 |
|||||||||
|
|
|
 |
|
|
|
Below are changes made between WinSpice versions. ***************************** ***************************** ***************************** ***************************** ***************************** ***************************** ***************************** ***************************** ***************************** ***************************** ***************************** 236. Reviewed the M=x parameter for the BSIM3 device versions. The drain current was not being scaled by M because the convoluted calculations ended up cancelling out the M parameter. ***************************** .OPTION MAXORD=1 228. Changed the default value of the DELMIN option from -1 to 1.0e-20. This changes the minimum timestep in a transient analysis from (1e-9*TMAX) to 1.0e-20. This allows many analyses to run that would have once failed. I am still experimenting on the best default value here. The aim is to avoid the dreaded 'Timestep too small' message as much as possible without hitting floating point problems. 229. Added colour to plot printouts and fixed the font which seemed to change on its own. 230. Fixed a bug in the vswitch model. 231. Fixed a crash bug in the plot code caused by having very long command lines. A number of static buffers were made dynamic to fix this. 232. Updated the BSIM4 device to version 4.3.0. 233. Fixed a longstanding problem with the plot command crashing if the first parameter was not a vector. 234. Made BSIM4 device selectable as levels 14 and 54. ***************************** 224. Fixed an infinite loop if an included file doesn't exist. 225. Fixed a parsing problem where a number like +1.0000e-7 would not get handled correctly and give an error. The problem is triggered by the '+' at the beginning of the number. If the '+' was removed, everything was OK. 226. Fixed an expression parsing bug which meant a line like B1 1 0 v=2^9 would result in v(1) being 1 volt instead of 512 volts. ***************************** set temp=50 would set the temperature but this was not being given to the a subsequent analysis. This is a long-running bug in Spice3 which I had fixed for the .option TEMP=50 case some time ago. 219. Added to fix 187 below to also work on G and H sources for compatability with PSpice. 220. Fixed a bug where the TEMP variable in a behavioural expression was being returned in Kelvin, not Centigrade. 221. Fixed a bug where a behavioural expression contained TEMP, TIME or FREQ together with a voltage like v(1), the program would crash. 222. Added support for temperature sweeps with the .TEMP directive. ***************************** R1 1 3 56 TC1=.1 TC2=.4 212. Added support for expressions to define the value of R and C devices e.g. R1 5 7 R=V(1)+100 The expressions allowed are the same as used in the B non-linear dependant sources. If the expressions contain voltages or currents, the voltages and currents are those from the DC operating point. 213. Added a DC convergence aid in addition to GMIN and source stepping. If DC convergence fails, WinSpice will try applying resistive shunts from all nodes to ground and then retries. It starts with a shunt value of 1/gmin and then ramps the shunt resistance down by a factor of 10 then tries again until a shunt value of 1e9 is reached. 214. For PSpice compatability, allow 'RES' to be used for the resistor model type in addition to 'R':- .model <modname> RES(<params>) Likewise allow 'CAP' to be used for the capacitor model type in addition to 'C':- .model <modname> CAP(<params>) 215. Added code to allow Spice2-style resistors to be defined where temperature coefficients are specified in the device instancel ine i.e. R1 1 2 100k TC=.001,.0003 216. Lots of fixes to .param code for better HSpice support. Fixed some problems with recursive definitions. 217. Modified the diode code to use 0.01 ohms as the default value for RS instead of zero. This allow diode circuits to converge where setting RS=0 does not. This change will have little or no affect in small signal conditions (the only condition modelled by Spice anyway) but prevents queries about convergence problems. Of course, RS can be specified as 0 if you want to override this behaviour. An example of a diode circuit which will converge with this change but not without it is:- * Nonconvergent diode circuit ***************************** ***************************** 209. Added support for parameter expression within single quotes as used by HSpice. ***************************** 207. Fixed a problem where {} were being expanded between .control and .endc. This breakes the globbing function in the scripting system. In fact, there is no mention of this feature in the manual & this has been corrected also. ***************************** 205. Fixed the terminal window output to a file using the -o command line option. The output had double carriage return characters in it. ***************************** ***************************** 202. Added a nag message. This message appears if a feature is used that I have implemented over and above the basic Spice3 features. Pressing any key will let WinSpice continue running. Other than the nag screen, all the functions of the program are available whether