Before Next Index

4. Questions about net output

1. When outputting PWS/CCF nets, an error "No part name has been input" is encountered and no nets can be output.


The properties required for PWS/CCF nets to be output are "Reference" and "Pin number." However, when outputting DEFINITION sections, "Part name" is also required. This is why an error message "No part name has been input" is output.

When outputting CCF nets, you can choose whether you want the CCF nets to be output with or without the DEFINITION sections. Therefore, if you want to output CCF nets using only Reference and Pin number, choose "Without DEFINITION."




2. When outputting nets, does the system look up the contents registered in the LCDB (Component Database for Schematic Design)?



Yes, the system looks up the LCDB (Component Database for Schematic Design) as it outputs nets.

However, this library can only be referenced.when "CDB name" (cdbName) and "Component name" (componentName) are set as part properties.

The LCDB is referenced when the default power supplies and default grounds are used to represent power supplies and grounds on the schematic.

CR-5000 System Designer Operation Guide -MASTER-
Chapter1. Editing Schematics 1-7-1 "Power and Ground Net"




3. The system outputs the components I do not want to be output in part lists.



The parts output to part lists by the Netlist Processor can be limited by "Format file" ($ZDSROOT/etc/xx.frm) and "Component property."

For the components you do not want to be output to part lists, set "NO" for the property: "Part Output to Part Lists by Processor (uselnPartslist)." In this way you can inhibit the components from being output within the format file.

Part table (sample) $ZDSROOT/etc/samplep.frm
$ZDSROOT/etc/samplep.frm

If undesired components are still output to part lists even though the property value is set correctly, there is a possibility that the format file is set to ignore the properties in it. Check the format file.




4. Although nets are output, a message "No CDB name has been input" is displayed. Is this a problem?


This varies with each netlist that is output.

The CDB name (cdbName) is required when the LCDB (Component Database for Schematic Design) is referenced for components.

When creating schematics, if you input symbols in symbol selection, no CDB name is input. If you input symbols in part selection, CDB names are input because the LCDB is referenced.




5. An error/warning occurred when outputting netlists. I want to know which component is the cause of this error.



There are two methods for outputting netlists: one by using the Sheet Editor and one by using the Netlist Processor. In either case, you can check which components are causing the error.

Checking from the Sheet Editor
If you use the Sheet Editor to output netlists, you can bring up a dialog box for checking error/warnings.
When you click on a message in this dialog box, the corresponding object (component or pin) is selected in the editor.

Checking from the Netlist Processor
If you use the Netlist Processor to output netlists, you can bring up a dialog box for checking error/warnings. If the schematic sheet is open, click on a message in this dialog box and the corresponding object (component or pin) will be selected in the editor.
Open the schematic sheet and while checking messages, use the Sheet Editor's select dialog box of specified object to check the components in error using component IDs and so forth as the keyword.




6. Is there any way to output netlists in DOS format?



You can output files in DOS format by setting the following in the netlist output format file (xxx.frm).

file Format: Dos text

Settings in $ZDSROOT/etc/samplep.frm




7. I want to change the format of part lists.



Use the format file (xxx.frm) to change the output format of part lists.

CR-5000 System Designer Operation Guide -MASTER-
Chapter1. Editing Schematics 1-7-1 "Power and Ground Net"



8. Is it possible to output nets for one sheet among schematics of multiple sheets?



When outputting from the Netlist Processor, you can specify the sheet you want to be output.

When selecting [Utilities]-[Forward Annotation] from the Sheet Editor, all the sheets are to be outputted to the netlist.




9. I want to know about the properties required for outputting GNF nets for PWS.



The following properties are required:
Part name (partName)
Function name (function)

Pin name (pinLabel)

Unless these properties are set, an error is generated and no nets are output.




10. What properties are required for outputting ECF nets for PWS?



The following properties are required:
Reference (reference)
Pin number (pinNumber)

Pin name (pinLabel)

Unless these properties are set, an error is generated and no nets are output.

Although nets can be output even when the part names (partName) and function names (function) are not set, they must always be set in PWS.



11. I don't know what the errors that occur when outputting nets mean, or how to correct the problem.



Regarding details, please refer to the online help.

Online help
[Guide to Applications] - [Transferring Data from/to PCB Design CAD] - [Transferring Data from/to PWS] or[Transferring Data from/to Board Designer] -[Trouble shooting]


12. If the Parts List output totals more than 1000 items, it will be written as "1k", but I want to write "1000" and output it as is.


Add a description "useSI:no" to the [File Format Define] section in the Component List Format file (.frm).

This is available in Rev.4.040 or later



13. I do not want to output No Mount parts to net lists or part lists.


"No Mount" is a property set for parts that are not to be mounted depending on the destination when Destination Management is used.

Net lists and part lists output
Destination operation for net lists and parts lists output means that parts differ with destination and that property value differences and other differences can be output.
It cannot be used to process schematics where the net lists differ by destination.
Consequently, parts labeled "noMount = YES" depending on destination differ only in property respects and net lists and parts lists can be output.

Consequently, parts labeled "noMount = YES" depending on destination differ only in property respects and net lists and parts lists can be output. However, parts lists can be set to not output parts labeled "noMount=YES".
This can be performed by adding the conditional statement (if noMount!="YES") in the parts list output format file.


$ZDSROOT/etc/samplepE.frm setting

"Destination Management" HOW TO USE
2-4 Creating net lists for different destinations
2-6 PCB design interfaces
HOW TO USE "For System Administrator"
Appendix A Format Definition File Reference

"Frequently Asked Questions"
I do not want to output No Mount parts during plotting or printing.

Before Next Index