The Project tab of the Navigator window shows the structure of all the design objects in your project. These are the objects that represent electrical elements of your design: boards, components, and connectivity.
The Project Navigator is a PADS Maker Schematic window that displays all sheets and design objects within the open schematic in a collapsible tree. This feature allows you to easily access any element of your design by double-clicking on its name.
The symbols folder shows the value in the REFDES and Symbol Name properties of the symbol. REFDES is the reference designator.
The Nets folder shows the value in the Name property of the net.
Below is the Project Navigator window for a reference design included in this wiki called Meter.zip.
A project is PADS Maker Schematic’s largest container of design data. You can have only one project open in PADS Maker Schematic at a time.
Each project contains a single board, for which there is a single schematic. A schematic is design data that you view and edit graphically. A schematic can contain multiple sheets in a flat design.
A Sheet is a piece of a schematic block. One sheet at a time is open in the schematic editor regardless of the number of sheets a schematic has. Sheets are connected by onsheet and offsheet connectors.
Symbols are graphical representations of components that you place on a schematic. They appear in the Project Navigator window under the sheet on which they are placed.
Nets define the connectivity among pins of components. Nets can be single nets or buses.
|Toggling the Project Navigator On or Off|
Toggling the Project Navigator On or Off
To toggle the Project Navigator on and off, go to View and check or uncheck Navigator.
|Moving Sheets in the Navigator|
Moving Sheets in the Navigator
By moving sheets around in the Navigator, you can affect the order in which the corresponding sheets are printed. To move a sheet in the Navigator, click-and-drag the sheet to its desired new location. A black bar will appear where the sheet will be placed. Release the mouse button to drop the sheet into its new location.
|Renaming a Selected Net from the Navigator|
Renaming a Selected Net from the Navigator
To give a particular net a more meaningful name than the default given in PADS Maker Schematic, simply click on the net in the Schematic window or click on its default name in Navigator. Then go to Properties and type in a new identifier next to Name.
Note that when you change the part's name, it is only changed for your particular project. The part retains its original name in the Parts library.
Sorting Objects in the Project Navigator
To sort symbols and nets for easier location, you can right-click the Symbols or Nets folders, navigate to Sort, then select what property you would like to sort the objects by as well as whether they are listed in ascending or descending order.
Working Within the Schematic Editor
The Schematic Editor is the window in which opened projects appear. This page will outline some basic information about working within the Schematic Editor.
New projects automatically start with one sheet, but you can add more by clicking the New Sheet icon in the top left corner of the page. To remove a sheet, right click on the sheet in the Navigator and select Delete.
Using Schematic Editor Tabs
The tabs at the top of the Schematic Editor window allow you to navigate through all open sheets. You can also convert other PADS Maker Schematic windows into tabbed windows. For more information on converting windows into tabbed windows in the Schematic Editor, see Customizing Window Layouts.
You can configure PADS Maker Schematic to display the names and properties of objects as tooltips. To do this, go to Tools > Settings > Display and check the appropriate boxes under Show Tooltips. You can choose to display tooltips for components, nets, and pins.
Schematic Properties Window
The Properties window displays the drawing area properties if no specific object is selected in the Pin or Symbol windows.
When an object is selected in either window or by clicking on the part in the drawing area, the properties
The checkboxes next to the property names and values allow you to choose whether to display the property name/value on the symbol.
To add a new property to the list, click on the last empty cell in the Properties window and a drop-down menu will appear from which you can add a new property.
Schematic Properties Window Options
Below are general properties that are displayed when no particular object is selected.
Contains the name of the schematic.
Here you can select a Drawing Area size from the drop-down menu.
This property allows you to create your schematic in either Landscape or Portrait mode.
Width & Height
To change the width or height, you must first select Custom from the drop-down menu next to Drawing Size. Then you click on the areas next to width and/or height and manually enter a number which will be automatically interpreted in inches.
Many optional properties are available to you besides those named in the Properties window in PADS Maker Schematic. To access these additional properties, go to the bottom of the Properties window and click on the last empty cell of the table. Clicking on that box should open up a drop down box from which to choose a variety of additional, optional properties. To change the properties of a particular part, click on its symbol in your schematic to view the part's properties, then go to the bottom of that Properties window list and follow the directions below.
Properties on the Sheet border in the Schematic.
Click on any of the properties from the drop-down box. Once selected, the property will appear in your Properties table.
Part Properties may be edited in the schematic or in the Symbol Editor.
To change the property of a part in the schematic, select the part by double-clicking on the symbol. The Properties Window is displayed. Properties changed in the schematic exist only in that schematic. If you wish to save the property change to the part for future use in other schematics, change the part in Symbol Editor and save it to the Library where this part is stored.
In the Properties window, scroll down through the list of properties to the property you wish to edit and make the desired updates. To add an additional property, scroll down to the bottom of the Properties window list, and follow the same directions as above.
The check boxes next to the names of the Properties and their values are toggles to display/not display the property name and property value on the part.
You may add as many additional properties as you like from the drop-down box.
To change properties in the Symbol Editor, see the section on Editing a Part in the Symbol Editor.
The Schematic Parts Window is where you can search and select parts to use in your schematic.
The left section is the Symbol View. This is a listing of all libraries setup on your computer and the associated parts (aka symbols). The right section displays a view what the symbol looks like as well as what the associated footprint looks like. (Note: Footprint name is in the PKG_TYPE property of a symbol)
When you first load PADS Maker, the Parts window will contain a list of all Starter libraries.
