<H1>Eeshow ‐ Schematics renderer and viewer</H1>
Eeshow reads schematics made by
and can be used as
interactive viewer, or as a command-line tool to convert schematics
to PNG, PDF, or FIG.
Eeshow can show the differences between two versions of schematics sheets
and it can retrieve files directly from a
<A href="https://git-scm.com/">git</A> repository.
Eeshow was developed as part of the
<A href="http://neo900.org/">Neo900</A> project.
Eeshow currently only works on Linux.
To build, the development libraries for Gtk+ 3, Cairo 2, and Git 2
have to be installed. It also uses the command-line tools from
transfig and imagemagick.
git clone http://neo900.org/git/eeshow
The Neo900 project uses complex schematics that are edited by several
people. We keep a revision history in git. For such a collaborative
project, it is crucial to coordinate changes and to be able to see
exactly what happened when conflicts occur.
Unfortunately, it is not
always easy to tell from a textual difference what has changed between
two versions of schematics. Worse, even small changes can sometimes
result in Eeschema producing large numbers of differences.
Eeshow aims to provide a convenient means for visually comparing differences
in schematics. Furthermore, by being able to work directly from a git
repository and not requiring files to be changed on disk, it helps
to streamline the workflow.
Eeshow has evolved from the much older
project that provided a collection of scripts that used Eeschema
(with the help of Wolfgang Spraul's
<A href="http://projects.qi-hardware.com/index.php/p/eda-tools/source/tree/master/kicad-patches">command-line patches</A>)
to render schematics to bitmap images and then to compare these,
producing a large HTML table.
However, this system was very slow
and the approach of using a table would not have scaled to a project
as large as Neo900.
Below is a quick tour of the key features of eeshow. We use the Neo900
schematics as an example. You can download them with:
git clone http://neo900.org/git/ee.git
Start eeshow with:
Eshow displays a progress bar while loading. Since it retrieves files
from the project's entire revision history, this can take a moment.
If the wait gets unbearable, consider using the option
to limit the number of revision eeshow uses.
Eeshow will typically complain about not finding files or components.
Such small problems are common in many projects, and eeshow just omits
parts it can't find, and skips revisions it cannot load.
Once done, eeshow displays the top-level page of the schematics. In
our case, this page contains all the sub-sheets.
You can drag to pan, use the scroll wheel or the + or - keys to zoom,
* to fit the sheet to the window,
click a sub-sheet symbol to open the respective sheet, get help with H,
or exit with Q.
Sheets are rendered almost like in Eeschema. The main difference is
that eeshow uses system fonts for text, which can sometimes produce
small size differences.
To return to the sheet next higher in the hierarchy, click on the box
with the sheet name. To show eeshow's sheet index, click on the box
with the name of the top sheet.
The index shows thumbnails for all the sheets. Clicking on a
thumbnail selects the respective sheet. Clicking anywhere else
(or pressing Escape) returns to the sheet.
While Eeschema largely avoids the use of settings that are invisible
to the user, there is one major exception: pin types.
displaying symbols representing pin types can be toggled by pressing E.
Another extension of eeshow is that it can help navigate nets using
global labels. When hovering over a global label, a pop-up showing the
net name and the sheets on which it used appears. Clicking on a sheet
Furthermore, all occurreces of the global label on the
sheet are highlighted. This highlighting remains effective also when
changing sheets. It can be removed by pressing Escape.
We now come to eeshow's main feature. On the left-hand side of the
screen, a box with the latest revision in the git history is shown.
Clicking on it displays the revision history, with all branches.
Clicking on an entry shows the schematics as they were at that revision.
To compare two revisions, click on the double triangle symbol and select
the revision to compare with. Eeshow then displays the difference beteen
The difference is generated by rendering both versions, then comparing
them pixel by pixel for differences. This means that only changes
resulting in a visible difference will be shown.
The two versions being compared can be shown also without differences:
O shows the old version, N the new version, D the differences. Tab
toggles between old and new.
Versions can also be selected by clicking on the respective box in the
upper left corner. Clicking on an already active version opens the
history viewer for changing the version.
When showing differences, sub-sheets containing changes (or that have
sub-sheets with changes) are highlighted. The same highlighting is
also applied on the index page.
Note: eeshow bases this highlighting on comparing objects and their
parameters ("delta mode"), not on rendering them and then comparing
images ("diff mode").
This can sometimes produce diverging results,
e.g., a sheet may be highlighted but have no visible changes.
Delta mode can also be selected for visualization, by pressing Shift-D.
Eeshow can also be used from the command line to render schematics.
The most common use may be to render the schematics as PDF. Example:
eeshow neo900.pro -- pdf -o neo900.pdf
Additional functions are explained in the