Design rules such as choosing fits, chamfers and reliefs, and easy-to-machine shapes. 12 terms. For each term: meaning, how to show it on a drawing, examples, common mistakes, and differences between JIS and ASME.
Printed from Kezuriba (kezuriba.net/en/drafting/design/)
Choosing a fithameai no erabikataselection of fits
Choosing the combination of hole and shaft tolerance classes from the function: whether the parts move, are fixed, or are disassembled. Start from a hole basis such as H7 and choose from the recommended combinations table.[1][2][3][4]
Choose the fit by function: a clearance fit for moving parts, a transition fit for locating, an interference fit for press-fit fixing. Start from an H7 hole and choose from the recommended combinations.
How to write it on the drawing
Classify by functionGet a first estimate from the function: clearance fits for parts that move relative to each other, around h and js for locating by hand and for parts that are disassembled, and k through p and beyond for fixed parts assembled with a hammer or press.[1]
Choose from the recommended tableChoose from the recommended hole-basis combinations in JIS B 0401-1.[2]
ExampleMISUMI's explanation: for a precision locating pin used in an H7 hole, it gives g6 on the side fixed to the base plate and h6 on the locating side as an example, and says to choose a combination with larger clearance where play is acceptable.[3]
Common mistakes
Using a fit more precise than necessaryWhy: machining and inspection take more effort, and manufacturing cost goes up.Fix: use the minimum accuracy the function requires.[5][1]
Using an interference fit at a point that gets disassembledWhy: it is hard to disassemble without damaging the parts.Fix: for points that are disassembled or replaced, use a combination that can be assembled and removed without damaging the parts.[1]
Standard: JIS B 0401-1:2016 (recommended fits).[2][6]
A hole drilled about 10-20% larger than the thread's outside diameter so that a bolt can pass through. Unlike a fit, the diameter values written on the drawing differ between the hole and the bolt.[4]1 source (for reference)
Clearance hole: the hole a bolt passes through is drilled larger than the thread's outside diameter (e.g., φ11 for M10, chosen from the standard table). The figure draws the clearance exaggerated.
How to write it on the drawing
Decide the diameters from the standard tableBolt hole diameters and counterbore diameters are specified in JIS B 1001.[7]
Common mistakes
Making both holes of the two fastened parts threadedWhy: The bolt engages both and cannot be assembled.Fix: make one a clearance hole and the other a threaded hole.[8]
Standard: JIS B 1001 "Clearance holes and counterbores for bolts and screws".[7]
C (45° chamfer)Chamfers (C chamfer, corner rounding)mentorichamfer / edge break
Cutting a part's corner at an angle (C chamfer) or rounding it (R). C is a supplementary dimension symbol for a 45° chamfer, written like "C2". Corners across the whole drawing are often specified together in a note.[9][10][11]
Chamfers: a 45° chamfer is written as C plus the length, like "C2". For other than 45°, give the length and angle as dimensions. Small corner chamfers and fine edge breaks are specified together in a note.
How to write it on the drawing
A 45° chamfer is C plus a dimensionWrite it like "C1" or "C0.5".[9][10]
Specify corners together in a notePut it together in a note, such as "Unspecified corners C0.3 MAX, with no burrs or turned-up edges".[10]
Make entries for press-fit and locating largeChamfer the entry of a hole that receives a part generously so that it goes in easily.[12][13]
Common mistakes
Not specifying corner treatmentWhy: burrs remain, jam into locating surfaces and cut hands during assembly.Fix: specify corner chamfers and no burrs together in a note.[14][15][10]
JIS and ASMEThe C symbol for 45° chamfers is a provision JIS Z 8317-1 added to its corresponding international standard (ISO 129-1). The same notation is not necessarily understood on drawings abroad.[11]
Standards: JIS Z 8317-1:2008 (based on ISO 129-1, with added JIS provisions such as 45° chamfers) and clause 11.6 of JIS B 0001:2019. For edges whose shape is not defined by dimensions, see JIS B 0051.[11][16][17]
A rounding on the inside corner of a pocket or step. When cut with a rotating tool such as an end mill, the inside corner is always rounded to the tool radius.[18][19]
Inside corner radius: when cut with a rotating tool, the inside corner of a pocket or step is always rounded to the tool radius. Give the corner radius explicitly or add a note such as "Unspecified corners R1 MAX".
