JIS Tolerance Chart: JIS B 0405 General Tolerances vs. ASME
Open a drawing from a Japanese customer or supplier and look near the title block (表題欄, hyodai-ran). You will often find a short note such as 普通公差 JIS B 0405-m (futsu kosa, "general tolerance") or JIS B 0419-mK. Those few characters set the tolerance for every dimension and feature that has no tolerance of its own.
The good news is that these JIS standards are translations of ISO standards. JIS B 0405 was prepared from ISO 2768-1 without changing its technical content, so "JIS B 0405-m" gives the same values as "ISO 2768-m" for linear and angular dimensions. The catch is in how the drawing is read. Japanese drawings follow the ISO independency principle, not the ASME Y14.5 Rule #1 (envelope principle) that many US engineers work with. The same "Ø20±0.1" can mean different things in each system.
This guide gives you the JIS general tolerance chart, explains how size tolerances and geometric tolerances work on a Japanese drawing, compares JIS with ASME Y14.5, and ends with a checklist of what to confirm with the Japanese side.
Contents
- What "JIS B 0405-m" Means on a Japanese Drawing
- JIS General Tolerance Chart (JIS B 0405 / ISO 2768-1)
- Size Tolerance vs. Geometric Tolerance
- Geometric Tolerances in JIS: B 0021, B 0022, and ISO 1101
- JIS vs. ASME Y14.5: Independency Principle vs. Rule #1
- Choosing Tolerances by Function
- Tolerance Design: Function, Process Capability, Inspection
- Checklist: What to Confirm with the Japanese Side
- Limits of This Guide
- Summary
- FAQ
- Sources
What "JIS B 0405-m" Means on a Japanese Drawing
Writing a tolerance next to every dimension would bury a drawing in numbers. Instead, the designer gives individual tolerances only where the function needs them and covers everything else with one general tolerance note. JIS B 0405 sets these general tolerances for linear and angular dimensions in four classes:
- f: fine (精級, seikyu)
- m: medium (中級, chukyu)
- c: coarse (粗級, sokyu)
- v: very coarse (極粗級, gokusokyu)
When the standard number and class, such as "JIS B 0405-m," appear in or near the title block, that class applies to every dimension without an individual tolerance. The standard covers parts made by metal removal (machining) or formed from sheet metal. Castings and molded plastic parts have their own general tolerance standards, so the right standard depends on the manufacturing process.
Geometric characteristics such as flatness and perpendicularity have a separate general tolerance standard, JIS B 0419, with three classes: H, K, and L. A note such as "JIS B 0419-mK" combines both: class m from JIS B 0405 for dimensions, and class K from JIS B 0419 for geometry.
JIS General Tolerance Chart (JIS B 0405 / ISO 2768-1)
The tables below list the permissible deviations in JIS B 0405. Because JIS B 0405 is a translation of ISO 2768-1:1989, the values are the same as the ISO 2768-1 tables. The larger the dimension and the coarser the class, the wider the tolerance.
Permissible deviations for dimensions without an individual tolerance. Find the size range in the left column, then read across to the class on the drawing.
| Size range | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 to 3 | ±0.05 | ±0.1 | ±0.2 | – |
| Over 3 to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| Over 6 to 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| Over 30 to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| Over 120 to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| Over 400 to 1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| Over 1000 to 2000 | ±0.5 | ±1.2 | ±3 | ±6 |
| Over 2000 to 4000 | – | ±2 | ±4 | ±8 |
| Size range | f, m | c, v |
|---|---|---|
| 0.5 to 3 | ±0.2 | ±0.4 |
| Over 3 to 6 | ±0.5 | ±1 |
| Over 6 | ±1 | ±2 |
| Shorter side | f, m | c | v |
|---|---|---|---|
| Up to 10 | ±1° | ±1°30′ | ±3° |
| Over 10 to 50 | ±0°30′ | ±1° | ±2° |
| Over 50 to 120 | ±0°20′ | ±0°30′ | ±1° |
| Over 120 to 400 | ±0°10′ | ±0°15′ | ±0°30′ |
| Over 400 | ±0°5′ | ±0°10′ | ±0°20′ |
"–" means the class sets no value for that range. For sizes below 0.5 mm, the tolerance must be given next to the dimension. The angular tolerance controls only the general orientation of the lines, not their form. Compiled from JIS B 0405:1991, Miki Pulley's JIS B 0405 excerpt, and published ISO 2768-1 tables. Check the official standard before using these values for acceptance.
