AC : CALCULATION OF TOLERANCE STACKS USING DIRECT-POSITION APPROACH IN GEOMETRIC DIMENSIONING AND TOLERANCING
|
|
- Eugenia Dorsey
- 5 years ago
- Views:
Transcription
1 AC : CALCULATION OF TOLERANCE STACKS USING DIRECT-POSITION APPROACH IN GEOMETRIC DIMENSIONING AND TOLERANCING Cheng Lin, Old Dominion University American Society for Engineering Education, 2009 Page
2 Calculation of Tolerance Stacks Using Direct-Position Approach in Geometric Dimensioning and Tolerancing Abstract Formulas for the calculation of position tolerance stacks of Geometric Dimensioning and Tolerancing (GD&T) are presented. This direct-position approach shows that the formulas can be observed directly from the extreme positions of the holes specified in an engineering drawing. When compared to other approaches for tolerance stacks, this method can be applied to all three material conditions (Maximum Material Condition, Least Material Condition, and Regardless of Feature Size.) and is easier for students to learn and remember the formulas. A graphical demonstration using position control on two holes in an engineering drawing is applied to explain the approach. 1. Introduction Tolerance stacks are used to describe the problem-solving process in calculating the effects of the accumulated variation that is allowed by specified dimensions and tolerances, which are typically specified on an engineering drawing. Arithmetic tolerance stacks use the worst-case maximum or minimum values of dimensions and tolerances to calculate the maximum and minimum distances between holes or between a hole and the edge of a part 1,2. The application is particularly important in the design stage to maintain a specified minimum solid distances in the part. In addition, stack analysis enables parts to be made precise enough to be assembled interchangeably with the largest possible tolerances permitted by part specification. Several methods are proposed to calculate tolerance stacks using the approaches of graphs, charts, tables, and formulas 3,4,5. However, they are all very complicated for students to learn. A graphical approach called gage method, using the concept of functional gages, seems to provide an effective way for this purpose 2. However, as the functional gages can only be applied to the Maximum Material Condition (MMC), this method can not be applied to other two material conditions: Least Material Condition (LMC) and Regardless of Feature of Size (RFS). In this paper, the direct-position method is proposed to derive the formulas for tolerance stacks. The method not only is easier for students or designers to understand and remember, but can be applied to three material conditions, which are explained in the following session. A graphical example using position control on three material conditions is applied to demonstrate the approach. 2. Three Material Conditions Based on the design and manufacturing needs, geometric tolerances can be specified with different material conditions, which include Maximum Material Condition (MMC), Least Material Condition (LMC), and Regardless of Feature Size (RFS). Characteristics of each material condition are described in the following paragraphs Maximum Material Condition (MMC) To indicate that a geometric tolerance is specified with MMC, a symbol m is added to either a geometric characteristic or a datum. Maximum Material Condition is particularly defined as having the maximum solid volume for a part. Therefore, for internal parts (such as holes or grooves, etc.), MMC is at its minimum feature of size (FOS). For external parts (such as pins or studs, etc.), MMC is at its maximum feature of size. When a geometric characteristic is specified with MMC, the geometric tolerance may have a bonus tolerance when its FOS is approaching to its Least Material Condition (LMC). Figure 1 6 shows a design drawing using MMC Position Tolerance with Datum A as the center axis of the φ0.8 hole. From the table shown in this figure, when the diameter of a part is measured at 1.02, which is the MMC, there is no Page
3 bonus tolerance and the Position Tolerance remains at However, when the diameter is measured at 0.98, which is the LMC, the bonus tolerance is equal to The total Position Tolerance in this case increases to MMC can be easily found in most GD&T design drawings. Figure 1: A design drawing using MMC position tolerance Least Material Condition (LMC) To indicate that a geometric tolerance is specified with LMC, a symbol l is added to either a geometric tolerance or a datum. Least Material Condition is particularly defined as having the least solid volume for a part. Therefore, for internal parts, LMC is at its maximum feature of size. For external parts, LMC is at its minimum feature of size. When a geometric tolerance is specified with LMC, the geometric tolerance may have a bonus tolerance when its FOS is approaching to its MMC. Figure 2 6 shows a design drawing using LMC Position Tolerance with Datum A as the center axis of the φ0.8 hole. From the table shown in this figure, when the diameter of a part is measured at 1.02, which is the MMC, there is a bonus tolerance and the Position Tolerance increases to However, when the diameter of a part is measured at 0.98, which is the LMC, there is no bonus tolerance. The Position Tolerance remains at LMC is particularly applied to guarantee a larger minimum thickness than the same drawing using MMC. Figure 2: A design drawing using LMC position tolerance Regardless of Feature Size (RFS) Unlike MMC and LMC, Regardless of Feature Size gives no additional geometric tolerance. The concept of RFS has been used prior to the introduction of MMC and LMC principles. Figure 3 6 shows a design drawing using RFS position tolerance. Since there is no modifier added to the position tolerance, according to Rule 2 6, the position tolerance is RFS. From the table shown in this figure, the position tolerance remains the same regardless the variations on the feature of sizes. Page
