Attachment 0004 - PdM MTV Drawing and Modeling Standards and Best Practices.pdf

Distribution Statement A: Approved for Public Release; Distribution is Unlimited

3-Dimensional Technical Data Package

Configuration Management, Modeling & Drawing

Interim Operating Procedure for PdM-MTV

DOCUMENT ID: FMTV-MODELING-STD-100T

14 March 2016

Revision M

3-Dimensional Technical Data Package Configuration Management, Modeling, & Drawing Interim Operating Procedure for PdM-MTV

15-Mar-1615-

Mar-16

Page i 14 March 2016 FMTV-MODELING-STD-100T Rev.M

Table of Contents

Table of Contents .......................................................................................................................................................... i

Table of Figures ........................................................................................................................................................... v

1 Foreword

1.1 0BBackground

2 Configuration Management Representations

2.1 1BStandards Application

2.2 2BDrawings Required

2.3 Engineering Changes

2.4 3BConfiguration Management

2.5 4BProducts

2.6 5BObject Status

2.7 6BSecurity

2.8 7BRevision Scheme

2.9 8BPromotion

2.10 9BQuality Assurance

2.11 10BRelease Level Flowchart

2.12 Notice of Revision

3 Part Modeling Standards

3.1 11BPart Modeling Practice

3.2 12BTolerances

3.3 13BMaterials

3.4 14BSurface Finishes

3.5 15BModel Notes

3.6 16BRelations

3.7 17BDefault Datums

3.8 18BPart File Names

127B3.8.1 Hardware File Names

128B3.8.2 Exceptions

3.9 19BModel Views

3.10 20BDeformed Parts

3.10.3 Creating Deformed Parts from Tabulated Parts

3.10.4 Creating Deformed Parts with Flexible Components

3.10.5 Promoting Deformed Parts

3.11 21BLayers

3.12 22BPart Parameters

3.13 23BPart Units

4 Assembly Modeling Standards

4.1 24BAssembly Modeling Practice

4.2 25BTolerances

4.3 26BModel Notes

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4.4 27BAssembly Default Datums

4.5 28BAssembly File Names

4.6 29BModel Views

4.7 30BAssembly Layers

4.8 31BBulk Items

4.9 32BAssembly Parameters

4.10 33BRelations

4.11 34BSurface Finishes

4.12 35BReference Objects

4.13 36BAssembly Units

5 Drawing Creation Standard

5.1 37BDimensions

5.2 38BGeometric tolerances

5.3 39BFormats

5.4 40BDrawing Setup Files

5.5 41BDrawing Standards

5.6 42BNotes

5.7 43BDrawing Views

5.8 44BDrawing Line-Weights

5.9 45BQuality Assurance Information

5.10 46BDistribution Statement

5.11 47BRevision Block

5.12 48BAssociated Models

5.13 49BParameters

5.14 50BLayers

5.15 51BFile Names

5.16 52BDrawing BOM Balloons

6 Templates

6.1 61BStart Parts

6.2 62BFormats

7 Electrical

7.1 116BSchematics

7.2 117B2D Drawings

7.3 118B3D Harness Modeling

7.4 119BElectrical Checklists

8 Piping

8.1 120BGeneral Overview

8.2 121BLine Stock Overview

8.3 122BCreating Routes / Pipelines

8.4 123BFittings and Other Piping Parts

8.5 124BFabricating / Creating Solid Pipes

8.6 Pipe Centerlines

8.7 125BSchematics

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8.8 126BPiping Checklists

Appendices

A Modeling Best Practices

A.1 63BPart Mode

A.2 64BDrawing Mode

A.3 65BAssembly Mode

B Poor Modeling Practices

B.1 66BBuried Features

B.2 67BOverwritten Dimensions

B.3 68BBlind Feature Depth (= to material thickness)

B.4 69BExcess Datums/Features

B.5 70BView Name and Scale Not Parametric

B.6 71BBending Back Using the Wrong Sheetmetal Surface

B.7 72B“0” Offset Assembly Mate

B.8 73BCongested Sketches

B.9 74BFlat pattern for Sheetmetal parts

C Miscellaneous Topics, Methods and Techniques

C.1 75BModel Relations

C.2 76BAssembly Relations

C.3 77BPROGRAM – From File vs From Model

C.4 78BCreo Parametric Layers

C.5 80BGeometric Dimensioning and Tolerance (GD&T) used in Creo Parametric

C.6 81BDatum Planes and GTOL

C.7 82BGTOL Datum Features Visibility

C.8 83BModelCHECK Process

C.9 84BGeometry Checks

C.10 85BMapkeys

C.11 86BSymbols

C.12 87BSkeletons and Assemblies

C.13 88BInstallation “Split Balloon” Find Number Technique

C.14 89BCreo Parametric pen table settings (default)

C.15 90BPDF print settings

C.16 91BPM-MTV Default configuration file settings

C.17 92BAnnotation Features

C.18 93BRelations (default)

C.19 94BCHECK mapkey

C.20 95BComponent Interface functionality

C.21 96BAUTO_PART_NUMBER functionality

C.22 97BItem ID

C.23 98BMass Properties – Manual Input

C.24 99BMilitary parts and Vendor parts

C.25 100BVendor supplied 3D models

C.26 102BNext Assembly Parameter

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C.27 103BHandling a Cancelled ECP

C.28 104BKeep All Down Parts and Drawing at Same Revision when Promoting

C.29 104BWeldments

D Procedures

D.1 105BCreating a new file

D.2 107BFamily Table Drawing Creation Procedure

D.3 109B2D Lightweight Backdrop Creation

D.4 110B3D Lightweight Backdrop Creation

129B3D-Backdrop Creation Checklist / Reference Guide

D.5 111BChecklists

D.6 112BProcedure for Promoting Objects to a new Revision

D.7 113BSuperseded and Obsolete Parts

D.8 114BLabels and Nameplate Modeling Procedure

D.9 115BInstallation Drawings/Assemblies

E Vehicle Coordinate System

E.1 53BVehicle Coordinate System (VCS)

E.2 54BCab Body Coordinate System (CBCS)

