punch, which someone suggested making, the centre point of the inclined hole is transferred to the top of the new plate. The new plate is positioned vertically under the original with mounting holes lined up. The centre mark produced will be offset to one edge by an amount that is the "opposite" side of a right angled triangle. The thickness of the original plate is the "adjacent" side. The measured angle we're currently assuming is 6º. Therefore, for a right angled triangle opposite/adjacent =tan 6º. This can be rewritten as Opposite=Adjacent x tan 6º
The value for the Opposite is the distance that the the centre mark must be relocated towards the middle of the new plate which then becomes the point that drilling/machining starts. This does assume that the bore of the hole is square to one of the edges. If not it becomes a little more complicated.

[sparky961]

Ok... fed.  Much happier now.

Thanks for the clarification.  Yes, there were definitely some important things left out the first time around.  I get what you're saying now.

Overall, I like the approach - mainly due to the simplicity (though we do need to make a punch).  However, one thing that bothers me in this case is the ratio of diameter to bore depth for the hole in question.  With the diameter being much larger than the depth, anything slid down the bore will have a tendency to cock and/or bind.  For this reason I wouldn't trust that a transfer punch would provide a mark that's aligned with the bore's axis.

The mathematical approach relies heavily on an accurate angular measurement as well, which tends to rub me the wrong way.  In this case, we don't know how fancy Ade's measuring tools are.  My original setup only relies on the ability to align/adjust the part on the machine and read an indicator; essentially using the machine as a CMM.

Now if the constraints included only a protractor and drill press, I'd be all over your idea. 

[sparky961]

Such things have traditionally been accomplished using (old name) Tooling Balls that are now called shoulder construction balls

I'm interested in learning more about how these are used in practice.  Do you know of any useful links, or would you be interested in writing up a separate thread showing some obscure but indispensable uses?

[Joules]

My assumption was you are angling the mill head, or you have an angle plate on the mill bed ?  Apologise for missing that in my description.

[Lew_Merrick_PE]

Such things have traditionally been accomplished using (old name) Tooling Balls that are now called shoulder construction balls

I'm interested in learning more about how these are used in practice.  Do you know of any useful links, or would you be interested in writing up a separate thread showing some obscure but indispensable uses?

Actually, I have started this, but it is an as time is available (something currently in short supply for me) task.  I have taught seven local machine shops how to use tooling balls over the past year.  Something that was part of my second six months as an apprentice back in the mid-1960's!

[AdeV]

Just for clarity, I've thrown together a CAD representation of what I need to do. As I forgot to bring the USB stick with the plate drawings to work today... I've re-created the plate as a simple block...

Not included are the gear on the bottom of the green shaft (for that I will use the original), nor is the "cap" and single-tooth "gear" wheel shown, nor the sensor mount. I'll do those later.

For the purposes of drawing up the final valley plate, this will do me; but when it comes to making it, as has been suggested, I need to be within a gnat's pubic hair's width of exactly the right place, or it's just not going to work properly. As far as getting everything in the right place for milling the hole:

1) I'll make a jig with 2 dowel pegs & 2 screw holes in opposite corners, these will allow me to both accurately locate, and secure, either the original valley plate, or the new one, to the machine in exactly the same place.
2) Jig will be mounted to the angle plate, angle plate mounted to the machine, align jig to be parallel to table.
3) Tilt angle plate until a dial gauge run around the outer-ish edge of the dizzy mounting flange reads zero at the four compass points at least, preferably fluctuating only with the roughness of the metal. That gets me the exact angle
4) Use a concentric dial gauge (? I think that's what it's called) to centre the quill over the bore hole.

So now the quill is directly over the centre of the hole, at the exact angle needed to bore it out.

5) Switch original plate for new plate. Mill the boss flat (to make the drilling easier, but also to mount the top-hat cover)
6) Drill/bore holes as required.

Quite easy really, once someone's pointed it out to you