managing multi part components (IC+Socket, Battery+Socket) into BoM

Discussion:

anool

2012-01-07 11:12:30 UTC

Hi,

When generating a Bill of Materials (BoM), how is it possible to include multiple items against a single Part.

For example, on the Board, I have a 14 Pin IC, but the actual bill of materials will have to include a 14 pin IC Socket AND the actual 14 pin IC.

Likewise for other parts like a Coin Battery (plus its socket).

For larger boards with a lot of components, it becomes quite unwieldy to manually edit the BoM to add in the additional components.

Is there a solution to this issue ?

Anool

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

<*> To change settings via email:
kicad-users-digest-***@public.gmane.org
kicad-users-fullfeatured-***@public.gmane.org

<*> To unsubscribe from this group, send an email to:
kicad-users-unsubscribe-***@public.gmane.org

<*> Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/

Lawrence

2012-01-10 13:32:23 UTC

Permalink

Anool,
The scenario of an IC and a socket, a battery and a battery holder, or a fuse and a fuse holder are not multi part components. These parts will have their own part number and will have their own reference designator. Thus they will be accounted for in the parts list.

The 14-pin IC will use class designation letter U unless it is an operational amplifier, in which case the class designation letter is AR. The class designation letter of the socket starts with X. If the IC is reference designated U3, for instance, the socket for U3 will be referenced designated XU3. The schematic diagram would show the IC with ref des U3 with no associated land pattern. Somewhere close to the U3 ref des put the ref des XU3, it will have no schematic diagram but would have a land pattern.

For a double coin cell battery holder the schematic diagram would show, for instance, two batteries (cells) with ref des BT1 and BT2, with no land pattern for either battery. Somewhere close to the BT1 ref des the double coin cell battery holder would be reference designated XBT1 with no schematic entry, but would have a land pattern.

This same scenario applies to a fuse or fuses and fuse holder. A fuse uses class designation letter F and the fuse holder (socket) class designation letter would be XF.

Regards, Lawrence Joy (9V1/WN8P)

Post by anool
Hi,
When generating a Bill of Materials (BoM), how is it possible to include multiple items against a single Part.
For example, on the Board, I have a 14 Pin IC, but the actual bill of materials will have to include a 14 pin IC Socket AND the actual 14 pin IC.
Likewise for other parts like a Coin Battery (plus its socket).
For larger boards with a lot of components, it becomes quite unwieldy to manually edit the BoM to add in the additional components.
Is there a solution to this issue ?
Anool

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

<*> To change settings via email:
kicad-users-digest-***@public.gmane.org
kicad-users-fullfeatured-***@public.gmane.org

<*> To unsubscribe from this group, send an email to:
kicad-users-unsubscribe-***@public.gmane.org

<*> Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/

sembazuruplus

2012-11-05 02:20:58 UTC

Permalink

I'm not quite so clear exactly how this works. How does the X part's land pattern get connections to the base part(s) schematic connections? Particularly with the example of the two batteries in a single holder. There would be a net connecting the two schematic symbols of the batteries, but no place for that net on the PCB. I'm also interested in this as a way of representing off-board parts that connect to a header. I'm looking for a way for the off-board part to still be on the schematic and in the BOM, but when I go to design a PCB I only have to place and route on-board components.

Is there a tutorial available that shows your method of getting this to work in KiCAD?

