The Match Pair Level Spacing Rules dialog is used to define explicit spacing values between two net items, optionally on a specific layer or within a specified area. These values will override the default values defined in the Design Level spacings and in the Net Class Level spacings.
A detailed description of how spacings are determined is given here.
Shortcuts
Menu: Setup
Default Keys: T
Command: Technology
Locating this option
Available from: Setup menu > Technology > Spacing Rules - Match Pair Level page
Using the Match Pair Rules dialog
The Spacing Rules page for a PCB design is shown below:
Navigation
The buttons to the right side of the dialog are used to navigate the grid, these are detailed on the Technology Navigation page.
Using the editing pane
The match pair spacing values are presented in a grid, allowing you to change the values directly. Click on the text of the value you wish to change and edit the text to show the required value. You can also take the value from one cell and apply it across the whole row, down the whole column, or to all the cells of the whole grid, by pressing the right-hand mouse button and selecting the required option from the context-sensitive menu. Greyed out cells cannot be changed because they are not relevant.
Item 1
Define the first net based item you wish to use in your Spacing Rule.
Item 2
Define the second net based item you wish to use in your Spacing Rule.
On Layers
You can decide whether the rules apply to a specific Side: or Layer: selected from the drop down
list selections provided. If you wish to run the rule on all layers, either define Side as
Within Areas
If you have any Areas defined in the design, a rule can be defined for a specific named area. Rules can be defined for any combination of Layers and Areas, as required.
Minimum Spacing
This allows you to define a minimum spacing rule that will be applied. If an explicit spacing rule has been defined on a Net Class Level, this will override a minimum value defined on a Match Pair.
Symmetric Grid
This check box allows you to define a symmetric grid (meaning each type pair is the same - Pad to Track equals Track to Pad spacing). You can therefore only edit the bottom left section of the grid, and values are mirrored in the top right section. If you want to break the symmetry, you must first uncheck this box.
Creating rules
Firstly, you must define, which two sets of Nets the Rule applies between. Each set of Nets are identified
by a net attribute and the corresponding wildcard value.
In particular, you can use the special attribute values of
You must also specify which electrical layers the rule applies to, this could be by side (Top, Bottom or all Inner electrical layers), or a layer name - which can be a wildcard that may match several layer names.
Lastly you can choose to add an area name as a condition, again using wildcard characters to specify the group of areas the spacing set is to used within. The areas must be set up correctly to be used for this, see Using Spacings By Area for more details. Note: using the wildcard ”*” will apply the spacing rule within any DRC area that is named.
All the rule pairs you have defined are listed in the upper grid. The rules are applied in the order they are shown in this list, so if more than one matches, only the first match will be used. You can use the Top, Bottom, Up and Down buttons to move the selected rule pairs up and down the list. You can select multiple rules by holding down the Shift and Ctrl keys.
Practical Examples
If you want to match the single net named CLK1, use attribute
Another example, if you have net classes called Ground, Pwr +5 &
Pwr +12, you could define a rule pair between
Leaving the wildcard
The wildcard
In particular, if either of the Net Names is * or (blank), then the spacings for Text and Board, against the other types of items will become editable. You could therefore define an explicit spacing rule such as: Tracks on Net Ground against Board (on Net *) on Inner Layers.
Similarly, a wildcard
Wildcard Wizard
There are two methods for creating wildcards in Pulsonix; the first is to type the wildcard, the second is to use the Wildcard Wizard.
The Wildcard Wizard is designed to enable you to select easy to understand phrases that represent your required choice and then populate the Match Value with a command that Pulsonix will understand. It simplifies the task of specifying a wildcard string without having to understand the wildcard syntax.
The Wildcard Wizard is available using the small icon
next to the Match Value entry: 
Colour Coding For Grids
The grid is colour coded to show what values apply:
Black for inherited from Design Level
Green for Minimum Spacing
Blue for an explicit value
You can change a value back to the default by selecting the value in the grid and deleting it. An explicit value can be removed by deleting it.
Export and Import CSV
Use the Export CSV button to export the data in your PCB design into a CSV format file. Using the Export CSV option will provide you with a formatted template ready for you to edit in your own data.
Use the Import CSV button to import data back into the PCB design using a CSV format file.
The data in the file represents a spreadsheet of dialog contents with the data headings along the top row.
Import Custom CSV
Use this button to import net class and class to class level spacing rules into the schematic or PCB design using a CSV file that has been created using a customer specific format file. The data in the file represents a spreadsheet with net class names along the top row and down the left most column, with the rest of cells of the table representing the spacing values required between the net classes. See the Import Custom CSV help page for more details on importing spacings.
Units
The Units button allows you to locally switch between Metric and Imperial units whilst in this dialog. Once the dialog is closed, the units revert back to the original design units. If switching to different units to the design units, the value typed will be converted when you next enter this page.
Linked Types
These are enabled using [Options - General
- Spacing Rules - Enable linking of types](../../Design-Settings/idh_design_settings_general.md#spacingrules). When this is done, some rows and columns on the spacing grid will disappear (provided the spacings are the same), and the values are linked together. You can show the hidden values by unchecking the appropriate options which appear under the spacing grid. You can link Pad - SMD Pad, Via - Micro-via, Track - Copper.
Related Topics
Spacing Rules Overview | Design Level | Net Class Level | Check Spacing Values | Importing Class To Class Spacings | Using Spacings By Area | Wildcard Wizard | Design Rule Check | Nets Page | Export CSV | Import CSV | Import Custom CSV