The Schematic Editor

Where a circuit is drawn: placing components from the Library Palette, wiring them, editing their values, and setting up the analysis that simulates the result.

The schematic is the electrical view of a cell — what the circuit is, as opposed to what it looks like on a symbol or what gets manufactured in a layout. It is the view you spend most of your time in, and it is the only one an analysis runs on.

Orientation

A schematic is a view of a cell, exactly as its symbol and its layout are; the cell folder holds schematic/, symbol/ and layout/ side by side and a cell need not have all three. Opening one opens a document tab.

You do not need a cell library to start. With no workspace open, File ▸ New Schematic opens a standalone scratch sheet you can wire up and simulate immediately, and save into a workspace later if it turns out to be worth keeping. With a workspace open, New Schematic and New Layout create a new cell holding that view instead, so nothing lands outside a cell.

Two things about the canvas are worth knowing before you draw on it:

• Connection is exact, not proximity. Every pin, wire vertex and junction lands on the coarse connection grid, and two things are joined only when they occupy the same grid point. A second, finer authoring grid positions labels and annotations. That rule, and what happens when you paste between designs with different grids, is Grid & Connectivity.
• Standard-library parts are drawn vertically. R, L, C, the sources, Term and Ground all put port 1 at the top and port 2 at the bottom, so a horizontal signal path means rotating them as you place them. That is the normal workflow, not a workaround — see Orientation convention.

The Library Palette

The palette is where every placeable part lives. It has two controls above the tiles and they do different jobs:

• The Type menu. The button shows what is selected, as a path such as Library ▸ Capacitors ▸ Series; in a narrow panel the leading levels give way to …. Clicking it opens a menu. All is the default and shows the whole built-in library in the palette's own pinned order — the parts you reach for most, first. All - Alphabetical is the same set sorted by name, Common is a short curated set, and Recently Used is what you have placed lately, vendor library parts included. Below those come the built-in categories — Lumped, Devices, System, Nonlinear, Sources, Terminals, Transmission Line, Microstrip, Matching, Data Files. Then come one sub-menu per imported kit holding the kit's own groupings, one sub-menu per vendor part library following the library's own folders, and Add Vendor Library…. Every sub-menu starts with All in …, so a folder can be chosen as well as opened, and a folder holding only one thing is shown as that thing (Inductors ▸ Series). A library's files show how many parts each holds. See PDK integration for where kit entries come from.

  System sits directly after Devices, because a system block is a signal-path part and a user who has found Devices is one row away from the blocks they want. It holds the ideal blocks a system block diagram is drawn out of — circulator, coupler, hybrid, balun, switch, amplifier, attenuator, filter, duplexer — plus the two mixer tiles, which keep Devices as their primary category and appear under both. See System Components.

• The search box. Matches a part's display name and its search terms, and a kit part's kit name as well. Searching inside a built-in category narrows within it; searching from All searches everything, built-ins and kits together. From All, a vendor library with matching parts adds one row at the top — 312 parts in Caps match — which opens that library with the search kept.

The tile grid is a reflow grid: the number of columns follows the panel's width, so widening the palette gets you more tiles per row rather than bigger tiles.

A vendor library's parts

Choosing a vendor library, or a folder or file inside it, replaces the tiles with a list of parts. Each row shows the part number and its value, then its description and frequency range. The list is sorted by value. Click Part, Value, Description or Range above it to sort by that, and click again to reverse.

The search box filters the list. Separate words with spaces; every word must match, in any order. A word matches when it appears in the part number, the description (with or without its brackets, so 50V finds 50[V]), the file or the folder name. Two kinds of word are read more exactly:

• A value — 10p, 10pF, 2.2n, 4n7 — finds the part whose stated value is that, however the library wrote it, and 10 pF with a space is the same word. A unit, when you give one, must match the part: 10nH finds inductors only.
• A case size — 0603 — is the imperial size the library states, and 1608M the metric one. The library writes both (1608M(0603)), and 0603 never finds a 0201 part through its metric 0603M.

So 0603 10pF C0G 100V narrows a library to the parts you want. Typing never waits on the disk; while a library is still being read after the workspace opens, the list says Indexing … instead.

↓ and ↑, from the search box or the list, arm the next or previous part, so you can type, step to the part and click on the schematic without touching the list. The ? button at the end of the column headers opens the documents the library came with (each in your system's own viewer), then circuitRF's help on vendor libraries.

