About Us
Durmapress specializes in designing, manufacturing, and selling various metal processing equipment, including bending machines, shears, punches, and laser cutting machines. The company was founded in 2014, with years of experience and technology accumulation. DurmaPress has become one of the well-known brands in China's metal processing machinery industry.
Contact Us
Recent Posts
Categories
Follow Us
Weekly New Video
Table of Contents
A drawing says 100 mm. The part measures 99.94 mm. Is that a defect?
The answer depends entirely on the tolerance written on that drawing. Sheet metal fabrication produces a range of results, not a single exact value, and tolerance is how engineers define the width of that acceptable range.
Set it correctly and parts assemble without adjustment. Set it too loosely and components rattle, leak, or misalign. Set it too tightly and you pay for precision the part never needed — sometimes several times over.
This guide gives you the typical tolerance ranges first, then explains what drives them: material behavior, process capability, forming variables, drawing standards, and the accumulation of small deviations across multiple operations.
1. Sheet Metal Tolerance Chart
The table below shows tolerance ranges commonly used for planning in general sheet metal fabrication. Use it to set expectations early in design, then confirm the values with your manufacturer.
| Process | Feature | Indicative Planning Range |
|---|---|---|
| Laser cutting | Flat profile and hole size | ±0.1 – ±0.3 mm |
| CNC punching | Hole size and position | ±0.1 – ±0.2 mm |
| Press brake | Bend angle | ±0.5° – ±1° |
| Press brake | Linear dimension after bending | ±0.2 – ±0.5 mm |
| Welding | Assembly dimensions | ±0.5 – ±2 mm or wider |
| Raw sheet | Thickness | Per material and mill standard |
Important: These are indicative planning ranges only. Actual capability depends on material, thickness, part size, machine configuration, tooling condition, number of operations, and inspection method. They are not a universal industry standard and should not be treated as a guaranteed specification.
Three patterns are worth noting before the detail:
- Flat features are the easiest to control. The sheet is fully supported and the geometry is two-dimensional.
- Accuracy degrades as operations accumulate. Cut → formed → welded, in that order.
- Angular tolerance behaves differently from linear tolerance. Its real-world impact grows with flange length, which the next sections explain.
2. What Are Sheet Metal Tolerances?
A sheet metal tolerance is the permitted deviation between the dimension on the drawing and the dimension on the finished part.
If a flange is specified as:
100 ± 0.5 mm
any measurement from 99.5 mm to 100.5 mm is acceptable.
Two common misreadings are worth correcting:
- A tolerance is an acceptance limit, not a prediction. A capable process clusters near the nominal value rather than at the extremes.
- Tighter is not automatically better. A tolerance should protect function. Beyond that point it only adds cost.
2.1 Why Sheet Metal Parts Need Tolerances
Most drawings operate on two levels.
General tolerances apply to every dimension without an individual callout, usually stated once in the title block.
Specific tolerances are written directly on a dimension and always override the general note.
A practical allocation for sheet metal parts:
2.2 General vs Specific Tolerances
Most drawings operate on two levels.
General tolerances apply to every dimension without an individual callout, usually stated once in the title block.
Specific tolerances are written directly on a dimension and always override the general note.
A practical allocation for sheet metal parts:
| Feature | Approach |
|---|---|
| Mounting holes that mate with another component | Specific, tighter |
| Enclosure dimensions constrained by an existing space | Specific |
| Sealing and gasket surfaces | Specific |
| Interfaces with machined parts | Specific |
| Cosmetic edges, clearance zones, non-mating faces | General |
Applying tight tolerances to every dimension is one of the most expensive and most common drawing errors in sheet metal work.
