+ Post New Thread
Results 1 to 7 of 7
  1. #1
    Junior Member level 1
    Points: 341, Level: 3

    Join Date
    Jun 2015
    Posts
    15
    Helped
    0 / 0
    Points
    341
    Level
    3

    "Less than 2 connections at node" error message in pspice

    Hi everybody. I have redesign a scheme I was using and was very successful. But when I tried to simulate a DC sweep, I got this error message (Pspice 9, student version):


    Code dot - [expand]
    1
    2
    3
    4
    5
    6
    7
    8
    9
    10
    11
    12
    13
    14
    15
    16
    17
    18
    19
    20
    21
    22
    23
    24
    25
    26
    27
    28
    29
    30
    31
    32
    33
    34
    35
    36
    37
    38
    39
    40
    41
    42
    43
    44
    45
    46
    47
    48
    49
    50
    51
    52
    53
    54
    55
    56
    57
    58
    59
    60
    61
    62
    63
    64
    65
    
    **** 01/14/16 12:47:12 *********** Evaluation PSpice (Nov 1999) **************
     
     * C:\Program Files\OrCAD_Demo\PSpice\Diodo MT 2.sch
     
     
     ****     CIRCUIT DESCRIPTION
     
     
    ******************************************************************************
     
     
     
     
    * Schematics Version 9.1 - Web Update 1
    * Thu Jan 14 12:47:12 2016
     
     
     
    ** Analysis setup **
    .DC LIN V_V9 -0.04 0.04 0.00001 
    .OP 
     
     
    * From [PSPICE NETLIST] section of pspiceev.ini:
    .lib "nom.lib"
     
    .INC "Diodo MT 2.net"
     
    **** INCLUDING "Diodo MT 2.net" ****
    * Schematics Netlist *
     
     
     
    L_L4         GCL 0  10uH  
    C_C3         GCL 0  1n  
    G_G2         GCL 0 VALUE { V(RG, 0) }
    R_R6         fteR RG  1k  
    V_V9         fteR 0 1mV
     
    **** RESUMING "Diodo MT 2.cir" ****
    .INC "Diodo MT 2.als"
     
     
     
    **** INCLUDING "Diodo MT 2.als" ****
    * Schematics Aliases *
     
    .ALIASES
    L_L4            L4(1=GCL 2=0 )
    C_C3            C3(1=GCL 2=0 )
    G_G2            G2(OUT+=GCL OUT-=0 IN+=RG IN-=0 )
    R_R6            R6(1=fteR 2=RG )
    V_V9            V9(+=fteR -=0 )
    _    _(GCL=GCL)
    _    _(gnd=0)
    _    _(RG=RG)
    _    _(fteR=fteR)
    .ENDALIASES
     
     
    **** RESUMING "Diodo MT 2.cir" ****
    .probe
     
     
    .END

    ERROR -- Less than 2 connections at node RG

    I attach an image of the scheme, so you can see the node names.

    Thanks in advance.

    M.

    Last edited by BradtheRad; 14th January 2016 at 17:13. Reason: added code formatted window

    •   AltAdvertisment

        
       

  2. #2
    Super Moderator
    Points: 251,535, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    43,802
    Helped
    13318 / 13318
    Points
    251,535
    Level
    100

    Re: "Less than 2 connections at node" error message in pspice

    Most easily achieved by omitting useless R6. Otherwise must connect a dummy resistor from RG node to ground, e.g. Gohm value.



    •   AltAdvertisment

        
       

  3. #3
    Junior Member level 1
    Points: 341, Level: 3

    Join Date
    Jun 2015
    Posts
    15
    Helped
    0 / 0
    Points
    341
    Level
    3

    Re: "Less than 2 connections at node" error message in pspice

    Quote Originally Posted by FvM View Post
    Most easily achieved by omitting useless R6. Otherwise must connect a dummy resistor from RG node to ground, e.g. Gohm value.
    What do you mean with ommiting? Because I checked the netlist and all the parts are present.



    •   AltAdvertisment

        
       

  4. #4
    Full Member level 2
    Points: 2,336, Level: 11
    Achievements:
    7 years registered

    Join Date
    Dec 2009
    Location
    India
    Posts
    144
    Helped
    64 / 64
    Points
    2,336
    Level
    11

    Re: "Less than 2 connections at node" error message in pspice

    You've written wrong expression for GVALUE.
    Change it from { V(RG, 0) } to { V(RG) }
    If you need a differential of input pins then write as { V(RG)-V(net2) }, V(net2) is zero in your circuit configuration.


    1 members found this post helpful.

  5. #5
    Super Moderator
    Points: 251,535, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    43,802
    Helped
    13318 / 13318
    Points
    251,535
    Level
    100

    Re: "Less than 2 connections at node" error message in pspice

    You've written wrong expression for GVALUE.
    Change it from { V(RG, 0) } to { V(RG) }
    If you need a differential of input pins then write as { V(RG)-V(net2) }, V(net2) is zero in your circuit configuration.
    The shown net list is automatically generated by PSPICE and hasn't been written by msmol. it's just the translated schematic entry.
    Because I checked the netlist and all the parts are present.
    And RG is a node with single connection, as the net list shows. The problem is that the G2 input is not loading the node, just sensing the voltage. For the same reason R6 is useless. I suggested two possible solutions. It could make sense to try it even if you don't understand why.


    1 members found this post helpful.

  6. #6
    Full Member level 2
    Points: 2,336, Level: 11
    Achievements:
    7 years registered

    Join Date
    Dec 2009
    Location
    India
    Posts
    144
    Helped
    64 / 64
    Points
    2,336
    Level
    11

    Re: "Less than 2 connections at node" error message in pspice

    Looks like "msmol" made some mistake on GVALUE part due to which the wrong netlist getting written.
    I checked at my end, it is written as below by tool. And it works fine.
    G_G2 GCL 0 VALUE { V(RG, 0) }

    I am using 16.6 version though.
    -------------------------------------------------------------------------------------

    Sorry for the above confusion.

    @msmol -- I checked your netlist as it is. And it is working fine at my end. I am using 16.6 version.
    Last edited by mvaseem; 15th January 2016 at 12:51.



    •   AltAdvertisment

        
       

  7. #7
    Junior Member level 1
    Points: 341, Level: 3

    Join Date
    Jun 2015
    Posts
    15
    Helped
    0 / 0
    Points
    341
    Level
    3

    Re: "Less than 2 connections at node" error message in pspice

    Quote Originally Posted by mvaseem View Post
    You've written wrong expression for GVALUE.
    Change it from { V(RG, 0) } to { V(RG) }
    If you need a differential of input pins then write as { V(RG)-V(net2) }, V(net2) is zero in your circuit configuration.
    I rewrited the netlist as follows:

    Code:
    Diodo MT 3
    V_V8         inR2 0 30mV
    R_R2         inR2 RG  1g  
    G_G1         GLC 0 VALUE { PWR((COS(5000*V(RG)-5)-COS(5000*V(RG)-40)),2)*(V(RG)*0.8e-8) }
    L_L3         GLC 0  6e-5  
    C_C3         GLC 0  1e5
    .END
    But I keep getting the same error message.

    Most easily achieved by omitting useless R6. Otherwise must connect a dummy resistor from RG node to ground, e.g. Gohm value.
    This solution effectively helped to jump over the problem, but for the work I need to do, it would be better not to add parts, just to keep this equivalent circuit as simple as possible.

    Thanks "FvM" and "mvaseem", I hope I can solve it with the recoding option. Nevertheless, If you can keep helping me, it will be so useful.



--[[ ]]--