CAD Guidelines

To keep things more consistent at WARG, we enforce a set of guidelines on all submitted CAD designs. This only applies to mechanical CAD files (not electrical). Since we use SolidWorks for most of our mechanical work, these guidelines mainly apply to it. 

Modeling Rules:

In order for your design to be accepted it must adhere to all the rules listed below. If the part does not you will be notified what modifications need to be made in order for it to be accepted. Once your part is accepted you can begin to manufacturer/make the part. If an assembly of parts is being made all parts and the assembly must be approved before manufacturing/making the assembly. If you are not sure if your part meets a specific guideline, please reach out to a current mech lead for advice!

1. All parts (sketches) must be fully defined (No blue lines!).

2. All fastening holes (screw, bolt etc.. holes) must be done using hole wizard. Extruded cut holes are not acceptable except for weight saving holes.

3. M5, M3, and M2 bolts should be used wherever possible. M2 bolts should only be used for mounting off-the-shelf electronics that require them.

4. All fasteners (bolts, washers, nuts) should be included in assembly CAD where possible. Fasteners should be added in a subassembly file to join components together. If there are fasteners that join a subassembly to a main assembly, these fasteners should be added at the main assembly level.

5. All COTS (commercial-off-the-shelf) components (fasteners, motors, electronics) should be added to the COTS folder on PDM and be renamed to match WARG’s COTS naming convention.

6. All components that mount on the main aircraft frame must adhere to the standard mounting pattern. For Pegasus aircraft, mounting holes must be spaced apart by 30mm x 30mm or a multiple of 30mm. For airframes made after AEAC 2024, mounting holes must be spaced apart by 30.5mm x 30.5mm or a multiple of 30.5mm. Some off-shelf avionics may have mounting holes that disregard this standard, in which case, a mechanical lead must be informed.

7. Wherever possible, SHCS (Socket Head Cap Screws) should be used.

8. If a fully threaded or partially threaded version of the fastener to be used both exist, the partially threaded option should be used whenever possible.

9. Use relations (mates & constraints) to eliminate redundant dimensions.

10. Parts must be made using WARG’s part template, including using MMGS scale.

11. Parts must use WARG’s standard naming convention.

12. Assemblies must contain ALL components fully defined and related with all relevant dimensions specified.

13. NO assembly features.

14. When making part revisions look at the previous version and identify any filing/drilling/sanding/machining you had to do to the parts to make them fit and ENSURE that the new part is modified so that the changes don’t have to be made again.

15. Similar fillets or chamfers must be made in the SAME feature. (Think: if you wanted to edit the size of a set of fillets, you’d want to edit them all in one step). All fillets/chamfers must be added as features and NOT included in the sketches.

16. Ensure that your assemblies are manufacturable with appropriate tolerances (ie parts have clearance to be assembled and parts don’t have to go through walls/break physics to work). Before designing a part, you must think about material choice and manufacturing method!

17. Consider the thickness and dimensions of parts to ensure that they are reasonable.

18. All of the relevant CAD files should be uploaded and synced on Solidworks PDM. The design will NOT BE REVIEWED if it is not on Solidworks PDM. Screenshots and stl files do not suffice.

Drafting Rules:

1. Any part that is being manufactured in the ESMS, or by a sponsor needs a drawing.

2. All drawings must be made using the WARG drawing template.

3. Any parts to be made on a mill must primarily use ordinate dimensioning, with limited exceptions for pitched dimensions of holes, or to use proper GD&T for locating geometry.

4. Drawings to be machined should be made with millimeters as the primary dimension. For drill, end-mill & reamer sizes, stock sizes, or parts that are being made by a machinist, dual dimensions should be used with mm as the primary dimension and inches as the secondary dimension. This can be done using the smart dimension feature, by configuring it in the side menu. In very limited scenarios, a part being made by a machinist may have a drawing that uses exclusively imperial dimensions, this should only be done with mechanical lead approval.

5. Greater precision than 0.00mm & 0.000in dimensions should never be used. Dimensions should be only as strict as they need to be, and proper GD&T practices should be followed. It is however acceptable to use 0.000in dimensions where not necessary if they are being made on a machine with a 0.000in DRO (Digital read-out).

6. Wherever reasonable, circular dimensions should be given as a diameter, not a radius. This is because it makes choosing drill, end-mill & reamer sizes easier.

7. All circular parts and features must have center marks & center lines.

8. All hole callouts must be made with the hole-callout feature, and the generated callout should not be modified except with valid reasons. To do this, your model must use hole wizard!

9. All drawings must be reviewed before manufacturing!

NOTE: If you violate one of these rules you must notify a team lead with a valid explanation as to the reason for violating the commandment

CAD Naming Convention

All CAD files should adhere to the following naming convention (snake upper case):

For regular part files

eg. C24_GIMBAL_P003_OUTSIDE_CASE.SLDPRT

For assemblies

eg. C24_GIMBAL_A001_MAIN.SLDASM

For assemblies within assemblies

Create a folder with the same naming convention as the part, and follow the same naming convention inside the folder, prepending the project name.

For example, if the gimbal assembly contains a part camera which itself is also an assembly:

1. Create folder named GIMBAL_CAMERA

2. Inside the folder follow the same naming convention, but prepend the original project name at the begining.

eg.

For drawings

In the assembly folder create another folder to store drawings.

For the actual part files, follow the same naming convention as above, and store them in this folder.

For COTS Fasteners

Bolts:

Bolt type codes are as follows:

SHCS - Socket head cap screw

FHCS - Flat head cap screw

BHCS - Button head cap screw

Thread codes are as follows:

FT - Fully threaded

PT<THREADED_LENGTH> - Partially threaded

Nuts:

Washers:

Other COTS Components

Renders

Create a separate Renders folder within your project and dump all your renders there. No naming convention here.

Renaming Files in an assembly

This is most relevant for reorganizing old files that do not follow the naming convention. In order to rename a part file that’s referenced in an assembly follow these steps to make sure the file path used in the assembly doesn’t break.

1. Go to Tools > Options > Feature Manager and ensure Allow component files to be renamed from FeatureManager tree is selected.

2. Right-click on the component in the assembly and rename it according to the naming convention.