Dimensional Tolerance Selection: What You Must Know When Ordering Precision Metalwork

What exactly is dimensional tolerance?

Simply put, no machine, no matter how advanced, is capable of manufacturing a part to an absolutely perfect nominal dimension. The machining process is influenced by numerous variables: machine tool rigidity, tool wear, vibrations, and even ambient and coolant temperatures.

Dimensional tolerance is the permissible, predetermined deviation from the nominal (ideal) dimension that still guarantees the correct functioning of the part. It is the difference between the upper and lower limit dimensions.

• Nominal dimension: The base dimension to which the tolerance refers (e.g., shaft Ø20 mm).
• Upper and lower limit dimensions: The maximum and minimum allowable actual dimensions.
• Tolerance zone: The difference between the upper and lower limit dimensions.

Example: The notation 20 ±0.1 means a nominal dimension of 20 mm, with a permissible upward deviation of 0.1 mm (max. 20.1 mm) and downward deviation of 0.1 mm (min. 19.9 mm). In this case, the tolerance zone is 0.2 mm.

Why Chase “Zero” Blindly? (The Downside of Over-Tolerancing)

A common mistake in machine component design is tightening tolerances excessively—often referred to as “over-tolerancing.” Designers frequently add hundredths of a millimeter everywhere “just to be safe,” assuming that more accurate always means better. This approach is flawed for several reasons:

1. Exponentially Increased Costs: The cost of manufacturing a part does not scale linearly with accuracy. Tightening a tolerance from ±0.1 mm to ±0.01 mm can multiply the price several times over. This often requires:
• A shift in manufacturing technology (e.g., from milling to grinding or Electrical Discharge Machining – EDM).
• The use of more expensive, high-precision tooling.
• More rigorous quality control (e.g., measurements on a Coordinate Measuring Machine – CMM).
• Frequent tool wear compensation.
2. Extended Lead Times: Higher precision typically means slower feed rates, more finishing passes, and more time spent on in-process measurements. The manufacturer will require significantly more machine time to complete such a part.
3. Higher Risk of Scrap: With very tight tolerances, the probability of a part failing to meet requirements increases, generating material waste and requiring the production process to start over.

The Golden Rule of Tolerance Selection in Precision Metal Machining

The golden rule is: Tolerances should be as wide as possible without compromising the functionality of the part, and only as tight as absolutely necessary.

How to achieve this in practice?

1. General Tolerances and Machining Tolerances (ISO 2768): Not all dimensions on a part are critical. The external dimensions of an enclosure housing or the depth of a bolt hole do not require micrometer-level accuracy. For such dimensions, general (or workshop) tolerances are applied, typically defined by the ISO 2768 standard or specified as the standard tolerances for a given machine shop. This range usually sits around ±0.1 mm to ±0.2 mm, depending on the accuracy class. Sourcing a project within this class guarantees optimal cost and lead time without unnecessary complications. All non-critical dimensions should fall under this standard, while tight tolerances should only be assigned where essential.

2. Fits Analysis: The Key to Proper Mechanism Functionality: Fits occur where two or more parts interact with each other (e.g., a shaft and a bearing, a slider and a guideway, or a positioning pin and a hole). This is where tolerance selection is critical to the project’s success. A fit that is too tight will prevent movement or assembly; a fit that is too loose will cause runout, vibration, and premature wear of the mechanism. In subtractive metal machining, fits are most commonly designated by tolerance classes according to the ISO system (e.g., H7/g6).

There are three main groups of fits:

• Clearance Fits (Running/Sliding Fits): These guarantee clearance between mating parts. They are used for sleeve bearings, guideways, or hinges. Examples include H7/f7 (frequently used for rotating elements with moderate clearance), H8/f7, and H8/e8 (larger clearance, e.g., crankshaft and journal bearings under hydrodynamic lubrication). In this type of fit, the upper limit of the shaft dimension is always smaller than the lower limit of the hole dimension.
• Transition Fits: Depending on the actual dimensions of the components within their tolerance limits, assembly may result in either a slight clearance or a slight interference. These are primarily used for locating parts without heavy dynamic loads, where precise coaxial alignment is the priority but assembly and disassembly should not require excessive force. Examples include H7/js6 (light locating fit) and H7/k6 (frequently used for rolling-element bearings on shafts).
• Interference Fits (Press/Shrink Fits): These guarantee that one part is pressed into another without any clearance, creating a rigid connection that should not rotate or slide freely. They are useful for joining components operating under load, such as gears on shafts mounted without keys. Examples include H7/p6 (light interference fit, e.g., for mounting bearings in housings subjected to shock loads) and H7/s6 (heavy interference fit, requiring a press or temperature differential for assembly). Here, the upper limit of the hole dimension is smaller than the lower limit of the shaft dimension.