A worked example (fictional): a machined bracket drawing says "JIS B 0405-m," and an untoleranced length reads 50. The size range "over 30 to 120" in class m gives ±0.3, so any length from 49.7 to 50.3 is acceptable. If the same drawing said "JIS B 0405-f," the range would tighten to 49.85–50.15.
General Geometric Tolerances (JIS B 0419)
JIS B 0419 is the JIS translation of ISO 2768-2:1989. It sets general tolerances for geometric characteristics in three classes, H, K, and L. Straightness, flatness, perpendicularity, symmetry, and circular runout have values in its tables. Other characteristics, such as roundness and parallelism, are derived from the size tolerance and related values instead.
Tolerances for features with no individual geometric callout, by class H, K, or L.
| Nominal length | H | K | L |
|---|---|---|---|
| Up to 10 | 0.02 | 0.05 | 0.1 |
| Over 10 to 30 | 0.05 | 0.1 | 0.2 |
| Over 30 to 100 | 0.1 | 0.2 | 0.4 |
| Over 100 to 300 | 0.2 | 0.4 | 0.8 |
| Over 300 to 1000 | 0.3 | 0.6 | 1.2 |
| Over 1000 to 3000 | 0.4 | 0.8 | 1.6 |
| Shorter side | H | K | L |
|---|---|---|---|
| Up to 100 | 0.2 | 0.4 | 0.6 |
| Over 100 to 300 | 0.3 | 0.6 | 1 |
| Over 300 to 1000 | 0.4 | 0.8 | 1.5 |
| Over 1000 to 3000 | 0.5 | 1 | 2 |
| Characteristic | H | K | L |
|---|---|---|---|
| Circular runout | 0.1 | 0.2 | 0.5 |
For flatness, use the longer side of a rectangular surface or the diameter of a circular one; for straightness, use the length of the line. Symmetry is omitted here. Compiled from Miki Pulley's JIS B 0419 excerpt. Check the official standard before using these values for acceptance.
Note that ISO withdrew ISO 2768-2 in 2021 and replaced it with ISO 22081:2021, which no longer uses the H, K, and L classes. Japanese drawings that call out JIS B 0419 still refer to the H/K/L tables. If your own drawing system has moved to ISO 22081, agree with the Japanese side on which rules apply before you redraw the part.
Reading Title Block Callouts
| Callout on the drawing | What it means |
|---|---|
| JIS B 0405-m | General tolerances for linear and angular dimensions, class m (medium) |
| JIS B 0419-mK | Class m from JIS B 0405 for dimensions, plus class K from JIS B 0419 for geometric characteristics |
| JIS B 0419-K | Class K general geometric tolerances only, with no JIS B 0405 class given |
| JIS B 0419-mK-E | As mK, plus the envelope requirement (E) applied to every single feature of size (one cylindrical surface or two parallel planes). Not suitable for stock material |
| ISO 2768-mK | The ISO form of the same callout |
Size Tolerance vs. Geometric Tolerance
A size tolerance such as "50±0.1" accepts any size from 49.9 to 50.1; the tolerance is the difference between the two limits, 0.2 in this case. It controls only the distance between two points, though. It says nothing about how flat a surface is, where a hole sits, or whether a shaft is bent. Geometric tolerances fill that gap by controlling form, orientation, location, and runout (wobble when the part rotates).
In short, size tolerances control how big a feature is, and geometric tolerances control its shape and position. A modern drawing needs both. Each does a different job, and only together do they capture what the designer needs from the part.
The split is between size on one side and form, orientation, and location on the other.
Since JIS B 0401-1:2016 and JIS B 0420-1:2016, JIS uses the term "size tolerance" (サイズ公差, saizu kosa) in place of "dimensional tolerance" (寸法公差, sunpo kosa). On the shop floor, sunpo kosa is still the common term.
The 2016 revisions also renamed the basic size. In current JIS documents it is the "nominal size" (図示サイズ, zushi saizu). Under these standards, a size with no modifier is judged by two-point size, the local distance measured between two opposite points. Keep the wording and this default in mind when you compare a new Japanese standard with older drawings or training material.
