Purpose: Look, I have zero clue what I'm doing either, but these are things I've run into the past 2 weeks that may be useful to know going in. This guide will hopefully speed up the process for you and make your life (and Todd's life, and your teammate who ends up machining this piece's life) a heck of a lot easier!!

Written by a clueless frosh, for clueless frosh/new RT members (or anyone else who could use this)

First: If you do not have a mouse, please get one. Track pads are not fun. Just a CAD thing.

Oh, and learn to CAD :) This guide assumes you have a part already fully modeled, so unless you have a completed CAD file from someone else, unfortunately this won’t be much help. If you’re on Rocket Team (or really just in college), however, you are surrounded by people who are very experienced with CAD - reach out! Everyone (at least that I’ve met) is super friendly and more than happy to help you out. It’s a super fun and useful skill to have, and pretty critical to design your own parts.

1. Creating a Drawing

Did I have to Google how to do this the first time? Yes. I could not find the drawing tab for anything.

Once you’ve made your CAD of a part (or have one someone else made), go to the symbol that looks like a sheet of blank paper at the very top and left of your screen. Left-click, and you’ll get a dropdown from which you should select “Make Drawing from Part/Assembly”

Image Description: Screenshot of option to “Make Drawing from Part/Assembly” in upper left of SolidWorks interface.

Choose a Template

I believe this is mostly up to you, but I typically go with the “A (ANSI) Landscape” option (basically just because it is first on the dropdown menu), and delete the sections at the bottom I don’t need so I have more space for actual drawings. This is probably a rookie mistake; please ask your subteam lead until I get clarification on this :)

Image Description: Screenshot of pop-up where you can select your drawing template.

Once you select your template, you’re ready to start filling it out!

Quick note: When you’re in “Edit Sheet” mode where you can drawing views but can’t edit the details at the bottom of the document like your name, the title, etc, to exit this mode, right click on empty space on your document and click “Edit Sheet Format”.

If you’re in “Edit Sheet Format” mode where you can edit all the details on the bottom of the document like your name, the drawing name, etc, you can’t create drawing views. To exit this mode, right click on empty space on your document and click “Edit Sheet Format”.

Filling Out Basic Info

First things first: fill out the “TITLE”, “DRAWN - NAME”, “DRAWN - DATE”, and “MATERIAL” sections of the sheet format. This way when people are looking at the file, even if it’s in progress (which you should add in the “COMMENTS” section), they know who to contact with questions/comments, as well as generally what this drawing is supposed to be of.

For “NAME”, add your kerb - it’s (usually) shorter than your name and gives people a way to contact you if they don’t know you/have your contact info directly.

This will be covered again later, but please give your drawing a more descriptive title than “Rocket Team Part” or “Nozzle”. To this end, the material is also useful for one to identify what this drawing is if the title is a bit ambiguous; some nozzles are graphite, some phenolic, etc.

To edit the text, make sure you are in “Edit Sheet Format” mode (see above if you are stuck in “Edit Sheet” mode) and just double-click on the box you want to edit. If what you’re entering doesn’t fit, decrease the font size, or for things like comments, see if you can clearly but concisely rephrase the text. You can also change the size of different portions of the table and delete the parts you aren’t using (e.g., all the table content to the left of the column with “unless otherwise specified”.

Image Description: Screenshot of portions of the “Edit Sheet Format” interface to fill out first.

Basic Document Property Settings

Seriously, do these before you start your drawing. Future you will thank past you. Best if you do all this when actually creating the CAD so you’re more familiar with the numbers you’re seeing as you create the drawing, but now you definitely need to swap.

Change Units to Inches (Bottom Right Corner!)

Look at the bottom right corner of your drawing
Left-click where it probably says "IPS" or “MMGS”
Make sure "IPS" is selected
This is what the team (and most US shops) use, and even though I love using millimeters, when you’ve learned to face in 20 thou chunks but your dimensions are metric, millimeters to thou is not fun

Image Description: Screenshot of units setting in bottom right corner of SolidWorks Sketch interface.

