Connection to unmodeled pin

15 posts / 0 new

Last post

#1 Oct 12, 2016

randress

Offline

Last seen: 7 years 6 months ago

Joined: 2016-10-12 11:24

Connection to unmodeled pin

I am attempting to implement a simple one shot using Orcad Lite17.2. I have tried several ICs including the 74121 and 74LS123. The circuits build with warnings "WARNING(ORNET-1018): Connection to unmodeled pin ...". on the pins where the timing R and C connect.

Thanks,

Randal

#2 Thu, 2016-10-13 02:36

RobertoGb

Offline

Last seen: 5 years 10 months ago

Joined: 2016-05-24 03:10

Hi Randal,

This Warning "Connection to unmodeled pin" means that the pins yor are connecting do not have any modelled behavior. That is why, whatever you connect with such pins will not be considered. Indeed, if you click with Rigth Mouse Button on such component and then select Edit PSpice Model, you will see a description of such model, where it is said that such pins are not implemented.

Many times there are components, which are modeled only for specific ranges, or for specific tasks, that is why it is always recommended to open the PSpice model of such component to see how it could be used und what you would have to consider to use it in a simulation.

Roberto

#3 Thu, 2016-10-13 03:29

randress

Offline

Last seen: 7 years 6 months ago

Joined: 2016-10-12 11:24

Hello Roberto,

Thanks for the reply!

I get it. But it seems strange to me (a pSpice novice) that none of the monostables that I tried (in addition to the 75121 and 54L121, I think I tried the 74LS122) modeled the pins to which the timing C and R were to be connected, eventhough the 'pSpice' icon was displayed when it was selected in the Library.

Perhaps you know of a multivibrator that is more completely modeled. That would save me from having to try each one. Or maybe there is a TI, Fairchild, or other model available. Any further help or suggestions would be appreciated.

-Randal

#4 Thu, 2016-10-13 03:41

RobertoGb

Offline

Last seen: 5 years 10 months ago

Joined: 2016-05-24 03:10

Hello Randal,

Before looking for other solutions, maybe you could send me an image of your circuit. I would like to see how you desgined such circuit, as they have worked in the past at me end. If you have any problem to attach the image, send me an E-Mail to PSpice@flowcad.de

In relation to a multivibrator that is more completely modeled, let me look for it.

#5 Thu, 2016-10-13 11:43 (Reply to #4)

randress

Offline

Last seen: 7 years 6 months ago

Joined: 2016-10-12 11:24

Good evening Roberto,

I have just emailed you a pdf of the 74121 circuit. Pins 9, 10, and 11 give the unimplememted warnings when executed. As I said I have not yet tried all the multivibrators - thought I would as the question first. It is certanly possible that the inadequacy is not with the 74121 model but with me :-)

I will look for your reply here on the forum.

Thanks for looking at this,

-Randal

BTW, can an attachment (pdf) be included in a forum response?

#6 Thu, 2016-10-13 16:58 (Reply to #5)

randress

Offline

Last seen: 7 years 6 months ago

Joined: 2016-10-12 11:24

Roberto/Anyone,

[Roberto]Thanks for telling me how to look at the model code. Good hint. 

I have included the header and subckt call below. As you see, the pulse width is defined by a subckt parameter PULSE. 

I modified the netlist with my desired pulse length but of course when I pressed 'run' it overwrote the netlist. 

Is there another way to add/change the parameter value PULSE so that it persists?

Is there a way to keep 'run' from regenerating the netlist?