Post by Lawrence
Anool,
The scenario of an IC and a socket, a battery and a battery holder, or a fuse and a fuse holder are not multi part components. These parts will have their own part number and will have their own reference designator. Thus they will be accounted for in the parts list.
The 14-pin IC will use class designation letter U unless it is an operational amplifier, in which case the class designation letter is AR. The class designation letter of the socket starts with X. If the IC is reference designated U3, for instance, the socket for U3 will be referenced designated XU3. The schematic diagram would show the IC with ref des U3 with no associated land pattern. Somewhere close to the U3 ref des put the ref des XU3, it will have no schematic diagram but would have a land pattern.
For a double coin cell battery holder the schematic diagram would show, for instance, two batteries (cells) with ref des BT1 and BT2, with no land pattern for either battery. Somewhere close to the BT1 ref des the double coin cell battery holder would be reference designated XBT1 with no schematic entry, but would have a land pattern.
This same scenario applies to a fuse or fuses and fuse holder. A fuse uses class designation letter F and the fuse holder (socket) class designation letter would be XF.
Regards, Lawrence Joy (9V1/WN8P)

Lawrence

2012-11-06 05:34:55 UTC

Permalink

The schematic diagram you normally look at is the schematic diagram of an "assembly". The accompanying "parts list" (PL) and the accompanying "assembly drawing" is for the complete assembly. The PCB is a cut-set (definition from graph theory) or only a (major) portion of the assembly schematic diagram. The parts you call off-board do not have land patterns on the PCB but they are still parts of the schematic diagram of the assembly. Thus the reference designator (serial) numbers of the parts off-board are in accordance with the assembly and are properly accounted for in the PL.

Ferrite beads put on leads of parts are another problem of parts that are/should be in the schematic diagram of the assembly but not part of the PCB. Such as putting ferrite beads on the leads of transistors or putting ferrite beads on the through hole leads of connectors. In these cases there is no land pattern for the ferrite beads. Another scenario is a heat sink clipped on to a transistor. The schematic diagram would use the class designation letter(s) "MP", for mechanical part, somewhere next to the transistor. There would be no land pattern and the heat sink would be listed on the PL.

Now to your question of how this is done with KiCad. I don't know and as far as I know there is no tutorial on this subject. No one has probably thought about this. One suggestion is that you have two (ugh!) schematics, one of the assembly and one of the PCB.

IF ANYONE HAS READ THIS FAR, UNDERSTANDS THE PROBLEM, AND CAN EXPLAIN--PLEASE RESPOND.

Regards, Lawrence Joy (9V1MI, WN8P)

Post by sembazuruplus
I'm not quite so clear exactly how this works. How does the X part's land pattern get connections to the base part(s) schematic connections? Particularly with the example of the two batteries in a single holder. There would be a net connecting the two schematic symbols of the batteries, but no place for that net on the PCB. I'm also interested in this as a way of representing off-board parts that connect to a header. I'm looking for a way for the off-board part to still be on the schematic and in the BOM, but when I go to design a PCB I only have to place and route on-board components.
Is there a tutorial available that shows your method of getting this to work in KiCAD?

Chris Elliott

2012-11-06 20:02:12 UTC

Permalink

Ah, I misunderstood. You were discussing how it should be done, not how
to do it in KiCAD. I actually agree with your sentiments. Maybe we
should work together in drafting a methodology to suggest to the devs
(especially since they seem to be doing a major overhaul to the backend
already).

Post by Lawrence
The schematic diagram you normally look at is the schematic diagram of
an "assembly". The accompanying "parts list" (PL) and the accompanying
"assembly drawing" is for the complete assembly. The PCB is a cut-set
(definition from graph theory) or only a (major) portion of the assembly
schematic diagram. The parts you call off-board do not have land
patterns on the PCB but they are still parts of the schematic diagram of
the assembly. Thus the reference designator (serial) numbers of the
parts off-board are in accordance with the assembly and are properly
accounted for in the PL.
Ferrite beads put on leads of parts are another problem of parts that
are/should be in the schematic diagram of the assembly but not part of
the PCB. Such as putting ferrite beads on the leads of transistors or
putting ferrite beads on the through hole leads of connectors. In these
cases there is no land pattern for the ferrite beads. Another scenario
is a heat sink clipped on to a transistor. The schematic diagram would
use the class designation letter(s) "MP", for mechanical part, somewhere
next to the transistor. There would be no land pattern and the heat sink
would be listed on the PL.
Now to your question of how this is done with KiCad. I don't know and as
far as I know there is no tutorial on this subject. No one has probably
thought about this. One suggestion is that you have two (ugh!)
schematics, one of the assembly and one of the PCB.
IF ANYONE HAS READ THIS FAR, UNDERSTANDS THE PROBLEM, AND CAN
EXPLAIN--PLEASE RESPOND.
Regards, Lawrence Joy (9V1MI, WN8P)