Change Sig Figs to 4* Decimal Places

Go to Tools → Options → Document Properties → Units
Change "Decimals" to 4 places (so it shows 0.0000)
Click OK
This makes things much easier down the line, I promise. Please don’t machine your parts with only the hundredths place of dimensions; sometimes your tolerances are literally ±0.0005”.

*Note: 3 decimal places is likely fine (it’s all you’re going to get accurate on most lathes), but I like to be safe rather than have to redo a whole part.

[IMAGE OF DOCUMENT PROPERTIES SETTINGS WINDOW]

Image description: Screenshot of Document Properties Settings Window.

Fill Out Your Title Block

Put in:

Part name (be specific, not just "bracket" or “RT Part”)
Your name or kerb (so people can contact you if they have questions)
Date
Material (ask your subteam lead if unsure; it is very important to machine the graphite nozzle out of, say, graphite, rather than aluminium)
Scale (This depends on how many detailed parts you have and generally just what fits reasonably; I’ve found 1:2 to be pretty typical, but make sure you adjust this in both the text of your document and the document properties at the bottom-right of the screen)

Sheet number (Sheet 1 of 2, etc.)

[IMAGE OF COMPLETED TITLE BLOCK]

2. What Even Is A Drawing

Okay so you made a cool part in CAD. Congrats! But someone can't just look at your 3D model and magically know how to make it. A drawing is basically a 2D instruction manual that tells the machinist:

What it looks like (the views)
What size everything is (dimensions)
How perfect it needs to be (tolerances)
Special stuff (threads, deburring, material, etc.)

This is similar to how you wouldn't show someone a picture of a random personalized cake and expect them to bake it without measurements and instructions.

3. Minimum Requirements for Rocket Team Drawings

According to official Rocket Team standards, at minimum your drawing shall:

Show dimensions for all critical features

Every feature that matters needs a size and location
If it affects fit, function, or performance = critical
When in doubt, dimension it

Note material and finish for the part

Material: what it's made of (6061-T6 Aluminum, 304 Stainless, etc.)
Finish: what happens after machining (anodize, paint, mill finish, etc.)
These go in your notes section or title block

Have three orthogonal projections in 3rd-Angle-Projection

Orthogonal = 90° from each other (front, top, right side)
3rd-Angle-Projection = US standard (this is what SolidWorks defaults to)
These are your basic three views - you'll always need them

Don't be afraid to have multiple sheets

2-3 sheets can be good for nozzles and more complex parts
Better to have an extra sheet of paper than cluttered, easy-to-confuse-dimensions drawings
Most people would much rather flip pages than squint at a crowded mess

[IMAGE OF GOOD MULTI-PAGE DRAWING EXAMPLE]

4. Making Views That Are Easy to Understand

The Basic Three Views (Required!)

Front View - The main view where you can see the most stuff

Pick the angle that makes the part most recognizable
This should show the most important features

Top View - Bird's eye view looking down

Shows the shape from above
One of your three required orthogonal projections

Right Side View - Looking at it from the right

Shows the profile
Completes your three orthogonal projections

[IMAGE OF FRONT, TOP, RIGHT VIEW LAYOUT]

How to Make Them in SolidWorks

Insert → Drawing View → Model
Pick your part file
Click to place the front view
SolidWorks will auto-project the other views - just click where you want them
Don't crowd them together, give them space to breathe

Fancier Views (Use These, They Help A Lot)

Section Views - For when you need to show what's inside

If you have pockets, internal holes, or anything hiding inside, USE THESE
They're way clearer than a million dashed lines
Insert → Drawing View → Section
Draw a line where you want to "cut" the part open
Label it (it'll auto-label as "SECTION A-A" or whatever)

[IMAGE OF SECTION VIEW EXAMPLE]

Detail Views - Zoom in on tiny stuff

Small holes? Tiny chamfers? Zoom in so people can actually see them
Insert → Drawing View → Detail
Draw a circle around what you want to zoom into
Make it 2:1 or 4:1 scale

[IMAGE OF DETAIL VIEW EXAMPLE]

Isometric View - The 3D-looking one

Optional but honestly really helpful for understanding the part
Just add it if you have space

Hidden Line View - The dashed lines one

Shows internal features with dashed lines
Honestly section views are usually clearer, but sometimes this works
Use sparingly, as too many dashed lines gets confusing fast

5. Dimensioning (a.k.a. actually having the measurements you need when machining)

It sounds stupid and maybe it’s just me, but this is where I spent like 80% of my time fixing mistakes, both from myself and others.

