Your First CNC Part: Complete Step-by-Step Project Walkthrough

A CNC machine does not care what you want to make. It follows the instructions you give it. Your job is to give it the right instructions.

This tutorial walks you through machining your first CNC part — a simple aluminum mounting bracket — from start to finish. You will design it in Fusion 360, generate toolpaths, set up the machine, and cut the part. By the end you will have completed the entire CNC workflow and understand what each step does.

The part we are making is a 3“ × 2“ × 0.5“ aluminum bracket with a pocket and two through-holes. It is simple enough to finish in one session but complex enough to teach facing, contouring, pocketing, and drilling.

---

What You Will Need

Item	Specification	Notes
CNC machine	Mill or router with at least 4“ × 4“ work area	Tormach, Shapeoko, Onefinity, or similar
Material	6061 aluminum, 3“ × 2“ × 0.5“	Available at Online Metals, McMaster, or local supplier
End mill 1	1/4“ 2-flute uncoated carbide	For facing, contouring, and pocketing
End mill 2	1/8“ 2-flute carbide	For smaller features if needed
Drill bit	#7 drill bit (0.201“)	For 1/4-20 tapped holes
Coolant	Mist coolant or WD-40	Prevents chip welding
Workholding	Vise or clamps	Must hold the 3“ × 2“ × 0.5“ blank securely
Software	Fusion 360 (free hobbyist license)	CAD + CAM in one package

---

Step 1: Design the Part in CAD

Open Fusion 360 and create a new design. The part is a flat plate with a pocket and two holes.

Create the Base Plate

1. Create a new sketch on the top plane
2. Draw a rectangle centered on the origin: 3“ wide × 2“ tall
3. Finish the sketch
4. Extrude the rectangle 0.5“ upward — this is the base plate

Add the Pocket

1. Create a new sketch on the top face of the plate
2. Draw a rectangle: 2“ wide × 1“ tall, centered on the plate
3. Offset the rectangle inward by **0.25“ — this creates the pocket walls
4. The pocket dimensions are: **1.5“ × 0.5“
5. Finish the sketch
6. Extrude the pocket 0.25“ downward (remove material)

Add the Mounting Holes

1. Create a new sketch on the top face
2. Draw two circles: 0.201“ diameter (#7 drill)
3. Position them 0.25“ from each edge in opposite corners
4. Finish the sketch
5. Extrude the holes through all (remove material, 0.5“ deep)

Save the Design

Save the Fusion 360 design as first-bracket v1. You now have a complete 3D model ready for CAM.

---

Step 2: Generate Toolpaths in CAM

Switch to the Manufacture workspace in Fusion 360. This is where you tell the software how to cut the part.

Setup

1. Select your machine type from the post-processor list (e.g., Haas, Tormach, GRBL)
2. Define the stock as the same size as your material: **3“ × 2“ × 0.5“
3. Set the stock box origin to the top center of the part (this becomes your G54 zero)

Operation 1: Face the Top

Parameter	Value
Operation	Face
Tool	1/4“ 2-flute carbide end mill
Spindle speed	10,000 RPM
Feed rate	50 IPM
Stepover	50% of tool diameter
Depth per pass	0.010“
Stock to leave	0.000“

This faces the top surface flat. Even if the material is already flat, facing ensures the top is parallel to the machine table.

Operation 2: Rough the Pocket

Parameter	Value
Operation	2D Pocket
Tool	1/4“ 2-flute carbide end mill
Spindle speed	10,000 RPM
Feed rate	40 IPM
Stepover	40% of tool diameter
Maximum roughing stepdown	0.050“
Stock to leave	0.010“ (for finishing)

Operation 3: Finish the Pocket Walls

Parameter	Value
Operation	2D Contour (finish pass)
Tool	1/4“ 2-flute carbide end mill
Spindle speed	10,000 RPM
Feed rate	30 IPM
Stock to leave	0.000“

This cleans up the 0.010“ left by the roughing pass, producing a smooth wall surface.