4 Figure 3: A design drawing using RFS position tolerance. 3. Formula for Solid Distance between Two Holes - Regardless of Feature Size (RFS) Figure 4 shows an engineering drawing using RFS in the position-tolerance control. In the drawing, A represents a datum feature; φd 1 and φd 2 represent the diametrical sizes of the two holes respectively; T 1 and T 2 represent the bilateral size tolerances of the two holes respectively; φp 1 and φp 2 represent the RFS position tolerances of the two holes respectively; L is the actual location between these two holes and is expressed in basic dimension 2,7 ; X represents the solid distance between these two holes. According to the definition of RFS 2, there is no bonus position tolerance for these two holes. Figure 4: Position Tolerance with RFS Formulas for X max RFS Figure 5 shows the extreme position to determine X max based on the following conditions: a. The two holes are made at their minimum sizes: φ (D 1 -T 1 ) and φ (D 2 -T 2 ) b. The centers of the two holes are located at their farthest positions of the position-tolerance zones: Points A and B in Figure 5. Page
5 Figure 5: Extreme Position for X max RFS. From Figure 5, X max can be easily determined through the following equation: (1) 3.2. Formulas for X min RFS Figure 6 shows the extreme position to determine X min based on the following conditions: a. The two holes are made at their maximum sizes: φ (D 1 +T 1 ) and φ (D 2 +T 2 ) b. The centers of the two holes are located at their closest positions of the position-tolerance zones: Points A and B in Figure 6. Figure 6: Extreme Position for X min RFS. From Figure 6, X min can be easily determined through the following equation: Equation (2) is similar to Equation (1) except using minus signs on P 2 /2 and P 1 /2 in the formula because Points A and B are at their closest positions. (2) Page
6 4. Formula for Solid Distance between Two Holes Maximum Material Condition (MMC) Figure 7 shows an example of an engineering drawing using MMC in the position-tolerance control. The drawing is very similar to Figure 6, except with m added in the feature control frame of the position tolerances. According to MMC 6, a maximum bonus position tolerance of 2T 1 is added to φp 1 when the diameter of the Hole 1 is made at φ (D 1 +T 1 ). Similarly, a maximum bonus position tolerance of 2T 2 Figure 7: Position Tolerance with MMC. can be added to φp 2 when Hole 2 is made at φ (D 2 +T 2 ). No bonus position tolerance will be allowed when the diameters of the holes are made at φ (D 1 -T 1 ) and φ (D 2 -T 2 ) respectively Formulas for X max MMC Figure 8 shows the extreme condition for X max. Similar to the Session 3.1, it is based on the following conditions: a. The two holes are made at their minimum sizes: φ (D 1 -T 1 ) and φ (D 2 -T 2 ). b. The centers of the two holes are located at their farthest locations of the position-tolerance zones: Points A and B. Figure 8: Extreme Position for X max MMC. Because there is no bonus position tolerance when the diameters of the holes are made at φ (D 1 -T 1 ) and φ (D 2 -T 2 ) respectively, Figure 8 is exactly the same as Figure 5. X max can be easily determined through the following equation: Page
7 (3) 4.2. Formulas for X min MMC Figure 9 shows the extreme condition for X min, which is based on the following conditions: a. The two holes are made at their maximum sizes: φ (D 1 +T 1 ) and φ (D 2 +T 2 ). Because the holes are made at their Least Material Condition (LMC), bonus tolerances of φ2t 1 and φ2t 2 are added to their respective original position tolerances φp 1 and φp 2. b. The centers of the two holes are at their closest locations, which are indicated as Points A and B. Figure 9: Extreme Position for X min MMC. From Figure 9, X min can be easily determined through the following equation: (4) 5. Formula for Solid Distance between Two Holes Least Material Condition (LMC) Figure 10 shows an example of an engineering drawing using LMC in the position-tolerance control. The drawing is very similar to Figure 4, except m is replaced with l in the feature control frame of the position tolerances. According to Foster 7, a maximum bonus position tolerance of 2T 1 can be added to φp 1 when the Hole 1 is made at φ (D 1 -T 1 ), and a maximum bonus position tolerance of 2T 2 can be added to φp 2 when the Hole 2 is made at φ (D 2 T 2 ). No bonus position tolerance will be allowed when the holes are made at φ (D 1 +T 1 ) and φ (D 2 +T 2 ) respectively. Page
