Machining Approach diff. between 2 plcs dim parts and 3 plc parts

What can you do on parts that are generally lower tolerance (2plcs, +/-.01) that you can't on higher tolerance (3plcs, +/-.003-.005)?
I am thinking in terms of prototype or one-off parts.

-Can I drill a hole on the VMC, then open it up manually a small amount on the drill press and still expect 3 plc positioning? Like if I drill/reamed it .250 to use as a locating feature, but need it to be .270 final.

-Is it (generally) acceptable to drill a hole on the machine, but ream 2nd OP on a drill press? Same with tapped holes?

-If I use a sharp machine length drill, and slow down the first .05", can I omit spot drilling if its a standard 3plc bolt circle?

-Do all small shops worth their salt use a cmm to check 3 place parts?

Thanks!

Ok, stupid question time: Why in the hell would you drill a hole on position in a VMC then pull it out to open the hole size and/or tap on a drill press?
If you need to flip the part, install a part stop and flip your part.

You don't need a CMM for positional measurement on .xxx dimensions. Indicator and digital height stand works fine or height stand, indicator and gage blocks.

vmipacman said:

What can you do on parts that are generally lower tolerance (2plcs, +/-.01) that you can't on higher tolerance (3plcs, +/-.003-.005)?
I am thinking in terms of prototype or one-off parts.

Click to expand...

Omit the spring pass, in some cases you can rough straight to the finish dim.

vmipacman said:

-Can I drill a hole on the VMC, then open it up manually a small amount on the drill press and still expect 3 plc positioning? Like if I drill/reamed it .250 to use as a locating feature, but need it to be .270 final.

Click to expand...

It depends on the way you open up the hole, and how accurate your starting position is. A piloted reamer is going to follow the existing hole, but drill presses in general suck for almost everything.

If you try to do it with a standard twist drill, there is a good chance it will grab and wreck the hole.

vmipacman said:

-Is it (generally) acceptable to drill a hole on the machine, but ream 2nd OP on a drill press? Same with tapped holes?

Click to expand...

Better to do it on a BP with the part secured and a quill that's not going to jump all over the place. The only thing I use drill presses for is deburring the backside of holes while the machine is running, and tapping long parts with a tapping head.

vmipacman said:

-If I use a sharp machine length drill, and slow down the first .05", can I omit spot drilling if its a standard 3plc bolt circle?

Click to expand...

Bolt circles are either clearance holes or tapped holes. In both cases there is usually some wiggle room since the fastener is loose in the mating part.

If you are talking about a screw machine drill, you generally do not need to spot the hole first or decrease the feedrate unless you are starting with an uneven surface.

vmipacman said:

-Do all small shops worth their salt use a cmm to check 3 place parts?

Click to expand...

No.

vmipacman said:

What can you do on parts that are generally lower tolerance (2plcs, +/-.01) that you can't on higher tolerance (3plcs, +/-.003-.005)?
I am thinking in terms of prototype or one-off parts.

-Can I drill a hole on the VMC, then open it up manually a small amount on the drill press and still expect 3 plc positioning? Like if I drill/reamed it .250 to use as a locating feature, but need it to be .270 final.

-Is it (generally) acceptable to drill a hole on the machine, but ream 2nd OP on a drill press? Same with tapped holes?

-If I use a sharp machine length drill, and slow down the first .05", can I omit spot drilling if its a standard 3plc bolt circle?

-Do all small shops worth their salt use a cmm to check 3 place parts?

Thanks!

Click to expand...

.
.
all machines have error and a drill press or a turret knee mill like a bridgeport the spindle quill can be leaning or out of tram
.
visualize spindle leaning at a 45 degree angle. the center of a short center drill is in one spot and a longer drill is more toward lean direction. this can effect hole locations on a part thats not a simple rectangle but has holes at different Z locations or heights. many parts are not simple rectangles and even a simple rectangle part the holes can be at a angle or not perpendicular so their location on other side of part can be not at expected position
.
a longer drill with flex tends to follow pilot hole thats how reamers work, the beginning of hole is bigger dia or bellmouthed til its in the hole enough to lower runout wobble
.
a short screw machine length drill is often used without a spot drill but if a spot drill is made big enough it leaves a chamfer around the drilled hole saving countersinking or deburring hole later
.
even on a big cnc a part just machined holes are rarely at true position to .0001", i often have to compensate for machine error. the X to Y to X axises are rarely all exactly perpendicular and the machine slides can have a looseness backlash and tilting action when slide travel is reversed