Operation 4: Drill the Holes

Parameter	Value
Operation	Drilling (G81 cycle)
Tool	#7 drill bit (0.201“)
Spindle speed	4,000 RPM
Feed rate	8 IPM
Depth	Through all (0.5“ + drill tip)
Cycle	G81 (standard drilling)

Simulate Before Generating G-Code

Click Simulate in Fusion 360 CAM. Watch the toolpath from start to finish. Verify:

• The tool does not crash into the vise or clamps
• The pocket is machined to the correct depth
• Both holes are drilled completely through
• The facing pass covers the entire top surface

Common CAM Mistakes to Avoid

Mistake	Consequence	How to Avoid
Wrong post-processor selected	G-code does not work on your machine	Double-check the post matches your controller
Stock box larger than material	Tool rapids through air, wasting time	Set stock box to exact material dimensions
Tool diameter wrong in CAM	Pocket comes out undersized or oversized	Measure each tool and enter exact diameter
No stock to leave on roughing	Finishing pass has nothing to clean up	Leave 0.005-0.010“ for finishing
Feed rate too conservative	Tool rubs instead of cutting	Use recommended starting feeds
Work offset mismatch	Machine cuts in wrong location	Verify G54 in CAM matches G54 on machine

---

Step 3: Post-Process and Load G-Code

1. Select the correct post-processor for your machine
2. Click Post to generate the G-code file
3. Save the file as first-bracket.nc or first-bracket.txt
4. Transfer the file to your CNC machine via USB, network, or SD card

What the G-Code Looks Like

The first few lines of your program should look something like this:

%
O1000 (FIRST BRACKET)
(T1 = 1/4 END MILL)
(T2 = #7 DRILL)
G90 G94 G17 G54  (Safety block: absolute, IPM, XY plane, G54)
T1 M06           (Load tool 1)
S10000 M03       (Spindle on at 10,000 RPM)
G00 X1.5 Y1.0    (Rapid to start position)
G43 Z1.0 H1      (Tool length offset, move to clearance)
Z0.1             (Approach)
G01 Z0 F20.      (Feed to top surface)
...              (Toolpath continues)

Verify that the G-code calls G54 (the work offset you will set on the machine) and that the tool numbers match the tools you have loaded.

---

Step 4: Set Up the Machine

Follow the setup procedure from the CNC Machine Setup Guide:

1. Home the machine — Z first, then X, then Y
2. Load tools — Tool 1 (1/4“ end mill) and Tool 2 (#7 drill bit)
3. Set tool length offsets — touch off each tool and record the offset
4. Mount the workpiece — clamp the 3“ × 2“ × 0.5“ aluminum blank securely in a vise
5. Set G54 part zero:
   • Z zero = top of the material
   • X zero = center of the part (left-right)
   • Y zero = center of the part (front-back)
6. Load the G-code program
7. Dry run — raise Z by 2“, run the program with spindle off, watch for clearance

---

Step 5: Make the First Cut

Setting	Value
Rapid override	25%
Feed override	50%
Single block	ON
Hand position	On Feed Hold

Press Cycle Start. Watch the first 10 seconds carefully. The tool should:

1. Move to the start position at reduced rapid speed
2. Lower to the clearance plane above the part
3. Start the facing pass across the top surface

Listen for: A smooth, consistent cutting sound. You should see chips forming — not dust. If you hear squealing (tool rubbing), increase the feed override. If you hear chatter, decrease the feed override.

During the pocket roughing: The tool will make multiple passes, each 0.050“ deeper. This is normal. The cut should sound consistent throughout each pass.

During drilling: The drill will feed into the material in one continuous motion (G81 cycle). It will retract after reaching full depth. Both holes should be identical.

---

Step 6: Inspect and Measure

After the program finishes, stop the machine and remove the part.

What to Check

Feature	Expected	How to Measure
Overall width	3.000“	Calipers
Overall height	2.000“	Calipers
Thickness	0.500“	Calipers
Pocket depth	0.250“	Depth micrometer or caliper depth rod
Pocket width	1.500“	Inside calipers
Hole diameter	0.201“	Drill gauge or pin gauge
Surface finish	Smooth, no visible tool marks	Visual inspection

Common First-Part Issues

Issue	Likely Cause	Fix Next Time
Pocket is shallow	Z zero was set incorrectly	Re-touch Z zero with the paper method
Holes are not through	Drill depth was wrong	Extend drill depth past material thickness
Rough surface finish	Feed rate too low or tool dull	Increase feed or replace end mill
Burrs on edges	Tool is cutting instead of shearing	Use climb milling for final pass
Part shifted during cut	Clamping was insufficient	Tighten vise or add more clamps