8 Figure 10: Position Tolerance with LMC Formulas for X max LMC The extreme condition of the two holes for X max is shown in Figure 11. Similar to the Session 3.1, it is based on the following conditions: a. The two holes are at their minimum sizes: φ (D 1 -T 1 ) and φ (D 2 -T 2 ). b. The centers of the two holes are at their farthest locations: Points A and B in Figure 11. Figure 11: Extreme Position for X max LMC. From Figure 11, X max can be easily expressed by the following equation: (5) 5.2. Formulas for X min LMC The extreme position of the two holes for X min is shown in Figure 12, which is based on the following conditions: c. The two holes are at their maximum sizes: φ (D 1 +T 1 ) and φ (D 2 +T 2 ). Because the holes are made at their Least Material Condition (LMC), no bonus position tolerance for these two holes. d. The centers of the two holes are at their closest locations, which are located at Points A and B in Figure 12. Figure 12: Extreme Position for X min LMC. Page
9 It can be seen that the drawing is exactly the same as Figure 6. Therefore the equation for X min is exactly the same as Equation (2). (6) 6. Examples Figure 13 shows an MMC design drawing. Based on the information, Equations (3) and (4) can be applied to calculate X max and X min : (7) (8) Figure 13: An MMC design drawing. Figure 14 shows an LMC design drawing. Based on the information, Equations (5) and (6) can be applied to calculate X max and X min : (9) (10) From the results shown in these two cases, both values in LMC are larger than the values in MMC. Therefore, it is better to use LMC in the design when using the same dimensioning to seek for larger X min. Page
10 Figure 14: An LMC design drawing. 7. Conclusions This method presents an alternate approach to calculate the tolerance stacks using the direct-position method. When compared all the derived equations, maximum value of X min can be obtained when the drawing is specified with RFS or LMC. Minimum value of X min, which is undesirable, can be found in the drawing when specified in MMC. From the teaching experience of GD&T, students prefer to use this approach because the formulas can be derived directly from the observing of the graphic expression. In addition, the approach can also be applied to derive the formulas for other geometric characteristic symbols such as parallelism, perpendicularity, concentricity, runout, and profile tolerances. Students also become more understanding of the total tolerance zone in the position control of GD&T when applying to three material conditions. References 1. Scholz, F., Tolerance Stack Analysis, Methods Research and Technology, Boeing Information and Support Service, Krulikowski, A., Fundamentals of Geometric Dimensioning and Tolerancing, Delma, Ngoi, B., Applying the coordinate Tolerance System to Tolerance Stack Analysis Involving Position Tolerance, International Journal Manufacturing Technology Vol. 15; PP , Ngoi, B., Nexus method for stack analysis of geometric dimensioning and tolerancing (GDT) problems, International Journal of Production Research, v 38, n 1, Jan 10, p 21-37, Yen, D., Graph-based set-up planning and tolerance decomposition for computer-aided fixture design, International Journal of Production Research, v 38, n 1, Jan 10, p 21-37, Lin, C., and Verma, A., Clarifications of Rule 2 in Teaching Geometric Dimensioning and Tolerancing, ASEE Annual Conference, Session 1147, June Foster, L., Geo-Metrics III, Prentice Hall, 1994 Page
AC : CLARIFICATIONS OF RULE 2 IN TEACHING GEOMETRIC DIMENSIONING AND TOLERANCING
AC 2007-337: CLARIFICATIONS OF RULE 2 IN TEACHING GEOMETRIC DIMENSIONING AND TOLERANCING Cheng Lin, Old Dominion University Alok Verma, Old Dominion University American Society for Engineering Education,
More informationIntroduction to GD&T Session 2: Rules and Concepts of GD&T
Introduction to GD&T Session 2: Rules and Concepts of GD&T An exploration of the language known as Geometric Dimensioning and Tolerancing Instructor: John-Paul Belanger Review Benefits of GD&T The GD&T
More informationGD&T Reckoner Course reference material for. A Web-based learning system from.
GD&T Reckoner Course reference material for A Web-based learning system from This is not the complete document. Only Sample pages are included. The complete document is available to registered users of
More informationSingle Part Tolerance Analysis 1
856 SALT LAKE COURT SAN JOSE, CA 95133 (408) 251 5329 Single Part Tolerance Analysis 1 2X Ø.250 ±.005 D 3.075-3.175.500 2.000.250 ±.005 E.375 C 2.050 1.950.609.859 1.375 G 1.125 B.375.750 1.125 1.500 1.875
More informationASME Y14.5M-1994 GD&T Certification Preparation Examination
ASME Y14.5M-1994 GD&T Certification Preparation Examination Directions: On the response sheet on the last page, fill in the circle of the letter which best completes the following statements. Do not write
More informationGEOMETRIC DIMENSIONING AND TOLERANCING (GD&T) Based on ASME Y14.5M-1994 Standard
GEOMETRIC DIMENSIONING AND TOLERANCING (GD&T) Based on ASME Y14.5M-1994 Standard Duration: 4 Days Training Course Content: Day 1: Tolerancing in Engineering Drawing (9:00am-10:00am) 1.0 Geometric Dimensioning
More informationGEOMETRIC DIMENSIONING AND TOLERANCING (GD&T)
GEOMETRIC DIMENSIONING AND TOLERANCING (GD&T) Based on ASME Y14.5M-1994 Standard Duration : 4 days Time : 9:00am 5:00pm Methodology : Instructor led Presentation, exercises and discussion Target : Individuals
More informationTerms The definitions of 16 critical terms defined by the 2009 standard 1
856 SALT LAKE COURT SAN JOSE, CA 95133 (408) 251 5329 Terms The definitions of 16 critical terms defined by the 2009 standard 1 The names and definitions of many GD&T terms have very specific meanings.
