2.8 Drill and Ream a Precision Hole
Key Takeaways
A drill produces the prepared hole. A reamer finishes a controlled amount of material from that hole.
Choose predrill size using the specified reamer and measured hole. Subtract the allowance on diameter from the target diameter, or subtract twice the radial stock.
A reamer tends to follow the prepared hole. Verify its position and alignment before reaming rather than using reaming as a location correction.
Check the available depth, lead, chip handling and withdrawal method for the selected tool. Verify size and location as separate dimensions.
2.8 Drill and Ream a Precision Hole
A CNC program can repeat the same hole-making motion while the prepared holes still vary in size, form or location. For a precision hole, decide which operation creates the starting hole and which operation brings it into its finished size range. The drawing and selected tools govern that choice. The NIMS milling crosswalk includes drilling, reaming and hole gaging.
Plan the Prepared Hole
Choose a drill and entry appropriate to the material and setup. Check the starting surface, the required diameter, the solid thickness or available depth, and the space beyond the part. A drill’s programmed tip depth is not necessarily the depth at which the full diameter is produced. The point projects beyond the full-diameter portion. Account for the actual point form when a hole must break through, and avoid backing plates, fixtures and obstructions.
A reamer removes a relatively small layer from an existing bore. It tends to follow the prepared hole. A hole that is already misplaced by drilling can stay misplaced after reaming. If the hole center, straightness or preparation is wrong, review the locating and drilling process and use an approved corrective machining method where enough material remains. Increasing reamer feed or changing reamer diameter does not locate the bore at a different XY point.
Worked Allowance
Suppose a process uses a 10.000-mm Kennametal RMS solid-carbide reamer with the helical-flute, internal-coolant family data. The manufacturer lists a recommended allowance on diameter of 0.20 to 0.30 mm for the range including 10.000 mm. Use this row only for the stated tool and size range.
A process choosing 0.250 mm of stock on diameter aims for a prepared diameter of mm. The remaining layer is 0.125 mm per side when the bore is concentric. Check the actual prepared hole. If it measures 9.700 mm, the measured allowance is 0.300 mm on diameter. If it measures 9.850 mm, the remaining stock is only 0.150 mm on diameter, below the selected tool guidance for this example. The drill’s marked size is not a measurement of its cut.
| Observation | What to examine |
|---|---|
| Prepared diameter is too small | Excess reaming stock, tool loading and chip removal |
| Prepared diameter is too close to final size | Insufficient stock for the intended finishing cut |
| Prepared position is wrong | Setup or drilling origin and method; reaming tends to follow the error |
| First reamed hole measures unexpectedly large or rough | Verify the measuring method, stock, tool runout, alignment, wear and cutting conditions before changing a setting |
Verify Depth, Exit and Results
Select the reamer for the actual access and depth. Check its cutting lead and effective length. On a through hole, verify the lead can pass far enough through the lower side to finish the specified length while clearing anything underneath. For a blind hole, the space for the lead and chips can limit the full-diameter depth. Choose a tool and preparation appropriate to the requirement. Use manufacturer guidance for coolant, chip flow and feed; the flute form and coolant delivery can be specific to the tool.
The control’s canned cycle describes motion. A Haas mill G85 is a feed-in, feed-out boring cycle that can suit a planned finishing operation requiring a controlled withdrawal. G81 is the basic drilling cycle with a rapid retract. Choose a cycle and settings compatible with the selected tool and verified hole/fixture geometry. Trace Z depth, return height, and the spindle state on withdrawal.
A size reading answers whether the finished opening is within the required diameter range. A dimension or feature-control frame can separately constrain the hole’s location. Check it using a method appropriate to the drawing. A bore gage or diameter limit plug does not independently establish that location. Record both checks where specified before turning the first piece into a production run.
For example, assume the drawing gives a size range of 10.000 to 10.015 mm. A measured size of 10.008 mm is within the size range. If inspection against the specified datums shows the location is outside its tolerance, the hole still fails the drawing. Reporting the actual size and the separate location result lets the next operator investigate the correct part of the process. Before measuring, check for chips, burrs, or other conditions that would compromise the gage contact.
Sources: NIMS CNC mill competency crosswalk, Kennametal RMS tool and allowance data, Guhring reaming technical guidance, and Haas G85.
A 10.000-mm reamer needs 0.250 mm allowance on diameter. What prepared diameter gives that allowance?
9.750 mm
9.500 mm
9.875 mm
10.250 mm
A drilled hole is in the wrong XY position. Why should the operator investigate the drilling setup before reaming it?
The reamer removes only the floor of the hole.
The reamer changes its cut to a thread automatically.
Reaming zeroes the X and Y machine axes.
A reamer tends to follow the prepared bore and may leave the location error.
What extra condition matters when selecting a reamer for a specified finished diameter down to a blind-hole depth?
The distance from the machine home switch to the program cursor
Whether the available bottom space accommodates the cutting lead and chips
Whether the tool pocket number matches the hole diameter
Whether return-to-machine-zero mode is absolute
Sections you finish are checked off in the contents.