Altium NEXUS Documentation

DocumentOptions

Последнее изменение: Susan Riege; 11.12.2020

Parent page: WorkspaceManager Commands

The following pre-packaged resources, derived from this base command, are available:


Applied Parameters: ObjectKind=Project|Action=ParameterManagement

Summary

This command is used to run the Parameter Management feature, from where you can add, edit and remove parameters across the entire active project, or across an entire library. These are parameters that are 'owned' by various object kinds in the source schematic documents of the active project, or components in the active library. This provides a fast, efficient way to bring all parameters together in a single place for editing, with the ability to create an Engineering Change Order to implement any parameter changes you make, directly to each affected 'owner' design object.

Access

This command is accessed from the Schematic Editor, and Schematic Library Editor by choosing the Tools » Parameter Manager command, from the main menus.

Use

If you want to manage the parameters across the schematics of an entire project, first ensure that a schematic associated to the required project is open as the active document in the main design window. If you want to manage parameters for a particular schematic library, first ensure that that library is open as the active document.

After launching the command, the Parameter Editor Options dialog will appear. Use this dialog to define which parameters you wish to include in the edit. Simply enable/disable the inclusion of parameters owned by the various object kinds as required.

You can further refine the scope of object inclusion using the drop-down field in the center of the dialog. Choose to include all objects, only objects with existing parameters, or only objects with existing parameters that are actually used.

Should you wish to edit the parameters for only specific objects in the design, select these objects as required and enable the Selected Objects Only option. Only objects in your selection will be included, provided the relevant object kind has been enabled in the Include Parameters Owned By region of the dialog.

Having defined editor options as required, click OK to open the Parameter Table Editor dialog, from where you can proceed to add, edit and remove parameters as required. Changes are then implemented through an Engineering Change Order, that you create from this dialog.

Tips

  1. An option to Exclude System Parameters is also available in the Parameter Editor Options dialog. These parameters include things like component model settings, document parameters that were defined in the template, and so on. This option is best explored when you are more familiar with managing parameters.


Applied Parameters: ObjectKind=Project|Action=ViewChannels

Summary

This command is used to run the Project Components dialog for the active project, from where you can view all components used in the project - across all source schematic documents - in terms of logical and physical designators, and across all defined channels (thereby supporting a quick view of designations in a multi-channel design).

Access

This command is accessed from the active document's editor by choosing the Project » View Channels command, from the main menus (where available).

Use

First, ensure that the project whose components you wish to view, is the active project. This is done by opening one of its associated documents (such as a schematic, or the PCB), as the active document in the main design window.

After launching the command, the source schematic documents for the active project are compiled and the Project Components dialog appears. The dialog lists, for each of the source schematic documents of the active project, the logical and physical designators assigned to each of the components, as well as the associated component comment.

If the design is not multi-channel, the physical designators will be listed in a single column, named Single Channel. If multiple channels have been used in the design, columns are added for each channel available, in order to show the unique physical designators that are used for each channel on the PCB document.

Tips

  1. Logical designators are those designators assigned to the components of the source schematics. Physical designators are those designators that are assigned to the components once they are placed in the PCB design. This is particularly relevant when considering multi-channel designs. The logical designators for the replicated channel components may be the same, but each component must have a unique physical designator in the PCB design.
  2. For multi-channel designs, changes to the component designator format are carried out on the Multi-Channel tab of the Options for Project dialog.
  3. All schematic source documents are required to be open for compilation. These documents are opened and automatically hidden in order to prevent clutter in the tabbed area of the main design window. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window.
  4. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - .


Applied Parameters: ObjectKind=FocusedProject|Action=ViewChannels

Summary

This command is used to run the Project Components dialog for the focused project, from where you can view all components used in the project - across all source schematic documents - in terms of logical and physical designators, and across all defined channels (thereby supporting a quick view of designations in a multi-channel design).

Access

This command can be accessed from the Projects panel by:

  • Right-clicking on the entry for the required project (or one of its source documents) and choosing the View Channels command, from the context menu.
  • Clicking to focus the required project (or one of its source documents), then clicking the Project button and choosing the View Channels command from the context menu.

Use

After launching the command, the source schematic documents for the focused project are compiled and the Project Components dialog appears. The dialog lists, for each of the source schematic documents of the focused project, the logical and physical designators assigned to each of the components, as well as the associated component comment.

If the design is not multi-channel, the physical designators will be listed in a single column, named Single Channel. If multiple channels have been used in the design, columns are added for each channel available, in order to show the unique physical designators that are used for each channel on the PCB document.

Tips

  1. Logical designators are those designators assigned to the components of the source schematics. Physical designators are those designators that are assigned to the components once they are placed in the PCB design. This is particularly relevant when considering multi-channel designs. The logical designators for the replicated channel components may be the same, but each component must have a unique physical designator in the PCB design.
  2. For multi-channel designs, changes to the component designator format are carried out on the Multi-Channel tab of the Options for Project dialog.
  3. All schematic source documents are required to be open for compilation. These documents are opened and automatically hidden in order to prevent clutter in the tabbed area of the main design window. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window.
  4. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - .


Applied Parameters: ObjectKind=Project|Action=ComponentLinking

Summary

This command is used to run the Edit Component Links dialog for the active project, from where you can check and control the status of the links between schematic components and their corresponding PCB component footprints. When a component is placed on a schematic sheet, it is automatically given a unique ID. As a precursor to comparison, Altium NEXUS scans the source schematic and target PCB documents for linked components. These are components that have been previously synchronized with one another and share a unique ID. If components have not yet been synchronized between documents, a dialog will appear alerting you to this fact and allowing components to be matched either automatically - by designator - or in a manual fashion. The Edit Component Links dialog provides controls to manually match and link components between the two domains.

It is a good idea to have all components matched using unique IDs so that annotation of designators in either the schematic or PCB document can be carried out with the knowledge that the documents can still be re-synchronized at any stage. The documents can still be synchronized even if components aren't matched by unique IDs, but in this case, you will be prompted to match the components by designators only - comment and footprint are not taken into account, and therefore it is possible that matching of some components is carried out incorrectly.

Access

This command is accessed from the PCB Editor by choosing the Project » Component Links command, from the main menus.

The reason that manual linking of components is only carried out from within the PCB document, is that only the PCB component footprints need to be updated with the unique ID information - it is already present on the schematic side.

Use

First ensure that the PCB document for the project is the active document in the main design window.

After launching the command, the Edit Component Links dialog will appear. The dialog essentially shows those components that have been matched and are linked by a unique ID, and those that are currently unmatched (and are therefore not linked by a unique ID). Use the dialog to match any components that remain unmatched - you can attempt to match by Designator and/or Comment and/or Footprint.

Once you have defined component linking as required, click the Perform Update button to effect the changes. If you have moved any entries in the Matched section of the dialog back into the Unmatched sections, a confirmation dialog will appear advising that existing component associations will be broken by proceeding. Clicking Yes will proceed with the update and an information dialog will appear giving a summary of the component links modified in the PCB document. A new entry in the Matched section is summarized as a Link Modified, whilst a previously linked entry that you have now unmatched is summarized as a Link Removed.

Tips

  1. Use the dialog at any stage during the design, to view the linking between components and to reassure yourself that the components on the schematic source documents are indeed correctly matched to the corresponding component footprints in the PCB design.
  2. When component information is transferred for the first time between schematic source documents and a blank PCB design document, using the Synchronizer, all components will automatically be linked by unique ID - the ID information from each schematic component being assigned to the corresponding component footprint.
  3. Unique IDs can be removed at any time by moving the linked components back to the unmatched regions of the Edit Component Links dialog. Removing a component link will remove the unique ID from the corresponding PCB footprint only. The schematic component retains the unique ID, unless a new one is generated (using a reset unique ID-related command, at either the schematic or component level).
  4. A unique ID is also automatically assigned to each parameter definition on a source schematic document. This is used for those parameters that have been added as design rule directives. When transferring the design to the PCB document, any defined rule parameters will be used to generate the relevant design rules in the PCB. These generated rules will be given the same unique IDs, allowing rule constraints to be changed in either schematic or PCB and those changes pushed across when performing a synchronization.


Applied Parameters: ObjectKind=FocusedProject|Action=ComponentLinking

Summary

This command is used to run the Edit Component Links dialog for the focused project, from where you can check and control the status of the links between schematic components and their corresponding PCB component footprints. When a component is placed on a schematic sheet, it is automatically given a unique ID. As a precursor to comparison, Altium NEXUS scans the source schematic and target PCB documents for linked components. These are components that have been previously synchronized with one another and share a unique ID. If components have not yet been synchronized between documents, a dialog will appear alerting you to this fact and allowing components to be matched either automatically - by designator - or in a manual fashion. The Edit Component Links dialog provides controls to manually match and link components between the two domains.

It is a good idea to have all components matched using unique IDs so that annotation of designators in either the schematic or PCB document can be carried out with the knowledge that the documents can still be re-synchronized at any stage. The documents can still be synchronized even if components aren't matched by unique IDs, but in this case, you will be prompted to match the components by designators only - comment and footprint are not taken into account, and therefore it is possible that matching of some components is carried out incorrectly.

Access

This command can be accessed from the Projects panel by:

  • Right-clicking on the entry for the source PCB document of the required project and choosing the Component Links command, from the context menu.
  • Clicking to focus the source PCB document of the required project, then clicking the Project button and choosing the Component Links command from the context menu.
The reason that manual linking of components is only carried out from the PCB document, is that only the PCB component footprints need to be updated with the unique ID information - it is already present on the schematic side.

Use

After launching the command, the Edit Component Links dialog will appear. The dialog essentially shows those components that have been matched and are linked by a unique ID, and those that are currently unmatched (and are therefore not linked by a unique ID). Use the dialog to match any components that remain unmatched - you can attempt to match by Designator and/or Comment and/or Footprint.

Once you have defined component linking as required, click the Perform Update button to effect the changes. If you have moved any entries in the Matched section of the dialog back into the Unmatched sections, a confirmation dialog will appear advising that existing component associations will be broken by proceeding. Clicking Yes will proceed with the update and an information dialog will appear giving a summary of the component links modified in the PCB document. A new entry in the Matched section is summarized as a Link Modified, whilst a previously linked entry that you have now unmatched is summarized as a Link Removed.

Tips

  1. Use the dialog at any stage during the design, to view the linking between components and to reassure yourself that the components on the schematic source documents are indeed correctly matched to the corresponding component footprints in the PCB design.
  2. When component information is transferred for the first time between schematic source documents and a blank PCB design document, using the Synchronizer, all components will automatically be linked by unique ID - the ID information from each schematic component being assigned to the corresponding component footprint.
  3. Unique IDs can be removed at any time by moving the linked components back to the unmatched regions of the Edit Component Links dialog. Removing a component link will remove the unique ID from the corresponding PCB footprint only. The schematic component retains the unique ID, unless a new one is generated (using a reset unique ID-related command, at either the schematic or component level).
  4. A unique ID is also automatically assigned to each parameter definition on a source schematic document. This is used for those parameters that have been added as design rule directives. When transferring the design to the PCB document, any defined rule parameters will be used to generate the relevant design rules in the PCB. These generated rules will be given the same unique IDs, allowing rule constraints to be changed in either schematic or PCB and those changes pushed across when performing a synchronization.


