+Type: schematics, symbols. + +
+EasyEDA is an EDA tool for the schematics-pcb-simulation workflow. It is +proprietary but offers essentially unlimited free access both as an online +web service and an offline desktop software. As of 2024 neither the service +nor the software do too much to lock users in: +
+EasyEDA alien format support may be of interest to Ringdove users because +EasyEDA is connected to: +
+EasyEDA offers two variants, called std and pro. The two +variants are essentially two distinct software projects with +differing file formats and menus. It seems like symbols are always in +the pro file format, even when loaded by the std variant. Symbols present +in the part file downloaded from lcsc contains files, including the symbol, +in the pro format. +
+The file saved from the std variant is really a project file that may +contain multiple sheets (pages). A schematic sheet in the std format +contains all symbols as embedded (in the std format), but there seems +to be no way to export or save symbols separately in the std format. + +
+At the moment sch-rnd provides support for: +
+Before trying any of these, make sure you use the right variant (std or pro), +the user interface and file formats really differ a lot. +
+
+There are some details that are not imported; the data model and the logics +of the software differ, so there are some manual editing steps needed after +loading alien format data. Below is a list of known cases for EasyEDA. + +
+In EasyEDA each drawing object has its own stroke and fill color and +text objects have font size and font properties. In sch-rnd +objects have a pen that determines all these. Sch-rnd will throw away +color information and will use standard pens on import. + +
+An EasyEDA std schematics file is always a multi-page file even if it contains +only a single sheet. Sch-rnd won't behave differently with a single-page +file and will always import the file as if it was a project file. In the sheet +selector the project name is deduced from the file name and the sheet names +are copied from sheet titles. + +
+In EasyEDA there's a single point, typically the outer endpoint, of the terminal +that is sensitive to wire and terminal connections. In sch-rnd the whole +terminal is sensitive. EasyEDA wires crossing the insensitive middle +section of a terminal are connected to the terminal when importing the +file in sch-rnd and upon compilation a multi-connection warning is generated +unless it is disabled. + +
+It is also common in EasyEDA to connect two or more terminals and a wire in the +same endpoint. While this works in sch-rnd, it is generating the multi-connection +warning on compilation. Best practice is to move the terminals apart and make +sure it's always exactly two objects participating in a connection (green circle). +
+The multi-connection warning can be disabled via a config node called +multiport_net_merge. + +
+In sch-rnd each terminal of a symbol must have a name that is unique within +the symbol. If a part has 4 GND pins, the symbol is either drawn as a single +terminal and is assigned 4 physical pin numbers or if the symbol is drawn +with 4 GND terminals they have 4 different name name attributes (e.g. GND1..GND4). +
+In EasyEDA there's no such requirement on uniquely named terminals so many +EasyEDA symbols will have multiple GND and VCC pins. Such a symbol will +break in sch-rnd and generate errors during compilation. The only way to fix +this is manually renaming the redundant terminals to unique names. +