The Main Rule: Pretend You're Machining It

Every single feature needs 2 main things:

SIZE - How big is it?
LOCATION - Where the heck is it?

A hole without a location is useless. A pocket without a depth is useless. Etc.

CRITICAL: If You're Unsure of a Dimension

If you're unsure of a dimension, contact whoever made the CAD and/or your subteam lead BEFORE continuing to machine. Preferably figure this out before you even get to the machine shop, but know Todd would, like you, prefer not to redo the part and would rather you take as long as you need to figure out the proper dimensions.

How to Add Dimensions

Click the Smart Dimension button (or just press D)
Click on edges, circles, points - whatever you need to measure
Place the dimension somewhere readable
It'll pull the value from your CAD model automatically

[IMAGE OF SMART DIMENSION TOOL]

What You Absolutely Need to Dimension

For any rectangular part:

Overall length, width, height

For EVERY hole:

Diameter (use the Ø symbol)
Location from edges (X and Y distances)
Depth if it doesn't go all the way through
If it's threaded: the thread spec (more on this later)

For pockets/cutouts:

Length and width
DEPTH
Location from edges
Corner radius if the corners are rounded

For chamfers and fillets:

Chamfers: "0.0625 X 45°" (size × angle)
Fillets: "R 0.0312" (radius)
Or just use a general note (see Notes section)

[IMAGE OF WELL-DIMENSIONED PART]

Where to Put Dimensions

Keep them outside the part outline when you can
Put them between views (like height dims between front and side view)
Don't let dimension lines cross each other
Space them out evenly - don't make it a cluttered mess
If it's getting cluttered, you need probably more pages (see Multi-Page section)

Additional Tips

Dimension from datum surfaces - these are the flat surfaces you'd clamp from when machining
Dimension multiple things from the same datum when possible
Don't dimension the same thing twice in different ways
If you can calculate it from other dimensions, don't add it (though sometimes I do find this convenient for myself and will make an extra sheet just for these drawings because addition and subtraction are hard and I don’t trust myself to input numbers into a calculator correctly)
Take note of where the zeroes for your part will likely be when machining; e.g., the face of the piece and the centerline through the diameter

6. Tolerances - Yes You Need Them

Tolerances are very important, and can drastically affect your part’s performance or usability. If you are unsure, it is best to contact your subteam lead.

What Is a Tolerance?

It's basically "how wrong can the machinist be and it's still okay"

Example: 1.0000" ±0.0050" means anywhere from 0.9950" to 1.0050" is acceptable.

General Tolerances

If all/most dimensions have the same tolerances, just add it in the notes at the bottom so you don't over-clutter your drawing:

UNLESS OTHERWISE SPECIFIED: TOLERANCES: .XX ± .01 .XXX ± .005 .XXXX ± .0010 ANGULAR: ± 0.5°

Translation:

Two decimal places (1.50) = ±0.01"
Three decimals (1.500) = ±0.005"
Four decimals (1.5000) = ±0.001"

When You Need Special Tolerances

If you have something specific with a different tolerance than everything else, just add it on that one dimension.

Example: Instead of writing "1.5000", write "1.5000 ±.0005"

When to use tighter (smaller) tolerances:

O-ring grooves (this will pierce your o-rings and cause you a lot of problems if wrong)
Parts that need to fit together closely
Bearing fits
Anything your lead says needs to be precise

When looser tolerances are fine:

Clearance holes
Non-critical dimensions
Overall sizes where exact numbers don't matter much

Tighter tolerances = more time = more expensive = more annoying to machine. Only make things tight where they need to be, but when they need to be, they NEED to be.

Not Sure? Ask!