Applied Parameters: ObjectKind=Project|Action=ImplementationManagement|ModelType=PCBLIB

Summary

This command is used to run the Footprint Manager, which enables you to review all footprints associated with each and every component in the active project. The Footprint Manager makes it easy to review and detect problems with footprint assignments across the entire design, particularly useful when you are working on a legacy design or one from another organization.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Footprint Manager command, from the main menus.

Use

First, ensure that a schematic source document, associated to the required project, is open as the active document in the main design window.

After launching the command, the Footprint Manager dialog will appear, presenting a list of all components across all source design schematics in the active project. Use the controls available on the right-hand side of the dialog to manage the footprints available to, and in current use by, the design's components. Features include:

  • Ability to add, edit, and remove footprint models for one or more selected components.
  • Copy footprints between components.
  • Changing current footprint assignment (the footprint that will currently be used to represent a component in the PCB domain, from multiple that may be available to that component).
  • Footprint validation - to ensure that footprint models are truly available, and especially those set to be the current model.

Once all changes to footprint model assignments have been made as required, those changes are then implemented through a standard Engineering Change Order (ECO). To do this, simply click on the Accept Changes (Create ECO) button, at the bottom-right of the Footprint Manager dialog.

Tips

  1. For a design containing device sheets, the components on those sheets will only be listed provided the sheets are not marked as being Read-only. Toggle the Read-only state for device sheets in projects from the Data Management - Device Sheets page of the Preferences dialog.


Applied Parameters: ObjectKind=Project|Action=PCBConfigurations

Summary

This command is used to access the Configuration Manager dialog, from where you can define and manage the configurations for the active/focused PCB design project. Configurations are part of the actual design project and provide the link from the design world to the manufacturing world. Each configuration represents an Item that we want to build in the real world, defining the data that will be required by a manufacturing organization to actually build that Item. When we release a board design project, we are in fact releasing a configuration of that project. The data generated from a configuration can be considered a specific set of "instructions", with which to build the Item.

Access

This command can be accessed for the active project, or a focused project:

  • Active project - with a source document for the project open as the active document, choose the Project » Configuration Manager command, from the main menus.
  • Focused project - access is made from the Projects panel by:
    • Right-clicking on the entry for the required project and choosing the Configuration Manager command, from the context menu.
    • Clicking to focus the required project, then clicking the Project button and choosing the Configuration Manager command from the context menu.

Use

After launching the command, the Configuration Manager dialog will appear. Use the dialog to create and configure configurations for the project as required. Each configuration of a PCB project on the design side, maps to a specific Item on the manufacturing side. As its output is simply a generated set of instructions, or 'blueprint' for how to make the Item, a configuration simply needs to define which variant and associated project Output Job files to be used, and nominate which Item - in the chosen Altium Vault - to target.

In summary, the formal set of elements used to define a configuration for a PCB project are:

  • Its name
  • Which variant it uses (if any)
  • The specific Item it is targeting. To successfully release, the configuration must point to a revision of that Item that is in the Planned state.
  • Which Output Job file(s) will drive the generation of its outputs – the instructions from which the targeted Item will be produced. A particular Output Job file can also include validation outputs, by which to constrain the release process, ensuring the design source used in the release is of the highest integrity.

When releasing a board design, a configuration can map to one of three types of Item:

  • Blank Board (altium-pcb-blank) – this type of Item is used to produce a fabricated bare board, containing no components.
  • Assembled Board (altium-pcb-assembly) – this type of Item is used to produce a Blank Board Item that is populated with components in accordance with a generated BOM.
  • PCB Design (altium-pcb-design) – this type of Item is essentially used to gather together all documentation - fabrication, assembly, and any other documentation - in a single place, a released 'master' copy of the design as it were.

The beauty of the Configuration Manager is its intuitive simplicity - enabling you to define the configurations you require with streamlined efficiency. For each configuration, simply specify a particular variant to be used (if applicable and/or required), assign which Output Job file(s) to be used, and browse the nominated Altium Vault to choose the Item to target (or map) the configuration to. Don't forget to give each configuration a meaningful name, so that you can easily distinguish the purpose of each!

After making all changes as required, click OK to save the configuration information with the PCB project.

Tips

  1. When the Configuration Manager dialog is first accessed for a PCB project, you will notice a single base configuration is automatically added - with the name Default Configuration. The configuration is set to ignore variants (that is, include all components if targeting an assembled board Item), and is not mapped to any Item. Any Output Job files you have added to the project will also be listed, but are not assigned to the configuration.
  2. Each configuration must be given a unique name, and must map to a unique Item in the vault.
  3. Note that variant settings made in an Output Job file are overridden by the variant specified in the Configuration Manager dialog.
  4. The Configuration Manager dialog can also be quickly accessed through various controls in the PCB Release View, when using the board design release process.
  5. If a configuration has been released, then to release that configuration again requires a new revision of the target Item to be created. Once a new planned revision of the Item is created, you will need to go back to the Configuration Manager dialog and point to that revision. And as updating the configuration modifies the project file, don't forget to save and commit to the Design Repository, otherwise the Design Source region in the PCB Release View will not be in a synchronized state, and you will not be able to proceed with the release.
  6. If you are not using Altium's Vault technology, but still want to use the board release process, simply select [None] for the Target Vault in the Configuration Manager dialog. This enables you to still use the process, with defined configurations, to generate the required manufacturing data. You simply won't be releasing/committing data to a target vault.


Applied Parameters: ObjectKind=Project|Action=VariantManagement

Summary

This command is used to run the Variant Management dialog, from where you can add, remove and edit variants for the active PCB design project. The ability to create variations of the same base design is a real strength of Altium NEXUS, and a tremendous productivity booster for designers. Using variants, you can define any number of variations of the base design, configuring each component to be: fitted; not fitted; fitted with modified component parameters, such as the component's value; or you can completely replace a component with an alternate part. Variants that use any of these types of variations are all referred to as Assembly Variants, as they only impact on the assembly process - all variants share the same fabricated bare board. There is also support for variations to component overlay information on the PCB, for example changing a component's comment. This type of variation requires two overlay screens to be produced, resulting in two different bare boards. This type of variant is referred to as a Fabrication Variant.

For an in-depth walk-through of Altium NEXUS's capabilities with respect to variants, see Design Variants.

Access

This command can be accessed from the Schematic Editor, and PCB Editor, by:

  • Choosing the Project » Variants command, from the main menus.
  • Clicking the  button on the Variants toolbar.

Use

First, ensure that a source schematic, or PCB document, for the project whose variants you wish to manage, is open as the active document in the main design window.

After launching the command, the Variant Management dialog will appear. The dialog presents two distinct regions of information:

  • Components - lists all of the components in the base design.
  • Component Parameters - details all of the parameters of the component(s) currently selected in the upper region.

Use the dialog to create variants of the original (base) design, and determine how each is populated, in terms of its components, in order to create different (varied) products as required. The following component variations are supported:

  • Fitted - this is the default state of a component, if it is Fitted, then it is not varied. When you create a new variant, all components default to Fitted. A component with a state of Fitted is represented in the Variant Management dialog as an empty cell.
  • Not Fitted - if a component is set to Not Fitted, it still exists on the schematic and is transferred to the PCB, but it is removed from the appropriate output documentation, such as the BoM. For a Not Fitted component the cell displays the text Not Fitted. You can also configure how Not Fitted components are presented in the documentation, for example they can be marked with a cross on the schematic and in PCB drawing outputs.
  • Alternate Part - it is also possible to select an entirely different component, as an Alternate Part. Once chosen, the cell displays the alternate part's Library Link. Since the Alternate Part is a different component, only one or the other component is presented on the compiled tab of the compiled schematic sheet. There is also the requirement that the alternate part shares the same set of pins, placed in the same locations, as the base part. This is an essential requirement to ensure the connectivity remains valid when the design is compiled.
After selecting an alternate part, the software checks for pin-compatibility between the chosen alternate component, and the original base design component. To be pin-compatible, the alternate must have the same number of pins as the original component, and those pins must be identical in their location, and electrical type. No equality in the graphical primitives used in the symbols for the two components is required. If the software detects that the alternate component is not pin-compatible, a Confirm dialog will appear, requiring your OK to proceed with the replacement. While you can proceed with the use of a pin-incompatible alternate component, bear in mind the potential impact on the wiring, and that you may also encounter an error violation when performing a subsequent compilation of the design.

In addition, you can also vary any of a fitted component's parameters. Modifying the value of a parameter is a local variation, only affecting the output documentation. The original schematic, and the component whose parameter is being varied, are not modified in any way.

Once variants and their configurations have been defined as required, click OK to save those configurations.

Tips

  1. To examine design variations, you must compile the design and then switch to the compiled tab of the schematic (thereby viewing the physical design). Choose the required variant using the Variants toolbar, to show the configuration of the physical components on that sheet.
  2. Alternate part variations within the channel of a multi-channel design are not supported.
  3. Double-click on a component in the Variant Management dialog to jump to that component on the schematic.
  4. It is often easier to work directly from the component(s) placed on the schematic sheet, rather than scrolling up and down through a list of components in a dialog. Simply select the component(s) on the sheet, then right-click and select Part Actions » Variants from the context menu. The Variant Management dialog will open, displaying only the selected components. In addition to only presenting the selected component(s) in the Variant Management dialog, if there is a variant currently selected in the Variants toolbar, then only that variant will be presented, irrespective of how many variants might actually be defined for the project.
  5. Variant settings are stored in the project file (*.PrjPcb). When the Variant Management dialog is opened, this data is read and analyzed, then loaded into the Variant Management dialog. If there are issues detected during data loading, such as mismatches between component designators or component UIDs, an Information dialog will open outlining the problem. Component UID mismatches are automatically resolved, simply close the dialog and save the project to retain these corrections. Duplicate designators must be resolved at the schematic level, recompile the project and check the Messages panel for warning/error details to resolve these.
  6. There are two ways an Alternate Part is handled on the PCB:
    1. If the footprint is the same - if the chosen Alternate Part has the same footprint name as the base part, then only one instance of that footprint will be transferred to the PCB. As multiple footprints can be assigned to a component, you should ensure that the correct footprint is selected in the Variant Management dialog for each variant.
    2. If the footprint changes - if the chosen Alternate Part has a different footprint name from the base part, then both footprints are transferred to the PCB. As the designer you must then decide how to position the two footprints on the PCB. Note that both footprints will have the same designator, as only one or the other component is ever fitted.


