Cloudline controller

Cloudline controller PCB: from files to finished board

The controller on a printed circuit board instead of perfboard:

• one copper layer (the bottom), no wire links;
• all parts through-hole, on the top;
• 100 × 75 mm, four M3 mounting holes.

It carries every part in the schematic, plus a 4-way screw terminal for the fan cable and two pin headers for the OLED module.

This page covers everything about the board:

• the three ways to get a board made, and every file involved;
• a walkthrough in separate sessions, from opening the files to a finished, boxed controller;
• reference: design notes, how the board was checked, regenerating the files.

Top (parts side)	Bottom copper (as seen from below)

Status: designed and checked, not yet made. The files pass KiCad's design-rule check, an independent copper-connectivity check, an independent review, and the milling and EAGLE export checks below. No board has been built from them yet, and nothing has been opened in Fusion 360 or run on the machine. Build the first one expecting to find something.

Contents

1. Three ways to get a board
2. Your setup (milling)
3. Files
4. The walkthrough, session by session
   • How the sessions work · Progress log
   • S0 Gather materials
   • S1 Get the files
   • S2 Review or edit in Fusion Electronics (optional)
   • S3 Prepare and measure the blank
   • S4 Fusion: import
   • S5 Fusion: setup and operations
   • S6 Fusion: simulate and post
   • S7 Machine: prepare, mount, zero
   • S8 Machine: isolation
   • S9 Machine: drilling
   • S10 Machine: outline
   • S11 Clean, inspect, test the bare board
   • S12–S17 Assembly and first power-up
   • S18 Enclosure
5. Ordering from a board house
6. Design notes · Verification · Regenerating

Three ways to get a board

To change the circuit or the layout, use Fusion Electronics (session S2). The milling files in fusion/ and the Gerbers in fab/ are made from the KiCad copy of the board. They don't change when you edit in Fusion. See Which copy is master.

Your setup (milling)

The milling files and the walkthrough are made for this setup:

Assumed and to confirm:

• the V-bit's angle and tip;
• the outline end mill size;
• the tool numbers in your changer.

S4 says how to change any of these.

Board numbers that matter for milling:

• Gaps: the smallest gap between copper of different nets is 0.64 mm. It sits between neighbouring 2.54 mm-pitch header pads, and no layout can make it larger. Tracks keep at least 0.69 mm from other copper. Copper is at least 3.15 mm from the board edge.

• Isolation cut: two passes with the V-bit, 0.20 mm deep, 0.207 mm wide. That clears about 0.33 mm around every pad and track.

  • The paths were simulated for a board up to ±0.10 mm off the Z touch-off height, because there is no height map.
  • At 0.10 mm deep the cut still goes through 70 µm copper and isolates every net.
  • At 0.30 mm deep it trims 0.027 mm off copper edges, which is harmless.

• Holes: 99, all non-plated:

  Size	0.75	0.80	1.00	1.10	1.20	1.30	3.20 (M3)
  Count	4	32	51	2	2	4	4

Files

For milling (route A): fusion/

For editing (Fusion Electronics): eagle/

For ordering or etching (routes B, C): fab/

For every route:

The walkthrough, session by session

How the sessions work

Each session is a block of work you can finish in one sitting, and each ends at a checkpoint: a state you can safely leave and come back to. Every session has:

• Start: the checkpoint you need before you begin.
• Steps.
• Checkpoint: how you know the session is done, and what to record.
• If something goes wrong: how to back out or resume, without starting over.

Three habits make this work:

1. Save a Fusion version at every checkpoint. Use File → Save with a description, for example S5 done. A mistake later in Fusion is then undone by opening the version before it from the Data Panel, under Versions.
2. Post one file per operation as well as the full program. Then a stop in the middle of the job is resumed by running the remaining files. You never restart a half-finished program or search for a line number.
3. Don't move the blank and don't re-zero X/Y between S7 and S10. As long as the blank stays taped down and X/Y zero is unchanged, any machine session can be repeated or resumed, even on another day.

