Pspice CD4000 mixed signal design troubles me :-(

  • Thread starter Klaus Vestergaard Kragelu
  • Start date
K

Klaus Vestergaard Kragelu

Guest
Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice (Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a 5Volt
supply? I first suspected (still do) that somehow it doesn't get the correct
supply and is fed througt protection diodes in the inputs. I have tried
various things with the CD4000_pwr part and setting IPIN(VDD) parameters and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus
 
On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
<klauskvik@hotmail.com> wrote:

Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice (Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a 5Volt
supply? I first suspected (still do) that somehow it doesn't get the correct
supply and is fed througt protection diodes in the inputs. I have tried
various things with the CD4000_pwr part and setting IPIN(VDD) parameters and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus
Click to expand...
Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...
On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice
(Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results
respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a 5Volt
supply? I first suspected (still do) that somehow it doesn't get the
correct
supply and is fed througt protection diodes in the inputs. I have tried
various things with the CD4000_pwr part and setting IPIN(VDD) parameters
and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus


Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.
Click to expand...
Thanks for the suggestion. Just tried that - sorry to say - gives the same
results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing something
like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus
 
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
<klauskvik@hotmail.com> wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...
On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice
(Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results
respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a 5Volt
supply? I first suspected (still do) that somehow it doesn't get the
correct
supply and is fed througt protection diodes in the inputs. I have tried
various things with the CD4000_pwr part and setting IPIN(VDD) parameters
and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus


Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.


Thanks for the suggestion. Just tried that - sorry to say - gives the same
results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing something
like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus
Click to expand...
In the library the values of $G_CD4000_V** should be shown... maybe
it's 2.6V?

A quick search for "*.lib" containing text "$G_CD4000_V" found a
discussion in dig_io.lib that you should read.

Also make sure that the libraries you have loaded don't conflict on
the definition... IIRC the last loaded library dominates.

Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:clduuv8mas2dt5ba0hto2m5ebskgnq6hca@4ax.com...
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...
On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice
(Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results
respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a
5Volt
supply? I first suspected (still do) that somehow it doesn't get the
correct
supply and is fed througt protection diodes in the inputs. I have
tried
various things with the CD4000_pwr part and setting IPIN(VDD)
parameters
and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus


Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.


Thanks for the suggestion. Just tried that - sorry to say - gives the
same
results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing
something
like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus


In the library the values of $G_CD4000_V** should be shown... maybe
it's 2.6V?

A quick search for "*.lib" containing text "$G_CD4000_V" found a
discussion in dig_io.lib that you should read.

Also make sure that the libraries you have loaded don't conflict on
the definition... IIRC the last loaded library dominates.

Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.
Click to expand...
I couldn't find where it said to be defined. But I found the dig_io.lib
file, and that one specified 5.0V

In this file they mention:

Qoute:

The default power supply voltage for TTL (and compatible CMOS) devices
* is 5.0v.
*
* The CD4000 power supply voltage defaults to 5.0v. Its level is
controlled
* by two global parameters CD4000_VDD and CD4000_VSS. To use a different
* power supply voltage, simply define the parameter CD4000_VDD in your
* circuit, which will override the value defined below. For example,
*
* .PARAM CD4000_VDD = 12.0V
*
* will change the default voltage for all CD4000 devices to 12.0v.

Unqoute

So I added ".PARAM CD4000_VDD = 12.0V" to the circuit and now the output
says 6.0V (half supply). Hmmmmmmm - at least that affected the
value............

I think I missing something essential like a digital ground or the
like.......

Cheers

Klaus
 
On Sun, 28 Dec 2003 22:24:38 +0100, "Klaus Vestergaard Kragelund"
<klauskvik@hotmail.com> wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:clduuv8mas2dt5ba0hto2m5ebskgnq6hca@4ax.com...
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...
On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice
(Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results
respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a
5Volt
supply? I first suspected (still do) that somehow it doesn't get the
correct
supply and is fed througt protection diodes in the inputs. I have
tried
various things with the CD4000_pwr part and setting IPIN(VDD)
parameters
and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus


Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.


Thanks for the suggestion. Just tried that - sorry to say - gives the
same
results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing
something
like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus


In the library the values of $G_CD4000_V** should be shown... maybe
it's 2.6V?

A quick search for "*.lib" containing text "$G_CD4000_V" found a
discussion in dig_io.lib that you should read.

Also make sure that the libraries you have loaded don't conflict on
the definition... IIRC the last loaded library dominates.

Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.