Applied Parameters: ObjectKind=FocusedProject|Action=VariantManagement

Summary

This command is used to run the Variant Management dialog, from where you can add, remove and edit variants for the focused PCB design project. The ability to create variations of the same base design is a real strength of Altium NEXUS, and a tremendous productivity booster for designers. Using variants, you can define any number of variations of the base design, configuring each component to be: fitted; not fitted; fitted with modified component parameters, such as the component's value; or you can completely replace a component with an alternate part. Variants that use any of these types of variations are all referred to as Assembly Variants, as they only impact on the assembly process - all variants share the same fabricated bare board. There is also support for variations to component overlay information on the PCB, for example changing a component's comment. This type of variation requires two overlay screens to be produced, resulting in two different bare boards. This type of variant is referred to as a Fabrication Variant.

For an in-depth walk-through of Altium NEXUS's capabilities with respect to variants, see Design Variants.

Access

This command can be accessed from the Projects panel by:

  • Right-clicking on the entry for the required project (or one of its source documents) and choosing the Variants command, from the context menu.
  • Clicking to focus the required project (or one of its source documents), then clicking the Project button and choosing the Variants command from the context menu.

Use

After launching the command, the Variant Management dialog will appear. The dialog presents two distinct regions of information:

  • Components - lists all of the components in the base design.
  • Component Parameters - details all of the parameters of the component(s) currently selected in the upper region.

Use the dialog to create variants of the original (base) design, and determine how each is populated, in terms of its components, in order to create different (varied) products as required. The following component variations are supported:

  • Fitted - this is the default state of a component, if it is Fitted, then it is not varied. When you create a new variant, all components default to Fitted. A component with a state of Fitted is represented in the Variant Management dialog as an empty cell.
  • Not Fitted - if a component is set to Not Fitted, it still exists on the schematic and is transferred to the PCB, but it is removed from the appropriate output documentation, such as the BoM. For a Not Fitted component the cell displays the text Not Fitted. You can also configure how Not Fitted components are presented in the documentation, for example they can be marked with a cross on the schematic and in PCB drawing outputs.
  • Alternate Part - it is also possible to select an entirely different component, as an Alternate Part. Once chosen, the cell displays the alternate part's Library Link. Since the Alternate Part is a different component, only one or the other component is presented on the compiled tab of the compiled schematic sheet. There is also the requirement that the alternate part shares the same set of pins, placed in the same locations, as the base part. This is an essential requirement to ensure the connectivity remains valid when the design is compiled.
After selecting an alternate part, the software checks for pin-compatibility between the chosen alternate component, and the original base design component. To be pin-compatible, the alternate must have the same number of pins as the original component, and those pins must be identical in their location, and electrical type. No equality in the graphical primitives used in the symbols for the two components is required. If the software detects that the alternate component is not pin-compatible, a Confirm dialog will appear, requiring your OK to proceed with the replacement. While you can proceed with the use of a pin-incompatible alternate component, bear in mind the potential impact on the wiring, and that you may also encounter an error violation when performing a subsequent compilation of the design.

In addition, you can also vary any of a fitted component's parameters. Modifying the value of a parameter is a local variation, only affecting the output documentation. The original schematic, and the component whose parameter is being varied, are not modified in any way.

Once variants and their configurations have been defined as required, click OK to save those configurations.

Tips

  1. To examine design variations, you must compile the design and then switch to the compiled tab of the schematic (thereby viewing the physical design). Choose the required variant using the Variants toolbar, to show the configuration of the physical components on that sheet.
  2. Alternate part variations within the channel of a multi-channel design are not supported.
  3. Double-click on a component in the Variant Management dialog to jump to that component on the schematic.
  4. It is often easier to work directly from the component(s) placed on the schematic sheet, rather than scrolling up and down through a list of components in a dialog. Simply select the component(s) on the sheet, then right-click and select Part Actions » Variants from the context menu. The Variant Management dialog will open, displaying only the selected components. In addition to only presenting the selected component(s) in the Variant Management dialog, if there is a variant currently selected in the Variants toolbar, then only that variant will be presented, irrespective of how many variants might actually be defined for the project.
  5. Variant settings are stored in the project file (*.PrjPcb). When the Variant Management dialog is opened, this data is read and analyzed, then loaded into the Variant Management dialog. If there are issues detected during data loading, such as mismatches between component designators or component UIDs, an Information dialog will open outlining the problem. Component UID mismatches are automatically resolved, simply close the dialog and save the project to retain these corrections. Duplicate designators must be resolved at the schematic level, recompile the project and check the Messages panel for warning/error details to resolve these.
  6. There are two ways an Alternate Part is handled on the PCB:
    1. If the footprint is the same - if the chosen Alternate Part has the same footprint name as the base part, then only one instance of that footprint will be transferred to the PCB. As multiple footprints can be assigned to a component, you should ensure that the correct footprint is selected in the Variant Management dialog for each variant.
    2. If the footprint changes - if the chosen Alternate Part has a different footprint name from the base part, then both footprints are transferred to the PCB. As the designer you must then decide how to position the two footprints on the PCB. Note that both footprints will have the same designator, as only one or the other component is ever fitted.


Applied Parameters: ObjectKind=Project|Action=All

Summary

This command is used to access the Options for Project dialog, from where you can set up project-specific options for the active project.

Access

With a document for the required project open as the active document, this command is accessed from that document's editor by choosing the Project » Project Options command, from the main menus.

Use

First, ensure that one of the target project's associated design documents is open as the active document in the main design window.

After launching the command, the Options for Project dialog will appear. The dialog is divided over a number of tabs, the availability and content of which, depends on the specific project type:

  • Error Reporting - enables you to define the reporting levels for each of the possible electrical and drafting violations that can exist on source schematic documents when compiling the project. When the project is compiled, these violation settings will be used - in conjunction with the defined settings on the Connection Matrix tab - to test the source documents for violations.
There may be points in the design that you know will be flagged as electrical violations, which you do not want to be flagged. To suppress these, place a No ERC schematic design directive object at each point.
  • Connection Matrix - delivers a matrix providing a mechanism to establish connectivity rules between component pins and net identifiers, such as Ports and Sheet Entries. It defines the logical or electrical conditions that are to be reported as warnings or errors. For example, an output pin connected to another output pin would normally be regarded as an error condition, but two connected passive pins would not. When the project is compiled, these violation settings will be used - in conjunction with the defined settings on the Error Reporting tab - to test the source documents for violations.
  • Class Generation - enables you to configure and control class generation. Classes are a logical collection of a particular type of design object. For example, a group of related components could be grouped into their own Component Class, which could then be used as the basis for creating a targeted rule. This tab provides controls to determine which classes are automatically generated, and which user-defined classes are generated when the source schematic documents are synchronized with the PCB design document.
  • Comparator - enables you to define which types of differences to find and which to ignore when comparing documents.
  • ECO Generation - enables you to configure which modification types can be included when generating an Engineering Change Order (ECO) based on differences found by the Comparator. Configuration of modification types on this tab should be performed in conjunction with configuration of the comparison types on the Comparator tab.
  • Options - enables you to specify the output path and related options for generated outputs for the project. You can also specify various netlisting options and the Net Identifier Scope.
The scope of net identifiers should be determined at the beginning of the design process.
  • Multi-Channel - enables you to define the room naming scheme and component designator format for use with multi-channel designs.
To check your multi-channel designators, you can view all components used across all source schematic documents in the project in terms of logical and physical designators. This is performed in the Project Components dialog.
For more detail on the concept of multi-channel design, see Multi-Sheet and Multi-Channel Design.
  • Default Prints - enables you to set up the default print outputs for various document types. It is these nominated defaults that are used when running the print command from the applicable editors' main menus.
  • Search Paths - enables you to specify search paths to library and model files for the project.
The libraries found along specified search paths, along with Project Libraries and Installed Libraries, constitute the set of libraries that are available to a project - the Available Libraries. When the available libraries are interrogated as part of model-link verification and the required model is not tied to an integrated library, or a fully specified file, the search order is: Project Libraries > Installed Libraries > Search Path Libraries. In each case, libraries are searched in top-down order, with user-control over this order. The search stops when the first match for the model is found.
  • Parameters - enables you to manage parameters defined for the project, often referred to as project-level parameters. Parameters defined at the project level are available for use across all schematic sheets and PCB documents in the project, through the use of special strings (=<ProjectParameterName> on a schematic, and .<ProjectParameterName> on a PCB).
Altium NEXUS supports parameters at various levels of the project - project-level parameters, document-level parameters (defined for a schematic sheet), and variant-level parameters. They also have a hierarchy, which means you can create a parameter with the same name at different levels of the project, each having different values. Altium NEXUS resolves this with the following order of precedence: Variant (highest priority) ---> Schematic Document ---> Project (lowest priority). That means the parameter value defined in the schematic document overrides the value defined in the project options, and the value defined in the variant overrides the value defined in the schematic document. (Note that schematic-level parameters are not available on the PCB or in the BOM; for these types of outputs you should use project or variant parameters.)
  • Device Sheets - enables you to specify device sheet folders for the project. Device Sheets are building blocks developed with the intent of being re-used in different designs. They usually contain predefined circuits which are commonly used between projects. Device Sheets are stored as normal Schematic Documents in special Device Sheet Folders. They are placed and referenced in your project, similarly to a simple component. When the project is compiled, Device Sheets are included in the project hierarchy.
Device sheet folders can also be managed from the Data Management - Device Sheets page of the Preferences dialog. This allows device sheets to be made available to all design projects. This page also provides additional options, such as controlling whether or not editing of device sheets is allowed (typically a device sheet would be edited outside of the project it is used, and therefore kept Read-Only when brought into a project).
For more detail on Device Sheets, and their use, see Device Sheets.
  • Managed OutputJobs - enables you to add one or more Output Jobs to the project, that are available from (have been released into) an Altium Vault. Once the project has been saved and recompiled – the chosen managed OutJob(s) will appear in the Projects panel.
If an environment configuration is currently in-force, then you will only be able to add Output Job Items defined for use by that configuration. For more information, see Environment Configuration Management.

After making any changes to project options, click OK to close the dialog, and then be sure to save the project file, which is where the options are stored.

Tips

  1. You can set all options, across all tabs, back to their defaults at the time of original installation. To do this, simply click the Set To Installation Defaults button, at the bottom-left of the Options for Project dialog.
  2. The process of compiling is integral to producing a valid netlist for a project. In fact it is the process of compilation that yields the unified data model of a design. Carefully check and resolve all reported errors prior to netlist generation.
  3. For a comprehensive reference describing each of the possible electrical and drafting violations that can exist on source documents when compiling a project, refer to the Project Compiler Violations Reference.
  4. When not using centralized environment configuration, or when the configuration chosen has no defined OutJobs, you are free to create new, unmanaged Output Job files, in addition to using those from a vault, should this be required.


