Thomas,
i tried it with the boolean values "TRUE" and "FALSE" for the fraction
parameter and it worked for me.
If fraction is selected "TRUE" the input_domain parameter has the meaning of
percentage (0.1 means 10%). So the "100" you choose might be a problem too.

Rolf Molitor
Ing.Buero i2e
Remscheid / Germany


-----Ursprüngliche Nachricht-----
Von: "Thomas Josefsson" <[EMAIL PROTECTED]>
An: "Protel EDA Forum" <[EMAIL PROTECTED]>
Gesendet: Dienstag, 1. Oktober 2002 03:01
Betreff: Re: [PEDA] Simulation Function Block, PWLR


> Rolf
>
> Since you have PWL working, I tried it again.
>
> The netlist generation worked without generating any errors, result for
the
> PWL was;
> AU1 AT FLUX AU1PWL
> .MODEL AU1PWL PWL(X_ARRAY=[0 10 20 30 40 50 60 70 80 90 100] Y_ARRAY=[0
> 0.005
> + 0.01 0.025 0.04 0.075 0.125 0.2 0.29 0.38 0.475] input_domain=100
> fraction=1)
>
> The simulation did however stop before it was completed with the following
> error message;
> INPpas2: Invalid code-model syntax or connection
> Error on line 9: au1 at flux au1pwl
> ERROR - model: au1pwl - Bad Boolean value
> Error: circuit not parsed.
>
> What does it mean? What am I missing? Have I given "input_domain" and
> "fraction" wrong values?
>
> Thomas
>
>
> ----- Original Message -----
> From: "Rolf Molitor" <[EMAIL PROTECTED]>
> To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> Sent: Monday, September 30, 2002 3:13 AM
> Subject: Re: [PEDA] Simulation Function Block, PWLR
>
>
> Thomas,
> i did have a look at the devices PWL and PWLR. you mentioned.
> PWL works ok (default as a voltage type). The PWLR (default as a
> differential voltage type) demands a "part type attribute must be a
value",
> but i think its just a protel bug.
> The parameter list of the PWLR includes the %vd(pin1, pin2) statement,
what
> simply means that the differential voltage between pin1 and pin2 should be
> taken as an in- or output parameter. An additional '%' (%%vd) should
prevent
> protel from interpreting the '%v' to insert the part type as a parameter
> here. But it doesn't ! Seems to be a simple protel bug (precompiler does
not
> recognize the '%%vd' but sees a '%v' and wants a value !).
> If you give the part type any legal value (e.g. '1' instaed of 'PWLR') the
> simulation works and the given value has absolutely no influence on the
> result (the netlist contains the '%vd()' statement, protel does not
inserts
> the value of the part type instead of '%v', the compiler itself seems to
> know how to handle '%%vd').
>
> Rolf Molitor
> Ing.Buero i2e
> Remscheid / Germany
>
> -----Urspr ngliche Nachricht-----
> Von: "Thomas Josefsson" <[EMAIL PROTECTED]>
> An: "Protel EDA Forum" <[EMAIL PROTECTED]>
> Gesendet: Sonntag, 29. September 2002 22:27
> Betreff: Re: [PEDA] Simulation Function Block, PWLR
>
>
> > Rolf,
> > I am using a current source to send a current proportional to the total
> > number of ampereturns through a resistor. I am planning to use the
> resistor
> > as an amplification control, but it could be set up differently of
course.
> I
> > connected this function block to measure the voltage across this
resistor.
> > The array values models the flux in a particular magnetic material as a
> > function of the ampereturns.
> >
> > I have not deliberately specified if it is a current or voltage source,
I
> > thought it automatically was a voltage source, but maybe that is a part
of
> > the problem?
> >
> > You can find the model in the Protel component library, got to;
> > http://www.protel.com/resources/libraries/library_search.asp and search