I couldn't find where it said to be defined. But I found the dig_io.lib
file, and that one specified 5.0V

In this file they mention:

Qoute:

The default power supply voltage for TTL (and compatible CMOS) devices
* is 5.0v.
*
* The CD4000 power supply voltage defaults to 5.0v. Its level is
controlled
* by two global parameters CD4000_VDD and CD4000_VSS. To use a different
* power supply voltage, simply define the parameter CD4000_VDD in your
* circuit, which will override the value defined below. For example,
*
* .PARAM CD4000_VDD = 12.0V
*
* will change the default voltage for all CD4000 devices to 12.0v.

Unqoute

So I added ".PARAM CD4000_VDD = 12.0V" to the circuit and now the output
says 6.0V (half supply). Hmmmmmmm - at least that affected the
value............

I think I missing something essential like a digital ground or the
like.......

Cheers

Klaus
Click to expand...
It's probably because you're playing Eminem at the same time ;-)

Looking at my schematics of digital things, I still used "AGND"
without problem.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:lpiuuvgnnfc704r0kbujjdrk7i3cl4vq2p@4ax.com...
On Sun, 28 Dec 2003 22:24:38 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:clduuv8mas2dt5ba0hto2m5ebskgnq6hca@4ax.com...
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...
On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

Hi

Ok - so I'm going mad. It's been a long time since I last did
Pspice
(Orcad
Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results
respectively:

http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a
5Volt
supply? I first suspected (still do) that somehow it doesn't get
the
correct
supply and is fed througt protection diodes in the inputs. I have
tried
various things with the CD4000_pwr part and setting IPIN(VDD)
parameters
and
much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus


Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.


Thanks for the suggestion. Just tried that - sorry to say - gives the
same
results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing
something
like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus


In the library the values of $G_CD4000_V** should be shown... maybe
it's 2.6V?

A quick search for "*.lib" containing text "$G_CD4000_V" found a
discussion in dig_io.lib that you should read.

Also make sure that the libraries you have loaded don't conflict on
the definition... IIRC the last loaded library dominates.

Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.


I couldn't find where it said to be defined. But I found the dig_io.lib
file, and that one specified 5.0V

In this file they mention:

Qoute:

The default power supply voltage for TTL (and compatible CMOS) devices
* is 5.0v.
*
* The CD4000 power supply voltage defaults to 5.0v. Its level is
controlled
* by two global parameters CD4000_VDD and CD4000_VSS. To use a
different
* power supply voltage, simply define the parameter CD4000_VDD in your
* circuit, which will override the value defined below. For example,
*
* .PARAM CD4000_VDD = 12.0V
*
* will change the default voltage for all CD4000 devices to 12.0v.

Unqoute

So I added ".PARAM CD4000_VDD = 12.0V" to the circuit and now the output
says 6.0V (half supply). Hmmmmmmm - at least that affected the
value............

I think I missing something essential like a digital ground or the
like.......

Cheers

Klaus


It's probably because you're playing Eminem at the same time ;-)

Looking at my schematics of digital things, I still used "AGND"
without problem.
Click to expand...
I solved it - nothing to do with supplies. An error (or not) in the model.
The 4bit counter has four parallel load inputs to preset the counter. I had
cleared those and never activated the parallel load pin. I had reset the
device so I assumed (assumptions are the mother of all *****ups) the were
cleared. But now I tried loading them with a zero nibble after I released
the reset pin and that did the trick

Thankyou very much for your time :)

Klaus
 
On Sun, 28 Dec 2003 22:44:12 +0100, "Klaus Vestergaard Kragelund"
<klauskvik@hotmail.com> wrote:

[snip]
I solved it - nothing to do with supplies. An error (or not) in the model.
The 4bit counter has four parallel load inputs to preset the counter. I had
cleared those and never activated the parallel load pin. I had reset the
device so I assumed (assumptions are the mother of all *****ups) the were
cleared. But now I tried loading them with a zero nibble after I released
the reset pin and that did the trick

Thankyou very much for your time :)

Klaus
Click to expand...
All problems are simple, just bitchingly obscure ;-)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
On Sun, 28 Dec 2003 15:01:40 -0700, invalid@invalid.invalid said...
On Sun, 28 Dec 2003 22:44:12 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

[snip]
I solved it - nothing to do with supplies. An error (or not) in the model.
The 4bit counter has four parallel load inputs to preset the counter. I had
cleared those and never activated the parallel load pin. I had reset the
device so I assumed (assumptions are the mother of all *****ups) the were
cleared. But now I tried loading them with a zero nibble after I released
the reset pin and that did the trick

Thankyou very much for your time :)

Klaus


All problems are simple, just bitchingly obscure ;-)

...Jim Thompson

Problems are just opportunities, cleverly disuised as
Click to expand...
insurmountable obstacles. -Unknown

--
Best Regards,
Mike
 
On Sun, 28 Dec 2003 13:13:19 -0700, invalid@invalid.invalid said...
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

snip
Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.