Applied Parameters: ObjectKind=FocusedProject|Action=All

Summary

This command is used to access the Options for Project dialog, from where you can set up project-specific options for the focused project.

Access

This command can be accessed from the Projects panel by:

  • Right-clicking on the entry for the required project and choosing the Project Options command, from the context menu.
  • Clicking to focus the required project, then clicking the Project button and choosing the Project Options command from the context menu.

Use

After launching the command, the Options for Project dialog will appear. The dialog is divided over a number of tabs, the availability and content of which, depends on the specific project type:

  • Error Reporting - enables you to define the reporting levels for each of the possible electrical and drafting violations that can exist on source schematic documents when compiling the project. When the project is compiled, these violation settings will be used - in conjunction with the defined settings on the Connection Matrix tab - to test the source documents for violations.
There may be points in the design that you know will be flagged as electrical violations, which you do not want to be flagged. To suppress these, place a No ERC schematic design directive object at each point.
  • Connection Matrix - delivers a matrix providing a mechanism to establish connectivity rules between component pins and net identifiers, such as Ports and Sheet Entries. It defines the logical or electrical conditions that are to be reported as warnings or errors. For example, an output pin connected to another output pin would normally be regarded as an error condition, but two connected passive pins would not. When the project is compiled, these violation settings will be used - in conjunction with the defined settings on the Error Reporting tab - to test the source documents for violations.
  • Class Generation - enables you to configure and control class generation. Classes are a logical collection of a particular type of design object. For example, a group of related components could be grouped into their own Component Class, which could then be used as the basis for creating a targeted rule. This tab provides controls to determine which classes are automatically generated, and which user-defined classes are generated when the source schematic documents are synchronized with the PCB design document.
  • Comparator - enables you to define which types of differences to find and which to ignore when comparing documents.
  • ECO Generation - enables you to configure which modification types can be included when generating an Engineering Change Order (ECO) based on differences found by the Comparator. Configuration of modification types on this tab should be performed in conjunction with configuration of the comparison types on the Comparator tab.
  • Options - enables you to specify the output path and related options for generated outputs for the project. You can also specify various netlisting options and the Net Identifier Scope.
The scope of net identifiers should be determined at the beginning of the design process.
  • Multi-Channel - enables you to define the room naming scheme and component designator format for use with multi-channel designs.
To check your multi-channel designators, you can view all components used across all source schematic documents in the project in terms of logical and physical designators. This is performed in the Project Components dialog.
For more detail on the concept of multi-channel design, see Multi-Sheet and Multi-Channel Design.
  • Default Prints - enables you to set up the default print outputs for various document types. It is these nominated defaults that are used when running the print command from the applicable editors' main menus.
  • Search Paths - enables you to specify search paths to library and model files for the project.
The libraries found along specified search paths, along with Project Libraries and Installed Libraries, constitute the set of libraries that are available to a project - the Available Libraries. When the available libraries are interrogated as part of model-link verification and the required model is not tied to an integrated library, or a fully specified file, the search order is: Project Libraries > Installed Libraries > Search Path Libraries. In each case, libraries are searched in top-down order, with user-control over this order. The search stops when the first match for the model is found.
  • Parameters - enables you to manage parameters defined for the project, often referred to as project-level parameters. Parameters defined at the project level are available for use across all schematic sheets and PCB documents in the project, through the use of special strings (=<ProjectParameterName> on a schematic, and .<ProjectParameterName> on a PCB).
Altium NEXUS supports parameters at various levels of the project - project-level parameters, document-level parameters (defined for a schematic sheet), and variant-level parameters. They also have a hierarchy, which means you can create a parameter with the same name at different levels of the project, each having different values. Altium NEXUS resolves this with the following order of precedence: Variant (highest priority) ---> Schematic Document ---> Project (lowest priority). That means the parameter value defined in the schematic document overrides the value defined in the project options, and the value defined in the variant overrides the value defined in the schematic document. (Note that schematic-level parameters are not available on the PCB or in the BOM; for these types of outputs you should use project or variant parameters.)
  • Device Sheets - enables you to specify device sheet folders for the project. Device Sheets are building blocks developed with the intent of being re-used in different designs. They usually contain predefined circuits which are commonly used between projects. Device Sheets are stored as normal Schematic Documents in special Device Sheet Folders. They are placed and referenced in your project, similarly to a simple component. When the project is compiled, Device Sheets are included in the project hierarchy.
Device sheet folders can also be managed from the Data Management - Device Sheets page of the Preferences dialog. This allows device sheets to be made available to all design projects. This page also provides additional options, such as controlling whether or not editing of device sheets is allowed (typically a device sheet would be edited outside of the project it is used, and therefore kept Read-Only when brought into a project).
For more detail on Device Sheets, and their use, see Device Sheets.
  • Managed OutputJobs - enables you to add one or more Output Jobs to the project, that are available from (have been released into) an Altium Vault. Once the project has been saved and recompiled – the chosen managed OutJob(s) will appear in the Projects panel.
If an environment configuration is currently in-force, then you will only be able to add Output Job Items defined for use by that configuration. For more information, see Environment Configuration Management.

After making any changes to project options, click OK to close the dialog, and then be sure to save the project file, which is where the options are stored.

Tips

  1. You can set all options, across all tabs, back to their defaults at the time of original installation. To do this, simply click the Set To Installation Defaults button, at the bottom-left of the Options for Project dialog.
  2. The process of compiling is integral to producing a valid netlist for a project. In fact it is the process of compilation that yields the unified data model of a design. Carefully check and resolve all reported errors prior to netlist generation.
  3. For a comprehensive reference describing each of the possible electrical and drafting violations that can exist on source documents when compiling a project, refer to the Project Compiler Violations Reference.
  4. When not using centralized environment configuration, or when the configuration chosen has no defined OutJobs, you are free to create new, unmanaged Output Job files, in addition to using those from a vault, should this be required.


Applied Parameters: ObjectKind=Project|Action=DefaultPrints

Summary

This command is used to open the Options for Project dialog, with the Default Prints tab made active. From here, you can configure the default setups for all print-related outputs for the active project. You can also nominate which output is used by default when using an applicable editor's standard Print command.

Access

This command is accessed from the Schematic Editor, and PCB Editor, by choosing the File » Default Prints command, from the main menus.

Use

First, ensure that one of the target project's associated design documents is open as the active document in the main design window.

After launching the command, the Options for Project dialog will appear, opened at the Default Prints tab. The tab lists each of the print-related outputs that can be generated from the active project, grouped together by output type. Use the Configure and Page Setup buttons to define the default print configuration and page layout for a selected entry in the list.

The Supports column defines which document editor the output is generated from. The Default Print column enables you to specify which of the print outputs will be used as the default when using the standard Print command. Only one print output can be enabled per document editor, at any one time.

Tips

  1. Print-related output can also be setup and generated from an Output Job Configuration file (*.OutJob). This file enables you to define all of your design output configurations - assembly, fabrication, reports, netlists, etc - exactly as required, and all in the one convenient and portable file.


Applied Parameters: ObjectKind=FocusedDocument

Summary

This command is used to access the Document Options dialog for the active BOM Document, from where you can configure parameters that can be used to differentiate components in a design that share a common Design Item ID. Many designers still employ old-style component methodologies. For passive components (resistors, capacitors, inductors), it is common to see libraries of schematic components, where those components share a common symbol, but when placed on the schematic, are given different values parametrically. So a group of capacitors might share the one symbol, and therefore have the same Design Item ID, but through a differentiating parameter typically their Comment field - they are given different values of capacitance, and are therefore unique - in terms of distinct physical components that are required when the board is manufactured and assembled.

A BOM document is the user interface to Altium NEXUS's ActiveBOM system. ActiveBOM offers a live presentation of the design from the outset, providing early and ongoing cost estimation. It allows you to define target pricing at the individual item level. You can then track how actual costing fares against these estimates, and so give a timely flag if any cost blow-outs are on the near horizon! In addition, you can quickly assess item availability, complete with notification if there is a risk in the supply of a chosen part. For a high-level walkthrough of the system, see ActiveBOM.

Access

This command is accessed from the BOM Editor, by choosing the Design » Document Options command, from the main menus.

Use

First, ensure that the BOM document (*.BomDoc) for the project is open as the active document in the main design window

After launching the command, the Document Options dialog will appear. Use the dialog to define a set of parameters that can be used by ActiveBOM to compare, detect, and separate common unmanaged component (non-vault or DBLib-based) design items. Controls are available to add new parameters to the list, edit existing parameters, or remove parameters, as required. For each parameter, use its associated Parameter State field to specify whether it is included as a variable for differentiation (Check) or excluded (Ignore).

Comment, Value, Description, and Footprint parameters are added to the differentiation list by default. In the majority of cases, it is one (or a combination) of these parameters that is used to distinguish components that share the same core schematic symbol (and therefore same Design Item ID).

With the required parameters specified, click OK. Any ambiguous components will be 're-assessed' for uniqueness based on the parameters enabled for checking. The BOM Catalog tab will be refreshed and the results presented. If components were able to be successfully differentiated, based on the supplied parameters, they will be listed as their own distinct entries, and their status will change to Up to Date. If differentiation could not be proven, the condensed component entry will remain, along with the status Ambiguous Component. In this case, add another parameter through the Document Options dialog, that differs between the affected components.

Once ambiguity is resolved, you can proceed to define separate and distinct supply chain solutions for the components.

Tips

  1. Within the BOM Catalog tab of the BOM Document, the Status Ambiguous Component is used to reflect the situation where multiple components exist in the design with the same Design Item ID, but differ in their parametric information.
  2. The default Comment, Value, and Description parameters are all set for inclusion in the checking, while Footprint is set to be ignored. For the most part, discrete components will vary in comment and/or value and/or description, therefore footprint checking isn't essential. However, the presence of the Footprint parameter for differentiation caters for the situation where discrete components, such as two resistors, might have the same value and description, but be available in two different packages (e.g. 0402 vs 0603). In this case, simply switch the Parameter State from Ignore to Check.


Applied Parameters: ObjectKind=Project|Action=Annotate

Summary

This command is used to perform Schematic Level Annotation, through use of the Annotate dialog. Schematic Level Annotation uses a purely logical view of the design to determine component designators. It is most useful for simple designs that do not use Device Sheets, but because it allows the order of processing to be specified, as well as the option to complete existing packages for multi-part components, it is also a pre-requisite to Board Level Annotation.

For a high-level overview of annotation, see Annotating the Components.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Annotate Schematics command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project you wish to annotate, is open as the active document in the main design window.

After launching the command, the Annotate dialog will appear. Use the dialog to systematically assign designators to all or selected parts in selected sheets of the active project, and ensure that designators are unique and ordered based on their position.