Post by sembazuruplus
I'm not quite so clear exactly how this works. How does the X part's

land pattern get connections to the base part(s) schematic connections?
Particularly with the example of the two batteries in a single holder.
There would be a net connecting the two schematic symbols of the
batteries, but no place for that net on the PCB. I'm also interested in
this as a way of representing off-board parts that connect to a header.
I'm looking for a way for the off-board part to still be on the
schematic and in the BOM, but when I go to design a PCB I only have to
place and route on-board components.

Post by sembazuruplus
Is there a tutorial available that shows your method of getting this

to work in KiCAD?

Lawrence

2012-11-09 03:55:00 UTC

Permalink

An understanding of what goes on the PCB that would have land patterns and what is part of the assembly is what needs to be clear. Here is a short treatise:
A) For loose ferrite beads (class letter E) put on the leads of leaded transistors or connectors the land pattern of the part is used as normal. On the schematic diagram use the graphic symbol for the ferrite bead (IEEE Std 315A-1986, Clause 6.2.11--an IEC symbol), without any pins (therefore, no net connections), placed over the "wire" connections.
B) For two coin cells in a single holder: On the schematic diagram show the socket (class letter XBT) with all pin connections. (I would use the male contact symbol(s) as shown in IEEE Std 315A-1986, Clause 5.3.8). In between the two male contacts show two battery symbols (class letters BT) without any pins (and therefore no net connections).
C) For the case of a fuse held by snap in fuse end clips: On the schematic diagram show the two fuse clips (ref des XF1A and XF1B). The land pattern on the PCB will be that of the fuse clips. Then show on the schematic diagram the symbol for a fuse (ref des F1) without any pin connections and, you should get the idea by now, there will be no net connections.
D) For an IC with a socket: Let's use a single op amp with an 8-pin DIP socket as an example. On the schematic diagram the op amp (ref des AR1) would show all eight pins and the net connections. No graphic symbol for the socket is needed, just place the ref des XAR1 next to AR1 to indicate a socket and the land pattern to use would be that of the 8-pin DIP socket.
E) Now for your parts connected to a header. You will have to describe this a little bit more. Is your "header" a male (pin) terminal strip where the parts are hard wired (soldered) to the male pins? Or is your setup a pair of connectors where you might have the male terminal strip on the PCB but your parts are soldered to a female terminal strip that is plugged into the male terminal strip?

Regards, Lawrence Joy (9V1MI, WN8P)

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

<*> To change settings via email:
kicad-users-digest-***@public.gmane.org
kicad-users-fullfeatured-***@public.gmane.org

<*> To unsubscribe from this group, send an email to:
kicad-users-unsubscribe-***@public.gmane.org

<*> Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/

Chris Elliott

2012-11-28 21:55:57 UTC

Permalink

That might work. I'll have to play with it and see if KiCad chokes.

Perhaps I used the wrong term 'header', when I more generically meant
connector. (I think i was thinking of using a 0.1" spacing pin header as
a connector for off-board parts, but it could also easily be applied to
basically any type of connector, especially when doing system-level
schematics instead of (or in conjunction with) PCB schematics.)

