Back to Forums
1 post / 0 new
#1 Aug 10, 2016
TeamPSpice
Offline
Last seen: 4 months 2 weeks ago
Joined: 2016-03-23 11:50

Incorrect Ground Symbol may Result in Floating Node or Convergence Problems?

 

Error Code

None

Error Message

ERROR (ORPSIM-15141): Less than 2 connections at node

 

ERROR (ORPSIM-15142): Node is floating

 

Definition

 

My circuit does not appear to have any open connections but is resulting in floating node errors.

 

Solution

 

The only valid ground in a PSpice simulation is ground '0'.  Either edit the ground symbol and change the names from GND to 0, or select 'Place > Ground', ensure that the source.olb library is configured from the <CDS_INSTALL_DIR>\Capture\Library\PSpice\Source.olb', which contains the 0 source.

 

If ground 0 is not used, the ground port only names the net with the symbol's name and does not represent a zero reference.  PSpice simulations must have a 0 ground reference in order to resolve initial DC bias calculations.  If any node in the schematic does not have a DC ground 0 reference, a floating node or less than two connections error will result.  Isolation caps may product a floating node error, as the capacitor is considered open when calculating the initial DC bias point calculation.  A large resistor may be place in parallel with the capacitor to help resolve the initial DC bias calculation.

 

Some devices that use subcircuit models may have an internal ground 0 reference.  For example, Opamps, which use a subcircuit model, are typically configured using internal behavioral blocks.  If an incorrect rail voltage is applied because a non-zero ground was used, the internal behavioral blocks may create voltage spikes of several thousand volts.  Otherwise, with an incorrect ground, the Opamp will became self powering and incorrect simulation results may result.

 

Another common problem is the incorrect usage of Power symbols in a schematic.  When placing a power symbol from the 'Place > Power', aside from the $D_HI, $D_LO, and 0 symbols which represent 5v, 0v, and 0v respectively, the other available symbols are just ports and do not supply any voltage.  These symbols only provide connectivity between an actual source and a wire or device pin.  Standard sources used for PSpice simulations can be placed on the schematic in the 'Place > Part' menu from the <CDS_INSTALL_DIR>\Capture\Library\PSpice\Source.olb' library or Sourcstm.olb stimulus library.

Download PSpice and try it for free! Download Free Trial
Cadence