Search PADS Maker Documentation

Searching PADS Maker Edition

All PADS Maker Documentation
Skip to end of metadata
Go to start of metadata

PADS Maker Edition and PartQuest provide tools to create or edit parts (symbols) for use in the schematic. Below is a graphic detailing the flow of each method. PartQuest is a free web-based tool by Mentor that combines Digi-Key part data with ADI graphics in a PADS Maker format.

Creating Parts/Symbols

There are 3 methods for creating parts for PADS Maker.

  • Method #1:  Use Partquest existing ADI part- Quickest automated method.  Does not allow for unique graphics.  Graphics are created by ADI.  Properties automatically copied to the Symbol. Footprints provided in most cases.
  • Method #2:  Use Partquest to create a custom part.  Quickest manual method.  Graphics are rectangles or discrete part shapes. Pins added in table or via .csv file.  Properties automatically copied to the Symbol.  Select footprint from Footprint Browser in PADS Maker or build Custom Footprint in Layout.
  • Method #3: Use Symbol Editor in PADS Maker. Slowest method but allows highest degree of Custom features such as graphics. User creates custom graphics. Pins added via table, by dragging or via .csv file.  Properties are added manually to the Symbol.  Select Footprint from Footprint Browser in PADS Maker or build Custom Footprint in Layout.

Method #1: Partquest- Download exising ADI part

This method of downloading or creating a new part is fast and easy. Partquest has over 500K symbols and footprints built by ADI. You will see AD next to symbols that have these parts available. ADI is a 3rd party company that makes CAD data.  You may download 25 ADI parts per day free of charge from PartQuest.

Searching PADS Maker Edition

Step 1 Sign in to PQ

Go to and sign in to your PartQuest account (see PartQuest wiki for setting up account link). When you click on the "Login" icon, you will be first be prompted to enter you account. If you do not already have a Mentor Graphics account, a link is provided on the login screen to create one.  

See the PartQuest wiki for assistance on setting up for PADS Maker.  You will have to select Maker in your PartQuest profile.

Step 2 Note Download Location

Partquest symbol and footprint downloads go to either a Dropbox or a directory on your computer (Direct Download).  See the PartQuest wiki.  You will select your download location in your PartQuest Profile.

Step 3 Enter Search Criteria

Go to the search bar at the top of the page and enter a part to search.  Check the Symbol/Footprint checkbox under the search bar for parts that have ADI symbol and footprint provided.

Step 4 Review Search Results

Review the results of your search and select a specific part.  Note the AD next to the Symbol and Footprint.  This indicates ADI created parts.

Now you choose a particular part from the list of available parts. Next to your chosen part, click the More button to reveal Symbol options.

Now click Choose Symbol.

Step 5 Select a Part and Download

Select Download.  The new parts will be in the Parts window of PADS Maker Schematic.  If you selected Direct Download, double click on the download to have the file show up in Parts.


If you have a PADS Maker Schematic and/or PADS Maker Layout project open when you initially setup PartQuest for PADS Maker Flow and download your 1st part, you will need to close the application(s) and restart them. Following this step, PADS Maker will automatically detect these locations and scan for any changes in your PartQuest Dropbox or Direct Download location.

For more details about PartQuest download, click here

Method #2 PartQuest- Create a Custom Symbol

If  the ADI symbols/footprints don't fit your needs or are not available for that part, you may create new rectangular symbol for your part in PartQuest or a discrete part.  Pins may be added in table or via .csv file. Digi-Key part Properties are automatically copied to the Symbol.  Select a footprint from Footprint Browser in PADS Maker or build a Custom Footprint in Layout.  This is the quickest manual method. 

Other options: Editing an Existing Part or follow the Creating a New Part in Symbol Editor flow.



Step 1 Sign in to PQ

Step 2 Enter Search Criteria

Go to the search bar at the top of the page and enter a part to search. To select a Standard Symbol, be sure to check the Symbol/Footprint checkbox under the search bar.

Step 3 Select a Part

Research the parts that result from your search.  Those with ADI symbol & footprint provided will have  a symbol/footprint indicator next to the part image.  Those without ADI CAD data will not have this indicator.

