Most of the information contained in these release notes is not included in the Capture manuals or online help. Please read the notes carefully to see if any apply to your designs.
These release notes are divided into the following sections:
The new spreadsheet editor in the schematic page editor can be configured to display any combination of properties for parts, nets, pins, and title blocks.
The spreadsheet editor shows instance and occurrence properties of objects at the same time. Occurrence properties can be hidden so only instance properties are shown.
Capture automatically assigns reference designators as you place your parts.
A new project wizard assists in creating the appropriate project for your design (PCB, PLD, general analog or mixed-signal circuit, or a plain simple schematic).
A new licensing approach that allows management of multiple seats floating across multiple clients.
Deleting net name in property editor causes crash. When you want to delete a net name from a net, select it on the schematic page, and press DELETE. Do not delete a net name from the drop down list in the property editor. If you are using Windows 98, this will cause a crash. Always delete from the schematic page rather than the property editor.
Schematic page can be "orphaned" when project manager closed. As in Capture v7.20, it is possible for a schematic page to be left open after a project manager is closed in Release 9 of Capture. Capture allows editing of that page, but any changes that you make are not saved to the design. To avoid problems simply close the orphaned page.
"Rebuild Physical Annotations" should be named "Rebuild Occurrence properties". Release 9 allows you to work in a single view rather than working with Logical or Physical mode. In this single view you will see both the Instance and Occurrence properties of your parts, nets, pins, and title blocks, in the design. In v7.20, Capture displayed instance properties in the Logical mode and the occurrence properties in the Physical mode. The Rebuild Physical Annotations command works the same in Release 9 as it did in v7.20; it deletes all the occurrence properties from your design, and makes the instance properties shine through to the occurrence properties. The Rebuild Physical Annotations command is on the Design menu when you are in the project manager. For more information on Single View, and Instances and Occurrences, read The project manager (pages 6-10) and Editing properties (pages 29-36) in Chapter 2 of the Capture User's Guide.
Design Rules Check flags an error when port names don't match due to case differences. Design Rules Check incorrectly flags hierarchical ports and matching hierarchical pins when the case of the characters are different. For instance if you have a hierarchical pin on a hierarchical block named "B2," and the hierarchical port that it connects to in the child schematic is named "b2," then DRC gives you two warnings. The netlist is not affected.
WARNING [DRC0013] Port has no matching pin in part instance above b2: SCHEMATIC2, PAGE2 (2.70, 0.60)
WARNING [DRC0014] Type of pin above does not match the pin type of corresponding port below hb0,B2: SCHEMATIC1, PAGE1 (3.20, 1.10)
Design Rules Check ignores scope in hierarchical designs. For hierarchical designs, Design Rules Check descends through any hierarchical block in the selected schematics, ignoring the fact that you've selected "Check Selection."
BOM takes header information from Page Number 1 as defined in Options, Schematic Page Properties. The Page Number is defined in two different places in Capture. It is defined inside the database and this is made visible if you open a page and look at Options, Schematic Page Properties, Misc. tab. It is also the Page Number property associated with the title blocks in the design file. Capture Release 9 places the Title, RevCode, and Document property values from the title block defined as Page Number 1 in Options, Schematic Page Props, into the BOM.
To force Capture to use the Title, RevCode, and Document Property values from the page whose title block defines Page Number 1, copy the pages into a new design file. Copy the page with the title block that has Page Number 1 defined in it first. Then copy the remaining pages to the new design file.
Clearing the selection in the Project Manager is not intuitive. When you select multiple folders in the project manager you cannot simply double-click inside the selection group to change the selection. To deselect, click on a folder outside of the selected set of folders.
Spaces in path name cause Capture to ignore a separate .INI file. You can set up a separate Capture icon that called for a unique CAPTURE.INI file. If the path to this CAPTURE.INI file contains a space in any of the directory names, it is necessary to use quotes to delimit it. For example, in the properties of your shortcut, the Target would read:
Replace Cache on all the parts in the design cache can cause a crash in older designs. Using Replace Cache on all the parts in a design can cause a crash in older designs. When this happens, Capture encounters one or more parts that are no longer used in the design. Before replacing the cache on multiple parts in the design cache, clean up the cache using the Cleanup Cache command on Design menu.
