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.

Table of Contents

How to Not To Waste Hours of Your Life: A Beginner’s Guide to SolidWorks Drawings 1

Table of Contents 2

1. Creating a Drawing 3

Choose a Template 3

Filling Out Basic Info 5

Basic Document Property Settings 6

1. What Even Is A Drawing 9
2. Minimum Requirements for Rocket Team Drawings 10
3. Making Views That Are Easy to Understand 11
4. Dimensioning (a.k.a. actually having the measurements you need when machining) 13
5. Tolerances - Yes You Need Them 15
6. Notes, a.k.a. The "Deburr All Edges" Section 16
7. Common Rocket Team Drawing Notes 18

Machining Notes 18

Part Marking Notes 19

Finish Notes 19

Testing Notes 19

1. How to Catch (almost) Everything Before Physically Machining 21
2. When to Use 2-3 Pages (Often) 22

Use Multiple Pages When: 22

How to Split It Up 22

How to Add Pages in SolidWorks 22

1. Checklist Before You Bug Todd 23
2. Easy-to-Make Mistakes 25
3. Working in Todd Shop 27

Before You Even Get to the Shop 27

While You're Machining 27

Random Machining Notes: 29

Quick Reference - Common Callouts 29

Most Common Rocket Team Standard Notes 29

Helpful Videos - This whole guide is intended to be a living document, so please add!! 29

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:

1. 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

1. 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

1. 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

1. 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

1. Insert → Drawing View → Model
2. Pick your part file
3. Click to place the front view
4. SolidWorks will auto-project the other views - just click where you want them
5. 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:

1. SIZE - How big is it?
2. 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

1. Click the Smart Dimension button (or just press D)
2. Click on edges, circles, points - whatever you need to measure
3. Place the dimension somewhere readable
4. 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:

1. DEBURR ALL EDGES
2. 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)
3. MATERIAL: 6061-T6 ALUMINUM (or whatever you're using)
4. FINISH: MILL FINISH (or anodize, paint, etc. if needed)
5. 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

1. Insert → Annotations → Note
2. Click where you want it
3. Type your note
4. 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

1. 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

1. 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

1. MACHINE FROM PN: ASNNN

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

1. 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

1. DRILL AND TAP PER UNC #4-40

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

1. 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

1. 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.

1. MARK PART NUMBER AND SERIAL NUMBER PER AS478 4.1.15

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

1. 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

1. 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

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

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

1. ANODIZE TO CLASS III PER MIL-A-8625F

• Hardcoat anodize (thicker and tougher)
• Dull gray color

1. 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

1. PAINT RED

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

1. APPLY CLEAR COAT

• Can specify brand or chemical formulation

Testing Notes

1. TEST PER MIT ROCKET TEAM FIREBOLT HYDROSTATIC TESTING PROCEDURE

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

1. 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:

1. "What surface would I clamp first?"; Do I have dimensions from that surface?
2. "What's my first cut?"; What do I need to measure to make that cut? Is that dimension on my drawing?
3. "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?
4. "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?
5. "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

1. Right-click on the sheet tab at the bottom
2. Add Sheet
3. 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

1. 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.

1. 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"

1. 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.

1. 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.

1. 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".

1. 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.

1. 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.

1. 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.

1. 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!

1. 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.

1. 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.

1. 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

1. Clean, printed drawings (NOT just your laptop)
2. Questions when you're unsure (he'd rather answer questions than have you mess up)
3. Honesty if you make a mistake (seriously, just tell him)
4. Patience with yourself - you're learning
5. 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:

1. Completeness - Every dimension is there (it's a minimum requirement!)
2. Clarity - It's not a cluttered mess (use multiple pages!)
3. 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:

1. DEBURR ALL EDGES (or BREAK ALL EDGES)
2. BREAK ALL SHARP CORNERS .010 MAX
3. MATERIAL: 6061-T6 ALUMINUM
4. FINISH: MILL FINISH
5. 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!!

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