Post by Lawrence
An understanding of what goes on the PCB that would have land patterns
and what is part of the assembly is what needs to be clear. Here is a
A) For loose ferrite beads (class letter E) put on the leads of leaded
transistors or connectors the land pattern of the part is used as
normal. On the schematic diagram use the graphic symbol for the ferrite
bead (IEEE Std 315A-1986, Clause 6.2.11--an IEC symbol), without any
pins (therefore, no net connections), placed over the "wire" connections.
B) For two coin cells in a single holder: On the schematic diagram show
the socket (class letter XBT) with all pin connections. (I would use the
male contact symbol(s) as shown in IEEE Std 315A-1986, Clause 5.3.8). In
between the two male contacts show two battery symbols (class letters
BT) without any pins (and therefore no net connections).
C) For the case of a fuse held by snap in fuse end clips: On the
schematic diagram show the two fuse clips (ref des XF1A and XF1B). The
land pattern on the PCB will be that of the fuse clips. Then show on the
schematic diagram the symbol for a fuse (ref des F1) without any pin
connections and, you should get the idea by now, there will be no net
connections.
D) For an IC with a socket: Let's use a single op amp with an 8-pin DIP
socket as an example. On the schematic diagram the op amp (ref des AR1)
would show all eight pins and the net connections. No graphic symbol for
the socket is needed, just place the ref des XAR1 next to AR1 to
indicate a socket and the land pattern to use would be that of the 8-pin
DIP socket.
E) Now for your parts connected to a header. You will have to describe
this a little bit more. Is your "header" a male (pin) terminal strip
where the parts are hard wired (soldered) to the male pins? Or is your
setup a pair of connectors where you might have the male terminal strip
on the PCB but your parts are soldered to a female terminal strip that
is plugged into the male terminal strip?
Regards, Lawrence Joy (9V1MI, WN8P)

Lawrence

2012-11-30 05:36:30 UTC

Permalink

I think you need to look at ASME Y14.44-2008, the rules for assigning reference designators in what is called the Unit Numbering Method. I found a PDF of this on a Chinese Website but can only view it, not down load it.

As an example if you have a motherboard that has plug in PCB assemblies (PBAs) [IPC definition as far as I know] the schematic diagram for each PBA is a separate entity and each entity is covered by its own documentation. Each subassembly would carry a ref des prefix. Following are examples:
1) A subassembly A1 with a connector P1 that connects to a socket. A1P1 mates with XA1 (or XA1P1) (X is the class letter for a socket not a crystal, Y is the class letter for a crystal) on the motherboard.
2) A subassembly A2 with fingers (no separate connector) that connects to a socket. A2 (the PBA) mates with XA2 on the motherboard.
3) A subassembly A3 with 2 sets of fingers (no separate connectors) that connects to 2 separate connectors. A3 (the PBA) mates with XA3A and XA3B on the motherboard.
I think scenario 1) covers what you want, but if not be more specific as to your setup and I will try to answer. Look at ASME Y14.44-2008, Figure 2 for sockets and Figure 3 for a system schematic diagram as examples.

Regards, Lawrence Joy (9V1MI, WN8P)

Post by Chris Elliott
That might work. I'll have to play with it and see if KiCad chokes.
Perhaps I used the wrong term 'header', when I more generically meant
connector. (I think i was thinking of using a 0.1" spacing pin header as
a connector for off-board parts, but it could also easily be applied to
basically any type of connector, especially when doing system-level
schematics instead of (or in conjunction with) PCB schematics.)

Chris Elliott

2012-11-30 22:39:14 UTC

Permalink

I'll try to find a copy of that spec somewhere.

You overestimate the complexity of my project. If it were multiple PCBs
obviously each would have their own schematic, if for nothing else to
keep their netlists separate. My project is a single PCB that connects
to various discreet components like motors, switches, encoders, etc. I
could draw the external parts with drawing objects, but then I wouldn't
get them on the BOM. Prefixing their Ref'ds with X would work well for
filtering the off-board parts when kitting up for assembly. (J1 on the
board connects to XP1 which is wired to motor XB1, J2 on the board
connects to XP2 which is wired to limit switch XS2, etc.)

