Modeling Standards - VTAstrobotics/Documentation GitHub Wiki

Modeling Standards

Contents

Prerequisites

To understand the content on this page, you should know how to

  • Have a basic understanding of Solidworks and 3D modeling.

Purpose

  • The purpose of this document is to provide the team with a standard for the creation and maintenance of CAD models in SolidWorks.
  • This document applies specifically to SOLIDWORKS files that will be created for use by the team.

Definitions

1.1 The following terms should be understood by any document author or revisor prior to creating/releasing parts.

  1.1.1. Can – Indicates a possibility.

  1.1.2. May – Indicates a permission.

  1.1.3. Should – Indicates a recommendation.

  1.1.4. Shall – Indicates a requirement.

  1.1.5. CAD– Computer Aided Design

  1.1.6. Design Intent – A CAD modeling philosophy that incorporates the designer’s expectations of how the model will be used and how it will change when modified.

  1.1.7. FeatureManager – The FeatureManager design tree on the left side of the SOLIDWORKS window provides an outline view of the active part, assembly or drawing.

General Requirements

2.1. SOLIDWORKS documents shall be opened from and saved into Sharepoint.

2.2 New SOLIDWORKS documents shall be created using the appropriate template files synced from the master template file location.

2.3 New SOLIDWORKS document file names shall be in the team part number format ##-##-##_DESCRIPTION

Sketches

3.1. User-created or modified sketches in SOLIDWORKS shall be fully defined.

3.2. Fillets, chamfers, and sketch patterns shall not be used in sketches. Part and assembly features allow for greater feature control, increased modeling efficiency, and improved file stability.

3.3. Sketches shall concisely convey the design intent of the part using both Sketch Relations and Sketch Dimensions.

Parts

4.1 The main part features should be centered on the part origin when possible. Midpoint relations, lines of symmetry, and the Mid Plane extrude direction should be used to center Base features. Base feature Revolve centerlines shall be coincident with the part origin.

4.2 Parts should be oriented to match the orientation of the component where it will most commonly be used (ex. The front plane of a part should be parallel with the front plane of the assembly where it will be used).

4.3 Parts shall have a material specified that match the intended design material.

4.4 Parts that will be cut out of flat stock or plate material including, but not limited to, sheet metal, plastic, rubber, and plywood, shall be modeled using SOLIDWORKS Sheet Metal features and have a DXF file of the SOLIDWORKS.

4.5 The Hole Wizard or Feature Patterns should be used to create multiple identical features (such as mounting holes). This implies design intent as well as reduces the feature tree and adds enhanced control of features.

4.6 Features, Planes, Origins, and Mates should be renamed as necessary to provide more clarity or convey design intent.

4.7 Folders should be used in the FeatureManager to organize groups of components or features.

Assemblies

5.1 Assembly origin position shall be carefully chosen to best represent design intent and make positioning in higher-level assemblies more efficient.

5.2 Assembly Models shall be in the Collapsed (un-exploded) state when saved in.

5.3 Component Patterns should be used to reduce the number of mates and parts in the feature tree.

Configurations/ Display-States

6.1 Configurations shall not be used to hide or show components for specific views in a drawing.

6.2 Display states shall be used to hide and show specific components in assembly drawings.

6.3 Part numbered configurations within the same SOLIDWORKS document shall be significantly similar and should be limited to one parameter or part variation among configurations.

6.4 Display States should be named for clarity

6.5 Components and features that are suppressed in all configurations of an assembly shall be removed from the assembly.

Mates

7.1 Standard Mates shall be used to constrain models whenever possible.

7.2 Mechanical Mates should be avoided unless no other mating technique can adequately constrain components.

7.3 Components should have their position fully defined by no more than 3 mates.

Supplier Models

8.1 Externally supplied models shall be evaluated for appropriate detail and accuracy.

8.2 SOLIDWORKS component mass shall be verified with supplier specifications or by weighing the physical component.

Drawings

9.1 Drawing title blocks and tables shall be linked to the model properties.