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 -----Urspr�ngliche 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/[email protected] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
