Связаться с нами
Связаться с нашими Представительствами напрямую
Parent page: Designing with a Connected Workspace
Altium Designer, in conjunction with your connected Workspace, offers the ability to update components in an existing board design to use components that reside in that Workspace. The components sourced from database and file-based libraries can be individually updated to Workspace components, or batch updated using automated Parameter matching through the Altium Designer Item Manager.
Using a highly configurable rule system to target suitable components in the Workspace, the Item Manager dialog provides a fast and effective way to convert the current PCB project to one that uses Workspace Components.
The Item Manager provides two key abilities in relation to components and sheets of re-usable schematic circuitry in a board design project:
By way of background, note that an individual component in a design can be updated to a Workspace component directly from the Properties panel in the Schematic Editor. To do so, select the component on the schematic sheet and then use the panel's Source drop-down menu to choose a Workspace as the component data source – you need to be connected to the Workspace for access. The subsequent Component source dialog provides the option to select a target component from the Workspace or simply link the component to the Workspace while retaining or replacing the component identifier (Design Item ID).
If the Workspace component has been selected, the accessed component data will replace the existing component and models, and update the component parameters. The panel will also indicate the component's current lifecycle state and revision status, as shown below.
Alternatively, components can be replaced through the project's ActiveBOM document (BomDoc).
While this would be a laborious approach to updating all of a design's local components to Workspace components, in even a small-scale board design, the Item Manager provides a simple and automated conversion method that uses advanced parameter matching (Automatching) and a bulk update approach. A typical application of the Item Manager would be to update an existing board design to use Workspace components and managed schematic sheets that have been migrated to a Workspace from company libraries.
The Item Manager dialog is accessed from the main Tools menu from an active schematic document (Tools » Item Manager) and presents all components and sheet symbols found in the active board design project.
Select the dialog's lower Unmanaged or Components tab to populate the list of components in the current design. In essence, the left section of the dialog shows component settings of the active project (Current Settings), while the right section lists how they will change (New Settings) when suitable Workspace components from the Workspace have been assigned. The New Settings region has the same fields as the Current Settings region. To view and access sheet symbols, select the Sheet Symbols tab.
The way in which component data is presented in the Item Manager dialog is highly configurable, based on the data columns that are enabled and/or grouped. This allows the list of design content and their associated system/user parameters to be shown in a way that matches specific approaches to component identification – all item parameters, such as proprietary company part numbers, for example, can be displayed as needed.
To configure which columns are presented in the Item Manager, right-click in the dialog's column heading area and select Columns » Select Columns from the context menu. The Select columns dialog will offer all available parameters, including those specifically from the local design (
[Current Settings]) and the content in the Workspace (
[New Settings]). Use the 'eye' control to the left of an entry to display the column () or not ().
Hover over a column heading to expose its filter icon which when selected, allows the listing in the Item Manager to be constrained to specific entry types or to a custom-created filter.
To group the listed content data by a particular parameter column, such as component type category or schematic document, etc., drag the desired column heading entry to the dialog's upper title row (as indicated by the hint text). The content list will reconfigure to group its entries by the assigned parameter column.
Assuming that the connected Workspace is populated with collections of components and managed schematic sheets, the current board design project can be converted to using these content where a suitable match is available. The local-to-Workspace matching can be performed manually, or as an automated process through the Item Manager based on configurable parameter matching. When complete, the local component definitions will be updated to their Workspace counterparts.
To manually replace a local component (or schematic) with a Workspace version, select its entry in the Item Manager list and then Choose manually from its right-click context options. You also can double-click an item in the grid to manually choose an item. In the subsequent Replace Component dialog, browse and select a suitably matched Item in the Workspace (the latest revision of that Item will be used).
When the dialog is closed (OK), the selected Workspace component information will populate the entry's New Settings region in the list. Note that since the entry is now a pending Workspace entity, the updated entry is transferred from the listing under the Unmanaged tab to the list under the Managed tab.
To automate the process of choosing matching Workspace content, the Item Manager provides a configurable auto-matching capability that attempts to match each local design component with a component in the connected Workspace. When a match is found, that Workspace component will be proposed for the update.
The key to the Item Manager's automatic parameter matching capabilities is the update rules and options available in the Item Manager Options dialog, accessed from the Item Manager dialog's button. The configurable rules determine which component parameters in the active (local) design are matched to the parameters of all Workspace components in the selected Source server.
How effective these rules are in achieving a local-to-Workspace component match will depend upon the available component parameters, which will be specific to company systems or individual preferences. In the simplest but perhaps unlikely scenario, the Comment or Component Name parameter entries may match between the local and equivalent Workspace components. In the ideal case, however, both the local and Workspace components will share a company reference or manufacturer part number parameter.
To create such a part number rule, for example, select and modify an existing rule (which can also be renamed) or use the button to create a new rule – a rule must be selected (checked) to be edited. Note that the Local Parameter and Server Parameter selection drop-down lists are independent, which allows differently named parameters to be nominated – in the below example, the local
Libray Reference parameter and the Workspace
Part Number parameter represent a company part reference number.
