[PCB_FORUM] Re: A question about the placement
- From: Ed Hickey <ehickey@xxxxxxxxxxx>
- To: "icu-pcb-forum@xxxxxxxxxxxxx" <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Fri, 4 Feb 2011 09:25:09 -0800
Sorry, the properties cannot be added to the package symbol.
The ALT_SYMBOLS property, attached to component definitions, comes in through a
device file for third-party tools or the pstchip.dat file for Design Entry HDL.
The property is not directly editable in the PCB Editor.
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of steven7522
Sent: Wednesday, February 02, 2011 7:38 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: A question about the placement
Thanks for your informative answer! I have a further question, are there some
properties I can set when I create a symbol (footprint) in the PCB Editor to
fulfill this goal?
At 2011-02-03 06:01:28，"Ed Hickey" <ehickey@xxxxxxxxxxx> wrote:
Restrict Component Placement Side with Alternate Symbol HARD Property
The ALT_SYMBOLS property, attached to component definitions, comes in through a
device file for third-party tools or the pstchip.dat file for Design Entry HDL.
The property is not directly editable in the PCB Editor. The ALT_SYMBOLS
property lets you specify a list of alternate package symbol names that can use
to substitute the primary package symbol during symbol manipulation. By
default, the symbol defined in the component’s Jedec_type can always be placed
on either the top or the bottom. The presence of the ALT_SYBOLS_HARD property
on the same component overrides this behavior.
Example using Alt_Symbols_Hard = True
Jedec_type = SOIC14
ALT_SYMBOLS = (T:SOIC14, DIP14_3; B:DIP14_3)
ALT_SYMBOLS_HARD = true
In this example, you can place the component on the TOP layer using the SOIC14
and DIP14_3 symbols, but to place a component on the BOTTOM layer, you can only
use the DIP14_3 symbol.
In your case, try this ….
Jedec_type = SOIC14
ALT_SYMBOLS = (B:SOIC14)
ALT_SYMBOLS_HARD = true
SOIC14 can only be placed on the bottom
From:
icu-pcb-forum-bounce@xxxxxxxxxxxxx<mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx>
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx<mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx>]
On Behalf Of steven7522
Sent: Wednesday, February 02, 2011 11:44 AM
To: icu-pcb-forum
Subject: [PCB_FORUM] A question about the placement
I want to restrict a footprint can only be placed on Bottom side. What can I
do? Thanks
Other related posts:
