Boring is a preferred method of producing accurate sized holes in manufacturing.

Boring offers distinct benefits over other hole making strategies such as reaming. Hole boring comes with a unique set of rules. This guide helps address those rules and will aid in maximising the cost benefits of your boring bar investment.

General Rule

The general rule in boring is to keep the boring bars to a minimum length. At the early stages of any production planning, maximum effort must be put into a machining strategy that will keep boring bars as short as possible.

In new projects the only limiting factor should be the length of the bore.

Machine (spindle) choice and fixture design should be highly characterised by the impacts of boring tool length.

Stability is greatly increased with larger spindles.

Rigibore and the Rigibore global distributor network will directly support you with your installation of tooling. This guide should be used as a way of best directing questions to Rigibore so when technical support is required we can quickly help your application.

Obtaining Quotes for Boring Bars

There are a number of factors that should be considered in the early stages of a manufacturing process that requires accurate hole production (boring).

The following is required to quote for a suitable boring bar:

  • Part drawings or key dimensions (length of the bore, diameter, tolerances required, critical relationships between features).
  • Material specifications
  • Fixturing & fixture clearances
  • Spindle type
  • Thru coolant
  • Maximum weight of tool
  • Tool change moment
  • Boring process...
    • Stock removal
    • Combination tooling (combined features on one tool or combined semi finish and finishing operations).

Tool Design

Tools will be designed from the component print and machine specifications. Recommendations will be made with regard to the boring process.

In designing the tool the Rigibore team will use experienced knowledge to maximise tool efficiency while minimising deflection and vibration.

As a fundamental rule, tools will be kept as short as possible.

On packages, tools will be combined where possible to reduce the investment needed to perform the machining operation.

Decisions will be made that, where possible, will reduce negative impacts of cutting forces on the bar.

These including cutting geometry, component selection, balancing and in some cases recommendations may be made to change the process variable or cutting technologies, such as depth of cut to maximise the efficiency of the boring bar.

Once a tool is designed the cutting technologies can usually be adjusted to achieve optimum results for the tool.

Quoting Process

In the quoting process a Rigibore applications engineer will design the tooling to the previously stated criteria. Each quote is given a reference number and all data relating to this quote request is securely stored against this reference.

Drawings are produced detailing the key dimensional characteristics of the tooling.

A quotation file breaking down the costing and options for individual tools and hardware will be sent along with the PDF drawings of the tools.

Sign Off

As with all bespoke tooling, Rigibore will expect to recieve a sign off print from the end user. As part of the sign off procedure end users should consider:

  • Critical dimensions of the tool in relation to the part
  • Clearance dimensions for fixtures
  • Clearance dimensions for machine tool change functions
  • Maximum weights and tool change moments
  • Insert selection and supply


Delivery of special tools is often shorter than expected, but it's still a good idea to plan well in advance:

  • Boring tools for all parts of the process, roughing, semi-finishing and finishing
  • Sister tools or backup tooling
  • Inserts
  • Pull studs
  • Coolant tubes
  • Tools for adjustment of cutting edges

Presetting Requirements

Required Consider Notes
1.0 Required PPE
  • Gloves
  • Eye protection
  • Ear plugs
  • Protective footware
Safety is a key priority (risk assessment)
2.0 Presetter
2.1 Correct spindle adaptor Adaptors can change the usable length of a presetter. Enure that the presetter is long enough with the correct adaptor
3.0 Tool drawings RADS printout contains all the required information to set the tool
4.0 Inserts Correct size
4.1 Correct grade
4.2 Correct geometry
4.3 Correct nose radius
5.0 Pull studs Details of the correct pull stud can be found on the machine tool
6.0 Coolant tubes Some shanks like HSK require separate coolant tubes - Failure to fit can damage spindle seals
7.0 Balluff chips Tool ID chips used for storing unique IDs and setting data
8.0 Adjusting tools
9.0 Blue tack Used for cleaning cutting edges when using non-contact measurement to preset tooling
10.0 Engineering blue

Setting Up Tooling

All CNC tooling should be treated as a precision product. Extra care should be taken not to damage tapers, connecting surfaces or introduce contaminating dirt onto connection surfaces.

