[PCB_FORUM] Re: same symbol - different number of pins

We handle this problem in the following manner.

For part 1 we add the pack_type at the end of the primitive line like this:

primitive 'LM1117', 'LM1117_DTX' 

This will give the pin mapping for one of the physicals.

 

Create a second primitive 

primitive 'LM1117_MTX' (note that the 'LM1117' is not repeated on the second 
primitive. That confuses Concept)

This will give the pin mapping for the second footprint.

 

In the part.ptf file you will need the Key Property Pack_type at the beginning 
of the table

 

:Pack_type

'DTX' (the rest of the entry for all part entries using the same pinout)

 

'MTX' (the rest of the entry for all part entries using the same pinout)

 

This process will allow any number of different footprints to be used for the 
same logic symbol as long

as the pin count is close to being the same. You would need two different logic 
symbols if you have

4 pins on one logic body and 3 on the other.

 

I would not recommend trying to create a 4 pin part, a 8 pin part, a 16 pin 
part as the same logic name.


Shirley in Oregon
It is a PRIVILEGE to be born free. 
    It is a RIGHT to live free. 
        It is a DUTY to die free. 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Ed Caldwell
Sent: Wednesday, October 11, 2006 7:40 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: same symbol - different number of pins

 


William, 

You did not ask... it is only a suggestion (to Cadence) to enhance Allegro. 

As far as I know, Allegro does not allow more than one pin number per pin in a 
footprint. 

The suggested solution is based on my experience with other tools... If two pin 
three's are possible in the footprint (as is with some tools), both common 
footprint pin 3's connect with the single pin 3 in the schematic symbol and in 
your situation, allows you to use the same schematic symbol for the two 
different footprints. 

Hope this helps... I am afraid I am only added confusion... If so, Please 
accept my apology. 
Ed 




"William Billereau" <William.Billereau@xxxxxxx> 
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx 

10/11/2006 10:06 AM 

Please respond to
icu-pcb-forum@xxxxxxxxxxxxx

To

<icu-pcb-forum@xxxxxxxxxxxxx> 

cc

 

Subject

[PCB_FORUM] Re: same symbol - different number of pins

 

 

 




Dear Ed, 
  
If Cadence was able to numbering 1,2,3 for a 3 pins and 1,2,3,4 (and not 
1,2,3,3) for a 4 pins device, it will be fine. 
We already have devices with different number of pins... either in NC_PINS 
section or POWER_PINS... 
So I was just asking for something I was thinking it can be possible. 
  
My english is probably not good enough to understand what you meant with this 
kind of comments.... 
could you explain? 
where did I ask for 1,2,3,3?? 
  
    William. 
  
  
  
  

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Ed Caldwell
Sent: 11 October, 2006 3:08 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: same symbol - different number of pins


Sorry to have submitted what you already knew. Sounds like you have your hands 
full trying to keep up with the EE's! 
If Cadence was able to allow numbering multiple pins the same (i.e. 1,2,3,3) 
your quest would be simpler. Perhaps a future enhancement??? 
Ed 

"William Billereau" <William.Billereau@xxxxxxx> 
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx 

10/11/2006 08:15 AM 

Please respond to
icu-pcb-forum@xxxxxxxxxxxxx

 

To

<icu-pcb-forum@xxxxxxxxxxxxx> 

cc

 

Subject

[PCB_FORUM] Re: same symbol - different number of pins

 

 

 





thanks, but I was just wondering how to avoid this. 
Just to warn schematic designers that by choosing LM1117 they can have 
different types. 
 
(we have a lot of them taking the first thing that "looks like" what they want. 
Then we have to change later for what they purchased....) 
 
If there is no other way I will do it as you suggest. 
 
   William. 
 
 
 

________________________________


From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Ed Caldwell
Sent: 11 October, 2006 1:59 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: same symbol - different number of pins


Make a different schematic symbol for each (part number) with appropriate pin 
counts. 

"William Billereau" <William.Billereau@xxxxxxx> 
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx 

10/11/2006 07:48 AM 

Please respond to
icu-pcb-forum@xxxxxxxxxxxxx

 

To

<icu-pcb-forum@xxxxxxxxxxxxx> 

cc

 

Subject

[PCB_FORUM] same symbol - different number of pins





 

 






Hello All. 

Is there a solution for such component in ConceptHDL: 
LM1117 from National: 

DTX type = TO252 3 pins 
MPX type = SOT223 4 pins . the fourth is the tab that has to be connected to 
OUT pin 2. 

How to do it to: 
-have only one symbol body 
(I think without any "tab" pin. I tried with 2 versions on with the TAB the 
other without. But Add Part only take version 1 by default.) 

-Connect this TAB automatically to pin 2 OUT 
(I tried to add in the parttable to MPX type a PACK_SHORT='(2,4)' but 
unsuccessfully.) 

- Select anyone of both different type in a single parttable.. 

Thanks in advance. 


PS. This case seems to be a common problem. By searching "regulator tab" in 
sourcelink, it returns a case for a MC7805CT2 (or 3). 
http://sourcelink.cadence.com/docs/db/kdb/1998/July/1816165.html 
<http://sourcelink.cadence.com/docs/db/kdb/1998/July/1816165.html>  
but the test2_archive.zip contains only a body with the tab, but selecting a 
new one shows a 3 pin JEDEC and the import logic returns a "incorrect pin 
number". 
So this test2 does not work. 
They speak about a multipin.tar available on ftp.cadence.com 
<ftp://ftp.cadence.com/>  but this FTP site is unaccessible. 
Does anybody get it somewhere? 


=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-= 
| Billereau William | PCB Designer | 
| | Tel: (+4122) 76 73403 | 
| CERN TS/DEM | william.billereau@xxxxxxx | 
| 1211 Geneve 23 Switzerland | Société: AMEC-SPIE/Electrotech | 
=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=

Other related posts: