EAGLE

Eagle Software Logo

If you create your circuit board layout with the EAGLE program from Cadsoft, please observe the following tips. Basically, it makes sense to use all the prescribed standard-layers of EAGLE.

We are happy to take care of generating the production data (Extended Gerber) for you. You just have to send us your *. brd file along with your order. All further steps are taken care of by our CAM engineers.

We naturally import your ODB++, Gerber-, Target-, Eagle-, IPC-2581- and Sprint layout data free of charge!

Design Rule Check: .dru file

To ensure the correct settings for your DRC, please use the corresponding EAGLE .dru file, which guarantees that we can produce your circuit boards free of errors. We have created a .dru file for each of the most common board setups.

Please download and unzip the file Multi-CB.dru-files directly into your "dru" directory of Eagle. Then you can select the suitable variant within the software.

From version 7.5 of the EAGLE software, our design rule files are already included.

Standard layers

To convert your EAGLE files, we use Eagle standard layers. Please specify any variations or extended layer specifications with your order.

Function EAGLE name EAGLE layer
FunctionTop LayerEAGLE nametopEAGLE layer1
Function EAGLE namepadsEAGLE layer17
Function EAGLE nameviasEAGLE layer18
FunctionBottom LayerEAGLE namebottomEAGLE layer16
Function EAGLE namepadsEAGLE layer17
Function EAGLE nameviasEAGLE layer18
FunctionSolder-stop TopEAGLE nametstopEAGLE layer29
FunctionSolder-stop BottomEAGLE namebstopEAGLE layer30
FunctionMarking PrintEAGLE nametplace (f.e. Platine Diode) EAGLE layer21
Function EAGLE nametnames (z.B. R1)EAGLE layer25
FunctionContour milled, line width 1milEAGLE namedimensionEAGLE layer20
Functionmilling paths with the tool Ø; scoring lines with 1milEAGLE namemillingEAGLE layer46
Functiondrills pth (plated-through)EAGLE namedrillsEAGLE layer44
Functiondrills npth (non-plated-through)EAGLE nameholesEAGLE layer45

The dimension layer 20 is only for display of the (outer and inner) milling contours with a line thickness of 1mil.

The milling contours including the milling diameter are defined in the milling layer 46.

Npth drill holes that are placed in the dimension layer will not be considered!

EAGLE Boardfile < version 4

In the EAGLE versions prior to version 4, the values of solder-stop oversize, solder paste and stop limit have been set directly at the output of Gerber data. These are not included in the boardfile (.brd). Only with version 4 (or higher) and the new DRC, these values are stored in the boardfile.

Boardfiles of EAGLE < version 4 use the default values (as in EAGLE V3.5x 10 mil for solder-stop oversize and stop limit 0).

If you send us boardfiles of an EAGLE version < 4, please clarify the abovementioned export parameters with our technicians (e.g. for covered vias). To avoid errors, we recommend upgrading to a newer EAGLE version.

Rasterize copper areas

For a better quality of the circuit boards, we generally recommend to rasterize the copper areas, except for high frequency circuit boards with sensitive HF interconnects.

Advantages:

  • More consistent copper within the throughplating of the vias.
  • Lower risk of Twist & Bow (see also Copper Balance)
EAGLE PCB Layout - Ratsnest

1) Ratsnest

 To make the filling of the copper areas (polygons) visible, run the command "Rats Nest".

EAGLE PCB Layout - Properties

2) Properties

Click on the dotted frame of the copper area in (I)nfo mode to mark it, then click the area again to open the "Properties window".

EAGLE PCB Layout - Polygon Pour

3) Polygon Pour

In the Properties window, please choose:

  • Polygon Pour: hatch
  • Width: stands for the line-width of the raster (e.g. 8 mil)
  • Spacing: stands for the line spacing of the raster, recommended is 3 x line width (e.g. 24 mil)

Marking print

Before exporting your data, you should always activate the option “vector font”, which is  found under: Options / User interface.

Otherwise your marking print will very probably be incorrectly applied (see EAGLE 5-Manual, page 44).

Marking print on panels

When copying and pasting circuit board layouts for panel creation, it may occur that EAGLE “increments” the labels, because only one unique part name is permitted. For instance, the name “R116” on the original board would become “R156” on the copy.

For a uniform marking print on panels, execute the EAGLE program’s “panelize.ulp”.

EAGLE-Bug

The program Eagle 4.11 contains an error that can lead to non-functional circuit boards. Here is the original notice from Cadsoft:

Due to a recent problem that has occurred to an EAGLE user we would like to inform you about a bug in EAGLE version 4.11, which could lead to non-functional boards.

The problem occurs if a user creates a board with EAGLE version 4.09 (or earlier), in which he uses polygons (for instance for supply signals) and places rectangles in the layer tRestrict, bRestrict or 1 through 16, respectively, in such a way that there are places where a polygon can only "flow" through with exactly its own line width. If the CAM data is then generated with EAGLE version 4.11 it can happen that polygons are not calculated in the same way as seen by the user with his version of EAGLE. This in turn may cause some parts not to be connected, and render the board non-functional.

The bug was present in all EAGLE versions from 4.10r01 to 4.11. It is fixed in the current version 4.11r2 (and all beta versions since 4.11r01). Therefore we strongly advise to use the latest version of EAGLE, which is available for download from our homepage www.cadsoft.de

Checking of Gerberdata

GC Prevue Logo

Your exported Gerber files can be checked and printed with the freeware GC PREVUE by GraphiCode. This allows testing if everything was exported correctly. You can find GC PREVUE on our download pages.

Directly to the download page for GC Prevue (on bottom of the page)

EAGLE Tutorial

The following EAGLE tutorial should just offer a good start to the program for beginners or trainees.