Use this to check that the pins of your schematic are connected to the right kind of pins in a net (e.g. make sure that there is only one Output pin in a net). The rules are set up in the Technology dialog. Also used to check the completeness of nets and the hierarchical rules are complete.
When errors are found Error Markers are added to the design on the appropriate page to help you find and correct the error.
Shortcuts
Default Keys: None
Default Menu: Tools
Command: Electrical Rules Check
Locating this option
Available from: Tools menu > Electrical Rules Check option
How To Run an Electrical Rules Check
There are several ways to get to the Electrical Rules Check Dialog as follows:
- On the Schematic Toolbar select the Electrical Rules Check Icon
- Under Tools on the menu bar, select Electrical Rules Check
- From within the ERC Errors Browser window, right click to use the shortcut menu and select the Electrical Rules Check option.
A dialog is then displayed which allows you to control which items are included in the check.
Pin Type Rules
Use this check box to check that the Pins on a net are connected to Pins of correct types. You can set up which pairs of pins that can be connected together on the Pin Type Pair Rules tab of the Technology dialog.
When the design has Variants, pins are only considered
connected if they are fitted in at least one common variant. Note that the
Note that this is the only check that is done by the Online ERC checks.
This check will normally only place an error marker for rules defined as Errors. If you also want error markers for Warnings, check the Mark Warnings box.
Busses
Use this check box to check that all the Nets attached to a bus are connected at least twice on a bus.
Hierarchy
Use this check box to check that there are matching block pins to block ports in the hierarchy.
Also checks that block ports are connected.
Unfinished Nets
Use this check box to check that all nets have at least two component pins in them. It will also report empty nets, although because they are empty it will not add error markers to the design because there is nothing visible onto which an error marker can be placed.
A net is unfinished if it only has one signal reference.
If you have a specifically designated a pin with the Single-Pin pin type (in the Technology), then this pin will be ignored in this check.
Validate Attributes
This option will check that the value of each attribute, which has a validation string define, matches that validation string. Validation strings are defined on the attribute names page of the technology dialog.
Unfinished Connections
Use this check box to check if there are connections which are unfinished. A connection is unfinished if it is on a net that has less than two component pins, or it is dangling (no item at its end) and has no visible net name at either end, or it is dangling and connected to a bus at the other end.
If you find connections are unexpectedly marked as unfinished, try selecting the open end of the connection and doing Show Net Name to display the net name at that end, these problems are generally caused when a net name appears to belong to the connection but is actually attached to a pin elsewhere on the net.
Unlabelled Nets
Use this check box to check that all separated parts of named nets have at least one Net Name showing, or contains at least one signal reference documentation symbol with a predefined net type or name.
You can automatically add all missing net names with the Apply To All option whilst using the Show Net Name interactive operation.
Unlabelled Net Pages
Use this check box to check that the any net which has the
Bridged 2-Pin Components
Check this box to ensure that the pins on two pin components are on different nets. If the pins in the symbol are on the same net, then it has been designed to bridge and will not generate an error.
Unmatched Page Links
Check this box to check that every Page Link on a net has a matching page link on the same net on the page that it links to.
For example, if net “A1” on page “Page1” has a page link to “Page2”, then it is an error if the net “A1” is not on page “Page2”, or if net “A1” on page “Page2” does not have a page link back to page “Page1”.
A page link on a net is a pad or junction on the net with the
Unmatched Signal Refs
Check this box to check that every Signal Reference on a net has a matching signal reference somewhere else on the net.
Common Pins
Checks that common pins on a component are all connected to the same net (some may be unconnected, in which case they will assume the net of the connected ones).
2-Pin Components
When selected, this checks for components with two pins where only one pin is connected.
Coincident Items On Different Nets
Use this to check that items that are not on the same net do not lie on top of each other. It will check every connection and bus corner, and every pin. Connections on different nets are allowed to cross each other as long as a corner on one does not lie on the other. Pins are checked against all connection and bus segments and against all other pins.
Note: On all but small designs it is a good idea to have the Fast Locate option switched on in the Display Options dialog.
Split Nets
Use this to add an error marker on all nets that are split into separated sub nets. These may be valid, but this allows you to quickly check if a net has been split by error. A sub net is not marked as being split if it is connected to a bus.
Use the If Not Linked By Doc Symbol check box to not mark a sub net as being split if it contains a documentation symbol of any type. It assumes that the documentation symbol is an off page reference or signal reference.
