Is there a good tool that will review the contents of Spice macros?

When I try to compile the Spice model for the AD8330, I get the useless 
warning "bad expression statement" in my old version of Tina Pro.  No 
line number is given.  I haven't found anything in the Tina FAQ that 
says what "bad expression statement" might mean, and there are no forums 
for Tina I've come across.

I expect that either the model is wrong or that this old version of Tina 
Pro isn't compatible.

I've looked through the model and don't see any obvious flaws in the 
formatting.

This is just a hobby thing so I don't want to bother the folks at ADI 
about this.  So I will ask you geniuses here:  Is there another tool I 
can use to just check the format of the Spice model?

Thanks,
MW

On Sat, 30 May 2009 21:54:05 -0500, Newsgroups
<H...@stimuluspackage.com> wrote:

>Is there a good tool that will review the contents of Spice macros?
>
>When I try to compile the Spice model for the AD8330, 

What do you mean "compile"?  It's just a text-based subcircuit
declaration.

>I get the useless 
>warning "bad expression statement" in my old version of Tina Pro.  

Did you look at the .OUT file?  (Assuming TINA has such a thing ;-)

>No 
>line number is given.  I haven't found anything in the Tina FAQ that 
>says what "bad expression statement" might mean, and there are no forums 
>for Tina I've come across.
>
>I expect that either the model is wrong or that this old version of Tina 
>Pro isn't compatible.
>
>I've looked through the model and don't see any obvious flaws in the 
>formatting.
>
>This is just a hobby thing so I don't want to bother the folks at ADI 
>about this.  So I will ask you geniuses here:  Is there another tool I 
>can use to just check the format of the Spice model?
>
>Thanks,
>MW
>

I see several E and G sources which have "TABLE", also an E source
with "LIMIT".

The most likely culprit is the "LIMIT".

Review the manual to see what TINA allows as "behavioral".

You'll probably need to re-write the subcircuit declaration in
old-fashioned 2G6 polynomial style.

Surf the web.  I seem to recall a post about a behavioral to
polynomial executable.

                                        ...Jim Thompson
-- 
| James E.Thompson, P.E.                           |    mens     |
| Analog Innovations, Inc.                         |     et      |
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    |
| Phoenix, Arizona  85048    Skype: Contacts Only  |             |
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  |
| E-mail Icon at http://www.analog-innovations.com |    1962     |
             
 I love to cook with wine     Sometimes I even put it in the food

On Sun, 31 May 2009 09:14:26 -0700, Jim Thompson
<T...@My-Web-Site.com> wrote:

>On Sat, 30 May 2009 21:54:05 -0500, Newsgroups
><H...@stimuluspackage.com> wrote:
>
>>Is there a good tool that will review the contents of Spice macros?
>>
>>When I try to compile the Spice model for the AD8330, 
>
>What do you mean "compile"?  It's just a text-based subcircuit
>declaration.
>
>>I get the useless 
>>warning "bad expression statement" in my old version of Tina Pro.  
>
>Did you look at the .OUT file?  (Assuming TINA has such a thing ;-)
>
>>No 
>>line number is given.  I haven't found anything in the Tina FAQ that 
>>says what "bad expression statement" might mean, and there are no forums 
>>for Tina I've come across.
>>
>>I expect that either the model is wrong or that this old version of Tina 
>>Pro isn't compatible.
>>
>>I've looked through the model and don't see any obvious flaws in the 
>>formatting.
>>
>>This is just a hobby thing so I don't want to bother the folks at ADI 
>>about this.  So I will ask you geniuses here:  Is there another tool I 
>>can use to just check the format of the Spice model?
>>
>>Thanks,
>>MW
>>
>
>I see several E and G sources which have "TABLE", also an E source
>with "LIMIT".
>
>The most likely culprit is the "LIMIT".
>
>Review the manual to see what TINA allows as "behavioral".
>
>You'll probably need to re-write the subcircuit declaration in
>old-fashioned 2G6 polynomial style.
>
>Surf the web.  I seem to recall a post about a behavioral to
>polynomial executable.
>
>                                        ...Jim Thompson

Try running you circuit on LTspice. I've had good luck importing
Analog Device parts to LTspice. LTspice is free, compatible with most
of PSpice syntax, and works well.

-- 
Mark

See below:

Jim Thompson wrote:
> On Sat, 30 May 2009 21:54:05 -0500, Newsgroups


> What do you mean "compile"?  It's just a text-based subcircuit
> declaration.

In the Tina Netlist Editor there is an button for "analysis-compile". 
It does some crude checking of the macro listing.

> 
>> I get the useless 
>> warning "bad expression statement" in my old version of Tina Pro.  
> 
> Did you look at the .OUT file?  (Assuming TINA has such a thing ;-)

I didn't find an "OUT" file.  I guess they don't use it.