How to write it on the drawing
Give the corner radius or a general noteThere are examples of a note such as "Unspecified corners R1 MAX".[10]
TerminologyUS teaching materials call an inside rounding a fillet and an outside rounding a round.[19]
Common mistakes
Drawing the inside corner of a pocket square (sharp corner)Why: with a rotating tool the inside corner is rounded to the tool radius, so it cannot be made as drawn.Fix: add a radius at least as large as the tool radius, or use a relief shape.[18]
Standard: no standard specifically governing inside corner radii could be confirmed in this research.
Relief and relief groovenige / nige-mizorelief / undercut / neck
A shape in which the root of a step or part of a contact surface is cut away in advance so that the tool corner radius, burrs, incomplete thread and the like do not interfere with the mating part.[20][14][15][21]
Relief (relief groove): with a groove at the root of a stepped shaft, the mating part's corner does not hit the leftover tool radius, so it seats flush against the shoulder face. Reliefs are also provided at thread ends and grinding ends.
How to write it on the drawing
Groove at the root of a stepped shaftCut a groove (neck) at the step where the diameter changes, so that the mating part's corner is not obstructed even if the tool radius remains.[20]
Groove at the end of a threadA groove smaller than the root diameter at the end of an external thread lets the mating thread engage all the way, and also serves as tool runout for thread cutting.[20]
How to dimensionShow the groove width and depth with a leader note or dimensions.[20]
Corners of contact surfaces and places where burrs formProvide reliefs at corners of fixture contact surfaces and where burrs form.[14][15]
Common mistakes
No relief at the root of a stepWhy: the tool radius remains, and the mating part's corner hits it so the parts do not seat tightly.Fix: provide a relief groove or chamfer the mating side.[20]
Standard: no standard defining the shape and dimensions of relief grooves could be confirmed in this research.
A taper applied to faces parallel to the mold-opening direction so that injection-molded parts and the like release easily from the mold.[22][23]1 source (for reference)
Draft: a taper applied to faces parallel to the mold-opening direction so that the molded part releases easily. Often about 2°, and larger on textured surfaces (Protolabs guidelines).
How to write it on the drawing
On all faces parallel to the mold-opening directionFor sections released by a slide, apply it to faces parallel to that release direction.[22]
Typical anglesProtolabs' guidelines give 0.5° on vertical faces, 2° in many cases, 3° or more for lightly textured surfaces, and 5° or more for medium textures.[23]
Common mistakes
Designing with no draft, as if it were a machined partWhy: the part drags against the mold on release, causing scratches and deformation.Fix: add draft to faces parallel to the mold-opening direction.[22]
Standard: no JIS defining draft angles could be confirmed in this research.
The wall thickness of a molded part. Uneven thickness tends to cause short shots, warpage from differential shrinkage, and sink marks and voids in thick sections, so keep it as uniform as possible.[22][23]1 source (for reference)
Wall thickness: if the wall thickness of a molded part is uneven, thick sections tend to show sink marks and voids, and differential shrinkage causes warpage. Core out thick areas and keep the thickness as uniform as possible.
How to write it on the drawing
Core out thick areasDo not make features with bumps and recesses solid; use a cored-out shape.[22]
Recommended range by materialEach resin has a recommended wall thickness range (in Protolabs' guidelines, 0.045-0.140 in for ABS).[23]
Common mistakes
Making walls extremely thin on machined partsWhy: it falls below the limit of what can be machined.Fix: Protolabs' machining guidelines recommend a feature thickness of at least 0.51 mm and an overall part thickness of at least 1.02 mm.[18]
Standard: no JIS defining wall thickness could be confirmed in this research.
Datum face (for machining, assembly, and function)kijunmenreference surface / datum surface
The surface used as the origin for dimensions and for machining, assembly and measurement. Choose it with thought to the surface that mates in assembly, the origin for layout and measurement, and the surface that sits on the machine tool table, and give dimensions from it.[4][8][24][25]
Datum surface: decide the surface that mates in assembly or serves as the measurement origin, and give dimensions from it (here, parallel dimensions from the left end face).