Related: How to Read Japanese Engineering Drawings (JIS B 0001)
Three Ways to Write a Size Tolerance
A Japanese drawing shows a size tolerance in one of three ways. Use "±" when the size may vary equally in both directions, separate upper and lower deviations when the tolerance should sit on one side, and a fit symbol when the size depends on how a hole and shaft go together. A tighter range costs more to machine and inspect.
All three set an upper and lower limit of size, and nothing more.
Fits (JIS B 0401)
Where a shaft goes into a hole, the combination of their size tolerances decides whether you get a clearance fit, an interference fit, or a transition fit. The fit system (はめあい, hameai) expresses this with symbols, and JIS B 0401-1:2016 corresponds to ISO 286-1:2010.
Capital letters are for holes, lowercase for shafts, and the number is the tolerance grade (IT grade). In the common H7/g6 fit at around Ø20, the hole is +0.021/0 and the shaft is −0.007/−0.020. There is always some clearance, so H7/g6 is often used for parts that rotate or slide.
Geometric Tolerances in JIS: B 0021, B 0022, and ISO 1101
A geometric tolerance sets how far a feature's form, orientation, location, or runout may deviate from its ideal geometry. JIS B 0021 defines how to show these tolerances on a drawing. The 1998 edition was translated from ISO/DIS 1101 (1996) without technical changes, so the symbols and rules match ISO 1101 of that period.
A size tolerance is a range of lengths, while a geometric tolerance is a zone in space. A flatness tolerance of 0.05, for example, means the whole surface must lie between two parallel planes 0.05 apart.
14 Characteristics in Four Categories
Geometric tolerances fall into four categories: form, orientation, location, and runout. Counted by symbol, there are 14 characteristics, each with its own symbol on the drawing.
Only form tolerances can be applied on their own, without a datum.
Profile of a line and profile of a surface act as form tolerances without a datum and as orientation or location tolerances with one. Coaxiality and concentricity share the same symbol.
In everyday drawings, six of them show up most often:
- Flatness
- Perpendicularity
- Parallelism
- Position
- Coaxiality
- Circular runout
Rather than memorizing all 14, start from what the surface or hole has to do, and work back to the symbol that controls it.
Feature Control Frames and Datums
Geometric tolerances go in a divided rectangle called the feature control frame (公差記入枠, kosa kinyu-waku). From left to right, it holds the characteristic symbol, the tolerance value, and the datum letters, and a leader connects the frame to the surface or hole it controls.
Read from left to right: symbol, tolerance value, datums.
For position, the true location is given by theoretically exact dimensions (basic dimensions), shown in a box and carrying no tolerance of their own. Only the value in the feature control frame sets the allowed deviation.
A datum is the theoretically exact point, line, or plane that a geometric tolerance is measured from. JIS B 0022, whose international counterpart is ISO 5459, also defines a three-plane datum system: three mutually perpendicular datum planes, in a set order of priority, that fix the part's orientation.
Choose datums by where the part actually touches and locates when it is assembled. The mounting face might be the primary datum and the face that a locating pin bears on the secondary datum. As a rule, the datum order should follow the assembly order.
Related: Datum Selection in GD&T: JIS vs ASME on Japanese Drawings
JIS vs. ASME Y14.5: Independency Principle vs. Rule #1
Many engineers assume that if the dimensions are correct, the form will be too. Under ASME Y14.5, Rule #1 makes the size limits control form as well. Under ISO and JIS, a size tolerance does not control form. This is a key difference to keep in mind when you read a Japanese drawing.
The Independency Principle (JIS B 0024 / ISO 8015)
JIS B 0024:2019 is a modified adoption (MOD) of ISO 8015:2011. It states that every requirement on a drawing must be met independently of the others unless a special indication says otherwise. Size is judged as size and geometry as geometry, each on its own.
Size is also judged by two-point measurement unless something else is specified. So a shaft that measures within Ø20±0.1 at every cross section can still pass on size even if the whole shaft is bowed.
Even with every two-point diameter in tolerance, the size tolerance alone does not stop the shaft from bending.
To stop the bend, add a geometric tolerance such as straightness, or add Ⓔ (envelope requirement) to the size. The numbers in the figure are fictional examples.