registered or not. If you only use standard Spice3 features, you won't see the nag message. The message is displayed at most once every 5 seconds. Licensed program users will never see the nag screen. ***************************** 200. Added MOS9 device model ***************************** 198. Increased the iteration limit in the pole-zero analysis. This was preset to 200. Now it is set to 300 and this seems to work better. A .cir file which would not work with 200 iterations works with 300. Ideally, this needs to be a configurable parameter. ***************************** 196. More fixes to parameter passing between subcircuits. ***************************** 194. Fixed some problems with parameter expansion in nested subcircuits. ***************************** 191. Fixed a buffer overflow problem in subcircuit expansion. I wasn't allowing for very large amounts of expansion of input lines caused by subcircuit expansion. I now allow for a 100x size increase! 192. A fix was made to remove (,) from Fxxx lines. This was already done for voltage source lines. ***************************** 187. Modifications to handle lines like F1 1 2 VALUE=<expr> as used by PSpice. 188. Better error handling and display in the source parser. 189. Fixed a crash problem when loading files with very long lines. Caused by a fixed sized buffer in the subcircuit expansion code. ***************************** 183. Fixed a problem caused by expressions within {} like { v(1)-v(2) } Expressions like this cannot use voltages like this because the expression must be fully resolved when the circuit file is read. So it treats v(1) as a non-existant function call. This should have caused an error message, but instead it caused the program to lock up or crash. 184. Fixed a problem with nested curly braces e.g. {{FRED}} would cause an error. 185. Added range checking to the asin() and acos() functions to prevent domain errors for out of range input values. ***************************** 180. More fixes to the subcircuit parameter code. Lots of problems were fixed in the logic used to expand parameter expressions in nested models and subcircuits. 181. Implemented *INCLUDE as used in IsSpice netlists. ***************************** let array[10] = 6 to work properly. 173. Noise analysis output format reverted to its original units (i.e. I have reversed change 99 below). However, if a Spice2 circuit is loaded, any plot or print commands will be adjusted to the units used by Spice2 for compatability. 174. Added support for *DEFINE and PARAMS: in the parameterisation code. 175. The behavioural expression parser used in the B circuit element has been rewritten to allow boolean operators and the condition operator. This allows expressions like:- B3 5 0 V= V(T) < 75 ? 0 : V(T) < 90 ? -5 + V(T) / 15 : 1 to be used. 176. Fixed some quirks in the BSIM1 and BSIM2 devices. Device parameters vbs, vgs and vds were returning initial values only and so these have been renamed to icvbs, icvgs and icvds. Code to return the expected values of vbs, vgs and vds has been added (actually, it was already there but there was no way to get these values - looks like some unfinished work in the original Spice3 code). 177. Changed how memory is allocated again. The Windows API I was using has some limitations one of which is that a maximum of 65535 blocks can be allocated. WinSpice can hit this limit for some circuits reported by several users. 178. Added code to the 'source' command to remove comment lines from the deck before doing much processing. This fixes some problems that had arisen with comments in subcircuits. This removes the need to handle comment lines in all parts of the code which process circuit files. ***************************** ***************************** 168. Fixed a problem where a faulty memory block would be detected if a DC analysis was interrupted & then resumed. 169. Fixed problems with semiconductor resistors and capacitors tripping up the library pre-processor code. 170. Preliminary support for parameterised subcircuits. An example of useage (a bit forced - its just to show you the syntax) is:- Basic RC circuit ***************************** 166. More optimisation to speed up simulation for simulations which generate a large number of output points (like the one in 165). ***************************** 162. Fixed problems reading out junction capacitances with the MOS1, MOS2, MOS3 and MOS6 device models. 163. Fixed a bug in MOS2 and MOS3 devices which caused a miscalculation of CGS after a OP analysis. 164. Fixed a problem where a node name lookup might fail. This was caused by the hash function in inpsymt.c not being case insensitive. ***************************** 160. Added support for handling vi(1,2) etc. ***************************** 153. Fixed DC analysis problem where the last voltage step would not be analysed. 154. Added progress messages for various analyses and the 'spec' command. 155. Fixed problems in the 'listing' command where long lines would not get displayed properly. 156. Improved handling of errors in the 'source' command. 157. Fixed problems with continuation lines in library files. Merging of continuation lines would fail if the library file did not start with a comment. Warning messages were also not getting displayed. 