Seriously, ask your subteam lead about tolerances for everything if you don’t know yourself, but especially for:

Pressure vessel stuff
O-ring grooves
Anything that sounds important
Anything you're unsure about

7. Notes, a.k.a. The "Deburr All Edges" Section

The Notes You Should Include

Add these at the bottom of your drawing:

NOTES:

DEBURR ALL EDGES
BREAK ALL SHARP CORNERS .010 MAX (*note: I actually haven’t seen this used myself but I believe it is generally important according to Google; please check with your subteam lead about this)
MATERIAL: 6061-T6 ALUMINUM (or whatever you're using)
FINISH: MILL FINISH (or anodize, paint, etc. if needed)
INTERPRET DIMENSIONS AND TOLERANCES PER ASME Y14.5 (not really necessary, but good practice)

[IMAGE OF NOTES SECTION ON DRAWING]

Why These Actually Matter

DEBURR ALL EDGES - The edges get really sharp and in addition to not being fun to handle, if your piece has o-rings this can pierce the o-rings and cause you a lot of problems. Just trust me on this one.

BREAK SHARP CORNERS - Makes it less painful to handle and less likely to cut your fingers

MATERIAL - Whoever is ordering stock and/or machining needs to know what to buy or grab from the stock. Also super important because some materials (like 306 stainless steel) are a pain to machine - Todd needs to know so he can give you the bad drill bits going in so you don't destroy all the good ones :)

FINISH - If it needs anodizing or coating, say so now

Hole Callouts (Super Important)

Instead of adding separate dimensions for hole diameter and depth, use a callout:

Through holes:

"Ø.2500 THRU" (quarter inch, goes all the way through)

Blind holes (don't go all the way through):

"Ø.2500 ↧ .500" (quarter inch diameter, half inch deep)

Threaded holes:

"1/4-20 UNC TAP ↧ .500"

1/4 = diameter
20 = threads per inch
UNC = thread type (ask your lead if unsure)
TAP = it gets threaded
.500 = how deep the threads go

For counterbored holes (for bolt heads):

"Ø.2500 THRU, C'BORE Ø.500 ↧ .250"

[IMAGE OF HOLE CALLOUT EXAMPLES]

How to Add Notes in SolidWorks

Insert → Annotations → Note
Click where you want it
Type your note
For symbols:

Diameter: <MOD-DIAM> or click the Ø button
Depth: <MOD-DEPTH> or click the ↧ button

8. Common Rocket Team Drawing Notes

These are official Rocket Team standard notes you can use on your drawings. The "X" just means whatever note number you're on (1, 2, 3, etc.). See: https://wikis.mit.edu/confluence/display/RocketTeam/Rocket+Team+Standard+Drawing+Notes for more details.

Machining Notes

MACHINE PER BEST SHOP PRACTICE

Use this when you don't care exactly how it gets made, as long as it matches the dimensions
Gives Todd flexibility in how he makes it
Alternative is to specify exact processes

USE MCMASTER-CARR PN: (YYYYYYYYY) AS STOCK TO FABRICATE THIS PART

For modified COTS parts (like firebolts, god-nuts, etc.)
Tells Todd where to get the starting part
Include the McMaster part number

MACHINE FROM PN: ASNNN

Use if you're machining from another Rocket Team part
Example: a bulkhead machined from a waterjet blank

THIS IS A DIGITALLY MANUFACTURED PART. ALL DIMENSIONS ARE FOR REFERENCE ONLY. THE CAD FILE SHALL BE THE MASTER FOR ALL DIMENSIONS NOT LISTED HERE.

For CAM/CNC parts where the computer does the work
Lets you be a bit lazy with dimensions on the drawing
All dimensions must be marked as reference dimensions

DRILL AND TAP PER UNC #4-40

Flag note before tapped hole callouts
UNC = Unified National Coarse (team standard thread)
Specifies thread type

SURFACE IS SEAL BEARING

Flag note pointing to o-ring or gasket surfaces
These surfaces are super critical - pay extra attention
Usually needs tight tolerances

BREAK ALL EDGES

Requires all edges be deburred
Can be done after machining or as part of CNC operation
Usually the chamfer isn't modeled in CAD

Part Marking Notes

Every part needs a part number and serial number for traceability. These follow aerospace standard AS478.