The dialog is partitioned into two primary sides:

  1. The left side is for configuring the Order of Processing, setting Matching Options for multi-part components, and setting the scope of annotation; including setting an Index and adding a Suffix for designators per Schematic Sheet.
  2. The right side lists the proposed changes that will be implemented. It includes the Current and Proposed designators along with the option to lock (exclude) specific designators and / or sub-parts from annotation.

Once annotation configuration options have been defined on the left, clicking the Update Changes List button will update the Proposed Change List on the right, so that all designator changes can be reviewed prior to being applied. Only designators that have not previously been set (i.e. R?, C?, etc) will be affected by the changes, so if the intention is to update all designators in the design, they should be first reset by pressing the Reset All button.

After reviewing the list of proposed changes, clicking the Accept Changes (Create ECO) button will launch the Engineering Change Order dialog, and a final layer of validation and reporting can be applied. Once the ECO is executed, the annotation changes will be applied to the design.

Tips

  1. If a schematic document is included in the scope of annotation but is not currently open, it is required to be automatically opened in order for the annotation to be carried out. To avoid clutter in the main design window, where an open document is normally added as another tab, the document will instead be opened and automatically hidden. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window.
  2. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - .
  3. When processing annotation order, the reference used for component location can either be the center of a component, or the location of its designator. With the latter, if the positional annotation is not performing according to your expectations, ensure that the designators are positioned correctly. It might be that the components themselves are in perfect alignment, but a misplaced designator is responsible for causing the undesirable annotation results.
  4. When Completing Existing Packages (as part of Matching Options), some consideration should be given to how power pins have been specified on active components.  For example, many designers include VCC / GND pins on the first part of a multi-part component but then don't include those pins on subsequent parts. If the first part in a multi-part component is packed into an alternate package and has its sub-part updated, it can lead to unconnected (or floating) Power connections.


Applied Parameters: ObjectKind=Project|Action=AnnotateQuiet

Summary

This command is used to interrogate all source schematic documents for the active project that are enabled for annotation, and assign a unique designator to any component that currently does not have a designator. Annotation is carried out quietly - making it possible to apply all of the previous settings of the Annotate dialog without needing to reopen the dialog. This is especially useful if the design is going through a rapid phase of development and the designer wants to quickly annotate prior to compiling the design.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Annotate Schematics Quietly command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project whose unassigned component designators you wish to annotate, is open as the active document in the main design window.

After launching the command, any source schematic documents that have been enabled for annotation, and that are currently closed, will be opened and hidden. A confirmation dialog will appear, summarizing the number of designators requiring update and asking whether you wish to proceed with the changes. After clicking Yes, all unassigned component designators across all annotation-enabled schematic sheets of the active project will be quietly annotated - each receiving a unique designator.

Tips

  1. Annotation will only be carried out for schematic sheets that are currently enabled for annotation in the Schematic Sheets To Annotate region of the Annotate dialog.
  2. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - . All hidden documents can be accessed by clicking on the drop-down button at the far right of the Document bar (containing all individual tabbed views).


Applied Parameters: ObjectKind=Project|Action=AnnotateAll

Summary

This command is used to interrogate all source schematic documents for the active project that are enabled for annotation, and re-annotate all components therein, in accordance with the annotation scheme currently defined in the Annotate dialog.

Running this command is equivalent to running the Reset Schematic Designators command followed immediately by the Annotate Schematics Quietly command.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Force Annotate All Schematics command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project whose component designators you wish to re-annotate, is open as the active document in the main design window.

After launching the command, any source schematic documents that have been enabled for annotation, and that are currently closed, will be opened and hidden. A dialog will appear detailing the number of designators that need updating, and asking for confirmation to proceed. After clicking Yes, all component designators across all annotation-enabled schematic sheets of the active project will be re-annotated, where necessary, to comply with the current positional annotation scheme defined in the Schematic Annotation Configuration region of the Annotate dialog.

Tips

  1. Annotation will only be carried out for schematic sheets that are currently enabled for annotation in the Schematic Sheets To Annotate region of the Annotate dialog.
  2. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - . All hidden documents can be accessed by clicking on the drop-down button at the far right of the Document bar (containing all individual tabbed views).


Applied Parameters: ObjectKind=Project|Action=AnnotateReset

Summary

This command is used to reset all component designators in the active project, across all source schematic sheets that are enabled for annotation. This can be especially useful if large portions of content have been cut and pasted from different sources into a new design.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Reset Schematic Designators command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project whose component designators you wish to reset, is open as the active document in the main design window.

After launching the command, any source schematic documents that have been enabled for annotation, and that are currently closed, will be opened and hidden. A confirmation dialog will appear, summarizing the number of designators requiring update and asking whether you wish to proceed with the changes. After clicking Yes, all component designators across all annotation-enabled schematic sheets of the active project will be reset, appearing in the form: R?, C?, D?, U?, etc.

Tips

  1. Annotation will only be carried out for schematic sheets that are currently enabled for annotation in the Schematic Sheets To Annotate region of the Annotate dialog.
  2. Any designators with a locked status are not reset or changed in any way.
  3. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - . All hidden documents can be accessed by clicking on the drop-down button at the far right of the Document bar (containing all individual tabbed views).
  4. Component designators can also be reset directly from within the Annotation dialog, by clicking the Reset All button.


Applied Parameters: ObjectKind=Project|Action=AnnotateResetDup

Summary

This command is used to reset all duplicated component designators in the active project, across all source schematic sheets that are enabled for annotation. Duplicate designators typically occur when duplicating portions of a design, whereby the newly copied components will still hold the same designator values as those that they were copied from. This command provides a fast way to reset duplicate designators to '?', after which another annotation command can be run to ensure those components are once again uniquely designated.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Reset Duplicate Schematic Designators command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project whose duplicate component designators you wish to reset, is open as the active document in the main design window.

After launching the command, any source schematic documents that have been enabled for annotation, and that are currently closed, will be opened and hidden. A confirmation dialog will appear, summarizing the number of designators requiring update and asking whether you wish to proceed with the changes. After clicking Yes, all duplicate component designators found across all annotation-enabled schematic sheets of the active project will be reset, appearing in the form: R?, C?, D?, U?, etc.

Tips

  1. Annotation will only be carried out for schematic sheets that are currently enabled for annotation in the Schematic Sheets To Annotate region of the Annotate dialog.
  2. Any designators with a locked status are not reset or changed in any way.
  3. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - . All hidden documents can be accessed by clicking on the drop-down button at the far right of the Document bar (containing all individual tabbed views).
  4. Duplicate component designators can also be reset directly from within the Annotation dialog, by choosing the Reset Duplicates command, from the menu associated with the Reset All button.


Applied Parameters: ObjectKind=Project|Action=BackAnnotate

Summary

This command is used to update the designators of the components in the source schematic sheets of the active project, using a Was-Is file (*.was), or Engineering Change Order file (*.eco).

This command is largely superfluous since the Design Compiler and Synchronizer are far more effective tools for managing design synchronization. It is still useful however, for legacy purposes, and for designers who use alternate PCB layout tools (such as Specctra®).

Access

This command is accessed from the Schematic Editor by choosing the Tools » Back Annotate Schematics command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project whose component designators you wish to back annotate, is open as the active document in the main design window.

After launching the command, the Choose WAS-IS File for Back-Annotation from PCB dialog will appear. Browse to and select the required .was (or .eco) file. After clicking Open, an information dialog will appear listing how many changes to designators have been made since the previous state and how many have been made since the original state. At this point, the changes aren't actually implemented. Click OK to bring up the Annotate dialog, from where you can view the proposed changes to the current designators before deciding to create an ECO to implement them.

Tips

  1. All source schematic documents for the project are required to be open in order for the annotation to be carried out. This is carried out automatically. To avoid clutter in the main design window, where an open document is normally added as another tab, unopen schematic documents will instead be opened and automatically hidden. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window.
  2. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - . All hidden documents can be accessed by clicking on the drop-down button at the far right of the Document bar (containing all individual tabbed views).
  3. When re-annotating designators in the PCB, each re-annotation produces a unique .was file, that carries the date and time in its filename. This enables you to load multiple .was files in succession - from oldest to newest - and not lose designation synchronization between the PCB and source schematic sheets.
  4. Back annotation can also be performed directly from within the Annotation dialog, by clicking the Back Annotate button.


Applied Parameters: ObjectKind=Project|Action=AnnotatePhysical

Summary

This command is used to perform Board Level Annotation, through use of the Board Level Annotate dialog. Board Level Annotation provides a mapping between designators used in the Schematic (Logical) Design and their real world counterparts on the PCB (Physical) Design. While Board Level Annotation can be used in any design, it is especially useful for multi-channel designs and/or designs that incorporate Device Sheets - where the designators cannot be edited on the Device Sheet itself. In this way, the entire design can be re-annotated without actually modifying the original Device Sheet(s). Board Level Annotation also resolves any conflicting annotation problems that may occur due to duplicate designators across a project, and stores its changes in a *.Annotation text file. It includes additional keywords for customizing naming schemes and allows them to be applied to all, or only a select range of parts.

Prior to running this command, you need to ensure that all components have been annotated through performing Schematic Level Annotation, so that the Schematic source data - including packaged options for multi-part components - is available as input for Board Level Annotation.

Access

This command can be accessed from the Schematic Editor by:

  • Choosing the Tools » Board Level Annotate command, from the main menus.
  • Using the Ctrl+L keyboard shortcut.

Use

First, ensure that one of the source schematic documents for the project you wish to annotate, is open as the active document in the main design window.

After launching the command, the Board Level Annotate dialog will appear. Use the dialog to assign designators to the PCB components as required.

The dialog is partitioned into two primary sides:

  1. The left side is for filtering and setting the scope of annotation.
  2. The right side lists the proposed changes that will be implemented. This side is color coded and displays the following information:
    1. Schematic Source Component (pink) – a list of all components set as eligible (according to the settings in the filtering options on the left side.
    2. Calculated Design Data (green) – the contents of this list will be dependent on the currently defined Annotation options.
    3. Naming Scheme (white) – checked items will have the annotation applied.
    4. PCB Component Instance (white) – the annotation that will be applied to the component on the PCB.

To complete Board Level Annotation:

  1. Click on the Annotate Options button to access the Board Level Annotation Options dialog. Use this dialog to define the naming scheme - either predefined or custom naming - used in determining the contents in the Calculated Design Data column.
  2. Click on the Annotate drop down and choose between Annotate Undesignated, Annotate All, or Annotate Selected. The Annotate Selected option will only be enabled if components were selected in the design prior to launching the Board Level Annotate dialog.
  3. The PCB Component Instance column will be updated indicating the designator to be annotated to each component on the PCB. Review the contents of this column to ensure it meets with the requirements.
  4. Click the Accept Changes (Create ECO) button to launch the Engineering Change Order dialog. This provides a final level of validation and reporting.
  5. Click the Execute Changes button within the Engineering Change Order dialog to apply the changes to the design and then click the Close button to return to the Board Level Annotate dialog.
  6. Finally, click the Close button on the Board Level Annotate dialog to return to the main editor.