158. Fixed a potential crash problem in library file processing. ***************************** 146. Added support for .global to control node name expansion in subcircuits 147. Added the gd() function to calculate group delay. Also added the deg() and rad() functions for angular conversions. 148. When automatically generating WinSpice commands when loading a Spice2 circuit, WinSpice now adds 'set units=degrees' so that phase plots are in degrees by default. 149. Fixed a problem in BJT noise analysis which could attempt to calculate log(0). 150. Fixed a buffer overflow in the code which writes to the terminal window. 151. Fixed a problem where the an internal array to take the output results could be undersized if the number of output equations in the circuit changed between 2 analyses. The result was that a memory block end overrun would be detected when the circuit storage was freed up e.g when a new circuit was loaded. This problem occurs when a noise analysis is performed after a dc, ac or op analysis because the noise analysis adds an extra output equation to the circuit. This problem will be found in most if not all ports of Spice3. ***************************** 144. Fixed a bug in recognition of the version of the BSIM3 model. ***************************** 141. Added code to allow plot colours to be chosen using 'set colorN=colour' where N can be between 0 and 19. 'colour' is a colour name which can be any of the following:- white color0 is used for the plot background (but this doesn't work yet - its always white) and color1 is the colour used for the grid and text. color2 to color19 are the plot colours. 142. Fixed problems with BSIM1 and MOS2 devices that I accidentally introduced. ***************************** 139. Fixed a crash if <RETURN> was pressed on an empty line. ***************************** 122. A fix has been made to prevent mag() being added to plot expressions after an AC analysis. If mag() or ph() is already used in the expression, WinSpice won't add extra mag() and ph() stuff. For example, if the following was entered to plot the result of an AC analysis:- plot db(mag(((v(11))+(v(3)))*2)) then earlier version of WinSpice would turn this into:- plot db(mag(((mag(v(11)))+(mag(v(3))))*2)) This expansion was added to WinSpice for compatability with Spice2 circuits. However, in this case the user has already used the mag() function so the extra mag() calls are a nuisance. 123. Added support for the '.option scale=x' option to the MOS1, MOS2, MOS3, MOS6, BSIM1, BSIM2, BSIM3 and BSIM4 device models. 124. Fixed a lockup problem which occured when trying to sort arrays of vectors by name. 125. Fixed a problem that occured if a Qxxx line defined NS (substrate node). This caused a spurious error message and would not allow the simulation to run. 126. Fixed a problem where v(x,y) would get expanded to v(x)-v(y). This could give the wrong answer is expressions like v(x,y)*v(a,b) were used. So v(x,y) now get expanded to (V(x)-v(y)). 127. Added missing 'unlet' and 'setscale' commands to the manual. 128. Updated the BSIM3SOI model to v1.3 129. Fixed problems with plotting polar plots. The automatic mag() function was getting in the way again (see item 122 above). 130. Added MOSFET levels 49 (BSIM3). This is the same as selecting level 8. In addition, WinSpice now supports v3.1, v3.2 and v3.2.2 of BSIM3. These can be selected by adding 'VERSION=3.1', 'VERSION=3.2' or 'VERSION=3.2.2' to the .MODEL line. If 'VERSION' is missing, v3.2.2 is assumed. 131. Added the 'rawfile' command. 132. Fixed a problem with the redrawing of plots when the 'vs' keyword is used. The plots were being redrawn with the wrong x-axis. 133. Added the Settings->Font menu to allow the user to pick the font. 134. Correction made to the EKV model to correct the effective channel width calculation to take into account the M parameter. 135. Fixed a problem where in a line like 'b1 1 0 v=v(3,4)' the v(3,4) bit would not be correctly parsed and caused a syntax error message to be displayed. This appears to be a bug I introduced by me a long time ago because the original Spice3f4 code is correct. 136. Fixed a problem where 'save all @q1[ic]' would only save @q1[ic]. Also added the ability to say 'save none'. Vectors in a save command are additive left-to-right so the command 'save none all @q1[ic]' will save all node voltage, all voltage source branch currents and the collector current for Q1. 137. Fixed a problem where the 'run' command would not rerun the previous analysis. ***************************** 114. Fixed a problem where the plot File->Print Setup dialog was not passing settings to the File->Print dialog. 115. Improved memory management when extending vector length during an analysis. This makes the efficiency of the system realloc() routine have a much lower impact on the speed of WinSpice. 116. Fixed a crash problem which occured after a .cir file was editied and WinSpice resimulated the circuit. 117. Added the 'scale=xxx' option to .option lines. This scales dimension parameters in .model lines. Currently, this only works with the EKV MOSFET model. 