Keyboard Shortcuts
Likes
- LTspice
- Messages
Search
|
Re: cursor dialog in way of schematic
This is the problem
1. Maximise LTSpice 2. Maximise the schematic 3. You run it, add cursors. 4. Swap back to tab: It's a pain to have to close the dialog - and moving it won't always help, as you'l have already placed it where you wanted when looking at the plot. |
|
cursor dialog in way of schematic
The cursor dialog shown on plots lives on top of the
schematic too: even in "full-screen" mode (not tiled, not cascaded). Surely it is not a good thing that the cursor dialog is visible when I change tabs in full-screen mode ? (It's fine in Tile or Cascade mode) Yes, sure "I can just delete or move it"... The way I see it, working full-screen (tabs at top) means "I want to see what the tab says over the full application window" not "I want to see all of the schematic and any dialogs associated with the plots". |
|
Re: How can I make my simulation oscillate like my poorly designed PC board does?
It can be a real chore to make something oscillate when it doesn't want to. You mentioned a long trace. ?Does your schematic include wires or traces? ?I mean REAL wires? ?SPICE nets are ideal: zero length, zero inductance, zero capacitance, no delay, no coupling ... unless you account for them. ?Another cause for oscillation can be poor grounds, not realizing that "ground" is an artificial and impossible concept. ?Ground potential is not the same everywhere. ?If your layout is sloppy, then there is potential for many "ills" that could be affecting you (grounding, wire lengths, coupling between everything, etc.) that you would need to add to the simulation.
It can take a lot of work to include many of these parasitics. ?It's impossible to include them all.
How good are your FET models? ?Do your transistor models include lead inductances and such? ?If the model is only a .MODEL statement (not a .SUBCKT), then it does not. ?Some VHF/UHF oscillations can be caused by resonance in transistor leads.
You said the oscillation occurs half way up the waveform. ?If this a switching circuit with nominally square wave inputs and outputs, this implies coupling from output into input, which lets it oscillate when the transistor passes through its linear (amplifying) region. I am puzzled by the use of the Miller capacitance to apparently stop the oscillation. ?An oscillation occurs because there is gain, but something has not enough loss (too high Q) to prevent it. ?Adding capacitance moves the frequency but doesn't add loss, so it's probably not the right way to stop an oscillation. ?It just shifts it to a different frequency. ?You might get lucky by shifting it to a frequency that happens to have greater loss or less loop gain, but I think that's taking a chance.
If you haven't done this already, you will want to make sure to use a very small maximum timestep in the .TRAN statement, and probably turn off waveform compression (.options plotwinsize=0), just to make sure the simulation doesn't miss anything.
Regards,
Andy |
|
Re: Clipping a Universal op-amp
John Woodgate
In message <lm7khm+a0mhfa@...>, dated Thu, 29 May 2014,
"sineysitch@... [LTspice]" <LTspice@...> writes: Would that actually help with my overdrive (saturation) recovery issue?I'm sorry, but I can't understand what you want to do. It seems self-contradictory. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: How can I make my simulation oscillate like my poorly designed PC board does?
Carl wrote:
? ?"I've uploaded my circuit (Oscillating Miller FETs.asc) for your viewing pleasure." Unfortunately you uploaded it to the wrong Yahoo Group! Please re-upload it to THIS group, the [LTspice] group. ?The Files area in this group is the right place to put it, in the Temp directory.
Regards,
Andy |
|
Re: Clipping a Universal op-amp
Hi John,
Would that actually help with my overdrive (saturation) recovery issue? That is, I'd like to be sure the op-amp itself never hits the rails. I don't yet see a way (in or out of loop) to add a follower in such a way that it affects the actual op-amp output pin level... The issue I face is that my circuit may well not be able to drive enogh so that Vin+ = Vin-.? When that occurs, I want the op-amp to give up, accept the desired Vout/Vin cannot be reached, and not start slewing at max rate to the rails. Regards Stephen. |
|
Re: How can I make my simulation oscillate like my poorly designed PC board does?
¿ªÔÆÌåÓýThat sounds like you have a trace on your circuit that is acting as what used to be known as a Lecher line, but these days would be classed as a transmission line stub. ?
? At the critical point on the wave form this has a higher Q than the rest of the circuit and so the oscillation occurs. ? I can¡¯t help but get the feeling that increasing the miller capacitance is only helping it oscillate. Put about 10 ohms in series with the drain, close to the FET, and see what happens. A series resistor right at the gate might be an alternative stopper to oscillation. ? ? ? From: carlvanwormer@... [LTspice] [mailto:LTspice@...]
Sent: 29 May 2014 16:25 To: LTspice@... Subject: [LTspice] How can I make my simulation oscillate like my poorly designed PC board does? ?