Sheet-metal and plate parts behave the same way. A 5±0.1 plate can be warped and still pass on size if the calipers read about 5.0 wherever you measure. If the surface must be flat, flatness is a requirement only when the drawing states it. That is the practical meaning of the independency principle.
The Envelope Requirement Ⓔ
To control size and form together on an ISO or JIS drawing, the designer adds the envelope requirement: a circled E after the size tolerance. The feature must then not cross the envelope of perfect form at maximum material size. For a shaft, that envelope is a perfect cylinder at the largest allowed diameter.
With Ⓔ added to the shaft in Figure 7, any bend that breaks out of the perfect Ø20.1 cylinder is rejected. A common approach is to put Ⓔ on mating holes and shafts so they are guaranteed to go together. To apply it to the whole drawing, the title block note can read "JIS B 0419-mK-E."
How ASME Y14.5 Differs
ASME Y14.5 applies the envelope principle by default, known as Rule #1. The limits of size of a feature of size also control its form, so a size tolerance doubles as a form control. ASME also has its own independency symbol for the cases where you want size and form separated.
ISO and JIS work the other way around: independency is the default, and Ⓔ requests the envelope. The same "Ø20±0.1" calls for different form control depending on which standard you read it under. That is why every drawing should state which system it follows.
| Point | JIS / ISO | ASME Y14.5 |
|---|---|---|
| Default relation between size and form | Independent (JIS B 0024 / ISO 8015) | Envelope principle (Rule #1) |
| To make size control form | Add Ⓔ to the size, or "-E" to the general tolerance note | Default; nothing to add |
| To separate size from form | Default; nothing to add | Add the ASME independency symbol |
| Effect of "Ø20±0.1" alone on a shaft | Controls two-point diameters only. A bent shaft can pass | Also limits form: the shaft must stay within a perfect-form boundary at maximum material size |
| Geometric tolerance symbols | JIS B 0021 (from ISO 1101) | ASME Y14.5. Most symbols look alike, but some symbols and interpretations differ |
Choosing Tolerances by Function
Which tolerance a feature needs depends on what it does. Ask first whether it fits into something, locates something, or seats against or rotates on something, and the choice narrows quickly. This is also a useful way to read a Japanese drawing: the callouts tell you which features the designer considered critical.
Decide what each feature does, then choose the tolerance that controls it.
Features That Fit: Size Tolerance and Fits
Where size itself sets the function, as with holes and shafts or keys and keyways, the size tolerance does the work. The fit symbol is chosen by how the parts are used, for example whether they rotate or are fixed.
If the part must always go into its mate, Ⓔ adds form to the guarantee. On fitting features, check that the drawing states the form requirement as well as the size. That check prevents the classic "it won't go in" problem at assembly.
Hole Patterns: Position Tolerance
For features such as flange bolt holes that must line up, datums with a position tolerance suit the function better than ± tolerances on coordinate dimensions. One reason is the shape of the tolerance zone.
If the hole center is toleranced ±0.1 in X and in Y, the zone is a 0.2 × 0.2 square. Whether a hole clashes with its bolt depends on the distance from the true center, though. If the corners of the square are acceptable, a circular zone that allows the same distance in every direction makes more sense.
If the square's corners are acceptable, a circle allowing the same distance in all directions gives a larger zone.
Worked example using a circle whose diameter equals the square's diagonal (0.2 × √2 ≈ 0.28). Real tolerance values come from the clearance between the bolt and the hole.
With position tolerancing, the theoretically exact dimensions in boxes set where each hole should be, and only the value in the feature control frame sets the allowed deviation. Diagonal offsets that would fail the square zone can pass, so yield goes up without any loss of function.
Chained coordinate dimensions have another weakness: the tolerances stack up, and the last hole in the chain drifts the most. Locating every hole by position from one set of datums avoids this and also makes it clear from the drawing which references the inspector should measure from.
Seating and Rotating Features: Flatness, Perpendicularity, Runout
Mounting and sealing faces that seat against a mating part get flatness for the surface itself, and perpendicularity or parallelism for its orientation to a datum. A warped face can cause looseness or leaks once the parts are bolted together.