118. Reinstated the Spice3 minimum timestep limit to prevent floating point faults when simulating non-convergent circuits. This limit can still be diasablted by using '.option delmin=0'. 119. Modified RES and CAP models to be largely compatible with PSPICE. The TC1 and TC2 parameters have been added to the CAP model and TC1, TC2, VC1 and VC2 parameters have been added to the RES model. 120. The SW switch model now takes the VON and VOFF model parameters and also has the alias VSWITCH for compatibility with PSPICE. Likewise, the CSW switch model now takes the ION and IOFF parameters and has the alias ISWITCH for compatability with PSPICE. ***************************** 108. Improved handling of things like v(x,0) etc. Multiple clauses of this form will be expanded to Spice3 form (useful in 'plot' lines). 109. Fixed a bug in bsim3soi model which caused a log() domain error. Checking of log() and exp() calls has been enabled. An error will be displayed giving the file and line number of the caller which will help track down maths errors. 110. Added the EKV v2.6 MOSFET model from Ecole Polytechnique Federale de Lausanne (EPFL). 111. Fixed problem where the POLY() keyword would not be recognised if written in mixed case e.g. pOLY() or Poly() would not be recognised. 112. Added parameter checking to 'tran' command to prevent floating point errors if no parameters are supplied. ***************************** 88. Fixed problems parsing a vector of the form '[ x -y z ... ]' where the numbers in the vector were prefixed with unary minus or plus. 89. Got rid of write-only model device and instance parameters because of problems this causes to the 'alter' command. If a line like alter @vinput[sin]= [ 0 $vain 10e3 ] was used, the parser would attempt to get the value of @vinput[sin]. This caused an error because the 'sin' parameter was flagged as write-only. The reason the parser behaves this way is because it treats assignment as an operator like a C compiler does. Strangely, the original Spice3 code includes provision for reading write-only parameters so it looks like write-only parameters are a more recent modification. However, some models might report an error if they do not contain code to read write-only parameters - let me know if you find one. 90. Removed the 'ic' write-only parameter for the vsrc device from the documentation. There was no code for it anyway. 91. Allowed for the 'sourcepath' variable to be a list or a string. If sourcepath was changed with the set command as follows:- set sourcepath=c:\winspice3\examples then a subsequent 'source astable.cir' would not find astable.cir in c:\winspice3\examples. The problem was caused by the fact that sourcepath is meant to be a list, but setting the string with the command above makes it a string. Either a string or a list is now allowed. 92. Fixed a problem that occurs when a command like 'plot all vs input' is entered where 'input' is the scale. This was causing a memory block to be freed twice. 93. Corrected a problem caused by fix 89 above. Typing 'show all' would cause a GPF. More work is needed to make sure that all input-only parameters can be read back for the 'alter' command. The BJT and BSIM1 models should work. The rest I'll sort out later. 94. Some fixes made to allow the 'alter' command to work properly. A new example 'altertest.cir' tests out the alter command for a BJT model. 95. Fixed a problem with the Windows code which could cause terminal window text to appear to be double spaced. 96. The terminal window size an position is now recorded in wspice3.ini. 97. Fixed a problem discovered with a valve model where WinSpice was being asked to evaluate pow(0, -0.8) or similar. This causes a maths error. To avoid this, I have made WinSpice return 0 for this expression. 98. Added the BSIM4 device. 99. Fixed the noise analysis so that the noise results are in units of V/root Hz instead of V squared/Hz. Anyone used to using Spice2, PSpice and other Spice programs will expect it this way. 100. Added code to handle Spice2 netlists properly when loaded from the source command. This attempts to generate some output by converting Spice2 directives into Spice3 commands and then execute them. If the input circuit contains .control or an Spice3 commands, no attempt is made to do this conversion - the circuit is loaded as in earlier versions of WinSpice. 101. Fixed a problem with batch mode operation when winspice was started with the -b option. The program would generate a page fault after running the simulations. 102. A minor change was made so that when a vector is looked up e.g. after a print or plot command, the vector would be searched for in all plot lists until found. Previously, the vector would only be looked up in the current plot. This was awkward for the noise command which generates two plot lists and sets the current plot to integrated noise results. This meant that 'plot onoise_spectrum' would not work after a noise analysis and was causing some confusion. 103. For easier compatibility with Spice2, using 'plot onoise' after a noise analysis is equivalent to 'plot onoise_spectrum'. Likewise, 'plot inoise' is equivalent to 'plot inoise_spectrum'. 