E.3 55BRoadside (aka RS and Driver Side) and Curbside (aka CS and Passenger Side)

F Special Part and Drawing Types

F.1 Standard Parts

F.2 Common Parts

F.3 132BDeformed parts

F.4 133BVendor Item Control Drawings

F.5 134BSource Control Drawings

F.6 135BInstallation Drawings

F.7 136BA1R ECP parts

References

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Table of Figures

Figure 1: ECP2 Release Level Flowchart

Table 1: Model Name Suffix Usage

Table 2: Part Layers

Table 3: Part parameters

Figure 2: Current Design Activity Cage Code

Table 4: Unit Systems

Table 5: Assembly Layers

Table 6: Drawing Line Weights

Table 7: Object Parameters

Table 8: Drawing Format Files

Table 9: Spool File Parameters

Figure 3: diagram_circuit_list.tble Example

Figure 5: Connector Example

Figure 6: Phantom Box Example

Figure 7: Twisted Pair(s) Example - Rigid vs. Smooth

Figure 8: Wire Break Example

Figure 9: Harness_BOM.tbl sample

Figure 10: Connector Assembly Example

Table 12: Harness Assembly Checklist

Table 13: Connector Assemblies Checklist

Table 14: Harness Part Checklist

Table 15: Drawing File Setup Checklist

Table 16: Harness Layout & Views Checklist

Table 17: Harness Dimensions Checklist

Table 18: BOM Table & Balloons Checklist

Table 19: Notes & Revision Block Checklist

Table 20: Sheet Setup Checklist

Table 21: Connectors & Symbols Checklist

Table 22: Wires & Cables Checklist

Table 23: Tables Checklist

Table 24: Notes & Revision Block Checklist

Figure 11: Commonspace Folder Structure

Figure 12: SAE Line Stock Example

Figure 13: SAE Line Stock Example

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Figure 14: Line Stock Create / Read

Figure 15: Line Stock Set-Up

Figure 16: Line Stock Design Rule Parameters

Figure 17: Line Stock Defined Tab

Figure 18: .TXT File of a Line Stock

Table 25: Piping Assembly Specific Parameters

Figure 19: Sample Hose Flowing Into Port and Z-axis Direction

Figure 20: Example of Creating Pipe Route in Segments vs. Following Curve

Figure 21: Two Examples of a Sample Tee Fitting w/ Entry Ports

Figure 22: Creating Pipeline

Figure 23: Fabricating Pipeline

Figure 24: Fabricated Pipeline

Figure 25: Sample Creo Piping Drawing Tree

Figure 26: Sample Schematic Line connection List

Figure 27: Symbol Legend Example

Figure 28: Color Legend Example

Figure 29: Sample Piping Diagram

Table 26: Piping Assembly Checklist

Table 27: Pipe Chart Checklist

Table 28: Sheet Setup Checklist

Table 29: Tables Checklist

Table 30: Notes & Revision Block Checklist

Figure 30: Layer Tree

Figure 31: Setting Visibility of Layers

Figure 32: Initiate GTOL

Figure 33: GTOL Model References Tab

Figure 34: GTOL Datum References Tab

Figure 35: GTOL Tolerance Value Tab

Figure 36: GTOL Symbols Tab

Figure 37: Initiating ModelCHECK

Figure 38: ModelCHECK Summary

Figure 39: ModelCHECK Types

Figure 40: Example of ModelCHECK Report

Figure 41: Beginning With Skeletons

Figure 42: 2D Curves and CSYS For Assembly

Figure 43: Imported Phantom Geometry

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Figure 44: Component Placement Dialog Box

Figure 45: Top View of Cab Assembly

Figure 46: Rear View of Cab Assembly

Figure 47: Completed Drawing - Cab Side View

Figure 48: Completed Drawing - Cab Top View

Figure 49: Reference Balloon Format

Figure 50: Steps to Insert Split Balloon Table

Figure 51: Split Balloon Table

Figure 52: Completed Split Balloon BOM Table

Figure 53: Example of Split Balloons on Drawing

Figure 54: Unfiltered BOM for Bulk Tubing

Figure 55: Filtered BOM for Bulk Tubing

Figure 56: Bulk Length define in views

Figure 57: Split Balloon Symbol

Figure 58: Relations for the cut length in the PARTS LIST

Table 31: Start Part Relations

Figure 59: Setup Mass Properties

Figure 60: Mass Properties Parameter

Figure 61: Assembly Structure - Next_Assy

Figure 62: Next Assembly List

Figure 63: Sample Weldment Parts List

Figure 64: Family Table

Figure 65: Family Table in Drawing

Figure 66: Entering Text in Table

Figure 67: Completed Family Table

Figure 68: Establish Offset CSYS

Figure 69: Create 2 - 1mm X 1mm Curves

Figure 70: Another 1mm X 1mm Curve Set

Figure 71: Create DXF from New Drawing

Figure 72: Create Required Views for Installation Drawings

Figure 73: Inspect Lines

Figure 74: Make other Views

Figure 75: Create Backdrop Parts

Figure 76: Create Coordinate System

Figure 77: Cleanup - Edit Definition

Figure 78: Delete 4 Format Lines

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Figure 79: Change Line Font

Figure 80: Completed Lightweight 2D Backdrop

Figure 81: Completed Lightweight Assembly

Figure 82 Completed Installation Assembly

Figure 83: Begin Installation Drawing

Figure 84: Installation Drawing Cleanup

Figure 85: Installation Drawing Cleanup - Component Display

Figure 86: Installation Drawing Cleanup - Blank Components

Figure 87: Completed Installation Drawing

Figure 88: Backdrop Assembly Tree

Figure 89: Create 3D Backdrop Part

Figure 90: Create Shrinkwrap Feature

Figure 91: Select Shrinkwrap Reference Model

Figure 92: Confirm Reference Model Selection

Figure 93: Choose Appropriate Options

Figure 94: Verify Required Geometry is Present

Figure 95: Toggle off "Dependent" Option

Figure 96: Access Appearance Editor

Figure 97: Select Gray Color

Figure 98: Select Geometry to Apply Color

Figure 99: Set Transparency

Figure 100: Resulting 3D Backdrop

Figure 101: Final Model Tree

Table 32: CM Checklist

Table 33: Standard Model Checklist

Table 34: PDF Drawing Checklist

Table 35: Vendor / Legacy / Standard Part Model Checklist

Figure 102: From-To Example

Figure 103: Superseded Callout

Figure 104: VCS established on roadside frame rail

Figure 105: VCS in Default view

Figure 106: VCS with framerail

Figure 107: VCS in default with framerail

Figure 108: Front Cab Mount Installation with VCS

Figure 109: Front Cab Mount assembly constraint

Figure 110: Front Cab Mount Installed

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Figure 111: CBCS offset from VCS dimensions