I just haven't had a chance to play with this in KiCad to see how badly
it chokes on schematic parts w/o pins linking to blank PCB footprints...
I may not get a chance to play with this until between Christmas and the
New Year when I have off of work. (But that should give me plenty of
time to find and study ASME Y14.44-2008...)

Post by Lawrence
I think you need to look at ASME Y14.44-2008, the rules for assigning
reference designators in what is called the Unit Numbering Method. I
found a PDF of this on a Chinese Website but can only view it, not down
load it.
As an example if you have a motherboard that has plug in PCB assemblies
(PBAs) [IPC definition as far as I know] the schematic diagram for each
PBA is a separate entity and each entity is covered by its own
documentation. Each subassembly would carry a ref des prefix. Following
1) A subassembly A1 with a connector P1 that connects to a socket. A1P1
mates with XA1 (or XA1P1) (X is the class letter for a socket not a
crystal, Y is the class letter for a crystal) on the motherboard.
2) A subassembly A2 with fingers (no separate connector) that connects
to a socket. A2 (the PBA) mates with XA2 on the motherboard.
3) A subassembly A3 with 2 sets of fingers (no separate connectors) that
connects to 2 separate connectors. A3 (the PBA) mates with XA3A and XA3B
on the motherboard.
I think scenario 1) covers what you want, but if not be more specific as
to your setup and I will try to answer. Look at ASME Y14.44-2008, Figure
2 for sockets and Figure 3 for a system schematic diagram as examples.
Regards, Lawrence Joy (9V1MI, WN8P)

Lawrence

2012-12-01 09:37:32 UTC

Permalink

Now that you have explained your "system" setup the answer is simple enough:
1) For the PBA "controller", like a solid state thermostat for a heating and air conditioning unit, the parts (KiCad = components) on the PCB would be done as usual and you will have a parts list (PL) (KiCad = BOM). These controllers use multiple terminal screw type terminal blocks (class letter TB) where all the wires coming from or going to the other parts or assemblies of the system get connected. In your case it sounds like you want to use mating connectors, so the connector on the PBA would use class letter J. [The ref des I use on a PL for the PCB is "U0"--class letter U is for anything that is potted, embedded, riveted, or hermetically sealed with the number zero as parts of the circuit on the schematic diagram always start with 1.
2) For the parts and assemblies that make up the rest of the system you would have a separate schematic diagram that shows the wiring. You don't care about the net list because these parts don't go on a PCB. 3) For the overall complete PL you have to combine the two PLs and it would look like the following:
A1 Controller PBA
A1AR1 Op Amp driver
A1BT1 Battery
A1BT2 Battery
A1J1 Connector
A1J2 Connector
A1S1 Switch
A1TB1 Terminal board or terminal block
A1U0 Controller PCB
A1U1 Microcontroller
A1VR1 Voltage regulator IC
A1XBT1 Dual battery holder
A1... All other parts on PCB
B1 Motor
E1 Encoder
P1 Connector
P2 Connector
S1 Switch
S2 Switch
W? Wire
... All other parts

That should take care of it. Check the standards.

Regards, Lawrence Joy (9V1MI, WN8P)

Post by Chris Elliott
I'll try to find a copy of that spec somewhere.
You overestimate the complexity of my project. If it were multiple PCBs
obviously each would have their own schematic, if for nothing else to
keep their netlists separate. My project is a single PCB that connects
to various discreet components like motors, switches, encoders, etc. I
could draw the external parts with drawing objects, but then I wouldn't
get them on the BOM. Prefixing their Ref'ds with X would work well for
filtering the off-board parts when kitting up for assembly. (J1 on the
board connects to XP1 which is wired to motor XB1, J2 on the board
connects to XP2 which is wired to limit switch XS2, etc.)
I just haven't had a chance to play with this in KiCad to see how badly
it chokes on schematic parts w/o pins linking to blank PCB footprints...
I may not get a chance to play with this until between Christmas and the
New Year when I have off of work. (But that should give me plenty of
time to find and study ASME Y14.44-2008...)