More informationTest Answers and Exam Booklet. Geometric Tolerancing
Test Answers and Exam Booklet Geometric Tolerancing iii Contents ANSWERS TO THE GEOMETRIC TOLERANCING TEST............. 1 Part 1. Questions Part 2. Calculations SAMPLE ANSWERS TO THE GEOMETRIC TOLERANCING
More informationGeometric Dimensioning & Tolerancing
Western Technical College 31420350 Geometric Dimensioning & Tolerancing Course Outcome Summary Course Information Description Career Cluster Instructional Level Total Credits 1.00 Total Hours 36.00 Recognition
More informationGeometric Tolerances & Dimensioning
Geometric Tolerances & Dimensioning MANUFACTURING PROCESSES - 2, IE-352 Ahmed M. El-Sherbeeny, PhD KING SAUD UNIVERSITY Spring - 2015 1 Content Overview Form tolerances Orientation tolerances Location
More informationDRAFTING MANUAL. Dimensioning and Tolerancing Rules
Page 1 1.0 General This section is in accordance with ASME Y14.5-2009 Dimensioning and Tolerancing. Note that Rule #1 is the only rule that is numbered in the 2009 standard. All of the other rules fall
More informationGeometric Dimensioning and Tolerancing
Geometric Dimensioning and Tolerancing (Known as GDT) What is GDT Helps ensure interchangeability of parts. Use is dictated by function and relationship of the part feature. It does not take the place
More informationAnswers to Questions and Problems
Fundamentals of Geometric Dimensioning and Tolerancing Using Critical Thinking Skills 3 rd Edition By Alex Krulikowski Answers to Questions and Problems Second Printing Product #: 1103 Price: $25.00 Copyright
More informationAdvanced Dimensional Management LLC
Index: Mechanical Tolerance Stackup and Analysis Bryan R. Fischer Accuracy and precision 8-9 Advanced Dimensional Management 14, 21, 78, 118, 208, 251, 286, 329-366 Ambiguity 4, 8-14 ASME B89 48 ASME Y14.5M-1994
More informationTolerancing Fixed Fasteners 1
+ 856 SALT LAKE COURT SAN JOSE, CA 951 (408) 251 529 Tolerancing Fixed Fasteners 1.274- Figure 8-5 Fixed fastener The fixed fastener in Fig. 8-5 is fixed by one or more of the members being fastened. The
More informationINDEX. Datum feature symbol, 21
INDEX Actual Mating Envelope, 11 Actual Minimum Material Envelope, 11 All Around, 149 ALL OVER, 157, 158,363 Allowed vs. actual deviations from true position, 82 Angularity, 136 axis, 140 line elements,
More informationVirtual CAD Parts to Enhance Learning of Geometric Dimensioning and Tolerancing. Lawrence E. Carlson University of Colorado at Boulder
Virtual CAD Parts to Enhance Learning of Geometric Dimensioning and Tolerancing Lawrence E. Carlson University of Colorado at Boulder Introduction Geometric dimensioning and tolerancing (GD&T) is an important
More informationAlessandro Anzalone, Ph.D. Hillsborough Community College, Brandon Campus
Alessandro Anzalone, Ph.D. Hillsborough Community College, Brandon Campus Sections: 1. Definitions 2. Material Conditions 3. Modifiers 4. Radius and Controlled Radius 5. Introduction to Geometric Tolerances
More informationConcentricity and Symmetry Controls
Concentricity and Symmetry Controls Alessandro Anzalone, Ph.D. Hillsborough Community College, Brandon Campus Concentricity and Symmetry Controls Sections: 1. Concentricity Control 2. Symmetry Control
More informationGeometric Dimensioning and Tolerancing
Geometric dimensioning and tolerancing (GDT) is Geometric Dimensioning and Tolerancing o a method of defining parts based on how they function, using standard ASME/ANSI symbols; o a system of specifying
More informationMeasurement and Tolerances
Measurement and Tolerances Alessandro Anzalone, Ph.D. Hillsborough Community College, Brandon Campus Measurement and Tolerances Sections: 1. Meaning of Tolerance 2. Geometric Dimensioning and Tolerancing
More informationEngineering & Design: Geometric Dimensioning
Section Contents NADCA No. Format Page Frequently Asked Questions -2 s e c t i o n 1 Introduction -2 2 What is GD&T? -2 3 Why Should GD&T be Used? -2 4 Datum Reference Frame -4 4.1 Primary, Secondary,
More informationClarifications of a Datum Axis or Centerplane Specifying in Maximum Material Condition of Geometric Dimensioning and Tolerancing
Paper ID #5813 Clarifications of a Datum Axis or Centerplane Specifying in Maximum Material Condition of Geometric Dimensioning and Tolerancing Dr. Cheng Y. Lin P.E., Old Dominion University Dr. Lin is
More informationFOREWORD. Technical product documentation using ISO GPS - ASME GD&T standards
Technical product documentation using ISO GPS - ASME GD&T standards FOREWORD Designers create perfect and ideal geometries through drawings or by means of Computer Aided Design systems, but unfortunately
More informationGD&T - Profile Tolerancing
GD&T - Profile Tolerancing PMPA Technical Conference Rapid Response to Make the Cut Grand Rapids, MI April 11, 2016 Gary K. Griffith Corona, California Gary K. Griffith 48 Years Exp. Technical Book Author
More informationTo help understand the 3D annotations, the book includes a complete tutorial on SOLIDWORKS MBD
