Before Next Index

37. I want the net names automatically assigned by the system to be reassigned collectively.



For nets whose net names are not input manually, the system automatically generates net names when you save the schematic sheet. The start characters of net names used at this time conform to the description sNetNameHeader:SIGN included in the first part of

$ZDSROOT/etc/CompKind (function type definitions file)

To collectively reassign net names that were automatically assigned, search for nets that begin with these characters. Then delete the net names collectively and save the schematic sheet. The system will automatically regenerate the net names.

It is possible to delete the net names as follows.
[Attribute] -[Change Attribute] ->Select Net Name Cell -> Delite valure

Inserting net is only available in [Net/Bus Label] dialog.




38. Net names cannot be changed from the Change Property dialog box. Why?



Net names cannot be changed from the Change Attribute dialog box.

To change or delete net names, use the Input Net/Bus Name dialog box or the net browser.
Select net, and specify [Place]-[Net/Bus label].

You now can input new net names or delete the existing net names from the dialog box.

To look up or delete net names, you also can use the Change Attribute dialog box or Net Browser.




39. Is there any way for nets placed in multiple sheets to be recognized as the same type of net.



There are two ways to have nets recognized as being the same.

1. Nets can be made the same net via sheet connectors.

First, connect a sheet connector to each of the nets you want to be recognized as the same type of net. Then input the same part name for the sheet connectors.
When nets are extracted, this part name is output as the net name.

Precautions to be observed when creating sheet connectors

2. Input the same net name for the nets you want to be recognized as the same type of net.

Leave the end of the net disconnected.




40. I do not know how to connect nets to the bus.



When connecting nets to the bus, pay attention to the following:

-Net names must be input for the nets that are connected to the bus.
Unless these net names are input, net extraction will result in an error.

-Input a bus name for the bus.

Unless this is input, a warning occurs when you save the file and when nets are extracted.

The process is as follows.

1. Input a bus by choosing[Place] - [Bus]
2. Input the nets you want to be connected to the bus
(choose [Place] - [Net])

Nets and net names can be input simultaneously.
Use [Place]-[Net Increment].

CR-5000 System Designer Operation Guide -MASTER-
Chapter1. Editing Schematics 1-8-1 "Inserting nets and buses"
1-8-7 "Using Assist Menu for Inputting or Editing Nets or Buses"

3. Input a bus name for the bus by choosing

[Place] - [Net/Bus Label]

4. Input net names for the nets by choosing

[Place] - [Net/Bus Label]

There is a simpler method. You can input net and bus names by referencing those that have already been entered.
Click [Reference Input] in the Net/Bus Label dialog box.

CR-5000 System Designer Operation Guide -MASTER-
Chapter1. Editing Schematics 1-8-3 "Entering net and bus labels"

You can input net and bus names in the following formats.

- Array bus - Range specification -
Array bus name "number of start bits - number of end bits - number of bit steps"
Bus name - BUS[a-b-c]

Net name - BUS [a],BUS[a+c],BUS[a+c+c],...BUS[b]

The number of bit stepscan be omitted. When omitted, 1 is assumed.

- Array bus - Bit specification -
Array bus name [number of bits, number of bits, ...]
Bus name - BUS[a0,a1,a2,a3...]

Net name - BUS[a0],BUS[a1],BUS[a2],BUS[a3]...

- Bundle bus -
Separate arrays of bus names or single net names by a comma.
Bus name - BUS[0-4],BUS[7]

Net name - BUS[0,],BUS[1],...BUS[4],BUS[7]




41. When I try to execute Copy to Buffer, an error "Failed to copy to cut buffer" occurs.



This is probably because the directory in which the cut buffer file should be stored does not exist or you do not have permission to access the directory or existing buffer file.
When you execute Copy to Buffer, the copy target is stored in buffer $HOME/cr5000/ds/LCBUF[1~5]
Check whether this directory exists and, depending on the situation, set up the environment following the procedure described below. Also, if the directory does exist, check whether you have permission to access the directory and its files.