How to write it on the drawing
Types of datumsThere are machining datums, mounting datums and functional datums.[8]
Dimension from the datumUse parallel dimensioning to give each position from the datum surface.[4][26]
End-face datum and centerline datumEnd-face datums are often used for high-precision assemblies, but for ordinary automated-machine parts, a centerline datum (symmetric dimensioning) reduces errors in developing part drawings and in assembly.[24]
Common mistakes
Dimensioning without thinking through the machining sequenceWhy: the machinist has to calculate positions, which adds mistakes and effort.Fix: starting from the stock, mentally walk through which surface each feature is machined from and how many mm away, and check the dimensions.[4]
Dimensions symmetric about the centerlinechushin furiwake no sunpodimensioning from center line
A method of dimensioning symmetric holes and shapes by distributing the dimensions to both sides of the part's centerline. It omits unnecessary dimensions, makes the drawing easier to read, and reduces assembly mix-ups.[24][8]
Dimensions symmetric about the centerline: for two symmetric holes, give only the hole spacing "60" from the part's centerline. This removes unnecessary dimensions and reduces assembly mix-ups.
How to write it on the drawing
Take the centerline as the datumGive the spacing of symmetric holes and the outline as dimensions straddling the centerline, and do not give position dimensions from the end faces.[24][8]
ExampleTwo holes 30 either side of the center: give only "60" between the holes from the centerline, and no position from the end faces.(An example built from the rules in the sources)[24][8]
Balancing tolerance and costkosa to kosutotolerance and cost
The idea that the tighter the tolerance, the more machining and inspection effort and the higher the cost, so apply tolerances only where function requires and leave the rest to general tolerances.[5][8][27]
How to write it on the drawing
Choose which dimensions get tolerancesApply tolerances only to dimensions that matter for function and assembly, and leave the others to general tolerances. Improve the finish only on surfaces that need it.[5]
ExampleMISUMI example: in a part drawing for a chuck jaw, dimensional tolerances are applied only to the slot width and sensor hole that matter for alignment, finish is improved on just three surfaces, and the rest is left rough.[5]
Common mistakes
Putting tight tolerances on every dimension out of cautionWhy: the machining cost of holding tolerances is added to every dimension.Fix: identify the dimensions that matter for function and apply tolerances only there.[5]
Layout of bolt holes and threaded holesboruto ana no haichihole pattern layout
How to lay out and dimension threaded holes and bolt holes on a base plate or cover. A layout that lets locating be done for several holes together reduces machining time and mistakes.[28][29]
Bolt hole layout: place the four corner holes of a rectangular cover at the intersections of two lines parallel to the edges, not following the corner arcs. Locating can be done together, so machining is faster and mistakes are fewer.
How to write it on the drawing
Align the locatingAlign holes on the same X and Y lines so that locating can be done together.[28]
ExamplePlacing the four corner holes of a rectangular cover at the intersections of two lines parallel to the edges, rather than along the outline's corner arcs, lets all holes be located at once and cuts cost.[28]
Common mistakes
Laying out holes along the outline arcWhy: Each hole needs separate locating, which raises machining cost.Fix: use a layout that lets locating be done together.[28]
Edge condition (burr and turned-up edge indication)ejji no jotaiundefined edge / burr-free edge
Specifying in a note, for edges whose shape is not defined by dimensions, matters such as leaving no burrs or turned-up edges. JIS B 0051 defines how to indicate dimensions for edges of undefined shape.[10][17][15]
Edge condition: for corners whose shape is not defined by dimensions, specify together in a note that no burrs (protrusions) or turned-up edges (rollover) remain.
How to write it on the drawing
General indication by noteWrite a note such as "Unspecified corners C0.3 MAX, with no burrs or turned-up edges".[10]
ExampleNote on the Shimane University drawing example: "Unspecified corners C0.3 MAX, with no burrs or turned-up edges".[10]
Standard: JIS B 0051 "Technical product documentation - Edges of undefined shape - Indication of dimensions" (details of its contents could not be confirmed in this research).[17]
Explanations without a mark are those on which two or more sources from different publishers agree. Because the text of the standards is paid, they were checked against technical materials from measuring-instrument and parts manufacturers, teaching materials from universities and public testing institutes, and public pages of the standards, and the explanations are written in Kezuriba's own words. The diagrams of the entry fields were drawn by Kezuriba.