如何将orcad产生的netlist导入到Expedition

请教如何将orcad产生的netlist导入到Expedition,使之能forward annotation而且不产生error.

如有兄台可提供资料可发送:alertcrazy@163.com

Thanks

同问！

为什么不懂的GOOGLE，我很纳闷！

因为google没解决我的问题,

如你知道的话请告知

Using the OrCAD to Expedition PCB Interface

The following diagram shows the workflow of the interface between OrCAD Capture and Expedition PCB. There are two kinds of flows: the first time flow (see red arrows) and after the first time flow (shown in pink color) through the interface. The common flow between these two flows is shown brown color.
After the first time flow through the interface, the directory structure has been created, along with the .prj and .pcb files.

Create a MentorKYN  netlist in OrCAD

1. Open OrCAD.

2. Open and edit the schematic.

3. Run Design Rule Checking.

This is a recommended but not a mandatory step. To run DRC in OrCAD, first click on the .dsn design file in the  Project Manager window, to enable the Tools menu on the menu bar. Select Tools->Design Rule Check.   In the Design Rules Checking dialog, select the required checkboxes under the Design Rules Check Tab > Report Section.
Recommendation: If any errors are found in this check, it is recommended to resolve them before generating a KYN netlist.

4. Create a Mentor KYN netlist.

Requirement: The pre-condition for this step is packaging.
Click on the .dsn design file in the Project Manager window to enable the Tools menu on the menu bar. Click on the Tools menu and then click on the Create Netlist option. Click the Other tab and choose mentorKYN.exe from the Formatters list. Click the OK
 button.
Caution: If an Expedition PCB session is active, new netlist creation is not recommended for it may leave the front and back end design databases in an inconsistent state.

5. Close OrCAD.

Interface session

1. Open Programs > Mentor Graphics SDD > WG200n > Orcad-Expedition Interface > Orcad-Expedition Interface.

2. Browse for and select the <project name>.opj created by OrCAD

3. (First time only) Select a template.

After selecting the .opj file, the interface will ask for a template to be selected. Browse for a template directory and select OK.
Once the template is selected, the interface creates a .prj file and this completes the current step.
Tip: Several standard templates are provided with the interface.
Warning: The chosen template must be the same one that is selected in the Job Management Wizard.
The <project name>.prj file is created by the interface when called the first time on the OrCAD design. It is the shared control file and once created, it will be used in the subsequent interface sessions.

Note: A set of indicators guide the forward and back annotation flows.

4. (Optional) Edit the net classes and net properties in the interface. If  you do not require edits in the interface, this step may be skipped (the direct pink color arrow in the workflow diagram indicates this after the first-time-flow).

Click on the appropriate buttons in the interface to activate the net class or net properties dialogs. The net names used in the OrCAD design are gathered from the netlist.
When these dialogs are active in the interface, new netlist creation from OrCAD can leave the net databases in the interface in an inconsistent state. Hence a new netlist should not be generated when these dialogs are being edited.
Simultaneous/parallel edits to net class and net properties in the interface and Expedition can leave the net databases in an inconsistent state on either side.

Job Wizard

1. (First time only) Invoke Job Wizard and create a .pcb file. This session creates a <project name>.pcb file. Once it is created, it will be used in the subsequent sessions.

1. Once Job Wizard

2. Select Create, then Next.

3. Browse for the project file that was created in OrCAD, then Next.

4. Select a Central Library when presented with the Project Editor dialog, then Next.

5. Select a PCB Template (this template should be the same as the template selected in the interface), then Next.

6. Select Finish.

7. Select Close. This step creates the <project name>.pcb file.

Expedition PCB

1. Open Expedition PCB.

2. Open the <project_name>.pcb file.

Warning: When an Expedition session is active, new netlist creation is not recommended for it may leave the front-end and back-end design databases in an inconsistent state.

3. Run Forward Annotation

4. (Optional) Edit the Net Class and Net Properties dialogs within Expedition PCB.

If required, edit the net classes and clearances and net properties dialogs in the Expedition session. This step assumes that the net databases are synchronized between the interface and Expedition sessions.
After save and close of the Expedition session, the net class and net properties databases are synchronized with their counter parts in the interface.
Warning: Simultaneous/parallel edits to net class and net properties in the interface and Expedition can leave the net databases in an inconsistent state on either side.

Handling Illegal Characters in Names used in the Schematic Design

Back Annotation in Expedition PCB

If any of the following transactions are performed in an Expedition PCB session, back annotation is required by selecting either ECO > Back Annotation or running Back Annotation from the Setup > Project Integration menu:
ECO > Renumber Ref. Des.
Setup > Net Properties
Setup > Net Classes
Setup > Editor Control (Rooms & Clusters Tab)
Route > Planes->Routed Plane Pins

1. Create a swap file in the OrCAD Interface

The KYN format needs to be converted to the format that OrCAD accepts (.swp files). To do this, select the Create Swap file button on the OrCAD-Expedition  Interface dialog.
Result: If any errors are encountered in the .swp file creation, a text editor displays with the erroneous .swp file.
A set of indicator guides the forward and back annotation flows. The association between an OrCAD schematic and an Expedition PCB design enables you to see which functions of integration are available by reading the settings in the dialog. By default, the indicators are green.

Forward Annotation allowed  Is red when the reference designators have been renumbered within Expedition PCB .  It remains red until Back Annotation (BA) is run in Expedition PCB.
Schematic and Layout databases synchronized  Is red when either the reference designators have been renumbered within Expedition or changes are made to either net class or net properties databases within the Orcad Interface or Expedition PCB.
Back Annotation allowed  Is red when the Project Integration option "Disable commands that create Back Annotation changes." in Expedition PCB is toggled on.
Back Annotate in OrCAD Capture

1. In order to incorporate the .swp file select the Tools-> Back Annotate option in OrCAD Capture and choose the Layout tab.

2. Browse for the created .swp file in the back annotate dialog and click OK. Observe that the back annotations are incorporated in the OrCAD design.

Requirement: Anytime you do a back annotation into Orcad you need to generate a new netlist and forward annotate into PCB.

3. Create MentorKYN Netlist in OrCAD Capture

4. Run Forward Annotation in PCB

不错,顶一下！感谢小编！

五楼的说得太复杂了,其实有比这简单得多的方法.

只要在导出netlist的时候在part的footprint选择正确即可.

太小儿科了.

并且五楼的方法需要用到Mentor公司的license,如果您公司用户的话很有可能你的公司不会为此花钱的.

www.ctzpcb.com

做中国最专业的PCB设计