To help understand the 3D annotations, the book includes a complete tutorial on SOLIDWORKS MBD Technical product documentation using ISO GPS - ASME GD&T standards FOREWORD Designers create perfect and
More informationAC : TEACHING APPLIED MEASURING METHODS USING GD&T
AC 2008-903: TEACHING APPLIED MEASURING METHODS USING GD&T Ramesh Narang, Indiana University-Purdue University-Fort Wayne RAMESH V. NARANG is an Associate Professor of Industrial Engineering Technology
More informationME 410 Mechanical Engineering Systems Laboratory
ME 410 Mechanical Engineering Systems Laboratory Laboratory Lecture 1 GEOMETRIC TOLERANCING & SOURCES OF ERRORS Geometric dimensioning and tolerancing (GD&T) is a symbolic language used on engineering
More informationGeometric Boundaries II
Geometric Boundaries II Interpretation and Application of Geometric Dimensioning and Tolerancing (Using the Inch and Metric Units) Based on ASME Y14.5-2009 (R2004) Written and Illustrated by Kelly L. Bramble
More informationA Strategy for Tolerancing a Part 1
856 SLT LKE OURT SN JOSE, 95133 (408) 251 5329 Strategy for Tolerancing a Part 1 The first step in tolerancing a feature of size, such as the hole in Figure 14-1, is to specify the size and size tolerance
More informationGeometric Boundaries
Geometric Boundaries Interpretation and Application of Geometric Dimensioning and Tolerancing (Using the Customary Inch System) Based on ASME Y14.5M-1994 Written and Illustrated by Kelly L. Bramble Published
More informationA R C H I V E
A R C H I V E 2 0 0 6 Tutorial Geometric Dimensioning And Tolerancing: A Primer For The BiTS Professional Thomas Allsup Manager of Technology Anida Technologies COPYRIGHT NOTICE The papers in this publication
More informationIntroduction. Objectives
Introduction As more and more manufacturers become immersed in the global economy, standardization plays a critical role in their success. Geometric dimensioning and tolerancing (GD&T) provides a set of
More informationDatum reference frame Position and shape tolerances Tolerance analysis
Datum reference frame Position and shape tolerances Tolerance analysis Šimon Kovář Datum reference frame Datum reference frames are typically for 3D. A typical datum reference frame is made up of three
More informationTolerancing. Summary
Tolerancing Summary Summary What will we learn We will learn about tolerancing and how important this technique is to mass production. Key points If a feature s size is toleranced, it is allowed to vary
More information1994 Dimensioning & Tolerancing
ASME Y14.5M-1994 1994 Dimensioning & Tolerancing The new scanning generation Zeiss / Applied Geometrics, Inc. Applied Geometrics, Inc. Copyright 2003 1 Zeiss Carl Zeiss is one of the world's leading enterprises
More information: Fits and Tolerances
Fits and Tolerances CONTENTS Why tolerances and fits are required? Due to the inevitable inaccuracy of manufacturing methods, a part cannot be made precisely to a given dimension, the difference between
More informationCOMMON SYMBOLS/ ISO SYMBOL ASME Y14.5M ISO FEATURE CONTROL FRAME DIAMETER/ SPHERICAL DIAMETER/ AT MAXIMUM MATERIAL CONDITION
1 82 COMMON SYMBOLS/ Shown below are the most common symbols that are used with geometric tolerancing and other related dimensional requirements on engineering drawings. Note the comparison with the ISO
More informationME 114 Engineering Drawing II
ME 114 Engineering Drawing II FITS, TOLERANCES and SURFACE QUALITY MARKS Mechanical Engineering University of Gaziantep Dr. A. Tolga Bozdana Assistant Professor Tolerancing Tolerances are used to control
More informationDavid A. Madsen. Faculty Emeritus
i Q eometric ' ' Dimensioning andtolerancing Ninth Edition Based on ASME Y14.5-2009 AWk A ejacy ofjejtccftence APPROVED PUBLICATION by David A. Madsen President, Madsen Designs Inc. www.madsendesigns.com
More informationGaging Exploration (Applications)
Gaging Exploration (Applications) PMPA Technical Conference Tomorrow is Today - Conquering the Skills Challenge Chicago, IL April 24, 2018 Gary K. Griffith Corona, California Gary K. Griffith 50+ Years
More informationGeometric dimensioning & tolerancing (Part 1) KCEC 1101
Geometric dimensioning & tolerancing (Part 1) KCEC 1101 Introduction Before an object can be built, complete information about both the size and shape of the object must be available. The exact shape of
More informationA Concise Introduction to Engineering Graphics
A Concise Introduction to Engineering Graphics Fourth Edition Including Worksheet Series A Timothy J. Sexton, Professor Department of Industrial Technology Ohio University BONUS Book on CD: TECHNICAL GRAPHICS
More informationGEOMETRICAL TOLERANCING
GEOMETRICAL TOLERANCING Introduction In a typical engineering design and production environment, the designer of a part rarely follows the design to the shop floor, and consequently the only means of communication
More informationPattern Inspection with Variable Geometric Tolerance Limits
Pattern Inspection with Variable Geometric Limits From Disregarding to Fully Applying Variable Feature Bonus and Datum Shift s in a Pattern Inspection By Paul F. Jackson Variable Limit Specifications and
More informationImproving Manufacturability