> I see several E and G sources which have "TABLE", also an E source
> with "LIMIT".
> 
> The most likely culprit is the "LIMIT".

This makes sense.  None of their example macros is as complicated as 
this one.
> 
> Review the manual to see what TINA allows as "behavioral".

Unfortunately they are pretty silent about the details of the Spice 
language they support.

> 
> You'll probably need to re-write the subcircuit declaration in
> old-fashioned 2G6 polynomial style.
> 

This might work.

> Surf the web.  I seem to recall a post about a behavioral to
> polynomial executable.
> 
>                                         ...Jim Thompson

Thanks for the detailed reply!
MW

qrk wrote:

> Try running you circuit on LTspice. I've had good luck importing
> Analog Device parts to LTspice. LTspice is free, compatible with most
> of PSpice syntax, and works well.
> 

Fair enough... I haven't tried LTSpice in a long time so I can't 
remember why I didn't like it.  I know it has a lot of fans.

I was able to get the circuit to simulate in LT Spice.  I am pretty sure 
the AD8830 model is working OK... SLOW... but it is a complex model.

I guess the version of Tina that I have is too old to understand the 
Spice syntax in the AD8330 model, or the Tina guide for using the model 
is too complicated for me to make work.

Thanks for the suggestion!
MW

"Newsgroups" <H...@stimuluspackage.com> schrieb im Newsbeitrag 
news:B9IUl.27855$c...@nlpi065.nbdc.sbc.com...
> qrk wrote:
>
>> Try running you circuit on LTspice. I've had good luck importing
>> Analog Device parts to LTspice. LTspice is free, compatible with most
>> of PSpice syntax, and works well.
>>
>
> Fair enough... I haven't tried LTSpice in a long time so I can't remember 
> why I didn't like it.  I know it has a lot of fans.
>
> I was able to get the circuit to simulate in LT Spice.  I am pretty sure 
> the AD8830 model is working OK... SLOW... but it is a complex model.
>
> I guess the version of Tina that I have is too old to understand the Spice 
> syntax in the AD8330 model, or the Tina guide for using the model is too 
> complicated for me to make work.
>
> Thanks for the suggestion!
> MW

Hello,

You may get it faster with the following options. Be very careful with 
cshunt.
Too much of it lets the circuit wrongly behave.

.options cshunt=1e-16
.options ptrantau=1u

.tran 0 500u 0 100n uic

Best regards,
Helmut 

On Tue, 2 Jun 2009 17:43:06 +0200, "Helmut Sennewald"
<h...@t-online.de> wrote:

>
>"Newsgroups" <H...@stimuluspackage.com> schrieb im Newsbeitrag 
>news:B9IUl.27855$c...@nlpi065.nbdc.sbc.com...
>> qrk wrote:
>>
>>> Try running you circuit on LTspice. I've had good luck importing
>>> Analog Device parts to LTspice. LTspice is free, compatible with most
>>> of PSpice syntax, and works well.
>>>
>>
>> Fair enough... I haven't tried LTSpice in a long time so I can't remember 
>> why I didn't like it.  I know it has a lot of fans.
>>
>> I was able to get the circuit to simulate in LT Spice.  I am pretty sure 
>> the AD8830 model is working OK... SLOW... but it is a complex model.
>>
>> I guess the version of Tina that I have is too old to understand the Spice 
>> syntax in the AD8330 model, or the Tina guide for using the model is too 
>> complicated for me to make work.
>>
>> Thanks for the suggestion!
>> MW
>
>Hello,
>
>You may get it faster with the following options. Be very careful with 
>cshunt.
>Too much of it lets the circuit wrongly behave.
>
>.options cshunt=1e-16
>.options ptrantau=1u
>
>.tran 0 500u 0 100n uic
>
>Best regards,
>Helmut 
>

Hi Helmut,

"cshunt" is pretty obvious, but what does "ptrantau" do?

Thanks!

                                        ...Jim Thompson
-- 
| James E.Thompson, P.E.                           |    mens     |
| Analog Innovations, Inc.                         |     et      |
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    |
| Phoenix, Arizona  85048    Skype: Contacts Only  |             |
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  |
| E-mail Icon at http://www.analog-innovations.com |    1962     |
             