For bearing and pulley seats on rotating parts, circular runout or total runout controls the wobble as the part turns about its datum axis. Runout is easy to check on the shop floor: set a dial indicator against the surface and rotate the part.
Tolerance Design: Function, Process Capability, Inspection
Tighter tolerances do not automatically mean better quality. Tolerances tighter than needed drive up machining and inspection costs, while loose ones lead to assembly problems or poor performance. Good tolerance design balances three things: function, process capability, and the inspection method.
- Function. State why the feature needs that accuracy, for example the clearance with the mating part, the allowable misalignment at assembly, or vibration in rotation. Then assign size and geometric tolerances to match. When parts stack, run a tolerance stack-up to confirm the combined result still meets the function.
- Process capability. Check that the actual equipment and process can hold the tolerance consistently. The process capability indices Cp and Cpk quantify how much margin the tolerance leaves over process variation. If capability falls short, decide before mass production whether to change the drawing or the process.
- Inspection. Size tolerances can be checked with calipers and micrometers, but geometric tolerances often need a surface plate and dial indicator, a roundness tester, or a coordinate measuring machine (CMM). If the datum setup for measurement is not agreed, the same part can pass for one inspector and fail for another. Agree with quality on what will be measured, and how, at incoming and in-process inspection before the drawing is released.
Related: Cpk 1.33 Explained: Cp vs Cpk, Sample Size, Japanese Specs
Common Mistakes
- Putting tight tolerances on every dimension, which raises cost on features that do not affect function
- Adding geometric tolerances without datums, so nobody knows what to measure from
- Assuming size tolerances also fix form, and leaving out flatness or perpendicularity
- Leaving the general tolerance standard and class out of the title block, so untoleranced dimensions have no clear limits
- Exchanging drawings with overseas partners without agreeing whether they are read under ASME or ISO
In 3D CAD, more companies now attach tolerance and datum information to the model itself so that the drawing and the 3D data state the same requirements.
Checklist: What to Confirm with the Japanese Side
Before you quote, redraw, or inspect a part from a Japanese drawing, these questions clear up most tolerance problems. Use the list as a template for your RFQ or first technical review.
| # | Check | Why it matters |
|---|---|---|
| 1 | Which general tolerance standard and class is stated (for example JIS B 0405-m or JIS B 0419-mK)? If none is shown, what applies to untoleranced dimensions? | The class sets the limits for most dimensions on the part |
| 2 | Is "-E" (envelope requirement) part of the general tolerance note? | It changes how every single feature of size is accepted |
| 3 | Is the drawing read under JIS/ISO (independency) or ASME Y14.5 (Rule #1)? Which editions? | The same size tolerance controls form differently in each system |
| 4 | If you redraw the part in ASME, which features need added form controls or the independency symbol to keep the original intent? | A one-to-one copy of the callouts does not keep the same requirements |
| 5 | Which manufacturing process does the general tolerance assume? Do castings or molded parts on the same drawing follow a different general tolerance standard? | JIS B 0405 covers machined and sheet-metal parts only |
| 6 | Does the customer still want JIS B 0419 (H/K/L), or have they moved to ISO 22081? | ISO 2768-2 was withdrawn in 2021 |
| 7 | Which surfaces are the primary, secondary, and tertiary datums, and how will the part be fixtured for inspection? | Without an agreed datum setup, results vary by inspector |
| 8 | Which features are critical to function (fits, hole patterns, seating faces, rotating seats)? | Tells you where to focus capability studies and inspection |
| 9 | What inspection method and equipment will the customer use for acceptance (two-point size, CMM, runout check)? | Your results need to match theirs |
| 10 | Does the drawing use the newer JIS terms (サイズ公差 saizu kosa, 図示サイズ zushi saizu) or the older ones (寸法公差 sunpo kosa, 基準寸法 kijun sunpo)? | Helps you tell which edition of the standards the drawing was made to |
Limits of This Guide
- The tables here are compiled from published excerpts of the standards. For contract acceptance, use the official JIS or ISO documents in the edition the drawing calls out.
- Some companies add their own drawing standards on top of JIS. When a drawing refers to a company standard, ask for a copy.
- JIS B 0405 covers machined and sheet-metal parts. Castings and molded plastic parts have separate general tolerance standards, which this guide does not cover.
