Attach 0014 - CCDC-AC Procedure 203.03.2 Dimensional Modeling Standards.pdf

Procedure ARDEC 203.03.2

June 2015

U.S. ARMY ARMAMENT, RESEARCH,

DEVELOPMENT & ENGINEERING CENTER

STANDARD PRACTICE

3-DIMENSIONAL MODELING STANDARDS,

GENERAL SPECIFICATION FOR

ARDEC Procedure 203.03.2

NOT MEASUREMENT

SENSITIVE

Comments, suggestions, or questions on this document should be addressed to RDAR-

EIS-P, Rock Island, IL 61299 or e-mailed to john.kreider@us.army.mil.

Table of Contents

1.0 Overview …………………………………………………………… Pg. 4

1.1 Overview ……………………………………………………. Pg. 4

1.1 Definitions …………………………………………………. Pg. 4

2.0 Best Practices ………………………………………………………. Pg. 5

2.1 Part Modeling Practices ………….………………………… Pg. 5

2.2 Assembly Practices …….…………………………………… Pg. 7

2.3 Drawing Practices ………..…………………………………. Pg. 7

3.0 Library ……………………………………………………………… Pg. 8

4.0 Start-Up/Set-Up Files ……………………………………….…….... Pg. 9

4.1 Start Part/Start Assembly …………………………………… Pg. 9

4.2 Drawings ……………………………………………………. Pg. 12

4.3 Configuration Files …………………………………………. Pg. 13

5.0 Part Modeling Requirements ……………………………………….. Pg. 14

5.1 File Name Convention ……………………………………… Pg. 14

5.2 Start Part ……………………………………………………. Pg. 14

5.3 Parameters ………………………………………………….. Pg. 14

5.4 General Notes ………………………………………………. Pg. 14

5.5 Material …………………………………………………..… Pg. 14

5.6 Units ………………………………………………………... Pg. 15

5.7 Conventional Tolerances …………………………………… Pg. 15

5.8 Set Datums …………………………………………………. Pg. 15

5.9 Geometric Tolerances ………………………………….. Pg. 15

5.10 Annotations …………………………………………….. Pg. 15

5.11 Relations ……………………………………………….. Pg. 16

5.12 Family Tables ………………………………………….. Pg. 16

5.13 Flexibility ………………………………………………. Pg. 16

5.14 Calculate Mass Properties ……………………………… Pg. 16

5.15 Layers …………………………………………………... Pg. 16

5.16 Forgings and Castings ………………………………….. Pg. 17

5.17 Sheet Metal …………………………………………….. Pg. 17

5.18 Standard Parts ………………………………………….. Pg. 17

6.0 Assembly Requirements …………………………………………… Pg. 19

6.1 File Name Convention …………………………………….. Pg. 19

6.2 Start Assembly …………………………………………….. Pg. 19

6.3 Parameters …………………………………………………. Pg. 19

6.4 General Notes ……………………………………………… Pg. 19

6.5 Assembly Constraints ……………………………………… Pg. 19

6.6 Flexible Parts ………………………………………………. Pg. 19

6.7 Annotations ………………………………………………… Pg. 19

6.8 Calculate Mass Properties …………………………………. Pg. 20

6.9 Layers ……………………………………………………… Pg. 20

6.10 Color Shading of Components ………………………… Pg. 20

6.11 Bulk Items ……………………………………………… Pg. 20

7.0 Fully Annotated Models …………………………………………... Pg. 22

7.1 View States ……………………………………………....... Pg. 22

7.2 Naming Conventions ……………………………………… Pg. 23

7.3 Annotation Features ………………………………………. Pg. 23

7.4 Datum Axis ……………………………………………….. Pg. 24

7.5 Datum Planes ……………………………………………… Pg. 24

7.6 Isometric Views …………………………………………… Pg. 24

7.7 Fully Annotating Legacy Models ………………………… Pg. 24

8.0 Drawing Requirements ……………………………………………. Pg. 26

8.1 Drawing Formats ………………………………………….. Pg. 26

8.2 General Notes ……………………………………………... Pg. 26

8.3 Drawing Detail Files ………………………………………. Pg. 26

8.4 Drawing Views ……………………………………………. Pg. 26

8.5 Axes ……………………………………………………….. Pg. 26

8.6 Dimensions, Tolerances, and Geometric Tolerances ……… Pg. 26

8.7 Drawing View Notes ………………………………………. Pg. 26

8.8 Surface Finish Symbols ……………………………………. Pg. 26

8.9 Weld Symbols ………………………………………….. Pg. 27

8.10 Assembly Tables ……………………………………….. Pg. 27

8.11 Custom Symbols ……………………………………….. Pg. 27

8.12 Layers ………………………………………………….. Pg. 28

8.13 Revision Block …………………………………………. Pg. 28

9.0 Checking/Verification ………………………..……………………. Pg. 29

9.1 Model Check ………………………………………………. Pg. 29

9.2 Assembly Interference Check ……………………………… Pg. 29

9.3 Manual Check ……………………………………………… Pg. 29

Appendix A – Part, Assembly and Drawing Steps ……………………. Pg. 30

Appendix B – Relations ……………………………………………….. Pg. 32

Appendix C – Drawing Detail Files …………………………………… Pg. 34

Appendix D – Config.pro Files ………………………………………… Pg. 35

Appendix E– Checking/Verification Check Sheets …………………... Pg. 37

1.0 OVERVIEW

1.1 Overview. This document describes the requirements for creating 3D models and drawings for Three Dimensional Technical Data Package (3D TDP) solid model repository, established and maintained by ARDEC. It is intended that models of ARDEC managed components will be stored in a central location accessible by all ARDEC customers, and will be maintained and configuration managed in accordance with standard Army configuration management practices. The procedures enclosed within this document are those utilizing the Pro/Engineer – Creo 2 software, and the ARDEC 3D

Windchill PDM Link data management system.

