I am new to LTspice, am using LTspiceXVII on Linux via Wine, works well but I have 2 problems. 1 - Ctrl+M does not give a new line on .op. 2 - I downloaded a model for CD4060 but cannot get it to work always getting an error "could not open CD4060Bg". I have also tried copying the 4060model to the circuit. What am I doing wrong? - other text file models have worked . my4066.asc uploaded

1. Ctrl-Enter does what you want.

2. You failed to upload your CD4060 symbol, so we can't run your simulation. "Could not open CD4060Bg" suggests LTspice couldn't find the file - probably because it doesn't exist. Are you sure it isn't named "CD4060Bg.lib" or "CD4060Bg.sub", or even "CD4060Bg.txt"? Check in Windows Explorer for the correct name. (Hint: make sure Explorer is set up to show file extensions.)

Regards,
Tony

On 21/01/2020 16:38, Dave wrote:

I am new to LTspice, am using LTspiceXVII on Linux via Wine, works well but I have 2 problems. 1 - Ctrl+M does not give a new line on .op. 2 - I downloaded a model for CD4060 but cannot get it to work always getting an error "could not open CD4060Bg". I have also tried copying the 4060model to the circuit. What am I doing wrong? - other text file models have worked . my4066.asc uploaded

Hello Dave,

the problem can be solved by switching to alternate solver in SPICE options.

You should not upload *.raw and other useless files generated during simulation, the *.asc and possibly the *.plt file are all you need. You can by the way save much disk space on your computer by selecting automatic deletion of raw files in LTspice Control panel/Operation.

Frank

I have uploaded CD4060Bg.txt which I have been trying also CD4060.asy. thanks for tip on .op

The CD4060Bg model is incomplete. There are missing internal sub-circuits CD40_IN_1, CD40_IN_S_1, and CD40_OUT_1X. I presume these are I/P and O/P buffers, but without them the model is useless.

The note in the CD4060Bg model file suggests it was derived from the CD4020B model, which is included in Helmut's CD4000 model library. I checked CD4000.lib and indeed those sub-circuits are included there.

I suspect the author - Geoff Western (aka Alec_t) - of the CD4060Bg file also had a .lib CD4000.lib directive in his test circuit for the CD4060Bg, so those sub-circuits were silently included.

I have copy-pasted the I/P and O/P buffers block of code from CD4000.lib into the CD4060Bg model file and it now appears to function, although I haven't checked if it works correctly. I've uploaded it as CD4060Bg.sub. I don't guarantee it is correct.

The best solution is to ask Helmut to include this device in an updated version of his CD4000 library. However, if someone asked me to do this, I'd want to carefully validate it first to make sure the performance was at least similar to the datasheet. This is not a trivial exercise.

Regards,
Tony

On 21/01/2020 18:06, Dave wrote:

I have uploaded CD4060Bg.txt which I have been trying also CD4060.asy. thanks for tip on .op

On Tue, Jan 21, 2020 at 08:06 AM, Dave wrote:

could not open CD4060Bg

Hello Dave,

You haven't used the full filename. You have only used ".lib CD4060bg".
Your example has immediately worked after I used the complete filename. See below.

.lib CD4060Bg.sub

Helmut

Hi Dave,

Can you try LTSpice on Windows OS? Just to check.

I am using it on Windows 10 and works perfectly fine.
CTRL M works when writing SPICE Directives and it does work with 3rd party Spice Models.

Good Luck,

Raymond

On Tue, Jan 21, 2020 at 9:07 AM Dave <davega@...> wrote:

I am new to LTspice, am using LTspiceXVII on Linux via Wine, works well but I have 2 problems. 1 - Ctrl+M does not give a new line on .op. 2 - I downloaded a model for CD4060 but cannot get it to work always getting an error "could not open CD4060Bg". I have also tried copying the 4060model to the circuit. What am I doing wrong? - other text file models have worked . my4066.asc uploaded

DaveA