Now you choose a particular part from the list of available parts. Next to your chosen part, click the More button to reveal Symbol options.

Step 4a: Option for Standard Symbol for Discrete Parts

Select Choose Symbol and then Choose a standard symbol to create your own part.

For Discrete parts, select Standard Symbol of your choice, the part will be usable from the Schematic Parts Window once it is downloaded. It will also have Digi-Key properties added automatically. 

The Footprint, the PKG_TYPE property, will be added in the Symbol Editor in PADS Maker Schematic using the Footprint Browser


Step 4b: Option to Create a Custom Symbol

Select Choose Symbol and then choose the  sign under Custom Symbols.

The part will be usable from the Schematic Parts Window once it is downloaded. It will also have Digi-Key properties added automatically. 

The Footprint, the PKG_TYPE property, will be added in the Symbol Editor in PADS Maker Schematic using the Footprint Browser

This will take you to the following welcome page if this is the first time you are creating a symbol. Click Got It to continue.

This will take you to the Symbol Creator page where you can either, (a) add pin names and properties manually or (b) import pins in a .csv file.

Option A: Custom Symbol- Add Pins Manually

Custom Symbol provides a rectangular shape to which you can add your pins.

Enter a pin name at the bottom, and then press Enter on your keyboard.

Next, you will see your pin added to your Pin List and Symbol.

You can continue to add pins in this way, and you can set the pin properties in the Pin List.

Select Return once the symbol is complete.

Now click Download to download your custom symbol to the Schematic Parts Window.

Option B: Custom Symbol- Import Pins in .csv File

You can create a new symbol from a pin list in Excel, which will allow you to name your pins and define their type, location, and other basic properties, all in one spreadsheet. Click here to download an Excel template.

To create a new symbol from an existing pin list, click Click to Upload CSV Pin List or the Upload Pin List button . You will be prompted to select the .csv file on your computer.

Select Choose File.

Click above to download an Excel example to enter your pin names and properties. When all details are entered, use Save As to save the file as a CSV file.

Select the CSV file from the file explorer, and the pins will appear in the Symbol Creator menu.

Once complete

Click Return, then click Download to make the part usable in the Schematic Parts Window.

Consult this table for accepted CSV headers and values. Note that the pin name is the only required field. You may fill in many details from some pins and leave others blank in within a single CSV.

Column Header

Accepted Values

Default Value (when not provided)

Name (required)

Up to 64 character alphanumeric string


Pin #

Up to 32 character alphanumeric string



Yes, No



In, Out, In/Out, N/A


Elec. Function

Signal, Ground, Power, No-Connect


Elec. Type

Digital, Analog


Output Type

Open Collector, Open Emitter, Tristate, Open Drain, N/A


Connect. Type

Load, Source, Terminator



Yes, No



Yes, No


Active High

Yes, No


Active Low

Yes, No



Yes, No



Yes, No



Yes, No


Passive Pull-up

Yes, No


Passive Pull-down

Yes, No


Rated Voltage

Number in volts


Power Dissipation

Number in watts


SideLeft, Right, Top, BottomLeft
OrderInteger (1, 2, 3...)Order of CSV entry

Method #3:  Use Symbol Editor to Create Parts

The Symbol Editor (SE) is accessed from PADS Maker Schematic. SE is a tool for creating custom symbols for schematic.  You may edit properties in Symbol Editor and save changes to Libraries.  Symbol Editor is the slowest method to create a part but allows the highest degree of custom features such as graphics and Properties. The user may create custom graphics. Pins are added via table, by dragging, or by uploading a.csv file.  Properties are added manually to the symbol. In particular you will want to set the PKG_TYPE property as this designates the footprint for the part on the PCB. See the section on Footprint Browser.  Additional properties may be added as well.  Select Footprint from Footprint Browser in PADS Maker or build Custom Footprint in Layout.  Similar results can also be obtained by editing an existing symbol downloaded from PartQuest.

Special pin setups such as gate and pin swapping as well as fractured symbols can be setup in Symbol Editor.