Progress log

Copy this table into a notebook or a text file next to the job and fill it in as you go. Then a session can be resumed by someone else, or by you a week later.

S0. Gather materials and check the fan

Start: nothing. Time: as long as shopping takes.

1. Board materials (route A):

   • an FR-4 single-sided copper-clad blank, at least 110 × 85 mm (100 × 160 Eurocard is fine);
   • thin double-sided tape;
   • a fine abrasive pad (Scotch-Brite), isopropyl alcohol;
   • optional: solder-through flux lacquer.

2. Tools for the tool changer:

   Slot	Tool
   T1	V-bit 30°, 0.1 mm tip
   T2	0.8 mm drill
   T3	1.0 mm drill
   T4	1.2 mm drill
   T5	1.3 mm drill
   T6	3.2 mm drill
   T7	2 mm end mill

   All carbide, 3.175 mm shank where possible. Put them in the changer and write down the slot numbers. If they aren't 1–7, you will renumber them in S4.

3. Measuring and testing: calipers, a multimeter with continuity beep, and a loupe or magnifier.

4. Electronic parts: ../bom.csv has part numbers. fab/pcb_bom.csv lists them by board reference. The ceramic capacitors need 5 mm lead pitch.

5. Safety: FR-4 dust is fine glass fibre. Use the dust extraction or a vacuum during every cut, wear a dust mask and eye protection, and never blow the dust away.

6. The fan: do the main README's pre-connection verification (checks M1–M6) whenever the fan is to hand. Its results decide whether R5 is fitted and whether anything else changes (S16).

Checkpoint: you have the materials and parts, and the tool slots are recorded.

S1. Get the files

Start: S0. Time: 10 minutes.

1. Download the repository: on GitHub, Code → Download ZIP, or git clone https://github.com/seesharp15/cloudline-fan-controller.
2. You need these folders: hardware/pcb/fusion/, hardware/pcb/eagle/ (only for S2) and hardware/pcb/fab/.
3. Print fab/assembly_top.pdf at 100 % (not "fit to page"). Check that the board outline measures 100 × 75 mm with a ruler. You'll use it in S11–S17.

Checkpoint: the files are on the computer running Fusion, and the assembly drawing is printed at the right scale.

Route B: go to Ordering, then continue at S11.

S2. Review or edit in Fusion Electronics (optional)

Start: S1. Time: 15 minutes to look, longer to edit.

1. In Fusion's Data Panel, choose Upload and select both eagle/cloudline_controller.sch and eagle/cloudline_controller.brd in one go. Fusion converts them into one electronics design with a linked schematic and board.
2. Open it. Run ERC on the schematic and DRC on the board. The board carries the rule set cloudline_single_sided:
   • 0.6 mm clearance;
   • 0.4 mm minimum track width;
   • 0.8 mm from copper to the board edge.
3. When editing:
   • Route on the Bottom layer only. Fusion draws a top-side ring on through-hole pads; on the real board that ring doesn't exist.
   • The schematic connects parts by net labels: a pin stub carrying the net name. Pins with the same label are the same net.
4. Save a version.

Checkpoint: the design opens, and ERC and DRC show nothing unexpected.

If you changed the board: the milling files in fusion/ no longer match it. Machine the edited board from Fusion's own 3D PCB instead of S4's STEP and DXF. The setup and operations in S5 stay the same idea, but the isolation needs a Trace or 2D Contour around the copper Fusion generates. If you only looked, carry on with S3 unchanged.

S3. Prepare and measure the blank

Start: S1. Time: 20 minutes.

1. Cut the blank to size, at least 110 × 85 mm, which leaves 5 mm around the board. Deburr the edges so it lies flat.
2. Measure the thickness with calipers at all four corners. Record the largest value in the log; it goes into the Fusion stock in S5. Typical values are 1.5–1.6 mm.
3. Clean the copper with the abrasive pad, then alcohol. Don't touch it with bare fingers afterwards.

Checkpoint: the blank is cut and clean, and its size and thickness are recorded.

S4. Fusion: import model, tools, isolation paths

Start: S1 (and the thickness from S3, needed in S5). Time: 20 minutes.

