Before Next Index

57. When making a command input, I want to change the default option.


Edit the Environment resource file (lanenv.rsc).
On the File manager, Double-click on the lanenv.res file to open the Environment Resource Editor.
Click on the [Command Default] icon and change the settings for each command as necessary.

Only the user like the "System Administrator", who has a write permission can change the settings for the master resource file, '$ZDSROOT/info/lanenv.rsc'.



58. The connector location for the sheet connector has gotten too long.
I want to make a carriage return.


When executing the Cross Reference, specify the [Max string length], or make a carriage return in the "Change Attribute" Dialog.

Specifying [Max string length] is available in Rev.5.0 or later.

Minimum number of characters will be the number of characters usable in case of a single connection in each output mode.
(In other words, in the mode where output is 002:A1, setting in less than 6 characters is not valid. )



59. I want to extend the end point of the bus beyond the the point where the net is connected.


Select [Place]-[Bus] and indicate [Auto-connect] in Right-click, then add an additional bus line at the end point of the existing bus.
The Bus Label will be set to that of the existing bus automatically.

Depending on the settings of [Enter Net] in the Command Default (defined in "Environment Resource" file), the operation may be different.




60. On the Circuit, I want to prohibit some of the component properties from editing.



In $ZDSROOT/etc/PropSpec, change the description of [LCDB Reference] to "CIRCUNEDIT". This will make it impossible to copy the LCDB settings at inputting component and to change the properties in the Schematic Editor.

This is available in Rev.4.040 or later.

Editing of PropSpec varies with each version.

  • Under Rev.5.020 or earlier:
    Open PropSpec with a text editor and proceed with editing.

  • Under Rev.6.0 or later:
    Activate PropSpec editor from CR-5000 Design File Manager and proceed with editing on the editor.



61. I do not know how to use the short symbol.


The short symbol is used to put a Net Label as a component somewhere on the net.
To insert a short symbol, set Component type to [Short] and set ON the property [Accept Net?] of the pin connected to the net which is output to the netlist.

If you have not set the [Accept Net?] to ON, the system might change the name of the Net.
In that case, when the Netlist is outputted, the net could possibly not be connected correctly with the designer's sheet. Make sure to set the property [Accept Net] to ON. If it not set, a warnning will appear when saving.

62. Cannot find parts by using a wildcard "*".


As a search condition, you can use a wildcard "*" as follows.

1. For properties of text type:

  • ABC* .... Matches any word that starts with ABC.
  • *XYZ .... Matches any word that ends with XYZ.
  • ABC*XYZ .... Matches any word that starts with ABC and ends with XYZ.
  • *LMN* .... Matches any word that includes LMN.
  • * .... Unlimited

(Use care that if there are 3 or more *, or if there are 2 of * which does not exist at the "beginning and end" of the target character string, search will not correctly be done.)


2. For properties of float/int type:
"*" cannot be used. Instead, you can do range search.

  • <1000 or 1000> .... 1000 or more
  • >1000 or 1000< .... 1000 or less
  • 1000<2000 .... More than 1000 and less than 2000
  • < or > .... Unlimited

Or you can proceed with search along with unit conversion mentioned below:
T (tera) / G (giga) / M or meg (mega) / k or K (kilo) / m or mil (milli) / u (micro) / n (nano) / p (pico) / f (femto)

For example, "1000<1000000" can be expressed as "1k<1M".



3. You can proceed with And/Or search within the same property.

In the descending order of priority: ! -> && -> ||.

(Example)

  • !1k ......Target other than 1k
  • A||B ......A or B
  • !A&&!B&&!C ......Other than A, B, and C
  • 100<1k&&!300<400 ......Any thing from 100 to 1k, excluding those from 300 to 400.
  • AB*Z&&*PQ*||Z*A ......A target that starts with AB and ends with Z including PQ, or target starts with Z and ends with A.

  1. Is it possible to use special symbols on schematic sheets?


Since 2-byte characters are not allowed in properties reserved for the system, fonts allocated to special characters are used to display such symbols.

  1. Use the "Change Attribute" dialog to set a font in the property viewer that allows the use of special symbols. (This is not required when the default font supports the use of special characters.)




