Build a small RC low-pass filter in the Trace app, from a plan in the chat to a routed, checked board and the files a manufacturer needs. The assistant does most of the work, and you check each step.
What We're Building
- R1: 1 kΩ resistor, 0805.
- C1: 100 nF capacitor from the output to ground, 0805, rated 10 V or more.
- J1 and J2: two-pin 2.54 mm headers. Pin 1 is the signal, pin 2 is ground.
- Board: 30 mm × 20 mm, two layers.
Here, 0805 means the imperial size (metric 2012), about 2.0 mm × 1.25 mm.
The signal comes from an outside source and goes to an outside load of 1 MΩ; there is no supply on the board. The cutoff frequency is fc = 1 / (2πRC) ≈ 1.59 kHz.
Before You Start
- Install the Trace app and sign in. See Installation.
- The steps work in both layouts. Buttons named here, such as ERC, DRC and Chat, are on the Simple layout's action bar; menus such as Tools show in the Full layout (Preferences > Interface > Layout), and on a Mac the menu bar is always there.
Step 1: Create a New Project
On the start page, press New project, name it RC-Filter and choose a folder. Open the schematic from the project tree. If you did the Quick Start, you can carry on with that project.
Step 2: Describe Your Circuit
Press Chat, pick a model, and choose Plan mode. Send:
Plan a passive RC low-pass filter on a 30 mm x 20 mm two-layer board.
R1 is 1 kΩ and C1 is 100 nF, both 0805.
Use two-pin 2.54 mm headers for J1 (input) and J2 (output).
J1 pin 1 is IN; J1 pin 2 is GND.
R1 connects IN to OUT. C1 connects OUT to GND.
J2 pin 1 is OUT; J2 pin 2 is GND.
The signal source and the 1 MΩ load are outside the board.
No supply, microcontroller or amplifier on the board.
Plan the schematic and footprints only. Don't lay out the board yet.
If you are continuing from the Quick Start, ask the assistant to review the existing schematic against this list instead.
Step 3: Review the Plan
Read the plan: the parts, values, packages and connections. Answer any questions the assistant asks. Then press Approve to let it draw the schematic, or Adjust Plan to change something first.
Step 4: Check the Schematic
When the assistant finishes, look at the sheet:
- IN connects R1 and J1 pin 1.
- OUT connects R1, C1 and J2 pin 1.
- GND connects C1 and pin 2 of both headers.
- Values, references and footprints match the plan.
Save, then press ERC and Run ERC. Click any finding to jump to it. Don't add a power source just to quiet a warning; ask the assistant what a finding means if you're unsure.
Step 5: Simulate the Filter (Optional)
Ask the assistant:
Simulate the AC response from 10 Hz to 100 kHz with a 1 V source on J1
and a 1 MΩ load on J2. Where is the -3 dB point?
It should come back close to 1.59 kHz. Press the result card to see the plot in the Simulation tab. See Simulation.
Step 6: Set Up the Board
- Ask the assistant: "Update the board from the schematic." Or open the board and use Tools > Update PCB from Schematic (
F8). You should see four footprints. - Pick your manufacturer, so DRC checks against their limits: ask "Use the JLCPCB rules for this board", or choose one in the Preferred Manufacturer list on the board editor's toolbar (Full layout).
- Ask for the outline: "Make the board outline 30 x 20 mm with two copper layers." Or draw a rectangle on the Edge.Cuts layer yourself.
- Check that the outline is one closed shape and the size is right.
Step 7: Place Components
Place J1 and J2 where cables can reach them, R1 between them and C1 close to J2 with a short path to ground.
- By hand: select a part, press
Mto move it andRto rotate it. - With the assistant: "Put J1 on the left edge and J2 on the right edge, R1 between them and C1 next to J2."
On bigger boards, advanced placement and routing can place parts for you.
Step 8: Route Traces
Route IN, OUT and GND.
- With basic routing (free): ask "Route this board with basic routing". Check the settings on the Basic routing card and press Route board. New traces appear as it works.
- By hand: press Route (
X), click a pad, click to place each corner and finish on the matching pad. PressEscto stop.
Ground must join both headers and C1, by traces or a filled copper zone.
Step 9: Run DRC
Save the board. Press DRC, keep Refill all zones before performing DRC ticked, and press Run DRC. Click each finding to jump to it, fix it, and run DRC again until it is clean.
Then press 3D and look the board over: connector pin 1 on the signal, parts the right way round, readable silkscreen.
Step 10: Export for Manufacturing
Ask the assistant for "Gerber and drill files", or follow Exporting Designs. The files go to your project folder, or the folder you name. You can also send the board straight to a manufacturer; see One-Click Manufacturing.
Open the Gerbers in a viewer and check the outline, copper, drill holes and size before you order.
Next: A Case for Your Board
Ask the assistant to "design a 3D-printed case for this board" and Trace Mechanical builds one around it, with openings for J1 and J2.
If Something Goes Wrong
- Stop in the chat stops the assistant; it does not undo what it already changed. Use Undo for that.
- Before you repeat a request, look at the design to see what already changed.
- To go back further, use Version History.