2.3 Bilateral vs Unilateral Tolerances
How a tolerance is written changes how the part is made and inspected.
| Format | Example | Acceptable Range | Typical Use |
|---|---|---|---|
| Bilateral | 100 ± 0.5 mm |
99.5 – 100.5 mm | Most general dimensions |
| Unequal bilateral | 100 +0.5 / −0.2 mm |
99.8 – 100.5 mm | When drift is safer in one direction |
| Unilateral | 100 +0.2 / −0.0 mm |
100.0 – 100.2 mm | Clearance or interference fits |
| Limit dimensions | 99.9 – 100.1 mm |
As stated | When absolute clarity is required |
Unilateral tolerances matter more than they appear. A slot that must never be undersized, or a panel that must never exceed an opening, should be toleranced in one direction rather than symmetrically. This single choice often prevents assembly rejections without tightening the total tolerance band at all.
3.Common Types of Sheet Metal Tolerances
Different features fail in different ways, so drawings control them separately.
3.1 Dimensional and Hole Location Tolerances
Dimensional tolerances cover the measurements that determine whether parts physically fit:
- overall length and width
- flange length after forming
- hole diameter and slot width
- hole-to-edge distance
- hole-to-hole distance
- hole-to-bend-line distance
One distinction explains a large share of real assembly failures: holes located on a single flat face inherit only cutting accuracy, which is highly repeatable. Holes located on different faces separated by bends inherit the variation of every forming operation between them.
Wherever possible, keep critical mating holes on one plane.
3.2 Bend Angle Tolerances
Angular tolerance defines how far a formed angle may deviate:
90° ± 1°
Angular tolerance deserves special attention because its consequence scales with flange length. The same ±1° produces a negligible offset on a short flange and a significant one on a long flange — a point examined with real numbers later in this guide.
The dominant cause of angular variation is springback, the elastic recovery that occurs when forming pressure is released.
3.3 Thickness and Flatness Tolerances
These describe the material rather than the fabrication.
Thickness is supplied to a mill tolerance, and gauge numbers are nominal designations. The same gauge corresponds to different thicknesses in steel, stainless steel, and aluminum. Because thickness feeds directly into springback behavior and developed length, thickness variation quietly shifts formed dimensions.
Flatness matters most on panels, doors, covers, and mating or sealing surfaces. Distortion originates from residual rolling stress, thermal input during cutting or welding, and handling. Thin sheets deform under process forces; thicker plate can spring out of flat when cutting releases internal stress.
3.4 Shape and Position Tolerances
Controlling size alone does not guarantee a usable part. Geometric controls address form and relationship:
- Flatness — deviation of a surface from a true plane
- Perpendicularity — how square a flange is to a reference face
- Parallelism — whether two faces remain evenly spaced
- True position — permitted shift of a hole axis from its theoretical location
A cabinet door that rocks, a flange that finishes at 89°, or a bolt pattern that drifts across a long panel are geometric problems, not size problems. Complex assemblies generally require GD&T with clearly defined datums so every party measures from the same reference.
4. Typical Sheet Metal Tolerances by Process
The chart at the top of this guide gives the summary. This section explains what drives each range.
4.1 Laser Cutting and Punching
Flat features are the most controllable stage of the process. The sheet is supported, the geometry is two-dimensional, and CNC positioning is highly repeatable.
Factors that still affect the result:
- kerf width and beam compensation, which influence small features more than large profiles
- thermal input, which can distort thin material and narrow islands
- minimum feature size relative to thickness — very small holes may not cut cleanly
- edge proximity, since features close to an edge weaken the part and shift more easily
- punch and die clearance and wear
- cumulative positioning error across a long series of punch hits
Cutting behavior varies significantly between material types, so understanding how fiber laser cutting handles different materials helps explain how that variation carries forward into every downstream dimension.
4.2 Sheet Metal Bending Tolerances
Bending is where most dimensional problems originate, because forming changes the material rather than simply removing it.
Three outputs must be controlled simultaneously:
- Bend angle — governed mainly by springback and material consistency
- Flange length — governed by backgauge positioning and flat pattern accuracy
- Distance between bends — governed by cumulative positioning and developed length
The flat pattern deserves particular attention. If the developed length is calculated using an assumed K-factor or an assumed inside radius that does not match the tooling in use, every formed dimension shifts even when the machine performs perfectly.