Rigibore tools are preset before shipping with gauge inserts. However, you will need to fit inserts and adjust preset dimensions prior to first use.

Action Notes
11.0 Setup presetter
11.1 Clean all connecting adaptor faces and assemble presetter components
11.2 Calibrate presetter Calibration hardware/software supplied by the presetter manufacturer
12.0 Unpack the tool Required adjustment tools may be fastened to the outside of the packaging
12.1 Keep any reusable packaging for future storage of the tooling
12.2 Fit required pull stud or coolant tube Correct torques must be applied to pull studs, over tightening can deform tapers causing performance problems or damaging spindles
12.3 Clean the tool taper and insert into presetter adaptor
12.4 Ensure the correct adaptor program is selected on the presetter
12.5 Clamp tool into presetter ensuring for good connection
13.0 Starting with the tool furthest from the taper carefully remove the insert screw with the correct torx key and fit the insert to the pocket Ensure correct radius of insert
13.1 Visually inspect for good seating Ensure there are no gaps between the pocket and the insert base. If unsure use a piece of shim to check for any clearances, if you cannot seat the insert, check for debris in the pocket or on the base of the insert, clean and repeat check
13.2 Tighten the insert screw Ensure for an element of pull back roughly 1/4 turn on the insert screw
13.3 Clean cutting edge using blue tack This removes any contamination that may affect non contact measurement systems on most modern presetters
13.4 Using the presetter, measure the position of the cutting edge and course adjust Make course adjustment > ±0.1mm, if required, to length first then the diameter
13.5 Repeat items 13.0 to 13.5 until rough setting is complete on all edges of tool
14.0 Establish critical component or reference dimensions for tooling Combination tools may contain a number of cutting edges, some of these edges may have critical relationships such as two blind holes. Other features may be relative but not critical to these features, for example a chamfer
14.1 Starting with the critical or reference edge, adjust to finish size. Continue to adjust all edges to finish size
15.0 Make a note of all edge positions and note and double check tool offset dimensions required for the machine
15.1 Clearly label tool as set

Run Offs Requirements

The most important part of this phase is the planning and pre assessment of the expected results.

As with all machining processes the entire process must be monitored and controlled to achieve tight tolerances and good process stability or a high CPK.

Besides the tooling there are many factors that impact the performance of hole boring processes.

Criteria Details Notes
Material variation Material variance has a huge impact on boring bars Hardness, inclusions, chemical composition
Core shift For boring processes the start process is usually a pre-formed hole. This may be pre-cast or pre-forged or it may be pre-drilled
Fixture/component positioning
Fixture/component clamping forces
Program datum positioning
Coolant supply
Details Notes
16.0 Required PPE
  • Safety glasses
  • Safety shoes
  • Ear protection
  • Gloves
17.0 Machine tool access Access to a guarded machine tool with all required safety features fitted including interlocks and guards
18.0 Parts Access to test parts
19.0 Programs Pre written programs, verified with correct offset requirements, required spindle orientations and clearance distances
20.0 Offsets Tool length offset measurements
21.0 Measurement equipment Manual methods of measuring tool cutting results
22.0 Start point speeds and feeds Estimated speeds and feeds for the tool based on standard industry prerequisites See specific section on speeds and feeds

Calculating Start Point Speeds & Feeds

To calculate a starting point for speeds and feeds you need specific information about the tool.

  • Largest cutting diameter of the tool
  • Material

Start points for speeds and feeds are calculated but are only a starting figure. They are based on the surface speed and the feed rate, outlined below.

Speeds & Feeds Calculator Tool

Surface Speed

Surface speed is the speed that the material moves past the cutting edge of the tool. So in boring operations the diameter is theoretically unwound. A constant RPM is applied based on a known surface speed which will give a technically established starting point.

Material Surface Speed m/min (carbide)
Steel 150
Stainless steel 100
Cast iron 250
Nodular cast iron 100
Aluminum 1000

Calculate the RPM using the following equation:

RPM = Cutting speed/π x Diameter

Feed Rate

The feed rate is the axial speed at which the boring bar is fed through the component. This feed rate will have an impact on surface finish.

