In the Search View, if you see the symbol icon below (resistor graphic), a symbol exists for this part. If the symbol does not already exist or you want a different symbol, use the Symbol Creator.
Select one of the methods below to start building symbols:
- Method #1: From Search, select More and Choose Symbol.
- Method #2: From the My Symbols page, select Create Symbol. Use this method to create a symbol regardless of whether a DigiKey search returns a result or not.
- Method #3: From the Home page, select Create Symbol which takes you to the My Symbols page.
Method #1: Search, Select the More down arrow, and Choose Symbol
Method #2: Select My Symbols page and Create Symbol
The My Symbols page lists all symbols- those searchable on DigiKey and those not searchable on DigiKey.
The columns are sortable, select the column heading name to sort ascending or descending.
Delete symbols (those without a DigiKey search match) and Download symbols from this page.
Method #3: From the Home page, select Create Symbol and follow Method #2.
The options to create or obtain a symbol are shown.
There are 3 methods of creating a new symbol in PartQuest.
The Symbol Creator captures more than the terminals(pins) you see on the symbol. With the Symbol Creator, you can
- Capture a complete terminal list and determine how you want to represent the symbol from that terminal list.
- Map the logical terminal names to the physical terminal numbers.
- Add electrical properties to the terminals.
- After completing the details of the terminal list, consider how to represent the symbol. Remove terminals from the symbol by marking them implicit in the terminal list.
- Use the terminal(pin) order view to give the relative locations of the terminals.
Focus first on the terminal list and then on how to represent the symbol. Keep checking back for new features.
Choose a Standard Symbol
To create a symbol using a Standard Symbol for a part, click the Choose Symbol button. These symbols are standard sizes and are not customizable at this time. The size will automatically adjust to display text properly.
Select one of the 78 common symbol shapes provided.
If we select one of the amplifier symbols, LM741CNNS/NOPB-ND, we get the following:
The grid in the background is set using Symbol Creator Settings at the top right. Terminal(Pin) spacing can be set on this menu as well as the location of the Reference Designator and property values from PartQuest.
The name of this part is displayed at the top, Texas_Instruments_LM741CN_NOPB. Use Edit to the right of this name to rename the symbol if desired.
Selecting the Datasheet link will display the details about this part giving functional pin names as well as the terminal numbering on the footprint. As we see below, pin 1 on the footprint has a functional name of Offset Null.
The default symbol includes optional pins. Remove these from the symbol by selecting Disable All button. Notice the optional pins are no longer shown on the symbol.
Per our datasheet, this part utilizes 2 of the optional pins, both called Offset Null, pins 1 & 5. Toggle the Disabled switch by these pins in the table to add them back to the symbol.
Enter the footprint terminal number in the Terminal # column of the table. This matches the functional name to the footprint terminal.
Per the datasheet, this part has a No Connect pin, terminal 8. Notice on the bottom that the Symbol Creator is tracking how many pins are currently unassigned in the Unassigned Footprint Terminals area.
Select Add to show this terminal in the table as a No Connect.
If you want to alter the functional names of the pins type them into the User-defined Name column. The symbol size will dynamically change to suit the length of the pin names inside the body. Pin names can repeat as these are labels. The real names are the JEDEC Names.
For example, the Vout is now called AmplifierOutputPin which caused the symbol size to increase. Offset1 and Offset2 have also been renamed. Notice the pin length has increased to adapt to this change.
The table columns are sortable. Select the column name at the top. Terminal Sorting: Exclude Disabled allows you to remove Disabled pins from the sort. When set to off, Disabled pins will go to the bottom of the sort and not be mixed in with Enabled pins with the sorting action. When set to on, Disabled pins will be sorted in with Enabled pins.
Creating a Custom Symbol for a Part
To activate the Symbol Creator for a part, click the Choose Symbol button, and then select Create Symbol.
To add terminals(pins) to your symbol, simply type in a terminal name and hit return.
Once you add a custom symbol to a part, it will appear next to the Choose Symbol button in search. Hover over the thumbnail image to see a larger image of the symbol.
There are two methods for entering terminal data. One is manually entering the terminal data using the instructions below. The second way is to upload a CSV with the terminal data.
Remember to upload a complete terminal list so that you may be able to properly generate a terminal map.
Adding and Editing Terminals(Pins)
If you would like to create a part from scratch or manage the terminals uploaded through a CSV, you can add or remove terminals through the Symbol Creator interface.
To add a terminal, simply type the name of the terminal into the Add Teriminal(s)/Pin(s) Name box and hit Enter. The terminal will appear in the terminal list, where you can edit its properties.
To rename a terminal, click the arrow under Actions and select Rename. The name box will become editable. You can also do this by double-clicking the name.
To remove a terminal, click the arrow under Actions and select Delete. You can also do this by selecting terminals and pressing the Delete key.
Uploading a CSV Terminal (Pin) List
Editing Terminal(Pin) Properties
Once you have added the pins to your symbol, you can adjust the property values. To see all of the properties in the terminal list, you can expand the terminal list by clicking the arrow at the bottom of the window. Click the arrow again to collapse the list.
The properties available for editing are listed below.