Improving Manufacturability GD&T is a Tool Not a Weapon Joe Soistman Quality Manufacturing Solutions, LLC Overview What is manufacturability, and why is it important? Overview What is manufacturability,
More informationTechnical drawings and their interpreta1on. ME Fall 2011 Eradat SJSU Based on notes on Jim Burge and other online resources
Technical drawings and their interpreta1on ME 297-1 Fall 2011 Eradat SJSU Based on notes on Jim Burge and other online resources Technical drawings Technical drawings Orthographic projec1on Isometric layout
More informationWorkpiece drawing factors. Size Shape Composition Dimensions Specifications
ITCD 301-001 Workpiece drawing factors Size Shape Composition Dimensions Specifications Tolerance Total amount of dimensional variation Designer specifies an unattainable condition Designer specifies a
More information1.0 What is tolerance analysis? 2.0 What is Tolerance Stackup? 3.0 Generally, the Tolerance Stackup Process 4.0 Method and Types of Tolerance
TOLERANCE ANALYSIS 1.0 What is tolerance analysis? 2.0 What is Tolerance Stackup? 3.0 Generally, the Tolerance Stackup Process 4.0 Method and Types of Tolerance Analysis 5.0 Worst-case Tolerance Stackup
More informationProduct and Manufacturing Information (PMI)
Product and Manufacturing Information (PMI) 1 Yadav Virendrasingh Sureshnarayan, 2 R.K.Agrawal 1 Student of ME in Product Design and Development,YTCEM -Bhivpuri road-karjat, Maharastra 2 HOD Mechanical
More informationCopyright Warning & Restrictions
Copyright Warning & Restrictions The copyright law of the United States (Title 17, United States Code) governs the making of photocopies or other reproductions of copyrighted material. Under certain conditions
More informationModule 1 - Introduction. In the space below, write any additional goals, objectives, or expectations you have for this module or course:
In the space below, write any additional goals, objectives, or expectations you have for this module or course: 1-1 Engineering drawings contain several typical types of information, as illustrated in
More informationhttp://blogs.solidworks.com/solidworksblog/2015/10/mbdimplementation-10-dos-and-10-donts-dont-hesitate-part-1.html Create MBE Vision Plan Identify Data Needs Assess PMI Consumption 3 DimXperts 2D Drawings
More informationUnit4 31. UnitS 39. Unit 6 47
Preface..................... xi About the Author......... xiii Acknowledgments... xiv Unit 1 1 Bases for Interpreting Drawings........ I Visible Lines............. 3 Lettering on Drawings... 3 Sketching...
More informationDimensioning. Dimensions: Are required on detail drawings. Provide the shape, size and location description: ASME Dimensioning Standards
Dimensioning Dimensions: Are required on detail drawings. Provide the shape, size and location description: - Size dimensions - Location dimensions - Notes Local notes (specific notes) General notes ASME
More informationHow to Spell GD&T Part II: Revenge of the Circled Letters Thomas Allsup
How to Spell GD&T Part II: Revenge of the Circled Letters Thomas Allsup Return of the Jedi Originally to be titled "Revenge of the Jedi" but producers thought the Jedi wouldn't seek revenge. Some posters
More informationProduct and Manufacturing Information(PMI)
Product and Manufacturing Information(PMI) Ravi Krishnan V 1 Post Graduate Student Department of Mechanical Engineering Veermata Jijabai Technological Institute Mumbai, India ravi.krishnan30@gmail.com
More informationEngineering drawing. Semester I/II Mechanical Engineering Department Technical University of Gdańsk. Lecture 8
Engineering drawing Semester I/II Mechanical Engineering Department Technical University of Gdańsk Lecture 8 Representing Tolerance Values Tolerance is the total amount a dimension may vary and is the
More informationSPECIFICATION
Rev. R SPECIFICATION 9-3800 Page 1 of 26 Amphenol Corporation Sidney, New York U TITLE STANDARD SPECIAL USE DESCRIPTION ENGINEERING DRAWING Revisions REV. LETTER ISSUE NUMBER ORIGINATOR DATE APPROVAL M
More informationGeometric Tolerancing
Geometric Tolerancing Distorted Objects by Suzy Lelievre Scale Transform SALOME Geometry User s Guide: Scale Transform Baek-Ki-Kim-Twisted Stool Mesh Geometric Tolerancing What is it? Geometric Tolerancing
More informationUnderstanding GO/NO GO Gauges (Fixed Limit Gauging)
Understanding GO/NO GO Gauges (Fixed Limit Gauging) How do I choose a plug gauge for my measurement application. Therefore I put together this document to help everyone understand the concept of fixed
More informationUsing Advanced GDT Analysis to Further Reduce Rejects and Improve Rework Time and Instructions
Using Advanced GDT Analysis to Further Reduce Rejects and Improve Rework Time and Instructions 3 rd TRI-NATIONAL WORKSHOP AND MEETING OF THE NORTH AMERICAN COORDINATE METROLOGY ASSOCIATION 3D Measurement
More informationUnderstanding Drawings
Chapter 3 Understanding Drawings LEARNING OBJECTIVES After studying this chapter, students will be able to: Read drawings that are dimensioned in fractional inches, decimal inches, and in metric units.