104. Code modified so that for every circuit line read in by WinSpice is associated the original filename and line number. If an error or warning is generated when the circuit is loaded, the filename and line number is also displayed. 105. The 'listing' command now shows the filename and line numbers relating to the original source files together with any errors or warnings found when the circuit was loaded. Previous versions of WinSpice would cause lines to be renumbered destroying any chance of tracking down a problem to a line in the circuit. 106. Added code parsing code for diodes, voltage sources and current sources to detect if they have been shorted out and display a useful warning message. In each case, the shortage component is not loaded into the circuit. ***************************** 77. Fixed any command which takes a filename to handle a quoted filename. This is needed to cope with long filenames which contain spaces. Also, removed treatment of '\' in a string as an escape character to prevent the mangling of file paths. 78. Added the 'cross' and 'strcmp' commands to the manual. 79. Fixed a problem where using x^y in dependent voltage and current source expressions could cause a floating point exception. This was caused by trying to take the log of zero under some circumstances. Fixed by substituting 1e-30 if zero is supplied as a parameter. 80. Improved the command line to include editing and history using cursor keys like doskey. 81. Improved formatting of the output of the 'print' command 82. Added the sum() vector function to calculate the sum of all elements of a vector. 83. Fixed a problem where ticmarks would not get redrawn on a plot window when it was resized. 84. Fixed a problem where the transient analysis maximum step size was getting set up incorrectly if the TMAX parameter to 'tran' or '.tran' was omitted. The code now agrees with the user manual in that it now sets the maximum step size to min(TSTEP, (TSTOP-TSTART)/50). 85. Implemented the '.option rshunt=x' option. This places a resistor between all voltage nodes and ground. This greatly helps the majority of circuits to simulate properly, particularly if the user is not aware of the quirks of standard Spice. By default, rshunt is inactive. It can be enabled by using '.option rshunt=1e9' to set the shunt resistor value (100Meg in this case). 86. Lots of fixes to reduce memory leakage as the program runs. The program still leaks memory, but at a much, much lower rate now. Use the 'destroy all' command to discard old simulation results and conserve memory. ***************************** 75. Fixed numerical overflow problems with the BSIM1 model caused by a complete lack of code to limit the values passed to the exp() function. During simulation, input values could exceed the maximum value allowed by exp(). ***************************** alter r1 = 10k This was caused by another 'improvement' to improve the error message from incorrect use of the 'alter' command. 72. Corrected a bug introduced when making change 53 below. If the x-axis of a plot was decreasing, no plot line would be drawn. 73. Looking into BSIM1 maths error problems. Seems to be endemic to the BSIM1 code. ***************************** 51. Fixed a problem with the asciiplot command which occured if the plot title was longer than about 80 characters. Some integer maths was getting evaluated to a negative value but was being evaluated as a very large unsigned value. This caused up to 2 billion spaces to be printed to centre the title on the page! 52. Corrected problem with pointplot plots where the plot window was not being redrawn properly. 53. Fixed a problem where 'flyback' would be seen on a plot if drawn using DC analysis which uses multiple sources e.g. to draw a transistor charactersitics. The resultant plot contains multiple curves but, when the plot was redrawn, the end of one curve was being connected to the start of the next resulting in linking up of the plots. 54. Improved plot window redraw speeds by exiting early if zero length lines are being drawn which could occur if closely spaced points are being drawn. 55. Fixed an occasional fatal error of the form 'txfree(): bad block signature'. This occured when a circuit structure was being freed up. 56. Fixed a problem with binary rawfile output using the 'write' command. It turned out that the rawfile could not be read back without getting an error message. 57. The 'help listing' command now shows all the possible listing possibilities. The [expand] option was missing. 58. Changed subcircuit expansion so that the expanded names now include the subcircuit reference. 59. Added support for vbe(), vce(), vb(), vc(), ve() in .plot lines etc. These expand to use the q?#base, q?#collector and q?#emitter output vectors, but these are currently voltages inside the BJT model, not terminal voltages as you might expect. I will try to fix this anomaly soon. 60. Fixed a problem with the 'sens' command when doing AC sensitivity. A parsing error was preventing the command from working. A new example .cir file (sens.cir) which illustrates sensitivity analysis has been added to the examples directory. 61. Disabled redirection for 'define' commands. The '>' and '<' characters can now be used in user defined function without problems (see sens.cir). 