The designer must carefully select the type of fit (per ISO), as it dictates specific tolerance zones to the manufacturer (on the order of hundredths or sometimes thousandths of a millimeter). These typically require final finishing operations such as grinding or reaming.

3. Geometric Dimensioning and Tolerancing (GD&T)

Linear dimensioning with a tight tolerance (e.g., ±0.02 mm) is often not enough on its own. What good is a shaft with the correct diameter if it is slightly oval or bent (warped into an arc)? In advanced applications, it is essential to implement geometric dimensioning and tolerancing (GD&T). These define the permissible deviations of the part’s actual geometry.

The most critical geometric tolerances include:

• Flatness: Specifies how much a surface can deviate from an ideal plane. This is absolutely critical for sealing surfaces, machine bases, or linear guideways, where a flatness error of just a few micrometers can cause leaks or excessive wear on mating components. Manufacturers achieve high flatness primarily through surface grinding, or less frequently, precision finish milling on highly rigid machine tools.
• Coaxiality: Mandates that the axes of two different cylindrical elements (e.g., two bearing journals on a single shaft) lie on the same centerline, within a permissible deviation defined by a cylindrical tolerance zone. A lack of coaxiality is the most common cause of vibration in high-speed rotary drive systems, leading to a drastic reduction in the drivetrain’s lifespan. Achieving proper coaxiality often requires turning or grinding in a single setup, or using centering centers.
• Parallelism and Perpendicularity: Define the relative position of two surfaces or axes. These are required, for example, when mounting bearings in housings, in angular guides, or for the datum elements of positioning mechanisms. Failing to maintain correct angles and parallelism can jam linear motion or lead to improper force distribution. These are frequently verified on precision surface plates using dial indicators, or measured via a coordinate measuring machine (CMM).
• Radial and Axial Runout: This is a composite tolerance controlling both form (circularity, flatness) and location (coaxiality) for a rotating component. It specifies the maximum variation in a dial indicator reading during a full rotation of the part around a designated datum axis (e.g., the shaft axis relative to which a gear journal’s runout is inspected). This is a critical parameter for turbine rotors, machine tool spindles, or drive shafts. Exceeding it immediately causes dynamic imbalance, resonance, and system failure during operation. Achieved through hard turning or precision cylindrical grinding, it requires perfect centering and rigid clamping on the machine tool.

Understanding and applying GD&T allows for a much more precise definition of requirements for the manufacturer than simply adding +/- 0.01 to a dimension. It also forces the designer to analyze “what actually needs to be accurate.”

4. Tolerancing in the Context of Heat Treatment and Finishing

Another aspect affecting dimensioning strategy involves the processes a part undergoes after machining. This is an area where the manufacturer’s expertise is invaluable, and the client must account for **machining allowances** (stock material).

• Heat Treatment (Hardening, Quenching and Tempering): Steel changes volume and undergoes deformations (shrinkage and expansion) during heating and rapid cooling. The more complex the shape (large differences in cross-sections), the higher the risk of warping. If a part needs to maintain a tolerance of, for example, ±0.05 mm or tighter after hardening, the process is **always** designed so that the final, high-precision surfaces (such as bearing raceways or mating shaft surfaces) are machined with an appropriate allowance before hardening. After heat treatment, the part is sent for grinding or processed using hard turning/milling technology. The client should indicate the final dimensions and tolerances for the hardened part on the drawing. The selection and size of these allowances within the manufacturing workflow are typically planned by the manufacturing engineer on the machine shop’s side.
• Galvanic Coatings and Paint Coatings: Layers of chromium, zinc, hard anodizing, or powder coating have their own thickness (ranging from a few to several dozen micrometers). This must be kept in mind when designing interference fits and precise tolerances like H7. The manufacturer must receive clear guidelines from the client stating whether the drawing dimensions apply “before” or “after coating,” allowing them to pre-compensate the machining process for the coating thickness (e.g., thread dimensions).

5. Material Matters

Different materials exhibit distinct machinability, dimensional stability after removing the outer surface layer (due to the release of internal residual stresses), and coefficients of thermal expansion.