Note: Some properties have dependencies on each other. The table will help ensure you only select valid combinations of properties. If your currently-selected property appears in gray, it cannot be changed without another property automatically changing to accommodate. If a property appears gray in the dropdown list, selecting the property will cause other properties to change.
The name describes the name of the terminal(pin) that is used on the symbol and is the only required field for a terminal(pin). This is the same name that is referenced when mapping the symbol terminal(pin) names to the footprint terminal(pin) names. Note that Symbol Creator will allow you to use duplicate terminal(pin) names, and these names will be displayed on the resulting symbol as duplicates; however, each duplicate entry will use a hidden name with a suffix of __x where ‘x’ is a number starting at 0 and incrementing by 1 for each duplicate terminal(pin) name on the same symbol.
Terminal #(Pin #) is used to map the terminal(pin) names to individual footprint terminal(pin) numbers. This field is not required to create your symbol, but your part may not be ready to use on your desktop unless you complete this, depending on what flow you are using with your PartQuest parts.
Inverted will mark the terminal(pin) as inverted. Graphics (line above terminal name) will be added to the terminal(pin) to represent it as inverted on the generated symbol:
Direction designates the direction of the signal for this terminal(pin) as In, Out, or In/Out. Graphic annotations will be shown for "In/Out". Use settings to control if graphic annotations will be shown for "In" direction terminals(pins) on the right and "Out" direction terminals(pins) on the left
Electrical Function describes the general function of the terminal(pin) as Signal, Ground, Power, or No-Connect.
Electrical Type is only valid for "Signal" terminals(pins). It defines whether the terminal produces or consumes an Analog or Digital signal.
Output Type is valid for any "Out" terminals(pins). It defines the terminal as Open Collector, Open Emitter, Tristate, or Open Drain.
Defines the signal as a Load, Source, or Terminator.
Implicit terminals(pins) are terminals that are included in the part, but you do not want them to show on your symbol. You will see that marking a terminal(pin) as implicit will exclude it from the symbol. Power, Ground, and No-Connect terminals(pins) can be set to implicit. The implicit terminals(pins) will be represented appropriately in the flow you are using. When sending the part to a flow such as Xpedition or PADS Professional, which require explicit terminal(pin) mappings, the appropriate terminal mapping data will be provided for the part definition. Similarly in the PADS flows the implicit terminals(pins) will added as “Signal” or “NC” properties in the symbol.
Setting this to one defines the terminal(pin) as a clock. Use the settings to specify if a graphic annotation should be shown for the clock.
Setting this to one defines the terminal(pin) as being activated on high. Use the settings to specify if a graphic annotation should be shown for Active High terminals.
Setting this to one defines the terminal(pin) as being activated on low. Use the settings to specify if a graphic annotation should be shown for Active Low terminals.
Setting this to one defines the terminal(pin) as being hysteresis. Use the settings to specify if a graphic annotation should be shown for Hysteresis terminals.
Setting this to one defines the terminal's(pin's) function is to enable. Use the settings to specify if a graphic annotation should be shown for Enable terminals.
Setting this to one defines the terminals's(pin's) function is to amplify the signal. Use the settings to specify if a graphic annotation should be shown for Amplify terminals.
Passive pull-up terminals(pins) are terminals with an internal connection through a passive device to a second, more positive, supply voltage in addition to the internal connection to an active device through a supply voltage. Use the settings to specify if a graphic annotation should be shown for Passive Pull-up terminals.
Passive Pull-down terminals(pins) are terminals with an internal connection through a passive device to a second, more negative, supply voltage in addition to the internal connection to an active device through a supply voltage. Use the settings to specify if a graphic annotation should be shown for Passive Pull-down terminals.
Rated voltage describes the max voltage that may be applied to the terminal(pin), beyond which damage may occur.
Power Dissipation describes the max power that may be applied to the terminals(pin), beyond which damage may occur.
Terminal(Pin) Order View
The display on the right side of the Symbol Creator allows you to view and edit your terminal(pin) arrangement. Click and drag a terminal to move it to another location on the symbol. Note that the terminals will snap to locations as you move them. You are only providing relative positions for the terminals. There is no concern for grids or spacing of the terminals. When the final symbol is generated, your settings will define how the terminals are spaced.
Troubleshooting Terminal(Pin) Mapping Errors
If a yellow exclamation mark appears beside the image of a part in a list, the terminal(pin) mapping is incorrect or incomplete. Check your terminals mapping for errors.
Possible errors include:
- List of terminal(pin) names does not match terminal numbers
Duplicate terminal(pin) numbers used in mapping
Request a Symbol from SamacSys
You may request a Symbol be built for you by SamacSys. This service is free and turn around time is generally 24 hours.
If a Symbol and/or Footprint are not available for download, the symbol and footprint icons will not exist.
Selecting MORE you will see a Request option.
Selecting Request will ask you relevant questions.
You will receive an email from email@example.com within 24 hours that the content is now available to download. Note: Very complicated parts will take 48-72 hours.
The email will contain a link to your part in PartQuest where you will see the part with content.
From within Partquest, download the new symbol and use it in your design.
To create a Custom Footprint, go to the Custom Footprint Generator.