MARK PART NUMBER AND SERIAL NUMBER PER AS478 4.1.15

Laser etch the part mark
Works on anodized aluminum and some composites

MARK PART NUMBER AND SERIAL NUMBER PER AS478 4.1.7.4

Electro-etch the part mark
Needs vinyl mask, current supply, and salt water
Works on stainless steel, unanodized aluminum, titanium

PART IS MARKED PER AS478 4.1.1 ENSURE INFORMATION IS UPDATED PRIOR TO FABRICATION

For integral part marks (cast in, machined in, or 3D printed)
Must update serial number and revision before making the part

Finish Notes

ANODIZE TO CLASS II, TYPE 2 (COLOR) PER MIL-A-8625F

Colored anodize (specify the color)
Can add minimum/maximum coating thickness if needed

ANODIZE TO CLASS III PER MIL-A-8625F

Hardcoat anodize (thicker and tougher)
Dull gray color

PRIME, FILLER, AND SAND TO FINISH PER BEST SHOP PRACTICE

Gives machinist authority to apply primer, bondo, sand
Can specify if substrate can't be sanded into
Important for composite laminates

PAINT RED

Self-explanatory
Can specify Pantone color, brand, thickness
Can include masking instructions

APPLY CLEAR COAT

Can specify brand or chemical formulation

Testing Notes

TEST PER MIT ROCKET TEAM FIREBOLT HYDROSTATIC TESTING PROCEDURE

References team procedures on the wiki
Any team standard document can be called out

VERIFY RESISTANCE OF AT LEAST (OR LESS THAN) XXX OHMS

Flag note for electrical resistance checks
Important for avionics/e-matches to avoid shorts

9. How to Catch (almost) Everything Before Physically Machining

Word of advice when creating the drawings: go through it like you're actively machining the part (can be after you get everything you think is good down); you will likely catch a lot of useful dimensions you missed by accident.

Step 1: Imagine You Have Raw Material

Picture your piece of stock sitting in front of you
You need to turn it into your part
If you've never machined before, try your best - you'll find out real soon if not :)

Step 2: Walk Through Making It

Ask yourself:

"What surface would I clamp first?"; Do I have dimensions from that surface?
"What's my first cut?"; What do I need to measure to make that cut? Is that dimension on my drawing?
"What's my second cut?"; Can I reach it, or do I need to flip the part? If I flip it, what do I measure from? Do I have those dimensions?
"How do I make this hole?"; Do I know the diameter? Do I know where it is? Do I know how deep? Is it threaded?
"How do I make this pocket?"; Do I know length and width? Do I know depth? Do I know where it is?

Step 3: For EVERY Feature, Ask:

Do I know the

SIZE?
LOCATION?
DEPTH?
TOLERANCE?

Common Things You'll Probably Realize You Forgot

Depth of holes or pockets
Location of holes from edges
Which holes are threaded
Corner radii
Material callout
Deburr note

10. When to Use 2-3 Pages (Often)

I highly recommend using 2-3 pages of drawings depending on how complex the part is, because it very quickly gets hard to read. Don't be afraid to have multiple sheets of drawings (In my extremely limited experience, 2-3 can be good for the nozzles and more complex parts, as it's better to have an extra sheet of paper than cluttered, easy-to-confuse-dimensions drawings.)

Use Multiple Pages When:

You have more than 8-10 dimensions crammed onto one view
You need section views AND detail views
The drawing is starting to look like a mess
You're squinting to read dimension numbers
Features are on multiple sides of the part
You're working on nozzles or other complex parts

How to Split It Up

Page 1: The Big Picture

Front, top, right views (your three required orthogonal projections)
Overall dimensions (length, width, height)
Major features
General notes (including the DEBURR one)
Material and finish callouts

Page 2: The Details

Section views showing internal stuff
Detail views of small features (zoomed in)
Specific hole callouts
Tight tolerance callouts
Surface finish requirements

Page 3: If You Need It

More complex features
Assembly notes if it's part of a bigger thing
Special instructions
Testing requirements

[IMAGE OF MULTI-PAGE DRAWING ORGANIZATION]

How to Add Pages in SolidWorks

Right-click on the sheet tab at the bottom
Add Sheet
Update your title block sheet numbers (Sheet 2 of 3, etc.)