To prevent this problem, learn how to calculate bend deduction correctly, because an inaccurate flat pattern produces out-of-tolerance flanges regardless of how precise the press brake is.
One distinction buyers frequently misread: machine repeatability is not part tolerance. Repeatability describes how consistently the ram and backgauge return to a commanded position. Part tolerance additionally includes material variation, tooling condition, handling, and part geometry.
4.3 Welding and Assembly Tolerances
Welding introduces concentrated heat, producing expansion, contraction, and residual stress. Components that are individually correct can still produce an assembly outside specification.
Practical controls:
- fixtures that restrain parts during welding and cooling
- balanced weld sequences that distribute heat rather than concentrating it
- stitch welding instead of continuous welds where strength permits
- allowance for post-weld straightening or machining on critical features
- assembly tolerances specified separately from component tolerances
5. Why Sheet Metal Parts Go Out of Tolerance
When parts drift out of specification, the cause almost always falls into one of four groups.
5.1 Material and Thickness Variation
Material behavior is the most underestimated variable in forming:
- Actual thickness often differs from nominal gauge and can vary within a single sheet.
- Yield strength differs between lots of the same grade, changing springback.
- Stainless steel typically springs back more than mild steel; aluminum behaves differently again.
- Grain direction affects minimum bend radius, consistency, and cracking risk.
A shop that produced perfect parts last month and rejects this month has often changed nothing except the material lot.
5.2 Bend Radius, Springback and Bend Allowance
These three interact, and errors here are systematic rather than random:
- In air bending, the actual inside radius is largely a function of the V-die opening, not the punch tip.
- Springback means the commanded angle and the achieved angle differ, so overbending is required.
- Bend allowance and K-factor determine developed length. A wrong assumption shifts every flange by a consistent amount.
Because the error is consistent, it is correctable — usually by measuring a test bend and updating the bend table with real values rather than generic chart figures.
For a more reliable starting point, review the validated K-factor values for common materials, while remembering that values confirmed for your specific material and tooling combination are far more reliable than generic reference numbers.
5.3 Tooling, Backgauge and Crowning
Machine setup determines how much theoretical accuracy actually reaches the part:
- Punch and die condition — worn tooling produces inconsistent radii and angles
- V-die selection — changing the opening changes the radius and therefore the developed length
- Backgauge accuracy — positioning error translates directly into flange length error
- Ram and bed deflection — under load, the center of a long bend can open relative to the ends
- Crowning — mechanical or hydraulic compensation counteracts that deflection
- Angle measurement and correction — compensates automatically for material variation
This makes choosing the right press brake tooling essential, because tooling condition and selection quietly control the inside radius, which in turn controls the flat pattern.
5.4 Part Size and Design Complexity
Geometry itself limits achievable tolerance:
- Long parts amplify angular deviation and are more sensitive to deflection.
- Large thin panels bow easily and are difficult to handle without distortion.
- Every additional bend adds another opportunity for variation.
- Parts requiring reorientation between bends accumulate positioning error.
- Short flanges, deep boxes, and non-standard radii may require special tooling and reduce repeatability.
6. How Tolerance Stack-Up Affects Bent Parts
Tolerance stack-up occurs when several individually acceptable variations combine into an unacceptable result.
Consider an enclosure formed from a single blank, with mounting holes on opposite walls. Each bend between those holes can shift position and tilt the wall. Both bends may sit comfortably within their angular tolerance, yet the distance between the two holes can drift far beyond what a matching lid will accept.
This is why parts pass dimensional inspection and still fail at assembly. Every callout was satisfied; the relationship between features was never controlled.
The effect grows with:
- the number of bends between two related features
- the distance from the bend line to the feature
- flange length, which converts angular error into positional error
- the number of separate components in the assembly
6.1 Practical Example: Why a 90° Bend Can Still Fail Assembly
Angular tolerance is often accepted without checking what it means in millimeters. Here is the calculation that changes how engineers specify it.
