This document is ALPHA quality and is under construction.

Component Symbol guide

This file discusses the creation of component symbols, including style conventions, and hints/tips and things to look out for when drawing symbols.

  1. Component symbol creation

    2. Component symbols (from here on known as "symbols") are drawn using gschem just like drawing a schematic sheet.

    1. Draw the symbol (see the style guide below for some conventions)

    2. Translate the symbol to the origin

      1. Zoom in at least one step
      2. Make sure the snap is ON (this is critical)
      3. Make sure grid snap size is set to 100 (this is critical)
      4. Select "Symbol Translate..." or the press equivalent hotkey
      5. Enter 0 into the entry field and press OK
        6. This step is required! All symbols must be translated to the origin. To translate a symbol elsewhere, enter a offset (in mils) which is a even multiple of 100. Make sure all pins are snapped to a 100 mil grid point.

    3. Save the symbol using Save or SaveAs... The name can be anything but I've started the following conventions
      • Symbols are named: symbolname-#.sym
      • Symbols end with a .sym extension
      • Symbols have a -# where # is a number. Typically # is 1 but if there are multiple symbols for a device then this number simply increments
      • Symbol names are typically lowercase but letters which are part of a part number are uppercase
      • The above case rule can be broken if the filename looks incorrect or wrong.

    4. Place the symbol in one of the directories specified by the component-library keyword in a gschemrc file. Once this is done, the symbol should be visible immediately and can be selected and placed with the "Add/Select Component..." menu item.

  2. Style Guide for symbols

    3. The styles described here are preliminary and can be changed so if you have an opinion, let me know. Please look at the current symbol libraries for examples. If you find something inconsistent, please let me know.

    Here are the current symbol conventions:

    1. Text labels should all be 10 pt in size.

    2. Pin numbers (which are attributes) should all be 8 pt in size.

    3. Text (labels not attributes) should be green.

    4. Lines, boxes, arcs, and any other graphics should be green.

    5. Pins should all be 300 mils (3 grid spaces) long.

    6. Pins should be white.

    7. Leave 400 mils (4 grid spaces) between (vertically) pins, unless you are drawing a special symbol, then just try to make it look good.

    8. Pin number attributes should be 50 mils above (or below; which ever makes the most sense) the pin which they are attached to.

    9. Polarity bubbles should be cyan

    10. Do not draw power and ground pins. That information will be conveyed using attributes (see netattrib.txt)

    11. Expanding on above, symbols are symbolic, they do not represent the physical package that the device comes in. Input pins belong on the left and output pins belong on the right of the symbol. Please do not mix inputs and outputs on the same side of the symbol, unless absolutely necessary. You can have pins on the top or bottom of a symbol.

    12. A gEDA user didn't like the above, so the following is okay too: Arrange the pins on a symbol logically so that they promote an uncluttered schematic. Note that this is frequently not the same pin arrangement as the physical device.

    13. Attached attributes should be yellow. The color is set automatically to yellow if the text item is attached.

    14. Attributes can be attached to some part of the symbol. Either a pin (if it's a pin number) or some other part of the symbol such as a line if it's just a device= attribute. Attributes used to be required to be attached to something to be attributes, but now they just have to exist in the symbol file as name=value

    15. Expanding a bit on the last sentence, as long as the text item has the format name=value, it is considered an attribute. Attributes inside a symbol do not have to be attached to anything. In order to see hidden attributes in gschem select Edit/Show Hidden Text.
    16. Required Attributes

      • device=device_name should be placed somewhere in the symbol and made invisible. device= is the device name and is required. If the object is a graphic then device= should be set to none (device=none). It is no longer required to attach this attribute anything; just having it exist as device=name is good enough.
      • graphical=1 should exist somewhere in a symbol which is purely graphical (such as a title block or decon symbol). Symbols which have this attribute have no electrical or circuit significance. Don't forget to set device=none.
      • All pins should have a pin#=# attribute attached to the pin object. The first # is a placeholder and increments sequentially starting at 1. The second # is the actual pin number. Both #'s are required! The order of pin#'s is significant since the netlister will output pins in sequential order starting at pin1 going through pinN. Example: pin1=1, pin2=2, pin3=5.
      • All pins should also have the label=value attribute attached to them. Please make this attribute green (instead of the default attribute yellow). Right now, the symbol libraries do not follow this convention, but they will.
      • If a component has multiple slots in a package (such as a 7400 (NAND) which has 4 NANDs per package) then you need a numslots=# attribute. The # is the number of slots the device has. numslots= should be exist somewhere in the symbol and made invisible. Additional slot related required attributes are below.
      • If a component has multiple slots in a package then you also need to attach a slot#=#,#,#... for every slot the component has. The first # corresponds to the slot number. If a device has 4 slots then there would be a slot1=, slot2=, slot3=, and a slot4= attribute existing somewhere in the symbol and made invisible. The subsequent # have a one-to-one correspondence to pin# attributes and specify what the pin# should be when that slot is set. Yes this isn't obvious and will be changing in the near future. See 7400-1.sym as an example of how this should all work.
      • It is recommended that all symbols which have slots have a slot=1 attribute attached in the same fashion as the device= attributed. The default pin#=#'s should reflect the first slot. You cannot override the pin#=# with a non-slot=1 when placing components (at least not yet).
      • footprint=package_name should exist somewhere in the symbol which might be used with the netlister. Attach this attribute just like the device= attribute. package_name is the pcb footprint or package type like DIP14 or DIP40. This is very new and so I'm not 100% sure this attribute will be call this or what the values should be, so it's not required yet. None of the current libraries use this.
      • The label= attribute should not be attached anywhere in the symbol. It is used for net name labels only! This statement contradicts the above pin label= attribute. For now, ignore this statement.
      • The name= attribute should not be attached anywhere in the symbol. It's currently unused.
      • You can put a uref= attribute inside a symbol. Make only the value visible and it will be promoted (attached to the outside of the symbol (so it can be edited) when the symbol is placed in a schematic.
      • Please look at the netattrib.txt doc file for info on how to assign power/ground information

  3. Hints/tips

    1. Avoid drawing things off of the grid. If you do, you cannot move the object(s) using the move command (if the grid is on) since the object will be snapped to the grid. [This was an old bug, which I think has been fixed, but avoid doing this anyway]. Use the symbol translate command instead (or move the object with grid snap off).

    2. If you need a finer grid then use Options/Snap Grid Spacing... to set a finer grid snap spacing. Just remember to set this back to 100 once you are ready to translate the symbol to the origin

    3. If you want to translate a symbol from the origin to elsewhere, then use the "Symbol translate" command and enter a non zero number. Make sure this number is a multiple of 100 (ie 1000, or 1100).

    4. Pins *MUST* be snapped on the 100 spaced grid (at least the end which will have nets connected to it)

    5. Pins *MUST* be snapped on the 100 spaced grid (at least the end which will have nets connected to it) (Yes this is line a duplicate. I can't stress this point enough

    6. Don't include nets inside symbols. That isn't implemented and doesn't make much sense anyway.