Figure 112: CBCS in Default orientation

Figure 113: Specification Parts Kit

Table 36: Reference Documentation List

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1 Foreword

This standard describes the requirements and procedures for the Three Dimensional Technical Data

Package (3D/TDP) solid model repository established and maintained by PdM-MTV. The 3D/TDP is based on

Creo Parametric Mechanical Design Automation software for the purpose of Computer Aided Design (CAD).

The 3D/TDP uses Windchill PDMLink Product Data Management (PDM) software for data management and storage. Creo Parametric and Windchill PDMLink are both products of PTC. All contractors and government personnel working with models contained within the 3D/TDP system shall follow the requirements of this standard regarding both Creo Parametric and Windchill PDMLink. Documents that are not solid model related but which normally comprise a TDP such as packaging sheets, quality assurance provisions, electrical schematics, etc. shall be stored in Windchill PDMLink.

1.1 0BBackground

In order to take advantage of available technologies, PdM-MTV has been maintaining the technical data system including 3D solid models. The intent is to develop, maintain, and provide these 3D/TDPs throughout the lifecycle of the item. 3D/TDPs will be used for development, production, life cycle management, configuration management, logistics support, and all other purposes that would normally use technical data. The

3D based system will have the following advantages:

Automated generation and update of line drawings

Automated Bills Of Material (BOM)

Infinite viewpoints and exploded views of assemblies

Rapid prototyping

Faster design updates

Improved logistics support

Improved system interface analysis

Better and faster engineering analysis capabilities (kinematic, dynamic, and structural analysis, tooling design, etc.)

Reduced TDP interpretation errors

In order to use solid models as a basis for the technical data it is important that the solid models be built to a set of common standards, using sound modeling practices, and be fully defined. Performing cosmetic modeling (in which a model looks like it is supposed to but is actually dimensionally incorrect), may be faster and easier; however, as a basis for product definition is inadequate.

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Appendix D.5 Checklists referenced within this standard, defines required criteria for promotion approval to the Released state. Any requirements made by this standard must be met, whether or not they are cited on the checklist.

The PdM-MTV Windchill User Guide document, referenced within this standard, defines procedures to be followed when using Windchill PDMLink in conjuncture with the 3D/TDP effort.

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2 Configuration Management Representations

2.1 1BStandards Application

The requirements of this specification apply to all objects, parts, assemblies, and/or drawings that are submitted through the formal release process via Windchill Change Notice from In Work to Released.

2.2 2BDrawings Required

All parts and assemblies promoted to Released shall have associated, fully defined 2D drawings or a PDF copy of the latest (requires prior PdM-MTV approval for PDF). Only the models/drawings representing the latest design configuration (i.e., the latest revision drawing plus any outstanding ECPs) shall be promoted through the release process. This does not apply to Standard Parts, which are defined in Appendix F.

2.3 Engineering Changes

Models and drawings shall be changed via approved Engineering Change Proposals (ECPs) only. ECPs shall conform to SAE EIA-649-1.

2.4 3BConfiguration Management

When 3D/TDP associated 2D drawing are released in the database that drawing becomes the master for configuration management purposes (i.e. drawings will not be input into the 3D/TDP and concurrently maintained in another CAD format.) Refer to SAE EIA-649-1 for complete Configuration Management standards.

2.5 4BProducts

The Product in Windchill PDMLink for the FMTV 3D solid modeling TDP will provide enough detail for files to be checked into the database in the appropriate location.

2.6 5BObject Status

The user making changes on a drawing, part, assembly, or other object for release in the FMTV database shall set the Commonspace status to Checked Out while change is in progress. The status should be applied when the drawings are identified for the ECP.

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2.7 6BSecurity

This system security falls under the Windchill system security settings.

2.8 7BRevision Scheme

The initial release of drawings, parts and assemblies will be the - revision level. Subsequent changes will be from a one to three digit alphabetic character (not including letters I , O , Q , S , X , or Z . (i.e., A, B, C,… AA, AB, AC, … YYV, YYW, YYY.) Refer to ASME Y14.35 for further information about

Revision Scheme.

2.8.1 The part or assembly revision scheme is dependent to its associated drawing and vice versa. The

Creo Parametric drawing, and model revision shall be the same for FMTV drawings/models. All changes to model and drawing will follow formal ECP procedures.

2.8.2 The revision of the drawing shall be displayed on all drawing sheets in accordance with the current acceptable drawing format. As new revisions of the models and drawings are created the next higher revision will be used for the current drawing.

2.9 8BPromotion

Drawings submitted for promotion shall follow instructions found in PdM-MTV Windchill User Guide.

2.10 9BQuality Assurance

All parts, assemblies, and drawings submitted for promotion shall be checked in accordance with

Appendix D.5 Checklists. All Creo Parametric objects promoted to Released are required to pass the FMTV

ModelCHECK process.

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2.11 10BRelease Level Flowchart

The following flowchart illustrates the FMTV release scheme using the ECP2 or ERR process in

Windchill PDMLink.

FIGURE 1: ECP2 RELEASE LEVEL FLOWCHART

2.12 Notice of Revision

The Notice of Revision (NOR) document shall be a redline markup of the previous revision of the drawing. If the drawing is an Initial Release drawing, the NOR is not required. The NOR/redline shall be submitted and stored with the ECP document.

