¶ 2910 CAD Standards
This page lays out the standards and guidelines used by the 2910 design team when developing CAD models for robots and other team related projects to ensure they are consistent and designed around our manufacturing capabilities. This includes overall CAD project and file organization, standard hardware and materials, part numbering conventions, COTS part usage, assembly conventions, and export standards for sponsor or 3D Printing.
These are meant to be general practices applicable to most CAD projects and are followed whenever practicable. Deviations should be discussed with a mentor or coach to determine both what the correct path forward should be as an exception, and if this document should be modified or expanded as a result.
It is a general expectation that all students and mentors working on CAD will refer to this guide as applicable.
¶ Document Structure
¶ Project Folders
Each new CAD project should have its own project folder located in either the Off-Season or Build Season folder, depending on what the project is for. All competitions season robot projects should be created in the Build Season folder.
¶ Project Documents
- Primary Geometry and Prototypes - Contains a part studio with just primary geometry sketches, and optionally a folder that can be used to ideate robot concepts and potentially create high-fidelity prototype models. This document should only contain an assembly if it is associated to a prototype.
- Subsystem Documents - Each subsystem gets its own document, which will contain at least one main part studio and one main assembly. Additional part studios and assemblies can be created as necessary. Each subsystem should have a mate connector, created in the main part studio and aligned to the origin, which is used to mate it in place in the main robot assembly.
- Main Robot Assembly - Contains only one assembly document with the main robot assembly. Each subsystem main assembly is inserted and fastened to the origin by the subassembly origin mate connector
- Other Documents - Separate documents may be created as necessary for things like 2D field layout or other reference files. If prototypes are not created in the Primary Geometry document, a separate Prototype document should be created.
For consistent navigation, each document should have any assembly tabs as the left-most tabs, followed by part studios, and then folders for imported parts and drawings as required.
¶ Versions and Branches
Versions should be created in the Primary Geometry document whenever a significant change is made and is ready to propagate to subsystems. It's not uncommon to have 100 or more versions of Primary Geometry.
Versions should be created in Subsystem documents whenever they are at a stage where the changes should be propagated to the Main Robot Assembly. This does not necessarily mean the subsystem is “done” - versions should be created early and often to check interfaces or interferences with other subsystems.
Versions should be created in the Main Robot Assembly only at specific times when it has reached a stable state. Examples would include the first time all subsystems are inserted, when a subsystem (or the whole robot) has received Ready-to-Cut approval, a major redesign is being undertaken, or the model is ready for public release.
Branches should rarely be used, and the use should be coordinated with design mentors. Branches are most frequently used for design explorations of alternative concepts. Branches can create significant challenges to ensuring the correct linkages are maintained between documents.
¶ Setting Up Primary Geometry
The Primary Geometry part studio must be set up correctly to work:
- Every mechanism must be represented
- Origin for all primary geometry is ground plane, center of chassis L/R and F/B
- Side view sketches at minimum
- Others (side, top) as necessary to define integration
- Should contain critical geometry such as:
- Interfaces (holes, hole patterns, etc) between subsystems
- Motors
- Gears/bearing/shaft locations
- Wheels
- Game pieces
- Major structural elements
- Field interfaces/Starting Box
- Envelope/motion path/stay-out zones
- Rough CG or CG constraints as needed
- Use multiple sketches
- Each subsystem should have at least one driving layout sketch
- Sketches should be split up and ordered logically to avoid over-complicating any one sketch
¶ Using Primary Geometry
The Primary Geometry sketches should be derived into each subsystem main part studio (and any other part studios that are making parts defined directly or indirectly by primary geometry) and named “Primary Geometry Derived" or similar. When creating the derived part, only select the sketches that are relevant to that subsystem. A derived part can only be hidden or shown as a complete set, sketches within it cannot be hidden or shown separately.
Multiple derived parts can be created from different sets of primary geometry sketches to make working with them easier. It is not recommended to derive each primary geometry sketch as a separate derived part, as this will significantly slow down the update process when a new version of primary geometry is generated. 2-3 logical groupings is recommended.
¶ Part Numbering and Naming Scheme
All documents and custom parts within a part studio will be named with a numbering scheme which allows quick navigation of the document structure to find the relevant parts in CAD and identify them physically for assembly.
