I have an LTspice .asc file that contains a .tran and an .include directive, and one component symbol: the Pentode "U1" that comes with current LTspice. In the SpiceModel field of that U1, it has "6267" - the subcircuit which gets included by the directive - and in the file included, the subckt is named like that also. Yet, when running the schematic, I get "unknown subcircuit called in". The included file is in the same folder as the .asc file, and LTspice seems to find it: if I right-click on the include directive and then on the "Open" button of the dialog that popped up, it opens the correct .inc file.
So why isn't it working?
The .asc file:
Version 4 SHEET 1 920 680 SYMBOL Misc\\pentode 144 176 R0 SYMATTR InstName U1 SYMATTR SpiceModel 6267 TEXT 104 -96 Left 2 !.tran 1m TEXT 584 48 Left 2 !.inc 6267.inc
The 6267.inc file:
* * Generic pentode model: 6267 * Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved. * Version 3.10, Generated on Sat Mar 8 22:42:16 2008 * Plate * | Screen Grid * | | Control Grid * | | | Cathode * | | | | .SUBCKT 6267 A G2 G1 K BGG GG 0 V=V(G1,K)+0.59868749 BM1 M1 0 V=(0.010782364*(URAMP(V(G2,K))+1e-10))**-0.70765893 BM2 M2 0 V=(0.67945278*(URAMP(V(GG)+URAMP(V(G2,K))/29.728844)))**2.2076589 BP P 0 V=0.0013378994*(URAMP(V(GG)+URAMP(V(G2,K))/43.754099))**1.5 BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.00078620809*V(M1)*V(M2) BIG IG 0 V=0.00066894969*URAMP(V(G1,K))**1.5* (URAMP(V(G1,K))/(URAMP(V(A,K))+URAMP(V(G1,K)))*1.2+0.4) BIK2 IK2 0 V=V(IK,IG)*(1-0.4*(EXP(-URAMP(V(A,K))/URAMP(V(G2,K))*15)-EXP(-15))) BIG2T IG2T 0 V=V(IK2)*(0.83966688*(1-URAMP(V(A,K))/(URAMP(V(A,K))+10))**1.5+0.16033312) BIK3 IK3 0 V=V(IK2)*(URAMP(V(A,K))+7510)/(URAMP(V(G2,K))+7510) BIK4 IK4 0 V=V(IK3)-URAMP(V(IK3)-(0.00071507731*(URAMP(V(A,K))+URAMP(URAMP(V(G2,K))- URAMP(V(A,K))))**1.5)) BIP IP 0 V=URAMP(V(IK4,IG2T)-URAMP(V(IK4,IG2T)-(0.00071507731*URAMP(V(A,K))**1.5))) BIAK A K I=V(IP)+1e-10*V(A,K) BIG2 G2 K I=URAMP(V(IK4,IP)) BIGK G1 K I=V(IG) * CAPS CGA G1 A 0.05p CGK G1 K 2.3p C12 G1 G2 1.5p CAK A K 5.3p .ENDS
The accepted reply does work. Changing the 6267 from SpiceModel field to Value field eliminates the "Unknown subcircuit" error, to produce a "count mismatch error", which is due to:
Most "pentode" SPICE models are actually tetrode models; very few model the pentode's suppressor grid because it is generally assumed to be connected to the cathode, rather than being used as a modulating element. So you should use the LTspice built-in tetrode symbol instead, ignoring the suppressor grid in your LTspice schematic. This should work.
... according to Ray Waters' post in this diyaudio thread
Changing the symbol to tetrode indeed gets rid of that.