1. Model: upload fusion/cloudline_pcb_MILL_copper_up.step and open it. Check that the board's corner is at the origin and the copper is on top. The Nano's row of pads is near the right edge.

2. Tool library:

   1. In Manufacture → Tool Library, right-click a local library folder and choose Import tool libraries…, then pick fusion/cloudline_pcb_tools.json.
   2. Open each tool and set its number to its slot in your changer.
   3. If your V-bit isn't 30° with a 0.1 mm tip, or your outline end mill isn't 2 mm, correct the tool's geometry here.

   For a different V-bit, also change VBIT_ANGLE / VBIT_TIP in fusion/make_fusion.py, run the script, and re-import the DXF. The isolation paths are made for a specific bit. See fusion/README.md.

   The library follows Fusion's JSON format, but it hasn't been tested in Fusion. If the import fails, create the seven tools by hand from the feeds and speeds table.

3. Isolation paths:

   1. In Design, create an offset plane 1.635 mm above the XY plane.
   2. Create a sketch on it, then use Insert → Insert DXF to bring in fusion/cloudline_pcb_MILL_copper_up.dxf, mm, at origin 0,0.
   3. The ISO_PASS1/ISO_PASS2 curves now lie on the copper surface, right on top of the model.

4. Save a version: S4 imported.

Checkpoint: the model, the 7 tools with correct numbers, and the DXF sketch at Z = 1.635 are all in one saved design.

If something goes wrong:

• The DXF lands in the wrong place: delete the sketch and redo step 3. Check that the units are mm and the plane is at 1.635.
• The tool import fails: create the tools by hand as described in step 2.

S5. Fusion: setup and operations

Start: S4, and the blank thickness from S3. Time: 45 minutes.

Setup (Manufacture → Setup → New Setup):

• Machine: your Stepcraft M.1000 definition, or a generic 3-axis mill.
• Stock: Fixed size box.
  • X × Y = blank size.
  • Z = measured thickness.
  • Model position: X offset from left 5 mm, Y offset from front 5 mm, Z offset from top 0.
• WCS: Z up. Origin Stock box point, top, front-left corner.
• Model: all bodies.

Operations, in this order, all in the one setup:

You have every drill size, so you can also use a 0.75 mm and a 1.1 mm drill for those holes. That gives a better fit, but costs two more tool changes.

The speeds and feeds come from the tool library presets. They are listed in fusion/README.md.

Save a version: S5 operations.

Checkpoint: the setup and eight operations exist, and every operation shows a generated toolpath with no warnings.

If something goes wrong:

• An operation shows an error: open it and check the tool, geometry and heights against the table.
• The stock is wrong: edit the setup. The operations regenerate on their own.

S6. Fusion: simulate and post

Start: S5. Time: 20 minutes.

1. Simulate the whole setup with stock.
   • Isolation: compare the result with fusion/isolation_preview.png. Every pad and track must be surrounded by a closed groove.
   • Drills: each one goes through the stock.
   • Outline: goes all the way round, with the 4 tabs.
   • Collisions: none, and no rapid moves through the stock.
2. Post the full program:
   1. Select the setup and choose Post Process.
   2. In the post library, search for UCCNC and choose Autodesk's UCCNC post. Units are mm.
   3. Name the file cloudline_ALL.nc.
3. Post each tool on its own, to resume from:
   • cloudline_1_iso.nc: ops 1 and 2, selected together;
   • cloudline_2_drill08.nc through cloudline_6_drill32.nc: ops 3 to 7, one file each;
   • cloudline_7_outline.nc: op 8.
4. Open cloudline_ALL.nc in a text editor and check:
   • it contains T1 M6, then T2 M6 and so on, in the order of the operations;
   • the spindle speeds are no higher than S20000.
5. Copy the 8 files to the UCCNC computer.
6. Save a version: S6 posted.

Checkpoint: the 8 .nc files are on the machine computer.

If something goes wrong: a simulation problem means going back to S5, fixing the operation, and posting again. The NC files are always re-created from the saved Fusion version.

