Drafting techniques. Preparation of manufacturing drawings. Speciality module. Preparing engineering drawings according to standards EDITION SWISSMEM

Transcription

1 Drafting techniques Preparation of manufacturing drawings Speciality module Preparing engineering drawings according to standards EDITION SWISSMEM

2 Impressum Published by: Title: Edition Swissmem Drafting techniques: Preparation of manufacturing documents Specialty module Preparing engineering drawings according to standards Edition: First edition 2016 Copyright Edition Swissmem, Zürich and Winterthur Order code: XXFMZE 1S e ISBN: Project manager: Joachim Pérez, Swissmem Vocational Training, CH-8400 Winterthur Author: Willi Tschudi, CH-8355 Aadorf Layout and drawings: Daniel Baur, Vocational Training, CH-8400 Winterthur Technical consultant: Prof. Dr.-Ing. Volker Läpple, Steinbeis-Beratungszentrum Konstruktion, Werkstoffe und Normung, D Schorndorf Egon Fässler, Maschinenfabrik Rieter AG, Winterthur Printing: Sources: Purchase from: Copyright Printed in Switzerland Swiss Association for Standardization SNV, DIN e.v., the object designated sources Swissmem Vocational Training Brühlbergstrasse 4 CH-8400 Winterthur Telefon Fax vertrieb.berufsbildung@swissmem.ch All rights reserved. The work and all its parts are protected by copyright. Any use other than as permitted by law requires previous written permission from the publisher.

3 Preparing engineering drawings according to standards 3 Contents / Explanation of symbols Contents: 1. Introduction Objective Basic requirements for the preparation of drawings General tolerances Data quality The changing world of engineering documents 5 2. Machining Machining of a drive shaft Machining of a holder flange Milling Heat treatments/coatings Heat treatment/coating Explanation of surface hardened Explanation of electrodeposited chromium coating ISO 6158-Fe//Cr50hr Injection moulding Injection moulded plastic part Tool-specific dimensions and non-tool-specific dimensions Cast iron/pressure die casting Cast iron ( Connection piece as-cast/ Connection piece finished ) Pressure die casting General tolerances for linear dimensions of castings (DCTG) Datum system for general tolerances for form and position Connection piece Quality class H RAL colours Material designation: Copper-zinc-lead alloy Plate Thermal cutting Extract from ISO Correction factor k for calculating the cutting dimensions of bent workpieces according to DIN Thermal cutting Welding Welded plate part Explanation of carrier Assemblies All parts, assembly drawing Exercises Exercise Tension pulley Exercise Support Exercise Tensioning unit Exercise Drive unit Exercise Monitoring unit Exercise Holder support Check list 74 Explanation of symbols: Important information Solve the problem using the best means available (e.g. text, sketch, CAD)

4 4 Preparing engineering drawings according to standards 1. Introduction For engineering drawings prepared in accordance with the global ISO GPS standards, the rules, concepts and principles in ISO 8015:2011 apply generally (without being specially agreed). 1.1 Objective The drawing examples in this specialty module are intended to illustrate the essential representation in various manufacturing drawings and to assist the reader to correctly interpret the information contained in the drawing. Not all basic concepts are explained. The drawings are only complete inasmuch as they address the described content. The given tolerance values serve only as examples, and must be decided from case to case. The drawing examples were prepared using CAD, and are partly based on third party drawings. Notes regarding CAD drawings: Because organizations have their own CAD rules, each must decide on its own CAD training. Coloured drawing entries: These are covered in the previous theory section. 1.2 Basic requirements for the preparation of drawings An engineer prepares a drawing of a part from an idea and/or as a result of collaboration with specialists in the areas involved. In order for the part to manufactured, the drawing must be complete and unambiguous. A drawing which does not fulfil the prerequisites of complete and unambiguous is unfit for manufacturing and quality assurance purposes. Especially so these days with increased requirements as regards quality and with legal consequences from product liability. Investigations have shown that the majority of drawings are neither complete nor unambiguous. A drawing must fulfil the following requirements: Functionality (the most important requirement) (For transparency, the drawings only show geometrical tolerances which are functionally critical.) Manufacturability (economical manufacture) Inspectability (quality assurance) A drawing which does not meet these requirements wastes time and money in manufacturing and quality management, i.e. is insufficient. 1.3 General tolerances To avoid ambiguity, a general tolerance is stated only once in a drawing.

