Orcad Capture/Layout question

[Active8]

Bueno:

Tactile switches. My preferred capture symbol from discrete.olb is

SW TACT-SPST which basically looks like;

-
|
---
1 --o-o o-o-- 2

then there's:

SW TACT-SPST-2

1 - 4
o | o
| --- |
+--o o--+
| |
o o
2 3


created by Andy´s ASCII-Circuit v1.22.310103 Beta www.tech-chat.de

the button looks better, though.

Problemo:

My tact switch is the 4 pin type but I want to use the first
Capture symbol

Notice how the pins numbers ain't gonna cut it? Know how Layout
would balk if the netlist pins don't jibe?

Aside from making a new Capture symbol with perhaps hidden pins (?)
what could I do?

I looked at the 2nd sybol in the parts editor and I don't see a way
to hide pins in "pin properties" or "user properties".

I might just try making a symbol of a switch at 45 deg angle so I
can stick 'em in a matrix, Even then, I'd need to hide pins, I
think. I'd like to know any other workarounds for this. It would be
nice to have the parts placed and have a ratsnest for the manual
route. I can't even copy multiple parts in layout. It just wants to
place one at a time, and with "new", I have to select the footprint
every time. That's bogus, eh?

TIA,
Mike

matrix. this could be a whole capture/layout part. hmm...

| | | |
-|--|--|--|--
|/ |/ |/ |/
-|--|--|--|--
|/ |/ |/ |/
-|--|--|--|--
|/ |/ |/ |/
-|--|--|--|--
|/ |/ |/ |/
| | | |

created by Andy´s ASCII-Circuit v1.22.310103 Beta www.tech-chat.de

 

[Meindert Sprang]

Bueno:

Tactile switches. My preferred capture symbol from discrete.olb is

SW TACT-SPST which basically looks like;

-
|

Problemo:

My tact switch is the 4 pin type but I want to use the first
Capture symbol

No Problemo.

Notice how the pins numbers ain't gonna cut it? Know how Layout
would balk if the netlist pins don't jibe?

No Problemo.

Aside from making a new Capture symbol with perhaps hidden pins (?)
what could I do?

Don't do a thing. Orcad will NOT balk about it, Layout will just leave pins
3 and 4 of your switch footprint unconnected. I have used this myself in a
few designs.
Layout will only complain if the footprint has LESS pins that the schematic
part.

Meindert

 

[Active8]

No Problemo.


No Problemo.


Don't do a thing. Orcad will NOT balk about it, Layout will just leave pins
3 and 4 of your switch footprint unconnected. I have used this myself in a
few designs.
Layout will only complain if the footprint has LESS pins that the schematic
part.

Ah! *That's* what it did to me before. It did work with the 2 pin
Capture part. I did make a diagonal switch, too. I couldn't get the
pins that I wanted to hide without making them invisible power
pins, but now I don't have to. I'll just have to make text notes on
the schem regarding the fact that they're not really 2 pin
switches. Like that really matters.

Works for me.

Hey. I can't remember what I had to do to get update cache and
replace cache to enable in the design menu. I can only get cleanup
cache to enable. Friggin' help files and pdfs are for the birds
sometimes.

Anyone?

tnx,
Mike

 

[Meindert Sprang]

Hey. I can't remember what I had to do to get update cache and
replace cache to enable in the design menu. I can only get cleanup
cache to enable. Friggin' help files and pdfs are for the birds
sometimes.

You have to select the part in the design cache first. Then "Replace Cache"
and "Update Chache" become enabled.

Meindert

 

[Active8]

You have to select the part in the design cache first. Then "Replace Cache"
and "Update Chache" become enabled.

Meindert

Duh. [Kicks self in ass again] which way do i go? So used to
highlighting the design file I thought that was the way when the
other option lit up.

how do you keep Jim Thompson from saying "I told you so" or
something as the computer's in David Letterman free fall from
waaaaay up?

thanks,
Mike

 

[Jim Thompson]

You have to select the part in the design cache first. Then "Replace Cache"
and "Update Chache" become enabled.

Meindert

Duh. [Kicks self in ass again] which way do i go? So used to
highlighting the design file I thought that was the way when the
other option lit up.

how do you keep Jim Thompson from saying "I told you so" or
something as the computer's in David Letterman free fall from
waaaaay up?

thanks,
Mike

I don't use Capture ;-)

...Jim Thompson

 

[Active8]

Hey. I can't remember what I had to do to get update cache and
replace cache to enable in the design menu. I can only get cleanup
cache to enable. Friggin' help files and pdfs are for the birds
sometimes.

You have to select the part in the design cache first. Then "Replace Cache"
and "Update Chache" become enabled.

Meindert

Duh. [Kicks self in ass again] which way do i go? So used to
highlighting the design file I thought that was the way when the
other option lit up.

how do you keep Jim Thompson from saying "I told you so" or
something as the computer's in David Letterman free fall from
waaaaay up?

thanks,
Mike

I don't use Capture ;-)

...Jim Thompson

That was the point. You also didn't have to walk through slushy
half-asses, snowy friggin' bs today either, so go do something
totally unpleasant Or go pick on Win. Yeah. That's the ticket.
Pick on someone your own age.

