Help With Alignment Pin Hole Drilling

M

Mike28303

Registered
Registered
Joined
Nov 26, 2016
Messages
21
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
 
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.
 
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
 
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
Click to expand...
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.
 
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.
 
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
 
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.
 
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.
 
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.
 
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).
 
You must log in or register to reply here.
Back
Top