OrCAD problems with floating nodes

Today i use the Orcad for the first time to create a simplest circuit, and a pspice simulation profile. i get every exponents linked on the schematics, then i click "run". but the result is :

ERROR -- Node N00171 is floating
ERROR -- Node N01129 is floating
ERROR -- Node N01044 is floating
ERROR -- Node N01140 is floating

then i check the circuit some times ,but it doesnt works. of course i didn't get any error.

Would you please help me find the problem? thanks!

problems with orcad

may be u used a wrong model for ground
open ground library then source u will find a ground model called zero

orcad capture node floating transformer problem

These errors appear when the Orcad can't calculate the DC point of these nodes I believe .This can be due to a capacitor that blocks DC .

error -- node gnd is floating+orcad

I had this problem too.Every time that you get a message with a floating node then try,by double-clicking to each node of your circuit(since it is very simple) to find which is the node you have problem. After you find it the problem maybe is the connection with the wire!!Delete the exact part, place it again and then reconnect the nodes with wire.If you have problem zoom in to this area to have better view. I hope this to help you

orcad pspice connections floating nodes

I think 2 case most happen for this hint:
1. the ground model is not correct.
2. You don't have retun road, for example, you may use a op+one resistor as a follower, however, you need to add a very large resistor to the non-invertering node and the ground. sometimes you need to parallel a large resistor with the capacitor too.

orcad finding node

Please check this note from Oracad

**broken link removed**

orcad capture error node floating

Thanks!
i tried your suggestions but they dont work. i suspect that the software i installed had some problems. am i right?
maybe i have to try to reinstall the software, is there other way i can try?

Thanks for suggestions!

orcad capture transformer

fryFox said:

Thanks!
i tried your suggestions but they dont work. i suspect that the software i installed had some problems. am i right?
maybe i have to try to reinstall the software, is there other way i can try?

Thanks for suggestions!

Click to expand...

no, is not software problem.

you must have DC-path to ground in every way in you circurit - 1000 GOhm is fine - but you must have it.

open path is example:


middle between cap have not DC-path to ground even i if input and output coupled to ground and spice cannot calculate on it

this case can replace this:


And this way make DC-path to ground (node 0) with near infinitive high resistanse - but DC-path exist and works in Spice calculate.

this problem can also exist together with transformer, optical couplers and transmissions-line (is not lumped component and have time delay between port) etc.


check also at every component is really connected with connection line and not only seems connected in drawing - if rubberband on, try moving component symbol around and see connections following component, or set node number visible and check is only one node number every node. if component have one number in connection point and connected node to component have another - component is not connected to node even if schematic seems perfectly drawing...

missing on above is a typical newbie misstake and all simulator users have do it more than one time...


---

If you not familair with simulator - begin always with simple circurits and simulate and se it working - add more componet, simulate , more component and simulate etc. and this way know ev. find trouble is only related to latest added components.

orcad search node

thx everyone!
i am a freshman, now with your help i get rid of the problems successfully!