A row places a part exactly as a tile does: click to arm, or drag onto the schematic. The part is a SPICE Model running from the library's own file. A capacitor or inductor draws as the ordinary C or L symbol, is named C1, L1, …, and is labelled with its part number, its name and, on a line of its own, its value (C = 10 pF). It arrives with the footprint of the case size its library states, also in a workspace that has no technology yet.

A library can also hold model folders, listed in the same rows. The search, sort and ? button work as they do for SPICE parts, and a model's ? opens the documents in its own docs/ folder. In the Type menu, a folder of models is one entry that lists them all. A model places as a cell: it draws the glyph its part.cpart names (R, C, L or a transistor, with the transistor's pins matched to the model's pin names), or the model's own symbol when it names none. It is named R1, C1, L1 or Q1 for those glyphs, and arrives with the model's parameters at their defaults. If the library goes missing, the part keeps drawing its glyph with the not-found mark.

Placing a component

There are two gestures, and they place the identical thing — a kit part in particular resolves through the same path either way, so a drag and a click can never disagree about what you get.

1. Click a tile to arm it. The tile highlights, and a ghost of the symbol follows the cursor over the canvas. Click on the canvas to drop one. The tool stays armed, so click again to place another — this is the fast way to lay down five capacitors. Click the tile a second time, or press Esc, to disarm.
2. Or drag the tile onto the canvas. The ghost follows the drag, snapped to the connection grid, and the component lands where you release. A drag places exactly one part and leaves nothing armed, which is what you want when you are placing one part in the middle of doing something else.

While a placement is armed, R rotates the ghost 90° counter-clockwise and Shift+R clockwise, M mirrors it left to right and Shift+M top to bottom — the same keys that rotate and mirror a selection when nothing is armed. The part lands the way the ghost faces, so an IProbe dropped onto a wire already points its arrow the way you want the current measured.

Dropping a part along a wire puts it in series. When two of its pins land on one straight stretch of wire, the wire between them is removed, so the part breaks into the run instead of being shorted by it. That holds for a two-pin part, for an MTEE whose pins 1 and 2 lie along the wire (pin 3 is left for you to wire) and for an MCROSS along the wire between its two pins on it. Nothing is cut when anything else meets the wire between the pins — a junction, another wire, another part's pin, a net label — or when the part's other pins also touch the wire.

Copy and paste

Ctrl+V (⌘+V on macOS) shows the copied parts as a ghost that follows the cursor, snapped to the connection grid. Click to place them there; Esc puts nothing down. Nothing connects to the ghost while it moves. Edit ▸ Paste does the same while the cursor is over the canvas; from the menu with the cursor elsewhere, the parts land in the middle of the view. A single part pasted along a wire goes in series, as a placed one does.

Parts keep their symbols when pasted into a schematic in another folder, so a part copied out of an imported schematic arrives as its own symbol rather than a box. A net label sitting on a copied pin comes with it; deleting a part takes the net label that sits on its pin, unless another pin or a wire also meets it there.

Placing the parts of a parts table

A parts list typed by hand is slow, and the one you have is usually a table in a datasheet, an application note or a spreadsheet. Copy it, click the schematic, and press Ctrl+V (⌘+V on macOS) — or drop a .csv file on the canvas. Every resistor, capacitor and inductor in it is placed, named by its reference designator, with its value and its case size as the footprint: one row of parts per type, below what is already on the sheet (or at the point where you dropped the file). It is one step on the undo stack.

What it reads, row by row:

• The reference — C4, a list (M11,M12,M16) or a range (C3-C5), one part each.
• The type — a Type or Description column (Capacitor, CAP CER …, C), otherwise the reference's own letter (C, R, L, FB), otherwise the value's unit.
• The value — 100 pF, 100pF, 4k7, or a number with its unit in the next cell.
• The case size — a Size, Case, Package or Footprint column: 0402, 402 (a spreadsheet drops the leading zero), C0805, or a series code the case table knows.

Text copied out of a PDF works too: the words of a wrapped cell (Capacito r) and a reference list that wrapped onto the next line are put back together. Rows marked DNP or -- are skipped. Anything it could not place — an IC, a ferrite bead whose value is in ohms, a row with no type — is listed in the Messages panel with the reason, and so is every reading worth checking: a bare 0402 is read as the imperial size, and says so, because the same digits are also a smaller metric part.

