Validation

Updated: February 11, 2022

The Project | Validation region is used to validate a project, update PCB and schematic documents, import changes, and show differences. The region is available in the PCB, PCB library, schematic, and schematic library editors, although not all commands can be accessed from all editors as described on this page

The Validation region of the schematic (left) and PCB editors (right)

The commands within the Validation region will differ depending on the editor.

Validate

The Validate command is available from the PCB and schematic editors.

After launching the command, the software will check for logical, electrical, and drafting errors between the Dynamic Data Model (DDM) and the validation settings in the active project. Any violations that are detected by the validation process will be listed as warnings and/or errors in the Messages panel. An example of the Messages panel after validation is shown below.

Resolving Errors and Violations

It is important to address each warning or error that is detected. The default error settings tend to be conservative since it is better for the software to err on the side of being cautious and let you decide if the testing boundaries can be relaxed.

There will be situations when you want to test the entire design for a certain condition, but you want to ignore a warning/error at a specific point in the circuit. For example, you might want to allow a net to be renamed at a specific location, but only in that location. This can be done by placing a No ERC directive at that location.

The software can test for a large number of potential error conditions. Information is available about each error check on the Project Options page.

Tips

A project is currently active when one of its associated design documents is active in the main design space.
The validation process uses the options defined on the Error Reporting and Connection Matrix tabs of the Project Options dialog (as applicable to the project type) when checking the source documents for violations.
For a PCB design project, the Projects panel can also be used to browse components and nets for the design.

Update PCB Document

The Update PCB Document command is available from the schematic editor.

This command is used to update the PCB document associated with the project with changes made to the project's source documents. After launching the command, the Engineering Change Order (ECO) dialog opens. The dialog lists all modifications required to implement changes to one or more design documents in order to synchronize those documents.

Perhaps the most important and most often encountered situation for the use of the Engineering Change Order dialog is when synchronizing the source documents of the captured design and the target PCB implementation of that design. Changes on either side will always need to be pushed to the other side in order to maintain synchronicity, which is where the Engineering Change Order dialog comes into play.

Engineering Change Order Dialog

The dialog can also be accessed from the Differences between (described below) and Annotate dialog.

The dialog is divided into two main regions: Modifications and Status.

Modifications

This region of the dialog lists all modifications necessary to implement the changes required to bring about synchronization. Modifications are grouped by modification type. The entry at this group level reflects the number of modifications of that type. Each specific modification in this region is listed in terms of the following:

Enable - this option determines whether or not the modification will be included when the ECO is executed. Click directly on the checkbox to toggle its state between enabled/included (checked) and disabled/excluded (unchecked).
Action - the specific action to be carried out. The types of actions are dependent on what type of ECO needs to be done. Choices are: Add, Remove, or Modify.
Affected Object - the object affected by the action.
Affected Document - the document upon which the action will be carried out.

Multiple modifications can be selected in the list using standard multi-select techniques (Ctrl+click, Shift+click).

Right-click Menu

Enable/disable each modification entry as required, either individually or use the following commands available from the right-click menu to change the enabled state of multiple modifications:

Validate Changes - click to run a validation check on the modifications enabled for inclusion in the ECO. Validation results will appear in the Check column under the Status region of the dialog.
Execute Changes - click to execute the ECO. Execution results will appear in the Done column under the Status region of the dialog. Remember, only changes that pass the validation stage will be executed.
Create Report - click to generate a report for the modifications contained in the ECO. The report will be loaded into the Report Preview dialog.
Cross Probe - click to cross-probe to target and reference objects that are involved in a modification action on the associated schematic and PCB documents.
Expand All - click to expand the view of all modifications in the listing.
Contract All - click to contract the view of all modifications in the listing.

You can also expand or contract individual modification groupings using the controls to the left of the entry.

Enable All - use to enable all modifications.
Disable All - use to disable all modifications.
Enable Selected - use to enable all selected modifications.
Disable Selected - use to disable all selected modifications.
Enable all of same Kind - use to enable all modifications of the same modification type as the currently focused modification.
Disable all of same Kind - use to disable all modifications of the same modification type as the currently focused modification.
Invert Selection - use to quickly select all modifications not currently selected in the list and deselect those that are.

Status

This region of the dialog presents the following status information for each enabled modification:

Check - this field shows the result of running a validation check on the modification. A green check () means that the proposed change is supported and will be carried out upon execution of the ECO. A red x () means that the proposed change is invalid and will not be carried out when the ECO is executed.
Done - this field shows the result of the execution of the modification. A green check () means that the valid modification executed successfully.
Message - if the modification fails the validation stage, an entry will appear in this field (and also in the Messages panel) giving an indication as to why it failed.

