IPC naming convention for schematic symbols?
Printed From: PCB Libraries Forum
Category: Libraries
Forum Name: OrCAD Capture
Forum Description:
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=54
Printed Date: 27 Nov 2024 at 6:47am
Topic: IPC naming convention for schematic symbols?
Posted By: Chian
Subject: IPC naming convention for schematic symbols?
Date Posted: 11 May 2012 at 9:37am
|
Hi,
Does IPC has the naming convention for the schematic symbols? I know we're using IPC-7351B for the SMT and IPC-7x51 for connectors land patterns. Maybe there is an existing one out there that i'm not aware of? Please advice.
Thanks,
Chian
|
Replies:
Posted By: Tom H
Date Posted: 11 May 2012 at 10:23am
|
IPC does not have a
standard naming convention for schematic symbols.
I would recommend that
every schematic symbol be named -
ComponentManufacturerName_MfrLogicalPartNumber
Example of a Texas
Instruments schematic symbol Name:
TI_SN74GTLPH32912ZKFR
This
way every schematic symbol has a unique name. There are almost 50 million
devices with Logical Part Numbers assigned by each manufacturer. Therefore
there are 50 million different schematic symbols.
I
would also store each schematic symbol in a component manufacturer library.
i.e.: If I use 100 different manufacturers I would have 100 different
libraries. This makes it easy to maintain and easy to locate parts.
|
Posted By: BryanT
Date Posted: 18 May 2012 at 11:46am
|
Hi Tom, Not sure if I agree with your approach. I think it definitely has to do with the tool you are using and how your library is setup, and the individual company's process. For example, if you are using Cadence and utilize Part Tables, all of your manufacturer's & ordering information would be entered in a part table. The schematic symbols would be given a generic name so it can be used with all manufacturer part numbers of the same type component, regardless of package. The package information would be chosen from the part table. This is true for Cadence Concept, Orcad Capture, DxDesigner, Cadstar and Altium - that I know of. So for example lets use DS9367A from TI. This part comes in 2 packages - an SO8 (DS9637ACM) and 8-pin Dip package(DS9367AMJ). The pinouts are identical for both parts so you would only need ONE schematic symbol called DS9367A. When the part is placed on a schematic, you would choose which package you'd want to use. So creating all the extra symbols that are identical creates more overhead and maintenance. You could still create individual libraries for each vendor if that makes sense for the company. As I said, I think what tool you use drives how you should name your symbols. Just my 2 cents.
|
Posted By: Randy Clemmons
Date Posted: 23 May 2012 at 8:44pm
Bryan,
I agree with your logic, for example I have only created 1 resistor schematic symbol for all resistors regardless of manufacturer.
I have one AND gate that covers LVC, AUP and other logic level families. I'm not creating library bloat or needlessly duplicating symbols.
I only create unique symbols as needed, and I assign the part number to the symbol only if it's unique to that part.
Randy
|
Posted By: Nightwish
Date Posted: 24 May 2012 at 1:02am
|
Randy and Bryan,
I also agree with you guys that this has something to do with the software you use and even the part number naming convention in the PDM system. If we create duplicate symbols in library it will be hard for the librarians to maintain the library. We use Mentor DxDesigner-Expedition flow and we only have one resistor symbol for all Resistor part in library no matter their Manufacture, Value and package type. We use the same rule for other discrete components like capacitor and inductor and even the logical symbol.
If a DDR chip have three AML from TI, Fairchild and may be Samsung while actually they have the same footprint and symbol, we only need to have one symbol and the part name may be called 200-00001 for example. The EE can search this in PDM or Value in Databook to find this part. In our PDM we don't use Manufacture part number because sometimes we need second source for one part.
Thanks,
Nightwish
|
Posted By: Mattylad
Date Posted: 02 Jun 2012 at 6:51am
It looks likes tom's theory on schematic symbol naming is totally off piste.
It's bad enough having different footprints for components that are essentially of similar sizes I do not know anyone that would want to have a different symbol for the same symbol just because a different manufacturer makes the device.
This would be a total nightmare to manage should something need changing, it would need changing on several symbols.
Although there is no "standard" for their naming it seems common sense to name them for what the represent. A resistor, capacitor, diode etc. Why call them something else.