- The ASME comparison covers the default rules only. ASME Y14.5 and the ISO GPS standards differ in many other details, and both are revised over time.
- This guide does not decide how a specific drawing must be read. The contract sets who owns the design and has the final say; when in doubt, get the interpretation in writing before production.
Summary
- "JIS B 0405-m" in the title block gives the same general tolerances as "ISO 2768-m"; for example, ±0.3 for sizes over 30 to 120 mm
- Size tolerances control size; geometric tolerances control form, orientation, location, and runout
- JIS B 0405 and JIS B 0419 fill in where the drawing gives no individual tolerance
- JIS and ISO follow the independency principle, so size tolerances alone do not stop bending or warping. ASME Rule #1 does the opposite by default
- Fitting features use size tolerances with Ⓔ, hole patterns use position, and seating or rotating features use flatness or runout
- Set tolerances by balancing function, process capability, and inspection method
FAQ
Is JIS B 0405 the same as ISO 2768-1?
Yes, in technical content. JIS B 0405:1991 was prepared by translating ISO 2768-1:1989 without changing its technical content, so the tolerance values for each class match. Only the designation differs: "JIS B 0405-m" on a JIS drawing, "ISO 2768-m" on an ISO drawing.
What tolerance does JIS B 0405-m give for a 50 mm dimension?
±0.3 mm. A 50 mm dimension falls in the "over 30 to 120" range, and class m (medium) allows ±0.3 there, so 49.7–50.3 mm is acceptable. Class f (fine) would allow ±0.15.
What does "JIS B 0419-mK" mean on a drawing?
It applies two sets of general tolerances at once: class m from JIS B 0405 for linear and angular dimensions, and class K from JIS B 0419 for geometric characteristics such as flatness and perpendicularity. Adding "-E" (JIS B 0419-mK-E) also applies the envelope requirement to every single feature of size.
Does Rule #1 apply to Japanese drawings?
No, not by default. Japanese drawings follow JIS B 0024, based on ISO 8015, where size and form are independent. To get envelope behavior like Rule #1, the drawing must show Ⓔ on the size or "-E" in the general tolerance note. Confirm this with the Japanese side if you plan to redraw the part to ASME Y14.5.
Which ISO standard matches JIS B 0021 for geometric tolerancing?
ISO 1101. JIS B 0021:1998 was translated from ISO/DIS 1101 (1996) without technical changes. Datums are covered by JIS B 0022, whose international counterpart is ISO 5459.
Sources
- General tolerances: JIS B 0405:1991 General tolerances – Part 1; Miki Pulley, General tolerances (JIS B 0405 / JIS B 0419 excerpt, Japanese); Wevolver, ISO 2768 general tolerances: tables, classes, and current status
- General geometric tolerances: JIS B 0419:1991 General tolerances – Part 2; SIS, SS-ISO 2768-2 (withdrawn, replaced by ISO 22081)
- Geometric tolerancing: JIS B 0021:1998 Geometrical Product Specifications (GPS) – Geometrical tolerancing
- Datums: JIS B 0022:1984 Datums and datum-systems for geometrical tolerances
- Independency principle: JIS B 0024:2019 Geometrical product specifications (GPS) – Fundamentals
- Size tolerance and envelope requirement: JIS B 0420-1:2016 Dimensional tolerancing – Part 1: Linear sizes
- Fits: JIS B 0401-1:2016 Basis of tolerances, deviations and fits
- ASME vs. ISO defaults: Keyence, International industrial standards and GD&T; GD&T Basics, A Comparison of GD&T Standards: ISO GPS vs. ASME Y14.5
Original article in JapaneseThis guide is adapted from a MONOSCOPE article written for readers in Japan: 寸法公差と幾何公差の違い｜図面での使い分けと公差設計の基本
About the editor
MONOSCOPE EditorFOUNDER & EDITORSpent about ten years at a plant equipment maker and a plant engineering company, proposing, designing, and commissioning equipment, then moved into web marketing. Now a web consultant for B2B manufacturers, helping them explain their products and technology. Licensed in Japan as an Energy Manager and a Third-Class Chief Electrical Engineer.
Has run an engineering blog since 2017 (500+ articles) and a Japanese YouTube channel with about 20,000 subscribers. Each English guide is written from the Japanese shop-floor point of view and checked against the cited standards.