Wiring, values and labels

Wire is W (or the toolbar button). Click from one pin to another; Enter finishes the wire in progress and returns you to Select, Esc cancels it. Select is S, and Esc from any tool comes back to it.

Clicking a wire selects one straight run of it, not the whole wire. Where a pin, another wire, a junction dot or a net label joins that run partway along, the click selects only the stretch between the junctions on either side of it. Delete then removes that stretch, and the rest of the wire keeps every connection it had. To disconnect one branch of a supply line, click the stretch between the two parts and delete it.

Double-click does three different things depending on what is under the cursor, and the distinction is worth learning because it is the fastest edit in the application:

Hold Alt (Option on macOS) while double-clicking a wire to select the whole run of wiring instead: every wire joined to the clicked one, in every direction — round corners, through junctions, and through pins where several wires meet — until the wiring ends at the components. A part ends the run, because the wiring on its other side is a different node; a net label does not carry it to another label of the same name. Delete then removes exactly that run.

Arrow keys nudge the selection by one connection-grid step, or five with Shift held. F5 begins Move Labels, for pushing a crowded label block clear of the artwork without moving the component it belongs to.

Values are expressions, not just numbers: a VAR block on the sheet declares variables that any component value can refer to, and the same expression language drives sweeps and measurements. See Expressions and Measurements.

The context menu

Right-clicking a component gives you the operations that apply to it: Edit Parameters, rotate and mirror, the two label commands, Labels ▸ for choosing which parameters show on the sheet, Disconnect, Copy and Delete. Items are disabled rather than hidden, so their positions stay put and you learn the menu by muscle memory.

Two more items appear only on a cell instance — Push In and Open Cell in New Tab. Those two are genuinely absent on a resistor rather than greyed, because they are not operations a resistor has; Hierarchy below is what they are for.

Right-clicking empty canvas gives a different, one-item menu: Pop Out. Nothing on the component menu applies when the click hit nothing, so the canvas menu carries only the one thing that always does — going back up a level. It is greyed out, with the reason on its tooltip, when you are already at the top of the schematic.

Keys at a glance

The right-click menu shows the same keys beside Rotate 90° and Mirror.

Hierarchy: putting one schematic inside another

Hierarchy is drawing a circuit once and using it in many places. A bias network, a matching section, a whole amplifier stage — draw it as its own cell, then drop that cell into a bigger schematic as a single component. The big schematic stays readable, and one edit to the cell reaches every place it is used.

Two things have to be true before any of it works, and they are the two that trip people up:

• Hierarchy needs a cell. A schematic on its own is not reusable — only a cell can be placed into another schematic. Making the cell is step 1 below, and it is not optional.
• The cell goes into a different schematic. A cell cannot contain itself, so the schematic you place it in must be another one. Pushing in is then how you get back down to the first.

Step by step: a cell inside another schematic

1. Create the cell. File ▸ New ▸ New Cell… (⇧⌘N / Ctrl+Shift+N), give it a name, and circuitRF makes the cell folder and opens its schematic. The command needs an open workspace — a cell is a folder inside one — so if it is greyed out, open or create a workspace first (The Workspace).

2. Draw the sub-circuit, and give it pins. Wire it up as you would any schematic, then place a Pin at every point the outside world needs to connect to. The pins are the cell's ports — the pin numbered 1 becomes port 1 — and a cell with no pins places as a component nothing can be wired to. Pin, Port and Term is worth reading once if that distinction is new. Save with ⌘S.

3. Open the schematic that will use it — a different one, and a saved one. A cell instance records where the cell is relative to the schematic holding it, so a scratch sheet from File ▸ New Schematic has nowhere to record it from; placing into one is refused with "Save the schematic before placing a cell" in Messages. Save it into the workspace first, or start it as a cell of its own.

4. Drag the cell out of the Project Tree and onto the canvas. That is the placement gesture. Cells you author are not in the Library Palette — the palette carries the built-in library and any imported kits, and your own cells live in the Project Tree instead. It lands as one component with your cell's pins on it.

   If the cell has no symbol yet, you are offered an auto-generated one, built from the pin count from step 2. Accept it to keep moving; draw a proper one later in the Symbol Editor.

5. Wire it in and set its parameters like any other component. Double-clicking its body opens the parameter editor for that instance.

