General CIS Question on Database tables.

So the ALT_SYMBOLS that came out of the old days of part tables in Concept + Packager have been simplified in CIS.  Just enter multiple footprints into the PCB Footprint column separated by commas and the alt symbols get carried into Allegro.

So I'm a bit unclear on the second question but here's how it *should* work:  There should be a separate entry in the CIS database for each value so that you buy the correct part for each resistor.  However, each row in the database can use the same schematic symbol and the same footprint symbol.  Let's say they want 100 different 0603 resistors.  A value from 1 ohm to 100 ohms...then there would be 100 entries in the database with a customer unique attribute for each part (the key) and then fill in the unique vendor name and part number for each row.  But each row carries *mostly* identical information for every part.

In my database table for resistors I use an internal part number for each resistor and mark that as the "key".  Then I uniquely describe each part in the "description" field and add the appropriate vendor name(s) and part number(s) in subsequent columns.

Red thanks for this info, very useful.

On the alt symbols new mechanism is this something that is supported in 17.4 only in that the pcb footprint can be combined to serve the alt_symbol function & IF 17.4 only how would that effect say what existed in 17.2.
Was wondering if one could use the dedicated Alt_Symbols field so as to support legacy versions of CIS instead of the combo pcb footprint and if a dedicated field for that is supported in say 17.4

The plan was to go with 17.2 instead of 17.4 and they would be doing the DB in the 17.2 realm.

I like how you have your DB constructed in that you are keying off an internal part number. I suspect alot of companies would go this road.

Just a note on the Alt Symbols. They have standard SMD Footprints that are made to IPC7351 standards in that there are 3 types, A ,B, C. A being the largest & type B which is pretty much the norm. The alternate footprint would be type A. Mainly the alt symbols would just be used for passive smd's only.

So here is a mind bender for you. If an alternate footprint is used in the PCB is there any way to know from the perspective of the BOM that this would be the one that gets used. It used to be that if you had used an alternate footprint and back annotated to capture, capture would not know that the Alt Symbol was being used as the "Primary Symbol" as capture just looked at the PCB Footprint field and used that for the BOM.

From a BOM perspective I was thinking they could also generate that out of Allegro, I kind of like the flexibility that Allegro has in doing BOM's more so than capture. Allegro would pick up that ALT Symbol for BOM purposes.

On the second part of my question I was alluding to something like having a pre-populated database similar to what you have for your resistors. For example manufacturers post this info in a xls format so that would
aid in less typing in of data to the DB. So say they got 100 resistors and they are all 1206 footprint type. Can those 100 resistors be selected and in one go each row be updated to reflect that the PCB Footprint to use
would be a 1206 ?.

Thanks Again.

Let me see if I can tackle your questions.

As far as using the comma in the PCB Footprint for alternate symbols this has been a feature of CIS since it was introduced so it works fine for *any* version of CIS.  I run it currently on 16.6, 17.2, 17.4.  Same exact database but different CIS config files...all promote the comma separated field as ALT SYMBOLS when placing.

You can *also* use the field ALT_SYMBOLS in your database but it is also a comma separated field that gets brought into Allegro via packager (a la Concept days from forever ago).  You just have to be sure that the Allegro.cfg file has ALT_SYMBOLS YES in it, which I believe it does when coming direct from Cadence but go check.

You are correct about Allegro being able to generate the BOM but I agree I don't think it traverses back up to Capture.  I by the way prefer the CIS BOM generation tool as it's way more flexible and it exports Excel native files which is nice.  I export and tag each field in CIS that I want to show as unique so for example, a resistor will have value, tolerance, package, wattage, voltage-rating all as key fields.   Perhaps Allegro allows that but some of that info is not natively imported into Allegro and I'm way too lazy to push it over to the PCB tool.

So for the database question, I think from what I read in your question, the answer is yes.  I use Access as my database and essentially it has most features that you would find in Excel.  So yes, you could add a column called PCB Footprint and fill it with 1206.  Access just needs a key field to prevent duplication and thus the unique part number concept I mentioned previously. You could also tag a field with an incrementing number to add uniqueness --  which is what the old component portal and now CIP do if you want to add a part on the fly to the database.

Let me know if you have more questions.

Thanks alot Red, Info helped me out and clarified my questions.

All the best