5 Preparing engineering drawings according to standards 5 1. Introduction 1.4 Data quality High data quality is the basis of team collaboration and process continuity (design and development > manufacturing > documentation). The earlier that mistakes are spotted, the lower the costs. The following rules must be followed: the zero defects principle governs, i.e. aiming for zero defects by good planning. the data user/engineer is responsible for the quality of the CAD models, the layout geometry and the drawing. Layout drawings can also be prepared by the production planners. Drawings must be checked using the four eyes principle at least, i.e. not just by one person. Design drawings are legal documents with regard to product liability, and in the case of damages to persons they can have criminal relevance. Values mentioned in standards are not mentioned explicitly in drawings (data redundancy). 1.5 The changing world of engineering documents The earlier rule that engineering documents can only exist as hardcopy drawings applied only before there were CAD systems or where the engineer had no access to such. In the CAD systems used today, the design is normally three dimensional (3D) and the drawing itself produced from it (linking of 3D to drawings). The drawing is augmented by drawing entries 1) and is a contractual document. The 3D model supports the drawing and assists, e.g. for a complicated part, in understanding it or in reducing the number of attributes in the drawing. A 3D model can also be transferred to modern manufacturing and inspection equipment and processed further (e.g. for CNC programming). In future, or even today in some companies, all information and attributes are given in the 3D model, i.e. no drawing is produced, or is only produced for an external provider where data processing is not available. A possible representation is shown on page 16, Guide In any case, complete and unambiguous data is required Further information can be found in ISO Technical product documentation -- Digital product definition data practices. To be noted in this respect: Attributes are drawing entries which are not visible, but available by query (e.g. mouse click) Notes are drawing entries which are directly visible without manual or other manipulation. Editorial note (see also Standards Compendium 2014, 1.3.1): In accordance with the ISO Directives, Part 2, clause 6.6.8, this document uses a) a comma for the decimal marker, b) a small space to separate a group of more than 3 digits, c) a half-high dot for multiplication of compound units, d) a small x for multiplication of numbers. 1) Drawing entries can be dimensions, tolerances, remarks, text or symbols.

6 6 Preparing engineering drawings according to standards Notes

7 Preparing engineering drawings according to standards 7 2. Machining

8 8 Preparing engineering drawings according to standards 2. Machining 2.1 Machining of a drive shaft (see drawing Drive shaft on page 11) The drawing indication Tolerancing ISO 8015 means that for the affected design drawing the rules, concepts and principles of the ISO GPS standards system (among others, ISO 8015:2011) apply generally (i.e. without being specially agreed). (The drive shaft is shown in the assembly drawing on page 55). One of these fundamental rules is the Principle of Independency (abbreviated: Independency Principle ). This means that each requirement applicable to a geometrical element (e.g. the diameter of a shaft) must be met independently of other requirements on this geometrical element (e.g. form deviation such as circularity or straightness). This applies unless deviating requirements are specified, e.g. E (Envelope Requirement) as in ISO , or M (Maximum material requirement) as in ISO Example 1: Diameter 30h11 (Standard material ex works) Tolerances: 0/ 0,13 mm Permitted geometrical deviation according to ISO , tolerance class K : For the general tolerance for straightness and flatness the value for tolerance class K is 0,1 mm For the general tolerance for circularity, the numerical value of the nominal size tolerance applies. This may however be not greater than the general tolerance value according to the Table for circular radial run-out. This means: Numerical value according to nominal tolerance: 0/ 0,13 mm 0,13 mm Numerical value according to the Table for circular radial run-out, tolerance class K : 0,2 mm Applicable therefore for circularity: 0,13 mm Because the general tolerance for parallelism does not make sense for cylinders, this is described here for the linear dimension 65. For the general tolerance for parallelism, the numerical value of the dimensional tolerance or the value according to the Table for straightness and flatness in the standard applies. The larger value is applicable. For the dimension 65 this means: The numerical value of the nominal size tolerance according to tolerance class m : ±0,3 mm 0,6 mm Numerical value according to the Table for straightness, tolerance class K : 0,2 mm Applicable value for parallelism: 0,6 mm Example 2: Diameter 20k5 E CT Limit deviation : +0,002 mm/+0,011 mm (tolerance class k5) Permissible geometric deviation for flatness, straightness, circularity, cylindricity: 0,009 mm; ; for parallelism of opposite surface lines: 0,009 mm (Standard tolerance grade IT5, see Standards Compendium 2014, page 73) The shape and position tolerances for the bearing seats on the shaft in this example are taken from the SKF main catalogue (see page 10).The entry «E» for the dimension Ø20k5 indicates the envelope requirement. The dimensional tolerance limits the shape deviations and the parallelism of opposite surfaces. The complete geometrical form must lie within the theoretical tolerance envelope (Ø20,011 mm) and the two-point size must not be less than 20,002 mm at any position. The envelope requirement is only applicable for linear features of size. The entry CT means common tolerance. The tolerance applies to the three geometrical features, i.e. the three diameters Ø20k5 must lie within a common envelope. ø20,011 0,