6. Push in to edit the cell from here. Click the instance once to select it, then use any of:

   • Right-click ▸ Push In — the item appears only on a cell instance. Right-clicking empty canvas offers Pop Out to come back up.
   • Toolbar button 18, and 19 to come back out (the toolbar below numbers them).
   • ⌘] / Ctrl+] in, ⌘[ / Ctrl+[ out — also on the View menu as Push Into Cell and Pop Out.

   You are now editing the cell's own schematic, in the same tab. A breadcrumb bar appears above the canvas showing how deep you are (X1, the instance you came through); every step in it is clickable, so you can jump straight back to any level rather than popping out one at a time. Push in again from there to go deeper.

Once that round trip works, everything else about hierarchy follows from it:

• An edit to a cell reaches every instance of it, live. That is the whole point — and it is also the thing to be careful about, because pushing in through X1 and changing a value changes X2 too. They are the same cell.
• Push In is not the only way in. Right-click ▸ Open Cell in New Tab opens the cell as its own document instead, which is what you want when you are going back and forth and would rather have both on screen than one behind the other.
• A library part cannot be pushed into. It is the publisher's design, placed in many; its menu offers Edit Vendor Model… and Copy to Workspace… instead (A placed part).
• Depth is not limited to one level. A cell can instance other cells, and the breadcrumb grows a step each time you push in. Elaboration flattens the whole tree into one netlist before an analysis ever runs, so depth costs you nothing at simulation time.
• Parameters pass downward. A cell can publish parameters that the parent sets per instance, so two instances of one cell can carry different values. See Expressions for how a cell evaluates them in its own scope.
• Only the top schematic is simulated. An analysis attaches to the test bench — the schematic you press Run on — and the hierarchy below it is flattened into that run. A cell in the middle of a tree has no analyses of its own.

The other three views

The schematic is one of a cell's four views, and each is edited in its own editor:

The symbol is what step 4 above places; the layout is what gets manufactured. A cell need not have all four — the cell folder holds schematic/, symbol/, layout/ and 3d/ side by side and any of them may be absent.

Two commands under the Design menu move work between the schematic and the layout — Update Layout from Schematic (⌘U) and Update Schematic from Layout (⇧⌘U). Neither ever runs by itself; both are described in Schematic ⇄ layout.

A part that has no layout view of its own still reaches the board: its Footprint parameter — the last row of its parameter editor — names an SMT case size, an imported part or a .clay you drew, and that is what Update Layout places. See Footprints.

Starting from a template

New Cell and the Project Tree's New Schematic offer a Template under the name field. (Empty) is pre-selected; any other choice writes a ready-made test bench — its components, wiring and analyses — into the new schematic, which you then edit like any other.

Include Data Display sits under the picker. It is ticked for a template that brings its own Data Display, and greyed out for one that does not. Ticked, the display is written beside the workspace's .cws and named after the new schematic (Amp.cdd for a cell called Amp), which is the display a finished run opens. The first Simulate therefore fills it and brings it forward; until then its source combo reads not yet run. If a Data Display of that name already exists it is left alone, Messages says so, and the schematic is still created.

Two Port Stability is what to reach for first with an amplifier's or transistor's two-port data. Set the SnP's File to your .s2p (Simulate refuses, naming the parameter, until you do) and the SP1 sweep to the file's band, then Simulate. The display holds six plots: the source and load stability circles, one Smith chart each and one circle per swept frequency; μ and μ′; |S11| and |S22|; |S21| on the left axis with |S12| on the right; and Max Gain. Each is a built-in metric of the run, defined in Derived Metrics, so there is no expression to maintain. The S-Parameters example's FetStability cell is this template, already pointed at a file.

Simulating: an Analysis

A simulation in circuitRF is called an Analysis, and it is configured before it is run. An analysis is not a property of the circuit — it attaches to the test bench, the top schematic you actually simulate — so drawing a circuit does not by itself give you anything to run.

Open Simulate ▸ Setup Analyses… (the same list is also available as a dock panel), add the analyses you want, then press Run — ⌘R / Ctrl+R, or the ▶ button at the top of the list.