1.2 Definitions:

Annotations. An annotation is an entity created to store model information without geometry. Annotations consist of notes, symbols, driven dimensions, reference dimensions, geometric tolerances and surface finish symbols.

Drawing. A 2-D representation that may define a part or assembly.

External References. A reference within a CAD object that creates dependencies between itself and another CAD object (s).

Fully Annotated Model. Fully Annotated Models are 3D models with view states containing all annotations within the model. The view states display the annotations in a logical manner to adequately define the model.

Inheritance Feature. Allows one-way associative propagation of geometry and feature data from a reference part to a target part.

Model. A 3-D representation with geometry necessary to define a part or assembly.

Nominal Value. The primary value of a dimension that does not include upper and lower tolerance values; also the average value of a limit dimension. Example of nominal dimensions: .257 +.003/-.003 (nominal value is .257), .250-.265

(nominal value is .2575), .260 max (nominal value is .260).

Parameters. Unique fields within the CAD model containing a string of text, numerical values, dates, or Yes/No data.

Parametric CAD Model. A variable CAD model in which the definition can be varied by modifying its attributes.

Relations. User defined equations written between symbolic dimensions and parameters.

Simplified Representations (Simplified Rep’s). A Pro/Engineer term meaning a subset of the parent model that displays fewer details (components, features, etc.)

than the complete model.

View State. A view state contains all the necessary annotations to completely define a feature. Orientation and cross-sections of a view state are to be such to best represent the feature. ARDEC’s start part/assembly contains ten predefined view states. A view state is typically created for each major feature of the part, and are renamed as appropriate (i.e. MBD2C_Takedown_Lug). Upon completion of part/assembly creation, unused view states are to be removed.

2.0 Best Practices.

2.1 Part Modeling Practice

2.1.1 If the part is a source controlled drawing or vendor item drawing, CAD files from the vendor will be requested. If the CAD file is unavailable, all interface dimensions shown on the drawing will be included and the basic dimensions and geometry will be modeled.

2.1.2 3D Models shall be valid at all material conditions. The model needs to be able to regenerate without error when set to min, mid and max material conditions.

Dim bound tables can be used to preset the material conditions.

2.1.3 When possible, dimensions on models shall be from datums or surfaces, not edges or tangency points. When this is not possible, datum curve(s) or point (s) should be inserted to avoid parent/child related failures if the edge is broken or rounded. When creating a feature, sketch references should be chosen from the base feature or primary datums. This will help reduce unnecessary parent/child relationships.

2.1.4 When converting from 2-D drawings to 3-D models, features will be created using the existing dimensioning scheme contained in the drawings. If insufficient dimensioning is encountered in the current drawings, dimensions may be taken from another source to complete the model. Any deficiencies will be noted so that the change can be incorporated in the ECP for that drawing. Changing the dimensioning scheme, or deriving dimensions will not be done unless absolutely necessary. If the dimensioning scheme is to change it must be detailed in advance with proper documentation from the engineer/agency responsible for the part.

Problems with tolerance stacking, checking, part interference validation, etc. make changing the dimensioning scheme on the fly undesirable.

2.1.5 Use of unnecessary datums should be kept to a minimum. Use “on the fly” datums when appropriate.

2.1.6 Parts should be able to stand on their own. While designing in assembly mode is often fast and easy to do, it creates parent/child relationships that are tedious to break. Features should be created only on the part to which they apply. An exception is features which are intended to be manufactured at assembly.

2.1.7 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 regenerated. Parts shall not contain buried features. An exception, are Family Table instances that allow for suppressed features.

2.1.8 Rounds, fillets and chamfers should generally be applied at the end of the model creation.

2.1.9 All tolerances and unit systems shall be identified.

2.1.10 Patterning and copying features can reduce the amount of work involved in creating models. Dependence/independence can be established between copied entities. Patterning allows one to create multiple instances of a single feature quickly. Pattern tables allow designs to be quickly changed and used in other models.

2.1.11 Depth options should reflect the dimensioning scheme and should be flexible if the design changes. Users should be careful when using “Through All” or when referencing other surfaces to cut too.

2.1.12 Renaming the three default datum planes (Front, Top, Side) is not allowed.

2.1.13 Fully Annotated Models. Implementing fully annotated model methodologies within the model changes the traditional way information is displayed. The decision to implement these methodologies is left to the affected program office and IPT. Typically a business case would be developed to determine the cost effectiveness to implement fully annotated models into existing legacy models. However, for new models implementation of fully annotated models should become standard.

2.1.13.1 When all work on the model has been completed, the model shall be saved in such a manner that the Title Block view state is displayed when the part is reopened. This would involve changing the combined state to

MBD0_Title_Block and saving the layer status.

2.1.13.2 The Title Block view state shall contain the title block, revision block, design activity block, distribution statements, proprietary statements, and general notes. An isometric view representing the 3D CAD item shall be shown. The isometric view shall contain no datum planes, datum axis, or any visible annotations.

2.1.13.3 Annotations within the model, normally shown “flat to screen”, shall use the “Named Orientation” option within Pro/Engineer - Creo 2, with the named option to reflect that of the appropriate combined state. (i.e. General notes, distribution statements, title block, etc shall be oriented to the

MBD0_Title Block orientation.)