More informationFACULTY OF ENGINEERING DESIGN AND PRODUCTION ENGINEERING DEPARTMENT. Credit Hour System Metrology Lab 1 MDP 240. Sine Bars. Metrology laboratory
FACULTY OF ENGINEERING DESIGN AND PRODUCTION ENGINEERING DEPARTMENT Report On: Credit Hour System Metrology Lab 1 MDP 240 (13) Sine Bars Metrology laboratory Class No: B.N. Student Name Remark Signature
More informationENVELOPE REQUIREMENT VERSUS PRINCIPLE OF INDEPENDENCY
ENVELOPE REQUIREMENT VERSUS PRINCIPLE OF INDEPENDENCY Carmen SIMION, Ioan BONDREA University "Lucian Blaga" of Sibiu, Faculty of Engineering Hermann Oberth, e-mail:carmen.simion@ulbsibiu.ro, ioan.bondrea@ulbsibiu.ro
More informationTECHNICAL DESIGN II (546)
DESCRIPTION The second in a sequence of courses that prepares individuals with an emphasis in developing technical knowledge and skills to develop working drawings in support of mechanical and industrial
More informationPipe threads are threads that seal. Pipe threads seal by various methods, but the ones we are going to concern ourselves
PIPE THREADS Pipe threads are threads that seal. Pipe threads seal by various methods, but the ones we are going to concern ourselves with here are those that are designed to seal at the threads. For threads
More informationInspection and Measurement
Inspection and Measurement Inspection An action to insure what is being manufactured conforms to the specifications by attributes use of gages: go or no-go by variables use of calibrated instruments Measurement
More informationPRODUCT ENGINEERING/ DEVELOPMENT TOOLS & METHODS
PRODUCT ENGINEERING/ DEVELOPMENT TOOLS & METHODS GD&T RESOURCES GUIDE ETINEWS.COM PRODUCT ENGINEERING TOOLS & METHODS GD&T RESOURCES GUIDE Get critical GD&T training and education from Effective Training
More informationROYAL ULTRA-PRECISION ER COLLETS " TIR
ROYAL C EXPANDING COLLETS q Unlike chucks and most collets that grip the OD of a workpiece, C expanding collets are designed to grip on the ID of a part. q Accu-length design ensures precise workpiece
More informationSpatial Demonstration Tools for Teaching Geometric Dimensioning and Tolerancing (GD&T) to First-Year Undergraduate Engineering Students
Paper ID #17885 Spatial Demonstration Tools for Teaching Geometric Dimensioning and Tolerancing (GD&T) to First-Year Undergraduate Engineering Students Miss Myela A. Paige, Georgia Institute of Technology
More informationDimensioning: There are a few simple best practices which can help us dimension a working drawing:
Dimensioning and Tolerancing Prepared by: Michael Hypes Cornell University Preparation: One of the most common problems for new designers is choosing dimension that do not reflect the purpose of the part.
More informationMeasurement Methods: Functional vs. Variable. FUNCTIONAL GAGING (Attribute or Hard Gaging)
Page 1 of 5 EffectiveTraining Inc., Westland MI, 734.728.0909 Volume 01: Issue 4 ETImail is a regular online publication devoted to Geometric Dimensioning & Tolerancing. Each edition features a host of
More information6/23/2016 Copyright 2016 Society of Manufacturing Engineers
6/23/2016 Copyright 2016 Society of Manufacturing Engineers --- 1 --- GEOMETRIC DIMENSIONING & TOLERANCING FUNDAMENTALS Form Controls & Datums - GDT2 TRT: 25:44 Minutes SCENE 1. GDT01A, CGS: FBI warning
More informationEmpowering GD&T. Introduction. 1. Concepts
Empowering GD&T Copyright by Multi Metrics, Inc. 2017 All Rights Reserved Introduction The materials contained in this document represent an effort to clarify some of the most important concepts, tools
More informationQuality Procedure QP159 General Requirements for Machined Parts
1. PURPOSE 1.1. This procedure provides general product fabrication requirements. It also provides interpretation of certain requirements specified on product drawings, models, and electronic files. 2.
More informationEN1740 Computer Aided Visualization and Design Spring /12/2012 Brian C. P. Burke
EN1740 Computer Aided Visualization and Design Spring 2012 4/12/2012 Brian C. P. Burke Last Time: Design Analysis Clearance/Interference Checking Sensitivity/Feasibility/Optimization Intro to GD&T Tonight:
More informationRepresentation of features Geometric tolerances. Prof Ahmed Kovacevic
ME 1110 Engineering Practice 1 Engineering Drawing and Design - Lecture 6 Representation of features Geometric tolerances Prof Ahmed Kovacevic School of Engineering and Mathematical Sciences Room C130,
More informationMechanical Drawing. Unit 2 Study Guide for Chapters 6-10
Mechanical Drawing Unit 2 Study Guide for Chapters 6-10 Chapter 6 Multiview Drawing Section 6.1 Understanding Orthographic Projection A. Technical Drawing: How can a technical drawing give more accurate
More informationAdvanced Dimensional Management LLC
Index for Tolerance Stackup, Tolerance Analysis and Tolerancing Manual: Plus and Minus Edition Accuracy and precision 3, 19 Ambiguity 20 ASME Y14.5M-1994 2 rule #1 2 Assembly Process 20, 28, 79-81 Assembly
More informationA Conceptual Data Model of Datum Systems
[J. Res. Natl. Inst. Stand. Technol. 104, 349 (1999)] A Conceptual Data Model of Datum Systems Volume 104 Number 4 July August 1999 Michael R. McCaleb National Institute of Standards and Technology, Gaithersburg,
More informationSoftware Validation Considerations within Medical Companies per FDA 21 CFR PART 11
Greg Hetland, Ph.D. International Institute of GD&T Software Validation Considerations within Medical Companies per FDA 21 CFR PART 11 One critical challenge facing today s medical OEMs and suppliers is
More informationTABLE OF CONTENTS DIMENSIONING, GAGING, AND MEASURING
TABLE OF CONTENTS DIMENSIONING, GAGING, AND MEASURING DRAFTING PRACTICES 606 Drafting Practices 606 Sizes of Drawing Sheets 606 Symbols for Section Lining 606 Geometric Dimensioning 609 ANSI and ISO Symbols
More informationDesign & Engineering
Paras is committed to provide cost-effective solutions that streamline manufacturing cycles, enable collaboration with outside vendors, and ultimately shorten product delivery time. With installations
More informationCopyright 2008 Society of Manufacturing Engineers. FUNDAMENTALS OF TOOL DESIGN Gaging & Inspection Tool Design SIZE.