Once completed, the Board Level Annotation process will add and/or update a *.Annotation file within the project. Some settings may also be changed within the main project document requiring it to be saved. you now need to pass the changes across to the PCB - that is, synchronize the Schematic Documents with the PCB Document.

Tips

  1. The project will be automatically compiled every time the Board Level Annotate dialog is launched, to ensure the most current design and preferences are used.
  2. Use the Reset All button to reset all of the designators back to the default names for Compiled Components - i.e. all current or previous Board Level Annotations will be removed. The default names for Compiled Components are configured on the Multi-Channel tab of the Options for Project dialog.
  3. If a schematic document is included in the scope of annotation but is not currently open, it is required to be automatically opened in order for the annotation to be carried out. To avoid clutter in the main design window, where an open document is normally added as another tab, the document will instead be opened and automatically hidden. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window.
  4. To display the current status of documents in the Projects panel, click the  button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - .


Applied Parameters: ObjectKind=Project|Action=LibrarySynch

Summary

This command is used to update placed instances of components on chosen schematic sheets, with modified information from a source library. This includes Standard Components (those placed from Schematic Component Libraries (*.SchLib), Integrated Libraries (*.IntLib), and vault-based components) and Database Components (those placed from Database Libraries (*.DBLib, *.SVNDbLib)). The update feature allows you to pass changes to parameters, as well as model and graphical information.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Update From Libraries command, from the main menus.

Use

First, ensure that one of the source schematic documents for the project whose components you wish to update, is open as the active document in the main design window.

After launching the command, the Update From Library dialog will appear. The dialog provides controls that allow you to fully control not only which components get updated, but also how. You can choose to fully replace the placed instance with that in the library, or just update any of: Graphical attributes, parameters, or models. Full control is available at the parameter-level, to determine which parameters get updated for a component, and how.

The dialog is essentially divided into two pages:

  1. The first page of the dialog deals with the scope of the update - which source schematic documents are to be included in the update and the specific component types contained thereon. also on this page, you can define the type of update required. The simplest form of update is to fully replace the components on the schematic sheet(s) with those defined in the source library. Graphical attributes, parameters and model links are all updated directly with the information that exists in the source library (or record and referenced libraries, for database components). Should you wish a little more control over what is updated, you can opt to update only specific attributes (graphical, parameters, models).

For parameter and model update actions, still further control is afforded through the Library Update Settings dialog. Access this dialog by clicking the Advanced button. Not only can you define the default, global update actions for parameters and models using this dialog, but also control which specific parameters and models are included in the update.

After defining the scope of the update as required, and the default actions to be carried out, you could simply click Finish. Should you wish to further refine the update on a per-component basis, prior to generating an ECO, click Next to access the second page of the dialog.

  1. The second page of the Update From Library dialog presents you with a detailed grid, listing all components instances involved in the intended update process. Whereas the first page of the dialog allows you to specify, at a coarse level, which physical component types get included in the update, this page allows you to fine-tune exactly which component instances of those types get updated. Essentially, the page is divided into three:
  • The current instances of components placed on the schematics.
  • The source library (or vault) that will be used in the update. This is typically the same source library from which the component was originally placed, but you do have the ability to complete change the component for another, in the same, or different library.
  • The specific update actions required for each component instance. These will initially be set in accordance with the default action settings defined on the first page of the dialog.
Should you wish to browse individual parameter changes proposed by the update, click on the Parameter Changes button. The Select Parameter Changes dialog will appear, summarizing the parameter changes for those component instances with a parameter update action enabled.

After all update options are configured as required, clicking the Finish button will launch the Engineering Change Order dialog, and a final layer of validation and reporting can be applied. Once the ECO is executed, the changes to the specified component instances are implemented on the affected schematic sheets.

Tips

  1. Although DBLib and SVNDBLib files present as libraries in the Libraries panel, they are only a source of connection and field mapping - not libraries in the true sense of the word. The update feature passes changes to parameters, symbol and model references in the external database, as well as graphical modifications made in referenced symbol and model libraries.
  2. Individual parameter-level changes for a component instance will only be shown provided the Full Replace option is disabled and the Parameters option is enabled, in the Actions region of the second page of the Update From Library dialog.
  3. Definitions on the first page of the Update From Library dialog, and the Library Update Settings dialog are persistent. They are stored in the project file upon saving.
  4. Definitions on the second page of the Update From Library dialog are not persistent. They will be lost if you go back to the first page, or close the dialog.
  5. While vault-based components can be updated (to later revisions), or switched out for different Component Items available in an Altium Vault, a far more powerful feature to manage these components is the Item Manager.
  6. Whether a design parameter gets updated or not can also be controlled on an individual parameter basis, directly from within the design. In the associated Parameter Properties dialog for a parameter, disable the Allow Synchronization With Library option to prevent that parameter from being included in an update process.


Applied Parameters: ObjectKind=Project|Action=PCBLibrarySynch

Summary

This command is used to check the component footprints on the active PCB document, against the libraries from which they were sourced, and perform updates to chosen components, as required. This ensures that all footprints in the design adhere to the authorized footprint libraries.

Access

This command is accessed from the PCB Editor by choosing the Tools » Update From PCB Libraries command, from the main menus.

Use

First, ensure that the PCB document whose footprints you wish to check, is open as the active document in the main design window.

After launching the command, the Update PCB Libraries - Options dialog will appear. Use this dialog to choose which layers of the PCB and library footprint you wish to compare. This is important, as in some designs, certain layers of the footprint may not be used, and extra comparisons will take extra time to process.

At this point, and if you want to update all footprints to match those in the source libraries, you can simply click the Update All Footprints (Create ECO) button, and implement the changes to the design through a subsequent Engineering Change Order. However, should you wish to inspect differences that are detected in detail, and determine which footprints to include in an update, prior to generating an ECO, click OK to access the Update From PCB Libraries dialog.

The Update From PCB Libraries dialog presents the results of the footprint comparison across two regions:

  • Upper region - presents a summary of the comparison results. The footprint of each component on the PCB is compared against the corresponding footprint in the indicated source library. If there are no differences, the footprints will be deemed to match, with a green tick icon () appearing in the Match column. No update is required in the case of a match. If, however, one or more primitives in a footprint are different - in terms of their locations within the footprint - then the footprints are flagged as not matching. A red cross icon () will be inserted into the Match column. An update is required to bring the placed component's footprint, and source library footprint, back into sync.
If a footprint in a source library can't be found, the Path field for the library component to compare against will reflect this, with the entry <Footprint not found>. In this case, comparsion can not be made for that particular component.
  • Lower region - lists any differences for the currently selected component entry in the upper region. For a non-matching footprint, the component primitives causing differences are listed, per enabled layer for comparison. A graphical comparison is presented, with the footprint divided up into cells. Cells where differences exist are shown in full color, with the differences highlighted. Primitive objects in the current PCB are shown full color, with the updated component primitives from the library shown as a "ghost" image over the top of them.
You also have the ability to create a html-based Footprint Comparison Report, but bear in mind that this will close the dialog, and you will need to launch the command again.

After browsing differences and configuring which footprints you wish to have updated, click the Accept Changes (Create ECO) button. The Engineering Change Order dialog will appear, with which to implement the changes.

Tips

  1. This command covers all PCB components, irrespective of the type of library from which they are sourced - PCB Footprint Libraries (*.PcbLib), Integrated Libraries (*.IntLib), Vault-based components (PCB Component Items referenced by parent Component Items), and Database Libraries (*.DBLib, *.SVNDbLib)). In the case of the latter, the libraries used in the update are those referenced in the corresponding records of the linked external database.
  2. The references to the underlying libraries - from where the footprints are sourced - are retrieved from the applicable schematic if available, or from the PCB footprints themselves. All source libraries must be part of the Available Libraries set.
  3. A Footprint Comparison Report can also be added as part of a set of validation outputs in an Output Job Configuration file.


Applied Parameters: ObjectKind=Project|Action=PCBLibrarySynch|ContextSensitive=True

Summary

This command is used to check the component footprint under the cursor (or the currently selected components) on the active PCB document, against the libraries from which they were sourced, and perform updates to those components, as required. This ensures that the chosen footprints in the design adhere to the authorized footprint libraries.

Access

This command is accessed from the PCB Editor, by:

  • Right-clicking over a placed component (not selected) and choosing the Component Actions » Update Current Component From PCB Libraries command from the context menu.
  • Right-clicking over a selected component (or a component that is part of a group of selected components) and choosing the Component Actions » Update Selected Components From PCB Libraries command from the context menu.

Use

After launching the command, the Update PCB Libraries - Options dialog will appear. Use this dialog to choose which layers of the PCB and library footprint you wish to compare. This is important, as in some designs, certain layers of the footprint may not be used, and extra comparisons will take extra time to process.

At this point, and if you want to update the footprint(s) to match those in the source libraries, you can simply click the Update All Footprints (Create ECO) button, and implement the changes to the design through a subsequent Engineering Change Order. However, should you wish to inspect differences that are detected in detail, and determine which footprints to include in an update, prior to generating an ECO, click OK to access the Update From PCB Libraries dialog.

The Update From PCB Libraries dialog presents the results of the footprint comparison across two regions:

  • Upper region - presents a summary of the comparison results. The footprint of each component on the PCB is compared against the corresponding footprint in the indicated source library. If there are no differences, the footprints will be deemed to match, with a green tick icon () appearing in the Match column. No update is required in the case of a match. If, however, one or more primitives in a footprint are different - in terms of their locations within the footprint - then the footprints are flagged as not matching. A red cross icon () will be inserted into the Match column. An update is required to bring the placed component's footprint, and source library footprint, back into sync.
If a footprint in a source library can't be found, the Path field for the library component to compare against will reflect this, with the entry <Footprint not found>. In this case, comparsion can not be made for that particular component.
  • Lower region - lists any differences for the currently selected component entry in the upper region. For a non-matching footprint, the component primitives causing differences are listed, per enabled layer for comparison. A graphical comparison is presented, with the footprint divided up into cells. Cells where differences exist are shown in full color, with the differences highlighted. Primitive objects in the current PCB are shown full color, with the updated component primitives from the library shown as a "ghost" image over the top of them.
You also have the ability to create a html-based Footprint Comparison Report, but bear in mind that this will close the dialog, and you will need to launch the command again.

After browsing differences and configuring which footprints you wish to have updated, click the Accept Changes (Create ECO) button. The Engineering Change Order dialog will appear, with which to implement the changes.