The 2910 Part Numbering Scheme is XX-YY-ZZ
- XX - Subsystem Designation
- YY - Part Studio Number
- ZZ - Part Identifier
Subsystem Designations consist of two digits. The first digit is the subsystem, the 2nd digit is the major revision level. Generally a subsystem will only have one revision, but if there is a significant change (e.g. full redesign of a subsystem with new primary geometry sketches) or we want a 2nd design while keeping the original design unchanged, we will assign the next number (e.g. 32-YY-ZZ)
Designations are assigned as follows:
- 01 - [Year] Primary Geometry
- 11 - [Year] Top Level Assembly
- 21 - [Year] Drivetrain
- 31 and up are assigned as needed for the distinct subsystems
Part Studios are numbered sequentially. Often a subsystem may only have one part studio.
Parts are numbered sequentially within a part studio as they are created. Some parts may later become obsolete and deleted, resulting in skip part numbers. Do not re-number subsequent parts if a numbered part was deleted, such as a duplicate part. Parts should be descriptively named in the BOM Description field.
All parts that are exact representations of COTS parts, such as spacers, belts, etc. should be named with their vendor or industry standard part number.
Examples:
- A 1" long #10 aluminum spacer from McMaster would be named “92510A569”
- A 90 tooth 15mm wide 5mm HTD belt could be named “450-5M-15”. “90t 5mm Belt” is also acceptable as the name the ContextlessBelt Featurescript automatically generates.
This scheme allows immediate identification of which assembly a part belongs to and whether the part is custom or COTS.
Examples of numbered documents, parts and part studios
¶ Standard Hardware
These are the preferred fasteners for 2910, but not an exhaustive list. Effort should be made to design using standard hardware, unless design constraints require a different solution.
¶ Bolts
#10-32 Socket Head and Button Head Cap Screws in the following lengths:
- 1/4" through 1" in 1/8" increments
| 0.250 | 0.375 | 0.500 | 0.625 | 0.750 | 0.875 | 1.000 |
- 1-1/4" through 3" in 1/4" increments
| 1.250 | 1.500 | 1.750 | 2.000 | 2.250 | 2.500 | 2.750 | 3.000 |
1/4-20 Socket Head and Button Head Cap Screws in the following lengths:
- 1/4" through 1" in 1/8" increments
| 0.250 | 0.375 | 0.500 | 0.625 | 0.750 | 0.875 | 1.000 |
- 1-1/4" through 3" in 1/4" increments
| 1.250 | 1.500 | 1.750 | 2.000 | 2.250 | 2.500 | 2.750 | 3.000 |
Bolts should be inserted into assemblies via the “Standard Content” option of the Insert function.
¶ Nuts
#10 and 1/4-20 Nylock nuts in Standard and Low-Profile heights
Standard height Nylock nuts can be inserted from MKCAD. Low-Profile Nuts will need to have the model imported from McMaster
¶ Rivets
2910 uses 3/16" Rivets. Rivet models can be inserted from MKCAD
¶ Hole Sizes
Following hole diameters should be used for hardware. Where possible, the hole feature should be used to select the appropriate clearance or tap size. Always use ANSI Close Fit clearance sizes.
| #4-40 | #6-32 | #8-32 | #10-32 or 3/16" Rivets | 1/4-20 | |
| Clearance/Thru | 0.116 | 0.144 | 0.170 | 0.196 | 0.257 |
| Tapped | 0.094 | 0.107 | 0.136 | 0.159 | 0.201 |
¶ Structural Parts
¶ Box Tube
Standard Box Tube Sizes:
Aluminum 6061 1" x 1" - 0.063" and 0.125" Wall Thickness
Aluminum 6061 2" x 1" - 0.063" and 0.125" Wall Thickness
Box Tube Hole Pattern:
WCP Punched Tube Style - 0.196 holes on 0.5" pitch. Single row on 1" faces, 3 rows on 2" faces. Custom patterns (made from raw stock) can omit holes as necessary.
¶ Sheet and Plate
Aluminum 6061 - 0.063", 0.125" and 0.250" thick. No partial-depth features.
Aluminum 7075 - up to 0.750" thick, maximum horizontal dimensions 10" x 16". Partial-depth features allowed.
¶ Billet
Aluminum 6061 or 7075 thicker than 0.75". Billet parts designs are typically made by SDS and need to be coordinated with Patrick to ensure they are manufacturable.
¶ Bent Sheetmetal
Aluminum 5052 - 0.063", 0.090", 0.125", 0.187"
Bent sheetmetal parts are made by Fabworks. Consult the Fabworks website for bending guidelines: https://www.fabworks.com/resources/guidelines/bending
¶ 3D Printed
3D Printed parts are typically made from Markforged Onyx material. There are no general design guidelines for 3D printed parts. Use the “3D Printed" Featurescript to apply a representative Onyx material to the parts.