Starting point feed rate for all boring operations is between 0.1 - 0.2mm per revolution.

Run Off

The following instructions should be carried out for each of the tools used in the operation.

This could be a rough boring bar, semi finishing boring bar or just a finish boring bar.

  • Roughing tools - set to size
  • Finishing tools - set to undersize

See section below on establishing a preset size.

Action Notes
23.0 Load part to machine fixture
23.1 Check fixture clamping
23.2 Check bore location to program datum
24.0 Pre-check program with tool removed from machine
25.0 Load tool to machine

Clean taper before inserting into machine. It's also worth double checking the following:

  • Tool length offset (in machine)
  • Tool weight - some tools may need to be set as large or heavy in the tool change settings on the machine
  • Tool change moment
  • Tool orientation for offset moves
26.1 Run cycle
27.0 Measure part
28.0 Adjust tool See notes (below) on established preset size for finish tooling

Established Preset Size

Because of the impact of deflection on boring bars they will not ultimately cut the size that they are set to. For this reason it is necessary to establish a preset size.

Establishing a preset size is relatively simple but many factors have a dramatic influence on the deflection.

Criteria Details Notes
Depth of cut Depth of cut affects the loading on the cutting edge which will ultimately affect push off and affect the cut size It's important to maintain a reasonable depth of cut for all operations
Insert wear Flank wear is the natural wearing of insert due to the abrasive wear mechanism Cutting times are estimated at around 15 minutes of contact for cutting edges. This can be affected by insert grades, coatings and applications.
Semi finish or rough bore size Semi finishers and roughers play an important part in maintaining a reasonable depth of cut for the finishing operation If the semi finish or rough size is dramatically changed this will increase the depth of cut on the finishing tool
Coolant supply Coolant supply - helps evacuate chips, helps prevent insert problems and removes heat from the workpiece. It also aids in cooling chips helping to fracture swarf into manageable chips

The most effective way to set a finish tool is to take half the stock off at a time.

Typically a finishing operation should be maximum of between 0.1 - 0.2mm depth of cut on radius.

Finishing tools are generally single point so that there is one effective cutting edge that can be used to hold size, this can have a negative impact on push off as the cutting edge is not supported.

Action Notes
30.0 Measure the semi pre finished bore size to establish the depth of cut for the finishing operation
31.0 Use engineering blue to mark the pre bore sides
32.0 Preset the finishing tool to only clean up the pre finished bore
33.0 Run tool through program making small adjustments until the pre finished hole is cleaned up by undersized
34.0 Measure the bored hole
35.0 Adjust the tool to remove the remaining stock
36.0 Adjust the tool to remove the remaining stock
37.0 Load a new part to machine
38.0 Run cycle
39.0 Measure result
40.0 Adjust tool to achieve finished size

Solutions to Common Problems

Problem Possible Cause Solution
Poor sizing/difficulty holding tolerance Cleanliness Clean tool holder and spindle mounting faces
Insert mounting (sufficient pullback) Check for pull back on insert
Unit or cartridge rigidity
  • Check that the cartridge or unit is correctly fitted and seating properly
  • Check that the cartridge or unit are being operated within the recommended range with the correct radius insert
Material variance
Roughing setup - depth of cut
Core shift
Datum offsets
Coolant supply
Swarf nesting Insert geometry (chip breakers)
Feed rate too low Increase feed rate
Chatter/vibration Cleanliness
Length diameter ratio
Poor finish Feed rate too high Decrease feed rate
Chip evacuation
Ovality Fixture clamping
Roughing tool setup
Excessive insert wear Excessive flank wear
  • Reduce cutting speed
  • Review and select a more resistant grade of insert
Crater wear Select insert with more positive geometry
Plastic deformation
Built up edge
Broken inserts Excessive load
  • Check for program errors (rapids)
  • Reduce depth of cut
Grade too brittle
Geometry too weak
Insert too small
Feed too high
Speed too high

Other Companies in the Bassett Group