62. Added experimental recording of branch currents for resistors and capacitors. This can be enabled by adding the line .option resbranch capbranch to your circuit. With branch currents enabled, capacitors are now replaced by 100gigohm resistors during operating point analysis. This might help some circuits work properly and probably more accurately simulates a real capacitor. Be aware that with branch currents enabled, some adjustments may be needed to get the circuit to converge. 63. Fixed problems with the .lib command and nested subcircuits (thanks to Fridger Schrempp). Another problem where the wrong subcircuit could get extracted from a library was also fixed (thanks to Fridger Schrempp again for highlighting the problem). 64. More fixes to the alter command. This now correctly accepts all three formats. 65. Removed spurious "Warning: vec_free: plot ptr is 0" message that sometimes occurred. 66. Fixed a problem where iplots could not be zoomed because the command line stored with the plot was incorrect. 67. More fixes to cope with filenames containing space characters in .include or .lib lines. 68. Modifications made to allow vectors to be defined in 'let' and 'alter' commands using the form '[ x y z ]' e.g. 'let params = [ 1 0.15 2.6 ]' which defines a three element vector. The standard Spice3 manual says this is possible, but I can't see that it was ever implemented. It is now (well in WinSpice it is!). 69. Fixed problems with writing lines like let rindex[index] = 23 which used to give an error message like 'left-hand expression is too small (need xx)'. The code seems to imply that 'let' can only assign a complete vector instead of only a few values in a vector at a specified index, but I can't see why so it has been fixed. A case of clutching defeat from the jaws of victory - the original Spice authors seem to have broken working code here. 70. Reduced memory leakage during subcircuit expansion. ***************************** 46. Fixed a problem with sensitivity analysis where a 'txfree(): Bad block signature' message could be displayed. 47. Added support for writing comma-separated files using the 'write' command. If a filename is given and it has the .csv extension, plot data is written to the file in comma-separated format so that it can be imported into a spreadsheet. 48. Fixed a problem with the 'alter' command not recognising model or device parameters. 49. Updated the BSIM3 model to v3.2.2 and added in our fixes. ***************************** 38. Fixed a problem introduced by me during recent changes. Basically, the 'print all' command was not working properly. This now works as in earlier versions. 39. Corrected incorrect code for the deriv() function which was causing GPFs. 40. Added zooming to graph windows. Click and drag to select a region of a graph and a new plot will be drawn when the button is released. 41. Fixed a crash which could occur when reading in zero-length include files. 42. Fixed a problem with opening spinit if WinSpice was installed in a directory with a space character in the path e.g. "c:\Program Files\winspice". 43. Fixed some typos in the tutorial document. 44. Fixed problem where a quoted string in a command would cause WinSpice to lock up. A command like:- cd "elmer fudd" or cd 'elmer fudd' will now work properly. ***************************** 21. Fixed a problem with the library code which was causing spurious, apparently random crashes when a circuit was loaded. WinSpice now seems much more reliable. 22. Fixed a problem with the alter command which could crash if the '=' character was omitted e.g. with a line like 'alter r1 10k'. The alter command now works with and without the '=' character i.e. 'alter r1 10k' and 'alter r1=10k' now work. 23. A compatibility problem with some Spice2 opamp macromodels has been fixed. Basically, lines like GO1 45 99 (99,40) 4E-3 cause a problem because Spice2 allows a pair of node numbers to be grouped with '(,)'. Spice2 ignores these characters and treats this line the same as GO1 45 99 99 40 4E-3 WinSpice now also ignores these characters (in fact it replaces them with spaces when the circuit is loaded). 24. Added code to comment out any lines beginning with '.view'. This is an option specific to Intusoft version of Spice3. However, this modification was made so that the free SpiceNet schematic editor program given away by Intusoft (http://www.intusoft.com). When SpiceNet saves a schematic, it also saves a .cir file. Now, if you open this .cir file with WinSpice, you can simulate the schematic by just saving it. WinSpice will reload the circuit file. Make sure the you add the user command '*#run' to your circuit. 25. Fixed the 'save' command so it now saves vectors with names like 'v(1)' properly. Previously, vectors with names containing '(' would not get saved (this bug is in the original Spice3f4 sources). 26. Got the 'iplot' to work properly, partially fixed by item 25 above. Also updated the manual because the original manual did not explain that iplot's are a sort of visual trace and show up under the 'status' command and can be deleted with the 'delete' command. 