Part conditions:
| Parameter | Value |
|---|---|
| Material | Mild steel |
| Thickness | 2 mm |
| Bend angle | 90° |
| Angular tolerance | ±1° |
| Flange length | 200 mm |
The positional deviation at the flange tip is:
Deviation=L×tan(θ)
For a 200 mm flange at 1° of angular error:
200×tan(1°)=200×0.01746≈3.49 mm
The result: a bend measured at 89° or 91° — fully inside the ±1° tolerance — moves the flange tip by roughly ±3.5 mm.
Now compare flange lengths at the same ±1°:
| Flange Length | Approximate Tip Deviation |
|---|---|
| 20 mm | ±0.35 mm |
| 50 mm | ±0.87 mm |
| 100 mm | ±1.75 mm |
| 200 mm | ±3.49 mm |
| 300 mm | ±5.24 mm |
Two conclusions follow directly:
- A single angular tolerance is not equally strict across a part. The same ±1° is tight on a short bracket and loose on a tall enclosure wall.
- Opposing walls compound the problem. If two walls both lean outward at the tolerance limit, the opening between them can shift by roughly double the single-wall value before any other error is considered.
This is why an enclosure can pass angle inspection and still refuse to accept its own lid. When flanges exceed roughly 150–200 mm and must mate with another component, specify angular tolerance based on the permitted positional deviation, not on a habitual ±1°.
6.2 How to Reduce Tolerance Stack-Up
The most effective fixes are design decisions rather than machine settings:
- Keep mating features on one plane. Holes cut on a single flat face inherit cutting accuracy, not forming accuracy.
- Dimension from a common datum. Chained dimensions pass error from one feature to the next.
- Design in adjustment. Clearance holes, slots, and floating hardware absorb small deviations.
- Respect distance from bends. Features too close to a bend line distort and shift.
- Control bend sequence. A consistent sequence and reference edge improves part-to-part repeatability.
- Prototype complex parts. A first article costs far less than an unusable production run.
7. How to Read Sheet Metal Tolerances on a Drawing
Most tolerance disputes are interpretation problems rather than manufacturing problems. Reading a drawing correctly takes four checks.
7.1 Check the General Tolerance Note
Look at the title block first. It usually contains a single note that governs every dimension without its own callout. Everything else on the drawing is read against that baseline.
7.2 Identify Specific Tolerances
Any dimension carrying its own tolerance overrides the general note. These are the features the designer considered critical, and they define where inspection effort belongs.
Watch for conflicts: a title block note and an individually toleranced dimension should never contradict each other in intent.
7.3 Interpret the Tolerance Format
Confirm whether the callout is bilateral, unequal bilateral, unilateral, or expressed as limit dimensions. 100 ± 0.2 mm and 100 +0.4 / −0.0 mm share the same total band but describe completely different acceptable parts.
7.4 Read the Geometric Callouts
Feature control frames specify flatness, perpendicularity, parallelism, or true position, along with the datum references. For formed parts, these controls often matter more than size tolerance, because they define how the part behaves in an assembly rather than how it measures in isolation.
Also confirm the measurement condition: whether a dimension applies to the flat blank or to the formed part, and whether the part is inspected free-standing or restrained.
8. ISO Standards for Sheet Metal Tolerances
Standards exist so that designers and fabricators interpret the same drawing identically. They define acceptance criteria — they do not describe what a specific machine or shop can achieve.
8.1 What Does ISO 2768-m Mean?
ISO 2768-1 provides general tolerances for linear and angular dimensions without individual callouts, organized into four classes:
| Class | Description |
|---|---|
f |
Fine |
m |
Medium |
c |
Coarse |
v |
Very coarse |
A title block note of ISO 2768-m applies the medium class to all un-toleranced linear and angular dimensions.
Two details are frequently missed:
- The permitted deviation is not one value. It varies with the nominal dimension range, so a 20 mm dimension and a 500 mm dimension have different limits under the same class.
- Angular general tolerances are typically tied to the length of the shorter leg, meaning short flanges are permitted more angular deviation than long ones.