S7. Machine: prepare, mount, zero

Start: S3 and S6. Time: 45 minutes.

1. Surface the spoilboard where the blank goes. Use a large flat end mill, about 0.2 mm deep. Vacuum up the dust.

2. Tape the blank down:

   1. Cover the whole back with thin double-sided tape. Tape only at the edges lets the middle bow up.
   2. Lay the blank square to the X axis and press it down hard, especially in the middle.

3. Zero X/Y at the blank's front-left corner. This is the WCS origin from S5. Use a pointed tool or an edge finder.

4. Zero Z on the copper at the board centre with the touch plate and T1 loaded:

   • X = 5 + 50 = 55 mm;
   • Y = 5 + 37.5 = 42.5 mm.

   Make sure your tool-changer setup measures every other tool's length relative to this zero; check the UCCNC/Stepcraft tool-length routine.

5. Flatness check (this replaces the height map):

   1. With the touch plate, probe the copper height at the four board corners: (5 + 5, 5 + 5), (95 + 5, 5 + 5), (5 + 5, 70 + 5) and (95 + 5, 70 + 5) mm.
   2. Record each height relative to the centre.
   3. All four must be within ±0.10 mm. If any is off, lift the blank, re-tape it or re-surface, and repeat from step 2.

6. Dry run:

   1. Raise the work Z by +5 mm (for example with the UCCNC Z offset).
   2. Run cloudline_ALL.nc in the air and watch the tool changes and that the paths stay over the blank.
   3. Then remove the +5 mm offset.

Checkpoint: the blank is taped flat (corner heights recorded), X/Y and Z are zeroed, and the dry run is clean. From here on, don't touch the blank or re-zero X/Y until S10 is done.

If something goes wrong:

• The flatness check fails: re-tape and re-check before cutting anything.
• The dry run hits a soft limit or looks wrong: stop. Check the WCS (S5), the X/Y zero and the post settings.

S8. Machine: isolation (T1)

Start: S7. Time: about 15 minutes running, plus inspection.

1. Run cloudline_1_iso.nc. Keep the dust extraction on.
2. Inspect before going on. Vacuum the board, then look with a loupe:
   • Every track and pad should be surrounded by a groove down to bare FR-4.
   • Copper that still bridges a groove means the cut was too shallow there.
3. If there are bridges:
   1. In Fusion, change ops 1–2's bottom offset to −0.25 mm and post cloudline_1_iso.nc again.
   2. Run it again without re-zeroing. The deeper cut follows the same paths, and the copper edges only lose about 0.04 mm.
   3. A worn V-bit tip also leaves bridges; replace the bit before you go deeper than −0.30 mm.
   4. Lone bridges can also be scraped away with a sharp knife after S10.

Checkpoint: all grooves are clean. Record the depth used.

If something goes wrong:

• The run stopped part-way: run cloudline_1_iso.nc again from the start. The finished grooves are simply cut again, which does no harm.
• X/Y zero was lost: re-find the blank's front-left corner exactly. The FIDUCIAL marks in the DXF help to check it. A shift of 0.1 mm or more will cut into tracks. If in doubt, start a new blank at S7.

S9. Machine: drilling (T2–T6)

Start: S8. Time: about 20 minutes.

1. Run cloudline_2_drill08.nc through cloudline_6_drill32.nc, in order. Alternatively, run the drill part of cloudline_ALL.nc if you are confident.
2. After each file, check that every hole of that size is drilled through (hold the board against the light only after S10).
3. Small carbide drills snap if anything wobbles. Keep the collet clean and the drill fully seated.

Checkpoint: all 99 holes are drilled.

If something goes wrong:

• A drill broke: replace it. Measure its length again with the tool-length routine. Then rerun only that size's file; holes already drilled are drilled again harmlessly.
• The stop was in the middle of a file: rerun that file.

S10. Machine: outline (T7)

Start: S9. Time: about 10 minutes.

