Optimizing Design Output Files for Large Batch Production

November 12, 2018 Altium Designer

Screenshot of AD18 3D layout in design output files

 

For as long as PCB designers have used CAD tools to design their circuit boards, they have also had to create output files from those CAD tools to get the design manufactured. This used to be a time-consuming task involving a lot of manual intervention. You would have to create several related documents in addition to the data files, and perhaps even use a different design tool to create manufacturing drawings. Anymore though, the process of creating final output files has become automated within the design tools. A good example of this can be found in Altium Designer which allows you to create the files you need for your manufacturer all within the core design tools.

 

Altium Designer provides you with the capability of creating each of your output files individually. You can also optimize your PCB design output files for large batch production with Altium Designer’s output job files. This gives you the ability to put all of those individual file creation tasks within a single automated batch file. This will end up saving you a lot of time, and it will also ensure that the next time you generate output files after a redesign, they will be the same file set, structure, and format.as your initial output files.

Design Output Files Created Individually

A circuit board design process should involve PCB design tools that you trust. Component placement, schematic capture and PCB layout are only parts of the puzzle to get your design into PCB manufacturing. Altium Designer gives you many different options for manufacturing output files. Gerber, Gerber X2, bill of material, and drawing PDFs are just some of the files and formats that you can create. All of these files can be easily created individually as needed.

 

 Screenshot of AD18 board output file menus in design output files

The menus for creating output files individually in Altium Designer

 

 

In the picture above you can see the fabrication outputs and the assembly outputs in the “File” pulldown menu of a PCB layout. In each of these menus you will find different commands for outputs. In the fabrication outputs you will find commands for generating outputs such as Gerber Files and NC Drill Files, while in the assembly outputs you will find Assembly Drawings and pick and place files generation commands.

 

Each output file command will have its own configuration and setup menus. For example, the Gerber Setup menu has multiple tabs for different configuration settings. The “General” tab allows you to set up the precision of the Gerber files, and the “Aperture” tab will allow you control over the photoplotter aperture settings in your Gerber files. In the picture below the “Layers” tab is open and we have selected to create Gerber files of the top and bottom layers of the board.

 

Screenshot of AD18 Gerber setup menu in circuit board design output files

The layers tab in the Gerber Setup menu

 

Creating and Configuring the Output Job Batch File

Altium Designer gives you the ability to combine all of the individual generation of output files into one batch operation. The output job file, or “OutJob”, is a pre-configured set of output commands in a single file that can be executed as a batch command. Altium Designer has a built in tool for this file called the Outputjob Editor. To enter the editor and create an output job file, go to the File pulldown menu and select “New > Output Job File” as shown below.

 

Screenshot of AD18 create output job file in printed circuit design output files

Creating a new Output Job file in Altium Designer

 

This will create a new output job file in your projects panel and open the Outputjob editor on it. As with any file in Altium Designer you can save it, or save it under a new name allowing you to create copies for other designs.

 

The output job file is broken into three sections in the editor:

  • The Variant Choice
  • The Outputs
  • The Output Containers

You can see the three sections in the picture below, and to start off you will add the data that you want created to the output job file in the “Outputs” section of the editor.

 

Screenshot of AD18 outputjob editor in circuit board design output files

The Outputjob Editor in Altium Designer

 

 

In the picture above you can see that the outputs that can be added are broken up into different categories including “Documentation Outputs”, “Assembly Outputs”, and “Fabrication Outputs” among others. We have clicked on “Add New Documentation Output” in order to add the creation of a 3D PDF of our layout to the output job file. Once a document is added we can configure its generation parameters according to our needs by double clicking on it. In this case the default settings for the 3D PDF are fine the way they are.

 

Next we will add some Gerber files to our output job file by clicking on “Add New Fabrication Output”. In the same way that we selected the 3D PDF out of the menu, we have selected and added “Gerber Files” to our list of fabrication outputs. Now by double clicking on “Gerber Files” we can configure the creation of those files as you can see below.

 

Screenshot of AD18 output job file Gerber setup in board design output files

Setting up Gerber files in the Output Job file

 

The “Gerber Setup” menu that you see in the picture above is the same menu that you saw earlier when generating individual Gerber files. As we did before, we have configured our Gerber setup to only generate the top and bottom layers of our design. You can go on to add many more outputs to your output job file then what we have demonstrated here.