9 Preparing engineering drawings according to standards 9 2. Machining The envelope requirement is only applicable for linear features of size. Of the geometrical tolerances, the envelope requirement only limits shape deviations (flatness, straightness, circularity, cylindricity) and the parallelism of opposite edges, surfaces and surface lines. Differing or additional shape and location tolerances must be stated separately. Definition Linear features of size can include circles, cylinders, spheres as well as parallel opposite edges or surfaces (which must be able to be measured between two points). Example 3: If it is not clear from the drawing which keyway form is used, this is specified with the number of the standard DIN 6885 and the designation N1, N2 or N3 with an arrow. DIN 6885-N1 Keys Keyway type for shafts - N1 - N2 - N3 Example 4: This symbol (see ISO 13715) is needed because the internal edge at the bottom of the groove for the circlips (DIN 471) and for the key (DIN 6885) in the respective standard are different from what is indicated in the drawing. Attention: The edge condition sharp for undercuts (circlips) must be specified separately for the external edge on the loaded side, because this is not mentioned in the standard, and may not be included in the general entry. 0,5 Drawing indication (all edges) Example 5: Advantages of location tolerancing using theoretically exact dimensions 1. The design requirements are designated based on a datum (in this case the functionally important surface D). The features to be toleranced always relate to the neighbouring part and not to freely chosen reference edges. 2) All requirements are geometrically unambiguous and able to be technically measured. 3) The starting points for dimensional entries are defined geometrically. j 0,3 D D 4) Dimensional direction (orientation) is defined geometrically (parallel, at a right angle or radial to the datum).

10 10 Preparing engineering drawings according to standards 2. Machining Example 6: Total run-out (Data from catalogues) For economical and functional reasons the shape and location tolerances (geometrical tolerances) do not always meet the recommendations in roller bearing catalogues. Inspection reasons could, instead of the total run-out tolerance of 0,009 mm, also call for a perpendicularity tolerance. Always consult with the project manager about which shape and position tolerances (geometrical tolerances) are functionally necessary. Geometrical tolerances for bearing seats on shafts and in housings ød A ødb øda ødb Surface Characteristic Symbol for geometrical characteristic tolerance zone Permissible deviations Bearings of tolerance class 1) Normal, CLN Cylindrical seat Total radial run-out 2 Flat abutment Total axial run-out Explanation For normal demands For special demands with respect to running accuracy or even support Source: SKF Drawing example: drive shaft on page 11 of SKF catalogue. Selected: roller bearings with tolerance class Normal, CLN 3 and normal requirements. 1) Example: ø20 IT5/2 = 9 µm/2 = 4,5 µm 0,0045 mm Drawing indication (rounded up): 2) For bearings with higher precision (P4 etc.), see SKF catalogue Super-precision bearings. 3) Tapered roller bearings with tolerances according to ISO 492 Tolerance class 6X

11 Preparing engineering drawings according to standards Machining -0,05 D j 20f7 2x CT -0,05 D j D ( ( All dimensions in mm Scale: 1:1 Sheet: 1/1 Responsible dept.: Created by: Approved by: Material: ABC 2 Jane Smith David Brown 11SMnPb30+C Item Number: Document type: Production drawing Title, Supplementary title: Document status: Company Released Drive shaft Rev. Date of issue: Lang.: (in assembly drg ) e * General tolerances ISO 2768-mK Tolerancing ISO 8015 Linear dimensions ISO Attention: The surface requirements for undercuts, keyways, etc. are only measurable with difficulty because they are not easy to reach and the measuring lengths are too short. * This indication is optional (see Specialty Module Independency principle page 3).

12 12 Preparing engineering drawings according to standards 2. Machining 2.2 Machining of a holder flange (see drawing Holder flange on page 13) The ISO standards of the geometric product specification (GPS) address various design, manufacture and quality assurance requirements for dimensions, shape, position and surface. Functionally suitable dimensioning with position tolerances is a good opportunity to define the part unambiguously and apply functionally correct measurement technology as part of quality assurance (part inspection). (The holder flange is shown in the assembly drawing on page 55) 0,2 A B Example 1: Datums A and B The datums A and B form the basis for the function of the part. Datums should be determined based on function because as a rule they are the interface to the (assumed theoretically exact) neighbouring part. This manner of indicating datum A is permitted by Rule G of ISO ,05 B A B A LP = Specification modifying symbol according to ISO Meaning: actual local size two-point size +0,025 LP Ø47 0 GX Features of size are: Circles, cylinders, spheres as well as parallel opposite edges or surfaces (and must be measurable between two points). LP Is a standard value, i.e. it need not be indicated without the addition of further modification symbols. GX = Meaning: Maximum inscribed association criterion GX is used for bores, GN (Minimum circumscribed association criterion) for shafts. The maximum inscribed association criterion cannot be used alone. LP and GX together mean two-point size with the criterion of maximum inscribed geometrical feature. Ø47 = maximum inscribed dimension +0,025 LP Ø47 0 GX This indication has the same meaning as ø47h7 but affects the measurement of the bore. Example 2: The permissible deviation for the length of the core hole according to DIN 76-1: +0,5 P 0 P for M8 thread = 1,25 mm 0,5 1,25 mm = 0,625 mm +0,625 20,2 0