summaryrefslogtreecommitdiff
path: root/cvt
diff options
context:
space:
mode:
authorWerner Almesberger <werner@almesberger.net>2016-07-21 11:31:17 -0300
committerGenerated from internal repo <nobody@neo900.org>2016-07-21 11:31:17 -0300
commit61b12104cc559272197f7ce7430b18be401f427a (patch)
tree548d5cb3b5bd105b0762056cdf55efe0d3585bbe /cvt
parent2abb25c3a5ca5bfce2b65cb899fb3b8dfa62efec (diff)
downloadee-61b12104cc559272197f7ce7430b18be401f427a.tar.gz
ee-61b12104cc559272197f7ce7430b18be401f427a.tar.bz2
ee-61b12104cc559272197f7ce7430b18be401f427a.zip
cvt/README: describe common post-conversion issues (some specific to Neo900)
Diffstat (limited to 'cvt')
-rw-r--r--cvt/README130
1 files changed, 129 insertions, 1 deletions
diff --git a/cvt/README b/cvt/README
index 62f551d..dd6fec0 100644
--- a/cvt/README
+++ b/cvt/README
@@ -1,4 +1,5 @@
-Conversion session transcript:
+Conversion session transcript
+=============================
git clone https://github.com/lachlanA/eagle-to-kicad.git
mkdir <base-directory>
@@ -73,3 +74,130 @@ Use the PACKAGE command to select a package variant first
[33:56] Log file dialog
- accept
+
+
+Common issues in converted schematics
+=====================================
+
+Component text size
+-------------------
+
+Component text (component reference, value, etc.), should have a size
+of 50 mil. The converted schematics frequently use 45 mil or 70 mil.
+
+KiCad stores the default size, location, and alignment of text fields
+in the definition of the schematics symbol ("component", .lib). This
+is copied into the schematics when placing a symbol, and can then be
+modified individually for each use of the symbol.
+
+To change a symbol in the library, right-click on the symbol in the
+schematics, Edit component > Edit with Library Editor
+Make the changes in the component editor. Important: make sure that
+all pins are aligned with a 50 mil grid. To abort changes, simply
+quit the component editor. To save changes, click
+Update current component in current library
+followed by
+Save current library to disk
+
+Eeschema will pick up changes in geometry and fixed text automatically,
+but it will not change fields of existing symbols. To update fields to
+the definitions in the library, press E to edit the component, then
+click Reset to Library Defaults.
+
+
+Component text alignment
+------------------------
+
+Many text fields in the converted schematics are vertically aligned
+with the bottom of the text. It is often more convenient to align with
+the center, such that a field can be placed near a wire (or anything
+else that follows the 50 mil grid) without getting too close.
+
+
+Pin types
+---------
+
+Some pin types in the converted schematics are incorrect or at least
+unusual. In general, passive components like LED should have their
+terminals marked as "passive", not as "power input" or such.
+
+Pin types can only be corrected by changing the component in the
+library.
+
+
+Label text size
+---------------
+
+Many labels have (or had) a text size of 65 mil. This makes global
+labels overlap when stacked with 100 mil spacing. The text size can
+be changed by pressing "E" on the label.
+
+
+Label type and direction
+------------------------
+
+Labels that should be global were converted to local. To change them
+back to global, right-click, Change type > Change to Global Label
+
+In KiCad, global and hierarchical labels (but not local labels)
+indicate a direction. This can be changed by pressing "E" on the global
+label.
+
+
+Tiny labels
+-----------
+
+The converter flags each net with a tiny label (10 mil), to ensure the
+net is really what Eagle said it was. Most of these labels have already
+been removed, but some remain.
+
+In general, all such labels should be deleted. Since they can sometimes
+indicate conflicts in the design (cf. VBUS), one should check, before
+deleting, that they are consistent with the net that is expected to be
+at this location.
+
+
+Power flag
+----------
+
+KiCad requires all nets that are used as power input to be driven by a
+power output (i.e., a pin marked as such). If a net has no implicit
+power source (e.g., if it is separated from a power output by a choke),
+the POWERED symbol (which is a single-pin power output) has to be placed
+on the net. (POWERED is a nicer form of PWR_FLAG from the default KiCad
+library.)
+
+
+Unusual wiring
+--------------
+
+The "normal" drawing style in KiCad is that pins are connected by a
+single wire that continues for at least 50 mil, better 100 mil, in the
+direction of the pin. This wire can then bend, form T-joints with other
+wires, etc.
+
+The converted schematics contain a large number of wires that are
+perpendicular to the pin they connect to, and some pins are even
+connected directly, without wire. While this "works", it often looks
+confusing and it complicates moving or dragging items. The best way to
+resolve such issues is often to just delete the wires and junctions of
+the net in question, move components to create a bit more room, then
+redraw the net.
+
+Caution: deleting a wire often deletes the entire wire, across
+junctions. Checking the result of major reconstruction against a PDF
+taken from the original state (or the Eagle original) is recommended.
+
+
+Unifying multi-unit components
+------------------------------
+
+Some components are drawn as consisting of a very large number of
+units. E.g., the rather simple digital microphones had no less than
+five units each.
+
+A quick way to reduce the number of units is to invoke the component
+editor on the component, setting the pins in units B and above to
+"Common to all units in component", reducing the number of units in
+"Edit component properties" to one, and finally arranging the pins in
+a suitable pattern.