1. Run cloudline_7_outline.nc.
2. Vacuum the dust. Lift the board out, then break or cut the 4 tabs and file the tab stubs flush.
3. Remove the tape residue with alcohol.

Checkpoint: you have a loose 100 × 75 mm board.

If something goes wrong: the run stopped, so rerun the file. Every pass repeats harmlessly, as long as the blank hasn't moved.

S11. Clean, inspect and test the bare board

Start: S10 (or a board from a board house, or etched). Time: 30 minutes.

1. Scrub the copper with the abrasive pad, then alcohol.

2. Look at every gap with the loupe, against fusion/isolation_preview.png (mill side) or fab/gerbv_copper_bottom.png.

3. Continuity test for shorts: test neighbouring pads with the meter's beep, especially the closest pairs in fusion/milling_report.txt:

   • the Nano socket rows;
   • J3 and J4;
   • U4's two rows;
   • +3V3 against SDA_3V3/SCL_3V3 near R1/R2.

   Beeping between different nets means a sliver. Cut it with a knife and test again. Test +5V to GND and +10V to GND at the end.

4. Optional: coat the copper with solder-through flux lacquer.

Checkpoint: no shorts between different nets. Record what was fixed.

S12–S17. Assembly and first power-up

Assembly follows the main README's build steps. Each README step is one session. Every one ends with its own measurements, so a mistake is caught at the step that made it. Solder on the copper side; the parts go on the side without copper. Use the printed assembly drawing (S1) for positions, because a milled board has no silkscreen.

TO-92 parts (Q1, U2): the footprint has 2.54 mm between leads. If your parts have straight 1.27 mm leads, bend the two outer leads out by about 1.3 mm.

Fan cable into J2. The terminal order is not the Molex pin order:

If the pre-connection checks (S0) asked for a change:

• M3 (no internal pull-up): fit R5. It has its place on the board.
• M4, opposite polarity:
  1. R4's +5V end is a fixed track. Cut that track at R4's lower pad (pad 2, the end away from the D9 track).
  2. Run a short wire from that pad to GND.
  3. Set FAN_PWM_INVERTED 0.
• M4b, RC filter: there's no place for it on the board. Fit the series resistor in the fan cable's PWM wire, and the capacitor across J2's PWM and GND terminals.
• M5 (more than 12 V on the tach pin): leave the fan's TACH wire out of J2.

OLED module: use nine female-female jumper wires, matched by label. J3's BAK CON PSH TRB TRA go to the module's pins of the same name; J4's SDA SCL VCC GND likewise.

Resuming assembly: the log records the last README step whose checks passed. Start at the next one. If a check fails, the fault is in what that step fitted. The README's troubleshooting table helps.

S18. Enclosure

Start: S17 passed. Time: 1 hour.

1. Choose a box whose inside is at least 115 × 90 × 35 mm. That leaves room for the box's corner screw posts and the socketed Nano (about 20 mm tall). Box makers publish drawings with inside sizes.
2. Mount the board on four M3 standoffs, about 6 mm tall, through its own holes. Use the printed assembly drawing as a drilling template for the box floor.
3. Cut an opening at the board's left edge for the Nano's USB plug, and fit a cable gland near J2 so the cable can't pull on the terminal.
4. Main README step 8.

Checkpoint: the controller is finished.

Ordering from a board house

Upload the zip and choose these options (names vary between board houses):

Tell the board house which side is which. Budget fabs often build 1-layer boards with copper, mask and legend all on one side. Paste this into the order remark (it is also FAB_NOTES.txt in the zip): "Single-sided: copper and solder mask on the BOTTOM (B_Cu.gbl, B_Mask.gbs, viewed from top, do not mirror); silkscreen on the TOP (F_Silkscreen.gto); all holes non-plated." If their online viewer shows the legend on the copper side, ask before paying.

The zip contains exactly these files:

• B_Cu.gbl, B_Mask.gbs, F_Silkscreen.gto, Edge_Cuts.gm1;
• the .drl file;
• FAB_NOTES.txt.