...Jim Thompson
Click to expand...
Is he Edmonson Engr., Cadence, or both? Or maybe you mentioned he
knew someone at Cadence.

--
Best Regards,
Mike
 
On Mon, 29 Dec 2003 06:11:08 GMT, Active8
<mTHISREMOVEcolasono@earthlink.net,invalid> wrote:

On Sun, 28 Dec 2003 13:13:19 -0700, invalid@invalid.invalid said...
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

snip
Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.

...Jim Thompson


Is he Edmonson Engr., Cadence, or both? Or maybe you mentioned he
knew someone at Cadence.
Click to expand...
Both.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Klaus Vestergaard Kragelund wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:clduuv8mas2dt5ba0hto2m5ebskgnq6hca@4ax.com...


On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:



"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...


On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:



Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice


(Orcad


Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results


respectively:


http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a


5Volt


supply? I first suspected (still do) that somehow it doesn't get the


correct


supply and is fed througt protection diodes in the inputs. I have


tried


various things with the CD4000_pwr part and setting IPIN(VDD)


parameters


and


much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus



Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.



Thanks for the suggestion. Just tried that - sorry to say - gives the


same


results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing


something


like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus



In the library the values of $G_CD4000_V** should be shown... maybe
it's 2.6V?

A quick search for "*.lib" containing text "$G_CD4000_V" found a
discussion in dig_io.lib that you should read.

Also make sure that the libraries you have loaded don't conflict on
the definition... IIRC the last loaded library dominates.

Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.




I couldn't find where it said to be defined. But I found the dig_io.lib
file, and that one specified 5.0V

In this file they mention:

Qoute:

The default power supply voltage for TTL (and compatible CMOS) devices
* is 5.0v.
*
* The CD4000 power supply voltage defaults to 5.0v. Its level is
controlled
* by two global parameters CD4000_VDD and CD4000_VSS. To use a different
* power supply voltage, simply define the parameter CD4000_VDD in your
* circuit, which will override the value defined below. For example,
*
* .PARAM CD4000_VDD = 12.0V
*
* will change the default voltage for all CD4000 devices to 12.0v.

Unqoute

So I added ".PARAM CD4000_VDD = 12.0V" to the circuit and now the output
says 6.0V (half supply). Hmmmmmmm - at least that affected the
value............

I think I missing something essential like a digital ground or the
like.......

Cheers

Klaus



Klaus,
Click to expand...
The problem was that the output was indeterminate. This translates to
an analog level of half voltage... neither hi nor lo. When you found
that you hadn't initialized the chip, then you found out why the outputs
were indeterminate.

This is one of the problems with simulation, sometimes things that work
on the bench won't work in the sim because things that we take for
granted aren't there. In this case, the output from any gate will be a
definite state, and the logic will resolve itself on the bench. In the
sim, we need to specify everything. People get upset if the sim makes
too many assumptions about digital states... :cool:

Thanks,
Charlie
Edmondson Engineering
Unique Solutions to Unusual Problems

PS. Cadence and most EDA firms do not maintain an official presence on
Usenet. Too easily a magnet for flame wars and other bad things.
Sometimes, you find someone who keeps an eye on things, or tries
occasionally to be helpful, though...
 
"Charles Edmondson" <cedmonds@cadence.com> wrote in message
news:3ff05513$1@news.cadence.com...
Klaus Vestergaard Kragelund wrote:

"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:clduuv8mas2dt5ba0hto2m5ebskgnq6hca@4ax.com...


On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:



"Jim Thompson" <invalid@invalid.invalid> wrote in message
news:q07uuvgjn2tbiei5sir4rjc3meu9roog2m@4ax.com...


On Sun, 28 Dec 2003 18:14:52 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:



Hi

Ok - so I'm going mad. It's been a long time since I last did Pspice


(Orcad


Capture 10.0) mixed analog/digital simulation.

Theese two files show my schematics and the simulation results


respectively:


http://www.microdesign.dk/tmp/sch.jpg
http://www.microdesign.dk/tmp/probe.jpg

Why does the output of the CD4516 counter give only 2.6Volts on a


5Volt


supply? I first suspected (still do) that somehow it doesn't get the


correct


supply and is fed througt protection diodes in the inputs. I have


tried


various things with the CD4000_pwr part and setting IPIN(VDD)


parameters


and


much more. But now I'm stuck....

