Got? it!? Thanks to all of you!

Right click on each of the common mode chokes.
The Value line should be blank.
Delete whatever you have typed on this line.
The file will run just fine.
Mike

I uploaded the .asc file to the temp directory.? ?Look for the file name Grid Filter 30m CMC BAL.asc.??
This is the WE-CMBNC.lib file:

* Manufacturer: ? ? ? ? ? Wurth Elektronik?
* Kinds: ? ? ? ? ? ? ? ? ?Common Mode Power Line Choke Nanocrystalline?
* Matchcode: ? ? ? ? ? ? ?WE-CMBNC?
* Library Type: ? ? ? ? ? Pspice
* Version: ? ? ? ? ? ? ? ?rev22a
* Created/modified by: ? ?Ella ? ? ?
* Date and Time: ? ? ? ? ?2022-05-26
* Team: ? ? ? ? ? ? ? ? ? eiSos EDA Service ?
* Contact: ? ? ? ? ? ? ? ?libraries@...

* Copyright(C) 2022 Würth Elektronik eiSos GmbH & Co. KG
* All Rights Reserved.

* Disclaimer: While Würth Elektronik eiSos has made every reasonable effort to ensure the accuracy
* of the simulation models provided, Würth Elektronik eiSos does not guarantee the exemption of error on
* the simulation models, nor does Würth Elektronik eiSos guarantee that the simulation model is current.
* Würth Elektronik eiSos reserves the right to make any adjustments at any time without notice.
* Würth Elektronik eiSos expressly disclaims all implied warranties regarding this simulation model.

***
.subckt CMBNC_S_7448021230_30m 1 2 3 4
X1 ?1 ?2 ?3 ?4 ?CMBNC ?PARAMS:
+ ?Rdc=0.28640000030398369
+ ?ck=2.01574164786085E-11
+ ?DC4=1.86840939855187E-13
+ ?DL4=1.59136141064664E-06
+ ?DR5=704.48291015625
+ ?DR6=6556.29541015625
+ ?DC3=3.03443589699803E-11
+ ?DL3=5.20691649519289E-12
+ ?DR3=18.1167163848877
+ ?DR4=766605248
+ ?L1=0.0208004059202671051
+ ?L2=0.00845833602175117
+ ?L3=0.00101479911245406
+ ?L4=0.00159177230671048
+ ?RS1=7904.43017578125
+ ?RS2=8743.3896484375
+ ?RS3=85064.4453125
+ ?RS4=19577.373046875
+ ?C1=0.92000004580825E-11
+ ?R2=0.104000002145767
+ ?C2=5.06184820501076E-07
+ ?L5=0.000372471375158057
+ ?RS5=302.954345703125
.ends CMBNC_S_7448021230_30m
***

Project schematics located in:
C:\Users\username\Documents\LTspiceXVII\Bernt_Projects\Force Sensor

symbols located:
C:\Users\username\Documents\LTspiceXVII\Bernt_Projects\Force Sensor\Lib

and then .lib dols located in separate folders under the above such as:
C:\Users\username\Documents\LTspiceXVII\Bernt_Projects\Force Sensor\Lib\INA826

The .sym files still have the old path from my other installation as in:

SYMATTR ModelFile %HOMEPATH%\Documents\LTspiceXVII\lib\sym\AutoGenerated\INA826.lib

I am confused now what that must change to for this to work and to work on different installations of LTspice

In addition to previous comment:
I have now created a subfolder inside my project (.asc) folder called "Lib" and placed all the components in there as in lib files and symbol files.
What should the path now become in each symbol file for the .lib file?



Regards
Bernt

I understand that.
However, what I do not understand is how to then place my symbols. In the Place component, it only shows stuff from the .lib (which includes Autogenerated) but nothing else so it is not possible to see other folders and components there.
?

Bernt

john23,

I am uncertain how to answer this.

You referred to Figure 12 of a datasheet for the lower two transistors, which is a GaN RF power amp.? I downloaded the datasheet from alldatasheet.com that you referred to.? Figure 12 is a plot of LSG (large signal gain?) versus frequency and Vd.? What does that have to do with how you used it?? Is there a different figure that you meant to use?

I am somewhat uncomfortable replacing the two RF transistors with two 3 ohm resistors.? I think what you wish to simulate is the switching circuit that supplies switched power to the two RF transistors.? M1 (or M1 and M2) switches the DC power on and off to the RF transistors represented by M4 and M5, or by the 3 or 1.5 ohm resistors which are the effective DC load that the RF transistors present to M1.? I think it's likely that the effective DC load presented by the RF transistors can vary a lot, so 3 ohms would be a VERY rough approximation.? And of course you also have the filtering of the switched supply voltage.

So, if I assume that the source pin of M1 represents the switched "DC" power to the RF transistors, then I think I understand your connection from the "VSS" pin of the UCC5304 to the source of M1.? Now, everything on that half of the UCC5304 should be referenced to that pin and that net.? The power source to the UCC5304's "VDD" pin also should be referenced to its "VSS" pin.? If it is not, imagine what happens when your circuit drives M1 to switch ON.? Its source pin pulls up towards +45 V.? Now you have a problem, because the UCC5304's VSS pin is around +40 V, but its VDD pin is only at +10 V (relative to the same Ground), so it has backwards DC power and it doesn't work.

