0603 wrong package places

[leef_me]

Back in july 2007    elong posted the question about the wrong footprint being placed.

Nestor suggested:

By any chance are you selecting package "Chip-C0603" ?

That is the one that is mapped to the footprint CAPMP7360X360N.

If you are selecting a footprint from Multisim, try:

1. Manufacturer: Generic    Footprint: 0603

2. Manufacturer: Ultiboard   Footprint: C0603

Those two give you a 0603 SMT footprint.

And my question is why isn't the  "Chip-C0603" footprint the correct one? 

Can you explain what the CAPMP7360X360N and therefore the "Chip-C0603" was modeled after?

And also, help me understand how the mapping works, and how to use it properly.

Thanks in advance.

[Tien_P]

In Multisim double click on a component>>Edit Footprint>>Standard Footprint and you will find a Footprint Column on the spreadsheet and this is the footprint name that is shown in Multisim such as 0603.  Also on the spreadsheet there should be a EWB_layout column and the name under this column is used to transfer to Ultiboard, when the EWB_layout column is empty the name under the Footprint column will transfer to Ultiboard.  Circuit Design Suite 10 uses many IPC standard footprints and the IPC name provides the footprint dimension.  A common footprint such as 0603 will have many sizes with IPC standard one reason is base on the type of design you are doing for example if you doing a RF board you will need a different tolerance  pad than you would for a power supply board.    Unfortunately, there are not many people who are aware of the IPC footprint name and if we use IPC name in Multisim many users will not be able to find any footprint and this is why the re-mapping table is there.  If you like more information about IPC standard please visit http://www.pcblibraries.com/ you can download sample software which should give you an idea the format of footprint name.

[leef_me]

Hello Tein P,

Thanks for your reply, and I better understand how/why the mapping works.

>>A common footprint such as 0603 will have many sizes with IPC standard one reason is base on the type of design you
are doing for example if you doing a RF board you will need a different tolerance  pad than you would for a power supply board.  
This a valid point, but it is not pertinent to the discussion.
>>Unfortunately, there are not many people who are aware of the IPC footprint name and if we use IPC name in Multisim many
users will not be able to find any footprint and this is why the re-mapping table is there. 
The problem arises when someone sees C0603 and thinks "there is the 0603 footprint I need for my capacitor", and it should be but it is NOT.

Here is what I observe:

1. The footprint mapping information in the Master Database is <<<<<WRONG  >>>   for the IPC-7351 "Chip-C0603".
The CAPMP7360X360N footprint should NOT be used for this size. In fact. it is also used for Chip-CaseE2.

If you look at the list of available capacitor footprints under the IPC-7351, this one does not follow the pattern of size increases.
Perhaps the footprint should be something like CAP1608X63N, but I don't know the proper dimensions.

2. Based on Multisim version 10.0.343, for a capacitor, your description on how to get to the spreadsheet is incorrect.
The correct method to get there is as follows:

While in a design double-click a capacitor component, select the value tab
click the "edit footprint..." button
click the "select from database" button
the spreadsheet is in the pop-up window that can be resized

3. Two different posters with "National Instruments" in their signatures,
have not addressed the issue that the Master Database is incorrect. And it has been incorrect since at least July of 2007.

Leef_me

[Tien_P]

Hi,

I misinterpreted your question previously; I like to apologize for that.  I double checked Chip-c0603 and you are correct it should not be mapped to the CAPMP7360X360N.   According to my reference any footprint name that starts with CAPMP is a polarized footprint and therefore, it should not be use for the 0603.  The correct footprint to map to is CAPC1608X95N and this footprint is already in the Ultiboard database.  I will ask R&D to fix this problem for the next release.

 

[leef_me]

>>The correct footprint to map to is CAPC1608X95N and this footprint is already in the Ultiboard database. 

>>I will ask R&D to fix this problem for the next release.

>>Tien P.

Very good. It nice to hear that a fix is being requested and what the correct value to use should be.

My apologies to you and to other readers, I did not intend my text to be quite so large. --  in effect yelling

Leef_me