2.1.13.4 The MBE start part and start assembly contain pre-set combined states, which contain the prefix, “MBD”. Any unused combined states are to be removed from the view manager and corresponding layer settings. In addition, the pre-set combined states can be renamed, to more appropriately define the information contained. For example, a combined state labeled

MBD1A_Takedown_Lugs can represent all dimensional and annotated information related to the takedown lugs.

2.2 Assembly Practices

2.2.1 Assembly sequence should follow the intended manufacturing assembly sequence.

2.2.2 Assembly features should not be used for such things as part features. For example, a cut or hole assembly feature should not be used on two or more parts to create mounting holes (unless these holes are intended to be created at assembly).

These features do not show up while in part mode unless shown on an existing drawing in this manner.

2.3 Drawing Practices

2.3.1 Drawings shall display dimensions that are directly parametric to the model upon which they are based. Specifically, these values must be driving or driven dimensions. In no case, should dimensional values be entered as text notes which are not parametric to the base model.

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

3.0 Library.

3.1 Libraries. Libraries contain standard models from which copies may be downloaded and used within ones product folder. To ensure the integrity of the library only the

ARDEC3D Librarian can add, delete or checkout items. Requests to add items to the library can be made through e-mail at: USARMY PICA ARDEC List ARDEC3D

PDMLink HELP DESK. All users have the ability to download items to their workspaces. The ARDEC3D Libraries can be found for the ARDEC3D system at:

https://ardec3d.pica.army.mil/Windchill/app/#ptc1/comp/netmarkets.library.list

3.1.1 ARDEC Parts Library. The ARDEC Parts Library contains commercial and military standard parts such as bolts, washers, detents, etc. Parts within this library have been categorized and defined in such a manner to allow for easy selection.

3.1.2 ARDEC Standard Files Library. The ARDEC Standard Files Library contains the ARDEC drawing formats, config.pro, .dtl files, start parts, start assemblies, symbols, and tables.

3.1.3 Materials Library. The Materials Library contains materials to be assigned to 3-D parts. If a needed material is not in the library, it shall be added to the library before use. Contact the ARDEC3D Librarian to add material to this library.

3.1.4 Shared Drawings Library. The Shared Drawings Library contains drawings to be used on many different systems.

3.1.5 Human Factors Library. The Human Factors Library contains human figures to aid a 3-D assembly as a reference.

https://ardec3d.pica.army.mil/Windchill/app/#ptc1/comp/netmarkets.library.list

4.0 START-UP/SET-UP FILES. The latest version of this document, along with Pro/E and PDM

Link help files can be found at:

https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.inf.library.WTLibrar y%3A99589115&u8=1

4.1 Start part/start assembly. Start part and start assembly files contain a group of features that have been set as a standard starting point for every part and assembly. These features are required standard features to be included with every part and assembly component. The start part and start assembly labeled “ardec_creo2_startpart” and

“ardec_creo2_startasm” respectively, can be found in the ARDEC Standard Files

Library mentioned in paragraph 3.1.2.

4.1.1 Layers. Layers allow part, assembly, and drawing features to be selectively displayed or hidden. The following layers are standard layers to be applied to every start part/assembly (these are the default when using the start part/assembly):

Layer Name Layer Features Status

Banner Contains the current design activity banner symbol.

Off

Cosmetics Cosmetic sketches, threads, etc. Off

Datums Default datum planes and coord. system On

Set Datums Contains set datum features Off

MBD0 Title

Block

Contains the title block annotation, the numbered drawing notes, revision block symbol, and title block symbol.

Off

MBD1_None Only the model is to be displayed. Off

MBD2

(MBD2A …

MBD2 …)

All view state associated layers will begin with MBD2A through MBD2…

The number of these view state layers depends on the complexity of the model.

Those default view states (A through J) not needed within the model are to be removed.

Off

The following layers are standard layers to be applied to the start assembly:

Layer Name Layer Features Default Suppress State

Assy_Datums Default datum planes and coord. system On

Banner Contains the current design activity banner symbol.

Off

Cosmetics Cosmetic sketches, threads, etc. Off

AMBD0 Title

Block

Contains the title block annotation, the numbered drawing notes, revision block symbol, and title block symbol.

On

Set Datums Contains set datum features Off

MBD1_None Only the model is to be displayed. Off https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1 https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1

AMBD2

(AMBD2A

AMBD2 …)

All view state associated layers will begin with AMBD2A through

AMBD2… The number of these view state layers depends on the complexity of the model. Those default view states

(A through J) not needed within the model are to be deleted.

Off

4.1.2 Parameters. Parameters contain administrative information for parts and assemblies that typically would be displayed on a drawing title block, revision block, or assembly table. Each part and assembly shall contain the below set of parameters at a minimum:

Parameter Name Description Recog. By

PDM Link Input

AGENCY Agency (Designated by relation) Yes -

CAGE_CODE Original Design Activity CAGE Code Yes REQ

CHECKER_NAME Person who checked model and dwg. No

CURRENT_CAGE_CODE Current Design Activity CAGE Code Yes REQ

DESIGN_ACTIVITY Design activity. Yes

DESIGN_ACTIVITY_LOCATION Location of design activity Yes

DRAWING_APPROVAL_NAME Person who approved drawing. Yes REQ

DRAWING_APPROVAL_DATE Date drawing was approved. Yes REQ

DRAWING_DATE Date 3D drawing was created. YeS REQ

DRAWING_REV Revision of current drawing. Yes REQ

DRAWN_BY Person who created 2D drawing. No

DESIGN_APPROVAL_NAME Person who approved design. Yes REQ

DESIGN_APPROVAL_DATE Date design was approved. Yes REQ

DESIGN_ACTIVITY Design activity (Designated by rel.) Yes -

DESIGN_ACTIVITY_LOCATION Location (Designated by relation.) Yes -

DISTRIBUTION_CODE Distribution statement code. Yes REQ

ECP_DATE Date ECP was approved to release Yes

ENGINEER_NAME_1 Engineer responsible for design No

ENGINEER_NAME_2 Secondary engineer. No

ERR_DATE Date current revision released. Yes REQ

ERR_ECP_APPROVAL Person who approved ERR. No

ERR_ECP_DATE Date of approved ERR Yes

ERR_ECP_NUMBER ERR number Yes

MATERIAL_ENGINEER Material engineer Yes

MODELER_NAME_1 Primary modeler. Yes REQ

MODEL_REV Revision of current model. Yes REQ

NB1 Used in relation for nomenclature. No

NB2 Used in relation for nomenclature. No

NEXT_ASSY_1 Next higher assemble part number. Yes REQ

NEXT_ASSY_2 “ Yes REQ

NEXT_ASSY_3 “ Yes REQ

NEXT_ASSY_4 “ Yes REQ

NEXT_ASSY_5 “ Yes REQ

NEXT_ASSY_6 “ Yes REQ

NEXT_ASSY_7 “ Yes REQ

NEXT_ASSY_8 “ Yes REQ

NOMENCLATURE Part name Yes REQ

NOMENCLATURE_1 Used in relation for nomenclature. No

NOMENCLATURE_2 “ No

NOMENCLATURE_3 “ No

NOMENCLATURE_LENGTH “ No

ORG_DRAWING_DATE Original drawing date of approval. No

PART_NUMBER Item part number Yes REQ

PROPRIETARY_CODE Proprietary info Yes

QA_ENGINEER_NAME QA Engineer for design No

REMARKS Yes

SOURCE_CONTROL Yes/No para regarding source control Yes

SPEC_CONTROL Spec control info No

STARTPART Revision of startpart used. No

TOLERANCE_1_PLACE General tolerance for .1 No

TOLERANCE_2_PLACE General tolerance for .01 No

TOLERANCE_3_PLACE General tolerance for .001 No

UNIT_WEIGHT Mass computed by 3D software. Yes -

USED_ON_1 End item component is used on. Yes REQ

USED_ON_2 “ Yes REQ

USED_ON_3 “ Yes REQ

USED_ON_4 “ Yes REQ

USED_ON_5 “ Yes REQ

USED_ON_6 “ Yes REQ

USED_ON_7 “ Yes REQ

USED_ON_8 “ Yes REQ

MBE_MATURITY Value from 0-6 No

4.1.3 Relations. Relations allow algebraic formulas to be computed utilizing dimensions or parameters for the purposes of implementing design intent and developing parameter information. The following relations are to be established for each part and assembly. See Appendix B for detailed set up of relations.

- Set parameter “DRAWING_NUMBER” equal to “PART_NUMBER”.

- Cut “NOMENCLATURE” parameter into a maximum of three parts, so it will fit appropriately into the title block of a drawing.

- Assign the “DESIGN_ACTIVITY” and “DESIGN_ACTIVITY_LOCATION” parameters based upon the “CAGE_CODE” parameter.

- Calculate the “UNIT_WEIGHT” parameter.

4.1.4 Default datum planes - Parts. All parts shall start with three default datum planes and a default coordinate system. The default datum planes shall be named

“FRONT”, “TOP” and “SIDE”. All parts shall have a datum coordinate system set with x, y and z correctly pointing to the parts final orientation (i.e. “FRONT” in the y-z plane, “SIDE” in the x-z plane, and “TOP” in the x-y plane). During part creation these three default datum planes shall not be renamed.

4.1.5 Default datum planes – Assemblies. All assemblies shall start with three default datum planes and a default coordinate system. The default datum planes shall be named “FRONT_ASSY”, “TOP_ASSY” and “SIDE_ASSY”. All assemblies shall have datum coordinate system set with x, y and z correctly pointing to the assemblies final orientation (i.e. “ASSY_FRONT” in the y-z plane, “ASSY_SIDE” in the x-z plane, and “ASSY_TOP” in the x-y plane). During assembly creation these three default datum planes shall not be renamed.

4.1.6 3-D general notes. All parts and assemblies shall contain, at a minimum, the following three notes:

- NUMBERED_DRAWING_NOTES: This note represents the general notes found on a 2-D drawing.

- Distribution_Note: This note allows placement of the distribution statement pertaining to the accompanying part or assembly.

- Proprietary_Note: This note allows placement of the proprietary statement pertaining to the accompanying part or assembly.

4.1.7 Model views. All parts and assemblies shall have separately named views defining the “MBD1A”, “MBD1B”, “MBD1C”,… “MBD1J. These views shall be created such that the named views correspond to the appropriate orientation of the named three default datum planes.

4.1.8 View States. All parts and assemblies shall have assigned view states. The view states shall define a model orientation, layer setting, and whether or not a cross section is to be displayed. The view states shall correlate to the layer naming convention sited in paragraph 4.1.1.