Running a part/reference number matching rule such as above is likely to create a near-complete match between the local and Workspace components. With the rule established, the matching process is initiated by the button in the Item Manager dialog.
When a match cannot be found, the entry will appear with the status icon, be in red text, and a reference included indicating the reason for the error or matching failure – a different or additional Rule will need to be created to achieve a successful match for those components. Also note that a rule may detect more than one Workspace component as a match, which is considered as a successful result but requires manual intervention to resolve. This conflict is regarded as an 'ambiguous' result, and can be resolved in the Item Manager dialog – see below.
When the automatch process is complete, close the Automatching items dialog (OK) to populate the Items Manager dialog with the proposed new component settings. The pending Workspace content that will be applied to matched entries are listed in the New Settings region under the dialog's Managed tab, or under the Components tab along with content that have not been matched.
To resolve any ambiguous content, generally caused by multiple matches, select the Ambiguous Items (or Ambiguous Footprints) tab and make a suitable choice from the drop-down menu of the Revision HRID cell in the dialog’s New Settings section (which displays as <Not selected> by default). Note that multiple matches, and therefore the available choices, can in fact be referencing different revisions of the same component. When the issue is resolved (no longer classed as ambiguous) the component entry will move to the Managed/Components tab lists.
As outlined above, Item Manager rules establish parameter matches between the local project components and Workspace components. Any number of rules can be created, and these work on descending priority basis. If the first (top) rule fails, then the next rule is applied – effectively a sequential Boolean OR relationship. A rule is active only when its associated checkbox is enabled.
When the automatch process is run, the State Notes column in the Automatching items dialog indicates which rules have failed in finding a match. In this case, a different or new rule is required to satisfactorily match the available parameters.
Use the Item Manager Options dialog’s button to create a new rule, and the associated button to apply multiple parameter matching conditions. As each parameter condition is added the rule becomes increasingly specific, and all conditions need to be satisfied before the rule match succeeds – effectively a Boolean AND condition.
Taking the example shown here, where (say) the components cannot be matched by part/reference number parameters, a new rule can be created to match suitable specifications for the listed unmatched capacitors shown above.
The Item Manager Options dialog provides a range of content updating options that can be used to further refine how automatched Workspace components are applied to the current board design.
The options are applied to the current design via the ECO process, and behave as follows:
The Library Update Settings dialog includes a list of all available parameters, for all components, in the current board project (right-click to access mass on/off functions). Those parameters checked in the list will be updated when a local component is replaced with/updated to a Workspace component – the behavior of that update is determined by the options outlined below.
The parameter replacement (or addition) behavior is determined by the lower two options in the dialog:
The proposed changes that have been set up in the Item Manager are applied to the current board design by generating and executing an Engineering Change Order (ECO). Select the range of listed components you wish to update, and then the desired ECO option from the button menu – the options are:
The executed ECO process will update the project components accordingly, which will then be listed in the Item Manager dialog as currently up-to-date Workspace components. Note that the previous icon for each entry () has changed to indicate the reference to a Workspace component ().
In the schematic editor, the updated components are linked to their matched components in the Workspace – the active link information will detect a change in the Workspace component's revision state when/if it is subsequently updated. Select a component in the design space and note its Source and associated information in the Properties panel.
During the course of product development, it is very likely that changes will occur in the design's source components or managed schematic sheets. For example, component models may be updated to a new drawing standard, or component definitions may have been updated to add new parameters. Any such changes made to the Workspace components and managed sheets used in a design need to be detected and made to flow through to any affected schematic sheets.
For an individual selected component or sheet symbol, appropriate Component or Sheet Symbol mode of the Properties panel will provide an immediate indication that an object is out of date relative to its Workspace source data. Use the associated or button to update the data for that object from its source Workspace.
As well as being used to detect and manage components and schematic sheets that are currently non-Workspace entities (indicated as [Not Managed] and not sourced from a Workspace), the Item Manager is also used to detect and manage all content that is out of date.
When the Item Manager is opened it automatically detects and lists all components and managed schematic sheets (indicating if they are sourced from a Workspace or not), and then compares the Item-Revision of each Workspace content on the schematics against the available revisions of that content in the Workspace. If there is content that has a newer revision available in the Workspace, that is flagged as Out of date in the Item Manager's Revision Status column.
To bring the out-of-date content up to date, it must be selected, and then the Update to latest revision command applied from the right-click context menu. The New Settings region of the dialog will then show the detail of each new Item-Revision.
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:
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. Access the Properties panel for a selected item, which will now show a link back to the corresponding source managed 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.
Before committing to a component update or change process in the Item Manager, it may be prudent to generate a snapshot of the current listing information using the dialog's Export function. To do this, right-click anywhere in the Item Manager and select Export from the context menu, and then navigate to a suitable location and name the report as required. The report is generated as an HTML file and presented with the same layout as the current Item Manager display.
Связаться с нашими Представительствами напрямую