Import properties produces an ERROR [IMP0007] (Line 8) Part not found in design or library. When Import properties produces an "ERROR [IMP0007] (Line 8) Part not found in design/library" message, you have a design with multiple schematics that all have PAGE1 in them. It is necessary to uniquely name each of the pages in the design before using Export Properties. This will produce a file containing all the properties of the parts and or pins in the design. Notice that these are grouped by page.
Invisible power pins connect to a wire if the wire end is positioned at the end of the pin. This particular problem may occur when you have short or line length power pins that are invisible in the schematic page editor. If you position the end of a wire, or a junction between wires at the end of the invisible power pin, the wires are connected to the power pin in the netlist. To avoid this situation, use zero-length power pins when you create your custom parts.
Invisible power pins will connect to wire if wire end is positioned on end of pin. When you create a page with a pin to pin spacing that is other than 0.10 inch (default), it will be difficult to edit the placement of the property values in your title block. To avoid this problem use the Browse spreadsheet to edit the values of the properties in your title blocks. All the properties in your individual title blocks can be displayed by going to the project manager, selecting the design name and choosing Browse and then Title blocks from the Edit menu. Then select the title blocks you wish to edit, and Properties from the Edit menu to display the Browse Spreadsheet. Editing your title block property values in this spreadsheet will leave them correctly placed in the title block.
Once a hierarchical pin is placed off-grid, it cannot be snapped back onto grid. If you place a hierarchical pin with the snap to grid function toggled off, it will be placed off-grid. From then on it cannot be moved back onto grid even when the snap to grid function is toggled on. you will have to deleted and replace it on the hierarchical block.
Changes to fonts in the Design Template dialog box don't affect all designs. The font settings in the Design Properties dialog box are meant to globally control the font size and type of all the different types of text in the design, for any new designs that you create. In Release 9, these settings don't affect the fonts displayed on hierarchical blocks, border text, or net names. The pin names in hierarchical blocks and net names are always displayed in Arial 7. Border text is always set to Arial and it will scale up and down in size with the width of the border.
It is possible to place parts off grid even when the snap to grid function is toggled on. Placing a part or a selection of parts too close to the border of the page can cause them to be placed off-grid, even when the snap to grid option is not selected. As a consequence, you will not be able to connect to the pins of parts. To avoid this, leave at least one grid space between the border of your page and where you intend to place your parts.
Repeatedly editing a part in place eventually causes Capture to crash. Avoid repeatedly editing a part after it is placed in a design. When you want to make changes to a part, make them in the library, and then update the cache from the design cache of your design to bring the changes into Capture.
Pin numbers of 4 characters or more will be displayed too close to the part border on the bottom of the part. Pin numbers of four or more characters may be displayed too close to the part border on the bottom of the part. When you place a part in a design that has vertically placed pins on the bottom of the part, long pin numbers can be displayed and printed on top of the part border, thus obscuring them.
To avoid this problem, place the pins with the shortest pin numbers on the bottom of the part when you place your pins on your part.
Not able to change part from Normal to Convert view inside Schematic Page. Once you place a part on a schematic page in Release 9, you will not be allowed to change it from Normal to Convert. This functionality will be added back into Capture at a later date.
Zero length pins do not show on schematic page. In Release 9, zero length pins are not visible. If the pin is not a power pin and it is not connected to a net, then the gray connection square is displayed indicating the position of the pin on the part border. Zero length power pins will only indicate their visibility by the visibility of their pin name and number near the position of the pin in the part placed on the page.
Dragging parts in direction of wires connected between pins can cause changes in connectivity. Single segment wires between two pins on a part may move inconsistently when the part is moved in same direction as the wire. If you have placed a 7400 part with a wire drawn between pins 1 and 2, and you drag the part vertically, you will see the wire move incorrectly.
When you need to move parts about on the schematic page, block select the wires around them as well, then they will stretch, drag or move as appropriate with the parts.
