Diptrace

Last Updated: June 27, 2019
You are here:
Tags:

Creating PCB Assemblies from your Diptrace PCB Project


If you use the EDA Tool Diptrace to design your PCB Assemblies, the best method to upload your design files to MacroFab is to create the following manufacturing package to upload to the MacroFab platform.

  • Component Placement Data from your Diptrace ASCII File
  • PCB Layer Information in Gerber Format
  • Bill of Materials from a .XLSX spreadsheet

Once you have created this manufacturing package you will be able to easily upload your PCB Assembly to the MacroFab platform.

In the PCB tab, simply drag-and-drop your manufacturing package into the file upload target. Alternatively, you can click the Upload Files button on the right side of the screen. More information about uploading files to the platform can be found on the knowledge base article Creating a PCB and Uploading Design Files. The Bill of Materials .XLSX format upload procedure can be found here.

Diptrace ASCII File Generation


For our process to know where your components on your PCB Assembly are placed and the size of the components, we require a ASCII  file from your Diptrace PCB project. The Diptrace ASCII file is used by the MacroFab platform to extract the component names, placement locations, values, and footprints of your Diptrace PCB project.

To generate the ASCII file start by clicking File -> Export -> Diptrace ASCII… and choose the destination of the file. This Diptrace ASCII file will be uploaded along with the Gerber files into the MacroFab platform.

PCB Layer Gerber File Generation


To open the Export Gerber RS274X window click File -> Export -> Gerbers… The left side of the window contains all the layers which are the different gerber files Diptrace will generate.

Some options will be greyed (N/A) out which means they can not be changed for that layer. The layers should have the following options selected.

LayerOptionStatus
Top AssyTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextChecked
TablesChecked
PicturesChecked
DimensionsUnchecked
Top SilkTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextChecked
TablesChecked
PicturesChecked
DimensionsUnchecked
 Top MaskTracesN/A
PadsChecked
ViasUnchecked
Pad/Via HolesN/A
Mt HolesChecked
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
Top PasteTracesN/A
PadsChecked
ViasUnchecked
Pad/V ia HolesUnchecked
Mt HolesN/A
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
TopTracesChecked
PadsChecked
ViasChecked
Pad/Via HolesUnchecked
Mt HolesN/A
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
 BottomTracesChecked
PadsChecked
ViasChecked
Pad/Via HolesUnchecked
Mt HolesN/A
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
Bottom PasteTracesN/A
PadsChecked
ViasUnchecked
Pad/Via HolesUnchecked
Mt HolesN/A
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
Bottom MaskTracesN/A
PadsChecked
ViasUnchecked
Pad/Via HolesN/A
Mt HolesChecked
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
Bottom SilkTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextChecked
TablesChecked
PicturesChecked
DimensionsUnchecked
Bottom AssyTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextChecked
TablesChecked
PicturesChecked
DimensionsUnchecked
Board OutlineTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextUnchecked
TablesN/A
PicturesUnchecked
DimensionsUnchecked
BoardTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextChecked
TablesN/A
PicturesChecked
DimensionsUnchecked
Top DimensionTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextN/A
TablesN/A
PicturesN/A
DimensionsChecked
Bottom DimensionTracesN/A
PadsN/A
ViasN/A
Pad/Via HolesN/A
Mt HolesN/A
TextN/A
TablesN/A
PicturesN/A
DimensionsChecked

Dimensions should be in inches. Enable G54 and Mirror should be unchecked for each layer. The Offset should be set to X: 0” Y: 0”.

Next the file names need to be set. Click Files on the upper right of the Export Gerber RS-274X window.

Change the names of the files to the settings above then press OK. Click on Apertures which is in the upper right corner of the Export Gerber RS-274X window. Click the Auto button in the lower left corner then close the window. Click Export All. Diptrace will then ask where to save all the gerber files.

Now go back to Files and click Export N/C Drill. In the Export N/C Drill window click Auto which will set the tooling. Check the box labelled Use Design Origin then click Export All and save the file.

Gerber File Extension Names

Double-check the extension names that Diptrace generated for the gerber files. They should match the file extensions listed in the Required Design Files article. If the gerber file extensions do not match what the platform expects, the gerbers will not be processed automatically and you will need to organize the layers in the platform using the Design Viewer.

Bill of Materials Generation


For the Bill of Materials Auto Fill to work on the MacroFab Platform, Manufacture Part Numbers (MPNs) must be supplied for the components. Diptrace does not have a standardized way to supply MPNs so a .XLSX spreadsheet will have to be made to do so. The spreadsheet only needs to contain designators and the corresponding MPN. For more information on making a .XLSX formatted spreadsheet and uploading it see the knowledge base article, Importing a Bill of Materials Spreadsheet.

Generating this Bill of Materials .XLSX file is optional for Diptrace PCBs. You will be able to fill out the Bill of Materials without MPNs by searching the market place for parts. The platform will use the footprint and value provided by the Diptrace ASCII file to suggest parts for you to select. See the Bill of Materials Management article for more information.

Cut Outs, Routs, and Slots


The MacroFab Platform currently only works with internal cut outs, routs, and slots that are defined as gerber features. To make this work in Diptrace, cut outs, routs, and slots will need to be defined on the  board outline layer. This causes the cut outs, routs, and slots to be combined with the border layer gerber file. The MacroFab platform currently does not support drill slots. For more information about cut outs, slots, routes, and board outlines check out this engineering article.

Additional Diptrace Questions?


If you have any other questions about creating a PCB Assembly with a Diptrace PCB Project please contact our support team.