Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Integrate PSpice netlist in OrCAD

Status
Not open for further replies.

pavel47

Member level 4
Joined
Nov 8, 2005
Messages
68
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Location
Switzerland
Activity points
1,790
Hello,

How to integrate PSpice netlist in OrCAD schematic.
I've tried 2 appoaches:

  • using Hierarchical block
  • using Library part

In both cases I failed: via hierachical block ... the port name exposed in netlist subcircuit don't appear in schematic, 2nd approach solicits Model Editor, where there is no option for .SUBCKT-type models (at least I didn't find how to do it), only templates such as diodes, bipoalires, opamps, etc.

My netlist is generated by 3rd-part tool and doesn't match any template, proposed by Model Editor.

How to proceed.

Thanks in advance.

Pavel.
 

mvaseem

Full Member level 2
Joined
Dec 22, 2009
Messages
144
Helped
64
Reputation
128
Reaction score
63
Trophy points
1,308
Location
India
Activity points
2,081
You have a netlist in subckt format.
The way to go is launcj model editor. Open the netlist in model editor. The file extension should be .lib. (Example netlist.lib)
Do File -> Export capture part library.
This would generate capture symbol (olb file) for the netlist model. The symbol ports would be same as subckt ports in netlist.
Use this symbol for simulation.
 

pavel47

Member level 4
Joined
Nov 8, 2005
Messages
68
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Location
Switzerland
Activity points
1,790
Thanks, it works.
Once more question: in the Implementation Type of Hierarchical Block there is option "PSpice Model".
What this option stands for and how it can be used ?
 

mvaseem

Full Member level 2
Joined
Dec 22, 2009
Messages
144
Helped
64
Reputation
128
Reaction score
63
Trophy points
1,308
Location
India
Activity points
2,081
The value "Pspice Model" should be there on a primitive and not hierarchical block.
If you have generated part using model editor, that would also be called a primitive.
Hierarchical block is something which can be descended into.
This property tells pspice netlister that the part is a pspice part and it should be netlisted for simulation flow.
 

pavel47

Member level 4
Joined
Nov 8, 2005
Messages
68
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Location
Switzerland
Activity points
1,790
The value "Pspice Model" should be there on a primitive and not hierarchical block.
Is there some methode/technique allowing to assciate pspice netlist with a hierarchical block ?
Or only possibility for using netlists - include them in some library .lib, that has the same name as .olb (from where symbols are put on schematics) ?

Sincerely
 

mvaseem

Full Member level 2
Joined
Dec 22, 2009
Messages
144
Helped
64
Reputation
128
Reaction score
63
Trophy points
1,308
Location
India
Activity points
2,081
You can use any part (not hierarchical block) to associate a subckt provided the following -

The part has same number of pins as the subckt.
The property called IMPLEMENTATION on part should have same value as subckt name.
The property called PSPICETEMPLATE has the port order defined. You can manually define the port order to be used by netlister.

Look at a case where you have already generated part using model editor. You'll get more clarity.
 

pavel47

Member level 4
Joined
Nov 8, 2005
Messages
68
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Location
Switzerland
Activity points
1,790
You can use any part (not hierarchical block) to associate a subckt provided the following -

The part has same number of pins as the subckt.
The property called IMPLEMENTATION on part should have same value as subckt name.
The property called PSPICETEMPLATE has the port order defined. You can manually define the port order to be used by netlister.

Look at a case where you have already generated part using model editor. You'll get more clarity.

Ok, thanks
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top