Better to have clear drawings on 3 pages than one incomprehensible page!!

11. Checklist Before You Bug Todd

Go through this before you show up. Seriously, it'll save everyone time.

Setup Stuff

Units = inches (bottom right corner)
Decimal places = 4 (0.0000)
Title block filled out (name, date, material)
Sheet numbers correct if multi-page
Using 3rd-Angle-Projection (SolidWorks default)

Minimum Requirements (Official Rocket Team Standards)

Dimensions shown for all critical features
Material noted
Finish noted
Three orthogonal projections present (front, top, right)

Views

Front, top, right views exist (required!)
Views are lined up properly
Section views for internal features (if needed)
Detail views for small stuff (if needed)
Not too many dashed/hidden lines (use sections instead)
Isometric view if you have space (optional but nice)

Dimensions - The Important Part

Overall length, width, height
EVERY hole has diameter (Ø)
EVERY hole has location from edges
EVERY blind hole has depth
EVERY threaded hole has thread callout (like "1/4-20 UNC TAP")
EVERY pocket has length, width, AND DEPTH ← don't forget depth!
EVERY pocket has location
Corner radii specified
Chamfers specified
No dimensions missing
No redundant dimensions
Dimensions aren't overlapping or impossible to read
Dimensions are from consistent datum surfaces
If unsure about ANY dimension, contacted CAD designer and/or subteam lead

Tolerances

General tolerance note exists
Special tight tolerances called out where needed (o-rings!)
Contacted subteam lead about critical tolerances

Notes

"DEBURR ALL EDGES" or "BREAK ALL EDGES" is there
Material specified
Finish specified (if applicable)
Part marking note included (if applicable)
Any special machining notes from Section 8

The Mental Exercise

Actually did the mental machining exercise
Can explain what surface you'd start from
Every dimension you'd need is on the drawing
Walked through how to make EVERY feature

*Note: Especially if you’ve never machined before or are pretty inexperienced, know that it’s totally fine if you don’t know what any of this means; your teammates and Todd are more than happy to help you out!!

Final Check

Not cluttered (if it is, add pages)
Neat and organized
Everything is readable
You'd be able to machine it from this drawing
Your teammate who ends up machining this won't hate you
Drawing is PRINTED OUT and ready to bring to Todd

12. Easy-to-Make Mistakes

Forgetting Hole Depths

The mistake: A hole shows diameter but not depth.

Why it's a problem: Can't machine it without knowing how deep to drill.

The fix: Always add depth "↧ X.XXXX" or "THRU" if it goes all the way through.

Not Specifying Threaded Holes

The mistake: Showing a hole without indicating it needs threads, or not specifying thread size.

Why it's a problem: You'll get an unthreaded hole back.

The fix: Use proper callouts like "1/4-20 UNC TAP ↧ .500"

Forgetting Pocket Depth

The mistake: A rectangular pocket shows length and width but not depth.

Why it's a problem: Can't machine it without knowing how deep to mill.

The fix: Always add depth to pockets! Show it in a side view or add a note.

Too Many Dashed Lines

The mistake: Trying to show internal features entirely with hidden/dashed lines.

Why it's a problem: Drawing becomes a confusing maze of dashed lines.

The fix: Use section views to show internal features clearly.

Over-Tolerancing Everything

The mistake: Making everything ±0.0005" because tighter seems better.

Why it's a problem: Takes way more time and is more expensive to machine. Unnecessarily difficult, don’t make your/the machinist’s life harder.

The fix: Only use tight tolerances where actually needed. Most stuff can be ±0.010" or ±0.005".

Forgetting the DEBURR Note

The mistake: No deburr note on the drawing.

Why it's a problem: Sharp edges are dangerous and will damage o-rings if present.

The fix: Always add "DEBURR ALL EDGES" or "BREAK ALL EDGES" to notes.