¶ Fillets and Lightening
Plates and Bent Sheet Metal up to 1/8" Thick
| Radius/Fillet | Rib Width | |
| Standard | 0.150" | 0.250" |
| Minimum | 0.100" | 0.188" |
Plates >1/8" Thick and all Box Tube
| Radius/Fillet | Rib Width | |
| Standard | 0.150" | 0.188" |
| Minimum | 0.100" | 0.150" |
Billet and 3D Printed
- No Standard - Application Dependent
¶ Shafts and Bearings
¶ Standard Shafts
1/2 Rounded Hex (aka Thunderhex) - 1/2" hex profile intersected with 13.75mm circle, and 0.159" through bore hole. Made from 7075 Aluminum
3/8" Rounded Hex - 3/8" hex profile intersected with 10.25mm circle, and 0.159" through bore hole. Made from 7075 Aluminum
1/2 Straight Hex - 1/2" hex profile, usually with the ends turned down to 13.75mm or 1/2" round for a bearing
Shafts can be modeled either with a sketched profile or with the Shaft Generator featurescript
¶ Standard Bearings
| Bearing Name | ID | OD | Depth | Overall Width | Flange OD | Flange Width |
| Flanged 1/2" Rounded Hex | 13.75 mm | 1.125" | 0.250" | 0.313" | 1.225" | 0.063" |
| FR8ZZ | 0.500" | 1.125" | 0.250" | 0.313" | 1.225" | 0.063" |
| Flanged 3/8" Rounded Hex | 10.25 mm | 0.875" | 0.218" | 0.281" | 0.969" | 0.063" |
| FR6ZZ | 0.375" | 0.875" | 0.218" | 0.281" | 0.969" | 0.063" |
¶ Standoffs and Spacers
¶ Threaded Standoffs
#10-32 Tapped - 1/2" Rounded Hex, 3/8" Rounded Hex
Hex is preferred due to the ability to grab it with a wrench for tightening and loosening the screws.
Model with the Shaft Generator Featurescript.
¶ Unthreaded Spacers
#10 Clearance (0.196"-0.201") - 5/16" Round is preferred, 3/8" Round or 1/2" Round for custom lengths or if larger face contact is required.
1/4" Clearance (0.257") - 1/2" Round preferred, 3/8" Round can be used if required for packaging.
Model as an extrude from sketch or use Spacer Generator Featurescript.
¶ Chain, Belt and Gears
#25 and #35 ANSI Chain
HTD 5mm Pitch Belts - 9mm or 15mm width
20DP or 10DP Gears
¶ COTS Parts
¶ MKCAD
MKCAD is a library of common FRC COTS components from all major vendors, as well as generators for parts like pulleys which can be 3D printed. MKCAD is available as both an App and in public Onshape Document form for importing parts into assemblies. 2910 prefers to use the Onshape Document version since it uses the same assembly insert menu, and can also be used to derive parts into part studios for modification (e.g. custom generated pulley or a sprocket that will get custom lightening).
¶
How to access MKCAD Documents:
- Make sure you are logged in to the 2910 Enterprise.
- Do a public search in Onshape by clicking this link.
- Click the label icon in the top right (next to the trash can) and then in the drop down click
Create New Label. Call it 'MKCad' - Next you will add all documents from this search to the label by right clicking on the document, clicking
Labels..., then adding to the newly created MKCad label - When you want to insert a part from MKCAD, use the Insert (for assemblies) or Derive (for part studios) feature, select the the “Other Documents” tab and the MKCAD label you created, then find the MKCAD document with the part you want.
¶ Imported Components
If a COTS component isn't available in MKCAD - for example a specialty screw, you will need to import a STEP file into your Onshape subassembly document. Put all imported components in a folder in the document to the right of all part studio tabs.
¶ Modifying COTS Parts
If you need to modify a COTS part, such as adding lightening to a gear or sprocket, insert it as a Derived part into it's own part studio in the relevant subassembly document. As a modified part, it should get an assigned Part Number
¶ Standard Featurescripts
Use only the Featurescripts loaded into 2910 Onshape Enterprise. This will ensure that you are using the correct and latest version.
Standard Featurescripts in 2910 Onshape Enterprise:
¶ Assemblies
¶ Duplicate and Mirror Parts
Coming Soon
¶ Group Mate
Coming Soon
¶ Replicate
Coming Soon
¶ Hardware
Coming Soon
¶ BOM
Coming Soon
¶ Configurations
Coming Soon
¶ Fab Handoff
¶ Identifying the Correct Part Version
Coming Soon
¶ Export for Sponsors
Coming Soon
- CREO
- SDS
- Fabworks
- Microsoft APC
¶ Export for 3D Printing
Coming Soon