 I love to cook with wine     Sometimes I even put it in the food

"Jim Thompson" <T...@My-Web-Site.com> schrieb im 
Newsbeitrag news:r...@4ax.com...
> On Tue, 2 Jun 2009 17:43:06 +0200, "Helmut Sennewald"
> <h...@t-online.de> wrote:
>
>>
>>"Newsgroups" <H...@stimuluspackage.com> schrieb im Newsbeitrag
>>news:B9IUl.27855$c...@nlpi065.nbdc.sbc.com...
>>> qrk wrote:
>>>
>>>> Try running you circuit on LTspice. I've had good luck importing
>>>> Analog Device parts to LTspice. LTspice is free, compatible with most
>>>> of PSpice syntax, and works well.
>>>>
>>>
>>> Fair enough... I haven't tried LTSpice in a long time so I can't 
>>> remember
>>> why I didn't like it.  I know it has a lot of fans.
>>>
>>> I was able to get the circuit to simulate in LT Spice.  I am pretty sure
>>> the AD8830 model is working OK... SLOW... but it is a complex model.
>>>
>>> I guess the version of Tina that I have is too old to understand the 
>>> Spice
>>> syntax in the AD8330 model, or the Tina guide for using the model is too
>>> complicated for me to make work.
>>>
>>> Thanks for the suggestion!
>>> MW
>>
>>Hello,
>>
>>You may get it faster with the following options. Be very careful with
>>cshunt.
>>Too much of it lets the circuit wrongly behave.
>>
>>.options cshunt=1e-16
>>.options ptrantau=1u
>>
>>.tran 0 500u 0 100n uic
>>
>>Best regards,
>>Helmut
>>
>
> Hi Helmut,
>
> "cshunt" is pretty obvious, but what does "ptrantau" do?
>
> Thanks!
>
>                                        ...Jim Thompson


Hello Jim,

If the DC-solver can't find the operating point, then pseudo-tran is used to
find the operating point.
There is some contol possible for this feature with "ptrantau" and 
"ptranmax".

Best regards,
Helmut

 

On Tue, 2 Jun 2009 18:06:14 +0200, "Helmut Sennewald"
<h...@t-online.de> wrote:

>
>"Jim Thompson" <T...@My-Web-Site.com> schrieb im 
>Newsbeitrag news:r...@4ax.com...
>> On Tue, 2 Jun 2009 17:43:06 +0200, "Helmut Sennewald"
>> <h...@t-online.de> wrote:
>>
>>>
>>>"Newsgroups" <H...@stimuluspackage.com> schrieb im Newsbeitrag
>>>news:B9IUl.27855$c...@nlpi065.nbdc.sbc.com...
>>>> qrk wrote:
>>>>
>>>>> Try running you circuit on LTspice. I've had good luck importing
>>>>> Analog Device parts to LTspice. LTspice is free, compatible with most
>>>>> of PSpice syntax, and works well.
>>>>>
>>>>
>>>> Fair enough... I haven't tried LTSpice in a long time so I can't 
>>>> remember
>>>> why I didn't like it.  I know it has a lot of fans.
>>>>
>>>> I was able to get the circuit to simulate in LT Spice.  I am pretty sure
>>>> the AD8830 model is working OK... SLOW... but it is a complex model.
>>>>
>>>> I guess the version of Tina that I have is too old to understand the 
>>>> Spice
>>>> syntax in the AD8330 model, or the Tina guide for using the model is too
>>>> complicated for me to make work.
>>>>
>>>> Thanks for the suggestion!
>>>> MW
>>>
>>>Hello,
>>>
>>>You may get it faster with the following options. Be very careful with
>>>cshunt.
>>>Too much of it lets the circuit wrongly behave.
>>>
>>>.options cshunt=1e-16
>>>.options ptrantau=1u
>>>
>>>.tran 0 500u 0 100n uic
>>>
>>>Best regards,
>>>Helmut
>>>
>>
>> Hi Helmut,
>>
>> "cshunt" is pretty obvious, but what does "ptrantau" do?
>>
>> Thanks!
>>
>>                                        ...Jim Thompson
>
>
>Hello Jim,
>
>If the DC-solver can't find the operating point, then pseudo-tran is used to
>find the operating point.
>There is some contol possible for this feature with "ptrantau" and 
>"ptranmax".
>
>Best regards,
>Helmut
>
> 
>

Thanks!

                                        ...Jim Thompson
-- 
| James E.Thompson, P.E.                           |    mens     |
| Analog Innovations, Inc.                         |     et      |
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    |
| Phoenix, Arizona  85048    Skype: Contacts Only  |             |
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  |
| E-mail Icon at http://www.analog-innovations.com |    1962     |
             
 I love to cook with wine     Sometimes I even put it in the food

"Newsgroups" <H...@stimuluspackage.com> wrote in message 
news:%amUl.4977$f...@flpi145.ffdc.sbc.com...
> Is there a good tool that will review the contents of Spice macros?
...
> This is just a hobby thing so I don't want to bother the folks at ADI 
> about this.  So I will ask you geniuses here:  Is there another tool I can 
> use to just check the format of the Spice model?

You could try running it through LTSpice, and see if that gives you any 
error or warning messages.

-- Mike --