The example above is an ordinary two-analysis test bench: a DC operating point, and a Harmonic Balance run wrapped in a parametric sweep of the drive level Pin. Reading the panel:

• The checkbox enables or disables a row. A disabled analysis stays in the design and is not run — the way to park an analysis without deleting it.
• The badge is the analysis type: DC, SP, HB, LP, LPP, and SW for a parametric sweep.
• A sweep is indented under the analysis it wraps, which is how the panel shows that Pin is sweeping HB1 rather than standing on its own. Analyses run in the order listed.
• Results file names the one file this run writes into the workspace's shared results/ folder. Leave it blank to use the schematic's own name; name it to keep a baseline instead of overwriting the current results.

Adding or editing a row opens the analysis editor, where the analysis is actually configured:

The Type picker at the top decides everything below it — the body changes to the settings that type has. Here it is the harmonic-balance body: the fundamental tone (given as the expression RFfreq, resolved and previewed underneath), the unit, how many harmonics to retain, the single-versus-multi-tone choice, an Advanced block for the convergence controls, and the Parametric Sweeps section that wraps this analysis in one or more swept variables. The dialog grows to fit whatever the chosen type needs and scrolls beyond that, which is why the sweep's own Start / Stop / Step row runs off the bottom of the figure above.

Every analysis type, its full settings, and what it computes are in Simulations — DC, S-Parameters, Harmonic Balance, Parametric Sweep, Loadpull and Loadpull Pursuit.

Finding a component

Design ▸ Find Instance… — ⌘F / Ctrl+F — opens the Instances panel for the schematic you are working in and puts the cursor in its search box, so you can type a name straight away. The panel lists every component on the sheet by Name, Type and, where it adds something, the Cell/Part it comes from, sorted so that R2 comes before R10.

• Type to filter by name — any part of the name, upper or lower case. The type picker beside the box narrows the list to one kind of component; the two combine.
• Double-click a row (or press Enter) to zoom to that component and select it. A single click only highlights the row, so you can arrow down the list without the view jumping about. Enter in the search box goes to the highlighted row, or the first match.
• Esc in the search box puts you back on the canvas.

The panel always shows the schematic that has focus, and says which one in its header. Grounds, VAR and MEAS blocks are left out — they are rarely what you are looking for, and a sheet's grounds would bury its parts. The command is greyed out unless a schematic or a layout has focus; the panel itself is also under View ▸ Panels ▸ Instances.

Searching inside placed cells. By default only the level you are looking at is listed. Tick Include sub-cells and the panel also lists every component inside every placed cell, all the way down, named by its path — X1.X3.R5 is R5 inside X3 inside X1, so typing x1. lists everything under X1. The top level appears at once; the rest arrives a moment later (the panel shows Searching… meanwhile), and the window stays responsive while it does. With the box ticked the panel lists the whole tab from its top level, wherever you have pushed in to, so double-clicking X1.X3.R5 pushes down into X1, then X3, and zooms to R5 — and the list stays put for the next result. Unsaved edits in a cell you have open are included. A search that finds more than 100,000 components stops there and shows a + after the count. The box is remembered between sessions.

The toolbar

Grouped by what you are doing, left to right:

• View — Zoom to Fit, a zoom box, and Zoom Out. F is the one to learn; a schematic is usually bigger than the window.
• Draw — Select, the Wire tool, and the three things you place constantly: Ground, Term (a numbered port with a reference impedance, for an S-parameter run) and Pin (a connection point of the cell you are drawing). Which is which is worth reading once.
• Text — a note on the drawing: click where it starts, type, Enter to place it, and Shift+Enter for a new line, so one text can hold a paragraph. In the Properties panel's Content box Enter starts a new line. It works as the Symbol Editor's Text tool does: double-click a text to change what it says, and the Properties panel sets its size, style, colour, alignment and rotation. Text copies between a schematic and a symbol both ways: paste a selection copied in the other editor and its texts come across, at the same size and orientation.
• Orient — rotate 90° either way and mirror in either axis, applied to the selection.
• Delete — on the selection.
• Snap — cycles the snap mode. Electrical points always land on the connection grid whatever this says; the snap mode governs the authoring grid.
• Disable — mark selected components open or short. This takes an element out of the circuit without deleting it, which is what you want when you are bracketing a problem.
• Save.
• Hierarchy — push into the selected cell, or pop back out.
• Export to Library… — package this cell as a model in a model library, for others to place. Greyed, with the reason in its tooltip, unless this is a saved cell's primary schematic with at least one Pin. Also on the File menu.

See also: Symbol Editor · Layout Editor · Grid & Connectivity · Components · Pins, Ports & Terms · Simulations · File formats (.csch).