Maker Pro
Maker Pro

Relay footprint with Orcad Layout

Hi everybody,
I have a little problem in assigning a footprint
to a 8 pins relay using "OrCAD Layout".
I have a power relay with 8 pins: 1 for coil1, 1 for coil2, 2 each for
NO, NC and COMON. Lagically speaking this component has 5 connetions
(coil1, coil2, NO, COMMON, NC) but 8 fisical connections.
So I have designed a schematic component with 5 pins and a footprint
with 8 pins.
So here comes the problem:how can I assign 2 padstacks to a same pin?
I am a bit baffled..."Layout" doesn't allow to rename two different
padstacks with the same name or link two pads with a same pin.

Hints?

Reagards,
Alex
 
E

Eeyore

Jan 1, 1970
0
Hi everybody,
I have a little problem in assigning a footprint
to a 8 pins relay using "OrCAD Layout".
I have a power relay with 8 pins: 1 for coil1, 1 for coil2, 2 each for
NO, NC and COMON. Lagically speaking this component has 5 connetions
(coil1, coil2, NO, COMMON, NC) but 8 fisical connections.
So I have designed a schematic component with 5 pins and a footprint
with 8 pins.
So here comes the problem:how can I assign 2 padstacks to a same pin?
I am a bit baffled..."Layout" doesn't allow to rename two different
padstacks with the same name or link two pads with a same pin.

How on earth can you make it a component with 5 pins ? I'd love to see it !

Graham
 
C

Christopher Ott

Jan 1, 1970
0
Eeyore said:
How on earth can you make it a component with 5 pins ? I'd love to see it
!

Graham

I think he means the schematic component has 5 pins due to dropping the
redundant pins for the relay contacts. The Layout part would have all 8
pins.

Personally, I would prefer to see all 8 contacts on the schematic. Makes
troubleshooting easier, and it's less confusing to the software.

However, you could probably make an elongated pad with the named hole on one
end, and place another plated hole in the other end. The second hole would
not carry a net identifier or pin number, but would be electrically
connected. This would have to be in the Layout footprint.

Chris
 
I think he means the schematic component has 5 pins due to dropping the
redundant pins for the relay contacts. The Layout part would have all 8
pins.

Personally, I would prefer to see all 8 contacts on the schematic. Makes
troubleshooting easier, and it's less confusing to the software.

However, you could probably make an elongated pad with the named hole on one
end, and place another plated hole in the other end. The second hole would
not carry a net identifier or pin number, but would be electrically
connected. This would have to be in the Layout footprint.

Chris

Thanks Chris for your answer!
Anyway in the meantime I have discovered a trick to move around the
problem: I have created a herarchical block with two 5 pins each block
(2 of them are shared ) nd then I have used only the first sub-block.
It seems to work.

And thanks also to Graham that probably doesn't know that the world is
full of componentswith 5 pins (e.g. many regulators)
 
S

Spehro Pefhany

Jan 1, 1970
0
On 30 Mar 2007 01:12:52 -0700, the renowned
Hi everybody,
I have a little problem in assigning a footprint
to a 8 pins relay using "OrCAD Layout".
I have a power relay with 8 pins: 1 for coil1, 1 for coil2, 2 each for
NO, NC and COMON. Lagically speaking this component has 5 connetions
(coil1, coil2, NO, COMMON, NC) but 8 fisical connections.
So I have designed a schematic component with 5 pins and a footprint
with 8 pins.
So here comes the problem:how can I assign 2 padstacks to a same pin?
I am a bit baffled..."Layout" doesn't allow to rename two different
padstacks with the same name or link two pads with a same pin.

Hints?

Reagards,
Alex

I think you should show the pins on the schematic with a line between
them on the symbol. You can connect them with traces on your layout,
or not, depending on the requirements.

There's a similar issue with tact switches which have internal jumpers
(4 pins for an SPST-NO switch).
 
Q

qrk

Jan 1, 1970
0
Hi everybody,
I have a little problem in assigning a footprint
to a 8 pins relay using "OrCAD Layout".
I have a power relay with 8 pins: 1 for coil1, 1 for coil2, 2 each for
NO, NC and COMON. Lagically speaking this component has 5 connetions
(coil1, coil2, NO, COMMON, NC) but 8 fisical connections.
So I have designed a schematic component with 5 pins and a footprint
with 8 pins.
So here comes the problem:how can I assign 2 padstacks to a same pin?
I am a bit baffled..."Layout" doesn't allow to rename two different
padstacks with the same name or link two pads with a same pin.

Hints?

Reagards,
Alex

Make the schematic show the part with all the pins. If two pins are in
parallel, show that on the schematic part and connect the two pins
together in the schematic drawing. This is common practice. Would you
make a schematic symbol of an FPGA showing only one ground pin when
the part actually has 78 ground pins? The nice thing about CAD, as
opposed to doing this the old way using tape, your net list from the
schematic is transfered to the PCB layout making wiring errors
non-existant if you remember to perform a DRC. Don't try short-cut the
system because you're too lazy to make a proper schematic symbol! It's
there to help you.
 
V

vasu

Jan 1, 1970
0
I think he means the schematic component has 5 pins due to dropping the
redundant pins for the relay contacts. The Layout part would have all 8
pins.

Personally, I would prefer to see all 8 contacts on the schematic. Makes
troubleshooting easier, and it's less confusing to the software.

However, you could probably make an elongated pad with the named hole on one
end, and place another plated hole in the other end. The second hole would
not carry a net identifier or pin number, but would be electrically
connected. This would have to be in the Layout footprint.

Chris






hi chris

this is vasu . i am learning orcad since one week. i have a problem.
how can i prepare two different padstacks for a single footprint. i
mean in a foot print for example for pin 1 i want a square shaped
padstack and for pin2 if want a round padstack. how can i prepare
these two padstacks and how to save them. please help me i am just
learning orcad.
 
Top