μblog: engineering from the trenches

To make prototyping of small PCBs more cost effective, it is helpful to merge several designs into one and then to panelize it so that there are multiple copies on the same board. After creating the two separate boards in Cadence Layout and then running the post processing, to create Gerber files and NC drill files, we open the created GDT file in GerbTool (Layout->Tools->GerbTool->Open). For each of the designs, we first allow GerbTool to update the design file version to the most current one and then we delete all of the unused layer files from the database. Next, we import the NC drill file by doing File->Import->NC (Drill/Mill). After picking throughole.tap, it is necessary to select the proper scaling. To learn more about this, go to Help->Help Topics and search for “decimal”, then select File|Import|NC (Drill/Mill). The problem is that NC files don’t contain decimal points so the software has to guess. To test this, when importing the NC Drill file, play with the m.n setting and click apply. When the board size above the preview is about the size of your board, click OK and verify that the drill holes overlap the proper locations in the other layers. Finally, save the design and do the same for all other designs to be imported. When you are ready to merge, simply open one design then merge the other designs into it using File->Merge. You can use the panelize tool to create multiple copies depending on your configuration. Be sure that all of the necessary layers are visible prior to panelizing as only the visible layers will be acted upon. Next, create the board outline in the silkscreen layer by right clicking it in the navigator and selecting it as active and then simply draw the rectangle around all of the artwork. Save the design here and export the NC Drill file as well as the Gerber files. These files will now be ready to be sent off to the PCB manufacturing house.

del.icio.us | digg