You can close out of the dialog at any stage in order to investigate why certain changes are failing and make any design changes necessary.

Additional Controls

The following controls are available at the bottom of the dialog and in the right-click menu:

Validate Changes - click to run a validation check on the modifications enabled for inclusion in the ECO. Validation results will appear in the Check column in the Status region of the dialog.

It is important to validate the proposed modification actions before executing them. This tests the logic of your proposed changes.

Execute Changes - click to execute the ECO and effect the valid changes. Execution results will appear in the Done column in the Status region of the dialog. Only changes that pass the validation stage will be executed.
Report Changes - click to generate a report for the modifications contained in the ECO. The report will be loaded into the Report Preview dialog.

Keep in mind that the report will list all modification entries regardless of whether they validate and execute successfully.

Only Show Errors - check this option to only show Engineering Change Order errors. Validated changes will not be displayed. Showing only the list of errors will enable you to quickly review and make necessary changes to your design so that the resulting ECO validates completely.

Update Schematics

The Update Schematics command is available only from the PCB editor.

This command is used to update the schematic document(s) associated with the project with changes made in the PCB. After launching the command, the Engineering Change Order (ECO) dialog opens. The dialog lists all modifications required to implement changes to one or more design documents in order to synchronize those documents.

Refer to the Engineering Change Order Dialog section above for information.

Import Changes

The Import Changes command is available only from the PCB editor.

This command is used to import changes from the project's source documents. After launching the command, the Engineering Change Order (ECO) dialog opens. The dialog lists all modifications required to implement changes to one or more design documents in order to synchronize those documents.

Refer to the Engineering Change Order Dialog section above for information.

Show Differences

The Show Differences command is available from the schematic, schematic library, PCB, and PCB library editors.

After launching the command, the Choose Documents To Compare dialog opens. The dialog is used to choose which documents to compare. Comparison is performed using CircuitMaker's Comparator with any detected differences presented to you

Choose Document To Compare Dialog

The dialog in basic (left) and advanced (right) modes.

The dialog is available in two modes: a basic mode that allows you to quickly select the target PCB document to compare against the project's source document hierarchy, and an advanced mode that gives control over the documents compared (document-to-document, project-to-project, or document-to-project).

For use in basic mode, ensure the project of interest is currently focused in the panel.

Documents list - this region lists the documents that can, and selectively are, to be compared. The appearance depends on the mode as determined by the Advanced Mode option.
- Basic Mode - a single list will present the PCB documents for the focused design project. Choose the specific PCB document to compare against the design hierarchy of that project.
- Advanced Mode - two lists are presented, each displaying the currently open projects and their documents. Choose a document on the left to compare with a document on the right. You can choose to compare a document with another document, a project with another project, or a document with a project (as per basic mode).
Advanced - use to toggle the dialog between its basic mode (disabled) and its advanced mode (enabled).

After choosing the documents then clicking OK, the comparator will perform the comparison. The Comparator will adhere to the setup defined for it on the Comparator tab of the Project Options dialog and, if any differences are detected whose associated comparison types are not set to be ignored, those differences will appear in the Differences between dialog.

OK - click to open the Differences between dialog.

Differences Between Dialog

The Differences between dialog allows you to browse through differences that have been detected between documents chosen for comparison. For each difference, you can decide whether to update one of the documents or not, ultimately creating an Engineering Change Order in order to synchronize the documents as required.

The synchronizer is bi-directional. This means you can specify updates to both documents in the same ECO. In order to synchronize compared documents, the aim is to determine for each difference whether or not to take action and in which direction the change is made - specifying which document should be updated in order to remedy the difference.

The dialog is essentially divided into three main regions: Differences, Update and Change Order.

Differences

This region of the dialog lists all differences that the comparator has found between the chosen documents. Each difference is listed in the corresponding column for the document in which it resides. Differences are grouped by comparison type as listed and enabled on the Comparator tab of the Project Options dialog. The entry at this group level reflects the number of differences of that type.

Double-click on an entry to cross-probe to the object on the relevant source document.

Use the Expand All and Contract All commands on the right-click menu to quickly expand or contract all entries. You also can expand or contract individual comparison type groupings using the controls to the left of each entry.

When comparing the design hierarchy of a project to its PCB document, the column for the project side will be labeled with the name of the top-level schematic sheet.

Update

Use this region of the dialog to specify which document should be updated in order to remedy the difference. By default, all Decision entries initially have a decision of No Change applied to them.

Even if differences are detected, you are under no obligation to take action on them. The software will only synchronize the elements you specify.

The update decision for each difference can be individually determined by clicking on the associated entry in the Decision column then selecting the required update action in the subsequent ECO Decision dialog (described below). Choose the direction of the update (which of the compared documents to update) or No Updates at all.