Configuring Containers in the Output Job Batch File

On the right side of the Outputjob Editor are the output containers. These containers will set up the location and formats of the output files that will be created. A new output job file begins with three containers in it; “PDF”, “Folder Structure”, and “Video”. By scrolling the container window all the way up, we have found and double clicked on the “PDF” icon. This will bring up the menu for configuring the output formats for any PDFs that we create in this job output file as shown below.

 

 

Screenshot of AD18 PDF container in circuit board design output files

Setting up the Output Job file PDF container in Altium Designer

 

 

Altium Designer uses a default destination path and naming convention as you can see in the “PDF settings” dialog box above. Usually this will be what you want, but for demonstration purposes we will change those values by clicking on the path elements in the middle of the dialog box. In the picture below we have changed these settings to place the generated output files into a directory on the C: drive with specific names for the folders and files. It is important at this step to click on each element of the path circled in the picture below in order to configure it to target the exact location that you want.

 

Screenshot of AD18 PDF container configuration in schematic design output files

Configuring the PDF container settings

 

 

The final step here is to enable our output and associate it to the container that we want. In our example we clicked on the PDF icon in the container window. Next we clicked on the enable dot next to the 3D PDF output as shown below in the picture below. You can see the green arrow that lights up to show which container the output belongs to. If you have a number of outputs that are going to a single container, you will also have the ability to prioritize their order here.

 

Screenshot of AD18 associating outputs and container in board design output files

Associating the outputs with the container in Altium Designers Output Job file

 

 

To complete our example, we configured the “Folder Structure” container and associated our Gerber files to it in the same way that we did with the PDF container. If our design had variants in it, the next step would be to configure the “Variant Choice” at the top of the editor window. Since our example doesn’t have these we are ready to use our output job file to generate our output files.

Using the Output Job Batch File to Generate Output Files

To generate output files you need to select the container that you want to create outputs from. In our example we have selected the PDF container. You can see in the picture below that when the PDF container is highlighted, some new options are presented. By selecting “Generate content,” all of the output files that have been configured for that container will be generated and located in the directory that was established earlier when you set up the output file destination path.

 

Screenshot of AD18 output generation in circuit board design output files

Generating the output files from the Output Job file

 

 

We generated content from both of the output job file containers in our example design, and it generated the files as you can see below including the 3D PDF of our layout. Altium Designer created the directory structure in the C: drive just as we directed it to, and populated our files into the appropriate sub-directories with the files names that we specified.

 

Screenshot of AD18 output files in board design output files

Output files created by Altium Designer’s Output Job file

 

Managing component, pad, vias, and PCB footprint information in a user-friendly PCB editor is paramount for establishing a strong design flow. Communicating with your PCB manufacturer has never been easier than when you can batch generate your final manufacturing output files as just one of the key features in Altium Designer. You will find that Altium Designer has a long list of powerful and helpful features like that; it is PCB design software that has been created with the needs of users like you in mind.

 

It has everything you need to take your design from schematic capture all the way through layout and the final manufacturing files. If you would like to find out more about how Altium Designer will help you, talk to an expert at Altium today.

 

 

About the Author

Altium Designer

PCB Design Tools for Electronics Design and DFM. Information for EDA Leaders.

Visit Website More Content by Altium Designer
Previous Article
Using Altium's PDN Analyzer and Incorporating Simulation-Driven Workflow
Using Altium's PDN Analyzer and Incorporating Simulation-Driven Workflow

Altium Designer makes it easy to diagnose power delivery and thermal problems in your next PCB.

Next Article
Utilizing Creative Routing Solutions with Tight Component Placement
Utilizing Creative Routing Solutions with Tight Component Placement

Altium Designer makes it easy to place your required interconnects when component placement is tight.

×

Enjoying our blogs? Subscribe to our mailing list to have a weekly Altium blog digest sent to your inbox.

First Name
Last Name
Country
Acknowledging Altium’s Privacy Policy, I consent that Altium processes my Personal Data to send me communications, including for marketing purposes, via email and to contact me by phone.
!
Thank you!
Error - something went wrong!