# Help With Alignment Pin Hole Drilling



## Mike28303 (Dec 8, 2016)

Greetings,

I've been trying to solve an issue with drilling alignment pin holes on my small aluminum molds.

I have tried g-code (circular interpolation) on my mill, and it made ovals (out by about .002-.0015"). 

Then I decided to try using HSS drill bits. 

Dowel Pin Diameter: 5mm (.1969")
Slip Fit Drill Bit: #8 (.199")
Press Fit Drill Bit: #9 (.196")

Problem: I drilled the holes, but they all ended up bigger than I wanted. The .199" was way too big, the .196" was a great slip fit, no good for a press fit.

To make things even more confusing, on the back side of the mold the holes appear perfect. One slips with little to no slop and the other won't allow the pin in without some light tapping.

What am I doing wrong?

- Mike


----------



## Bob Korves (Dec 8, 2016)

Drills remove metal.  They do not make a hole to an accurate size or in the desired location.
Boring bars can make round holes in the desired location.  They are poor at removing large amounts of material, and are poor at cutting a hole to an accurate size.
Reamers are good at making round holes to an accurate size.  They are poor at removing large amounts of material, and are poor at locating holes.

The answer is to use a drill to remove the bulk material, leaving the hole under size.  Then use a boring bar to enlarge the drilled hole a bit while establishing the correct location for it, and leaving the hole slightly under size.  Finally, ream the hole to the finish size.  Let each tool add its strengths to the job, and none of its weaknesses.


----------



## talvare (Dec 8, 2016)

Ditto to what Bob said. You will never get truly accurate hole placement or truly round holes with drill bits. I have found that I can do pretty well in some cases by plunging with a four flute, center cutting end mill. It's not what they're designed for, but they tend to make pretty accurate holes , but unless you have them ground to custom sizes, you're kind of stuck with the standard sizes.

Ted


----------



## Bob Korves (Dec 8, 2016)

talvare said:


> Ditto to what Bob said. You will never get truly accurate hole placement or truly round holes with drill bits. I have found that I can do pretty well in some cases by plunging with a four flute, center cutting end mill. It's not what they're designed for, but they tend to make pretty accurate holes , but unless you have them ground to custom sizes, you're kind of stuck with the standard sizes.
> 
> Ted


Yes, Ted, the rigidity of the end mill and the milling machine is pretty good at establishing location and a round hole.  Even using split point, 135 degree screw machine length drills gives better holes than jobber drills do, but still not good enough for precision work.  Short of getting a jig borer or a jig grinder, the drill, then boring bar, then reamer does about the best you can do.  

Mike, it sounds like you have numerical control tooling so you might try plunging an undersized end mill followed by a circular finish pass to size.  Or, finish with a reamer.  That might be close enough to get the job done, though end mills that small are not very rigid.


----------



## Wreck™Wreck (Dec 8, 2016)

Even on higher end milling machines interpolating accurate sub .025 MM circles is a sketchy proposition at best as there are way to many variables.

Spot, drill and ream.


----------



## Mike28303 (Dec 9, 2016)

Wow, thank you for the replies everyone! Bob, your explanation was excellent. It makes perfect sense. 

I already have tried using a smaller endmill and running shallow circular passes, but I could not get a perfect circle. That's when I decided to try drilling to my desired sizes.

I just put an order in for the under and over sized reamers for my pins. I appreciate all the advice, and am excited to see how this turns out! 

- Mike


----------



## Wreck™Wreck (Dec 10, 2016)

You will find anomalies at the points where one axis stops and changes direction, on an analog clock this will be at the 12, 3, 6 and 9 positions, the bigger the hole or arc the better.


----------



## hanermo2 (Mar 7, 2017)

As they said.
If you can drill undersize, and then plunge with an endmill, you should be within 0.02 mm or so in size, smooth and straight.

An endmill on a near-net hole acts kind of like a multi-flute boring/bar cum reamer.
IF using rigid machine, and you can use a carbide endmill, much better than 0.02 mm, sub 0.01 mm on size and straightness.

If you use higher rpm or slow feed, both have a similar effect, the endmill will just bore the hole perfectly straight.
To near your spindles accuracy in tir.
But wear on the endmill corners will be very high, relatively.

A reamer should leave sub 0.01 mm in size and excellent surface finish.
Leave about 0.1 mm in D for the reamer.