I have a PC board with a FET that has a high-frequency oscillation because of my sloppy layout.? I'm trying to simulate the oscillation effect, but I'm unable to make my simulated circuit oscillate!? I know that most requests to the group are to stop the time-wasting oscillations in our simulations, ?but I need help making my circuit oscillate.? I've uploaded my circuit (Oscillating Miller FETs.asc) for your viewing pleasure. The goal of my final circuit is to slow down the rise and fall times with a large cap between the Drain and Gate, increasing the Miller Effect that we often try to minimize.? I usually tweak the value of the Miller Effect cap in the final circuit to balance the reduced noise switching harmonics (30MHz, for this design) with the increased heating losses of the slower switching speeds.? Unfortunately, I get a burst of oscillation (150-220MHz) about half way up the switching waveform on my circuit board.? I've traced the problem to a long trace to a poorly placed Miller Effect cap.? Any help in making my simulation oscillate would be appreciated. ? Thanks,
|
|
How can I make my simulation oscillate like my poorly designed PC board does?
I have a PC board with a FET that has a high-frequency oscillation because of my sloppy layout.? I'm trying to simulate the oscillation effect, but I'm unable to make my simulated circuit oscillate!? I know that most requests to the group are to stop the time-wasting oscillations in our simulations, ?but I need help making my circuit oscillate.? I've uploaded my circuit (Oscillating Miller FETs.asc) for your viewing pleasure.
The goal of my final circuit is to slow down the rise and fall times with a large cap between the Drain and Gate, increasing the Miller Effect that we often try to minimize.? I usually tweak the value of the Miller Effect cap in the final circuit to balance the reduced noise switching harmonics (30MHz, for this design) with the increased heating losses of the slower switching speeds.? Unfortunately, I get a burst of oscillation (150-220MHz) about half way up the switching waveform on my circuit board.? I've traced the problem to a long trace to a poorly placed Miller Effect cap.? Any help in making my simulation oscillate would be appreciated.
?
Thanks,
|
|
Re: Li-ion BAttery models
Lohith Vamsee wrote: ? ?"...?I need a li-ion battery model inorder to simulate.
? ? Can u suggest me some links or models?"
There may be a few in our group's Files section. ?Download the Table of Contents file (see instructions on the group's main webpage) and search it for "lithium". ? A few matches come up. ?It's not much, but you might find one of them works.
Regards,
Andy |
|
Re: Li-ion BAttery models
Lohith, It just happens that I have been using this same charger on a project and created a simulation for it that contains a Saft battery model that is fairly representative.? Maybe it will be useful. I just uploaded it to the Temp directory.??Normally that battery model is set for 1200mAh?but notice that I convert that to?10 msec to give quick looks at the charger behavior for different chemistry configurations.? In the battery block there are three configurations with SOC etc that can be selected by commenting. Tim |
|
Re: firing control in LTspice?
Hello Dave,
You missed the parameter FIREANGLE. I have added it. I also reduced the number of curly braces. Please use curly braces only around the whole expression. PULSE(0 10 {(FireAngle+240)/360*1/freq} .1u .1u {FireTime} {1/freq}) If you set the risetime in PULSE to 0, LTspice will automatically make it 10% of the pulse width. Normally you don't want this value. Instead you should specify it, e.g 0.1u which can be abbreviated to .1u . I uploaded your circuit with these changes and beautified the schematic a little bit. Files > Temp Best regards, Helmut PS: I don't know whether the pulse width of 100us is long enough. ? |
|
firing control in LTspice?
Hi team, I've a simulation?of a three phase voltage converter with resistive/inductive load. The switching devices are back to back SCRs. I wish to control the firing angle for the SCRs based on the current going through them. I know mathematically what I want to do, but have no idea how to put this into LTspice. Any help is appreciated :-) param: FireAngleStart = 45 degrees FireAngle? Iset =?100? amps initialisation: FireAngle = FireAngleStart; at the end of each mains cycle I wish to apply the following correction: If (I(V1) > Iset)?? then FireAngle = FireAngle +1 If (I(V1) < Iset)??
then FireAngle = FireAngle - 1 // where I(V1) is the supply current on phase 1. apply the new fireAngle to the SCRs. wait until the end of the next mains cycle and do this calculation again. my simulation is uploaded as "140529a_drentoul" Cheers Dave? |
|
Re: Pull-Push transformer for valve amp in LTspice
Sorry for the late response - catching up after return from vacation.
I've successfully simulated numerous p-p valve (tube) amp circuits using the simple model posted by the OP, albeit with higher values of inductance as pointed out by John Woodgate. Staying within linear range for input signals (ie little ouput distortion) gives good agreement between simulated and actual performance as measured on the bench. Eg. The SOVTEK Mig 50 (50w Marshall copy) usies EL34s (6CA7 equivalent) and the measured values of the primary inductors are 6H with a series resitance of 64ohms. Guitar amps only need to have a limited? bandwidth of approx 100Hz - 5kHz. Hi-Fi quality transformers will typically have higher values of inductance for a similar power output - but they'll weigh considerably more. Believe me, I know from bitter experience that the transformers in 50w - 100w guitar amps are more than heavy enough! Martin |
thutches