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3 Part Modeling Standards

3.1 11BPart Modeling Practice

3.1.1 Parts should be functional and created in a logical sequence. Features should be simple and be created such that they are easily modifiable by another user. Parts shall have every feature that the real part is required to have. For example, plastic parts should contain every draft angle and radii detail expected on the real part. If text (e.g. part number) is stamped or molded into a part, that should also be modeled. Parts should be able to stand on their own without reference to other parts or assemblies.

3.1.1.1 If the part is a source controlled drawing or vendor item control drawing, CAD Files from the vendor will be requested. If the CAD file is unavailable, all interface and envelope dimensions shown on the drawing shall be modeled. The part shall be modeled in Creo

Parametric.

3.1.1.2 For Creo Parametric conversion efforts, features will be created using the existing dimensioning scheme contained in the drawings or other appropriate source. All changes to the drawing shall be documented by the NOR/ECP.

3.1.1.3 For new parts and design changes, features will be created in a logical manner in which the dimensioning scheme for the new part will be shown with no created dimensions on the drawing (unless required).

3.1.2 All models shall regenerate successfully with all features in the unsuppressed state. When parts are modified, the next higher assembly shall also be capable of being successfully regenerated.

3.1.3 The latest FMTV_START_PART or FMTV_START_ SHTML _PART shall be used for part creation.

3.1.4 Sheetmetal parts shall be created with the Creo Parametric Sheetmetal module.

3.1.5 All routed tubing or piping models and assemblies shall be created using the Creo Piping and

Cabling Extension.

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3.1.6 All wiring and cabling models and assemblies shall be created using a combination of Creo Piping and Cabling Extension.

3.2 12BTolerances

All dimensions shall include tolerances as required to be shown appropriately on the drawing. When geometric tolerances, geometric tolerance datums, inspection dimensions, datum targets, and/or basic dimensions are required, these shall be set in the model using the appropriate GTOL commands.

3.3 13BMaterials

Materials shall be identified on the part in two locations:

1. The materials section under Model Properties in Creo Parametric. Material file creation shall be requested from the custodian of the material file library for any material required that is not in the current library.

2. In the materials note section of the 3D notes which are applied to the drawing.

3. The material file used on the part shall match the material called out in the notes (for example: ASTM

A36 material file shall be used over a generic STEEL material file)

3.4 14BSurface Finishes

Surface finishes shall be shown on the part as required.

3.5 15BModel Notes

Sufficient model notes (annotations) shall be used to describe the part and part features. If notes are intended to apply to specific features, they shall be attached to those features. Notes found in the FMTV start parts include:

a. Distribution_Note: The drawing distribution statement shall be included in this note.

b. Proprietary_Note: If a proprietary legend is required on the drawing, this legend shall be entered on the model in this note.

c. Export_Control_Note: The drawing export control warning note shall be included in this note.

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d. Design_Intent_Note: This note shall be used to document design intent. Design Intent is any optional information the designer believes is valuable to those who might view the model at some future point.

An example of design intent note is as follows:

THIS PART IS MADE OF ALUMINUM 7075-T6. CARBON STEEL WAS

TESTED BUT CORRODED DURING USE. USE OF STAINLESS WAS

CONSIDERED BUT NOT PURSUED DUE TO TIME CONSTRAINTS.

e. DRW_NOTE: This note shall be used to document all drawing notes required to be shown on the drawing. The note information within DRW_NOTE shall be listed in numerical sequence as started in the FMTV start models. This note is the one that is listed on the first column of the drawing. Example:

1. APPLICABLE STANDARDS / SPECIFICATIONS:

A. ASME Y14.100-2013

B. ASME Y14.5-2009

2. MATERIAL:

3. IEEE/ASTM SI 10 SHALL BE USED IN CONVERTING

AND ROUNDING OFF. 1 INCH = 25.4 mm APPLIES.

4. FINISH:

5. REMOVE ALL BURRS AND BREAK SHARP EDGES.

6. DIMENSIONAL LIMITS APPLY BEFORE PAINTING.

7.

8.

Etc.…

If additional drawing note columns are required, additional note(s) shall be created to document new column information (i.e. DRW_NOTE_2, DRW_NOTE_3) and associated parametric notes shall be created on the drawing (i.e. &DRW_NOTE_2, &DRW_NOTE_3).

Earlier DRW_NOTE was structured with separate notes (Note1, Note2, Note3, Note4, Note5, etc.…) which was then summarized by DRW_NOTE. Existing models that follow this format can remain the same and are not required to be changed to follow the current DRW_NOTE format.

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3.6 16BRelations

Relations shall have no errors upon regeneration. Relations found in feature CS0 and ACS0 of the FMTV start models are required.

3.7 17BDefault Datums

All parts will start with default datum planes and a default coordinate system identical to those found in the FMTV start models. The default datum planes shall be named FRONT, TOP, and SIDE. The coordinate system shall be named CS0 with its orientation as follows; Z-axis is elevation, X-axis is along the length of the vehicle, Y-axis across the vehicle width.

3.8 18BPart File Names

Parts shall be named using the following convention:

CAGE_PartNumber.prt i.e. 19207_8448510.prt

If the model requires an extension (or suffix) it will follow the convention described in Table 1 – Model

Name Suffix Usage.

Suffix Range Description

-001 -399 Fully detailed down level parts on a drawing.

-100 -150

Down-Level detailed parts that are part of weldment that are the same base number of the weldment assembly. (Note: This is an overlap for the -001 thru -399, but the down-level weldment parts are to start at -

100. Fully detailed parts are still allowed to use -100 thru -150).

-400 -499 Parts modified in the field for the application of a kit.

-500 -599 Non-detailed down level parts on a drawing.

-5000 - Top Level 87T – Used for Large Assemblies

-600 -699 Routed systems models (cabling, piping, etc.…)

-6000 -6999 Overflow for routed systems models (cabling, piping, etc.…) if more than the original -600 through -699 are required

-6circuit# Used for routed systems where circuit number is part of the suffix

-700 -799 Simulation models (as well as the extension _FEA)

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-800 -899 Backdrop Parts / Assemblies

-900 -998

Overflow or for miscellaneous (deformed, die, shrinkwrap parts, etc.)