Tips

  1. This command covers all PCB components, irrespective of the type of library from which they are sourced - PCB Footprint Libraries (*.PcbLib), Integrated Libraries (*.IntLib), Vault-based components (PCB Component Items referenced by parent Component Items), and Database Libraries (*.DBLib, *.SVNDbLib)). In the case of the latter, the libraries used in the update are those referenced in the corresponding records of the linked external database.
  2. The references to the underlying libraries - from where the footprints are sourced - are retrieved from the applicable schematic if available, or from the PCB footprints themselves. All source libraries must be part of the Available Libraries set.
  3. A Footprint Comparison Report can also be added as part of a set of validation outputs in an Output Job Configuration file.


Applied Parameters: ObjectKind=Project|Action=DatabaseUpdate

Summary

This command is used to update the parameters in components placed on schematic documents (or defined in a schematic library document), with values specified for those same parameters in corresponding linked component records in an external database. Linkage is performed through the use of an intermediary linking file, which can be one of the following:

  • Database Link file (*.DBLink) - used when linking existing placed components to an external database or, more typically, defined components in a source schematic library.
  • Database Library file (*.DBLib) - used when placing components directly onto a schematic sheet from an external database.
  • SVN Database Library file (*.SVNDbLib) - as for DBLib, but with symbol and model libraries stored under version control.

Access

This command is accessed from the Schematic Editor, and Schematic Library Editor, by choosing the Tools » Update Parameters From Database command, from the main menus.

The command is only available in the Schematic Library Editor, provided the source library is part of an Integrated Library package (*.LibPkg), and a DBLink file is used to provide the linking from library components to component records in the external database.

Use

After launching the command, the Update Parameters From Database dialog will appear. Use this dialog to determine the scope of the update. For placed components, for example, this would entail specifying which schematic sheets in the active project are included, and the component types. After clicking OK, the external database will be queried for matching components. If there are parameter differences between the placed/library components and the matching records in the database, you will be taken to the Select Parameter Changes dialog.

The Select Parameter Changes dialog lists all parameters that exist in the database records for placed/library components falling under the scope of the update. Only those parameters that are mapped - between the external database and the placed/library component instance - will be listed. The dialog will initially show proposed updates to bring the placed/library component parameters into sync with those in the database, based on the update actions you have defined in the applicable intermediary link file (DBLink, DBLib, SVNDbLib).

Parameter differences are distinguished by the use of a unique icon inserted in the relevant cell. For example, a blue triangle in the corner of a cell means that a difference has been detected between the value of a parameter in the placed/library component, and the same parameter in the linked database record.

Use the controls provided in the dialog to fully control which updates to proceed with, and which to reject. You can reject updates to all parameters for a selected component, or for specific parameters of that component.

When you are satisfied with the update solution, click the Accept Changes (Create ECO) button. Use the Engineering Change Order dialog that appears to validate and then execute the updates accordingly. If you realize there is an update you really don't want to proceed with, simply disable the applicable change order entry.

Tips

  1. Any parameters that are defined for a placed/library component, but which are not a field in a database table, will not appear listed in the Select Parameter Changes dialog. This can happen, for example, when one or more parameters have been added to a component on a sheet after placement from a database library.
  2. Whether a placed/library component parameter gets updated or not can also be controlled on an individual parameter basis, directly from within the design/library. In the associated Parameter Properties dialog for a parameter, disable the Allow Synchronization With Database option to prevent that parameter from being included in an update process.


Applied Parameters: ObjectKind=Project|Action=SheetNumber

Summary

This command is used to access the Annotate Compiled Sheets dialog. This dialog allows you to quickly number the compiled sheets (physical instances of a sheet) in the active design project.

This command relates to the numbering of the compiled (physical) sheets. To number the logical sheets, use the Number Schematic Sheets command.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Annotate Compiled Sheets command, from the main menus.

Use

After launching the command, the Annotate Compiled Sheets dialog will appear. Use the controls available in the dialog to define sheet numbering as required. If your organization has a specific number or naming system that can't be automated through the Annotate Sheet controls, custom sheet names and numbers can be written directly into the SheetNumber field.

Tips

  1. The Sheet Number allocated by the dialog can be referenced on printed outputs of the compiled (Physical) sheet using the =SheetNumber special string. This will then be updated in any printed outputs of the design.
  2. Sheet Numbers updated by the Annotate Compiled Sheets dialog are stored in the project's *.Annotation file. This ensures that annotation information and settings are remembered across project editing sessions.
  3. Device Sheets are treated like any other sheet in the design project, and are annotated according to the chosen Annotation options.
  4. Once the compiled sheets have been annotated through the Annotate Compiled Sheets dialog, the $SheetNumber keyword can be used as part of the Naming Scheme in the Board Level Annotation Options dialog. If the project's compiled sheets have not yet been annotated, the sheet numbering defined through running the Tools » Number Schematic Sheets command will be used by default.


Applied Parameters: ObjectKind=Project|Action=ItemManager

Summary

This command is used to access the Item Manager dialog. The Item Manager is a powerful tool providing two key abilities in relation to components and sheets of re-usable schematic circuitry in a board design project:

  • Migration - firstly, it facilitates the migration of a design project from using components and schematic sheets based on older component management methodologies, to using vault-based entities (managed components and managed sheets). In this respect it can be thought of as providing 'Update to Vault' functionality.
  • Synchronization - secondly, once your designs have been 'converted' to using managed (vault-based) Items, it facilitates the synchronization of instances of those managed components and sheets in a design project, with any changes to the source Items in the vault(s). In this respect, it can be thought of as providing 'Update from Vault' functionality.
For a detailed look at the Item Manager, see Managing Vault Items with the Item Manager.

Access

This command is accessed from the Schematic Editor by choosing the Tools » Item Manager command, from the main menus.

Use

After launching the command, the Item Manager dialog will appear. The dialog presents all components and sheet symbols found in a single schematic sheet (free document), or the set of schematics in the active design project. Use the controls available in the dialog to replace unmanaged items with managed ones, or to keep existing managed items synchronized with their source items in an Altium Vault, as required.

  • Migration - you need to replace the unmanaged entities with managed ones from a vault. For both components and sheet symbols, this can be done by manually choosing vault Items to use. When you click on an entry in the grid, the Choose button becomes available at the bottom-right of the grid. Clicking this will give you access to a dialog, from where you can browse within any of your currently connected vaults and select the required Item, and specific revision of that Item. The choice of Item is reflected in the New Settings region of the grid, back in the Item manager.

For design components, this can also be performed in a more automated fashion, using the manager's auto-matching feature - taking the unmanaged design components and attempting to match each one with a managed Component Item in a connected vault. The matching process takes the Design Item ID of an unmanaged design component and compares it against the Comment property of managed Component Items in a vault. When a match is found, that managed Component Item will be proposed for the update. To run this process, simply click the Auto-Match Unmanaged button. The Link Unmanaged Components To Vault dialog will appear, with the results of the matching process.

For a successful match, the Messages field will display Success: No Errors. If there is an error preventing a successful match, an alternative message will be displayed. If more than one Item-Revision exists in a vault with the same value for its Comment property, the Messages field will display Warning: Multiple components matched. While a match is still proposed, selecting a component entry with this message will enable the Choose Alternative Component From Vault button. Use this to choose the specific Item-Revision as required, if the proposed match is not suitable. Click OK to accept the links – the information in the New Settings region of the Link Unmanaged Components To Vault dialog will be copied to the New Settings region back in the Item Manager.

  • Synchronization - when the Item Manager is opened it automatically compiles the schematic project, detects and lists all components, flagging if they are managed or not, and then compares the Item-Revision of each managed component on the schematics against the available revisions of that Item in the Vault. If there are Items that have a newer revision available in the Vault, these are flagged in the Revision Status column of the Item Manager, which will state Out of date for those Items.

To bring out of date items up to date they must first be selected. Once they are selected, right-click and choose Update to Latest Revision from the menu. The New Settings region of the dialog will then show the detail of each new Item-Revision.

Before committing to perform all of the changes detailed in the Item Manager, you may want to inspect the design and confirm that you approve of each change. To help in this process you can generate a snapshot HTML-based report of the current listing in the Item Manager. To do this, right-click anywhere in the Item Manager and select Export from the menu. Navigate to a suitable location and name the report as required.
Additional update options are available at the bottom of the Item Manager. These include the ability to update the Locked property associated to a component's designator and/or sub-part fields, as well as controlling the update of parameters. If you have made any component parameters visible on the sheet, there are also options to Preserve Parameter Visibility, and Preserve Parameter Location, ensuring the look and feel of your placed design components are not graphically affected when switched over to vault-based instances.

Once changes have been set up as required, those changes need to be implemented. This is done through an Engineering Change Order (ECO). The drop-down menu associated with the ECO button, at the bottom of the Item Manager, provides two ways in which to effect an update:

  • Generate ECO - use this command to generate and execute an ECO through the Engineering Change Order dialog. Using the dialog, you are able to browse the actions that will be taken to implement those changes. You can disable any actions as required - you always have full control of what gets changed. When ready, execute the ECO and the changes will be effected.
  • Apply ECO - use this command to directly create and execute an ECO quietly - without the Engineering Change Order dialog appearing.

Verification that replacement has indeed been successful can be performed at the individual component/sheet symbol level within the schematic sheets of the board design project. Simply access the associated properties dialog for an item, which will now show a link back to the corresponding source vault Item. Alternatively, verification can be performed quickly back in the Item Manager, which updates to reflect the new settings for the items in the board design project, in the Current Settings region of the grid.

Tips

  1. The New Settings region simply presents information about the proposed change. It has the same fields as the Current Settings region.
  2. For multiple instances of the same component used in a design, you can select a group of components and manually choose the required vault-based Item - the choice will be applied to all components in the selection. Standard multi-select features (Ctrl+click, Shift+click) can be used to select the grouping.
  3. The auto-matching process is very effective, since the act of creating the source component definitions in Component Library files from source Schematic Library files - at the time when you migrated the components to a vault - uses the Design Item ID for each schematic component and writes this to the Comment parameter for the corresponding component definition. In other words, by migrating the components to a vault using the exact source libraries that were used to place the components in the board design project, matching is guaranteed.
  4. When using the component auto-matching feature, if a Component Item has multiple revisions, the first revision detected will be used. This will mean the proposed Item Revision is out of date to begin with. This situation will be reflected back in the Item Manager, through the Release State field in the New Settings region. So if the proposed Item Revision is not suitable, and is not dealt with through the Link Unmanaged Components To Vault dialog, it can still be modified through the manual choosing process back in the Item Manager.


Applied Parameters: ObjectKind=Project|Action=NoERCManager

Summary

This command is used to access the NoERC Manager dialog, from where all No ERC directives - used across the entire active project - can be reviewed and edited. The No ERC object is a design directive that can operate in two modes. In its generic mode, the directive is placed on a node in the circuit to suppress all reported Electrical Rule Check warnings and/or error violation conditions that are detected when the schematic project is compiled. In its specific mode, the directive is configured to target one or more specific violations, allowing suppression of selected warning or error conditions, while allowing any other warning or error to be detected and reported.

