Problems importing NE5534 model and with OPA164x convergence

QSPICE
1

Hi,
I’m trying to compare a few op-amps in a very simple balanced to unbalanced audio converter.
I successfully tested the schematic with AD797, now I am trying to test NE5534 but all I am able to get is “Fatal error: .ends without matching .subckt”. This is the model.

…

  • NE5534 OPERATIONAL AMPLIFIER “MACROMODEL” SUBCIRCUIT
  • CREATED USING PARTS RELEASE 4.01 ON 04/10/89 AT 12:41
  • (REV N/A) SUPPLY VOLTAGE: +/-15V
  • CONNECTIONS: NON-INVERTING INPUT
  •            | INVERTING INPUT

  •            | | POSITIVE POWER SUPPLY

  •            | | | NEGATIVE POWER SUPPLY

  •            | | | | OUTPUT

  •            | | | | |  COMPENSATION

  •            | | | | | / \

.SUBCKT NE5534 1 2 3 4 5 6 7
*
C1 11 12 7.703E-12
DC 5 53 DX
DE 54 5 DX
DLP 90 91 DX
DLN 92 90 DX
DP 4 3 DX
EGND 99 0 POLY(2) (3,0) (4,0) 0 .5 .5
FB 7 99 POLY(5) VB VC VE VLP VLN 0 2.893E6 -3E6 3E6 3E6 -3E6
GA 6 0 11 12 1.382E-3
GCM 0 6 10 99 13.82E-9
IEE 10 4 DC 133.0E-6
HLIM 90 0 VLIM 1K
Q1 11 2 13 QX
Q2 12 1 14 QX
R2 6 9 100.0E3
RC1 3 11 723.3
RC2 3 12 723.3
RE1 13 10 329
RE2 14 10 329
REE 10 99 1.504E6
RO1 8 5 50
RO2 7 99 25
RP 3 4 7.757E3
VB 9 0 DC 0
VC 3 53 DC 2.700
VE 54 4 DC 2.700
VLIM 7 8 DC 0
VLP 91 0 DC 38
VLN 0 92 DC 38
.MODEL DX D(IS=800.0E-18)
.MODEL QX NPN(IS=800.0E-18 BF=132)
.ENDS
…

At the end there was a 0x1a char that I deleted, after first test.
I have successfully used a SSM2017 model which is quite similar, so I am not able to find anything wrong, and where I had doubts I checked just to find that they are normal, even though old time, spice elements. I suppose there plainly is something Qspice rejects, but cannot find what.

Othe issue: I also tried to test OPA164x in the same simple circuit, but I initially got

Starting Gmin stepping.
Warning: Gmin stepping failed.
Starting source stepping.
Warning: Source stepping failed at 0.49899(1e-15)
Starting pseudo transient analysis.
Pseudo transient analysis failed.
Warning: Using skipbp
Fatal error: Timestep too small(1.26335e-19) at t=1.06769e-08

and I’ve not been able to solve the issue. I also tried adding
uic, .options gshunt=1e-12, .options gmin=1e-11, .options RelTol=0.00001
in various combination to no result (message changed, but always a timestep problem. Is there anything else that I might try??

Thank you in advance
Giorgio

2

Remove this character for the NE5534 if you link it with the .lib directive.

image
image704×326 15.4 KB

3

Upload your schematic (including any necessary libraries).
By the way, read this to learn how to upload a netlist as text into a message.
Qspice Forum - New User to Basic User (File Upload) - QSPICE - Qorvo Tech Forum

4

KSKelvin, thank you very much, I should have remembered that a backslash is a line continuation character.

I was able to solve the other problem while preparing to send you the netlist. Was indeed a strange thing: I assigned the Vdd label to negative power supply node, and referenced it at OPA164x negative power pin. Later I made a few changes at PS node, deleting the negative rail and redrawing it : apparently the label kept a single orphaned point of the original rail alive, but I did not realize this as the label was near the new rail, so I thought that the label was attached to it. As a result the IC had no negative supply.

It would probably better to delete also the labels directly attached to a connection section when this is deleted: no one would expect to find a self standing label in the schematic.

Sorry for disturbing you on sunday: I did not expect such a fast answer.
Tank you again
Giorgio

1 Like
5

Qspice Update
Mike just released an update that solves the error for a subcircuit netlist with \ in the comment line.

Custom Symbol for NE5534
By the way, I made a custom symbol for NE5534 as its pin definition is not in a standard form of generic subcircuit opamp.
example.OpenLoopGain.NE5534.qsch (8.2 KB)
NE5534.301 - download from TI.com
NE5534.qsym (1.1 KB)

image
image1646×713 88.1 KB