Precision Manufacturing with Mini Mill

[aldaeron]

Hi CD,

Our team has a mini mill with a DRO and were interested in making some simple plates for gearboxes. Since this machine is not as robust as some larger machines I have used in the past, plus it has been used by students for a few years, I am concerned that we cannot repeatably attain the accuracy needed for cutting mounting holes for bearings/CIM and getting the correct spacing for spur gears.

The typical gear spacing formula for 20 DP gears I have seen here many times is: (Total # teeth from both mating gears)/40 + .003.

For a 84T spacing this distance would be 2.103, for 96T it would be 2.403 (Vex demonstrates this here).

Vex bearings are nominally 1.125 (Hex are 1.124)

A CIM mounting boss is 0.750 +/- 0.002

What we want to do is accurately cut a mounting hole for the CIM and a bearing to support a spur gear on some 6061 aluminum bar stock 3/16 or 1/4 thick.

Is the feasible to do this repeatably on this mini mill? What tolerances are acceptable on the mounting hole sizes and between centers? How would you measure these distances (if at all)? For cutting the bearing mounting holes, should the final cut be with a 1-1/8 endmill or should we try to use a 1-1/8 reamer? A stock reamer is way too long to fit in our tiny mill – can we cut the shank down?

Any help is appreciated, especially if you have experience with precision manufacturing on one of these mills. We typically use it for simple operations. We do not want to attempt this if we cannot meet the tolerances and end up spitting out gear teeth. We have been fortunate to get offers from other teams to have parts made on their CNCs, but we are trying to learn to do this in house.

Thanks!

-matto-

[topgun]

Couple of thoughts here:
An endmill or reamer that size is bigger than what the machine can handle, so then you go to something that can cut big without the stress on the machine. That would suggest a boring head. https://littlemachineshop.com/produc...3662&category=

You have a DRO, so unless it's damaged, you should be able to travel from your starting spot to the various spots you need to drill, bore pretty accurately.

Poor Man's Way:
Draw up your part in SolidWorks (or some other CAD tool). All are available free to the FRC teams. Print the drawing on a laser printer (not inkjet). Use the printed drawing as a template and transfer punch the hole centers through the paper to the work piece. Then mount in mill and drill out or bore out the holes. If you are careful, this method is pretty accurate, though the DRO will be more accurate.

Another thought is to have a machinist (retired or working) volunteer to show you and your team how to do this one night on your mill. They would probably get a kick out of it. Then practice. Taking your time and being careful can lead you to pretty good results.

[sanddrag]

You can definitely cut the shank on a reamer using an angle grinder and a cutoff wheel. But, I would recommend a boring head to finish up with. You're getting pretty limited on height on that machine, so you'll have to see what fits.

[asid61]

For the CIM hole, the method I like is to drill with a 1/2" drill, then a 5/8" endmill, and finally a 3/4" endmill to finish the hole. This gives a solid fit, and using an endmill ensures that the hole is exactly where the DRO says it is.
For the bearing, I normally go for a 1/2" drill, then a 3/4" endmill, then a 1" endmill, and finish with a 1.125" endmill which gives a nice slip fit or tight fit on bearings. If you can't step up from 3/4" to 1" safely and don't want to have to use a 7/8" endmill, or if you want a press fit, then a boring head is your best bet. However, if properly designed you'll never need a press fit.
Using the template method mentioned above works for inaccurate parts, but I wouldn't do a gearbox. It's good for finishing a gearbox so it doesn't look or weigh all square and clunky.

[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.

[RoboChair]

Originally Posted by aldaeron

Is the feasible to do this repeatably on this mini mill? What tolerances are acceptable on the mounting hole sizes and between centers? How would you measure these distances (if at all)? For cutting the bearing mounting holes, should the final cut be with a 1-1/8 endmill or should we try to use a 1-1/8 reamer? A stock reamer is way too long to fit in our tiny mill – can we cut the shank down?

Any help is appreciated, especially if you have experience with precision manufacturing on one of these mills. We typically use it for simple operations. We do not want to attempt this if we cannot meet the tolerances and end up spitting out gear teeth. We have been fortunate to get offers from other teams to have parts made on their CNCs, but we are trying to learn to do this in house.

If you have a DRO most of the hard locating work is done for you. You just need to make sure the gibs are adjusted well to keep it square and lock it in place during critical hole operations. If you need to make something larger than your bad travel you can use locating holes to re-zero or locating pins on the bed to shift it a known amount.

Your mounting holes should be drilled to no tighter than a close fit for your bolts, but can be as much as a free fit if you are having tolerance stack up issues.

For your 1.125" holes you have a few quick and dirty options that your mill can accommodate. Quickest would be to use a step drill such as this or this, they produce reasonable holes while requiring much less torque. You can then use Retaining Compound to help hold your bearings in place and fill any gaps in your bearing bores.
Another option is a fly cutter or boring head, both can easily make a hole close in size with little work and the boring head can be dialed in to exact size but takes time and skill. You can then finish up with a 1.125" or 1.124" reamer with a cut down and reduced shank.
This is the important thing about reamers, drill bits, and the like; almost none of them have hardened shanks, only the important bits get hardened. Just take a good file to the shank and if it is able to scratch and bite into it then you can machine it however you like. Somewhere down the shank it will stop being able to bite in and just skate across the metal and that marks the spot where you can no longer work the metal normally.
It is also important to note that reaming a hole does not require precise locating of the bit, it will center into your hole just fine and can be easily done as a second operation with a drill press, after all the precise machining is done. If your reamer is rigid and stiff when you go to ream a rigidly mounted part, any runout in your reamer will be transferred to your hole and it will end up larger than the reamer is supposed to make it. For this reason you will probably not want to ream your holes with your part rigidly mounted.

[RoboChair]

Originally Posted by asid61

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.

I like these cheap DRO scales

Originally Posted by aldaeron

I can't afford to buy a set of plug gauges so will a measurement with a caliper be close 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?-

Yes, calipers are just fine.

Backlash doesn't matter when you have a DRO so long as you lock your axes when it matters. If it's moving you need to either lock harder of adjust your gibs tighter. If you are worried about getting your vise really square just put a straight bar in it and tram off of that. You can also just clamp a plate to the bed with a piece of sacrifice material under it and go entirely off of coordinates for making gearbox plates.

[sanddrag]

If you really wanted to measure it after the fact, you could go in with a coaxial indicator in the mill spindle, and use your DRO.