Preview of an imported selection shows text that is too large in some cases. The text size in the preview window is essentially zero. Microsoft Windows response to a zero-size font is to give you a default size font, for instance size 12. So, the preview looks bad with the pieces of text being written on top of one another, but when imported and placed on the schematic page, the text is properly sized.
Parts without pins don't stay on grid when placed on a schematic page. Capture uses the end of a pin as a reference guide to allow movement of parts on the grid in the schematic editor. When there is no pin on the part, the part is treated like a graphic and the geometric center of the part is used as a reference point.
To avoid this problem, copy and paste the part instead of moving it.
Moving the first vertex of a polyline reveals another segment. If you want to edit the shape of a polyline, use any vertex except the first one placed. When you try to move the first vertex, you will find that another segment is drawn. This can be confusing. Avoid this by using the other vertices to change the shape of the polyline or redraw it.
Parts contain a polyline graphic. If you placed a polyline inside your custom part, every time you close the part in the part editor, Capture asks if you want to save the changes. Even if you just open then immediately close the part, the message box asks if you want to save the changes.
The Save As command is not available when editing a part inside the library. This functionality was disabled in Capture v7.10. If you were allowed to save the part under a different name, the schematic would have no way to access the new part.
When you want to create a part similar to an existing part, select the part name in the project manager, and choose Copy from the Edit menu. With the same part selected choose Rename from the Edit menu to change the name of the part in the library. Then, select the name of the library (.OLB) in the project manager and choose Paste from the Edit menu to paste back in the original part. This creates two uniquely named parts that are identical in the library.
Before translating a Schematic's design set grid spacing to be either 0.10 inch or 2.50 mm. If you translate a Schematic's design with a grid spacing other than 0.10 inch or 2.50 mm into Capture Release 9, everything will be translated in off-grid. The resulting translated schematic pages preserve all connectivity, but when trying to edit the objects, they will snap to grid. To avoid this either change the grid spacing in your Schematic's design before translation and move everything on grid, or after translation select all the objects on the page and move them together to make them snap to grid. Set the grid spacing before translation to be 0.10 inch or 2.50 mm in your Schematic's design.
Translator does not detect when a Global Symbol is connected to a hierarchical port or off-page connector. In Capture when a hierarchical port is connected to a global symbol or net, that net is isolated to the schematic folder. When an off-page connector is connected to a global symbol or net, that net is isolated to the schematic page. Thus, the net is no longer global in nature and the netlist will be changed. The Schematics to Capture translator does not detect this condition in the translated design. Use Hierarchical Ports and Off-page Connectors commands from the Edit menu's Browse command to find these connections. When you find one, delete the off-page connector and replace it with a power symbol (global symbol). If the global is connected to a hierarchical port, you may have to rework the schematic so that the global is not connected to the hierarchical port. Or, you may be able to delete the port or off-page connector and connect the net to a power symbol.
Capture can't find the SDT library if the file uses the same name as the associated schematic file. If the SDT library name (*.LIB) is the same as the schematic file (.SCH) that you are trying to translate into Capture, then you must rename the .SCH file and try to translate again.
Tab spacing is not changeable in text editor. In Capture Release 9, the tab spacing cannot be changed from the 0.25 inch default setting. The tab spacing that you set in the Preferences dialog box's Text Editor tab does not affect this setting.
Layout Macros no longer necessary. Chapter 18, Preparing your Capture design for use with Layout of the Capture User's Guide, describes how to find and use the Layout macros. These macros were used in v7.20 to apply specific Layout properties to parts, nets and pins in your design. These macros are no longer necessary, nor are they supplied with Release 9.
Property editor filter replaces Layout macros. Capture Release 9 includes a new filtering function that is part of the property editor. This Filter drop down list allows you to select from prepared templates what properties are displayed in the Property Editor. When you choose the Layout filter, all the associated part, pin, or net properties will be displayed in the spreadsheet. When you add a value to any cell in that spreadsheet, the property and the value you entered will be applied to the part or pin or net.
Use Layout properties in property editor using Layout filter. Use the Layout properties described on pages 274 through 280 in the Capture User's Guide, in the property editor. These properties automatically appear when the Layout filter is used.
