Get email delivery of the Cadence blog featured here
Starting with release 16.5, it is possible to export data from Allegro PCB Editor into PDF files. PDF files are more portable and secure in comparison to .brd files and can be used by customers to share a subset of design data with their vendors who do not need direct access to design data. PDF files can easily be posted on websites and opened within browsers. Read on for more details …Basic Information
The PDF output is driven by Artwork Film Records. It also exports net and component data along with properties. If you try to export all the data, the file size becomes larger than the board file.
Here’s what the PDF Publisher form contains:
The PDF generation is based on the Artwork films defined. Each film becomes one sheet of the PDF file. There are many control options available in the PDF generation.
Some of these key options are:
Security There is a separate password for opening the file -- and another for modifying the permissions. The permissions are listed under File > Properties in the Adobe Reader. The permissions can be changed in Adobe Acrobat (if it is not protected with a password).
Board/Symbol OutlinesIf this is option is set, the board and symbol outlines are added to all layers if the PIN CLASS is exported in the film.
Filled Pads, Filled Shapes, Drill holesCan be turned on and off.
Property DataProperty data can be made made visible in Adobe Reader's model property dialog (the lowest part of the model tree). Property data consumes a lot of space. It needs to be added judiciously. You can control which properties are added to the PDF file in the Property Parameters tab.
Test PointYou can generate test point information in the PDF file and it will be available in the PDF output model tree.
Automation The PDF file can be generated directly from a batch command.Here’s a screenshot of the various Layers and Model Tree objects available in the PDF output:
As always – I look forward to your feedback in using this great new capability.
Jerry “GenPart” Grzenia
Hi Barry -
I spoke with one of our Allegro PCB Editor AE experts. He says the following command will accomplish what you require:
pdf_out cds_routed.brd -a -g
-a Header/Footer filter
-g Drawing origin filter
Command line arguments for pdf_out.
Utility to export Allegro data to PDF Format.
pdf_out <design_name> [-slBCrhpPtUnmiveSx] [-o output_name]
[-f <artfilm_name1> -f <artfilm_name2> ...]
[-c <config_file_name>] [-u user_pass] [-w perm_pass]
-o Output file name. Default: <design_name>.pdf
If the global filename affixes are set the resultant output name
-c Configuration file used to control paper size, margins, scale factor,
and export extra properties for Component and Net.
-f Art film name. Default is to export all films.
-u User password to open the PDF file.
-w Permmision password to open and edit PDF file
-s Create separate PDF file for each art film, Default is to generate
one single PDF file for all the exported art films.
The output file name for each film would be:
-l List artwork films in the board.
-p Pad filled
-P Create size optimized PDF file for printing, no design data exported
-C Display component by RefDes without package name
-B Create PDF file in black and white. Default to use the design colors.
-r Export board/symbol outlines, refdes as well if pins exported
-t Trace filter
-h Hole filter
-U No shape fill
-x Vector text and invisible text string for search.
-D Create PDF/A file.
Meta Data Options:
-n Net Data Tree
-m Component Data Tree
-T TestPoint Tree and testPoint outline
-i Pin property
-v Via property
-e Cline property
-S Shape property
<design_name> Name of the design file.
Example 1: Create one PDF File to export all art films, and export board
outline, symbol outline, refdes as well if symbol pins are
pdf_out test.brd -o test -r
Example 2: Create a PDF File with configuration file:
pdf_out test.brd -o test -c pdf_out_config.txt
Note: The format of object property parameter is:
Object_Type/Property_Name, one entry per line.
page_setup/unit=Inch or page_setup/unit=Millimeter
page_setup/scale_factor=fit_page or page_setup/scale_factor=1.50
page_setup/orientation=landscape or page_setup/orientation=portrait
Example 3: Create one PDF File to export two art films – TOP and BOTTOM:
pdf_out test.brd -o test -f TOP -f BOTTOM
Example 4: Create separate PDF Files for each exported art film:
pdf_out test.brd -o test -f TOP -f BOTTOM -s
Example 5: Create PDF File to export the art films "TOP" and "BOTTOM", and
export meta data for component, net, pin, via, cline, shape:
pdf_out test.brd -o test -f TOP -f BOTTOM -m -n -i -v -e -S
How do you turn off the header and origin when running the program from the command line?
Good point. Currently, Allegro PCB Editor exports PDF Films in the same order as they are in the database. There is no option to change the order.
However, there were several enhancement CCR requests for this feature and the good news is that an option has been added for a film sequence order in the PDF export utility. This has just been fixed in internal code and will go through our standard QA testing. The enhancement will be available in a future 16.6 HotFix (no update to the 16.6 release is planned).
The pdf creator is a great help generating documents. One drawback however, is if i create a multi-sheet pdf file, after selecting multiple film control files, the result pdf file doesn't seem to put them in any kind of alpha numertic order based on my film control file names. Is there a way of setting this up in Allegro so the pdf file is generated with L1 first and L16 last?
Hi Win Min,
There should be nothing special in Allegro PCB Editor to insure you see data in the Model Tree view in Adobe Reader. Check that you have some properties listed in the Property Parameters tab of the PDF Publisher form. Then make sure you see the Model Tree icon in Adobe Reader per the image above in the blog post.
When I generate the pdf , I still couldn't generate model tree, component tree or net tree in my pdf file. I choose these options in PDF publisher. Is there any step that I am missing?
You are correct. This option is licensed separately from the Allegro PCB Editor. It uses the Allegro Design Publisher Option license ( which is also used by the Design Entry HDL product ). The Product Number is PA1220.
I have longed for such a feature, since trying to create a .PDF output by using the plot function always means that I have to mess with colors in order to get a readable output (.PDF becomes all black or whatever color has the preference if there is a ground plane). But: It seems that the described feature is not included in Allegro PCB Designer. When loading a .BRD and the trying to do File|Export|PDF I get an error message "No License Found. Please contact your Cadence sales support".