4.2 Drawings.

4.2.1 Drawing formats. Drawings formats have been established for all drawing sizes. Formats shall link the appropriate part and assembly parameters to the drawing title and revision blocks. 3-D notes “NUMBERED_DRAWING_NOTES” and

“Distribution_Note” shall be linked to the drawing to be displayed in the appropriate location. The distribution statement shall appear on each sheet of a multi-sheet drawing. The revision block contains the parameters “DRAWING_REV”, and

“ERR_DATE” on the last line of the table. Previous revision data should be entered into the table manually. ARDEC drawing formats can be found within ARDEC3D

PDM Link library at https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.Sub Folder%3A99592075&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1

4.2.2 Drawing detail files. Drawing detail files are to be established for each corresponding drawing format, for both metric and English units. Drawing detail files contain preassigned values for text height, projection view type, arrow head length, dimension leader length, tolerance display, etc. See Appendix D for a complete list of drawing detail settings for each drawing size. ARDEC drawing detail files can be found within ARDEC3D PDM Link library at

Folder%3A101774435&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1

4.3 Configuration files.

https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.SubFolder%3A99592075&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1 https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.SubFolder%3A99592075&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1 https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.SubFolder%3A101774435&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1 https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.SubFolder%3A101774435&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1

4.3.1 Config.pro files. Configuration files are standard set up files for each part and assembly. Configuration files contain preassigned values for plotter pen weights, model display, tolerance display, identify location of material, symbols, library, format files, etc. See Appendix D for standard ARDEC config.pro settings. ARDEC config files can be found within ARDEC3D PDM Link library at

Folder%3A99589728&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1

4.3.2 Mapkeys. Mapkeys are special keyboard inputs that will launch a pre-programmed sequence of commands.

https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.SubFolder%3A99589728&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1 https://ardec3d.pica.army.mil/Windchill/app/#ptc1/tcomp/infoPage?oid=OR%3Awt.folder.SubFolder%3A99589728&ContainerOid=OR%3Awt.inf.library.WTLibrary%3A99589115&u8=1

5 PART MODELING REQUIREMENTS. When creating parts, design intent must be considered throughout the modeling process. The notion of design intent arises from the fact that there are always alternate ways of creating model features. Features should be simple and created such that they are easily modifiable by another. It is better to have several simple features than one complex feature. In addition, there are numerous dimensioning schemes to describe the geometry. When creating part features the modeler must choose from alternatives based on how the feature is to relate to the rest of the part, and how it will respond to changes elsewhere in the model. See Appendix A for recommended part modeling steps.

Parts must be functional and created in a logical sequence. Features should be simple and be created such that they are easily modifiable by another user at any time. Parts must have every feature that the real part is required to have. For example, plastic parts must 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 shall also be modeled. Exceptions include 1. threaded parts may be represented with cosmetic threads; 2, break edges are not typically to be modeled into the part.

Models created from 2-D drawings shall contain as much of the information from the drawing as possible. This includes, conventional tolerances, geometric tolerances, notes, materials, surface finishes, weld symbols, Quality Assurance Provision symbols, title block information, and revision information. If deficiencies or errors are encountered during the conversion they are to be so noted that the change can be incorporated in an Engineering

Change Proposal for that drawing.

5.1 File name convention. Parts, where the contractual baseline is the 2D drawing, shall be named using the parts CAGE code and part number as follows:

CAGE code_part number (i.e. 19200_12345678)

If the parts part number contains a dash it will be included in the file name

(i.e. 19200_12345678-001).

Parts, where the contractual baseline is the model, the file name convention shall be named with MBD, the parts CAGE code and part number as follows:

MBD_CAGE code_part number (i.e. MBD_19200_12345678)

5.2 Start part. Parts shall use the appropriate ARDEC start part defined in 4.1.

5.3 Parameters. The parameters identified in 4.1.2, requiring input, are to be completed in accordance with the pertaining part.

5.4 3-D general notes. General notes “NUMBERED_DRAWING_NOTES” and

“Distribution_Note”, established in 4.1.6, are to be completed in accordance with the pertaining part. Both notes are to be placed on the MBD0_Title Block layer.

5.5 Material. Material is to be defined in two locations for each part. The first location is identifying the material from the software’s material library. When a unique material is used, all material properties must be provided. The second location is the description of the material in the 3-D general note

“NUMBERED_DRAWING_NOTES”.

5.6 Units. Units shall be set to those stipulated by the part configuration. For English units the “Inch lbm Second” units are to be used.

5.7 Conventional tolerances. Conventional tolerances shall be adjusted accordingly for each dimension. Although conventional tolerances can be modified in either the drawing or part, as a result of the parametric relationship between models and drawings, it is recommended to adjust these tolerances during part creation. For newly created models, it is recommended to use mid tolerances (+/- symmetric).

5.7.1 2-D to 3-D conversion. If part creation occurs when converting a 2-D drawing to a 3-D model, then conventional tolerances should reflect those of the

2-D drawing.

5.7.2 Additional dimensions. Additional dimensions, used only for part creation, are to be identified as such. These additional dimensions shall have the conventional tolerance converted to a nominal style with the following text attached to the dimension: “DIMENSION FOR MODELEING PURPOSES

ONLY”.

5.7.3 Dimensions associated by relations. Dimensions governed by relation are to be identified as such. These dimensions shall have the conventional tolerance converted to a nominal style with the following text attached to the dimension:

“DIMENSION GOVERNED BY RELATION”.

5.8 Set datums. Set datums define datum features, such as axes or planes, considered as primary features of the part. Set datums are typically called out in geometric tolerance feature control frames. The set datum can be a standalone feature or assigned to a dimension.

5.9 Geometric tolerances. Geometric tolerances shall be created in accordance with

ASME-Y14.5. If part creation occurs when converting a 2-D drawing to a 3-D model, then geometric tolerances shall reflect those of the 2-D drawing. Geometric tolerances should be created after Set Datums in order for the datum labels to appear in the feature control frame.

5.10 Annotations. The following annotations shall be created for each part as required:

5.10.1 Surface finish. Surface finishes shall be shown on the part as required.

5.10.2 Custom symbols. When appropriate custom symbols (i.e. Quality

Assurance Provision (QAP) symbols) should be shown on the part as required.

