In TimingDesigner, open a new diagram by choosing File - New. From the file menu choose, Import/Merge and under the files of type, select Value Change Dump. Select the saved VCD file and press Open. Now the file import dialog box appears, in which you can choose preferred signals from the list of available signals.

The diagram will contain all of the graphical elements of the waveforms that were produced by the NC-Sim output, but will contain causal relationships. Timing relationships are represented only as edge positions. A VCD file doesn't provide causal information. Only the waveform names, specific points of change on each waveform at a given time, and the value to which the waveform changes is what are contained in a VCD file. A fully annotated diagram may originate this way, allowing the designer to add timing and edge relationships to complete the diagram.

Return to EMA Currents eNewsletter

Printer friendly version

Split Part symbol generation - enhancement in OrCAD Capture 10.5

The Split Part feature was introduced in OrCAD Capture® 10.3 and was well received by OrCAD Capture users worldwide. Enhancements to this same feature in OrCAD 10.5 make it more powerful and now even easier to use.

The Split Part section input spreadsheet in OrCAD Capture 10.5 allows you to:

• Split a part into multiple sections
• Choose the numbering format that should be used for numbering sections in the split part (i.e. you can split a part into multiple sections that are alphabetically numbered)
• Enter or select a section from a drop-down list you want to associate with a specific pin
• Add and/or delete new pins to the Split Part Section Input Spreadsheet
• Save the selected part as a new part with a new name in the same library with changed property values

You may need to split a part into multiple sections in the following situations:

• Using large pin-count designs - To manage large pin count devices in your design, you can split the part into multiple sections based on your specification and you can place different sections on different schematic pages, which will ease the design process.
• Partitioning a large part based on its functionality - In certain situations it is advantageous to partition a large part based on its functionality and work with sections individually/separately (for example, you want to create different sections for pins with the same voltage rating)

To use this option at the source library, select the symbol that needs to be split into multiple sections, RMB click and choose Split Part or Tools - Split Part

Return to EMA Currents eNewsletter

Printer friendly version

How do I create a new part from a spreadsheet?

You can use the New "Part Creation Spreadsheet" to create new parts (multi-section/single-section). The New Part Creation Spreadsheet has a spreadsheet like interface, it allows you to paste content copied from a part data sheet into the spreadsheet. Each row in the New Part Creation Spreadsheet corresponds to a pin while each column corresponds to properties associated with the pins. The property names are listed as the column header.

Please Note: Before you copy and paste part information (pin number, pin name, pin type, etc.) from a datasheet, make sure that you arrange the part information in the same column header format/sequence as it appears in the New Part Creation Spreadsheet.

To create a new part from a spreadsheet:

1. Select a library (.OLB) file that will contain the new part in the Project Manager.
2. Select the Design menu and choose the New Part from Spreadsheet command or right-click on the library file and select New Part from Spreadsheet from the pop-up menu. The New Part Creation Spreadsheet appears.
3. Specify a name for the new part in the Part Name text box.
4. If you want to create a multi-section part, specify the number of sections you want to have in your new part in the No. of Sections text box. The New Part Creation Spreadsheet creates single-section parts, by default.
5. Specify a part reference prefix for the part in the Part Ref Prefix text box.
6. Select Numeric or Alphabetic in the part numbering group. If you select Alphabetic, a letter (between A to Z) will be added as a suffix to the current part reference for each of the new parts. If you select Numeric, a number (between 1 and 1024) will be added as a suffix to the current part reference for each of the new parts. To sort on any property, double-click its name in the column header.
7. Specify a name for the pin in the Name Property column.
8. Select the type of pin from the Pin Type Property column list box.
9. Select a shape for the pin from the Shape Property column list box.
10. Specify a value for a swappable (input) pin of the part in Pin Group text box.
11. Select the position where you want this pin to appear in the part for the Position Property column list box.
12. Select a section number you want to associate with the pin from the Section Property column list box.

* For more information on this feature see page 146 in the OrCAD Capture User's Guide

Return to EMA Currents eNewsletter

Printer friendly version

Figure 1: A design with DRC error

Figure 2: A view of the source part

Figure 1 - Illustrates a section of a design which has the DRC error (DRC0031) and the schematic appears to be correct. The homogeneous OPAMP part U9 has its power pins 4 & 11 connected ONLY to power nets +5V and -5V and NOT to multiple nets. However, when you observe the actual part (the OPAMP U9) either at its source library (by opening the corresponding .OLB file) or by choosing to Edit Part at the schematic level, you can see where the problem is.

Figure 2 - presents a view of the OPAMP U9 at its source library where the power pin 4 is called Vcc. However on the schematic, only U9A is physically connected to power net +/-5V but the other sections of the same part, U9B and U9C are left unconnected. OrCAD Capture expects an explicit connection to power nets +/-5V at the power pin sections of U9B &U9C else it internally connects them to Vcc. In this example the power pins of U9B, C are left unconnected and this leads to a mismatch, which OrCAD Capture then reports as a DRC Violation.

To solve this problem, you can either rename the power pins at the source library to match the power net to which it is going to be connected in the schematic level (here change from Vcc to +5v) or connect all the power pins of all the parts in the package that is placed in the schematic, explicitly to the appropriate power nets (here connect all pin 4's &11's to +/-5V).

Return to EMA Currents eNewsletter

Printer friendly version

Edit>Properties adjust your find filter for nets

Type in the name with which you want to identify the net i.e. Clock

After the nets have been identified in the constraints you need to add a constraint set name called CLOCK. Customize the design rules for these nets as needed i.e. set line to line at 10 mils.

Once the design rules have been set you need to open the assignment table. In the assignment table you need to set which rules are applied when nets of different types are near each other.

If a CLOCK TYPE is next to a DEFAULT TYPE, apply the CLOCK rule. If a DEFAULT TYPE is near a DEFAULT TYPE, apply the DEFAULT rule. Any number of combinations can be defined in the table. The more NET_SPACING_TYPE's there are in a design, the more possible combinations have to be considered.

Nets can only have ONE spacing type assigned to them.

Setup>Constraints>Spacing rule set > Assignment table

Net physical types are applied and treated in the same way. A NET_PHYSICAL_TYPE is applied to a net or group of nets (e.g. 8mils)

Edit>Properties adjust your find filter for nets

In the constraints create a set of design rules for this group of nets. (e.g. 8mils) adjust the rules to your requirements line width or vias.

Setup>Constraints>Physical (lines/vias) rule set >Set Values

After the rules are defined for this group of nets the assignment table needs to be reviewed just like in the NET_SPACING_TYPE to adjust which rule is applied to which nets when different conditions exist.

Setup>Constraints>Physical (lines/vias) rule set >Set Assignment Table

Return to EMA Currents eNewsletter

Printer friendly version