FUNDAMENTALS OF TOOL DESIGN Gaging & Inspection Tool Design SCENE 1. GI06A, tape FTD40, 13:13:28:00-13:13:49:00 wide, parts being air gaged GI06B, CGS: Tolerance BECAUSE OF THE LIMITS OF MANUFACTURING,
More informationDrawing & Design. Lecture 3. Lecturer: Dr. John Cheung
MECH 313 Engineering Drawing & Design Lecture 3 Lecturer: Dr. John Cheung Outline Limits and tolerances Fits and allowances Surface texture Why ygive Tolerance? Manufacturing Practice is 6000 years old,
More informationThe Author. 1 st Edition 2008 Self-published by Frenco GmbH
The Author Graduate Engineer (Dipl. Ing., FH) Rudolf Och was born in Bamberg, Germany in 1951. After graduating in mechanical engineering he founded FRENCO GmbH in Nuremberg, Germany in 1978. In the beginning,
More informationComputer-Aided Manufacturing
Computer-Aided Manufacturing Third Edition Tien-Chien Chang, Richard A. Wysk, and Hsu-Pin (Ben) Wang PEARSON Prentice Hall Upper Saddle River, New Jersey 07458 Contents Chapter 1 Introduction to Manufacturing
More informationSYSTEM OF LIMITS, FITS, TOLERANCES AND GAUGING
UNIT 2 SYSTEM OF LIMITS, FITS, TOLERANCES AND GAUGING Introduction Definition of limits Need for limit system Tolerance Tolerance dimensions ( system of writing tolerance) Relationship between Tolerance
More informationARCHIVE Thomas Allsup President Anida Technologies
T H I R T E E N T H A N N U A L ARCHIVE B GEOMETRIC DIMENSIONING AND TOLERANCING FOR BURN-IN AND TEST PROFESSIONALS by Thomas Allsup President Anida Technologies uilding on his 2006 Geometric Dimensioning
More informationRecommended Dimensional Guidelines for Single Screws
The Society of the Plastics Industry s Machinery Component Manufacturers Division Recommended Dimensional Guidelines for Single Screws The following recommendations for single screws of injection molding
More informationModule 1 Fundamentals of machine design. Version 2 ME, IIT Kharagpur
Module 1 Fundamentals of machine design Lesson 3 Brief overview of design and manufacturing Instructional Objectives: At the end of this lesson, the students should be able to understand: Concept of limits
More informationIntroduction. In engineering you are usually concerned with a number of parts or components fitting together to make an: assembly
Limits and Fits Introduction In engineering you are usually concerned with a number of parts or components fitting together to make an: assembly To assemble components together engineers must control the
More informationHelpful Alignment Tips for Machine Shops
Table of Contents Background... 3 Offset or Centerline Misalignment... 3 Parallelism or Angular Misalignment... 4 Alignment Equipment Needed... 5 How it Works... 5 Measuring Procedure... 5 Making the Measurements...
More informationHenrik S. Nielsen HN Metrology Consulting, Inc. Communicating Functional Requirements with GD&T
Henrik S. Nielsen HN Metrology Consulting, Inc. Communicating Functional Requirements with GD&T In The Beginning Move from craft to industry Emerging need for interchangeable parts Design and manufacturing
More information. Technical and Operating Conference, Chicago, IL, November )
(Proceedings of the 1994 Steel Founders Society of America. Technical and Operating Conference, Chicago, L, November 9-12. 1994) The mplications of Tolerance System nterpretation on Past and Present Dimensional
More informationComputer Modeling of Geometric Variations in Mechanical Parts and Assemblies
Yanyan Wu, 1 GE Global Research, Schenectady, NY Jami J. Shah Joseph K. Davidson Department of Mechanical and Aerospace Engineering, Arizona State University, Tempe, AZ 85287-6106 Computer Modeling of
More informationCompetency, knowledge and skill areas often offer varying definitions. For purposes of this toolkit, NIMS defines them in the following manner:
Toolkit Roadmap Title of report Credential name Narrative description of credential DEFINITION OF TERMS Competency, knowledge and skill areas often offer varying definitions. For purposes of this toolkit,
More informationMACHINIST TECHNICIAN - LATHE (582)
DESCRIPTION Students will demonstrate technical knowledge and skills to plan, manufacture, assemble, test products, and modify metal parts using machine shop and CNC processes in support of other manufacturing,
More information