---

Step 7: Finish and Deburing

1. Remove burrs from all edges with a deburring tool or file
2. Clean the part with alcohol or degreaser to remove coolant residue
3. Inspect the final dimensions — if everything is within 0.010“ of the target, call it a success
4. Tap the holes (optional): If you have a 1/4-20 tap, thread both holes

---

Summary: The Complete Workflow

CAD (15 min)     →  CAM (15 min)    →  Post (2 min)
  Design part        Generate            Create G-code
  in Fusion 360      toolpaths

Setup (10 min)   →  Dry Run (3 min)  →  Cut (20 min)
  Home, load tools,   Verify paths,     Machine the part
  set offsets         check clearance

Inspect (5 min)   →  Deburr (5 min)
  Measure features,   Remove burrs,
  check dimensions    clean part

Total time for your first part: approximately 60-75 minutes from start to finish. After you have done it once, the same part takes about 30-40 minutes.

---

My First Part Story

My first CNC part was not a bracket. It was a simple square with a hole in the middle — a practice piece recommended by a friend. I spent three hours designing it in a CAD program I did not know how to use, another two hours fighting with CAM settings, and then crashed the machine on the first cut because I forgot to set the tool length offset.

The second attempt worked. The square was slightly out of square by 0.005“, the hole was 0.003“ oversized, and the surface finish looked like sandpaper. But it was a real CNC-machined part that I designed and made myself. I kept that part on my desk for two years.

What I learned: The first part is about learning the workflow, not making a perfect part. Every subsequent part will be better because you are building on what you learned from the previous one.

How to Diagnose Problems by Looking at Chips

The chips your machine produces tell you whether the parameters are correct.

Chip Appearance	Meaning	Action
Fine dust	Feed too low — tool rubbing	Increase feed 20%
Short curled chips	Parameters correct	Keep cutting
Long stringy chips	Feed slightly low	Increase feed
Blue/discolored	Too much heat	Increase coolant
Welded to tool	Wrong coating/no coolant	Stop, fix, restart

Stop after each operation and examine the chips. This habit teaches more about feeds and speeds than any guide.

Next Steps After Your First Part

Now that you have completed one part, here is what to do next to build your skills:

Make the same part again. The second time will be faster and the result will be better. You will catch mistakes from the first attempt and improve the setup. Making the same part repeatedly is the fastest way to develop muscle memory for the CNC workflow.

Modify the design. Change the pocket shape to a circle. Add more holes in a pattern. Increase the pocket depth to 0.375“. Small modifications teach new CAM operations without the overhead of designing from scratch.

Try a different material. Cut the same bracket in plastic (HDPE or Delrin) to feel the difference in cutting characteristics. Then try hardwood. Each material teaches you something new about feeds, speeds, and cutting sound.

Add a finishing operation. After the basic part works, add a chamfer operation to break all sharp edges in the CAM program instead of doing it by hand. This teaches contour toolpaths and chamfer mills.

Reduce cycle time. Try increasing feed rate by 20% while keeping the same depth of cut. If the cut still sounds good and surface finish is acceptable, keep the new feed rate. Repeat until you find the limit of your machine.

---

FAQ

What is the best first CNC project for a beginner?

A simple mounting bracket with a flat plate, one pocket, and two holes. It teaches all the essential skills: facing, contouring, pocketing, and drilling — but the geometry is simple enough that you can focus on the process.

What material should I use for my first CNC part?

Use 6061 aluminum or hardwood. Aluminum machines well and produces good results. Wood is more forgiving but produces dust. Avoid steel for your first part.

What software do I need for my first CNC project?

Fusion 360 is the best choice. It is free for hobbyists, combines CAD and CAM in one program, and has extensive beginner tutorials.

How long does it take to machine a simple first part?

About 15-30 minutes of cutting time. Design and CAM setup add 1-2 hours the first time, dropping to 15-30 minutes after you have done it once.

What if my first part does not come out perfect?

That is normal. Your first CNC part will have imperfections. The goal is to complete the full workflow from design to finished part, not to produce a perfect part.

---

Related Guides

• CNC Machine Setup Guide — Full setup from power-on to first cut
• CNC Machining Aluminum Guide — Feeds and speeds for aluminum
• CNC Workholding 101 — How to hold your workpiece
• CNC Safety Guide — Essential safety before you start