Deformed parts may also use the _def naming convention. Same intent for dies and shrinkwraps.

-9000 -9999 Overflow or miscellaneous parts if more than the original -900 through -

998 are required.

-999 or -gen Non-useful generic components used in Family Tables.

_skel Skeleton Models

-opt, -oc Optional Configuration (either is acceptable)

-cast Use for castings when a casting is an Alternate Design

TABLE 1: MODEL NAME SUFFIX USAGE

127B3.8.1 Hardware File Names

Hardware naming convention shall generally start with -001 and is not required to follow Section 3.8.

128B3.8.2 Exceptions

- Refer to Section 7 - Electrical for naming convention on Schematics and Electrical related components.

- Refer to Section 8 - Piping for naming convention for Piping Assemblies.

3.9 19BModel Views

All models shall have separately named views defining the TOP_VIEW, BOTTOM_VIEW, LEFT_VIEW, RIGHT_VIEW, BACK_VIEW, FRONT_VIEW, and DEFAULT views. These views exist in the FMTV start part. The FRONT view is oriented facing the yellow (or primary) side of the FRONT datum plane, with the yellow side of the TOP datum plane facing up. The remaining orthogonal views follow standard third angle projection practice. Current drawing models should be created such that the named views correspond to the existing drawing views.

3.10 20BDeformed Parts

Deformed parts will have to be handled on a case to case basis. If a part can be deformed in numerous shapes (rivets), then use the non-deformed part. This makes it easier, rather than having 100+ deformed parts.

In addition, Flexible Components shall be considered first and is preferred over a deformed part. This will help keep the data management aspect to a minimum.

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3.10.1 Naming Convention for Deformed Parts

Only use the non-deformed part’s part number with the extension starting with a -9xx. Also, -9xxx can be used if there are numerous instances of the deformed parts. Do not use the top assembly name with -900 as was previously used.

3.10.2 When to use Deformed Parts

1. Create a deformed part if it will only be needed on a particular drawing. (Examples are lanyards, cables, etc.).

2. Create a deformed part if the non-deformed part causes a major interference.

3. Create a deformed part if the non-deformed part will not work in any way possible.

3.10.3 Creating Deformed Parts from Tabulated Parts

If a deformed part is made from a tabulated part, keep the tabulation and add the -900 extension after.

(Ex: 19207_12345678-001 will be 19207_12345678-001-900 when it is deformed).

3.10.4 Creating Deformed Parts with Flexible Components

The preferred option when creating deformed parts is using flexible component functionality. Flexible components allow the model to be represented in different states within different assemblies. Flexible components shall always be looked at first for any deformed part/assembly. An example of this is if a drawing of a spring requires it to be modeled in its free state but when it needs to be assembled it must be represented in its compressed state. With flexible component functionality it would not require that a second model to be created. It allows the designer to vary dimensions, parameters, resume or suppress features (or components if flexible component is a sub-assembly).

3.10.5 Promoting Deformed Parts

When promoting a deformed part, promote it with the assembly where the deformed part is used. Keep the deformed part at the same revision level of the most current non-deformed part in Windchill PDMLink database. Also, remember to relate all deformed parts back to the non-deformed parts drawing while the drawing is being updated. If the deformed part is just being used on a next higher assembly, it shall be related back to

FMTV-MODELING-STD-100T Rev.M Page 12 14 March 2016 the deformed parts drawing the next time the drawing is revised. When a previously released deformed part is required to be changed in an ECP due to other changes that affect said part and the base part is not part of that

ECP, either a new flexible model state or a standalone model shall be created with another -9xx extension. The new model shall have the same revision as the base number.

3.11 21BLayers

The following layers shall be used in part mode (these exist in the FMTV start part). Other layers may be added as needed, for example, a datum required on a drawing may be placed on a separate layer so that it can stay on while the other datums are layered off.

Layer name Layer Assignments Default

State

a. DTM_AXES All datum axes Hide

b. DTM_CSYS All datum coordinate systems Hide

c. DTM_CURVES All curve features Hide

d. DTM_PLANES All datum plane features Hide

e. DTM_POINTS All datum point features Hide

f. G_DTM_PLANES All geometric tolerance datum planes Hide

g. ITEM_ID Only the cosmetic/curve feature describing the part identification number Hide

h. NOTES All part notes Hide

i. SURFACES All surface features and quilts Hide

j. THREADS All cosmetic and actual threads Hide

k. XSEC_DATUMS All cross-section datums Hide

TABLE 2: PART LAYERS

FMTV-MODELING-STD-100T Rev.M Page 13 14 March 2016

3.12 22BPart Parameters

The following parameters are required when entering a part or assembly into the 3D/TDP Product Release Process. Required items are noted in the Input column.

Line # PARAMETER NAME TYPE PARAMETER DESCRIPTION

FORMAT

EXAMPLE

POPULATE

PARAMETERS FOR

INITIAL DELIVERY

(REQ=REQUIRED)

PLM

SEARCHABLE

(DESIGNATED)?

1 AGENCY String Agency or service US ARMY REQ Yes

2 AUTO_PART_NUMBER Yes No Used in relation to generate Part_Number attribute Yes No

3 CABLING_ASSY Yes No Used in relation to when working on a Electrical Cabling

No No

CAGE_CODE

String

Original Design Activity CAGE code-The activity originally authorizing/creating the design. For TACOM Army Ordnance Part

Numbers, use 19207; commercial designs use original design manufacturer

CAGE corresponding to the original design manufacturer’s part number in parameter name PART_NUMBER

19207

REQ

Yes

5 CHECKER_NAME String Person that checked the original drawing E.KHALIL REQ No

6 CIRCUIT_NUMBER String Circuit Number used for Electrical Cables / Hydraulic Hoses (Manually generated when PIPING_ASSY set to Yes)

J159 No

7 CONTRACT_NUMBER String Contract # under which technical data is being delivered W31P4Q-11-R-0043 REQ Yes

8 CRITICAL_SAFETY_ITEM Yes-No Part Criticality to System Operation YES REQ Yes

DATA_RIGHTS_CODE

Data rights concern the ability to modify, reproduce, perform, display, release, or disclose recorded information.

