PCB layout New
Design Variants
One board design often makes more than one product: a Lite build without the radio, a HighGain build with a different feedback resistor, a build for a customer who buys one part themselves. A design variant says what changes for that build — and only that.
For each part, a variant can say:
| Meaning | |
|---|---|
| Fitted off | Not fitted in this build (DNP). It stays in the BOM, marked DNP, and in the position file — as KiCad's outputs do. |
| In BOM off | Not bought for this build: left out of the BOM. |
| Placed off | Left out of the position (pick-and-place) files. |
| Value | The part's value in this build (22k instead of 10k). |
A part a variant says nothing about is as drawn. The default variant is the design as drawn.
Set up variants#
Tools ▸ Design Variants opens the variant window.
- Variants lists the project's variants. Type a name and Add; edit the description in place; Rename or remove one (removing it removes what it did to every part). The Active column picks the variant the outputs build by default.
- Parts in … lists the parts of the open sheets (or of the board when no sheet is open) for the variant selected above: tick off Fitted, In BOM or Placed, or type the part's value in that variant. Open the project's sheets opens them when none are.
A change goes to every open sheet and board that holds the part, so the schematic and the board always agree. Update PCB from schematic also carries each part's variants to its footprint.
Build a variant#
In File ▸ Export ▸ Fabrication Outputs, the Board card has a Variant list when the design has variants. Pick one and generate: the pick-and-place file, the BOM (flat and grouped), the assembly drawing, IPC-2581, ODB++ and the X2 component files describe that build. The package's README.txt starts with the variant it is for, and switching variants marks a generated package out of date, so a package for one build is never saved as another.
The outputs agree with KiCad's: on a test design checked with kicad-cli sch export bom --variant and kicad-cli pcb export pos --variant, WireFrame's BOM and position files list the same parts with the same values for every variant.
KiCad and Altium#
| KiCad 10 | Altium Designer | |
|---|---|---|
| The list | schematic.variants in the .kicad_pro, (variants …) in the board |
[ProjectVariantN] in the .PrjPcb (the description is the name) |
| Per part | (variant …) in each symbol instance and each footprint |
VariationN — Not Fitted for a part left off |
| Read and written | all of it | Not Fitted, alternate-part values; the BOM, position-file and value changes Altium has no field for go under WireFrame's own keys |
Import a KiCad 10 or Altium project with variants and they are there; export and they go back out. Both directions are part of the round-trip check.