• Mild Steel and Aluminum: Generally easy to machine, but very tight geometric tolerances can be difficult to maintain in thin-walled or large-scale components due to the low rigidity of these alloys, clamping forces, and elevated temperatures generated during machining. This is particularly true for copper due to its high density, thermal conductivity, and “gummy” structure.
• High-Strength Alloy Steels: These hold dimensions well during the machining process (minimal deformation during grinding) and allow for precise finishing with excellent surface roughness (low Ra).
• Difficult-to-Machine Materials and Superalloys (Inconel, Titanium, etc.): These require a completely different manufacturing approach, highly rigid and precise machine tools, and premium-grade tooling. They generate the most heat during cutting, which leads to severe residual stresses in the surface layer of the workpiece. Consequently, maintaining tight tolerances on these materials significantly drives up the baseline costs of carbide tools and indexable inserts, increasing the overall project budget.
• Plastics (POM, PEEK, Polyamide/Nylon, Polyethylene): Caution is required when applying strict tolerances. Plastics are highly susceptible to elastic deformation when clamped in machine tool fixtures. Thermal expansion caused by heat generated during machining is also a major factor; applying liquid emulsion coolants is often not feasible. Tolerances tighter than 0.05 mm frequently “drift” once thermal stabilization occurs. Furthermore, certain plastics (like Polyamide) absorb ambient moisture, up to several percent of their own weight. As a result, a dimension may inspect perfectly on a CMM at the machine shop, yet swell by up to a tenth of a millimeter by the time the part arrives at the customer’s facility. Generally, machining tolerances for most thermoplastics should be specified within a rougher tolerance class, such as 0.1 to 0.2 mm. Ultra-tight tolerances measured down to 1–2 micrometers on a CMM are primarily reserved for very expensive, high-rigidity polymers (like PEEK), whose machinability more closely resembles that of an aluminum alloy.

Summary: How to Make Life Easier for Yourself and the Manufacturer

Sourcing precision metal machining involves more than just handing over a 3D model (which contains no tolerances and defaults to perfect nominal dimensions). It is a communicative process based on understanding the limitations and capabilities of manufacturing technology.

Here is a compilation of proven best practices when preparing Requests for Quotes (RFQs) and engineering documentation for subtractive metal machining.

1. Use 2D Engineering Drawings: While 3D models are necessary for generating toolpaths in CAM software for 4-axis and 5-axis NC machining centers, only 2D engineering drawings contain dimensional tolerances, GD&T callouts, and required surface roughness classes. Submitting an RFQ without a 2D drawing forces the manufacturer to produce the entire part according to general ISO 2768 standards, which omits tight tolerance zones required for dowel pins, bearings, or press fits.
   
   
2. Specify the Surface Roughness Class: Surface roughness directly impacts dimensional accuracy and is an essential component of precision machining quality. Grinding a toleranced hole to an H7 fit for a bearing requires simultaneously defining the surface finish (e.g., an Ra value of 0.4 to 0.8 µm). A standard rough finish from a cutting tool can cause play between a shaft and a bushing once the surface peaks flatten out under operational loads. Finer dimensional and geometric finishes demand stricter requirements for the surface layer structure (Ra / Rz / Rmax). This typically increases the number of manufacturing steps—for example, replacing a single drilling operation with a drill-and-endmill pass followed by final precision reaming using a TiN-coated reamer at low feed rates with liquid coolant, significantly driving up cycle times and tooling costs. RFQs should always specify the optimal machining finish and context (e.g., surface ground, finish turned with flood coolant, etc.).
   
   
3. Tolerance Only What is Critical: Apply general tolerances on 2D drawings for all non-critical sections of CNC-machined parts (such as sensor enclosures, threaded standoffs, or raw stock chamfers and edge breaks). Use standard ISO 286 limits and fits systems for mating shafts and holes. Avoid blindly adding ten-thousandths of a millimeter (e.g., ±0.001 mm) to titanium, heat-treated parts, or non-functional assembly interfaces. Such sub-micron tolerances are typically reserved for master shafts, gauge blocks, or micrometer calibration components in laboratory environments, which are measured at exactly 20°C in specialized metrology facilities. In industrial engineering, the most common standard for precision tolerances falls within hundredths or tenths of a millimeter relative to a base parameter (e.g., 15 mm ±0.05 mm for the production of hard-anodized, masked, non-stick blister sealing molds made of PVC).
   
   
4. Be Open to Dialogue: An experienced manufacturer will often suggest minor design or geometry modifications—or even consolidating two parts into a single monolithic component via 5-axis CNC turning/milling—to reduce costs, optimize workholding on trunnion-style NC mills, and minimize machining allowances. This technical feedback is invaluable, as the CAM programmer and machinist are ultimately responsible for achieving the final tolerance zones on the shop floor. Correct tolerance selection should not be an arbitrary restriction; it should be the result of understanding the manufacturing process to build a high-performing mechanism within an optimized budget.