U - Unlimited Rights. All uses for all purposes, Government and

Commercial.

G - Government Purpose Rights. All uses, but only for Government purposes.

L - Limited. Internal Government use for Government purpose with very little else authorized.

R - Restricted Rights. Internal Government use for Government purpose with very little else authorized.

SB - Small Business Innovative Research (SBIR). A special catch-all category

(SBIR Rights) and alters the normal use of some of the other legends. When dealing with a SBIR contract, the SBIR data rights clause must be applied.

SL - Special License Rights. As specified by the negotiated contract terms.

Often used to alter the default rights under the clauses or agree to an apportionment of rights which does not fit neatly into the default categories.

U

FMTV-MODELING-STD-100T Rev.M Page 14 14 March 2016

DESIGN_ACTIVITY

Design activity

TANK AUTOMOTIVE

& ARMAMENTS

COMMAND

11 DESIGN_ACTIVITY_LOCATION String Design activity city, state and zip code

WARREN,

MICHIGAN 48397-

REQ Yes

12 DESIGN_APPROVAL_NAME String Government approver name for engineering design J.DAVIS *REQ Yes

DESIGN_CONTRACTOR

Contractor/Agency/Office physically creating drawings and models for the original design activity (optional with commercial data; mandatory with

Government funded noncommercial or mixed funded product data)

STEWART &

STEVENSON

SERVICES, SEALY

TEXAS U.S.A.

DISTRIBUTION_CODE

Technical Distribution Statement Code (DoDD 5230.24)

A (Approved for public release; distribution is unlimited)

B (Distribution authorized to U.S. Government Agencies only)

C (Distribution authorized to U.S. Government Agencies and their contractors)

D (Distribution authorized to the Department of Defense and U.S. DoD contractors only)

E (Distribution authorized to DoD Components only)

F (Further dissemination only as directed)

X (Distribution authorized to U.S. Government Agencies and private individuals or enterprises eligible to obtain export-controlled technical data)

D

15 DRAWING_APPROVAL_NAME String Government approver name of drawing. J.ZEBROWSKI *REQ Yes

16 DRAWING_DATE String Date original drawing created 12/4/2013 REQ No

17 DRAWING_NUMBER String Drawing number the part/assembly is defined on 12414568 REQ Yes

18 DRAWN_BY String Person who created original drawing J.DAVIS REQ No

19 ENGINEER_NAME_1 String Primary design engineer C.GOWARD REQ No

20 ENGINEER_NAME_2 String Secondary design engineer A.WURFEL No

21 ERR_ECP_APPROVAL String Government approving official of latest ECP W.DEARMIT **REQ No

22 ERR_ECP_DATE String Date current revision was released 12/9/2020 **REQ No

ERR_ECP_NUMBER

Approved Engineering Change Proposal (ECP), Change Request or Change Order, Change Notice, or Engineering Release Record (ERR) authorizing initial release or new revision. (For Level 3 product data the three-character contractor name prefix as assigned by the government followed by the 5 alpha-numeric characters the

Contractor assigns from the Government-issued block of ECP/ERR numbers.) ERR number required for level 3 product data at initial Product Baseline and beyond;

ECP or contractor’s change documentation number required for tech data prior to

Product Baseline. (if assigned, otherwise put “NA”)

TACV1234

**REQ

No

24 EXPORT_CONTROL Yes No Controlled by International Traffic in Arms Regulation YES REQ Yes

FMTV-MODELING-STD-100T Rev.M Page 15 14 March 2016

25 HOSE_LENGTH

Real

Number

Hose Length – Relation generated by PRO_MP_MASS /

WEIGHT_PER_LENGTH. Automatically generated when PIPING_ASSY set to YES

12.5 No

26 MATERIAL_ENGINEER String Person who approved material for design K.TEBEAU REQ No

27 MATERIAL_TYPE String Material type used for part or assembly Steel REQ No

28 MODEL_CHECK String ModelCHECK last run on object Thu Mar 26 2009

10:45:05 GMT-0500

No

29 MODEL_REV String Only alpha revisions following ASME Y 14.35M revision standard allowed after Product Baseline release for production Product Data. . REQ Yes

30 MODELER_NAME_1 String Primary Creo Parametric modeler R.BRNJAC REQ No

31 NEXT_ASSY_1 String First next higher assy part no. (shall match USED_ON_1 above) 12419847 REQ No

32 NEXT_ASSY_2 String Second next higher assy part no. 12586793 No

33 NEXT_ASSY_3 String Third next higher assy part no. 12957485 No

34 NEXT_ASSY_4 String Fourth next higher assy part no. 12456873 No

35 NEXT_ASSY_5 String Fifth next higher assy part no. 12213484 No

36 NEXT_ASSY_6 String Sixth next higher assy part no. 12436875 No

37 NEXT_ASSY_7 String Seventh next higher assy part no. 12435623 No

38 NEXT_ASSY_8 String Eighth next higher assy part no. 12986458

No

39 NOMENCLATURE String Drawing name. It can be a combination of the three nomenclature lines or represents only the first line.