  2. Enter the character to which the desired special symbol is assigned in the property value.




  3. The special symbol "" is displayed as "'" on the schematic sheet.

To allow the use of a font, the corresponding font file must be registered in the character size table of the data resource file (landata.rsc).
When not registered, add or edit a font. Font files are provided in $ZLOCALROOT/zsys/font/eng/.

Font files that support special symbols
_zafont0.vec
zafont0.vec
zpafont0.vec
ISO-3098-2.vec




64. Will the display speed slow down when hatching is used frequently?


The display speed is not supposed to slow down when there is an increase amounts of hatching.
However, frequent use of hatching increases the amount of redraws, thus the display speed slows down.



65. What happens when you attempt to reference the fourth or later data by referencing a data resource having only up to third data.


Nothing is displayed on the Editor.



66. Is it possible for a figure to be chipped by restrictions on a displayed object (narrow pitch, many nodes, etc.).


There is no specific problem if a figure has about 200 nodes.
If the pitch is too narrow, it may look like paint.



67. Search Parts Num. in a Parts Rule Based Search becomes 0.


Although Search Parts Num. are supposed to be indicated according to specifications, parts that are registered in LCDB are imported using the CDB name as the key when components are placed. Since CDB names identify parts, there are no identical CDB names in LCDB. Thus the Search Parts Num. is limited to 1 when components are placed.

When placed parts are selected to display them in a "Parts Rule Based Search" dialog, entered properties and symbol file names are used as keys in searching LCDB.

The following are probable causes of the Search Parts Num. becoming 0.
*You may be searching for the wrong condition, so try changing the condition of Parts Rule Based Search.
*The part or the property that is the keyword of the rule search condition may not be registered in LCDB. Check.
*The LCDB path cannot be referenced either because it is not set using the Components Library Path of landata.rsc (Data Resource File) or is incorrectly set. Check.

However, even if the Search Parts Num. is 0 and the check in "Check consistency between parts and symbol" under the "Options" button in the "Parts Rule Based Search" dialog is deselected, the part property information can still be selected even if the symbol file name differs as long as the part property matches the part property registered in LCDB.
Note that the pin information is not updated. The setting "Reload Even If Symbol Unmatched" handles only component properties.


"Frequently Asked Questions"
Although I placed parts on the schematic or selected parts using a Parts Rule Based Search, no properties are loaded from the LCDB (parts info library for schematic design) into the schematic at all.

68. The following message appears when a schematic sheet is opened. "Please see (log/upsmb001.log) for checking updated symbols ".


Schematic sheets store the update record of the referenced symbol files internally.
When a schematic sheet is opened, it checks the update record of the symbol file. If this information differs from information in the schematic sheet, a "upsmbXXX.log" file is generated and a message is displayed.


This message is not displayed if "Reload Symbol Figure" is performed.
It is recommended to check what symbol figures deviate from the update clock kept by the schematic sheet before reloading.

Do as shown below to check updated symbols.
1. Click [Utility] a [Open/Save Log Check] in the schematic sheet editor.


2. The content of the log file output when the sheet is opened can now be viewed in the dialog. You can locate its place in the schematic sheet by clicking the updated symbol figure in the list.


3. Click [swapSymbol] in step 2 to perform "Reload Symbol Figure" for the selected symbol figure.
Clicking [swapSymbol All] allows you to perform "Reload Symbol Figure" for all updated symbol figures. @@

The log files are named as follows.
001.sht...upsmb001.log
002.sht...upsmb002.log
:
The files are generated not for each symbol but when a schematic sheet is opened.
(Even if symbols 002.sht are edited when only 001.sht is opened, "upsmb002.log" is not generated.)

Unless "Reload Symbol Figure" is performed, the message appears when a schematic sheet is opened even if the log file is deleted and the schematic is saved.

The latest update time of the symbol file is checked when a schematic is opened. It is possible to turn off the symbol update check by setting "Updated Symbol Check" to "OFF" in the command default setting of lanenv.rsc (environment resource file). The message will not appear since a log file is not generated.