QAP symbols for small caliber weapons are to be in accordance with ARDEC drawing 12993884. If QAP symbols are placed on the part, the following general note is to be placed in the NUMBERED_DRAWING_NOTES: “QUALITY

ASSURANCE PROVISIONS PER DRAWING 12993884 SHALL APPLY.”

5.10.3 Notes. Additional notes, pertaining to the part, shall be shown on the part as required. If notes are intended to apply to specific features they shall be attached to those features.

5.11 Relations. Relations shall be created as necessary to strengthen parametric relationships and design intent. Each relation shall have a comment preceding the relation to describe its purpose.

5.12 Family tables. Family tables are collections of parts or features that are essentially similar, but deviate slightly in one or two aspects, such as size or detail.

They are used when creating alternate design options for a part, or when creating a part with two or more varying dimensional values. Family table instances must be uniquely named to reflect the alternate design or the dash number of the varying dimensional feature. Instance names shall also begin with the CAGE code_part number of the generic part.

Example: 19200_12345678_ALTN

19200_12345678-1

5.13 Flexibility. Deformed parts (i.e. springs, rivets, etc.) are created as flexible parts. Flexible parts allow 1) key dimensions to be replaced based upon the size and location of the next assembly, and 2) allow key features to be suppressed and resumed to alter the appearance of the part. See Appendix F and G for detailed procedures for implementing flexibility into the creation of springs and other flexible parts.

5.14 Calculate Mass Property. Mass properties are to be calculated at the end of the model creation activity using correct material, density, etc. Any changes to the physical model will result in the mass properties to be recalculated.

5.15 Layers. Additional layers, than those identified in the start part, 4.1.1, can be created as needed. The following default layers have been established to capture most features.

5.15.1 Cosmetic. The cosmetic layer allows placement of cosmetic features (i.e.

cosmetic threads, sketches, etc.).

5.15.2 Datums. The datums layer allows placement of datum features (i.e. datum planes, axes, points, and coordinate system). Additional datum features created in the part will automatically be placed on the datums layer, as a result of the config.pro settings.

5.15.3 Notes. The notes layer allows placement of notes identified in 4.1.6 and

5.4.

5.15.4 MBD. The MBD layers capture annotations to support fully annotated models. Annotated dimensions, geometric tolerances, datums, symbols, and 3D notes are to be assigned to MBD5x layers representing the appropriate view to be displayed. Insure the selection filter is set to “Annotation” prior to placing annotated dimensions on layers.

5.16 Forgings and castings.

5.16.1 Single part number. Parts made from forgings or castings, in which the as forged/cast part and the machined part are depicted using a single part number, shall have the forging/casting completely modeled as the generic instance of a family table. The machined portion of the part shall be placed on a separate family table instance labeled CAGE CODE_PART NO_MACHINED. (Example:

19200_12345678_MACHINED)

5.16.2 Dual part number. Parts made from forgings or castings, in which the as forged/cast part and the machined part are depicted as separate part numbers, shall be created as separate parts.

5.17 Sheet metal. Sheet metal parts should be created in Pro/Sheetmetal, or equivalent, or be capable of being imported into Pro/Sheetmetal. It is recommended that sheet metal parts be started as a solid part using the start part, 4.1, and standard naming convention, then converted to a sheet metal part by starting the

SHEETMETAL application. However, if one chooses to create a new part as a sheet metal part, the ARDEC sheet metal start part is to be used.

5.18 Standard parts. Military specification and other specification controlled parts consist of such items as screws, bolts, pins, rivets, etc. and generally consist of a table of shapes and sizes. These parts are controlled by MS, NASM, ANSI, ASTM, or other similar governing body. The 3-D solid models of these parts are not intended to define the part, but are for visualization, weight and center of gravity, manufacturing and bill of material purposes only. Standard parts have a wide application across many systems and therefore must be centrally stored and controlled to prevent duplication and errors due to multiple occurrences of the same part existing in the database. These parts shall be named using the following convention:

For MS and NASM specifications:

CAGE Code_Part Number (i.e. 96906_MS16633)

For ANSI and ASTM specifications:

CAGE Code_Part Number (80204_ANSI_B18_7)

For ASME specifications:

CAGE Code_Part Number (05047_ASME_A330)

When the need for a standard part occurs, the organization creating the models shall first determine if the standard parts exist in the ARDEC Parts Library, per paragraph

3.1.1, of the ARDEC3D PDM Link database. If the parts exist, those parts shall be used.

If a standard part is needed which does not exist in the library, that part shall be created using standard modeling procedures defined in this document, except that parts do not have to be completely defined, but defined to the extent necessary to visually represent the item, and to give accurate weight and center of gravity characteristics. When modeling a standard part, if the governing specification contains a table of various shapes and sizes, all instances of the table must be created

(even if only one instance is needed for the project at hand). The ARDEC3D

Librarian must check the model prior to implementing the part file into the

ARDEC3D Library.

6 ASSEMBLY REQUIREMENTS. When creating assemblies components should be added to the assembly in a logical assembly order. Assemblies shall include all components that clearly define the entire assembly including: sub-assemblies, pins, screws, nuts, washers, springs, decals, warning labels, etc. See Appendix A for recommended assembly modeling steps.

6.1 File name convention. Assemblies, where the contractual baseline is the 2D drawing, shall be named using the assembly’s CAGE code and part number as follows:

CAGE code_part number (i.e. 19200_12345678)

If the assembly’s part number contains a dash it will be included in the file name

(i.e. 19200_12345678-001).

Assemblies, where the contractual baseline is the model, the file name convention shall be named with MBD, the parts CAGE code and part number as follows:

MBD_CAGE code_part number (i.e. MBD_19200_12345678)

6.2 Start assembly. Assemblies shall use the appropriate ARDEC start assembly defined in 4.1.

6.3 Parameters. The parameters identified in 4.1.2, requiring input, are to be completed in accordance with the pertaining assembly.