If an IC then name it for the IC it is, if the symbol represents a range of IC's from the series then call it after the range rather than adding component specific naming to it.
Sorry Tom but IMO your over complicating what should be simple.
|
Posted By: Tom H
Date Posted: 02 Jun 2012 at 8:26am
|
Of course all 2-pin descrete components will have 1 symbol for Capacitor, Resistor, Diode, Inductor, Fuse, Crystal, etc. It's the millions of one-of-a-kind Logical Part Number for IC's where each individual electronic device has various pin assignments, logical part number, logical description, it's unique web-link to datasheet and pre-mapped to the correct IPC footprint name. These even contain Digi-Key links to order the parts. When we open the Parts On Demand (POD) the PCB Library Vending Machine and allow everyone to upload the manufacturer recommended schematic symbol for PCB Libraries, Inc. to sell to 6 million EE engineers worldwide, do you think anyone is going to purchase a resistor in every value? I don't think so. As a mater of fact I don't think we'll sell 1 resistor schematic symbol. I am creating the entire Texas Instruments product line of library parts and there are 43,000 different logical part numbers and 43,000 different schematic symbols. No one will ever use them all, but they're all available to download, loaded with unique properties for each one, if anyone needs them.
|
Posted By: konraditen
Date Posted: 14 Jun 2012 at 4:23pm
|
I have written up 2 schematic symbol naming conventions for
different companies. It is quite the challenge, because you will never cover
everything. What we wanted was a unique method to describe each schematic symbol,
so when you place it within the schematic editor you know what part is used. When
you place a part in the schematics you will need to know the very least the
most important parameters of the part you pick. There is just no way you place
a 1uF cap and be done with it. How do you know if it is a SMT or THT component?
1206 or 0805, maybe 0402. Is it being used in a commercial environment or maybe
in a military environment? What the temperature range of the cap?
The most elegant solution so far is I have used is a database
library, that contains all parameters and a link to symbol, footprint and datasheet.
This is very convenient for the end user to work with. It was a simple pick and
place. And no editing parts once they were placed in the schematics.
|
Posted By: jonathan s
Date Posted: 21 Jun 2012 at 6:32am
|
Konrad,
Our company is looking to implement a 6? digit part number and naming convention for our parts, and I'd love any ideas our thoughts you might have in how to go about setting up a good convention. At previous jobs we had good luck with such a system, so I'm very interested in establishing one here as well.
For that matter, if anyone has any good resources for some examples of naming conventions for parts, I'd be happy to take a look at what has been done elsewhere.
Thanks,
Jonathan
|
Posted By: konraditen
Date Posted: 21 Jun 2012 at 11:08am
Hi Jonathan
Our naming convention relied on describing a part so you can identify what it is right away without having to look it up. For example a cap:
C,NP,220p,100V,C0G,5%,0805,M
It's just like Digikey used the description of the part, just a little more detailed.
If you simple use digit part numbers you cannot know what a part is. You would always have to go and look it somewhere.
Another naming convention I came across was the combination of letters and numbers. 4 letters to describe what type of part and then the manufacturing part number separated by a period.
For example SMTF.MMBT5551. In this case it is a SMT FET MMBT5551.
Regards,
Konrad
|
Posted By: Randy Clemmons
Date Posted: 21 Jun 2012 at 8:24pm
Take a look at:
http://ottobelden.blogspot.com/2011/08/significant-andor-insignificant-part.html" rel="nofollow - http://ottobelden.blogspot.com/2011/08/significant-andor-insignificant-part.html
|
Posted By: JohnH
Date Posted: 24 Jun 2013 at 12:45am
|
As mentioned it very much depends on the system. In general I prefer systems which can support the "one to many" approach where a symbol can map to multiple footprints. These systems are typically supported by a database. For symbols which incorporate the pin number mapping I use this convention: [Prefix]_[item]_[Variant] For an IC the prefix would be IC and the item would be the manufacturers part number with RoHS and packaging codes removed. For other parts such as Transistors the prefix would be Transistor the item could be NPN and the variant would be the pin mapping in the order of pin e.g. Transistor_NPN_ebc This is an NPN transistor with emitter pin 1, base pin 2 and collector pin 3
|
|