Anyone see the obvious flaw?

Thanks

Klaus



Your biggest problem is that you are using Capture (gag me with a
spoon :)

Try creating a 5V DC supply. Label plus end as $G_CD4000_VDD and
negative end as $G_CD4000_VSS. See if that makes it work.

Also try making your load resistors larger and see if the levels
increase.



Thanks for the suggestion. Just tried that - sorry to say - gives the


same


results:

www.microdesign.dk/tmp/sch2.jpg
www.microdesign.dk/tmp/probe2.jpg

Can I somehow get what voltage the digital part "see" (by probing


something


like $G_CD4000_VDD or the IPIN(VDD) or something like that?)

Cheers

Klaus



In the library the values of $G_CD4000_V** should be shown... maybe
it's 2.6V?

A quick search for "*.lib" containing text "$G_CD4000_V" found a
discussion in dig_io.lib that you should read.

Also make sure that the libraries you have loaded don't conflict on
the definition... IIRC the last loaded library dominates.

Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.




I couldn't find where it said to be defined. But I found the dig_io.lib
file, and that one specified 5.0V

In this file they mention:

Qoute:

The default power supply voltage for TTL (and compatible CMOS) devices
* is 5.0v.
*
* The CD4000 power supply voltage defaults to 5.0v. Its level is
controlled
* by two global parameters CD4000_VDD and CD4000_VSS. To use a
different
* power supply voltage, simply define the parameter CD4000_VDD in your
* circuit, which will override the value defined below. For example,
*
* .PARAM CD4000_VDD = 12.0V
*
* will change the default voltage for all CD4000 devices to 12.0v.

Unqoute

So I added ".PARAM CD4000_VDD = 12.0V" to the circuit and now the output
says 6.0V (half supply). Hmmmmmmm - at least that affected the
value............

I think I missing something essential like a digital ground or the
like.......

Cheers

Klaus



Klaus,
The problem was that the output was indeterminate. This translates to
an analog level of half voltage... neither hi nor lo. When you found
that you hadn't initialized the chip, then you found out why the outputs
were indeterminate.

This is one of the problems with simulation, sometimes things that work
on the bench won't work in the sim because things that we take for
granted aren't there. In this case, the output from any gate will be a
definite state, and the logic will resolve itself on the bench. In the
sim, we need to specify everything. People get upset if the sim makes
too many assumptions about digital states... :cool:
Click to expand...
Yes, but the thing is the datasheet for the HEF4516
(www.microdesign.dk/tmp/hef4516b.pdf) states:

Qoute "A HIGH on MR resets the counter (O0 to O3 = LOW) independent of all
other input conditions." Unqoute

So I think the model is wrong since if I reset the device the outputs should
go low and NOT indeterminate.

Cheers

Klaus
 
On Mon, 29 Dec 2003 07:48:42 -0700, invalid@invalid.invalid said...
On Mon, 29 Dec 2003 06:11:08 GMT, Active8
mTHISREMOVEcolasono@earthlink.net,invalid> wrote:

On Sun, 28 Dec 2003 13:13:19 -0700, invalid@invalid.invalid said...
On Sun, 28 Dec 2003 20:55:53 +0100, "Klaus Vestergaard Kragelund"
klauskvik@hotmail.com> wrote:

snip
Maybe Charlie Edmondson will weigh in, although Cadence may be closed
until January 5, and he may not follow newsgroups from home.

...Jim Thompson


Is he Edmonson Engr., Cadence, or both? Or maybe you mentioned he
knew someone at Cadence.

Both.

...Jim Thompson

Ah. Moonlighting's cool.
Click to expand...

--
Best Regards,
Mike
 
Happy new year to all.
Don't know if this was solved but in PSpice/Schematics, you could solve this
type of problem by going into Analysis Setup/Digital setup and initialise
flip-flops to 1 or 0.

regards,
John
 
"John" <John.Evans@cern.ch> wrote in message
news:bted6p$2mv$1@sunnews.cern.ch...
Happy new year to all.
Don't know if this was solved but in PSpice/Schematics, you could solve
this
type of problem by going into Analysis Setup/Digital setup and initialise
flip-flops to 1 or 0.

regards,
John
Click to expand...
Thanks for the tip John :)

In Orcad 10 the place to find that is: -> Simulation Settings -> Options ->
Category = Gate Level Simulation

Cheers

Klaus
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top