Question
I would like to import Gerber files into an Altium Designer PCB document for re-using an in-PCB spiral inductor but the importer fails to interpret the Gerber files in a correct way. Has anyone here knowledge on how to import Gerber files into an Altium Designer layout?
Background/What I have tried
The design containing this PCB spiral is a reference design from Linear Technologies and there are design files available for download here (clicking link will download a .zip-file). The design files contains a Mentor Pads PCB file but also Gerber files.
The ECAD system I'm using is Altium Designer 15.1. Since the Mentor PADS PCB file is of binary type I can't import it into an Altium Designer layout document. Altium designer can only import ASCII type Mentor PADS PCB files and I don't have access to conversion tools for converting from PADS binary format to PADS ASCII format. Therefore I tried to import the Gerber files into an Altium layout document. The result is not right at all, there is just a mess of top layer copper.
I have opened the Mentor PADS PCB file into the free Mentor PADS viewer and the design looks like it is supposed to. I have also imported the Gerber files into CAMtastic (the built in Gerber viewer in Altium Designer) and the design looks like it is supposed to. I also tried to export new Gerber files from CAMtastic and then import them into an Altium Designer PCB document but I had no luck with that.
Added to original post (1)
The way I've been trying to do the import of Gerber files into an Altium Designer PCB document is that I open a new PCB document and then I import one Gerber file at a time by choosing File->Import->Gerber File. I stop after the first import since I just get a mess of tracks and pads.
Added to original post (2)
Just opening the Gerber file using the Built in Altium CAMtastic viewer is not the complete answer for me. I would like to transfer some design elements from these Gerber files into a design for reuse.
Answer
I have downloaded the design you are dealing with. The gerber files, all layer files have .PHO extension.
Import gerbers into Altium
If you rename the files as follows you will be able to open them in Altium:
- Layer4.pho \$ \longrightarrow \$ Layer4.GBL, this is the bottom layer
- Layer1.pho \$ \longrightarrow \$ Layer1.GTL, this is the top layer
- Layer2.pho \$ \longrightarrow \$ Layer2.GP1, GND plane 1
- Layer3.pho \$ \longrightarrow \$ Layer3.GP2, GND plane 2
- SoldermaskBottom.pho \$ \longrightarrow \$ SoldermaskBottom.GBS
- SoldermaskTop.pho \$ \longrightarrow \$ SoldermaskTop.GTS
I have identified the layers by the PDF appendix. For Pastemask (GBP, GBT) and Silkscreen layers you should search for their Altium extensions.
These modified files can be dragged and dropped into Altium, example for Top layer:
This way all layer files are easily openable in Altium.
Export TopLayer gerber into PCB document file
- Select Layer1.GTL tab in Altium
Select the Menu → Tables → Layers Order option. Following dialog will be shown: Fill the cells as below.
Enable the Export to PCB option as follows: Menu → Tools → Netlist → Extract.
"After a netlist has been extracted from your CAM data, the File » Export » Export to PCB command becomes enabled" source
Now, select Menu → File → Export → Export to PCB and a new PCB document will be opened with the Top Layer.
Result:
No comments:
Post a Comment