Precision Manufacturing with Mini Mill

[aldaeron]

I did not think of a boring head. Good call!

I do have a decent enough background machining and detailed tolerancing myself, but am having trouble coming up with what is acceptable and how to measure it.

If the nominal center to center spacing is 2.103 for 84T 20 DP spur gears, what is an acceptable tolerance when considering bore size and center to center spacing? .001? .003? .005? .010? I can't afford to buy a set of plug gauges so will a measurement with a caliper be close enough? I would prefer to not get a gearbox built and have to run it then examine tooth wear to see if I manufactured precisely enough.

If the DRO is perfectly installed (unlikely), the 4" wide vice is perfectly square to the table (hard to measure with a 4 inch vice), the screws have some backlash (even when locked) and the head has much more flexure than a large knee mill (to the point that its .001 or more), what error am I adding with such a cheap mill that the DRO cannot measure?

Appreciate the feedback though!

-matto-

[techhelpbb]

http://sherline.com/Wordpress/wp-con...1/3049inst.pdf

This will likely fit but the largest bore is a little too small for the bearing.
You'll have to work out how to get it in the R8 taper <- I keep forgetting I made an shank holder for this.
Could ream that 25mm hole out.

LittleMachineShop carries this boring head:
http://littlemachineshop.com/product...ProductID=3662

Criterion is known for making inexpensive small boring heads:
http://www.ebay.com/itm/Criterion-Ad...AOSwaZdXIXu K

You could use a rotary table if you can rotate the entire piece within the confines of the system.

This is much less a problem on a CNC retrofit.

If a Sherline under CNC control can manage this - that machine from Little Machine Shop is rigid enough to do it in aluminum.
https://www.youtube.com/watch?v=rmuDwlAenfU

I don't have video but I've been able to pocket a hole on my MaxNC 10 CNC mill within a thousandth of the intended center repeatedly. This machine is aluminum so the key is to take light passes and low cutting travel speed.

[asid61]

Originally Posted by aldaeron

I did not think of a boring head. Good call!

I do have a decent enough background machining and detailed tolerancing myself, but am having trouble coming up with what is acceptable and how to measure it.

If the nominal center to center spacing is 2.103 for 84T 20 DP spur gears, what is an acceptable tolerance when considering bore size and center to center spacing? .001? .003? .005? .010? I can't afford to buy a set of plug gauges so will a measurement with a caliper be close enough? I would prefer to not get a gearbox built and have to run it then examine tooth wear to see if I manufactured precisely enough.

If the DRO is perfectly installed (unlikely), the 4" wide vice is perfectly square to the table (hard to measure with a 4 inch vice), the screws have some backlash (even when locked) and the head has much more flexure than a large knee mill (to the point that its .001 or more), what error am I adding with such a cheap mill that the DRO cannot measure?

Appreciate the feedback though!

-matto-

The nominal C-C spacing for 2 84t 20p gears is actually 84/40 + 84/40 = 4.200". People here recommend adding between 0.001" and 0.003", and for your purposes/tooling 0.003" should be fine. I've done some very basic tests with C-Cs down to -0.005" apart without interference problems, and given how abused the profile on Vex gears is, you shouldn't need to worry too much about it as long as you stay within a few thousandths of your target.

I've always just used calipers to measure both bore and C-C, on the rare occasion that I have the time to do so. Granted, these were B&S dial calipers on a heavy Bridgeport, so checking was not always the most important, especially because I was essentially just "reaming" with a 1-1/8" endmill. Speaking of which, if you are planning on drilling 1/2", and then boring out to 1-1/8" from there, you can give up on doing more than 1-2 holes per day.

I used to use a boring head to do all bearing holes before I realized I didn't need the press fits given proper design. Even for those I just measured with a pair of quality calipers, as the tolerance only needed to be +/-0.001" anyway and using a telescoping gauge + micrometer was too difficult to get consistent. If you design your robot for a slip fit on bearings, then you will be golden even if it turns out as a press fit. I would give up on aiming for a press fit however, as a 0.001" tolerance on diameter (which is what the calipers can measure) is not close enough to get consistent presses to rely on.

Why wouldn't your DRO be perfectly (or very close to perfectly) installed!? That's probably one of the most important things you'll need to get perfectly square with the table. Take pains to get that within 0.003" on a 12" travel; even my cheapo Ebay DROs are within that.
As a side note, you probably won't benefit much from a DRO Pros on a mill that small IMO. I've had good results even with just the 0.0005" resolution things off Ebay. It seems like a waste to spend $800 on a DRO for a $900 mill, when you could probably get a CNC upgrade for less.
If you invest in a 0.0001" or 0.01mm dial test indicator instead of or in addition to a normal 0-15-0 indicator, you will thank yourself. I can get my 6" vise within 0.0003" on the width with ease, simply because the graduations are so far apart that it's easy to adjust.
Your head will flex minimally if you are using the boring head, and even if you go from a 1" hole to a 1.125" endmill there's very little force involved. I would wager that you will be able to hold a 0.001" tolerance on location and concentricity without much trouble, or even closer if you take care to take a light-but-not-too-light finishing cut on the boring head (provided you get very good at measuring with calipers). Again, I like using the endmill method because you don't need to worry about measuring the hole.
Keep in mind that if you're not doing fancy lightening patterns, 3/16" or even 1/8" plate is thicker than you'll ever need.