Mechanica Technical Solutions
Home | Contact | About
Manufacturing Processes > Machining processes > Reaming

 

Reaming

 

Process description

The removal of small amounts of material by chip processes using tools of various types with several cutting edges to improve the accuracy, roundness and surface finish of existing cylindrical holes in a workpiece. The tool or the work can rotate relative to each other.

Materials

All metals (mostly free machining).

Reaming

Process variations

  • No special machines are used for reaming. Reaming can be performed on drilling machines, lathes, milling machines and machining centers, or by hand.
  • Basic reamer types include: hand (straight and tapered), machine (rose and fluted), shell, expansion, adjustable and indexible insert reamers. Titanium nitride coatings are sometimes used to increase tool life. Combination drills and reamers are also available.

Economic considerations

  • Production rates ranging from 10–500/h.
  • Lead times varying from short to moderate. Reduced by automation.
  • Minimum amount of material removed.
  • Flexibility high. Little dedicated tooling and generally short setup times.
  • Production volumes usually low to moderate.
  • Can be used for one-offs.
  • Production costs significantly reduced with multiple spindle machines.
  • Tooling costs low.
  • Equipment costs low.
  • Direct labor costs low to moderate. Low operator skill required.
  • Finishing costs low. Cleaning and deburring required.

Typical applications

Any component requiring accurate, cylindrical or tapered holes with good surface finish, either blind or through after a primary hole making operation, typically drilling.

Design aspects

  • Complexity limited to straight or tapered cylindrical blind or through holes.
  • Ideally, reaming allowances should be 0.1mm per 5mm of diameter, i.e. for a finished reamed hole Ø20 mm, the pilot hole should be approximately Ø19.6mm. However, drilled holes prior to reaming should be standard size, wherever possible.
  • Allowances should be made for reamer-end chamfers and the slight taper on some reamers when machining blind holes, although more suited to through holes.
  • Standard sizes used wherever possible.
  • Through holes preferred to blind holes.
  • Sizes ranging Ø3–Ø100 mm.

Quality issues

  • Machinability of the material to be processed is an important issue with regard to: surface roughness, surface integrity, tool life, cutting forces and power requirements. Machinability is expressed in terms of a ‘machinability index’ for the material.
  • Any misalignment between workpiece and reamer will cause chatter, oversize holes and bellmouthing of hole entrance. Piloted reamers ensure alignment of the workpiece and reamer.
  • Most accurate holes are center drilled, drilled, bored and reamed to finished size.
  • Proper maintenance and reconditioning of reamers is required to maintain correct hole size and surface finish requirements. To work efficiently, a reamer must have all its teeth cutting.
  • Pick-up or galling is caused by too much material being removed by the reamer.
  • Selection of appropriate reamer geometry (including relief and rake angles), coolant/lubricant (if required), size of hole, feed rate and cutting speed with respect to material to be machined is important.
  • Reaming is performed at one-third the speed and two-thirds the feed rate of drilling for optimum conditions.
  • Coolant also helps flush swarf from cutting area in long through holes, and blind holes.
  • Surface detail is good.
  • Decreasing feed rate improves surface finish.
  • Surface roughness values ranging 0.4–6.3 µm Ra are obtainable.
  • A process capability chart showing the achievable dimensional tolerances is provided . Note, the tolerances on this chart are greatly influenced by the machinability index for the material used.

costing