I feel better now.

Mike

 

[Peter Bennett]

No Problemo.


No Problemo.

Wrong: Problemo.

In the four pin symbol, pins 1 and 2 are the same contact, so the PCB
program would connect to those two pins - switch no work!

I would make a new PCB and/or schematic symbol to suit the new switch.

 

[Meindert Sprang]

Wrong: Problemo.

In the four pin symbol, pins 1 and 2 are the same contact, so the PCB
program would connect to those two pins - switch no work!

I would make a new PCB and/or schematic symbol to suit the new switch.

As I understand it, the OP wants to use the 2 pin symbol in the schematic,
while the PCB symbol has 4 pins. In that case, it IS no problem. And yes, I
tried it first, before I replied to him ;-)

Meindert

 

[Active8]

Wrong: Problemo.

In the four pin symbol, pins 1 and 2 are the same contact, so the PCB
program would connect to those two pins - switch no work!

I would make a new PCB and/or schematic symbol to suit the new switch.

BTDT been there... I wouldn't know which foot print went with a
Mountain Swich .256 tactile PB. So I made the footprint ersta.

Kein problem. Das mas nicht.

Mike

 

[Active8]

As I understand it, the OP wants to use the 2 pin symbol in the schematic,
while the PCB symbol has 4 pins. In that case, it IS no problem. And yes, I
tried it first, before I replied to him ;-)

Meindert

Thanks.
mike

 

[Spehro Pefhany]

Ah! *That's* what it did to me before. It did work with the 2 pin
Capture part. I did make a diagonal switch, too. I couldn't get the
pins that I wanted to hide without making them invisible power
pins, but now I don't have to. I'll just have to make text notes on
the schem regarding the fact that they're not really 2 pin
switches. Like that really matters.

For this same problem, I tried putting shorts between internally
connected pins in the footprint, but that was a BAD idea. I ended up
using a 4-pin footprint with the connections shown on the schematic
symbol because I insist on all 4 pins being connected (and who knows,
I might do a SS layout someday where the jumper effect is useful).


Best regards,
Spehro Pefhany

 

[Active8]

For this same problem, I tried putting shorts between internally
connected pins in the footprint, but that was a BAD idea. I ended up
using a 4-pin footprint with the connections shown on the schematic
symbol because I insist on all 4 pins being connected (and who knows,
I might do a SS layout someday where the jumper effect is useful).


Best regards,
Spehro Pefhany

SS? Super Spehro? SS doesn't do layout. What is SS "jumper effect."

Mike

 

[Spehro Pefhany]

SS? Super Spehro? SS doesn't do layout. What is SS "jumper effect."

Ha. ;-)

Single-sided. You can use the internal connections in the switches as
jumpers to allow a single-sided X-Y matrix switch layout without
having to add real jumpers.

Best regards,
Spehro Pefhany

 

[Active8]

Ha. ;-)

Single-sided. You can use the internal connections in the switches as
jumpers to allow a single-sided X-Y matrix switch layout without
having to add real jumpers.

Best regards,
Spehro Pefhany

Argh! I got a decent route with my 2 terminal switch symbol. I was
manually routing the internally connected pins together and letting
the router do the rest. I'm not going to have plated through holes
right away, so I used route keep-outs to keep traces off the top
layer where I can't solder.

The schematic looks great with the diagonal switches. I wish I
could hide the extra pins somehow. I don't want to make them hidden
power pins 'cause that will foul things up later.

Not sure what to do here. What do you do? The internal connection
in the Capture symbol is *drawn*, but it's not really there.
Connect both pins to the matrix and the router wants to connect
them with a trace.

BRs,
Mike

 

[Spehro Pefhany]

The schematic looks great with the diagonal switches. I wish I
could hide the extra pins somehow. I don't want to make them hidden
power pins 'cause that will foul things up later.

Zero length line, passive?

Not sure what to do here. What do you do? The internal connection
in the Capture symbol is *drawn*, but it's not really there.
Connect both pins to the matrix and the router wants to connect
them with a trace.

BRs,
Mike

Best regards,
Spehro Pefhany

 

[Active8]

Zero length line, passive?

That's what I did. It still shows a terminal circle and then, you'd
still have to have a way for the netlister to know it's connected
to the other pin internally. For some reason, the "Display" button
for display properties isn't enabled and that's how you're supposed
to be able to set the visibility. Power pins are the only ones that
allow the "pin visible" check box to be changed and that's in the
first dialog. The Display button is in the pin user properties
dialog.

I think the only way to use the switch as a jumper is to manually
route it. There's no way to tell the netlister what's going on,
AFAIK. You'd have to decide which common terminal to route out to
the next component and if the pin isn't in the netlist, the router
would try to connect to the one that is. The only way to stop that
is with a keep-out.

I did just manage to place a zero length pin next to pin num 1 name
1 and call it num 1, name 1. I was warned repeatedly when I tried
to close the part editor and then asked to update or discard. I
chose to discard and was repeatedly admonished again for the
duplicate pin. They really do want you to remember not to do that,
I guess.

BRs,
Mike