I don't know how well the UCC5304 functions when its two halves move up and down fast.? That's something you need to worry about, to make sure that it works.? Also, there is likely more to the RF part of the circuit, such as supply filtering and bypassing.

What is the question (the "riddle")?? Is there still a question?? In your earlier circuit, you did not have a connection or path from the UCC5304's "VSS" pin to ground.? But in the photo 11.png, it does.

Andy

Checking back through the messages, I think this question was about the Wurth S_7448021230_30m common-mode choke.

I threw together a dummy simulation with that choke in it, and it ran without error.? Definitely not the "Unknown subcircuit" error you say you had.

Just to be clear -- you did select the part number by right-clicking on the symbol, and then selecting it from the choices in the drop-down menu after SpiceModel -- right?

That is also what the part selector in LTspice tells you:


If you edited the text line and typed in anything, that would be wrong, and likely would cause that error to occur.

You also wrote, "I do have the statement .lib WE-CMBNC.lib in the schematic."? ?Why did you do that?? Dis? someone suggest that you should do that?? It should not be there.? Delete it.? Wurth's symbol for the choke takes care of including the correct model file.

Andy

开云体育

Did you upload your .ASC? If not,we can't help much. There are already two .ASCs for common-mode chokes in the Temp folder. Search for 'common'.

Thanks for the info!? I did find the model and got the correct P/N in my circuit.? However, when I ran the sim, I got an error message saying "Unknown subcircuit called in" and referenced the part number of the Common Mode Choke.? I do have the statement .lib WE-CMBNC.lib in the schematic.

re: "Unknown subcircuit called in"

I guess that means you did something wrong.? Your subcircuit call (the netlist line starting with X) refers to a subcircuit name, which was never defined.? Maybe the names don't match.? Maybe the subcircuit definition is missing.

There is also some chance that the subcircuit call has a confusing arrangement of nodenames and parameters, so that it causes LTspice to use the wrong one as the subcircuit's name.

I don't recall if we had any information (or enough information) about what you are simulating, so that we can offer more advice.? We need to see what you tried to simulate, before we can see where your mistake is.? Can you upload it?? If you do, make sure to check the instructions for uploading simulations to the group's Files.

Andy

Thanks for the info!? I did find the model and got the correct P/N in my circuit.? However, when I ran the sim, I got an error message saying "Unknown subcircuit called in" and referenced the part number of the Common Mode Choke.? I do have the statement .lib WE-CMBNC.lib in the schematic.

Hi,

I'm not sure if it is already known, and it is definitely not mentioned in the "Undocumented LTspice" Wiki page:

I have a 8x8 matrix of signals and wanted to split off a bus by column.
signal[0],signal[8]...signal[56]

As a wild stab in the dark, I tried signal[0:63:8] to add a "stride" to the matrix notation. And it worked!
The dialog box prompt is correct:

"signal[0:63:8]" is a the name of a BUS with 8 conductors: signal[0], signal[8], signal[16], signal[24], signal[32], signal[40],signal[48], and signal[56]. Is this what you want?

Is there anyone that has edit permissions and would like to add this to the wiki?

Kind regards,
Hendrik

On 15/05/2024 02:05, Berntd via groups.io wrote:

I am trouble with this right at this moment.

I am not sure where to put the .lib files. On the previous install, it seemed to be wanting them in the .lib main folder.
And, the next issue now on a new install of v17, it is looking for them in the Autogenerated folder.

The error message is:
Could not open
'%HOMEPATH%\Documents\LtSpiceXVII\lib\sym\Autogenerated\INA826.lib



On this new install however, it puts the libs into c:\\username\AppData\Local\LTspice\lib\lib\Autogenerated

Are all the previously created symbols now useless unless each one is edited manually between machines?

I am also stumped that the default lib top folder is not selectable for LTSpice. That seems crazy.

Yes, the location for libraries and examples was changed on 17.1 for reasons that were explained at the time, but didn't get everyone's approval.

I think you have the new location slightly wrong:
c:\\username\AppData\Local\LTspice\lib\lib\Autogenerated

..should be
c:\users\<username>\AppData\Local\LTspice\lib\sym\Autogenerated

However, the new 17.1 install may have deleted the contents of the '%HOMEPATH%\Documents\LTspiceXVII\lib folder. I can't remember. See if you can locate it in Explorer. If it's still there, you should be able to find the symbol library and copy the contents somewhere else.

If it's all missing, it will be a salutory lesson that things should be BACKED UP, before anything major is done that might affect valuable data. When 17.1 was first announced, it was, after all, tagged as a "beta".

Anyway, things have changed again for the new V24. The "standard" libraries and examples are still in the AppData location, but I think with the exception of the Autogenerated folder, anything that you add there will be removed on the next "Component Update". This seems a bit draconian, but is designed to end the situation with users adding their own stuff to the standard libraries, which results in everyone's being different. To mitigate this, users can now keep all their own stuff in:

c:\users\<username>\Documents\LTspice

..and LTspice won't touch them.

