| Author |
 Topic  |
|
|
cioma
125 Posts |
 Posted - 24 Aug 2016 : 15:18:21
|
| Could someone please describe part types "Schematic Only" and "PCB Only" (their intended usecases, relation to PDC, schematic-layout synchronization etc)? Neither help file nor user guide gives any details. Sure, I understand their intended use judging by the names but it would be great to understand them in details. |
|
|
jameshead
United Kingdom
125 Posts |
Posted - 25 Aug 2016 : 09:14:24
|
A PCB Only component may be some type of testpoint or fixing hole, that you don't want to show on a circuit diagram, and don't want to appear on a BOM if you drive your BOM from the schematic.
A Schematic only component may be some type of component that doesn't have a footprint on the PCB but you want on the schematic, and want on your BOM if you drive your BOM from the schematic.
There maybe parts you have on the PCB for mechanical fittings that you don't want on a PCB Assembly BOM because they are assembled later, not by the PCB Assembler, but you do want a footprint to define keep/out clearance areas.
Examples include:
Fuse and Fuse Holders
PLCC integrated circuit and PLCC holder
PCB pins and a component that plugs into them
Mounting hardware such as screws/washers
Female mating half to a Pin Header
0.1" Jumper to go over a pin header to select different functions
Memory Card socket and a Memory Card
How users deal with these things is different depending on company and their preferences, how they drive their BOMs and PCB Assembly instructions.
|
 |
|
|
cioma
125 Posts |
Posted - 25 Aug 2016 : 09:25:31
|
Many thanks for the explanation, it's very useful to have such part types.
Is there a way to have a part with symbol and footprint but omit it from BOM (report)? Currently I filter such components out if a certain component attribute is blank but maybe there is a better way of doing that. |
|
|
|
jameshead
United Kingdom
125 Posts |
Posted - 25 Aug 2016 : 09:59:10
|
I use Variants for this by creating one variant called "PCB Assembly" and select the component as "not fitted". I re-inforce it by having an attribute "Supply & Fitting" and indicate in this attribute whether the component is fitted by the PCB Assembler, at final assembly, or Not Fitted.
There is an IPC standard that lists the following as "standard" indentifiers:
DNI Do Not Insert
MO Model Only (i.e. Prototype)
ALT Alternative
I can't remember the number of the standard and I've never seen anyone else use it! "Not Fitted" should be clearer.
At Toshiba we used the word "Ketsu" to indicate a not-fitted component. It allegedly meant not-fitted in Japanese but they did have a habit of trying to pull one over on us from time to time!
One thing I have come across is that I have been asked to remove components that say they are "Not Fitted" from BOMs before boards are released because PCB Assembler purchasing teams find it confusing, then a few weeks later I get querys from the PCB Assembler's Production Engineers about components that are on the board but not listed on the BOM and asking if they should be fitted or not.
|
|
|
|
cioma
125 Posts |
Posted - 25 Aug 2016 : 10:55:43
|
Thanks for detailed explanation.
BTW, I looked up definition of "ketsu" and it doesn't seem to mean "not fitted" at all ;) |
|
|
|
steve
United Kingdom
316 Posts |
Posted - 31 Aug 2016 : 10:54:40
|
SCM and PCB Only parts have been within the product from its early days, but in the main have been replaced by SCM Doc Symbols and PCB Doc symbols and their various types. They are however used for alien design translation to deal with similar marked components in those incoming designs, where for instance, their nets on pins on a SCM Only part can still synchronise to the same part, which has been manually placed in the PCB, using the Ignore SCM Only Status switch in Design Settings.
Parts with ancillary hardware such as sockets are dealt with by using an Associated Part for the socket, that can appear in a BOM and which is defined either at the Part or Footprint level. This will also deal with mounting hardware, bolts, washers, nuts etc. Associated Parts can also be added at the Design level.
Placement areas for other build items, with or without silkscreen/pads etc are created as Doc Symbols and as such are not considered in Synchronisation.
Items like Fixing Holes are added as a Mounting Hole directly, in which case are not considered during a BOM output.
Testpoints are dealt with by the system by being a Testpoint item as are StarPoints.
Pulsonix Assistance |
|
|
|
jameshead
United Kingdom
125 Posts |
Posted - 31 Aug 2016 : 13:49:08
|
I've found schematic only parts to be more powerful and flexible than associated components and doc symbols.
For example you can add a schematic-only part that has the usual attributes set up in the Part technology file for a 2.54 mm pitch jumper link, or any number of such jumper links, and add them to your schematic to fit on a 2.54 mm pitch header. That header can be any number of pins and/or rows. The jumper link may be a specific colour and you may have specific colour jumper links to be fitted onto different headers on the PCB.
Another bonus is you can use the Attributes button in the Library dialogue window to open the spreadsheet view to edit schematic-only components but this isn't available for schematic doc symbols.
You can't do this as easily with associated components as they can't be edited as easily for quantity or for a different type.
The same can be applied to fuse holders and fuses whether you add the fuse to the circuit diagram and the fuse holder as a schematic only component or vice-versa.
I find associated components are useful for wire to board connectors, such as the Molex friction-locked series such as 22-27-2021 where you can add the wire-end housing (Molex 22-01-2025) as an associated component, and then add the crimp terminals (Molex 08-50-0032) as an associated component to the housing. |
|
|
|
jameshead
United Kingdom
125 Posts |
Posted - 31 Aug 2016 : 13:55:37
|
Just to clarify, when I say Associated Parts can't be as easily edited I mean you can't edit them easily from the component they are associated with. You can edit them in Design Properties but that's not as clear or useful.
For my jumper link example, you would need to add every colour of jumper link that you want available in your library as an associated part to every pin header connector you may want to use them with, that's in your library, and then edit them in Design Properties for the quantity you want on the PCB. I think this is more cumbersome that just having a schematic only component. |
|
|
| |
Topic |
|