> for
> > Generic Components, Simulation and Function Block. The search should
> return
> > roughly 32 matches on one page. You should find two variants of the
model;
> > PWL and PWLR.
> >
> > I am not sure I understand what you mean with 'part type as a
parameter',
> > could you explain?
> >
> > Thomas
> >
> >
> > handled The output from this
> > ----- Original Message -----
> > From: "Rolf Molitor" <[EMAIL PROTECTED]>
> > To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> > Sent: Friday, September 27, 2002 3:15 AM
> > Subject: Re: [PEDA] Simulation Function Block, PWLR
> >
> >
> > Thomas,
> > but what kind of signal do you want to model with the 'PWLR' ? Is it a
> > voltage like with VPWL or a current as with IPWL (with time/value pairs
as
> > parameters) ? Where can i find this part 'PWLR', where can i find the
> > library you got it from (what .ddb is it in) ? Maybe the 'PWLR' does
take
> > the part type as a parameter (%) ?
> >
> > Rolf Molitor
> > Ing.Buero i2e
> > Remscheid / Germany
> >
> > -----Urspr ngliche Nachricht-----
> > Von: "Thomas Josefsson" <[EMAIL PROTECTED]>
> > An: "Protel EDA Forum" <[EMAIL PROTECTED]>
> > Gesendet: Freitag, 27. September 2002 03:41
> > Betreff: Re: [PEDA] Simulation Function Block, PWLR
> >
> >
> > > I am working with 99. The component seems to be a table with (input)
> > > x-values in one array and (output) y-values in a second array.
> > > The output/input is interpolated to create the correct output from any
> > input
> > > value.
> > > From the model description it seems to be similar to the Simcode model
> > > PWL_TABLE.
> > >
> > > Thomas
> > >
> > > ----- Original Message -----
> > > From: "Rolf Molitor" <[EMAIL PROTECTED]>
> > > To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> > > Sent: Thursday, September 26, 2002 2:56 AM
> > > Subject: Re: [PEDA] Simulation Function Block, PWLR
> > >
> > >
> > > Thomas,
> > > is it DXP or 99SE you are working with ?
> > > Never seen this 'simulation function block' library in 99SE and never
> seen
> > > the component PWLR. Is it a piece-wise linear resistor ? Just know the
> > IPWL
> > > and VPWL sources.
> > >
> > > Rolf Molitor
> > > Ing.Buero i2e
> > > Remscheid / Germany
> > >
> > > -----Urspr ngliche Nachricht-----
> > > Von: "Thomas Josefsson" <[EMAIL PROTECTED]>
> > > An: "Protel EDA Forum" <[EMAIL PROTECTED]>
> > > Gesendet: Donnerstag, 26. September 2002 02:57
> > > Betreff: [PEDA] Simulation Function Block, PWLR
> > >
> > >
> > > >
> > > > I am trying to use the piece-wise linear controlled source from the
> > > > "Simulation Function Block Sch.Lib" to create a non-linear magnetic
> > > circuit
> > > > model.
> > > >
> > > > As a start I hooked the PWLR to a previously verified circuit and
got
> > the
> > > > following error message;
> > > >
> > > > "U1 Error: PART TYPE attribute must be a value."
> > > >
> > > > What value am I supposed to use?
> > > >
> > > > Grateful for a detailed explanation (or a reference to where I can
> find
> > a
> > > > detailed explanation) since I am new to this software package.
> > > >
> > > > Thanks
> > > > Thomas
> > > >
> > > > The Netlist contains the following statement;
> > > >
> > > > AU1 %VD(AT,0) %VD(NETLABEL26,0) AU1PWL
> > > > .MODEL AU1PWL PWL(X_ARRAY=[0 10 20 30 40 50 60 70 80 90 100]
> Y_ARRAY=[0
> > > > 0.005
> > > > + 0.010 0.025 0.040 0.075 0.125 0.2000.290 0.380 0.475]
input_domain=0
> > > > fraction=0)
> > > >
> > > >
> > >
> > >
> >
> >
>
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to