PCB Design Tools in 2024: Why Altium Is the Industry Standard and Why KiCad Caught Up

Introduction

The choice of an electronic computer-aided design (ECAD) tool is rarely a purely technical decision. It is bound up with licensing cost, team collaboration, library management, and — often underestimated — the quality of the data the tool emits for manufacturing. For most of the last two decades the high end of this market has been defined by a handful of proprietary suites, while free options were treated as adequate only for hobby work. That framing no longer holds. KiCad has reached a level where it appears on production designs, and the commercial vendors have responded by competing on cloud collaboration and high-speed design features rather than on raw layout capability alone. At the same time, the manufacturing interface — the set of files a fabricator actually consumes — has been quietly modernizing, which changes how much the native tool format matters at all.

The Professional Suites and Why Altium Sits at the Center

Altium Designer occupies an unusual position: it is not the most expensive tool, nor the strongest for the most extreme high-speed designs, yet it is the one most often cited as the industry reference. Several structural reasons explain this.

The first is the unified environment. Schematic capture, layout, library management, bill-of-materials (BOM) handling, and manufacturing documentation live in one application with one data model, rather than being stitched together from separate programs. This reduces the integration friction that historically characterized competitors. The second is ecosystem breadth: managed component libraries, supplier data, and the Altium 365 cloud platform for version control and design-review collaboration. The third is the documentation toolset — Altium's Draftsman feature produces assembly drawings, fabrication notes, and dimensioned views directly from the board, which matters because production handoff quality is often where weaker tools fall down.

There is also a market-signal dimension. The early-2024 announcement that Renesas, a major semiconductor manufacturer, intended to acquire Altium (a transaction reported at roughly USD 5.9 billion and, as of mid-2024, pending completion) underlines how strategically valuable a dominant design-tool position is judged to be. Whatever the long-term product implications, it reinforces Altium's standard-bearer status.

Above Altium in raw capability sit the genuinely high-end suites. Cadence (the OrCAD X front end with the Allegro engine) and Siemens EDA (PADS in the mid-range, Xpedition at the top) lead on signal integrity (SI) analysis — the modeling of how fast signals degrade on real traces — and on very large, dense designs. These tools are common in telecom, server, and advanced packaging work, but their licensing cost and learning curve place them outside the reach of most small teams.

The licensing models differ meaningfully:

• Altium Designer: proprietary; historically a perpetual license plus a paid annual subscription for updates, with term-subscription options. Per-seat cost is in the five-figure range.
• Cadence / Siemens (Xpedition): proprietary subscription, premium tier; typically the most expensive options on a per-seat basis.
• Autodesk Fusion Electronics (the successor to EAGLE): subscription only — the standalone perpetual EAGLE line is being wound down and folded into Fusion — at a comparatively low price point, with capability limits on lower tiers.

KiCad: What Is Actually Driving the Acceleration

KiCad is free and open-source software released under the GPL, cross-platform, and — importantly for professional use — imposes no limits on board size, layer count, or commercial use. Its progress from "usable for simple boards" to "credible for production" did not happen by accident; it has identifiable causes.

The most consequential was sustained engineering funding from outside the volunteer community. CERN contributed the interactive routing engine — including the push-and-shove router (which lets traces displace existing ones rather than blocking), differential-pair routing, and length tuning for matched timing — features that were previously a clear separator between free and commercial tools. The second driver is corporate sponsorship: Digi-Key and other industry players fund development directly, and distribution-and-fabrication businesses have a commercial incentive to lower the barrier to designing boards that they then sell parts for or manufacture. The third is the architectural reset in KiCad 6 (a new, text-based S-expression file format and a rewritten design-rule-check engine) which created a stable foundation. KiCad 7 (2023) and KiCad 8 (early 2024) built on it with a stronger constraint-driven design-rule system, improved high-speed routing, and better manufacturing output, including IPC-2581 export (a vendor-neutral manufacturing data format discussed below).

The honest limitations remain in SI/PI (signal- and power-integrity) analysis and in the depth of managed library/lifecycle tooling, where the commercial suites still lead. But for a large class of designs — embedded controller boards, FPGA carrier and breakout boards, mixed-signal instrumentation — the capability gap is now narrow enough that licensing cost, not capability, often decides.

The Practical Middle and Web-Native Tools

Two further options matter for the cross-domain reader. EasyEDA is a browser-based tool with a free Standard edition and a low-cost Pro subscription; its defining trait is tight coupling to the JLCPCB/LCSC manufacturing-and-parts ecosystem, which makes it fast for getting a simple board ordered. DipTrace is an affordable proprietary tool with perpetual, tiered licensing (priced by pin and layer limits) and a gentle learning curve, popular with small firms and educators.

