Electronics > Circuit Studio

Altium Newbie (CS) coming from EAGLE PCB

<< < (10/10)

Hi all,

Elecrow compatible 2-layer, SMD/TH gerber files.
Took me two attempts at sending a ZIP to Elecrow till they confirmed the gerbers were fine. They sent back screenshots to me to confirm.
The only issue I had with the original default gerber settings was that I was getting lots of extra lines etc on every layer. The right hand pane on the layers tab was to blame. See below.


On the OUTLINE layer draw a line around the edge of your board to match Altium's board limits. Not sure if Elecrow actually need this, but I happened to have it on because OSHPARK needed it.
The settings below probably more than cover a 2-layer board etc, but this is just what I had mostly from defaults.


General tab:
- Units = Inches
- Format = 2:4

Layers Tab:
- Select GTO, GTP, GTS, GTL, GBL, GBS, GBP, GBO only
- In right hand pane de-select all 5.
- Bottom pane select Include unconnected mid-layer pads

Drill Drawing Tab:
- Drill Drawing Plots - select Bottom Layer-Top Layer
- Drill Guide Plots - select Bottom Layer-Top Layer

Apertures Tab:
- Select Embedded apertures (RS274X)

Advanced Tab:
- Film size X=20000mil, Y=16000mil, B=1000mil
- Aperture Matching Tolerances Plus=0.004mil, Minus=0.004mil
- Batch Mode = select Separate file per layer
- Leading/Trailing zero = Keep
- Position on Film = Ref to absolute
- Plotter type = Unsorted
- Other - select Optimize change & Generate DRC rules

NC Drill Setup:

- Units = Inches
- Format = 2:4
- Leading/Trailing zero = Keep
- Position on Film = Ref to absolute

Any checkboxes not detailed above leave un-checked.

Hit the GERBER button then once it's finished, hit the NC DRILL FILES button. Under your project in a folder starting "Project Outputs for........" will be a host of files. ZIP up the files starting with "PCB1" only and thats it.



[0] Message Index

[*] Previous page

There was an error while thanking
Go to full version