BODY ASSEMBLY,

CARGO, MTV LWB REQ Yes

40 NOMENCLATURE_1 String First line of drawing nomenclature BODY ASSEMBLY, No

41 NOMENCLATURE_2 String Second line of drawing nomenclature CARGO, MTV LWB No

42 NOMENCLATURE_3 String Third line of drawing nomenclature No

43 PART_NUMBER String Item part number 12423205 REQ Yes

44 PIPING_ASSY Yes No Defines if the assembly is a piping assembly Yes No

45 PMIC String Precious Metal Indicator Code A No

46 QA_ENGINEER_NAME String Quality assurance engineer C.JONES REQ No

47 REMARKS String Remarks PRELIMINARY REQ (See 3.12.2) No

48 SPEC_NUMBER String Spec number MIL-STD-105 No

49 TOLERANCE_1_PLACE String Default tolerance if indicated on drawing No

50 TOLERANCE_2_PLACE String Default tolerance if indicated on drawing No

51 TOLERANCE_3_PLACE String Default tolerance if indicated on drawing No

52 TOLERANCE_ANG String Default tolerance if indicated on drawing No

FMTV-MODELING-STD-100T Rev.M Page 16 14 March 2016

UID_MARKABLE

Yes No In accordance with contract requirements, indicate if part requires

Unique Identification (UID) marking

YES

54 UNIT_WEIGHT

Real

Number Mass value 1.25 REQ No

55 USED_ON_1 String First used on item M270A1 REQ No

56 USED_ON_2 String Second used on item No

57 USED_ON_3 String Third used on item No

58 USED_ON_4 String Fourth used on item No

59 USED_ON_5 String Fifth used on item No

60 USED_ON_6 String Sixth used on item No

61 USED_ON_7 String Seventh used on item No

62 USED_ON_8 String Eighth used on item No

63 WEIGHT_PER_LENGTH

Real

Number

Numeric Value of the weight/length given in the line stock file (manually entered, should be the same as line stock file) .00417 No

64 WEIGHT_UNIT String Automatically filled out - toolkit application lb REQ No

TABLE 3: PART PARAMETERS

* Parameter value will be added after approval.

** Parameters are 'REQ' when relevant.

Page 17 14 March 2016 FMTV-MODELING-STD-100T Rev.M

3.12.1 The parameter CAGE_CODE refers to the original design activity. If the current design activity is different than the original design activity then the current one is entered into the

CURRENT_CAGE_CODE field. A table must also be placed on the drawing showing the current design activity cage code (see sample below).

FIGURE 2: CURRENT DESIGN ACTIVITY CAGE CODE

3.12.2 The parameter REMARKS should initially default to PRELIMINARY. This will automatically appear on the drawing until the value is removed during the final stage of the release process.

3.12.3 The parameter NOMENCLATURE will automatically be assigned a value based upon

FMTV start part relations. The value is equal to the sum of the individual parameters

NOMENCLATURE_1, NOMENCLATURE_2, and NOMENCLATURE_3, which shall be entered appropriately by the modeler.

3.12.4 The part or assembly parameter UNIT_WEIGHT is automatically filled out by Creo

Parametric (PRO_MP_MASS calculated parameter) when the part or assembly is regenerated.

This is accomplished using relations found in the FMTV start parts. The parameter value for unit weight shall be representative of the weight of its true physical counterpart.

3.13 23BPart Units

Creo Parametric system units shall match the following:

Unit type METRIC ENGLISH

Length mm in

Mass kg lbm

Time sec sec

Temp ºC ºF

TABLE 4: UNIT SYSTEMS

Note: English and metric unit systems exist in the FMTV start parts

Page 18 14 March 2016

4 Assembly Modeling Standards

4.1 24BAssembly Modeling Practice

4.1.1 Assemblies shall have all components and features of the assemblies defined, including pins, screws, nuts, washers, the part number etc. This includes items such as decals, warning labels, bulk items, etc., which are required to be attached to the assembly.

4.1.2 Assembly of models shall follow a logical sequence.

4.1.3 Assembly features shall only be used for features manufactured at the assembly level and not for features created on individual parts.

4.1.4 All assembly models shall regenerate successfully with all features and components in the unsuppressed status. When assemblies are modified, the next higher assembly shall also be capable of being successfully regenerated.

4.1.5 All assembly components shall be fully constrained unless the function of the assembly benefits from adding certain degrees of freedom through connections. The FIX constraint should avoid being used. The use of Creo Mechanism joints, for example, is acceptable in this case.

4.1.6 The latest FMTV_START_ASSY shall be used for assembly creation.

4.2 25BTolerances

Refer to Section 3.2 Tolerances.

4.3 26BModel Notes

Refer to Section 3.5 Model Notes.

4.4 27BAssembly Default Datums

All assemblies will start with default datum planes and a default coordinate system identical to those found in the FMTV start parts. The default datum planes shall be named FRONT_ASSY, Page 19 14 March 2016

TOP_ASSY, and SIDE_ASSY. The coordinate system shall be named ACS0 with its orientation as follows; Z-axis is elevation, X-axis is along the length of the vehicle, Y-axis across the vehicle width.

4.5 28BAssembly File Names

Assemblies shall be named using the following convention:

CAGE_PartNumber.asm i.e. 19207_12432300.asm

For additional guidelines for assembly naming refer to Section 3.8 Part File Names.

4.6 29BModel Views

All models shall have separately named views defining the TOP_VIEW, BOTTOM_VIEW, LEFT_VIEW, RIGHT_VIEW, BACK_VIEW, FRONT_VIEW, and DEFAULT views. These views exist in the FMTV start part. The FRONT view is oriented facing the yellow (or primary) side of the

FRONT datum plane, with the yellow side of the TOP datum plane facing up. The remaining orthogonal views follow standard third angle projection practice. Current drawing models should be created such that the named views correspond to the existing drawing views. When applicable, the addition of ROADSIDE and CURBSIDE views is recommended.

4.7 30BAssembly Layers

The following layers shall be used in assembly mode (these exist in the FMTV start assembly).

Layer name Layer Assignments Default

State

a. ITEM_ID Only the cosmetic/curve feature describing the part identification number Hide

b. DTM_AXES All datum axes Hide

c. DTM_CSYS All datum coordinate systems Hide

d. DTM_CURVES All curve features Hide

Page 20 14 March 2016

e. DTM_PLANES All datum plane features Hide

f. DTM_POINTS All datum point features Hide

g. G_DTM_PLANES All geometric tolerancing datum planes Hide

h. NOTES All assembly notes Hide

i. SURFACES All surface features and quilts Hide

j. THREADS All cosmetic and actual threads Hide

k. XSEC_DATUMS All cross-section datums Hide

TABLE 5: ASSEMBLY LAYERS

4.8 31BBulk Items

Bulk items are classified into two different categories. These items will be referred to as TYPE

1 and TYPE 2 categories. TYPE 1 bulk items are commodities that are used in a volume, such as adhesives, fluids, lubricants, etc. TYPE 2 bulk items are cut to length or stock parts, such as seals, gaskets, convoluted tubing, tape, etc.