The Fabrication Hand-off: Why Native Files Usually Do Not Travel

A point often missed when comparing tools is that fabricators rarely consume native design files. The board house works from a manufacturing dataset, and the dominant exchange formats are tool-independent:

• Gerber (RS-274X / X2 / X3): the long-standing standard for copper, mask, and silkscreen layers. X2 adds attributes (machine-readable metadata identifying each layer's function), and X3 carries component placement data. Maintained by Ucamco.
• Excellon: the NC drill file describing hole positions and sizes.
• IPC-2581: an open, vendor-neutral single-file format carrying the full intelligent dataset — layers, stackup, netlist, BOM, and placement together. Promoted as a neutral alternative to proprietary formats.
• ODB++: a mature, widely accepted single-database format originated by Valor and now controlled by Siemens. Technically rich, but its governance sits with one EDA vendor.
• IPC-D-356A netlist for bare-board electrical test, and a pick-and-place (centroid) file plus BOM for assembly.

Because of this, the relevant question is not "does my fabricator accept Altium files?" but "does my tool emit clean, complete Gerber X2/X3 (or IPC-2581/ODB++) with correct drill and assembly data?" All the serious tools do. Altium, Cadence, and Siemens export Gerber, ODB++, and IPC-2581; KiCad exports Gerber X2/X3, Excellon, IPC-D-356, and IPC-2581 (from v7 onward) but has no native ODB++ output — a gap that matters only for fabs that specifically require it.

Native-file acceptance is a real but narrower phenomenon, concentrated among prototype-friendly fabricators. OSH Park and Aisler accept native KiCad and EAGLE board files directly (Aisler also takes Fusion and some other native formats), absorbing the export step for the user. JLCPCB is Gerber-driven but integrates natively with EasyEDA and pairs the board with a BOM and component-placement-list (CPL) for assembly. PCBWay publishes plug-ins that push designs from Altium, EAGLE, and KiCad and is itself a KiCad sponsor. Higher-end and aerospace-grade fabricators tend to prefer ODB++ or IPC-2581 precisely because those formats reduce the manual interpretation that plain Gerbers can require.

Where a workflow leans on scripting, KiCad's Python interface (pcbnew) is illustrative of how reproducible output generation looks in practice:

# KiCad 8 / pcbnew — minimal scripted fabrication-output generation
# Method names follow the pcbnew Python API; intended as an illustrative pattern.
import pcbnew

board = pcbnew.LoadBoard("controller_board.kicad_pcb")
plotter = pcbnew.PLOT_CONTROLLER(board)
opts = plotter.GetPlotOptions()

opts.SetOutputDirectory("fab/")          # keep generated data out of the source tree
opts.SetUseGerberX2format(True)          # emit X2 attributes, not legacy RS-274X only
opts.SetCreateGerberJobFile(True)        # .gbrjob ties the layer set together for the fab
opts.SetSubtractMaskFromSilk(True)       # avoid silkscreen printed over exposed pads

# A real script then iterates the required layers (copper, mask, silk, edge cuts),
# calling SetLayer()/OpenPlotfile()/PlotLayer() per layer, and generates the
# Excellon drill set separately. Full examples are published in the KiCad docs.
plotter.ClosePlot()

The value here is not the specific calls but the principle: scripted, version-controlled output removes the human variability that causes most re-spins at the fabricator.

Recommendation Summary

Conclusion

The defensible reading of the 2024 landscape is that tool choice now hinges on team scale, design class, and budget more than on whether a free tool can physically produce a manufacturable board.

Altium remains the reasonable default for professional teams that need a single integrated environment, managed libraries, cloud collaboration, and first-class documentation — and that can absorb the licensing cost. The Cadence and Siemens high-end suites are justified specifically when signal-integrity analysis and very large, dense, or high-speed designs dominate the requirements; outside that envelope their cost is hard to justify. KiCad has become the appropriate choice for individuals, labs, startups, and even production work on embedded, FPGA-carrier, and mixed-signal boards where extreme SI tooling is not the gating concern — its no-cost, no-restriction model and scripting support are decisive advantages, with the caveat that SI/PI analysis and lifecycle/library management still favor the commercial suites. EasyEDA fits fast, simple boards bound for JLCPCB; DipTrace suits small teams wanting a low-cost perpetual license.

On manufacturing, the practical conclusion is that the export pipeline matters more than the native format. Because fabricators standardize on Gerber X2/X3, IPC-2581, and ODB++, any of these tools can hand off cleanly when its output is configured correctly — and native-file acceptance, while convenient at prototype-oriented fabs, is not a real constraint on tool selection for production work.

References / Further Reading

1. Ucamco, The Gerber Layer Format Specification (current revision), Ucamco, Ghent, Belgium.
2. IPC, IPC-2581: Generic Requirements for Printed Board Assembly Products Manufacturing Description Data and Transfer Methodology, IPC International, Bannockburn, IL.
3. IPC, IPC-D-356A: Bare Substrate Electrical Test Data Format, IPC International, Bannockburn, IL.
4. KiCad Project, KiCad Documentation (Schematic, PCB Editor, and Python pcbnew scripting), kicad.org.
5. Altium, Altium Designer Documentation (Draftsman, Output Job, and Altium 365), Altium LLC.