Other tidbits (for curiosities sake):
For ultra precise sizes, roller burnishing gets you 2-3x better after reaming.

For fast and accurate in production, a custom boring tube, takes 3-4 secs to make a large deep bore to better than 0.01 mm in size and straighness.
These are tools with impregnated diamond coatings, very fast to use, last forever.
A single tool can last 300.000 bores, or more.
Common for example to make the cylinder bores in cast iron, for auto engine production.
I have seen a few.

A custom diamond boring tool might cost as little as 500$.
Some might cost 3000€, made to order, as the ones I handled.

In high-production stuff the boring tubes are good as no intermediate steps are needed.
Drill (6-8 secs), bore (4-6 secs), done.
A single machine might make 4 x 300.000 bores per year.
Or 300k chip pans, alu, for engines.
No tool changes. Single same diamond tool, all year.
Flat to 0.02 mm, or so, and runs about 20-30 secs cycle time.


----------



## Mike28303 (Mar 7, 2017)

Thank you for giving such an in-depth explanation, hanermo2. The time you save in getting an accurate hole with a boring bar is incredible. 

I ended up using an endmill to mill the hole, leaving some stock for the reamer. After reaming, I was satisfied to see the holes were well within the tolerance for what I was doing.


----------



## whitmore (Mar 9, 2017)

If an inaccurate hole is available, you can still put in your alignment pins; using jeweler's wax (basically, hotmelt glue) I made a 'line head' driver with six 0.040" pins, and it all worked.   Because, the glue gave
me enough compliance, and the loose holes meant there was room for the glue.

Boring and reaming would be a problem, with that size of pin.   I did have a center drill
small enough to start the holes, though.

Six circular posts engage six dimples around the head of the 'line head' screw, found in some
video games (NEC TurboGrafix was the one being targeted).


----------



## Bob Korves (Mar 9, 2017)

Mike28303 said:


> The time you save in getting an accurate hole with a boring bar is incredible.


Using an ordinary boring head to bore holes is a fussy and slow business if you are trying to hit your diameter dead nuts on.  It is maddeningly easy to overshoot your desired size.  Most of the reason is because of spring in the boring bar.  I prefer to bore to slightly under size to establish the location for the hole, then ream to final dimension.  If it is a shallow or blind hole, the reamer must be one without a taper on it's end for centering the hole and starting the cut.  It must be the type that is cylindrical for the full length and with angled cutters at the end to open the hole.


----------



## ewkearns (Mar 10, 2017)

Best practice in aluminum for straight holes is:

1) drill to remove metal, (through holes are your friend)

2) bore to clean up drill marks to locate hole - leave at least .004, or more for finish, if holes persist in being oversize, increasing feed and/or decreasing hole size can help, as well,

either,

3a) finish bore to size (1,000,000,000 jig borers can't be wrong)

or

3b) ream to size using a floating helical reamer, using plenty of lubrication, but don't remove under power.

If you do this and still get oversiz holes, it is time to talk about:

Rigidity, worn ways, tool holding issues, adjustment of tool slides, or errors in indexing.....


----------



## Bob Korves (Mar 10, 2017)

ewkearns said:


> 3a) finish bore to size (1,000,000,000 jig borers can't be wrong)


I don't see that many jig borers (or jig grinders) around in our hobby shops...  They will certainly do the job very nicely if you are lucky enough to have one in your shop.  Ordinary boring heads love to blow past the intended size, regardless of being careful...


ewkearns said:


> 3b) ream to size using a floating helical reamer, using plenty of lubrication, but don't remove under power.


Totally agree, and reamers are something that mere hobbyists can get their hands on for a reasonable cost and taking up little shop space.

Your sequence of operations is right on for any real chance of making a hole to the desired size and in the correct location.

Where are these 1 billion jig borers hiding?  They must be cheap and everywhere, but I sure don't see much that I could afford to buy or find room for in my shop...


----------



## ewkearns (Mar 10, 2017)

I've never had much trouble hitting the mark with a boring head, but RIGIDITY is the word....   Many of these jig borers are quite cheap!  They are ideal for the home machinist, as it seems they have lost favor to the CNC folks. Ever the multitasker, I opted for a Kearney & Trecker Model "D," with micrometer standards and dial indicators. For those unfamiliar, see Page 10 of this document for an example. I bought a 9 foot radial drill and the milling machine for $6,000... sold the drill for $6,000, so I guess I have $0.00 in the mill!


----------

