Exporting to Other Tools

A design that works on the desk is often only the beginning. You might want to turn it into a real circuit board, or keep simulating it somewhere else. Desktop ▸ Export To writes the desktop on screen in another program's format. You can also right-click any desktop's tab and choose Export To to export that desktop. There are two formats, one for each of those jobs:

• KiCad Project… writes a project for KiCad, the free schematic and circuit-board program. Use it to go from breadboard to PCB.
• Digital Circuit… writes a circuit for Digital, a free logic simulator with its own 74xx library. Use it to keep simulating the design with the same chips.

Exporting only reads the desktop, so you can do it while the circuit is running. It never changes your design, and the exported files keep no link to it. Export again whenever the design changes.

The export report

Some things on a breadboard have no exact equivalent in the other program. If anything won't come across as it is, Chip Hippo tells you before writing a single file:

• Won't come across: parts the other program has nothing for. Everything wired to them is still exported, and their nets keep their names.
• Changes: parts that are exported as something that behaves a little differently. For example, a push button becomes a toggle switch in Digital.
• Footprints to check: KiCad parts that got a stand-in footprint (see below). Choose the real one before laying out a board.

Parts are listed by the same names the exported file uses (U7, R1–R3). Choose Export… to go ahead, or Cancel to write nothing. If nothing changes in the export, the report is skipped and you go straight to choosing where to save.

Part names and net names

A schematic names every part with a letter and a number, so the export gives each part one:

Parts are numbered in the order you placed them, so the same desktop always exports with the same names. To choose a part's name yourself, set its Name to a designator of the right kind (U5, R12) in Properties…, and the export keeps it.

Nets are named the same way in both formats:

• a net you named yourself keeps its name (see Probing & Net Names);
• a wire in a bus is named after the bus and its bit, so bus D[7:0] gives D0…D7;
• the supply rails are +5V (or +3V, +12V) and GND;
• every other net is numbered N1, N2, … in reading order.

Characters the other programs can't use in a net name become _. A name marked active-low with a leading /, ~ or ! gets an n prefix instead, so /CLR exports as nCLR.

KiCad

Export To ▸ KiCad Project… asks for a folder, not a file name. A KiCad project is several files that belong together, so choose (or create) a folder for it. Chip Hippo writes four files there, named after the desktop:

• <desktop>.kicad_pro, the project itself. Open this one in KiCad.
• <desktop>.kicad_sch, the schematic.
• chiphippo.kicad_sym, the symbols for the parts on it.
• sym-lib-table, which tells KiCad where those symbols are, so the project opens anywhere without any setup.

The files are written in KiCad 8's format, so KiCad 8 and every later version can open them.

What the schematic looks like

Parts are laid out in the same arrangement as the Schematic View, including any symbols you moved there. Each chip is one symbol with every pin in its physical numbering, the way it sits on the breadboard. (KiCad's own library draws a 74xx chip as a set of separate gates.) Inputs are on the left, outputs on the right, and power on the top and bottom.

Pins are connected by net labels rather than drawn wires: each connected pin has a short stub ending in its net's name, and KiCad joins every label with the same name. The supply rails use power symbols, with one PWR_FLAG on each rail a power supply (or a regulator) feeds, so KiCad's electrical rules check knows they are supplied — a rail nothing feeds gets none, so the check points out the chips on it. A desk too wide for KiCad's largest sheet (about 3 m) is wrapped onto it in bands. A pin that isn't connected to anything gets a no-connect flag. The sheet passes KiCad's electrical rules check with nothing to report.

