OrCad Capture

[Vitaliy]

Hello,
I am using OrCAD 10.5 full suite for my school project. I'm fairly new
to it as well. I got stuck with the following problems:
1) From what I read, the schematics and pcb footprint aren't exactly
correlated. I am using Capture CIS. I could not find how to represent
PCB footprint for OPA655 (SOIC) from TI.
http://focus.ti.com/docs/prod/folders/print/opa655.html
In fact, I am not sure what the PCB footprint code for any opamp is. Or
should I use SOG.050/8/WG.something/L.something. I am not sure what 050
in SOG represents, because there are different options (i.e. 025 as
SOG.025), so I do not know which one to use. Also, if I were to use SOG
and
http://focus.ti.com/general/docs/lit/getliterature.tsp?literatureNumber=msoi002c&fileType=pdf
is my opamp, which dimensions am I supposed to match? Chip with the
pins or chip without the pins? Or somewhere in the middle so it is
easier to solder.
2) I am also supposed to use OPA657 (SOIC)
http://focus.ti.com/docs/prod/folders/print/opa657.html. However, there
is no electrical model for it in the libraries. So, I downloaded this
opamp library from TI website. The model looks ugly though with some
pins in the middle of the chip. I can move the pins around, also it
still wouldn't look like an opamp after that. Is there a way to make it
look like opamp, not a rectangle. As far as I understand it wouldn't
matter for Layout.

Thanks,
Vitaliy

 

[Ned Forrester]

Vitaliy wrote:

Hello,
I am using OrCAD 10.5 full suite for my school project. I'm fairly new
to it as well. I got stuck with the following problems:
1) From what I read, the schematics and pcb footprint aren't exactly
correlated. I am using Capture CIS. I could not find how to represent
PCB footprint for OPA655 (SOIC) from TI.
http://focus.ti.com/docs/prod/folders/print/opa655.html

In fact, I am not sure what the PCB footprint code for any opamp is. Or
should I use SOG.050/8/WG.something/L.something. I am not sure what 050
in SOG represents, because there are different options (i.e. 025 as
SOG.025), so I do not know which one to use. Also, if I were to use SOG

The 050 is the pin pitch in mils, .001 inches. The 8 means it has 8
pads for an 8 pin part. WG is the width of the gull-wing leads; be sure
to find a foot print with a larger number here than the TI spec sheet
shows for the maximum width of the part. L is the length of the molded
body of the part; this really only affects the silk-screen, place
outline, etc. of the foot print, so be sure to use foot print with the
same or larger length than the actual part. Note that similar packages
from different vendors can have different dimensions. Foot prints that
have their basic dimensions specified in mm instead of inches, usually
have an "m" in the numbers.

You will be advised by others, and I would second that advice, to learn
to make your own foot prints, or at least to check the Orcad supplied
foot prints carefully against the vendors recommended layout. It is not
that hard. Foot prints are made in the Library Manager of the Layout
package.

I am not sure about CaptureCIS 10.5, I use CaptureCIS 7.2, but the
Capture package needs to know how to find the footprint libraries
(separate from the schematic symbol libraries) in order to display the
foot print when selecting parts from the database. This was/is done by
creating a layout.ini file with the Layout package that contains all the
foot print libraries you want to use, and then copying the layout.ini
file from the Layout installation directory to the Capture installation
directory.

and
http://focus.ti.com/general/docs/lit/getliterature.tsp?literatureNumber=msoi002c&fileType=pdf
is my opamp, which dimensions am I supposed to match? Chip with the
pins or chip without the pins? Or somewhere in the middle so it is
easier to solder.

The pads in the foot print need to extend farther than the maximum
spread of the leads.

2) I am also supposed to use OPA657 (SOIC)
http://focus.ti.com/docs/prod/folders/print/opa657.html. However, there
is no electrical model for it in the libraries. So, I downloaded this
opamp library from TI website. The model looks ugly though with some
pins in the middle of the chip. I can move the pins around, also it
still wouldn't look like an opamp after that. Is there a way to make it
look like opamp, not a rectangle. As far as I understand it wouldn't
matter for Layout.

I am not familiar with that part, so I don't know if it has a standard
8-pin opamp pinout, but you can use any library symbol that looks good
to you and that contains numbered pins for every pin you want connected
on the layout. The only information transfered from the schematic
symbol to the layout is the pin numbering information that is used to
create the netlist. The netlist is what transfers information about the
schematic to Layout. It makes no difference what the name of the symbol
is, so long as the pin numbers match the functions, AND there is a foot
print available that matches the pin numbers to the right physical pins
on the package (SOT-23 and TO-92 packages, amongst others, are often
numbered in conflicting ways by various vendors, so be careful about
this). If you don't like the look of the available symbol, and there is
no standard available, make your own. I rarely use any Orcad supplied
symbols, except for simple things like standard gates and op-amps.

Note that there is other information in the netlist for each part, such
as the name of the footprint to be loaded (but which can be overridden
once the design is in layout), the "value" of the part, the reference
designator, etc.

--
NOTE: to reply, remove all punctuation from email name field

Ned Forrester n_f_orrester@whoi.edu 508-289-2226
Applied Ocean Physics and Engineering Dept.
Oceanographic Systems Lab http://adcp.whoi.edu/
Woods Hole Oceanographic Institution, Woods Hole, MA 02543, USA

 

[Vitaliy]

Hello Ned,
Thank You very much. I found your advices very helpful.
Vitaliy