POWER PCB轉ALLERGO的方法

dinodino66 · 发表于 2012-8-31 02:00

EDA365欢迎您登录！

您需要登录才可以下载或查看，没有帐号？注册

x

請問有沒有那位高手有碰過POWER PCB轉ALLERGO{:soso_e144:}

最近收到客戶的資料不知如何是好

langexie · 发表于 2012-8-31 08:23

1.从 PADS 导出 asc文件。选取 powerpcb  V5.0格式导出。将 asc文件放在你工作的目录下
2.在allegro菜单 files-》import-》PADS
第一项  PADS  ASCII  FILES 选择导出的 asc文件
  第二项  option 选择  allegro 安装路径下的 X:\Cadence\SPB_16.X\tools\pcb\bin\pads_in.ini 执行run 就 ok

xidgli · 发表于 2012-8-31 08:43

本帖最后由 xidgli 于 2012-8-31 08:52 编辑

langexie 发表于 2012-8-31 08:23
7 H) n: D7 u9 F5 i0 h" h1.从 PADS 导出 asc文件。选取 powerpcb V5.0格式导出。将 asc文件放在你工作的目录下 6 ?# {2 w3 ?# ^* T, {. G, R. T
2.在allegro菜单 ...

你好，刚刚用您的方法试了一下，可是出现提示：unable to open log file.不知道是怎么回事？我的版本是PADS9.2。ALLEGRO版本是16.2.

langexie · 发表于 2012-8-31 10:49

xidgli 发表于 2012-8-31 08:43
; N: e7 x& r& L6 O9 z8 N你好，刚刚用您的方法试了一下，可是出现提示：unable to open log file.不知道是怎么回事？我的版本是 ...

在setup-》user preferences 在paths->library里面更改库的路径为你的工作文件夹,再试试！

xidgli · 发表于 2012-8-31 11:08

langexie 发表于 2012-8-31 10:49 , W& F" W+ C" q2 R7 V
在setup-》user preferences 在paths->library里面更改库的路径为你的工作文件夹,再试试！

还是不行。

mike9016 · 发表于 2012-8-31 11:17

版本太高，用15.5的打开试试

xidgli · 发表于 2012-8-31 11:48

langexie 发表于 2012-8-31 08:23
3 V+ q: b9 h3 l3 w1.从 PADS 导出 asc文件。选取 powerpcb V5.0格式导出。将 asc文件放在你工作的目录下
& G |* x% `" [2 S8 T1 k* B2.在allegro菜单 ...

看来这种方法是行不通的。

langexie · 发表于 2012-8-31 12:28

本帖最后由 langexie 于 2012-8-31 14:41 编辑

xidgli 发表于 2012-8-31 11:48
) z* f# ^0 |3 J% d2 p0 \看来这种方法是行不通的。

以下为Cadence，Help：

pads in
Syntax | Dialog Box | Procedures
The pads in command imports information from PowerPCB and Pads Layout 2005 ASCII database files into Allegro PCB Editor board databases. It is assumed that the PADS databases being translated are completed (placed and routed).
Familiarity with PowerPCB and Pads Layout 2005 is assumed. For additional information, refer to PowerPCB and Pads Layout 2005 documentation or contact the vendor.
The PowerPCB and Pads Layout 2005 translator reads PowerPCB and Pads Layout 2005 database files and writes an Allegro PCB Editor board database. Due to format differences, other types of input files cannot be read. PowerPCB and Pads Layout 2005 can be used to convert an ASCII database file to a version 4 or 6 file. For further information on how to do this, see the PowerPCB and Pads Layout 2005 documentation.
Before running the PowerPCB and Pads Layout 2005 translator, you must create an ASCII version of a PADS job file, which contains all decal, part type, part, signal, route, and graphic data.
During translation, the Pads to Translator dialog box displays information about the translation progress. End the translation by clicking Cancel on this dialog box. All generated files write to your output directory, and you can use these temporary files for reference. You need the board file (.brd) file to edit the design.
When the translation finishes, the status dialog box closes. Use File - Viewlog or File - File Viewer to open the pads_in.log file and review any errors. Also examine netin.log file for any warnings or errors.
Menu Path
File - Import - PADS
Syntax
To translate several databases using DOS batch files, you run the PADS translator in batch mode by specifying all required information on the command line.
Note: Before attempting to run pads_in, export a PADS job file to a PADS ASCII database that can be read by the translator, as explained in Creating a PADS ASCII Database File.
pads_in <input_file> <output_directory> <options_file>

PADS ASCII input file
Specifies the full path and name of the PADS ASCII database file.

Output Directory
Specifies the full path and name of the output directory.

Options File
Specifies the full path and name of an options file. If this does not exist, it is created.

If you run pads_in (note the underscore) at the operating system prompt without specifying arguments, a dialog box appears, prompting you for the data listed above. For details, see Importing a PADS Database in Batch Mode.
PADS IN Dialog Box
Use this dialog box to convert PADS database information.

PADS ASCII input file
Specifies the full path and name of the PADS ASCII database file.

Options File
Specifies the full path and name of an options file. If this does not exist, it is created.

Output Design
Specifies the full path and name of the output directory.

Browse
Searches for the required files on your system.

Run
Continues with the translation

Close
Closes the dialog box.

Procedures
These procedures describe converting a PADs database to a board/substrate file.
Creating a PADS ASCII Database File
The PADS job file must be converted to a PADS ASCII database that the translator can read. This file contains all decal, part type, part, signal, route, and graphic data from the job file. An ASCII database is self-contained and does not require any information from PADS library files.

1.
Run PADS - Perform and load the JOB database file to translate.

2.
Re-pour all copper pour areas (if any).

3.
Click In/Out, then ASCII OUT to display the ASCII OUT form.

4.
Choose the All option to output all data in the database. Choose this option only if you want to translate the complete database.

5.
Choose the Convert miters to lines option to convert any route miters to lines (or arcs). If you do not choose this option, miters are not converted.

6.
Specify the output file name and click OK.

See the PADS-Perform documentation for more information on this subject.
Importing a PADS Database in Interactive Mode

1.
Run pads in at the command prompt.

The PADS IN dialog box displays.

2.
Enter the PADS ASCII file to translate in the PADS ASCII Input File box. Use the Browse button to locate the file if necessary.

3.
Enter the full path and name of an options (.ini) file in the Options File box. The translator saves all options in this file, which can be used for later translations of the same or different ASCII files.

Note: If you enter a file name that does not exist in the Options File box, the Translator Options dialog box displays.

4.
Enter the output file name in the Output Design box. By default, this box contains the path to your current working directory where the output file is stored

5.
Click Run.

The PADS Translator dialog box displays the translation status.

6.
When the translation stops, click Close to dismiss the PADS IN dialog box.

Note: Click Cancel to stop the translation.
Importing a PADS Database in Batch Mode
This section describes the procedure for running pads_in from the operating system prompt when you do not qualify the command with arguments.

1.
Export a PADS job file to a PADS ASCII database that the translator can read, as explained in Creating a PADS ASCII Database File.

2.
At a command line prompt, type:

pads_in
The File Names dialog box appears.

3.
Enter the name (and full path) of the .ascii file being input in the PADS ACSII Input File field. Use the Browse button to locate the file if necessary.

4.
Enter a directory to which to write the output file in the Output Directory field. Use the Browse button to locate the directory if necessary.

5.
Enter the full path to an options file in the Options File field. Use the Browse button to locate the file if necessary.

6.
Click OK to continue.

Pads_in reads the input file and determines the number of etch/conductor layers it uses. If all required program arguments are not specified, the PADS to Allegro Translation Options dialog box appears.
The PADS To Allegro Layer Mapping fields define the element-layer mappings. The list box contains all PADS objects (Lines, Copper, Text, Decals, Pads and Vias) and the name of the class and subclass to which to map the objects. Each element appears once for each PADS layer, for a total of 31 entries per element.
All 2-D lines on PADS layer 0 map (are added) to the BOARD/SUBSTRATE GEOMETRY class and the subclass ALL, which is not pre-defined. Lines on PADS layer 1 map to the ETCH/CONDUCTOR class and the subclass TOP/SURFACE and so on. The translator presets all necessary ETCH/CONDUCTOR class mappings by default, even if a previous translation created the options file. This is also true during batch translations.
Changing an element mapping

1.
Choose the mapping in the list box of the PADS to Allegro Translation Options dialog box.

The element's target class and subclass mappings are chosen in the Class and Sub Class fields.

2.
To change the target class, click the arrow to the right of the Class field, and choose one of the allowed class names.

3.
To change the target subclass, click the arrow to the right of the Class field, and choose one of the allowed class names

-or-
Type a new subclass name in the Sub Class field.
Note: You cannot define new subclass names if the class is PIN or VIA.

4.
Choose Create solder layers to create solder mask and solder paste padstack layer entries.

5.
Specify the oversize radius in mils.

All non-zero sized pad entries are copied, and the oversize radius added to the pad entry size. For example, if the oversize is 15, a 60-mil pad generates a 75-mil solder mask and paste layer entry. The solder mask pad layer entry is added to the SOLDERMASK_TOP subclass, and the solder paste entry is added to the PASTEMASK_TOP subclass.