8.2 ISO 2768-2 and ISO 22081
Legacy drawings often show a combined callout such as ISO 2768-mK, where the second letter refers to general geometrical tolerances.
Check the current status before relying on it: ISO 2768-2:1989 is listed by ISO as withdrawn, with ISO 22081:2021 identified as the new version. Older drawings still reference the withdrawn part, so both appear in practice.
The practical rule: follow the standard and edition stated on the drawing or contract, and verify requirements against the controlled document rather than a summary table.
8.3 ISO Tolerances vs Shop Capabilities
A general tolerance states what will be accepted. It does not confirm that a given process route can deliver it.
- Laser cutting may comfortably meet a tight class on flat features.
- The same part may not meet that class after bending, because forming adds variation.
- Welded assemblies usually require looser limits than their components.
For critical work, ask the manufacturer to confirm achievable tolerance for the complete process route, and validate it with first-article inspection rather than assumption.
9. How to Choose Practical Tolerances
Effective tolerancing balances function, process capability, and cost.
A workable sequence:
- Define what the part must actually do — fit, seal, align, move, or carry load.
- Identify the features that control those functions.
- Assign specific tolerances only to those features.
- Apply a realistic general tolerance to everything else.
- Consider the full process route before finalizing values.
- Review the drawing with the manufacturer before release.
9.1 When Tight Tolerances Are Necessary
Precision earns its cost when the feature controls function:
- hole patterns that must align with a mating component
- enclosure dimensions constrained by an existing space or rack
- sealing and gasket surfaces
- interfaces with machined parts, bearings, or linear guides
- interchangeable parts in service and spare-part programs
- safety-critical or regulated assemblies
9.2 When Tight Tolerances Add Cost Without Value
Unnecessary precision drives cost through several mechanisms simultaneously:
- longer setup, calibration, and test bending time
- slower cycle times and reduced throughput
- special tooling or additional operations
- more frequent and more detailed inspection
- higher scrap and rework rates
- fewer suppliers willing to quote the work
The impact is not proportional. Tightening a tolerance past a certain point changes the required process, not merely the effort within the existing process — and that is where cost rises sharply.
10. How to Improve Sheet Metal Bending Accuracy
Most accuracy problems are solved through disciplined routine rather than new equipment.
- Measure the actual material. Check thickness with a micrometer and record the lot.
- Confirm the real inside radius. Bend a test coupon using production tooling and measure the result.
- Reverse-calculate the bend deduction. Use measured flanges and a known blank length instead of a generic chart value.
- Update the bend table. Store validated values by material, thickness, and tooling combination.
- Verify backgauge calibration. Positioning error appears directly in flange length.
- Inspect tooling. Check wear, damage, and alignment before any tight-tolerance run.
- Confirm die selection. The V-opening sets the radius that every calculation depends on.
- Apply crowning on long bends. Keep the angle consistent from end to end.
- Use angle measurement where material varies. Automatic correction reduces dependence on operator experience.
- Run and verify a first article, then monitor critical dimensions during production, especially after a material change or tooling swap.
Review how to select the correct V-die opening before the first production bend, because die selection determines the radius your flat pattern assumes.
10.1 Matching Press Brake Features to Tolerance Requirements
When process discipline is not enough, the limitation is usually machine configuration. This table maps common accuracy problems to the capability that addresses them.
| Accuracy Problem | Capability That Helps |
|---|---|
| Flange length varies between parts | CNC control with programmable backgauge |
| Complex parts with multiple reference edges | Multi-axis backgauge |
| Angle differs between center and ends of a long bend | Crowning system |
| Angle drifts when material lots change | Angle measurement and automatic correction |
| Inconsistent results between operators | Stored programs and repeatable setups |
| Deep boxes and short flanges | Application-specific tooling and gauging |
| High-volume repeatability requirements | Servo control, automation, or robotic bending |
You can compare CNC press brake series and configurations, but the right configuration depends on the part and its tolerance requirements, not on a general accuracy claim.
