Continue to Site

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.

net0093 error on orcad pspice

Status
Not open for further replies.

spice

Newbie level 3
Joined
Mar 16, 2006
Messages
3
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,319
no pspice template

hello, currently i''m working on my project. im studying on a circuit and trying to simulate it on orcad capture. im using AD844 cfoas and LM124A opamp in my circuit. i created the model libraries for both components and placed those two files in orcad's default library folder. i draw the circuit on capture and tried to simulate it, but it an error occured, telling that there was an error while creating the netlist. when i look at the session log, it had those warnings and an error message:

WARNING [NET0093] No PSpiceTemplate for C1, ignoring
WARNING [NET0093] No PSpiceTemplate for R5, ignoring
WARNING [NET0093] No PSpiceTemplate for R1, ignoring
WARNING [NET0093] No PSpiceTemplate for C2, ignoring
WARNING [NET0093] No PSpiceTemplate for C3, ignoring
WARNING [NET0093] No PSpiceTemplate for R2, ignoring
WARNING [NET0093] No PSpiceTemplate for R3, ignoring
WARNING [NET0093] No PSpiceTemplate for R4, ignoring
ERROR [NET0075] Unconnected pin, no FLOAT property or FLOAT = e U16 pin '28'
WARNING [NET0093] No PSpiceTemplate for U20A, ignoring


i placed those capacitors and resistors from orcad's model library named "discrete" . and there is an unconnected pin on one of the AD844's (current feedback op amp - CFOA), as it should be so in my circuit diagram.

why does it give those [NET0093] warnings? how can i avoid it? and is it wrong to have an unconnected pin on that opamp?

one more thing, im trying to do a transient analysis. the circuit im working on is a random bit generator thus it has no ac or dc voltage generators. im trying to let the capacitors to have initial voltages, is it possible to perform a transient analysis that way? im sending the circuit file as an attachment. thanks!
 

no pspicetemplate

well
is it wrong to have an unconnected pin on that opamp?


yes , dont leave any unconnected pin in the circuit . it will consider it floating
 

warning: [net0093]

how do you simulate if you do`nt have a pspice template of your circuit ?
 

pspice template

Hey spice!

Don't use the disctrete library for resistors and capacitors for simulation purposes. Use the analog library and choose r and c.
Always choose components from the directory /orcad/library/pspice

Hope this helps
Giri
 

net0093

thanks, that really helped, you are right, discrete library doesnt work.
 

warning [net0093]

Hi,
thx for this response, it help me a lot. But I still have a problem.
I'm using a library TRANSISTOR because I need a 2N3904. But when I clic on create netlist, a box is coming and say WARNING: [NET0093] No PSpiceTemplate for Q2, ignoring

What can I do??

Thx a lot![/b]
 

no pspicetemplate for

There should be a property called Pspice Template on the symbol. The
value should be something like this, X^@[EMAIL PROTECTED]
%LGND %PAD %VCC @[EMAIL PROTECTED]
%LGND %PAD %VCC are the pins of the symbol.
 

While it looks like some of your problems have been fixed by using the appropriate libraries, I wanted to add the following tip to help with your final components (and for anyone else who stumbles on this thread for a similar problem).

When you run into the case where you have to download a PSpice model for a part from the supplier's website, you have a few key steps to follow.

1. Put the model text into a *.lib file, or just change the file extension, so that OrCAD will recognize it.
2. Create a schematic symbol for the part in a Capture library (*.olb). You can create a new library or add the part to an existing library.
3. *DON'T FORGET THIS STEP* After you have created the schematic symbol for the part, you need to select the part and "Associate PSpice Model". This brings up a wizard to help you match the pins from your schematic symbol to the pins in the PSpice model.
4. Now you can place the part into your simulation schematic. (You may need to update your Design Cache, if you've already tried to place it.)

If you forget step 3, you will still get the NET0093 error, even if you have a valid symbol and PSpice model.

I hope this helps!
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top