6.
Choose Create Dynamic Shapes if you want the translator to create dynamic shapes from POUROUT and HATOUT pieces from the *POUR* section. For more information on dynamic shapes, see Preparing for Layout in the user guide.

7.
Click OK to translate or Cancel to stop translating.

Editing the Database After Importing PADS Data
After the PADS or PCAD translation finishes, load the board/substrate file into the editor. To create a design that can be maintained completely within the editor, follow these steps:

1.
Run viewlog to display the translators' log file. Examine the file for any errors or warnings. Also examine netin.log file for any warnings or errors.

Note: The log files are pads_in.log and pcad_in.log.

2.
Choose Display - Color/Visibility (color192 command) and choose All Invisible from the Global Visibility box of the Color /Visibility dialog box.

3.
Click Yes in the confirmation box, and click Apply on the Color/Visibility dialog box.

All the classes and subclasses in the design become invisible.

4.
Enable visibility for the following classes/subclasses:



Drawing Format/Outline in the Manufacturing group



Pin, Via, DRC, and Etch/Conductor in the Stack-Up group

5.
Set colors for the following classes/subclasses.



Drawing Format/Outline in the Manufacturing group



Pin, Via, DRC, and Etch/Conductor in the Stack-Up group



Ratsnest in the Display group

Cadence recommends for ease of viewing that you set DRC and ratsnests in red.

6.
Click Apply.

The reset classes/subclasses in the design become visible.

7.
Click OK.

8.
Choose Setup - Design Parameters (prmed command) to display the Design Parameter Editor.

9.
Choose the Display tab and set DRC Marker Size to 125 (or a parameter of your own choosing) and clear the Grid check box.

The grid display in the interface disappears.

10.
Choose the Design tab and set Default Symbol Height to 125 (or a parameter of your own choosing).

11.
Click OK to implement the changes and close the dialog box.

12.
Verify the keepin/keepout areas. (The translator creates placement keepouts for all package/part symbols based on the boundaries of objects found within the PADS decal.)

13.
Set the appropriate constraints for your design. Depending on the version of the tool you are using and the type of constraints you are setting, choose Setup - Constraints Constraint Manager (cmgr command.

14.
Choose Tools - Database Check (dbdoctor command) to verify the integrity of a design drawing database.

The DBdoctor (Database Health Monitor) dialog box appears.

15.
Set the parameters and click Check to verify the database.

16.
View the log file, and make the necessary corrections.

The translator also adds an anti-pad and thermal-relief layer entries to padstacks. Thermal reliefs are a flash with the same name as the pad. You may modify these settings. The translator determines the size of anti-pads using the COPPOURSPACE parameter in the *PCB* section of the ASCII file. Any oval or rectangular finger pad entries convert to shapes in the design database because PADS allows ovals and fingers to be rotated within a padstack.
If your PADS database contained negative power planes with power ties, generate these ties as thermal-reliefs during film creation.

xidgli · 发表于 2012-8-31 12:45

langexie 发表于 2012-8-31 12:28
' f9 N# w6 P3 W/ p5 A9 Z* ^3 Q自己好好看看Cadence，Help：8 Y. j8 q0 j/ ] x" o

9 X8 t2 P p* Tpads in

多谢指点，但是也太多了吧，而且本人英语水平也不咋地。

JIMDENG · 发表于 2012-8-31 13:15

本帖最后由 JIMDENG 于 2012-8-31 17:56 编辑

学习一下

JIMDENG · 发表于 2012-8-31 13:16

本帖最后由 JIMDENG 于 2012-8-31 17:55 编辑

看明白了，这个英文说明。

JIMDENG · 发表于 2012-8-31 13:19

本帖最后由 JIMDENG 于 2012-8-31 17:55 编辑

谢谢！

xidgli · 发表于 2012-8-31 13:52

xidgli 发表于 2012-8-31 12:45
2 w3 G3 \( T/ d# s# \, a# @多谢指点，但是也太多了吧，而且本人英语水平也不咋地。

哪位高人指点下Allegro16.2到底怎么转呢?

JIMDENG · 发表于 2012-8-31 14:12

本帖最后由 JIMDENG 于 2012-8-31 17:57 编辑

l转好后一定要认真检查！

nbhand · 发表于 2012-8-31 14:56

langexie 兄弟已经在2L,4L给出了正解。

帐号		自动登录	找回密码
密码			注册

POWER PCB轉ALLERGO的方法

EDA365欢迎您登录！

浏览过的版块

推荐内容 /1