This still doesn't address the problem of users forgetting where custom symbols and models are located for schematics that they want to be portable. That's why the usual suggestion here is that they be placed in the same folder as the schematic(s) that use them.

The other lesson is that you really shouldn't use stuff in the autogenerated folder. Instead, if you insist on using autogenerated symbols, immediately save or copy them somewhere else and delete (or edit) the ModelFile attribute, as previously described.

--
Regards,
Tony

开云体育

Just move the symbol and/or library files from wherever they are now to the folder or directory where the schematic is, using the operating system's file browser (or whatever they call it), or the command line, whichever suits you.

Then edit the symbol and schematic, per Tony's instructions.

All done.

Donald.

It is from Circuit Maker or latter Altium:
chrome-extension://efaidnbmnnnibpcajpcglclefindmkaj/https://wiki.bu.ost.ch/infoportal/_media/hardware/altium_designer/tr0113_simulation_models_and_analyses_reference.pdf

page 250

Thanks.
I need square wave vco for PLL tests. Currently I am using:

V=u(sin(2*pi*(fc*time+df*idt(V(m)))))

It can be dome in many ways wit B sources, although I am not sure how to add FM:

?

Triangle wave with period 1/fc:

V=fc* idtmod(1,0,1/fc)

?

Square wave with period 1/fc:

V=u(fc* idtmod(1,0,1/fc) - 0.5)

?

Staircase with period 1/fc:

V= floor(time*fc)

But as I remember in the good old Circuit Maker there was square/triangle vco, latter adopted by Altium.
I thought I could use it with LTSpice.

On Tue, May 14, 2024 at 07:56 PM, <bb_petrov@...> wrote:

Too few nodes: A1 %vd(1,2) %vd(3,4) ASQRVCO

Just curious: I know such error messages from XSPICE. Are you
mistakingly invoking ngspice (or KiCAD) somewhere in the chain?

-marcel

开云体育

I'm struggling to understand what you are trying to do with:

.MODEL ASQRVCO...

AFAIK, you can only define .models as being these types of LTspice primitives:

C, R, L, D, SW, CSW, URC, LTRA, NPN, PNP, NJF, PJF, NMOS, PMOS, NMF, PMF, NIGBT, PIGBT, VDMOS

See: Help > LTspice XVII > LTspice? > Dot Commands > .MODEL

--

Of course the model is in a circuit

* C:\Users\BoyanP\Documents\srt_marine\EP1_HH_eval\PLL\sim\pll_avg_mod\Draft3.asc
V1 N001 0 SINE(2.5 2.5 100)
XU1 N001 0 N002 0 SQRVCO C1=0 C2=1 C3=2 C4=3 C5=4 F1=0 F2=1k F3=2k F4=3k F5=4k LOW=0 HIGH=5 CYCLE=0.5 RISE=1u FALL=1u
.tran 130m
.lib C:\Users\BoyanP\Documents\LTspiceXVII\lib\sym\AutoGenerated\sqrvco.sub
.backanno
.end

Just a voltage source and autogenerated symbol.

开云体育

It won't run my itself. It needs to be included in a schematic with specifications of parameters (the symbols in { }).

Hello, I need little help, please. I am trying to run old square wave vco model:

*Voltage Controlled Square Wave Oscillator?
*LOW ? = Peak output low value?
*HIGH ?= Peak output high value *CYCLE = Duty cycle ?
*RISE ?= Rise time *FALL ?= Fall time?
*C1 ? ?= Input control voltage point 1?
*C2 ? ?= Input control voltage point 2?
*C3 ? ?= Input control voltage point 3?
*C4 ? ?= Input control voltage point 4?
*C5 ? ?= Input control voltage point 5?
*F1 ? ?= Output frequency point 1?
*F2 ? ?= Output frequency point 2?
*F3 ? ?= Output frequency point 3?
*F4 ? ?= Output frequency point 4?
*F5 ? ?= Output frequency point 5?
* Connections:?
* ? ? ? ? ? ? ?In+?
* ? ? ? ? ? ? ?| In-?
* ? ? ? ? ? ? ?| | Out+?
* ? ? ? ? ? ? ?| | | Out-?
* ? ? ? ? ? ? ?| | | |?
.SUBCKT SQRVCO 1 2 3 4 PARAMS: C1=0 C2=1 C3=2 C4=3 C5=4 F1=0 F2=1k ?
+ F3=2k F4=3k F5=4k LOW=0 HIGH=5 CYCLE=0.5 RISE=1u FALL=1u?
A1 %vd(1,2) %vd(3,4) ASQRVCO?
.MODEL ASQRVCO square(cntl_array=[{C1} {C2} {C3} {C4} {C5}]?
+ freq_array=[{F1} {F2} {F3} {F4} {F5}] out_low={LOW}?
+ out_high={HIGH} duty_cycle={CYCLE} rise_time={RISE} fall_time={FALL})?
.ENDS SQRVCO

The error is:
Too few nodes: A1 %vd(1,2) %vd(3,4) ASQRVCO?
What I am doing wrong?
Thank you.