6.4 3-D general notes. General notes “NUMBERED_DRAWING_NOTES” and

“Distribution_Note”, established in 4.1.6, are to be completed in accordance with the pertaining assembly.

6.5 Assembly constraints. Each component of an assembly shall contain enough constraints to fully constrain the component. Components shall not be left unconstrained. Upon completion, the assembly shall be checked for interferences.

Although there is occasion to warrant an interference fit, an interference check will highlight potential errors in the assembly construction.

6.6 Flexible parts. Parts identified as flexible shall utilize the flexible feature when the component is added to the assembly. The flexible functionality shall capture the design intent of the assembly.

6.7 Annotations. The following annotations shall be created for each assembly as required:

6.7.1 Surface finish. Surface finishes shall be shown on the assembly as required.

6.7.2 Custom symbols. Custom symbols (i.e. Quality Assurance Provision

(QAP) symbols) shall be shown on the assembly as required. If QAP symbols are placed on the assembly, the following general note is to be placed in the

NUMBERED_DRAWING_NOTES: “QUALITY ASSURANCE PROVISIONS

PER DRAWING 12993884 SHALL APPLY.”

6.7.3 Weld symbols. Weld symbols shall be shown on the assembly as required, and attached to the specific features accordingly.

6.7.4 Notes. Additional notes, pertaining to the assembly, shall be shown on the assembly as required. If notes are intended to apply to specific features they shall be attached to those features.

6.8 Calculate Mass Properties. Mass properties are to be calculated at the end of the model creation activity. Any changes to the physical model will result in the mass properties to be recalculated.

6.9 Layers. Additional layers, than those identified in the start assembly, 4.1.1, can be created as needed. The following default layers have been established to capture most features.

6.9.1 Assy datums. The assy_datums layer allows placement of datum features

(i.e. datum planes, axes, points, and coordinate system).

6.9.2 Assy notes. The assy_notes layer allows placement of notes identified in

4.1.6.

6.9.3 MBD. The MBD layers capture annotations to support fully annotated models. Annotated dimensions, geometric tolerances, datums, symbols, and 3D notes are to be assigned to MBD5x layers representing the appropriate view to be displayed.

6.10 Color shading of components. All components shall be assigned a unique color for ease of viewing the assembly. Similar components can be grouped together with a single color (i.e. all springs are colored green). When possible, grouped colors should be maintained throughout the entire project (i.e. all springs, in all assemblies of the project are colored green).

6.11 Bulk Items.

6.11.1 Bulk items not identified with a unique drawing number (i.e., adhesives, lubricants, paints, etc) shall be created as bulk items in assembly mode as necessary in order that they appear in bills of material.

6.11.2 Bulk items such as adhesives, lubricants, paints, etc identified with unique drawing numbers and which have drawings defined, shall be created in the part mode. The items will be created as “empty” models containing only default datum planes and coordinate systems with necessary notes and parameters input into the model. The model will then be assembled to its assemblies using the default datum planes. This will allow the bill of materials for the higher assemblies to correctly identify the bulk item.

7. FULLY ANNOTATED MODELS. Fully annotated models are in support of 3D pdf’s.

ARDEC is planning to update its technical data system from one based on 2-dimensional line drawings to a technical data system based on electric 3-dimensional solid models.

Solid model based technical data has many uses including automated generation and update of line drawings, automated bills of material, rapid prototypes, engineering analysis, technical manual development, maintenance training, tooling design, etc.

ARDEC utilizes the Anark software for creation of the 3D pdf’s. This software resides on the ARDEC3D Windchill PDM Link system and is capable of generating and storing the

3D pdf’s within Windchill. The standards listed in this document, along with ASME

Y14.41, define how ARDEC will fully annotated 3D models in order to develop TDP quality 3D pdf’s. An Engineering Change Proposal (ECP) is required to adopt the 3D pdf as the official government item of record. Upon approval of the ECP, the traditional 2D drawing will no longer be maintained.

7.1 View States. View states contain all the annotations necessary to completely define the model. This includes dimensions, reference dimensions, geometric tolerances, datums, surface finishes, notes and symbols. The ARDEC start part / start assembly dated 30 Jan 2015 to the present contains the correct view state naming conventions and parameters. The proper default naming convention is as follows:

MBD0_Title_Block

MBD1_None

MBD2A

MBD2B

MBD2C

MBD2D

MBD2E

MBD2F

MBD2G

MBD2H

MBD2I

MBD2J

The MBD0_Title_Block view state contains the general notes, general symbols, distribution statement and proprietary statement.

The MBD1_None view state contains no annotations or datums, but provides only a

3D representation of the model.

The MBD2A … contain all annotations specific to that view state.

The above listed default view states MBD2A – MBD2J are intended for the modelers ease to reduce the time necessary to create the view states. The modeler may increase the number of view states as needed, using a consistent naming convention. Any unused view states are to be removed.

7.1.1 View States within View Manager. Within the View Manager of

Pro/Engineer the All tab contains the listed default view states. The view states listed here contain the associated orientation, layer status, cross section and applied simplified rep for each view state.

7.1.2 Layer States within the View Manager. Within the View Manager of

Pro/Engineer the Layer tab contains the listed default layer states. The naming convention reflects the same convention as outlined in paragraph 7.1. The layer states contain the layer settings as to what has been hidden/unhidden when the layer state was saved.

7.1.3 Layers. Layers will contain the datum axis and planes necessary for annotating the view state. The naming convention reflects the same convention as outlined in paragraph 7.1.

