"Like" AX84 on facebook

'Public Domain Modeling Software'
Author:B1ggjoe (registered user: 158 posts )
Date: Fri, Nov 02nd, 2007 @ 09:01 ( . )

I notice a lot of modeling of circuits going on on the site and it's impressive.

I would be interested in what free packages are available that are easy to use to model audio response of circuits in the time and frequency domains. I stress easy to use. I guess it would be nice if there were a library of linear models of transistors and tubes as well.

I'm actually an EE but haven't done much design for quite some time. I really don't want to dust off the old slide rule.

Could you let me know what you use?

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:B1ggjoe (registered user: 158 posts )
Date: Fri, Nov 02nd, 2007 @ 09:03 ( . )

It would also to be able to have a package that does schematics as well....

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:AROlson (registered user: 223 posts )
Date: Fri, Nov 02nd, 2007 @ 09:49 ( . )

While the ease of use quality has been debated by some, I find that LTspice from Linear Technology Corp is very capable, and free.

[link]

There is a schematic editor, basic parts library, good graphic output, and available models for valves and transformers. It is made available by LTC to sell switching power supply components, but I use it for many applications.

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:Tim Benson (registered user: 192 posts )
Date: Fri, Nov 02nd, 2007 @ 10:24 ( . )

Another +1 to LT spice. Duncan's Amp Pages [link] has a lot of models and such that can be used with LT Spice, plus links to more. I haven't really come across any other free sim software that is as comprehensive as LT Spice.

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:B1ggjoe (registered user: 158 posts )
Date: Fri, Nov 02nd, 2007 @ 21:34 ( . )

Tim and AROIson - Thanks for your recommendation !!

The last time I used a simulation it was a command line type on a mainframe using a terminal. You had to type in the network topology, I don't need to tell you how tedious that could be.

LTspice is excellent! Very east to build your circuit. I've got some learning to do but this is a beautiful program for stuff in the audio frequency range. It looks extremely powerful for linear circuit simulation. It looks like it is well supported with tube and transistor models as well from the DIY community.

Joe


-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:Proman (guest: search)
Date: Sat, Nov 03rd, 2007 @ 04:15 ( . )

I have used LT to simulate variations of the usual tone stack, came up with a new tone stack design, and solved a seemingly impossible frequency slope problem. Highly recommended program.

Proman

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:AROlson (registered user: 223 posts )
Date: Mon, Nov 05th, 2007 @ 15:10 ( . )

On 11/02/2007 @ 21:34, B1ggjoe wrote :
Tim and AROIson - Thanks for your recommendation !!
:
: The last time I used a simulation it was a command line type on a mainframe using a terminal. You had to type in the network topology, I don't need to tell you how tedious that could be.
:
: LTspice is excellent! Very east to build your circuit. I've got some learning to do but this is a beautiful program for stuff in the audio frequency range. It looks extremely powerful for linear circuit simulation. It looks like it is well supported with tube and transistor models as well from the DIY community.
:
: Joe
:
:
--



Being the geek that I am, I modeled the entire P1 amplifier before building one. This might get you started.

[link]

ARO

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:B1ggjoe (registered user: 158 posts )
Date: Tue, Nov 06th, 2007 @ 06:55 ( . )

ARO,

I noticed that you modeled the entire P1 from another thread. It is already on my hard drive.

This is very cool. now I can mod it to a P1-eX and look at things like different tone stacks. This will be a good way to learn the program.

It might be interesting to add gain stages or cathode followers.

I'd love to simulate the 12BZ7 version of the P1-eX, I don't suppose I'll find a model for that tube on-line. I guess I could change the model for the 12AX7 or just parallel two of them.

Thanks from one Geek to another.

Joe

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:AROlson (registered user: 223 posts )
Date: Tue, Nov 06th, 2007 @ 11:26 ( . )

On 11/06/2007 @ 06:55, B1ggjoe wrote :
ARO,
:
: I noticed that you modeled the entire P1 from another thread. It is already on my hard drive.
:
: This is very cool. now I can mod it to a P1-eX and look at things like different tone stacks. This will be a good way to learn the program.
:
: It might be interesting to add gain stages or cathode followers.
:
: I'd love to simulate the 12BZ7 version of the P1-eX, I don't suppose I'll find a model for that tube on-line. I guess I could change the model for the 12AX7 or just parallel two of them.
:
: Thanks from one Geek to another.
:
: Joe
--



Joe,

I had forgotten that I previously posted the zip file. I'm glad you found it useful.