To recommend a configuration responsibly, a machine supplier needs the part drawing, material and thickness, bend length, required angular and dimensional tolerance, and production volume. Any accuracy promise offered without that information should be treated cautiously.
11. Sheet Metal Tolerance Checklist
Use this before releasing a drawing or starting a production run:
- Critical fit and assembly features identified
- Material grade, thickness, temper, and grain direction confirmed
- Flat-pattern dimensions separated from post-bend dimensions
- Critical dimensions referenced to a common datum
- Hole-to-edge and hole-to-bend distances verified
- Angular tolerance checked against flange length in millimeters
- Bend radius, K-factor, and bend sequence agreed
- General and specific tolerance notes checked for conflicts
- Measurement method and inspection stage defined
- Test bend or first article scheduled for complex parts
- Achievable tolerance confirmed with the manufacturer
12.FAQ
There is no single standard tolerance covering sheet metal fabrication. The achievable value depends on the process route, the material, the thickness, and the part geometry. A realistic approach is to define the tolerance per feature and per operation, then confirm the complete route with the manufacturer before production.
For planning purposes, laser-cut flat features are often held in the range of ±0.1 to ±0.3 mm, bend angles around ±0.5° to ±1°, and welded assembly dimensions considerably wider. These are indicative ranges rather than guaranteed values, and they shift with thickness, part size, and equipment.
No. Cutting removes material from a supported flat sheet, while bending permanently deforms it. Forming adds springback, thickness sensitivity, and positioning variables, so post-bend dimensions normally require wider tolerances than the same dimensions in the flat pattern.
Two reasons. First, material stretches at the bend, so an inaccurate developed length shifts every downstream feature. Second, holes located too close to a bend line deform during forming. Increasing the distance from the bend and validating the flat pattern usually resolves both.
No. Gauge is a nominal designation, and the same gauge number corresponds to different thicknesses in steel, stainless steel, and aluminum. Actual thickness also varies within the mill tolerance, which is why measuring material before tight-tolerance bending is standard practice.
It applies the medium class of general tolerances from ISO 2768-1 to all linear and angular dimensions without individual callouts. The permitted deviation changes with the nominal dimension range, and any specifically toleranced dimension overrides the general note.
ISO lists ISO 2768-2:1989 as withdrawn, with ISO 22081:2021 as the new version. Older drawings may still reference it, so follow the standard and edition stated on the drawing or contract and verify against the controlled document.
No. Springback, thickness variation, and grain direction differ between materials and even between lots of the same grade. Machine repeatability is consistent; material behavior is not. Angle measurement and correction systems reduce this variability but cannot eliminate it.
13.Conclusion
Sheet metal tolerances are not just numbers in a title block. They determine whether a part assembles cleanly or consumes hours of rework.
Key points to carry into your next project:
- Tolerance should follow function. Tighten only the features that control fit, sealing, alignment, or safety.
- Flat cutting accuracy and formed part accuracy are different. Neither predicts the other.
- Angular tolerance must be evaluated in millimeters at the flange tip, not only in degrees.
- Most bending deviation traces back to material variation, actual bend radius, springback, and the flat pattern — all measurable and correctable.
- Tolerance stack-up across multiple bends causes more assembly failures than any single out-of-spec dimension.
- Standards define acceptance criteria; process capability determines what a shop can actually deliver.
The most reliable improvement path is straightforward: measure the real material, validate the real radius with a test bend, update your bend data, calibrate the backgauge, apply crowning on long parts, and verify the first article before running the batch.
If your parts require consistent bend angles, repeatable flange dimensions, or tight dimensional tolerances, DURMAPRESS can review your part drawing and recommend a press brake configuration based on your material, thickness, bend length, tolerance requirements, and production volume.
You can send us your part drawing and tolerance requirements so our engineering team can advise on the bending setup that matches your accuracy and production needs.
Stay Updated on Industrial Innovations
Subscribe to our newsletter for the latest insights on manufacturing technology, sustainability, and industry trends.