Note: if a sub net is marked as being split and you cannot find another occurrence of the net, it may be because the net exists on ungated pins on some components. Use the Find bar with Search All Pages on to find components that are using the net for ungated pins. This situation may be valid, but again this allows you to check if the net was used on this sub net or on an ungated pin by mistake.
Select the check box, If Net Name Is Not Shown On All sub-nets to ignore the split net error if all the sub-nets have a Net Name attribute position.
Use the check, If Splits Are On Different Pages, to ignore the split net error if it is on the same page.
Select the check, Unless Pin Type Is PCB No Connect, to ignore the split net error if the Ungated Pin is type, No Connect in PCB.
Pins Not On A Net
Use this to add a marker on all pins that are unused and have not been added to a net. It will also add markers on a component if its ungated pins are not on a net.
Note: Pin Types defined as No Connect, Ancillary Pad and Mounting Hole are ignored and not marked.
Net Pins With No Connection
It is possible to select a pin and add it to a net without adding a connection to it. These are not obvious in the design and can now be found using this check box. Use this along with Pins Not On A Net to mark all pins that do not have a connection attached in the design.
Nets Only On Ungated Pins
Use this option to check for nets that are only on Ungated Pins.
Net On No Connect Pin
This checks for any No-Connect Pin Types that are connected on a net.
Power Net / Power Pin Pin
Use the Power Net/Power Pin option to check if non-power nets are connected to power pins and vice-versa.
Schematic Only Component
Select, Schematic Only Component to check for Schematic-only Components in the design. That is, Parts with no footprint assigned and thus will not translate to PCB.
Dialog Switches
Acceptance Rule Set
The electrical rule switches that are shown in this dialog can be saved into the design to form the acceptance rule set. This is the set of rules that should be checked before the design is to be accepted as finished. Use the Load button to change the switches in the dialog to the acceptance set in the design, and the Save button to change the acceptance set in the design to the switches in the dialog. The summary at the end of the ERC report says if all acceptance checks were checked or not.
You can run the Acceptance Rules for ERC from a user defined report created in the Report Maker.
Error Markers
Clear Locked Errors
Check this box to cause locked Error Markers to be deleted. Error Markers are deleted, either when performing an Electrical Rules Check, or when using the Clear All Errors option. Normally, locked Error Markers are not deleted because they are considered to be marked as acceptable by the designer. If they are not deleted, the error is not reported during the Electrical Rules Check. This option will be disabled when there are no locked Error Markers to delete.
Clear All Errors
Normally, only the Error Markers of the type you are checking will be removed from the design prior to running the checker. If you want to remove all the errors in the design, press the Clear All Errors button. This button will be disabled when there are no errors in the design to delete.
On running Electrical Rules Check, if locked errors are present, the option will prompt to Clear locked errors? The option is defaulted to No, (to not clear locked errors).
Output
Check the Generate Report box to produce a report of all Errors Markers that are generated by this Electrical Rules Check session. Errors Markers that were already in the design prior to this session will not be included.
If generating a report, check the Report Rules Not Checked box to include a list of all rules not checked during the session.
Select the Show Errors Bar check box if you wish to run an ERC and display the error markers in the Errors Bar immediately.
Source
Use this to choose between checking the whole Design or just checking a Selection of items. If no items were pre-selected, this option is not available. If checking the Selection only, then each selected item will be checked against all other items (selected or not) in the design.
You can also choose to check Inside Named Area. The radio button is only available if there is a named area defined in the design. If there are multiple named areas, there will be a drop-down list with all the available named areas in the design.
Performing the checks
Press Check to perform the checks.
Press Close to leave the dialog, retaining any changes you have made in the dialog.
Press Cancel to leave the dialog, losing any changes made.
Electrical Rules Error Markers
When an error is found an Error Marker is added to the design on close to the error location. This Marker is displayed as a text string showing a Code for the type of error found.
For more information about a Electrical Rules Error, select the Error Marker in the design and use Properties. This will give details of the item(s) in error.
After an Electrical Rules Check, you can find the Error Markers in the design using one of two methods:
- Find Error - This option allows you to find Error Markers by specific type and cycle through them using a Next Error command.
- Electrical Rules Errors Browser
- Use this modeless dockable window to show you an ordered list of the Error Markers in the design. You can Double Click on an error in the list to find it in the design.
Related Topics
Add Page Link | Electrical Rules Errors Browser | Show Net Names | Technology - Pin Type Pair Rules | Online ERC