TYPE 1bulk items are non-solid representations of objects within an assembly. They shall be used for all objects that must appear in the Bill of Material or PARTS LIST but do not require solid models. Bulk items shall be used to represent adhesives, lubricants, sealants, paint, etc. Bulk items are a unique subset of the .prt model type and are represented by a unique icon (paint can) in the Creo

Parametric Model Tree. New bulk items can be created by using the start_bulk.prt template in the

Commonspace Templates folder.

It is not acceptable to create a -500 suffix component of the base object in the assembly and add

Table relations to overwrite the parameters reported in the columns. The bulk item shall be created with the proper cage code, name, and description to automatically populate the table repeat region. The typical table relation for bulk items relates the reporting the quantity which is typically set to "AR".

TYPE 2 bulk items shall have a Creo Parametric 3D solid model to represent the item. The models will either fall into the deformed/installed state or flexible component category.

Page 21 14 March 2016

4.9 32BAssembly Parameters

Follow the same guidelines as Section 3.12 Part Parameters.

4.10 33BRelations

Relations shall have no errors upon regeneration. Relations found in feature ACS0 of the FMTV start assembly are required.

4.11 34BSurface Finishes

Surface finishes shall be created on the assembly as required.

4.12 35BReference Objects

Reference components displayed in phantom on installation or similar drawings should not be fully associated 3D models. These should be developed using 2D curve data or 3D model data as required (refer to Appendix D.3 for 2D and Appendix D.4 for 3D Lightweight Backdrop Creation.

Any components specifically defined on the drawing must have a valid associative 3D model as per

Paragraph 4.1.1.

4.13 36BAssembly Units

Follow the same guidelines as Section 3.13 Part Units.

Page 22 14 March 2016

5 Drawing Creation Standard

5.1 37BDimensions

Drawings shall display dimensions that are directly parametric to the model upon which they are based. Specifically, these values shall be either driving or driven dimensions.

5.2 38BGeometric tolerances

Geometric tolerances shall be attached to the base dimensions when applicable and not added as unattached notes.

5.3 39BFormats

Standard FMTV 3D/TDP drawing formats located in the Standard CAD Template Library /

Start Parts and Formats in Windchill PDMLink shall be used.

5.4 40BDrawing Setup Files

Standard FMTV 3D/TDP drawing setup files (.dtl) located in the Standard CAD Template

Library / Configs in Windchill PDMLink shall be used.

5.5 41BDrawing Standards

The drawing standard used shall be ASME Y14.100-2013 and ASME Y14.5-2009. These standards shall be called out in DRW_NOTE of the drawing model.

5.6 42BNotes

All notes on drawings shall originate as model notes in .prt and .asm files, except when deemed necessary.

Page 23 14 March 2016

5.7 43BDrawing Views

2D draft entities shall be related to the drawing view to which it belongs. Views shall be capable of being moved with no entities of the view being left behind.

5.8 44BDrawing Line-Weights

The following line weights and colors shall be used:

COLOR STYLE ITEMS

WHITE Normal Weight object lines, view arrows, format borders

YELLOW Thin Weight leader lines, dimensions, notes, symbols, tables

GRAY Phantom hidden object lines, RED Bold special lines needing extra emphasis

WHITE Phantom Tangent Lines

TABLE 6: DRAWING LINE WEIGHTS

5.9 45BQuality Assurance Information

The preferred method for identifying Quality Assurance Information is on the product drawing instead of having a separate QAP sheet.

5.10 46BDistribution Statement

The drawing distribution statement shall appear on each sheet of a drawing. (This is automatically accomplished when the model note Distribution_Note is filled out in the drawing model.)

5.11 47BRevision Block

Revision blocks shall conform to ASME Y14.35

5.11.1 For legacy conversion ECP’s, include only the latest revision, redrawn with change/redrawn without change and ECP number in lieu of full delineation of the changes on

Page 24 14 March 2016 the drawing for Administrative changes. For individual Major or Minor changes, those changes shall be listed in the revision block.

5.11.2 For design effort ECPs that make drawing changes the revision block shall include the latest revision, redrawn with change, ECP number and full delineation of the changes on the drawing.

5.11.3 For design effort ECPs that release a new drawing the revision block shall include Initial

Release, Product Baseline, and the ECP number.

5.12 48BAssociated Models

All parts that are defined by a drawing shall be related to the drawing even if they are not used in a view on the drawing.

5.13 49BParameters

The following parameters shall be filled out for the drawing model:

Part_Number

Drawing_Date

Drawn_By

Modeler_Name_1

Checker_Name

Engineer_Name_1

Material_Engineer

Design_Approval_Name

Nomenclature

QA_Engineer_Name

Drawing_Number

Revision

Distribution_Code

Itar

Err_Ecp_Number

Page 25 14 March 2016

Err_Ecp_Date*

Err_Ecp_Approval*

* These parameters are not required to be filled out at the In Work state. Their values shall be determined later in the release process.

5.14 50BLayers

Drawing layers may be created as required to properly display information on the drawing.

Layer status may be set (this works independent of the part/assembly) as required to properly display information on the drawing.

5.15 51BFile Names

Drawings shall be named using the following convention:

CAGE_DrawingNumber.drw i.e. 19207_12428511.drw

5.16 52BDrawing BOM Balloons

BOM balloons will use a standard diameter of 0.375 inches (9.525 mm). If the numbers within the balloon extend beyond the balloon then the size of the text will be decreased to best fit within the standard balloon. Refer to Appendix C.13 for additional information.

Page 26 14 March 2016

6 Templates

Creo Parametric object templates are used to customize the default content of newly created objects. Object templates belong to one of two categories: model templates (also known as start parts) and drawing templates. Model templates are standard Creo Parametric models that contain predefined features, layers, parameters, named views, and other attributes. Drawing templates are special drawing files that contain instructions to create d