Creating a New Part in Symbol Editor

Step 1:  Open Symbol Editor

To access the Symbol Editor and create a new symbol, go to File New Symbol, or select the New Symbol icon  in the toolbar.

To edit an existing symbol, right-click the symbol in the schematic Drawing Area and select Edit Symbol. The Symbol Editor also allows you to edit symbols in local libraries. For details on the Symbol Editor and it's windows, see Symbol Editor Windows.

Step 2:  Creating Symbol Graphics

Graphical elements in Symbol Editor work in much the same way as they do in the Schematic Editor. For more information, see Symbol Window and Adding Graphics and Text to a Schematic .

Step 3 Add or Edit Pin Names

Step 3 Option A:  Creating Symbols from a Pin List

To create a new symbol from an existing pin list, click Symbol from pin list either on the Start page or in the File > New menu. You will be prompted to select the .csv file on your computer. 

Step 3 Option B:  Adding and Editing Pin Names and Data
Placing Single Pins

To place pins on a symbol using the Add Pin feature in the Symbol Editor, use the following procedure.

  1. Go to Symbol Add Pin, or select Add Pin  from the toolbar.
  2. To control the side, type, or inversion of the pin, right-click within the Symbol window and select an option from the menu.
  3. Click to place the pin. 
  4. Place as many pins as you need, and press Esc to end pin placement mode.

Pin properties can be edited in the Pins window. You can also create pins directly in the Pins window by clicking "Click here to add new row." Once the pin has been defined, click-and-drag it into the Symbol window and onto the symbol.

Placing Pin Arrays

You can create multiple pins at once by using the Add Pin Array  function. The pin array dialog box allows you to create pins by defining a range (for contiguous pins) or set (for non-contiguous pins). Currently, the Properties feature is not functional.

Special Pin Setups in Symbol Editor

Below are some examples of ways in which pins can be arranged and properties assigned for specific situations in symbol creation.


To create a bus in Symbol Editor, append the width of the bus, separated by commas and surrounded by brackets, to the name of the pin. For example: DataB[0,7].

Then, include a list of pin numbers in the Pin Number category.

Pin and Gate Swaps

See Gate and Pin Swapping.

Implicit and Explicit Pins

See Implicit and Explicit Pins.

Fractured Symbols

See Fractured Symbols.

Step 4:  Adding or Editing Symbol Properties

You will have to add all properties manually. You may also edit existing properties. Symbol properties can be edited using the  Properties Window. Some properties are required for all parts, while others are required for special circumstances.  Set the PKG_TYPE property as this designates the footprint for the part on the PCB. See the section on Footprint Browser or build a Custom Footprint in Layout.  Similar results can also be obtained by downloading a similar part on ParQuest and editing it.

Required for PCB Layout:

DEVICEUnique identifier for each part. Auto-assigned in Symbol Editor for new parts.  Parts created from templates will need this number assigned manually. One DEVICE value must have only one PKG_TYPE value.

Alphanumeric characters.

Auto-generated: 0c031a7c-0a06-4030-907c-0be03b00c1ad
PARTSNumber of occurrences of symbol in physical component.  Value defaults to 1 if gate swap is not set up.  See Gate and Pin Swapping for other requirements.String. The value cannot exceed 255 characters.

In a DM7408 with 4 AND gates, PARTS would be 4.

PKG_TYPEFootprint Name. Footprints are assigned using the Footprint Browser. Footprints supplied by this product follow the IPC naming standard (  IPC footprints are in millimeters (mm). Additional footprints are listed in the ALT_PKG_LST property. Any characters. The value cannot exceed 255 charaters.DIP762W46P254L1918H533Q14B
REFDESReference Designator. Must end in a question mark (?) for the packager to run.  Indicates to the packaging utility which symbols are to be put in the same component. Typical REFDES assignments include IC? or U? for integrated circuits, R? for resistors, and C? for capacitors.Any characters. The value cannot exceed 255 characters.IC2, C1, R3
PINTYPERequired for each pin. Defines type of pin.String. The value cannot exceed 255 characters.