Archive menu command. You can use the Archive menu command to save your project and associated files to a different directory. The Archive menu command is accessible if the Project Manager window in Capture is active. Use the following steps:
From the File menu, choose the Archive Project command. The Archive Project dialog box appears.
Specify the directory to which the files need to be saved.
Specify what optional files need to be saved by selecting the appropriate options. The library files option saves part library files and other related files (.OLB, .SML, etc.) from the Library directory; the output files option saves files generated by Capture's tools (.XRF, .EDN, etc.); the referenced projects option recursively saves any projects referenced from within the current project.
For PSpice projects, the simulation profiles and the local files (.LIB, .STL, .INC) are archived along with the project. The output files option currently does not archive simulation output files (.DAT, .OUT, etc.).
Using the Save As command. A Capture a design file (.DSN) is always accompanied by a project file (.OPJ). Each time you use the Save As command from the File menu to save a design file to another name or directory, it is recommended that you also use Save As for the project file. Use the following steps:
In the Project Manager, select the name of the design file.
From the File menu, choose Save As.
Change the drive and directory as appropriate, and then select the filename.
Click Save.
Select the Design Resources folder.
From the File menu, choose Save As.
Change the drive and directory as appropriate, and then select the filename.
Click Save.
This process saves a .DSN file and an .OPJ file into the same directory and allows you to continue editing the current project without altering the original files.
Displaying occurrences. In the property editor, when you want to display all the occurrence properties on your parts, nets, pins or title blocks quickly, press and hold the CTRL key while clicking on one of the plus (+) symbols in the left most column. If you then click on the dash (-) symbols in the left column, all the occurrences collapse so that you only see the instance properties of your design.
Saving schematic pages and folders. In Capture v7.20, saving schematic information was done on a page by page basis, with Capture prompting you when the page or design was closed whether or not to save each page. In Release 9, this paradigm has been changed. Now, when you make changes to the pages in your schematic folder, you have the option to either save all the pages in the folder or none of them. Thus, if you make a change in SCHEMATIC1 to PAGE1 and a change to PAGE2 and you close the design or one of these pages, you will have to keep the changes on both pages or none of the changes made to the pages.
Property editor filter. The property editor's filter allows you to filter the properties displayed in the spreadsheet. Since there can be hundreds of properties assigned to your parts, nets, pins, and title blocks, it is more efficient to view only the properties that you want to see. Capture provides a template that defines the properties that are displayed if you are targeting your design for Layout, or PSpice, or a number of the digital tools that Express supports.
To see this filter in action, open a page in a design and choose Select All from the Edit menu. Click the right mouse button, and choose Edit Properties from the pop-up menu, to display the property editor. Click the Parts tab to display all the properties of the parts you selected. The filter drop-down list is near the top of the window to the right of the command buttons. Click the filter's down arrow to expand the list and select, for instance, Layout. The displayed properties are changed to include those properties that you might want to apply to your parts for use in your Layout netlist. When you enter a value into one of the cells in these columns, and click Apply, the property with the new values are applied to your part.
Property editor elements. The figure below is a picture of the property editor illustrating the way properties are displayed. Library definitions, instance properties and occurrence properties are all shown. Library definitions (and package properties from library parts) are shown in cells that have a white background with grey slashes. Instance properties are shown in cells with white backgrounds. Occurrence properties which "shine through" from the instance property are shown in cells with yellow background and grey slashes. Occurrence properties which override the instance values are shown in cells with a yellow background. It is possible to have properties without values. These are shown as cells that have a white (instance) or yellow (occurrence) background with no values. Some of the cells have a drop down list or browse button as appropriate.
Capture's libraries have been updated. Many new parts were added, and the parts are now grouped by type instead of by manufacturer. When you do a typical installation of Capture, you get these new libraries. If you are an experienced Capture user, you may find that your favorite parts are now located in different library names. If you want the original Capture libraries installed along with the new libraries, then do a custom installation and select the Previous Capture Libraries option as one of the items to be installed. Or, you can search the new libraries using the part search capability in the Place Part dialog box to locate the parts you are accustomed to using in the new libraries.