From schematic to circuit board

Every part is given a footprint from KiCad's standard libraries:

• Chips get Package_DIP footprints at their real width: 300 mil for logic, 600 mil for the wide memory chips and processors. A chip you designed yourself in a size KiCad's library has no plain DIP for (a 26-pin, or a wide 14-pin) is listed under footprints to check.
• Resistors, LEDs, switches, DIP switch banks, resistor networks, oscillator cans and the 16×2 LCD each get their matching standard footprint.
• Capacitors come across with their value (100nF, 4.7uF) as their KiCad Value, drawn the way KiCad draws them — the plain capacitor for a ceramic, the polarised one for an electrolytic, whose + is pin 1 — on a 5 mm ceramic disc or a 5 mm radial electrolytic footprint. Resistors carry their value the same way (4.7k). Every value keeps the figures the part's Properties… card shows, written in plain ASCII — u for µ, and no Ω — as SPICE and BOM tools expect. On the breadboard a capacitor connects nothing; in KiCad it is wired where it sits, which is the point of exporting it.
• Diodes, inductors and transistors come across as KiCad's own shapes — the diode, the Zener (its bar bent), the inductor's coil, and the NPN, PNP and N- and P-channel MOSFET symbols. A diode or a transistor's Value is its part number (1N4148, 2N2222), or the plain type (D, NPN) until it has one; a Zener adds its voltage (1N4733A 5.1V); an inductor's is its inductance (10uH). Any part number also rides along as an MPN field for KiCad's BOM tools. Diodes get a DO-35 footprint on 7.62 mm, its pad 1 the cathode.
• A bridge rectifier is drawn as the diamond of four diodes, + at the top and − at the bottom, its Value its part number (DB105). It gets KiCad's own bridge DIP (Diode_Bridge_DIP-4_W7.62mm_P5.08mm), pads numbered as its pins are: 1 +, 2 −, 3 and 4 the AC pins.
• An inductor's footprint is the part its Style says, on the pitch its Holes between leads says: a Coil is a standing toroid, on exactly 5.08, 7.62 or 10.16 mm; a Can is a radial drum, and KiCad's round radial inductors are on metric pitches, so it gets the nearest (5.00, 7.00 or 10.00 mm) and the report lists it under footprints to check.
• Transistors get a TO-92 footprint on 2.54 mm — or, for a MOSFET whose Package is TO-220, a standing TO-220 — its pads numbered in the order the desk prints the pins (E B C, S G D). That is no one maker's pinout, so the report lists every transistor under footprints to check: make sure the pads match the real part's datasheet before laying out.
• The tactile button gets KiCad's own 6 mm tactile footprint (SW_PUSH_6mm), with the two legs of each side on the same pad number, because they are one contact in the switch. The DPDT push switch gets the nearest DPDT push switch KiCad's library has (C&K PVA2, two rows of three on 2.5 mm), and the report lists it under footprints to check.
• The power supply and the clock source become pin headers labelled POWER (two pins) and CLOCK IN (three: the clock, its supply and its ground). That's where power and a clock come in on a real board. The clock needs an oscillator in its place, which the report points out.
• The 7-segment digits, the 8-segment bar graph, the 20×4 LCD and the latching push button get a stand-in footprint (a pin header or a tactile button of the right size). Chip Hippo's versions of these are idealized parts, with no single real part to match. Choose the real part's footprint before laying out the board.

With the project open in KiCad, Tools ▸ Update PCB from Schematic in the PCB editor brings every footprint onto the board, connected.

Exporting again

To update an exported project after changing the design, export into the same folder. Chip Hippo rewrites the schematic and its symbol library, but leaves your .kicad_pro and any board you've laid out alone. Every part keeps the same identity from one export to the next, so Update PCB from Schematic only adds, removes and rewires what actually changed, and the parts you've already placed stay put.

Chip Hippo never overwrites a schematic that some other program wrote. If the folder already holds a .kicad_sch of that name from somewhere else, the export stops and changes nothing. Choose an empty folder instead. (A schematic Chip Hippo exported is still recognised after KiCad has saved it, by the "Exported from Chip Hippo" line in its title block — leave that line in.)

What isn't exported

Breadboards and jumper wires don't appear as parts: they become the connections between the parts. External signals and Arduino Output and Input elements are stimulus for the bench, not parts, so they are left out (the report lists them). Notes and labels are left out too, and so is the electronic load, a bench instrument; the report names it. A pin left alone on its net once the load is gone (a resistor's lead that only met the load) is marked as a no-connect. Mains becomes a two-pin AC IN header, as the power supply becomes a power header, the transformer a four-pin header standing in for its leads (P1, P2, S1, S2), and the AC adapter a two-pin header for its output (S1, S2).