For detailed information about this object type, see No ERC.

Access

This command is accessed from the Schematic Editor by choosing the Tools » NoERC Manager command, from the main menus.

Use

First, ensure that a source schematic document for the project whose No ERC directive you wish to interrogate, is open as the active document in the main design window.

After launching the command, the active project is compiled and the NoERC Manager dialog will appear. From here, you can move through the list of nets with directives applied, and edit any number of No ERC directives.

When editing is complete, click the Generate ECO button to access the Engineering Change Order dialog. Using the dialog, you are able to browse the actions that will be taken to implement those changes. You can disable any actions as required - you always have full control of what gets changed. When ready, execute the ECO and the changes will be effected.

Tips

  1. To show only those items with No ERC directives, enable the Show only nets with NoERC option.


Applied Parameters: ObjectKind=DatabaseLink

Summary

This command is used to access the associated options dialog for the active intermediate linking file (DbLink, DBLib, SVNDbLib) that is being used to connect to an external database.

Access

This command can be accessed from the Database Link Editor, Database Library Editor, and SVN Database Library Editor, by:

  • Choosing the Tools » Options command, from the main menus.
  • Right-clicking within the Table Browser tab and choosing the Options command from the context menu.

Use

After launching the command, the Database Options dialog will appear. The dialog is divided into two tabs, the nature of which depends on the type of linkage file you are using:

  • Default Actions - this tab is present for all three types of linkage file, and allows default parameter update options to be defined in the one convenient, central location. When defining the update options for individual mapped parameters, in the Field Mappings region of the document, an entry of Default uses the setting defined on this tab, but can be overridden as required, allowing you to completely tailor update options on a per-parameter basis. All actions (Add To Design, Remove From Design, Update Values) are used during a 'synchronize with database' operation. In addition, the Add To Design setting is applied when placing a component from a DBLib/SVNDbLib.
  • Symbol & Model Search Paths - this tab is present for DbLink and DBLib types of linkage file, and allows you to define search paths to determine where symbol and model files can be found when placing from the database library, and when searching for a model after placement. Entering paths, even relative, in a database table can be a little restrictive. If you move the location of a library or model file, you would need to update the database table accordingly. By specifying library search paths as part of the linkage file, you can simply specify the name of the source library or model file in the database or, better yet, not define it at all!
  • SVN Repository - this tab is present only for an SVNDbLib linkage file, and allows you to configure the connection to the Subversion repository, including the base directories therein, in which the symbols and footprint models reside.

Tips

  1. The Database Options dialog can also be accessed by clicking the Options button, in the Field Settings region of the main document window.


Applied Parameters: ObjectKind=DatabaseLink|Mode=EditConnection

Summary

This command is used to access a dialog with which to define the connection to the external database, and additional advanced options relating to

Access

This command is accessed from the Database Link Editor, Database Library Editor, and SVN Database Library Editor, by choosing the Tools » Database Connection command, from the main menus.

Use

After launching the command, the Database Connection dialog will appear. This dialog is divided into two tabs:

  • Connection - use the controls available on this tab to define the connection to an external database. Connection can be made either through the use of a Microsoft Data Link File (*.udl), which is essentially a storage vessel for a connection string, or through the use of a connection string that you 'build' yourself. The controls provided here are the same as those available in the Source of Connection region of the linkage file being edited (*.DbLink, *.DBLib, or *.SVNDbLib).
  • Advanced - use the controls available on this tab to enable/disable the use of quoting, and the quote characters used, with respect to database field (table column) entries in a Where clause, used when defining advanced matching criteria for the link file. Most databases have tables that are identified by the table name. Other databases, such as Oracle, have tables that also have a prefix called table schema name. Enable the corresponding option provided, to include such tables. You also have a control for defining the type used for new data fields.

Tips

  1. Any database which provides OLE DB support can be connected to. The options provided in this region of the window each use an OLE DB connection string to connect to the target database. Some databases may not offer OLE DB support. However, virtually all Database Management Systems in use today can be accessed through the Open Database Connectivity (ODBC) interface. The database link feature uses Microsoft's ODBC provider, which allows an ADO (ActiveX Data Object) to connect to any ODBC data source. The result is that any ODBC database can be connected to. The OLE DB provider for the ODBC database is specified as part of the connection string.
  2. The Select Database Type option - in the main editing window for the linkage file - simply offers an expedited method of creating a connection string when the target database has been created using Microsoft Access or Microsoft Excel. Using this option, simply select the database type and then browse to and select the required database file. The corresponding connection string will automatically be composed and entered into the field for the Use Connection String option (in the main editing window, and reflected on the Connection tab of the Database Connection dialog).
  3. When quoting tables, the specific quote characters used will depend on the database you are using. For example, square brackets [ ] are only usable in Microsoft databases like Access, Excel via ADO, or MSSQL (later versions). MYSQL would use the ' character for quoting. You really only need to quote column names, in any database, if they include spaces or are reserved words (for that database). Check the documentation for your particular database software to see which quote characters are used (if any).


Applied Parameters: ObjectKind=DatabaseLink|Mode=ImportFromIntLib

Summary

This command is used to access the Integrated Library to Database Library Translator Wizard. Use the Wizard to convert your company Integrated Libraries into the Database Library structure. The Wizard essentially decompiles nominated integrated libraries, with each library used to build a separate database table in a chosen target database, complete with parameter and model information extracted from the components therein. A specified Database Library file is then used to provide connection to that database.

Access

This command is accessed from the Database Library Editor by choosing the Tools » Import From Integrated Libraries command, from the main menus.

Use

First, ensure that the Database Library file to be used as the linkage file to the external database, is open as the active document in the main design window.

After launching the command, the Integrated Library to Database Library Translator Wizard will appear. Use the pages of the Wizard to set up for translation as follows:

  1. Specify the Target Database - this can be either a new Access database, or an existing one. For an existing database, if a table already exists with the same name as an integrated library, the information from that library will be appended to the existing table.
  2. Specify the Target Database Library - either specify the path and name for a new Database Library file to be created or browse to and open an existing file. Typically, you would use an existing DBLib file when converting one or more integrated libraries into the existing Access database to which the DBLib file is currently connected. If you do use an existing DBLib file and the target database is changed, after the Wizard finishes, the DBLib file will be connected to the new target database.
  3. Choose the Integrated Libraries - specify the integrated libraries that you wish to convert. Use the Add button to access the Select Source Integrated Libraries dialog, from where you can browse to and select the required libraries. The constituent schematic symbol and model libraries (where they exist) will be extracted and saved into the location specified in the Destination Folder field.

After choosing the source integrated libraries, click Next to proceed with the conversion. A progress bar will be displayed, along with information on the current library being translated. After the conversion has completed, click Finish to make the specified Database Library file active in the main design window.

Tips

  1. The Wizard will only extract footprint model information - in terms of model reference and path to that model. For PCB3D and Simulation models, link information will need to be entered manually into the external database.

 

Обнаружили проблему в этом документе? Выделите область и нажмите Ctrl+Enter, чтобы оповестить нас.

Связаться с нами

Связаться с нашими Представительствами напрямую

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
Вы сообщаете о проблеме, связанной со следующим выделенным текстом
и/или изображением в активном документе:
Бесплатная пробная версия Altium Designer
Бесплатная пробная версия Altium Designer
Давайте приступим. Для начала, Вы или Ваше предприятие уже используете Altium Designer?

Если Вы хотите поговорить с представителем, пожалуйста, свяжитесь с местным офисом Altium.
Copyright © 2019 Altium Limited

В таком случае, для чего Вам необходима пробная лицензия?

Если Вы хотите поговорить с представителем, пожалуйста, свяжитесь с местным офисом Altium.
Copyright © 2019 Altium Limited

Вам для этого не нужна пробная лицензия.

Нажмите кнопку ниже, чтобы загрузить установщик самой новой версии Altium Designer

Загрузить установщик Altium Designer

Если Вы хотите поговорить с представителем, пожалуйста, свяжитесь с местным офисом Altium.
Copyright © 2019 Altium Limited

Пожалуйста, заполните форму ниже, чтобы получить ценовое предложение.

Нажимая [Получить бесплатнную пробную версию], Вы соглашаетесь с нашей Политикой конфиденциальности. Вам могут приходить сообщения от компании Altium, и Вы можете изменить настройки уведомлений в любой момент.

Если Ваша подписка Altium активна, у Вас нет необходимости в пробной лицензии.

Если у Вас нет активной подписки Altium, пожалуйста, заполните форму ниже, чтобы получить пробную версию.

Нажимая [Получить бесплатнную пробную версию], Вы соглашаетесь с нашей Политикой конфиденциальности. Вам могут приходить сообщения от компании Altium, и Вы можете изменить настройки уведомлений в любой момент.

Для чего Вы хотите попробовать Altium Designer?

Если Вы хотите поговорить с представителем, пожалуйста, свяжитесь с местным офисом Altium.
Copyright © 2019 Altium Limited

Вы нашли нужное место! Пожалуйста, заполните форму ниже, чтобы начать использование пробной версии.

Нажимая [Получить бесплатнную пробную версию], Вы соглашаетесь с нашей Политикой конфиденциальности. Вам могут приходить сообщения от компании Altium, и Вы можете изменить настройки уведомлений в любой момент.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

Нажимая [Получить бесплатнную пробную версию], Вы соглашаетесь с нашей Политикой конфиденциальности. Вам могут приходить сообщения от компании Altium, и Вы можете изменить настройки уведомлений в любой момент.

Вы можете загрузить бесплатную лицензию средства просмотра Altium Designer Viewer сроком действия 6 месяцев.

Пожалуйста, заполните форму ниже, чтобы запросить эту лицензию.

Нажимая [Получить бесплатнную пробную версию], Вы соглашаетесь с нашей Политикой конфиденциальности. Вам могут приходить сообщения от компании Altium, и Вы можете изменить настройки уведомлений в любой момент.

Замечательно! Создавать новое - отличное занятие. У нас есть превосходная программа для Вас.

Upverter - бесплатная платформа, разработанная специально для любителей проектирования.

Нажмите здесь, чтобы попробовать!

Если Вы хотите поговорить с представителем, пожалуйста, свяжитесь с местным офисом Altium.
Copyright © 2019 Altium Limited

Вы можете загрузить бесплатную лицензию средства просмотра Altium Designer Viewer сроком действия 6 месяцев.

Пожалуйста, заполните форму ниже, чтобы запросить эту лицензию.

Нажимая [Получить бесплатнную пробную версию], Вы соглашаетесь с нашей Политикой конфиденциальности. Вам могут приходить сообщения от компании Altium, и Вы можете изменить настройки уведомлений в любой момент.