Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source
Hi Rolf. It appears you are correct, the netlister is not doing its job... After a lot of messing around I've come up with a way of fixing the problem which might be of interest to you and others. The simplest way around this is to click on Simulate-Create netlist and then paste the contents of the data file in-between the PWL( ) brackets in the netlist. Leave the *.nsx file open and then run the simulation. A dialog box appears asking if you want to use the open netlist file, we click YES and we're away. A better way is to fix the symbol's read only Field5 netlist description (library field 5) in the Simulation Symbols.lib. Using this solution a few changes have to be made in the way we use a data file: 1. In the File Name part field we have to type the full path to the file. This means we can now store the *.pwl file anywhere we like and not in the same directory as the database file. 2. In the file itself we can't use any comments (*) , only time/value pairs. We must still use the + symbol on new lines of data. 3. The file doesn't have to have a *.pwl extension. Here's how... Open the Sim.dbb, you'll find IPWL and VPWL in the Simulation Symbols.lib. Once you've selected the vpwl or ipwl symbol click on the Description button, a dialog box appears, select the Library Fields tab clear the text in the Text Field 5 text box and type the following... netlist=%D %1 %2 DC %F1 PWL | + ( | %IF(%F4 ) %IF(.INCLUDE %F5) ) %IF(AC %F2 %F3) Click OK, Save and Update Schematics and we're done. You can see the difference in the nsx file. The netlister still doesn't add the data to the netlist, the spice engine does that thanks to the .INCLUDE command If you'd like an explanation of that line of code, let me know I'll be more than happy to post it Alfonso Baz Wollongong Australia - Original Message - From: Rolf Molitor [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Friday, October 04, 2002 8:46 PM Subject: Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source Alfonso, i had the same problem some time ago and i gave up on it. I think i did try everything but couldn't get it working. I think it is a bug. SPICE just knows pwl (time/value ..). If the netlist contains pwl(file=...), SPICE does not know how to handle it. The protel netlister should have inserted the data from the file into the pwl statement, but it doesn't. I once asked Protel about it but never got any answer. Try contacting Altium once again on this matter, just to make sure. Rolf Molitor Ing.Buero i2e Remscheid / Germany -Ursprüngliche Nachricht- Von: Alfonso Baz [EMAIL PROTECTED] An: Protel EDA Forum [EMAIL PROTECTED] Gesendet: Freitag, 4. Oktober 2002 10:36 Betreff: Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source I noticed that the text was missing from my post in the archives so I thought I'd better post this again. I apologise if you guys are getting this twice but just in case... - Original Message - From: Alfonso Baz [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Thursday, October 03, 2002 7:06 AM Subject: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source Hello all In the Protel 99SE schematic editor I've placed a Piecewise Linear Current Source (IPWL) and I've created a file with time/value pairs to use in conjuction with the current source. I believe I've followed all of the instructions and syntax correctly but the simulator still spits out: Error on line 4: i1 neti1_1 0 dc 0 wl( file=h:\electronics\promburner\fipwl.pwl ) No such parameter on this device Protel creates the SPICE netlist ok and if I delete the file from the databases directory or make a mistake in the layout of the *.pwl file protel generates an error while creating the netlist. The problem appears to be that the SPICE engine only accepts paramater pwl (time/value...) and not ( file=...). If I copy the values from the file (256 time/value pairs) and paste them into the netlist it works ok. Is this a bug in the schematic to SPICE netlist genaration or am I missing something? Thanks in advance for any help whatsoever. Alfonso Baz * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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
Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source
Oops!! A couple of mistakes... In the data file you have to start the data with a + symbol and the line I gave is wrong ! this what I wrote earlier netlist=%D %1 %2 DC %F1 PWL | + ( | %IF(%F4 ) %IF(.INCLUDE %F5) ) %IF(AC %F2 %F3) I didn't test it properly... it breaks when you dont use a data file This works for both data file and time/value pairs in the properties box, so long as the data file starts with + netlist=%D %1 %2 DC %F1 PWL | + ( | %IF(+ %F4 ) %IF( .INCLUDE %F5) ) %IF(AC %F2 %F3) the only difference between this one and the broken one is the '+' in front of the %F4 Alfonso Baz Wollongong Australia * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source
I noticed that the text was missing from my post in the archives so I thought I'd better post this again. I apologise if you guys are getting this twice but just in case... - Original Message - From: Alfonso Baz [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Thursday, October 03, 2002 7:06 AM Subject: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source Hello all In the Protel 99SE schematic editor I've placed a Piecewise Linear Current Source (IPWL) and I've created a file with time/value pairs to use in conjuction with the current source. I believe I've followed all of the instructions and syntax correctly but the simulator still spits out: Error on line 4: i1 neti1_1 0 dc 0 wl( file=h:\electronics\promburner\fipwl.pwl ) No such parameter on this device Protel creates the SPICE netlist ok and if I delete the file from the databases directory or make a mistake in the layout of the *.pwl file protel generates an error while creating the netlist. The problem appears to be that the SPICE engine only accepts paramater pwl (time/value...) and not ( file=...). If I copy the values from the file (256 time/value pairs) and paste them into the netlist it works ok. Is this a bug in the schematic to SPICE netlist genaration or am I missing something? Thanks in advance for any help whatsoever. Alfonso Baz * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source
Alfonso, i had the same problem some time ago and i gave up on it. I think i did try everything but couldn't get it working. I think it is a bug. SPICE just knows pwl (time/value ..). If the netlist contains pwl(file=...), SPICE does not know how to handle it. The protel netlister should have inserted the data from the file into the pwl statement, but it doesn't. I once asked Protel about it but never got any answer. Try contacting Altium once again on this matter, just to make sure. Rolf Molitor Ing.Buero i2e Remscheid / Germany -Ursprüngliche Nachricht- Von: Alfonso Baz [EMAIL PROTECTED] An: Protel EDA Forum [EMAIL PROTECTED] Gesendet: Freitag, 4. Oktober 2002 10:36 Betreff: Re: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source I noticed that the text was missing from my post in the archives so I thought I'd better post this again. I apologise if you guys are getting this twice but just in case... - Original Message - From: Alfonso Baz [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Thursday, October 03, 2002 7:06 AM Subject: [PEDA] Protel 99SE Simulator Piecewise Linear Current Source Hello all In the Protel 99SE schematic editor I've placed a Piecewise Linear Current Source (IPWL) and I've created a file with time/value pairs to use in conjuction with the current source. I believe I've followed all of the instructions and syntax correctly but the simulator still spits out: Error on line 4: i1 neti1_1 0 dc 0 wl( file=h:\electronics\promburner\fipwl.pwl ) No such parameter on this device Protel creates the SPICE netlist ok and if I delete the file from the databases directory or make a mistake in the layout of the *.pwl file protel generates an error while creating the netlist. The problem appears to be that the SPICE engine only accepts paramater pwl (time/value...) and not ( file=...). If I copy the values from the file (256 time/value pairs) and paste them into the netlist it works ok. Is this a bug in the schematic to SPICE netlist genaration or am I missing something? Thanks in advance for any help whatsoever. Alfonso Baz * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