Digital

Export To ▸ Digital Circuit… writes one .dig file. Open it in Digital with File ▸ Open.

The chips are Digital's own: its library models most of the 74xx family as DIL packages, pinned exactly like the real parts. It has no CD4000 folder, but six CD4000 parts have a pin-for-pin twin there, and the export uses it:

Chip Hippo places each chip and connects its pins through tunnels named after their nets, which Digital joins the way KiCad joins labels. Switches, LEDs, bar graphs, 7-segment digits, clock sources, oscillator cans and the power supply each become the matching Digital element. The switches start in the position they're in on the desk. External signals become Digital buttons (momentary) or inputs (toggle), labelled with their names.

These exports have been run in Digital itself and checked against Chip Hippo's own simulation. For the example circuits, every chip output and every lamp reads the same in both, at a range of switch settings.

What changes

Digital is a logic simulator, so some parts have to be exported as what they mean rather than what they are:

• Resistors are exported as what they do in the logic. A resistor to a supply rail becomes a pull-up or pull-down on the net at its other end, which is what a lamp's current-limiting resistor and a switch's pull-down amount to. A resistor between two signals becomes a plain wire (the report lists it). A resistor from rail to rail does nothing in logic and is left out. A divider — a potentiometer's wiper, or two resistors from one net to both rails — keeps only the side that decides it, as Chip Hippo reads it (two thirds of the pull or more); Digital won't run a net with both a pull-up and a pull-down. A divider near the middle, which Chip Hippo reads as unknown, gets neither, and the report says so.
• Lamps nothing drives: when an LED's or display's driver doesn't come across (a chip Digital has no model of, below), the lamp is tied dark, since Digital won't run a file with a lamp that nothing drives. The report lists the lamps.
• Clock rates are whole hertz in Digital, so a fractional rate (2.5 Hz) comes across as the nearest whole one, and the report says so.
• Floating inputs: an unconnected TTL input reads HIGH. Digital treats an undriven input as an error, so the export adds the pull-up that makes it HIGH in Digital too. It doesn't add one where a resistor already sets the level. An unconnected CMOS input gets the same pull-up, but there it changes the answer: Chip Hippo reads a floating CMOS input as unknown, and Digital has no unknown to give it. The report names each CD4000 chip this happens to.
• Open-collector chips (74LS01, 74LS03, 74LS05) get a pull-up on each output. Chip Hippo simulates their outputs driving both ways, but Digital simulates them as the real parts, which only pull low. The pull-up makes the two behave the same, as it would on a real board.
• Push buttons (and tactile buttons) become toggle switches, because Digital has no momentary switch contact.
• A DPDT push switch becomes two changeover switches, one per pole. Click each one in Digital to change it.
• Unpowered chips are powered, because Digital can't simulate a chip with its supply pins unconnected — and Digital powers every rail it's given, so a chip on rails that no power supply reaches runs there too. Either way the report lists the chip as unpowered, since it does nothing in Chip Hippo.

What doesn't come across

• Eight 74xx parts that Digital's library doesn't include: 74LS73, 74LS75, 74LS92, 74LS169, 74LS240, 74LS259, 74LS279 and 74LS533. Each one's place in the circuit is marked with a note, and everything wired to it is still exported.
• The other 40 CD4000 CMOS parts, which have no twin in Digital's library. The same note marks each one's place.
• The 555 timer, which Digital's library doesn't have either.
• Capacitors. A capacitor connects nothing in Chip Hippo, so leaving it out changes nothing about the circuit.
• Diodes (a bridge rectifier's four too) and transistors: Digital has none that pass a level one way, or switch, the way Chip Hippo's do.
• Inductors. An inductor is a wire in Chip Hippo, so the two nets it joins come across apart — the report says so; join them in Digital if you need them joined.
• Memory chips, because their contents are stored in files the export doesn't carry.
• The processors and their peripheral chips (W65C02, Z80, W65C21, W65C22).
• The character LCD modules.
• Arduino Output and Input elements.

Digital needs its own library to find the chips. It comes in the lib folder of the Digital download, which has to stay beside Digital.jar. If a chip shows up as missing, check that folder and Digital's library settings.