Required Under Certain Circumstances:

PropertyDescriptionSyntaxExamplesWhen Used
PINSWAPIdentifies pins that can be swapped for other pins. Use the pin name here, not the pin number. See Gate and Pin Swapping for other requirements.Any characters. The value cannot exceed 255 characters.Example in an AND gate: PINSWAP=A,B.  This means that A and B are interchangeable in function and result.Pin swapping
ValueValue of a discrete device (e.g. inductance, resistance, capacitance). Not required for PCB netlist.Any characters. The value cannot exceed 255 characters.100 ohmOnly for discretes
SIGNALDefines a signal (e.g. power, ground) connecting to a component’s supply pin. See Implicit and Explicit Pins for more details.Any characters. The value cannot exceed 255 characters.14;VCC, 7;GNDFor implicit pins

For information on additional properties that can be assigned to symbols, consult the Properties Glossary.

Saving Symbols in Schematic

To save a symbol, go to File Save or Save As, select the partition (folder) you would like to save the symbol to, type in a name into the empty field, then click Save. Saving a symbol in a standard library will make the part available to all projects by default, while saving in a custom or project-specific library will require you to load the symbol library for each project you need the symbol for.

Note: The symbol name cannot contain the following characters: ~ @ * ‘ / “ . space

Updating Symbols in Schematic

For changes in the Symbol Editor to be reflected in PADS Maker Schematic, the symbol libraries must be updated. To update symbol libraries to display new or changed symbols, go to Tools > Update Symbols in the PADS Maker Schematic menu. 

After editing symbols in the Symbol Editor, you must update the symbols in PADS Maker Schematic for changes to be reflected in your libraries and designs. If more than one symbol has changed, or there are multiple components for a changed symbol, you can choose which symbols or components to update.

  1. Select Tools > Update Symbols.
  2. In the Component definition update dialog box, select the checkbox next to the library name of the symbols you want up update (or click Select All to update all symbols listed) and click OK.
Updating Individual Components

After editing a symbol in the Symbol Editor, you can update all instances of that symbol in an open project by doing the following:

  1. Select a symbol.
  2. Right-click > Symbol Update > Update Symbol. The symbol is updated and the highlight on the selected symbol is cleared.
Flag Out-of-Date Symbols

Enable PADS Maker Schematic to flag out-of-date symbols by doing the following:

  1. Open the Advanced Settings window with Tools > Settings > Advanced.
  2. Set the Flag out-of-date symbols checkbox. Out-of-date symbols will be flagged with a blue box in any subsequently opened project.



If you edit a symbol in the Symbol Editor while a project is open in PADS Maker Schematic, any instance of that symbol on the currently opened project may not immediately be flagged. Be sure to use Tools > Update Symbols after you've finished editing symbols in the Symbol Editor.

Editing an Existing Part

There are 2 methods for editing parts for PADS Maker.

  • Method #1:  Download a similiar Partquest and edit it.
  • Method #2:  Edit an existing Library part.

Editing a Part in the Symbol Editor

Starter libraries and PartQuest downloaded parts are available in the PADS Maker Schematic in the Parts window.   There are 3 ways to access these libraries

  • Method #1:  In the Parts Window Symbol View, search and select a part you would like to edit.  R click and select Edit Symbol.  The Symbol Editor opens with the part loaded.
  • Method #2:  If the part is already placed in the Schematic, R click on it and select Edit Symbol.  The Symbol Editor opens with the part loaded.
  • Method #3:  From Schematic select File/New/Symbol which opens the Symbol Editor.  Once in the Symbol Editor select File Open>Library Symbol. Next you choose where the symbol you want to add is located. This is also where you access your saved symbols.

Method #1 Image

Method #2 Image

Method #3 Image

Loading Symbol Libraries


To access symbols from libraries outside of the default ones listed, you can add the libraries to your Parts view. For more information, see Importing Library Symbols.

Just as you can create a new part, you can also create new graphics. For details, see Adding Graphics and Text to a SchematicAdding and Editing Pin Names and Data–Placing Pins, and Adding or Editing Symbol Properties

From there, continue with the steps above following Adding or Editing Symbol PropertiesSaving Symbols in Schematic, and Updating Symbols in Schematic.  

  • No labels