Homework Assignment #1

a) Create a file named 12BZ7.cir containing the following code:

***** 12BZ7 MODEL *****
.SUBCKT 12BZ7 1 2 3 ; P G C; MODEL (TRIODE)
+ PARAMS: MU=203.95 EX=1.25 KG1=306.9 KP=278.41 KVB=1717.7 VCT=0.5
+ RGI=2000 CCG=6.5P CGP=2.5P CCP=.625P
E1 7 0 VALUE=
+{V(1,3)/KP*LOG(1+EXP(KP*(1/MU+(V(2,3)+VCT)/SQRT(KVB+V(1,3)*V(1,3)))))}
RE1 7 0 1G
G1 1 3 VALUE={(PWR(V(7),EX)+PWRS(V(7),EX))/KG1}
RCP 1 3 1G ; TO AVOID FLOATING NODES IN MU-FOLLOWER
C1 2 3 {CCG} ; CATHODE-GRID
C2 2 1 {CGP} ; GRID=PLATE
C3 1 3 {CCP} ; CATHODE-PLATE
D3 5 3 DX ; FOR GRID CURRENT
R1 2 5 {RGI} ; FOR GRID CURRENT
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDS 12BZ7
*****

b) Create the symbol file 12BZ7.asy by modifying the 12AX7.asy file. (hint: use the attributes editor)

c) Create a test circuit using the 12BZ7 to generate an average plate characteristics plot. (hint: source V1 drives the grid, V2 drives the plate, ground the cathode, simulate using DC sweep analysis, and plot the plate current)

I generated the model for the 12BZ7 using a Matlab program from Norman Koren and the published plate curves from the Sylvania receiving tube manual.

Report back with your findings :^>

ARO

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:B1ggjoe (registered user: 158 posts )
Date: Tue, Nov 06th, 2007 @ 12:20 ( . )

This will keep be busy for some time. Is the final open book?

Thanks for the text file on the tube model this is much better than looking at RC low pass filters.

Joe


-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:Bob Hoffman (registered user: 15 posts )
Date: Thu, Jan 01st, 2009 @ 14:10 ( . )

Hello
I'm just starting out on LTspice and have been checking out your impressive modelling of the P1. I'm thinking of doing a similar modelling of an amp so was looking into what you did. First stop was the mains AC and noticed you put 180V for the amplitude. How come not 120V?
Bob

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:AROlson (registered user: 223 posts )
Date: Thu, Jan 01st, 2009 @ 15:16 ( . )

The 120 volts value for the AC mains is an RMS (root-mean-square) measurement. For sinusoidal signals, the peak value of the sine wave (amplitude) is 1.414=sqrt(2) times the RMS value. In LTspice you enter the peak voltage value rather than the RMS value.

I don't recall why I used 180 volts peak, which is like 127 volts RMS. I usually use 170 volts peak to simulate a 120 volt RMS power source.

ARO

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:Bob Hoffman (registered user: 15 posts )
Date: Thu, Jan 01st, 2009 @ 16:11 ( . )

Thank you!
Bob

-- REPLY: [With No Quote] --- [With Quoted Text]

'Public Domain Modeling Software'
Author:Danny Noordzy (registered user: 934 posts )
Date: Thu, Jan 01st, 2009 @ 18:03 ( . )

On 11/02/2007 @ 09:49, AROlson wrote :While the ease of use quality has been debated by some, I find that LTspice from Linear Technology Corp is very...

+ another one for LTspice
I've just started a week or so ago with it( for which I do need to thank John Hynes, Stephen Keller and Dustin Lobner,et alia, for getting me started on it). Not only can it do sims, but it is also great for just drafting schematics.

Another great resource for LTspice is yahoo-group [link]
There are a plethora of models that are not include by default in LTspice, such as transformers and potentiometers. Though you do have to register to view the files.

-- REPLY: [With No Quote] --- [With Quoted Text]


--- 38 Users Online --- 26 Recent Unique Posters

Q165=1485233972 - Threads: / 1485233972