For UNIX versions
user setup for CR-5000 System Designer/Board Designer. Buffers, logs, and tool parameters are saved in this directory.
When a user setting is not possible, make the following entry as superuser.
/usr/local/zuken/install/setup.sh
Make the following entry in Rev 5.0 and later versions.
/usr/zuken/bin/setenv.sh
Make these entries to perform a user setting.
CR-5000 Installation Guide Vol.1

Chapter 10, "Setting Up a Personal Environment"


For Windows versions
Follow the instruction mentioned below to confirm the environment variable HOME, and if the directory named $HOME/cr5000 does not exist, create a new directory with the Explorer on Windows or cr5000 Design File Manager.
($HOME/cr5000 defaults to cr5000\home\cr5000. You may copy it to create the directory.)

How to confirm $HOME:

If the necessary directory does not exist, newly create it.




42. I want to use the figures I've created in schematics as symbols. How can I do this?



First, choose the figures you want to use as a symbol and copy it into the buffer. Next, open a new symbol file and paste the figure you just copied.

Edit the figure however you like and save the file.
1. Select the figure you want to use as a symbol, then choose
[Edit] - [Copy to Buffer] or [Copy]

2. Open a symbol file, then choose
[Edit] - [Paste Buffer] or [Paste]




43. I want to move circuits from 999.sht to 001.sht.


First, choose the circuits you want to move to 001.sht and copy them into the buffer.
Next, open 001.sht and paste the circuits you just copied.

1. Open 999.sht and choose the desired circuits, then choose
[Edit] - [Copy to Buffer] or [Copy].

2. Open 001.sht, then choose
[Edit] - [Paste Buffer] or [Paste]

Frequently Asked Questions

When copying objects or saving sheets in another name, I want to leave references and net names intact.

When you use Buffer Copy/Paste, the IDs added to the symbols are reassigned. Care must be taken when you enter Forward Annotation after using Buffer Copy/Paste. (When Forward Annotation for PWS is entered, the parts that have had their IDs reassigned are kept waiting.)




44. I want to use the default power supply and ground settings.



When connecting power supply and ground pins as parts to a single net, you can have these connections recognized by the system without having to write them on the schematics.

To do this, you need to set defaults for the power supply and ground, and then register for the LCDB.
The default power supply and ground are reserved properties set in schematics.

Leave the schematic sheet with no object selected, select [Attribute]-[Change Attribute] (or [Change Attribute] from the assist menu).
With the dialog activated, define the default power/default ground name.



Although pins 7 and 14
are not written on the schematic
(Change Attribute Dialog Box for Sheet Property)

Defined as power supply
and ground pins in the LCDB
component information.
Recognized as connected to
the default power supply and ground nets
that are defined as schematic sheet properties.

When registering for the LCDB, always make sure the package information is defined. This is because if only gate information is defined, the system cannot determine the total number of pins.




45. I do not know how to create multi-power supply circuits.


You cannot define multiple nets for the default power supply and ground.

Therefore, you need to place the power supply and ground symbols which have had part names input for each net on the schematic, and then connect the component pins.

If default power and ground are shared with others, recommendation is to set high frequency power/ground as the "default power/ground" and enter low frequency power/ground as a symbol.

For the pins to be connected, you can use pins for power supply boxes, in addition to ordinary part and gate pins.

Connect the power supply and ground symbols to the pins that are connected to the power supplies and grounds, respectively.

Input net names as part names for the power supply and ground symbols.


Connect power supply
and ground symbols to the power supply and ground pins.
Create a power supply box,then connect the power supply and ground symbols to the power supply and ground pins.

For the power supply and ground pins connected to the default power supplies, you can omit descriptions on the schematic.
Frequently Asked Questions and Answers
I want to use the default power supply and ground settings.




46. I do not know how to create schematics using power supply boxes.



Prepare symbols for which only power supply and ground pins of parts have been input, and connect the power supply and ground symbols.

Input net names as part names for the power supply and ground symbols.

Follow the rules below to create a power supply box:

Before Next Index