Thanks,
Randal


*-------------------------------------------------------------------------
* 74121  Non-retriggerable Monostable Multivibrator w/Schmitt-Trigger Inputs
*
* The TTL Data Book, Vol 2, 1985, TI
* rbh 06/14/91 Created
* rbh 06/02/92 Added dummy R/C pins
*
* Notes:
* 1. The RINT, CEXT, and REXT/CEXT pins are not functional.  The output
*    pulse width, tw(out), is controlled with the PULSE subcircuit 
*    parameter.  Note that this means that the pulse width is FIXED for 
*    the duration of the simulation.  You can specify this value in the 
*    subcircuit call, e.g. X1 ... 74121 PARAMS: PULSE=1us
* 2. Instead of a fixed minimum input pulse width (50ns), this model requires
*    the input pulse to be at least as long as the propagation delay through
*    the device.  Input pulses which are shorter than this value produce 
*    an X which is tw(out) in duration.
*
.subckt 74121 A1 A2 B Q Qbar
+    optional: DPWR=$G_DPWR DGND=$G_DGND
+    params: PULSE=30ns IO_LEVEL=0 MNTYMXDLY=0
*

#7 Thu, 2016-10-13 17:51

randress

Offline

Last seen: 7 years 6 months ago

Joined: 2016-10-12 11:24

Ok. The PULSE parameter is in fact accessible for modification in the model "interface" obtained by left-double-click on the schematic drawing of the 74121. The default value being passed from the netlist by default was VERY small (30ns). I saw what looked like a 'spike' on the output at the trigger time but because of the total simulation time being so large I did not recognize it as a pulse with controlable width.

So, what I take from this, as a pSpice learner, is "when all else fails, read the model header!". Seriously, any help or tutorial information regarding the "unimplemented" warning should include, as you suggested, looking at the model code - at least the comments. We may not all be modelers, but we can all read the comments.

Thanks, Roberto. I think that takes care of my problem with the 74121 and I assume the others that were giving me similar unimplemented warnings.

-Randal

#8 Fri, 2016-10-14 02:45

RobertoGb

Offline

Last seen: 5 years 10 months ago

Joined: 2016-05-24 03:10

Hello Randal,

Thank you very much for the whole information. I am happy that you could understand the behavior of such model as it is implemented. I will notice what you say in order to improve it in the future. Have a nice day!

#9 Sun, 2022-10-02 21:29

jessicausa

Offline

Last seen: 11 months 3 weeks ago

Joined: 2022-10-02 21:22

WARNING(ORNET-1018): Connection to unmodeled pin ... may be due to faulty network connection wordle or your paths are doing it wrong. Please check the network connection and path to see where the error is. getting over it

#10 Thu, 2022-11-24 02:17

celinecdd

Offline

Last seen: 9 months 4 days ago

Joined: 2022-11-23 23:48

I have followed the instructions, but I am still not able to create a working page. Mapquest driving directions Can you help me?

#11 Sun, 2023-03-26 22:16

katyswift468

Offline

Last seen: 5 months 1 week ago

Joined: 2023-03-26 22:13

Whether you're commuting to work, running errands around town, or embarking on a cross-country road trip, mapquest driving directions has you covered

#12 Thu, 2023-06-22 00:38

karausa

Offline

Last seen: 3 months 3 weeks ago

Joined: 2023-06-22 00:34

When you encounter a WARNING (ORNET-1018) then you need to re-establish the battery connection

aa route planner from scratch because this warning indicates you have installed it completely wrong.

#13 Sun, 2023-07-16 21:39

victorpatrick

Offline

Last seen: 3 months 3 weeks ago

Joined: 2023-05-24 04:46

The warnings you are encountering in Orcad Lite 17.2 regarding the unmodeled pins on the timing resistors and capacitors are likely related to the fact that these specific components are not included in the built-in library models of Orcad Lite. As a result, Orcad cannot simulate their behavior accurately. Dave The Diver

#14 Tue, 2023-08-15 07:29

SaintOtis12

Offline

Last seen: 8 months 1 week ago

Joined: 2023-07-04 02:59

I am using version 17.2-2016. is it too old?

Tower Defense

#15 Tue, 2024-03-19 14:41

Phingers2001

Offline

Last seen: 1 month 1 day ago

Joined: 2024-03-19 14:32

I was disappointed that certain components are not included in the built-in library models of Orcad Lite. Currently I work in bail bonds setting up bail payment plans. I like my job but it doesn't pay a well as being a licensed bail agent.