summaryrefslogtreecommitdiff
path: root/cvt/README
blob: 46dbd7ab039f3f2de1e5f931c09c09e6b7b2e496 (plain)
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
132
133
134
135
136
137
138
139
140
141
142
143
144
145
146
147
148
149
150
151
152
153
154
155
156
157
158
159
160
161
162
163
164
165
166
167
168
169
170
171
172
173
174
175
176
177
178
179
180
181
182
183
184
185
186
187
188
189
190
191
192
193
194
195
196
197
198
199
200
201
202
203
204
205
206
207
208
209
210
211
212
213
214
215
216
217
Conversion session transcript
=============================

git clone https://github.com/lachlanA/eagle-to-kicad.git
mkdir <base-directory>
cd <base-directory>
mkdir eagle
cp ../gdc/sep18/* eagle
mkdir cvt

Some of the following interactions are timestamped, to indicate roughly
when to expect interactions. The timestamps are [minutes:seconds] of
total CPU time of the "eagle" process on a Q6600.

Note: it is best not type anything else during the conversion, especially
around the time when new dialogs may pop up. The Eagle pop-ups will appear
unannounced and grab the input focus. Keystrokes will therefore end up in
Eagle dialogs, changing inputs.

- open schematics in Eagle

File > Run ULP (.../eagle-to-kicad/renumber-sheet.ulp)
- set script path to .../eagle-to-kicad/
- set output directory (.../cvt/)

[10:54] "This ULP will change unconnected VIA's to PADS"
- accept defaults

[11:01] "Consult log file for unncontded via's and tracks"
/home/n9/ee/cvt/GTA04b7_conversion_log.txt
- 1469 unconnected tracks
- 6 unconnected vias
- accept

[11:01] /home/n9/ee/cvt/modified_eagle_files/GTA04b7~fix_via_hack.scr, Line 85:
The Light edition of EAGLE can't perform the requested action!
You can't add parts to this sheet.
- accept
- idem, lines 89, 93, 97, 101, 105. accept.

[11:04] Unknown element VP_0
line 11889
- accept
- idem, VP_1, VP_2, VP_3, VP_4, VP_5. accept.

[11:10] Large dialog
- Output: set all sheet sizes to A3
- Sheet size: set to A3
- accept

[32:11] Library dialog
- Accept (note: dialog stays open after clicking "OK")

[33:21] "There were Errors during the export please read the log for more
	 information"
- Accept

[33:44] /home/n9/ee/cvt/GTA04b7.scr, Line 31320:
Package SOT223-6 doesn't have enough pads for
all 10 pins of device TPS73733
- accept

[33:44] /home/n9/ee/cvt/GTA04b7.scr, Line 31321:
Use the PACKAGE command to select a package variant first
- accept
- idem, lines 31322 to 31326. Accept.

[33:46] Output ... dialog.
- accept defaults

[33:55] There are: 217 missing part prefix(s).
	Conversion finished!
- accept

[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.


Oversized arcs
--------------

KiCad arcs can be either clockwise or counter-clockwise, and there is
no explicit indication of the direction. To avoid ambiguities, arcs are
limited to < 180 degrees. The converter seems to be unaware of this
restriction and produces arcs >= 180 degrees. (Even when drawing an arc
of 180 degrees in KiCad, it is saved with a start and end angle of 0.1
and 179.9 degrees, respectively.)

To fix this, oversized each arc needs to be broken into two (or more)
smaller arcs.