分立元件的Pspice Model怎样转成Spectre能用的Model？？

88王道

1、在做一个功率管（NPN）在片外的LDO；
2、从供应商的网站上只找到了该NPN的Pspice/Spice2/Spice3/Saber Model；
3、现在想将驱动电路及NPN加在一起进行仿真验证；
4、使用Spectre仿真器，怎样将上面4个仿真model（之一）转换成Spectre能用的仿真Model呢？
5、有没有老铁有这方面的经验，传授一下，拜谢！！

david_reg

PSpice Netlist and Device Model Support

Spectre supports PSpice netlist format targeting to include PCB components modeled in PSpice format into a Spectre integrated circuit simulation. This solution does not support PSpice-only designs. The top-level netlist and control statement need to be defined in Spectre, or SPICE format. The recommended approach is to define a subckt in PSpice netlist format and to instantiate the subckt in the Spectre netlist.

You can include a PSpice netlist in Spectre using the following statement.

pspice_include <file> (Spectre format)

.pspice_include <file> (SPICE format)

All content of the included file is required to be in PSpice format. If the file includes files, they are required to be in PSpice format. Elements and device models used in the PSpice netlist are simulated using PSpice default values and equations.

The Spectre PSpice feature does not support digital PSpice elements and PSpice encryption. Spectre encryption is recommended, if encryption is required.

david_reg

SPICE Compatibility

The Virtuoso Spectre circuit simulator parser and elaborator now offers greatly increased capacity. Circuits that previously failed due to insufficient memory are now easily read in by the Spectre circuit simulator. The Spectre circuit simulator also provides SPICE netlist compatibility, eliminating the need for the Spice Pre-Parser (SPP) in your flow.

For migration issues , see Spectre Circuit Simulator Migration Guide.

You can add the +spice option to the spectre command line option:

spectre +spice options inputfile

The +spice option


sets tnom and temp to 25C.

sets parameter inheritance to global rather than the Spectre default of local. This means that global parameter definitions override local ones.

sets flags on files that do not have an .scs extension or those that have sections with simulator lang=spice to be HSPICE compatible. This maps models in the SPICE sections to their Spectre equivalents, but does not modify Spectre files or sections.

enforces .IC statements and initial conditions on elements for DC and OP analyses. By default, Spectre only forces initial conditions if the DC analysis force option is set.
Support for SPICE Netlists

The Spectre circuit simulator can read syntax that is consistent with other commercial SPICE simulators. These features include, but are not limited to.


Hierarchical identifiers
These are used to allow a parasitic device to connect to an internal node of the subcircuit.

Miscellaneous SPICE syntax
Identifiers (instances, nodes, parameters, etc.) can include characters such as #, @ and |.

Multiple namespaces
The same identifier can be used for different types of objects. In the following example,
.param res=1k
res res 0 res
.model res r r=res
res is an instance, node, model, and parameter.

Global nodes
You can now have multiple global statements in a design.

Mixed Spectre and SPICE syntax
You can include both Spectre and SPICE languages in a design, as long as you insert simulator lang switches.

Behavioral primitives
The Spectre circuit simulator supports the SPICE feature that allows a source, resistor, capacitor and/or inductance value to be expressed as a behavioral expression.

Library files and sections
The Spectre circuit simulator supports the .lib card for model inclusion.

Model binning
With the new parser, the Spectre circuit simulator supports the syntax of popular SPICE models, including the syntax that allows you to bin models according to geometry size.

88王道

david_reg 发表于 2019-5-29 13:47
PSpice Netlist and Device Model Support

Spectre supports PSpice netlist format targeting to include ...

1、多谢回复；
2、按照你所给的方法是，可以直接使用Pspice格式的网表用Spectre来进行仿真；
3、我目前的问题是，我只有从官网上下载的PSpice格式的.lib文件，怎样能从这个.lib文件得到一个仿真的symbol？用这个symbol来搭建仿真bench，从而得到仿真的netlist？
谢谢！

david_reg

可以试试调用analogLib里面的npn, 然后在model参数那里填pspice的模型名.

peterlin2010

88王道 发表于 2019-5-29 16:39
1、多谢回复；
2、按照你所给的方法是，可以直接使用Pspice格式的网表用Spectre来进行仿真；
3、我目前的 ...

hspice 可以套, 但是 spectre 的 SCS model 格式跟HSPICE 不同, 你可以 自己改或是   SPECTRE  叫用 spice model , 我记得 spectre 可以用HSPICE  model

88王道

david_reg 发表于 2019-5-29 20:21
可以试试调用analogLib里面的npn, 然后在model参数那里填pspice的模型名.

好的，我试试，多谢！

88王道

peterlin2010 发表于 2019-5-29 22:08
hspice 可以套, 但是 spectre 的 SCS model 格式跟HSPICE 不同, 你可以 自己改或是   SPECTRE  叫用 spic ...

说是在Setup-->Simulation Environment下面可以设定仿真文件，但在IC616这个版本下没有看到有Pspice的设定
我再找找吧，谢了！

peterlin2010

88王道 发表于 2019-5-30 08:54
说是在Setup-->Simulation Environment下面可以设定仿真文件，但在IC616这个版本下没有看到有Pspice的设 ...

spectre有一個內建指令,它可以幾近百分之百包容HSPICE的語法和指令
spectre +csfe filename.sp

==

https://eric0703.pentaxfans.net/2620

HSPICE Netlist 轉換成 Spectre .scs格式
HSPICE Netlist 轉換成 Spectre .scs格式
首先要確認有安裝Cadence IC5.x 軟體
軟體內有spp ，我們是使用spp來做轉檔的

舉例來說:
把一個Inverter Netlist 轉換成 Spectre .scs格式
所以原本的HSPICe netlist 如下

.SUBCKT INV A Y
M0 Y A GND GND n_3p3 l=0.28u w=1.2u
M1 Y A VDD VDD p_3p3 l=0.28u w=1.73u
.ENDS INV

使用轉換指令
spp -convert  INV.scs
檢查一下INV.scs

// .SUBCKT INV A Y
simulator lang=spectre insensitive=yes
global 0 gnd
m0 ( y a gnd gnd ) n_3p3 l=0.28u w=1.2u
m1 ( y a vdd vdd ) p_3p3 l=0.28u w=1.73u
ends inv

如果使用的是新版的MMsim7.2以後的版本，其實就不需要轉netlist了
新版 mmsim已經有支援 HSPICE
模擬指令如下
spectre +hspice INV.sp

===

http://bbs.eetop.cn/thread-297147-1-1.html

1. 你可以使用spectre v7  , 可以直接仿真hspice 网表，就像hspice那样！   输入spectre xx.sp 就可以了，不需要做任何改动！

2. 你只有spectre v5， 使用：  “ spp  -convert < bjt.lib ”把hspice的model  bjt.lib转换成spectre model，结果显示在屏幕上，使用: “ spp -convert <bjt.lib  > bjt.scs ” 把转换的结果写到文件bjt.scs， 最终你可能需要修改bjt.scs中引用文件包含的文件名称才能使用。 spp是cadence自带的命令，可以转换hspice的netlist、model成spectre格式

西决1998

88王道 发表于 2019-5-29 16:39
1、多谢回复；
2、按照你所给的方法是，可以直接使用Pspice格式的网表用Spectre来进行仿真；
3、我目前的 ...

大哥，你这个问题解决了吗，最后这么做的啊，能教教我吗
我发了悬赏，你也可以去回答一下，我把币给你