1. LTspice
  2. Теми

New version of Koren_tubes.cir

 

Hello all  Valve, Tubes or lampes LTSpice users

 

Just to let you know that I have just uploaded a new version of the koren tubes library

 

The major new thing is a approximation of a hexode / heptode model that I have cobbled together

 

The anode response is close but the screen grid is a bit dodgy.

 

Happy simulating

 

Suusi Malcolm-Brown
 

Suusi
 
Has the EH90 Heptode model in Koren_tubes.cir been tested? I cannot get it to work generating V/I curves.
 
The line below is generating log of a negative number. 
 

G2 2 4 VALUE={(EXP(EX*(LOG((V(2,4)/MU)+(V(3,4)+V(5,4))))))/KG2}

Do you have any LTspice test files you used? I only found Koren_tubes.cir and Heptode.asy.
 

On Sun, Nov 10, 2024 at 03:20 AM, Tom wrote:
The line below is generating log of a negative number. 
 

G2 2 4 VALUE={(EXP(EX*(LOG((V(2,4)/MU)+(V(3,4)+V(5,4))))))/KG2}

Do you have any LTspice test files you used? I only found Koren_tubes.cir and Heptode.asy.
 
Tom,
 
Do you have a circuit you can upload that illustrates this happening?  Please include not only the schematic (.ASC), but also all symbols (.ASY) and model files (.CIR and others) needed in your schematic.  Even if you downloaded any of the files from this group, include them as well.  No photos, please; they do not help.  Then ZIP them together into one .ZIP file (make sure it is .ZIP), and upload it into the Temp directory.
 
I don't notice anything in that formula that would prevent log() of a negative number, if the voltages are in the right - or wrong - range.  It's possible that it was inevitable if the voltages elsewhere in your circuit are like that.
 
Andy
 
 
 
 

Well, obviously one of those three voltages must be negative and its magnitude greater than the sum of the other two, in order to make the total negative. Or two of the voltages are negative and the magnitude of their sum is greater than the third. Or all three voltages are negative! It should be easy to find out.

On 2024-11-10 13:39, Andy I via groups.io wrote:
On Sun, Nov 10, 2024 at 03:20 AM, Tom wrote:
The line below is generating log of a negative number. 
 

G2 2 4 VALUE={(EXP(EX*(LOG((V(2,4)/MU)+(V(3,4)+V(5,4))))))/KG2}

Do you have any LTspice test files you used? I only found Koren_tubes.cir and Heptode.asy.
 
Tom,
 
Do you have a circuit you can upload that illustrates this happening?  Please include not only the schematic (.ASC), but also all symbols (.ASY) and model files (.CIR and others) needed in your schematic.  Even if you downloaded any of the files from this group, include them as well.  No photos, please; they do not help.  Then ZIP them together into one .ZIP file (make sure it is .ZIP), and upload it into the Temp directory.
 
I don't notice anything in that formula that would prevent log() of a negative number, if the voltages are in the right - or wrong - range.  It's possible that it was inevitable if the voltages elsewhere in your circuit are like that.
 
Andy
 
 
 
-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.www.avg.com
 

It is possible that a voltage might swing far negative while SPICE/LTspice is trying to converge on a solution, and that might trigger an illegal math operation even when none of the voltages end up with negative values.  That (the need to try unreasonable voltages or currents) is how SPICE works.  It may need to try values that are waaay out of bounds, if the derivatives drive it in that direction, on the way to finding the actual solution.  The model should be robust enough to handle that without falling over.
 
In IBIS models, that was a question many would ask - why do IBIS models require tables of I/V values that far exceed normal operation?  You might never in your right mind apply -5 V directly to an input pin that clamps below ground.  But the simulator may try that voltage, on its way to finding a solution, and the I/V table inside the model needs to provide the right value - or at least something appropriate to send the simulator back into the normal range of operation.
 
Andy
 
 
 

Holger at ngspice made the following observation:
 

"There is a bug in the Koren model description. The correct node sequence is
.SUBCKT HEXODE 1 2 3 4 5 ; A G2 G1 C G3
with G1 and G3 the controlling grids and G2 the screen grid(s). That is G2 and G3 had been mixed up."

