在线咨询
eetop公众号 创芯大讲堂 创芯人才网
切换到宽版

EETOP 创芯网论坛 (原名:电子顶级开发网)

手机号码,快捷登录

手机号码,快捷登录

找回密码

  登录   注册  

快捷导航
搜帖子
查看: 9283|回复: 15

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

[复制链接]
发表于 2019-5-28 10:27:43 | 显示全部楼层 |阅读模式

马上注册,结交更多好友,享用更多功能,让你轻松玩转社区。

您需要 登录 才可以下载或查看,没有账号?注册

x
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!!
发表于 2019-5-29 13:47:19 | 显示全部楼层
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.
发表于 2019-5-29 13:49:47 | 显示全部楼层
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.
 楼主| 发表于 2019-5-29 16:39:13 | 显示全部楼层


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!
QQ截图20190529163503.png
发表于 2019-5-29 20:21:31 | 显示全部楼层
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.
发表于 2019-5-29 22:08:17 | 显示全部楼层


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

 楼主| 发表于 2019-5-30 08:52:27 | 显示全部楼层


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!
 楼主| 发表于 2019-5-30 08:54:02 | 显示全部楼层


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!
发表于 2019-5-30 22:14:19 | 显示全部楼层


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


发表于 2021-5-29 21:32:41 | 显示全部楼层


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

您需要登录后才可以回帖 登录 | 注册

本版积分规则

关闭

站长推荐 上一条 /1 下一条

×

小黑屋| 关于我们| 联系我们| 在线咨询| 隐私声明| EETOP 创芯网
( 京ICP备:10050787号 京公网安备:11010502037710 )

GMT+8, 2024-3-29 02:18 , Processed in 0.032171 second(s), 7 queries , Gzip On, Redis On.

eetop公众号 创芯大讲堂 创芯人才网
快速回复 返回顶部 返回列表