27. Fixed some problems with temperature handling. Some of the basic models like BSIM1 and BSIM2 seem to be implemented incorrectly here. 28. Fixed a problem with transient analyses. The original Berkeley code was imposing a minimum limit to the time delta using the undocumented formula 1e-9*TMAX (see the User Guide in the section describing .TRAN for the meaning of TMAX). If a transient analysis hits this limit, a 'Timestep too short' message was being printed but with no guidance given as to how to fix the problem. Removing a check for this limit seems to make some circuits work properly with no apparent ill effects. 29. Lots of memory leaks fixed, although there are some left. This was partly done by adding a new variable to control the number of circuits stored by WinSpice3. Every time a new circuit is loaded, if the number of in-memory circuits exceeds the value of 'maxcircuits', the oldest circuit is deleted. The value of 'maxcircuits' defaults to 1 which helps limit memory usage. 30. Printer menu items for plot windows now work properly and use standard dialog boxes. 31. 'help' command with no parameter now gives some useful hints (this form of 'help' command is in the original Berkeley sources but it was not being used). 32. Updated the BSIM3 device model to v3.2. 33. Fixed the history command list. This was being screwed up by some dodgy code from the original Spice3 code. 34. Another correction to the POLY expansion stuff to handle coefficients like '1.9M' which were not being converted to the form of number expected by Spice3 i.e. 1.9e-3. This now give better compatibility with Spice2 models that can be found on the internet. 35. More memory leaks fixed, particularly in the command line code. Spice was pointlessly saving all commands entered from the terminal window on a linked list. It now only does this if a foreach, dowhile or while command is being entered and the commands are freed when 'end' terminates these composite commands. 36. Fixed a problem where the 'show' command would not redirect to a file. Possibly more of these are lurking. ***************************** 16. The BSIM3 and BSIM3SOI models now work. 17. Fixed a problem with parsing the .cir file when looking for POLY directives to expand. The POLY directives were not getting expanded. 18. Plot windows and the terminal window now have menus. Circuits can be loaded and run using the 'File'/'Open' menu sequence in the terminal window. 19. Editorial changes to the User Manual have been made. Added a description of program installation and use at the head of the document. Removed all references to command completion. ***************************** 9. WinSpice3 includes the BSIM3 and BSIM3SOI models. Problem is, they don't work yet so don't bother trying. The drain-source current always comes out as zero when I run the supplied tests - anyone have any ideas? 10. Plot windows and the terminal window can now be resized by dragging the borders. 11. WinSpice2 includes a new level 2 JFET model (also by Anthony Parker, anthonyp@sr.hp.com). Again, no details in the User Guide yet. 12. WinSpice3 no longer hogs the processor when waiting for keyboard input (thanks to Horacio Gonzalez for pointing this out). 13. The 'cd' command no longer crashes if typed on its own (thanks to Sparc Han for reporting this). It now displays the current directory. 14. The plot windows now have a print option on the system menu (click the top left corner of the window. The Print Setup option still doesn't work though. ***************************** 2. This port fixes lots of severe memory management problems which existed in the original code. These cause lots of crashes when I first compiled the code. It now seems quite stable. 3. The scripting language (based on the Unix C-Shell) now works as advertised. The original Berkeley code contained a fundamental error, duplicated about 100 times in the code, which meant that this feature does not work on most, if not all ports of Spice3. However, scripts now work as advertised in the documentation. 4. I have added support for the POLY statement from Spice2 so that many device models from Spice2 and PSpice, particularly opamp macro models, can still be used. POLY has been replaced by an expression in Spice3 so what happens is that in WinSpice3 the POLY statements are expanded to a Spice3 expression before the circuit is analysed. 5. I have added support for libraries of concatenated models as used by PSpice. This is done by using the .lib directive in the .cir files. WinSpice3 searches for any unresolved models in the file specified on the .lib file and extract the required model lines before the circuit is analysed. 6. A separate pre-processor, capable of performing model library searches and POLY statement expansion is also provided (spicepp.exe). This program is essentially embedded in the WinSpice3 executable. However, having a separate pre-processor is handy sometimes. 7. There are loads of demo circuits in the examples directory. Some illustrate the use of the scripting language to perform quite complex tasks with very little effort (see examples\bjt.cir forexample).
|
|
|
|
[WinSpice Home] [News] [FAQ] [Purchase] [Forum] [Links] [Change Log] [Contact Us] |