The "corrected" model doesn't have the prior issue. I am doing further testing to see if this pentagrid model works better than the 6BE6 and 6CS7 models I have that work at "DC" but when used as a mixer/oscillator don't use plausible L/C values.
 

 

Hi Tom The current version is Koren_Tubes_23 in which is is somewhat fixed

Taken from the latest header. Hope that this helps

* 18. 14 June 2018

*     Fixed the Hexode labels from A, G3, G1, C, G2 to A, G4+G2, G1, C, G3 as pointed out by Dirk Reefman Thanks

* 19. 25 June 2018

*     Added

*     Triode: 12B4A

* 20. 07 April 2019

*     Added

*     Triode: 6BC8

* 21. 25 May 2020

*     Major reorganisation and the replacement of the contact potential diode model

*     with Stefano Perugini's second improved diode model. Based on the original article

*     Vacuum diode Models & PSpice Simulations by Stefano Perugini

*     https://digilander.libero.it/paeng/vacuum_diode_models.htm

* 22. 02August 2020

*     Added voltage regulator tubes as a modificaion to LTspice's neon bulb

*     Vrtubes: OA2, OA3, OB2, OB3, OC2, OC3, OD4, 85A2, 5651, 5651A, 5783, STV70/6, STV85/10

* 23. Added

*     Triode 6S7B

*

* Suusi Malcolm-Brown May 2008 - 31 Dec 2023

Suusi M-B

From: LTspice@groups.io On Behalf Of Tom via groups.io
Sent: 10 November 2024 17:16
To: LTspice@groups.io
Subject: Re: [LTspice] New version of Koren_tubes.cir

 

Holger at ngspice made the following observation:

 

"There is a bug in the Koren model description. The correct node sequence is
.SUBCKT HEXODE 1 2 3 4 5 ; A G2 G1 C G3
with G1 and G3 the controlling grids and G2 the screen grid(s). That is G2 and G3 had been mixed up."

The "corrected" model doesn't have the prior issue. I am doing further testing to see if this pentagrid model works better than the 6BE6 and 6CS7 models I have that work at "DC" but when used as a mixer/oscillator don't use plausible L/C values.


Virus-free.www.avg.com
 

 

Hi Tony,

 

As for the pentagrid I didn’t even try as I was working on a hexode simulation at the time. But I will be rather surprised if it did work.

As an observation of the EH90 model is that it reads the Ig2+g4 at ¼ of the correct value

Philips data sheet   Model

Va         = 100 V

Ia          = 800 uA    800uA

Vg2+g4 =  30 V

Ig2+g4  =  1.2 mA   300uA

Vg1       = 0 V

Vg3       = -1 V

I hope that helps.

 

Suusi M-B


From: LTspice@groups.io On Behalf Of Tom via groups.io
Sent: 10 November 2024 17:16
To: LTspice@groups.io
Subject: Re: [LTspice] New version of Koren_tubes.cir

 

Holger at ngspice made the following observation:

 

"There is a bug in the Koren model description. The correct node sequence is
.SUBCKT HEXODE 1 2 3 4 5 ; A G2 G1 C G3
with G1 and G3 the controlling grids and G2 the screen grid(s). That is G2 and G3 had been mixed up."

The "corrected" model doesn't have the prior issue. I am doing further testing to see if this pentagrid model works better than the 6BE6 and 6CS7 models I have that work at "DC" but when used as a mixer/oscillator don't use plausible L/C values.


Virus-free.www.avg.com
 

The Heptode.asy I downloaded last week is wrong. I updated it to match Koren_Tubes_23.cir and added pin labels. I did not check Hexode.asy for accuracy.
 
I have a EH90 mixer/oscillator simulation semi working in ngspice. I need to convert it to LTspice.
 
I uploaded my files.

 

Hello Suusi M-B
 
Will the models you up loaded support class B and possibly class C operation? 
 
Thank you, 

1 - 10 з 10