Not Doing the Mental Exercise

The mistake: Thinking the drawing is complete without walking through machining it.

Why it's a problem: Missing dimensions won't be caught until you're at the machine.

The fix: Walk through machining it mentally. Catches most missing dimensions.

Cramming Everything on One Page

The mistake: Trying to fit too many dimensions and views on a single sheet.

Why it's a problem: Creates an unreadable, cluttered mess that's easy to misinterpret.

The fix: Use 2-3 pages. Better to flip pages than squint at crowded dimensions.

No Material Callout

The mistake: Forgetting to specify what material the part is made from.

Why it's a problem: Machinist has to guess or ask what to use.

The fix: Always put material in title block or notes. It's a minimum requirement!

Skipping the Checklist

The mistake: Assuming the drawing is complete without going through verification steps.

Why it's a problem: Missing critical information that causes delays or mistakes.

The fix: Actually use the checklist in Section 11. Takes 2 minutes, saves hours.

Forgetting to Print It Out

The mistake: Showing up to the shop with only a laptop.

Why it's a problem: Physical paper is far easier to reference and mark up during work, and Todd requires it.

The fix: ALWAYS bring PRINTED drawings. Clean, readable prints. If you can’t print it yourself, email as a pdf to trb@mit.edu before arrival.

Not Asking When Unsure

The mistake: Being uncertain about a dimension (or anything else) but continuing anyway.

Why it's a problem: Can result in machining the part incorrectly and wasting material. You can also injure yourself or damage the machine, so ASK.

The fix: If unsure about anything, STOP and ask the CAD designer, subteam lead, or Todd before continuing. Also, your life is way more important than “bothering” someone if you’re not sure if the machine is supposed to be making that noise or if the parting tools can be moved on the Z-axis while in a part (DO NOT DO THIS).

13. Working in Todd Shop

This is important stuff about actually machining your part in Todd Shop.

Before You Even Get to the Shop

Make sure ALL your dimensions are clear and correct
If you're unsure of ANY dimension, contact whoever made the CAD and/or your subteam lead BEFORE continuing to machine
Preferably figure this out before you even get to the machine shop
Todd would, like you, prefer not to redo the part and would rather you take as long as you need to figure out the proper dimensions

While You're Machining

If you are unsure of something while machining, tell Todd immediately.

He is incredibly kind (kind of scary how much patience he has) and you will learn so much from him. He knows you're learning and is an incredible teacher.

Also tell him if you think you've made a mistake.

Again, you're learning. It's way better to catch a mistake early than finish the whole part wrong.

Safety First - Always

Please do not do anything stupid. Machining, though fun, can be incredibly dangerous and everything that is told to you is for a reason.

Listen to ALL safety instructions
Wear safety glasses ALWAYS
Keep long hair tied back
No loose clothing or jewelry
If something feels wrong, STOP and ask
Never reach over or into moving machinery
Wait for tools to completely stop before touching them

What Todd Needs From You

Clean, printed drawings (NOT just your laptop)
Questions when you're unsure (he'd rather answer questions than have you mess up)
Honesty if you make a mistake (seriously, just tell him)
Patience with yourself - you're learning
Following safety rules - no exceptions

What You'll Get From Todd

So much knowledge about machining
Patience while you learn
Help catching mistakes before they're permanent
Tips and tricks that aren't in any textbook
Understanding that you're new at this

Todd has a ton of experience, and he's worked with countless students who are learning. He'd much rather you:

Take your time and get it right
Ask questions when confused
Admit mistakes immediately
Follow safety rules like your life (and others’) depends on it, because it does

Than:

Rush and mess up the part
Guess and get it wrong
Hide mistakes and compound them
Do something dangerous

Clean up!!!

Do not leave a mess. When you’re done for the day, make sure to use the compressed air to blow any chips into a paper towel (not on the floor, but you do need to vacuum if there are chips/other stuff on the floor.
Wipe up the motor oil with a paper towel with a bit of SimplyGreen (the spray bottles on top of the lathes)

Look, none of us really know what we're doing. That's okay! This is how you learn. But following this guide will:

Make Todd's life easier
Make your teammate who machines it happier
Make your life easier when you have to remake stuff
Actually get your parts made correctly

Three things to remember:

Completeness - Every dimension is there (it's a minimum requirement!)
Clarity - It's not a cluttered mess (use multiple pages!)
Do the mental exercise - Walk through machining it

If you mess something up, it's fine. We all do. Just learn from it and update this guide for the next person.

