Product Infomation, Here.
Manual Download
Before using
Account/License
Quadcept
Schematic Capture
PCB Layout CAD
Quadcept DesignConverter
Quadcept ProjectFinder
Quadcept Maintenance
Quadcept Sign
NET CHANGER
forum
Converting Projects from v9 to v10
FAQ

PCB Layout CAD : Reading Net Information

Transferring to PCBs (Net Reading) and Importing Netlists

In Quadcept, when designing a schematic, Component Information and Connection Information (Netlists) can be transferred automatically from the schematic to a PCB. When designing a schematic using another company's CAD, Component Information and Connection Information (Netlists) can be read by importing the Netlist.

Reading Nets
Schematic Design Method

When a schematic is created using Quadcept

Component Information and Connection Information (Netlists) can be read automatically by using Transfer to PCB. It is necessary to assign footprints to schematics before transferring.

When a schematic is created using other CAD
(Import Netlist)

Component Information and Connection Information (Netlists) can be read by executing Import Netlist for the PCB design drawing.

 

When a schematic is created using Quadcept
Component Information and Connection Information (Netlists) can be read automatically by using Transfer to PCB.
The following will explain how to use Transfer to PCB.
(1) Open the schematic that you want to transfer.
(2) Select [Project]
>> [Transfer to PCB].

=> The transfer destination PCB sheet screen will be created automatically.
(3) Components (footprints) assigned on the schematic will be placed on the drawing, and are connected using the Rats Net based on Netlist Information.

If an error is detected while transferring, the Netlist cannot be read correctly and an error will be displayed.
The Error Description will be shown at the bottom of the screen. After making corrections, execute "Transfer to PCB" again.

 

When a schematic is created using other CAD
The following explains how to import component / connection information to your design with a netlist file.
(1) Select [File]
>> [Create New]
>> [Project].
(2) Check the [PCB] and then click "Create".
* For Name and Location, set any project name and export destination folder respectively.
(3) Select [Project]
>> [Import Netlist]
and choose a netlist format you want to import.

Here, [Telesis] is selected.
* When online, by selecting Connect to NET CHANGER, it is possible to import formats from various CAD systems.
(4) Select a netlist exported from another CAD, and then click "OK".
(5) Configure each setting and then click "OK".
* For details on the settings, see Import Netlist Screen.
* When unreadable content has been found in a netlist file, an error message will appear. To import the netlist, fix the error and try again.
(6) Components (footprints) will be placed automatically, and the Rats Net will also be connected.

It can be read even after components have been placed and routing has been done.
If there is a difference with the Connection Information between the design drawing and Netlist, Annotation will be performed, and the differences can be confirmed as a list.

Import Netlist Screen

Component Information
Item Description

Place or Change the Components

Executes new placement and replacement of components and footprints.
In the middle of designing, differences between the PCB drawing and Netlist are detected, and Annotation is performed.

Placement Object

Selects either "Component" or "Footprint".
Specify the object name that is the standard recorded in the Netlist.

During Import Netlist, it is determined based on the match between the Object Name specified as the Reference Object and the Name recorded in the Netlist.

All Databases

Places / Replaces components or footprints based on all the libraries stored in databases.

Specify Directory in local-db (Including Subdirectories)

Places / Replaces components or footprints based on the libraries stored in the specified directory (including subdirectories) in a local-db.

Specify Directory in master-db (Including Subdirectories)

Places / Replaces components or footprints based on the libraries stored in the specified directory (including subdirectories) in a master-db.
* This setting is not displayed when the use of master-db is disabled.

Use Library Cache Preferentially

Enables to place / replace components or footprints based on the libraries stored in a library cache in priority to the ones in databases.
* This setting is not available when the use of Library Cache is disabled.

Update Placed Component/Footprint

Enables to perform a graphical update of components / footprints placed on a PCB sheet based on those in a Quadcept database or a library cache(*).
* Objects stored in a library cache are referenced only when the Use Library Cache Preferentially option is enabled.

Import Component Values from Netlist

Enables to import the values listed in a netlist into the component attributes.

Delete the Component which does not exist in Netlist

Enables to delete components / footprints that do not exist in a netlist.
Net Information
Item Description

Delete the Unnecessary Net Objects (Route/Via/Jumper/Test Land)

Enables to delete the objects (Routes/Vias/Jumpers/Test Lands) with the nets that are not listed in a netlist.