The Gerber and drill attributes say one copper layer and non-plated holes. KiCad's .gbrjob job file is left out of the zip, because it would describe two copper layers: KiCad keeps a top layer (F.Cu) in every design. Here that layer is marked as a jumper layer and holds nothing.

Design notes

• One copper layer, no wire links. The router in make_pcb.py works on a 0.25 mm grid in eight directions, one net at a time:

  • short, straight nets first, the power nets last;
  • it may bridge an earlier track with a wire link if it has to; with this placement it needs none.

  The placement is what makes that possible:

  • J3 sits directly above the Nano pins it connects to;
  • the I²C lines run straight from the Nano to the level shifter and on to J4;
  • the fan terminal's pin order matches where each signal goes.

• Clearance for milling. The design rule is 0.6 mm, and the router keeps tracks 0.75 mm (grid) from other copper, so at least 0.69 mm in practice. The 0.64 mm between 2.54 mm-pitch header pads is the smallest gap. It was re-routed from 0.35 mm for isolation milling, with the same placement.

• Pull-ups standing up. R1 and R2 stand vertically under the level shifter, each body over its +3V3 lead.

• Ground.

  • Only the Nano's GND pin 29 is wired; the Nano joins its two GND pins on its own board.
  • U4's GND pins are not wired at all. On the BOB-12009 they connect only to each other (SparkFun's board file); the module uses only HV and LV.

• R5 (not fitted by default) pulls the PWM line up to the fan's +10 V before F1 (J2 pin 1), as in the schematic and PINOUT.

• Pads.

  • Every pad is at least the hole + 0.9 mm, and never under 1.7 mm. The holes are unplated, so the copper ring is what holds the lead.
  • On the 2.54 mm-pitch rows that gives 1.9 mm pads, 0.64 mm apart.
  • J2's pads are 3.3 mm, so they survive the screw torque.

• Tracks: 0.8 mm for GND, +5V and the fan supply; 0.5 mm for signals; 0.8 mm from the board edge.

• Footprints come from KiCad 7's standard library, except two in cloudline.pretty:

  • SparkFun_BOB-12009, with pad positions from SparkFun's own Eagle board file;
  • PTC_Radial_P5.10mm, for the Bourns MF-R020.

  The ceramic capacitors need 5 mm lead pitch (TDK FG28 series in ../bom.csv).

Which copy is master

The KiCad project (cloudline_controller.kicad_pcb, made by make_pcb.py) is the master. fab/, fusion/ and eagle/ are all generated from it. If you edit the design in Fusion Electronics (S2), that copy becomes your master for your boards: machine it from Fusion. The files here won't follow your edits.

Verification

Not verified:

• Nothing has been manufactured, milled or assembled.
• Nothing has been opened in Fusion 360: STEP, DXF, tool library, EAGLE files, or the posted UCCNC code.
• The mechanical fit against real parts. Check these on the first board:
  • the BOB-12009;
  • the capacitor lead pitch;
  • the TO-92 bend;
  • the screw terminal's wire-entry direction;
  • the Nano's USB plug at the board edge.

Full test output: VERIFICATION.md §8.5–8.5c.

Regenerating

sudo apt install kicad kicad-footprints gerbv librsvg2-bin poppler-utils   # KiCad 7
pip install shapely ezdxf build123d matplotlib lxml

python3 hardware/pcb/make_pcb.py                  # placement + routing -> .kicad_pcb
python3 hardware/pcb/make_fab.py                  # DRC + netlist checks, fab/ package
python3 hardware/pcb/fusion/make_fusion.py        # milling STEP/DXF/report (stops if isolation fails)
python3 hardware/pcb/fusion/make_tool_library.py  # Fusion tool library
python3 hardware/pcb/fusion/check_fusion.py
python3 hardware/pcb/eagle/make_eagle.py          # Fusion Electronics .sch/.brd
python3 hardware/pcb/eagle/check_eagle.py

Routing is deterministic: the same script produces the same tracks.

• To change the placement, edit PARTS in make_pcb.py.
• To change the routing order, edit ROUTE_ORDER.
• To change the clearance, edit CLEAR / ROUTE_CLEAR.