pcb-rnd knowledge pool


Micro-Cap to pcb-rnd (schematics/netlist import)

import_microcap by Tibor 'Igor2' Palinkas on 2020-08-21

Tags: howto, micro-cap, microcap, schematics, netlist, import

node source



Abstract: Micro-Cap is a freeware schematics capture and simulator program running on windows. It supports a variety of different netlist formats, from which multiple formats are suitable for a pcb-rnd layout flow. This article provides step-by-step instrictions on a forward annotation from schematics to pcb-rnd.


1. Draw your schematics in Micro-Cap. (The details on this step is out of the scope of this document, please consult the user manual for Micro-Cap on using the software.)

A simple example schematics with an lm117

2. Assing footprint TO220 to the X1

Footprint assignment on X1

3. Assing footprint 1206 to the all the passives; make sure you use footprint names thare are accessible in your pcb-rnd footprint library. To check that, run pcb-rnd, open the librayr window and browse the tree and/or enter footprint names in the filter entry. NOTE: footprint names in pcb-rnd are case sensitive, to220 is not the same as TO220!

Footprint assignment on the passives

4. When done, take a final look at the schematics to make sure all footprints are filled in.

Schematics with the footprints filled in

5. Alternatively you can edit footprint values in the Package Editor. Note: different output formats may have different footprint (package) name overrides. Since the default name can not be modified, you need to modify the per format override name. We are going to export in the accel EDA format so it is essential to have the footprint value right in that field.

Package editor

6. Export the the netlist from Micro-Cap. The preferred format is Accel EDA netlist, but Protel netlist 2.0 should work too.

Export dialog to Accel EDA netlist

The accel export from our test file is included here for reference.

7. Import the netlist in pcb-rnd: start with a blank board, then File menu, Import, Import schematics; this will bring up the import dialog box:

Blank import schematics dialog

8. Select the file format: change tEDAx to accel_net; then click on the browse button and select the exported netlist file:

Import schematics dialog filled in

9. Click on the import button - this will load all footprints mentioned in the netlist file and place them on the board. Press {c r} (that is 'c' then 'r') for rat nest optimization: this will draw the logical connections imported form the netlist. Press {w n} to open the netlist window, which will also show the netlist.

Board ready to layout: subcircuits placed, rats nest drawn

10. Save the board. This will save your import settings too; if you use File/Import/Import schematics again, it will remember the file format and the file name. The normal forward-annotation workflow is making modifactions to the schematics, doing a new export in MC, then doing a new import in pcb-rnd. That will replace a few subcircuits and updates the netlist to reflect changes in the schematics.

Note: do not use the orcad netlist format because the export code in MC and/or the file format does not support quoting comlex footprint names, so parametric footprints, such as dip(14) will cause syntax error in the file saved from MC.

Note: do not use the PADS netlist format, because it does not include component values. Missing component values may render your later BOM or XY export useless.

Note: requires pcb-rnd newer than 2.2.3 (at least svn revision r32333).