7.2 Naming Conventions. The naming convention outlined in paragraph 7.1 represent the default names associated with each view state. It is intended that a more descriptive name will be provided to each view state for those view states beginning with MBD2A – MBD2J. View state names are to be feature based and reflect the feature to which the annotation applies. Examples included: MBD2A_General, MBD2B_Takedown_Lug, MBD2C_Firing_Pin_Hole, MBD2D_Holes, MBD2E_Outside_Contour.

7.3 Annotation Features. All annotations associated with a view state are provided within the Annotation Feature dialog box. All annotations for a given view state are to be placed within a single annotation dialog box. The annotation feature shown within the model tree is to be renamed consist with the view state for which it is associated.

7.3.1 Dimensions. All annotated dimensions are to be created as driven dimensions within the Annotation Feature dialog box. All surfaces or entities are to be identified that reflect that to which the dimension describes. All created driven dimensions are to be linked to the models driving dimension. Also, dimensions are to be placed logically to best represent the feature to which it represents.

7.3.2 Reference Dimensions. All annotated reference dimensions are to be created as driven reference dimensions within the Annotation Feature dialog box. All surfaces or entities are to be identified that reflect that to which the dimension describes.

7.3.3 Geometric Tolerances. All geometric tolerances are to be created within the

Annotation Feature dialog box.

7.3.4 Set Datums. All set datums are to be created within the Annotation Feature dialog box.

7.3.5 Surface Finish. All surface finish symbols are to be created within the

Annotation Feature dialog box.

7.3.6 Notes. All notes are to be created within the Annotation Feature dialog box.

7.3.7 Symbols. All symbols are to be created within the Annotation Feature dialog box.

7.4 Datum Axis. At times datum axis are required to identify the center of a diameter or radius. View states will require an axis to be displayed when dimensions are referencing the center of a diameter or radius. Datum tags are not to be displayed with the axis and are to be placed separately on the Datums layer.

7.5 Datum Planes. At times additional datum planes are necessary for placement of dimensions. Dimension are to be placed logically to best represent the interpretation of the feature.

7.6 Isometric Views. In many cases annotations are not contained within the same viewing direction and orientation. It may become necessary to place annotations in two or more viewing directions (x, y, z) to better describe the feature to which the annotation is associated. When this is the case, the modeler shall create an isometric view and set this view as the orientation for the given view state.

7.7 Fully Annotating Legacy Models. Legacy 3D models, depending on when they were created, will not contain the default view states listed in paragraph 7.1, nor will they contain the necessary parameters needed for developing a 3D pdf. Therefore, these models will need to be updated prior to creation of any annotations.

7.7.1 General Notes. At one time the ARDEC start part / start assembly required each individual general note be placed on its own separate note. Today, all general notes are placed in the single note, NUMBERED_DRAWING_NOTES.

If the legacy model does not contain the NUMBERED_DRAWING_NOTES note then it must be created and the individual notes are to be cut and pasted on the new single note.

7.7.2 Parameters. The following parameters must be added to the model:

Units

Drawing_Note

Dist_Note

Prop_Note

These parameters are to be created as a parameter string. The parameter value for the Units parameter will be English or Metric. The parameter value for

Drawing_Note, Dist_Note and Prop Note will be the numerical note ID of each.

This value can be found within the properties of each note. For example:

. These numerical ID numbers may vary from model to model.

7.7.3 Map Keys. The current config.pro file stored within the Standard Files of the ARDEC3D Windchill PDM Link system contains map keys that will facilitate to creation of the layers, layer states and view states. Simply type “mbd” to initiate the map key.

8. DRAWING REQUIREMENTS. 2-D generated drawings reflect the information contained in the 3-D model. Creating 2-D drawings requires drawing information (i.e.

general notes, parameters, dimensions and tolerances, geometric tolerances, annotations, etc.) to be “pulled” from the 3-D model and placed logically on a drawing, such that information on the drawing and model remain parametric. See Appendix A for recommended drawing steps.

8.1 Drawing formats. Only ARDEC established drawing formats are to be used for

ARDEC managed drawings. Information found in the title and revision blocks shall be populated from the part/assembly parameters in 4.1.2.

8.2 3-D general notes. Notes “NUMBERED_DRAWING_NOTES” and

“Distribution_Note” shall be placed on the drawing appropriately.

8.3 Drawing detail files. The appropriate drawing detail file, in 4.2.2, pertaining to the drawings format size, shall be imported into the drawing.

8.4 Drawing views. Drawing views shall be created to accurate reflect the configuration of the part/assembly. When recreating a drawing from a pre-existing 2-

D drawing (i.e. 2-D to 3-D conversion effort) the newly created views should be the same type of views as the original, and located in approximately the same location.

8.4.1 Isometric views. When possible, drawings should contain an isometric view of the part/assembly. For assembly drawings, the isometric view can be shown as color shaded view to enhance the visual understanding of the assembly.

8.4.2 Display settings. Each view shall be assigned a permanent line display style (hidden lines, no hidden lines, wireframe) and a tangent line display style

(none, solid, dimmed, centerline, phantom).

8.5 Axes. Axes shall be displayed in all views where appropriate.

8.6 Dimensions, tolerances and geometric tolerances. All dimensions, tolerances and geometric tolerances to completely define the part/assembly shall be displayed in the drawing views. The use of created driven dimensions should be kept to a minimum, whereby the use of parametric driving dimensions shall be used to the maximum extent possible. When recreating a drawing from a pre-existing 2-D drawing (i.e. 2-D to 3-D conversion effort) the dimensions, tolerances and geometric tolerances should be located in approximately the same location.

8.7 Drawing view notes. Notes associated to a view shall be attached to the view, such…