multi-part symbols and pcb footprints

[asa386-/[e-mail] [kicad-users]]

imagine if you will that I am using a lattice ECP2 FPGA in my schematic and I drew the schematic symbol as follows:
Loading Image...

such that I have two separate symbols:
ecp2_core = vcc, gnd, jtag, config inputs
ecp2_io = generic i/o interface pins for all banks

now the above two devices need to map into one 144 pin qfp ecp2 device. THAT (144 qfp) footprint already exists in kicad.

will I have problems mapping the above seperate/distinct pins on the two symbols to that ONE foot print?

I am trying to save myself having to redo the symbols as one symbol with two parts.
I am re-reading the eeschema and pcbnew,cvpcb manuals right now but thought Id ask just the same.

[Peter Ogden [e-mail] [kicad-users]]

You need to use a " "Multi-Unit" part. In other programs its known as
"Multi-gate" part. (For example, an IC that has 4xAND gates you want to
place as individual units).

When creating a new part in the eeschema library editor set the number of
units. See attached screenshot1.

[image: Inline image 1]

You choose which gate to edit using the toolbar dropdown menu in
Screenshot2.
[image: Inline image 2]
Note that if you want to have unique pins on each gate you have to have the
option set properly as you edit, otherwise it will apply all edits to all
units simultaneously and mess up your drawing. (Screenshot2)

Attached is an example for an Cyclone IV FPGA that I made with multiple
gates.

Post by asa386-/***@public.gmane.org [kicad-users]
imagine if you will that I am using a lattice ECP2 FPGA in my schematic
http://i.imgur.com/qbv6J7v.jpg
ecp2_core = vcc, gnd, jtag, config inputs
ecp2_io = generic i/o interface pins for all banks
now the above two devices need to map into one 144 pin qfp ecp2 device.
THAT (144 qfp) footprint already exists in kicad.
will I have problems mapping the above seperate/distinct pins on the two
symbols to that ONE foot print?
I am trying to save myself having to redo the symbols as one symbol with two parts.
I am re-reading the eeschema and pcbnew,cvpcb manuals right now but
thought Id ask just the same.

[asa386-/[e-mail] [kicad-users]]

what if I already have to two symbols done in kicad (from a previous project) that I want to combine into ONE multipart symbol under eeschema?

I used to import tools but they default to editing properties for one symbol and I can seem to add the other one.


is there a way to take two symbols created in kicad and from it create one MULTIpart symbol ?

[Peter Ogden [e-mail] [kicad-users]]

I think your best bet for taking two separate parts and combining them is
as follows:

1. Create a new blank multi-unit symbol with the number of units you want.
2. set unique editing per gate
3. add a dummy pin to each gate (so you can identify the two sections of
the multi-unit symbol)
4. save the symbol
5. open the .lib with a text editor, find your dummy symbol.
6. Copy the drawing/pin portions of each of your separate symbols into the
dummy symbol units.
7. Save the .lib and reload with kicad.

Post by asa386-/***@public.gmane.org [kicad-users]
what if I already have to two symbols done in kicad (from a previous
project) that I want to combine into ONE multipart symbol under eeschema?
I used to import tools but they default to editing properties for one
symbol and I can seem to add the other one.
is there a way to take two symbols created in kicad and from it create one
MULTIpart symbol ?

[asa386-/[e-mail] [kicad-users]]

This worked like a charm ... also noticed the format in the kicad file format pdf and was able to do the switch over and addition. One of the benefits of open source is configuration files like these are all text and hand editable.

Thanks again - time for me to find the kicad developers group and donate some money ...