We recommend you setup PartQuest immediately as PartQuest offers more than 500K symbols and footprints and it’s free! PartQuest requires a login at Mentor.com and DigiKey.com. See the PartQuest section for more details.
Once PartQuest is setup and at least 1 part is downloaded, PartQuest Dropbox or PartQuest Direct will be listed in the Parts window as well. Enter any information that you know about the part in it’s part properties and the list will be filtered to parts that contain that piece of text. The “Matched” column will display what text matched the criteria on the part.
Selecting the Partquest icon will open PartQuest so you can search for additional parts.
From the list view you can R click and place the symbol, edit the symbol, etc. Editing the symbol will open the symbol up in Symbol Editor (SE).
On the right side there is a graphical preview of the symbol that would be used in the schematic.
If the PKG_TYPE property is filled out and that footprint is in the library, you will also see a graphical preview of the footprint.
If you select “Place Symbol” you will be able to place multiple copies of the symbol in the schematic.
If you R click in the footprint preview window you can browse for additional footprints using the Footprint Browser.
To add more libraries to theParts window, see the section on Drawing a Schematic–Importing Library Symbols.
To create a new part or edit an existing part, use the Symbol Editor.
The Footprint Preview window provides a view of the footprint assigned to a symbol. Selecting a specific part in the schematic window will show a graphic image of the layout footprint (where assigned).
Not all symbols have footprints assigned. If there is no footprint assigned to a selected symbol (PKG_TYPE property is black), this window will display the text "No Footprint". Special components, power and ground symbols, will not have a footprint during the layout phase so the window will display "No Footprint" in this case. For symbols that have a footprint assigned (PKG_TYPE property), but the footprint is not in the footprint library, the window will display "Not Found". To add or change the footprint assigned to a symbol, use the Footprint Browser while you are working on a design in PADS Maker Schematic. If there is no symbol selected, the window will display the text "No Decal".
For more information on footprints, see The Footprint Browser.
PADS Maker Schematic ships with over 16,000 footprints (also called packages), included in the Footprint Browser, built and named in compliance with the IPC-7351 Standard. All dimensions are in millimeters.
The Footprint Browser allows you to assign footprints to components, designating both the pattern and space that the component will take on the PCB.
You can access the the Footprint Browser from either the Footprint Preview window or from the Symbol Editor.
From the Footprint Preview Window:
- In the Schematic Editor window, select the symbol that you would like to assign footprints to.
- Right-click anywhere within the Footprint Preview window and select Browse Footprints.
From the Symbol Editor:
Go to Tools > Footprint Browser to assign footprints to the symbol currently open in the Symbol Editor window.
The Footprint Browser makes it easy to locate and assign the desired footprint to a symbol. Use the following procedure to optimize your search and receive the most relevant results.
- Select a footprint library. PADS Maker Schematic offers 15 libraries to choose from. Note: The terms Most, Nominal, Proportional, and Least refer to material condition, or pad size.
- Next, you can filter footprints within the library.
- If you know all or part of the footprint name, it can be typed into the By Name field. Note: For incomplete name searches, the wildcard asterisk (*) must be appended to the incomplete part of the name typed. For example, if you need a footprint with the prefix BGA, a search of BGA* will return all footprints with names that begin with BGA.
- You can also filter using the By Standard Footprint Name category, first by selecting an item from the Family dropdown menu.
- After selecting a footprint family, search filters specific to that family will appear below. Numbers can be entered in ranges to expand number of search results returned (with the exception of pin count).
- To apply all filters and complete the search, click Apply Filter.
When searching for specific measurements, note that the units of measurement are determined by the selection made above the footprint information window. If this option is toggled while there is a value in a field of measurement, the measurement will automatically be converted.
Once you narrow down your search results, assigning the desired footprints to a symbol is fairly straightforward.
Unassigned Footprints lists the results of your search. Assigned Footprints contains a list of all footprints currently assigned to the symbol.
Footprint assignment type toggles between assigning the footprint as the default footprint (PKG_TYPE) or as alternate footprint types (ALT_PKG_LST). Be sure to press Apply to Symbol a the bottom of the Footprint Browser before toggling between these options to save your list.
The Design Rules for a printed circuit board determine how close traces and footprints can be to other traces and footprints. These are often called clearances. Footprints may be built to one of these material condition standards so users need to take board density into consideration when selecting footprints.
Most Material Condition refers to the most space around the component and the lead contact area. This results in larger footprints, which in turn drive low design density products.
Nominal Material Condition refers to the nominal space around the component and the lead contact area. This results in nominal size footprints, which in turn drive medium design density products.
Least Material Condition refers to the least space around the component and the lead contact area. This results in smaller footprints, which in turn drive high design density products.
The Output window provides feedback on actions in the Schematic Maker. Below is a list of the most common examples.
- Licensing information at Startup
- PartQuest sync activities when a new part is downloaded
- Files generated like bill of materials
- Errors/Warnings/Messages during Packaging (Tools/Prepare for Layout)
- Errors/Warnings/Messages during Netlist generations (ECO/Forward Annotate)
Using the Output Window to Find Errors
The Output window will display any notes, warnings, and errors that occur when packaging a design for use in a layout program . Warnings appear in blue text, and will not inhibit the packaging process. Errors appear in red, and will need to be resolved before packaging can be completed. See the Table of PADS Maker Schematic Error Messages for information on specific warnings and errors.
Any message preceded by a green box with an arrow will take you to the specific location of the note or warning when clicked.
The Output window will pop up when there is a new message in the Output window and it is not currently open.