Also seriously, ask for help when you're not sure about something. Ask Todd, ask your more experienced teammates, ask your subteam lead. That's what they're there for.

Now go make some good drawings and get your rocket parts made!

Tapping holes in the mostly-machined piece I used for this tutorial! Did I spend 80+ hours on this project in the span of 2 weeks? Maybe, but hey, Todd still got his (morning) coffees uninterrupted :) Fun note: it’s best to arrive at shop not at 9am, but 9:30am so Todd can turn on all the machines, make sure everything is in working order, figure out who he needs to help with what, and finish his coffee!

Random Machining Notes:

Quick Reference - Common Callouts

Through Holes: Ø.2500 THRU

Blind Holes: Ø.2500 ↧ .500

Threaded Holes: 1/4-20 UNC TAP ↧ .500 M6x1.0 TAP ↧ 10mm

Counterbored Holes: Ø.2500 THRU, C'BORE Ø.500 ↧ .250

Chamfers: 0.0625 X 45°

Fillets: R 0.0312

General Note Format:

NOTES:

DEBURR ALL EDGES (or BREAK ALL EDGES)
BREAK ALL SHARP CORNERS .010 MAX
MATERIAL: 6061-T6 ALUMINUM
FINISH: MILL FINISH
MACHINE PER BEST SHOP PRACTICE

UNLESS OTHERWISE SPECIFIED: TOLERANCES: .XX ± .01 .XXX ± .005
.XXXX ± .0010

Most Common Rocket Team Standard Notes

For Basic Parts: X. MACHINE PER BEST SHOP PRACTICE X. BREAK ALL EDGES X. SURFACE IS SEAL BEARING (flag note for o-ring surfaces)

For Modified COTS Parts: X. USE MCMASTER-CARR PN: (YYYYYYYYY) AS STOCK TO FABRICATE THIS PART

For Threaded Holes: X. DRILL AND TAP PER UNC #4-40

For Anodized Parts: X. ANODIZE TO CLASS II, TYPE 2 (COLOR) PER MIL-A-8625F X. MARK PART NUMBER AND SERIAL NUMBER PER AS478 4.1.15

For Steel/Titanium Parts: X. MARK PART NUMBER AND SERIAL NUMBER PER AS478 4.1.7.4

Helpful Videos - This whole guide is intended to be a living document, so please add!!

Link	General Description of Application/Level of Detail	Useful Timestamps
https://www.youtube.com/watch?v=wPb50okM7Rc	Solidworks Drawing Mode: 7 Genius Tips You Probably Didn’t Know About!
https://www.youtube.com/watch?v=50dKqlQthTg	SOLIDWORKS Tutorial - Drawings Tips and Tricks More for multi-part models than machining

If you're drilling/boring steel: NO you don't need a pilot hole.

Seriously, don't do it. When you drill a pilot hole and then come back with a larger drill bit, the larger bit wants to "walk" into the existing hole. This concentrates all the stress on one side of the drill bit's cutting edge instead of distributing it evenly. This breaks the drill bit. And will continue to break drill bits. Please don’t.

Instead: just use the correct size drill bit from the start. The drill bit is designed to center from the center drill alone and cut evenly when starting on a flat surface. It'll be fine, and Todd's drill bits will survive :) This is particularly important for steel because it's already harder to machine than aluminum - don't make it worse by snapping all the good drill bits!

Written by a frosh who learned all this the hard way - I did choose MIT to learn by doing, after all

Last updated: December 2025

Questions? Bug someone on your subteam or ask in Slack

Found this helpful? Feel free to pass it on to the next clueless frosh/anyone else; we’re all learning, but it’d be nice to save a few people many hours where possible! :)

Have something to add? Please do!! This is intended to be a living document

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