Change Order

This region of the dialog lists the action to be taken for each difference that you decide to act upon, the object affected by the action, and the document upon which the action will be carried out. It is this information that is used to compile the subsequent ECO that will be used to create the updates. Common actions that will be listed in this area are:

Remove - where the update is in the direction of the document that contains the object causing the difference; the object will be removed.
Add - where the update is in the direction of the document that does not contain the object causing the difference; the object will be added.
Update - where both documents contain the same object that differs in some way; the object changed depends on the direction chosen.

If the Update Decision is No Change, there will be no action taken and the Change Order entry will be No Action.

Right-click Menu

Create Change Order - use to create an Engineering Change Order (ECO).
Generate Report - use to generate a report for the differences found by the Comparator. The update decisions you have decided to make and the actions will be included in the generated ECO. The report will be loaded into the Report Preview dialog. Use this dialog to browse the report, before ultimately exporting it to one of various supported formats or printing it directly.
<< Update All in - use to set the update direction for all differences to the left-hand document (where applicable).
Update All in >> - use to set the update direction for all differences to the right-hand document (where applicable).
Reverse Direction For All - use to quickly reverse the update direction for all differences (where applicable). If it is not valid to change the direction for a difference, the entry will be set to No Change.
Set No Action For All - use to quickly set the update decision for all differences to No Change.
<< Update Same Kind in - use to set the update direction for all differences of the same comparison type as the currently focused difference to the left-hand document (where applicable).
Update Same Kind in >> - use to set the update direction for all differences of the same comparison type as the currently focused difference to the right-hand document (where applicable).
Reverse Direction For Same Kind - use to quickly reverse the update direction for all differences of the same comparison type as the currently focused difference, where applicable. If it is not valid to change the direction for a difference, the entry will be set to No Change.
Set No Action For Same Kind - use to quickly set the update direction for all differences of the same comparison type as the currently focused difference to No Change.
<< Update Selected in - use to set the update direction for all selected differences to the left-hand document (where applicable).
Update Selected in >> - use to set the update direction for all selected differences to the right-hand document (where applicable).
Reverse Direction For Selected - use to quickly reverse the update direction for all selected differences (where applicable). If it is not valid to change the direction for a difference, the entry will be set to No Change.
Set No Action For Selected - use to quickly set the update decision for all selected differences to No Change.
Invert Selection - use to select all differences not currently selected in the list or deselect those that are.

Multiple differences can be selected in the list using standard multi-select techniques (Ctrl+click, Shift+click).

An update in a particular direction will only be set if it is valid to do so.

Additional Controls

The following buttons are available at the bottom of the dialog:

Create Engineering Change Order - click to generate an ECO. The Engineering Change Order dialog (described above) will open in which you can validate and execute the updates in order to synchronize the documents.
Report Differences - click to generate a report for the differences found by the Comparator. The update decisions you have decided to make and the actions will be included in the generated ECO. The report will be loaded into the Report Preview dialog. Use this dialog to browse the report before ultimately exporting it to one of various supported formats or printing it directly.
Explore Differences - click to investigate further the differences found by the Comparator prior to generating an ECO. The Differences between dialog will close and you will be returned to the main design space with the Differences panel open. The panel will contain all of the differences listed by the Comparator and in the same categories. Use the panel to cross probe to an object responsible for a difference on its parent document.

Exploring differences in this way will cause any update decisions you have made in the Differences between dialog to be lost. You will need to open the dialog again and redefine updates as required. Alternatively, you can cross probe to an object directly from within the Differences between dialog. Double-click the object's entry in the Differences region of the dialog. Since the Differences between dialog remains open, it is a good idea to have the source and target documents open and the dialog placed so that your view is not obscured.

ECO Decision Dialog

After choosing and comparing two documents, the Comparator lists any differences found between them. The ECO Decision dialog allows you to decide the direction of update (which of the compared documents to update) on an individual difference basis. It also allows you to specify that no update is required, which translates to no action being taken in either document.

In order to synchronize compared documents, the aim is to determine whether or not to take action for each difference and in which direction the change is made, specifying which document should be updated in order to remedy the difference.

Update Schematic - click to specify that the left-hand document is to be updated in order to resolve the difference.
Update PCB - click to specify that the right-hand document is to be updated in order to resolve the difference.

The dialog shows schematic and PCB sides for the update directions since the design hierarchy of the project is typically compared against the PCB document.

The dialog provides an indication of whether or not an update in a particular direction is valid. If valid, the left arrow and right arrow buttons (for an update to left or right, respectively) will be enabled. If a change is not supported, the corresponding button for that update direction will be grayed out.

No Updates - click to set the Update Decision to No Change (neither document is updated).

Printer-friendly version

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.