Forums » CircuitLab Support Forum

I'm trying to set up my circuit so that I can test different resistor values but I'm stuck at what I should make the load resistance - what value I should put in for the load (the motor). Here's the circuit: https://www.circuitlab.com/circuit/2ap55v/7kw-brushed-motor-rectifier-circuit/

You need to work out what resistance represents a 7kW load at the voltage you get across it when it is a 7kW load.

A bit recursive but all you do is run the circuit with a swept load resistance parameter and plot power in the load. Then choose the appropriate load resiatnce from the plot.

However, there are several other problems with your circuit.

i) A motor is not a simple resistance. Google to find more. I'm not a motor expert.

ii) 7kW with 158V peak and a 100R resistor in series through 1N4148 small signal diodes?

Your circuit can't supply 7kW through a 100R source resistance. The max power you can supply is set by the maximum power theorem which says for a source resistance of R, the max power delivered to the load is when the load = R.

You'll get silly answers if only because you can't expect the 1N4148 diode model to extrapolate accurately out to the currents set by a 158V/100R let alone 7kW/158V load.

You need to edit the diode model to look like a higher power part. Browse vendor spice models for suitable high power diodes and pull out the parameters you can use in CL (i.e. not many).

That's why I stated in my circuit description that the diodes were named wrong but were rated at 100 amps. I don't know what the names of the diodes are because the diode bridge came from China and has no other markings than 100 A 250 V. I can't find a way to rename the diodes anything other than 1N4148, 1N4007, & 1N5817 anyways. Thank you for the other information however. Also, I only made the motor a resistive load because I thought that was how Circuit Lab wants it from the examples I saw. I understand that motors are more inductive than anything, but I don't know how to represent the motor in the schematic.

@Sublime: The very first question you should ask yourself is “WHY do I want to simulate WHAT exactly?”. The second is “What do I expect to find?”.

The answer to the first question would probably tell you the most important point:

• How far your effort has to go.

The answer to the second question may:

• Determine the timeframe and accuracy the simulation should cover.

• Result in a description of mechanical details regarding motor (serial / mixed / parallel field coil) and type of load.

• Focus your thoughts to some details you have to investigate.

• Last not least to get a feeling wheter your simulation results may be true or not.

I’m not really an expert for big DC motor theory and this (which?) kind of application, but I doubt your motor has a permanent magnet field. @Signality posted very useful links (the last one is top!) but it seems they are already beyond what I would (and could) use after answering the first question. I also doubt CL would be the best platform to go into such details.

In reality:

a) Don’t think about a voltage divider to reduce generator tension, get it done at the generator.

b) You may need a startup resistance (but it depends on controlling the generator). You have to think about how to stop before you switch on (how?).

c) You can skip the capacitor, it won’t help anyway (OK, you may have to think about emitting “some” radio frequency noise).

d) Don’t care about diode type or parameters anyway, they won’t blow in CL (sadly).

e) You have to think about controlling motor speed - at least at sudden loss of load (your motor could explode ! ) and power at load. You may think about protecting your rectifier, too !!!

You can measure all internal resistances (generator, rectifier, wiring, motor) using a bench top power supply. Set it to, say, 15 Volts and adjust the current limit to exactly 1A , measure voltages across the object, calculate…

• But take care, inductivity will seriously bite when simply disconnecting the current …

Regards, Sancho

@Sancho_P,

That's a very good critique.

Just one minor comment about your point (d):

@Sublime's project is:

" ...to power a 97 volt 70 amp DC brushed motor."

At 70A, the forward voltage of the CL 1N4148 model is 40.48V.

@Sublime's circuit puts two diodes in series because of the bridge rectifier.

You do need to use a more appropriate diode model because, in a high current application like this, without it you will get seriously silly answers.

; )

@Signality: (cough) You’ve caught me !!!

I did not check CL’s 1N418 model before.

Now this makes me wonder whether CL simulation is realistic, super - realistic or - - simply wrong.

Personally I tend to the latter: It’s simply wrong. Sorry.

41 V * 70 A = 2870 Watt at a 0.5 W glass body diode without explosion is an epic fail.

Simulation should be realistic, and this would be fairly simple for non academic use.

However, for academic use it should be foolproof, but that may be impossible :-((

@Sublime: OK, take the 1N4007, still 140 W per diode but you could simulate at least 23.4 nsec longer before it vaporizes ;-)

Regards, Sancho

@Sancho_P,

"Now this makes me wonder whether CL simulation is realistic, super - realistic or - - simply wrong.

Personally I tend to the latter: It’s simply wrong. Sorry."

CL is not "wrong". It gives exactly the same answer as spice.

In the same way you cannot shove 70A through a real 1N4148 and expect it to work, you cannot expect to be able to shove 70A through the model of a 1N4148 and get a forward drop of around a volt.

In just the same way as a bang or a burning smell on a real PCB, a 41V forward drop in a simulation is a clue to the fact that something is very wrong.

A simulator is a tool. You have to understand the limitations and possible hazards of using any tool (RTFM!).

You can use a hammer to fix a sheet of hardboard onto wooden batten using a panel pin. You could use it with the same type of panel panel pin to fix a sheet of hardboard onto a steel girder but you would not expect the panel pin to survive, let alone do the job you have asked of it.

You have to exercise your common sense and your judgement when using any tool.

If you misuse the tool expect things to get broken.

A good simulator is also not a toy. It does not have flashing lights, animated gifs or flash videos and .wav sounds to show you fancy graphics of your components exploding with a loud bang and a puff of iSmoke.

There are very good reasons why a circuit simulator allows the user to run components beyond their rated parameters.

Accidentally overload a component or make a design error in the real world and your circuit has gone bang, You don't get any 2nd chance to rewind to see what went wrong or why.

You do not expect a commercial flight simulator to kill trainee pilots if they crash. They get to walk away and learn from their mistakes. Rewind. Have a 2nd chance.

Precisely because you can't destroy a component at the instant you exceed some maximum rating, simulation allows you to do just that. Rewind. Have a 2nd chance.

You can investigate in detail exactly what will happen as the current through an inductor goes beyond the point where it saturates or where the power dissipation in a resistor would make it ignite.

You can see all the events leading up to that point and what would happen if you used a higher rated part or whatever.

You can see that what made component X blow was actually component Y hitting the supply rail because you had a wrong resistor value or calculated the wrong time constant.

If you really need to have a component destroy itself when you exceed it's current or voltage or power rating then you can build a behavioural circuit round it that opens or shorts a switch at the crucial point.

Or you put in a comparator with an output that goes to 1MV as soon as you exceed some defined limit.

No one is stopping you from doing any of that. It just takes more effort.

There are many more reasons why simulators don't simply blow things up. Simulation based FMEA;

http://signality.co.uk/ms.html

and Worst Case Circuit Analysis are two examples.

Having said all of that it is still up to the design engineer to use their common sense, judgement and experience as well as their specialist knowledge to look out for or check for those devices that are being run close to their limits and to redesign affected areas to reduce the stress on any such components as necessary.

Specialist knowledge, experience, judgement and a large part of common sense are skills that have to be learned.

A simulator is a good, safe and cheap way to do that.

@Signality: Oh, with all due respect, try to find back to reality. It’s not correct because it gives exactly the same answer as spice. It may be as wrong as … because of that.

Following your argument we wouldn’t live in houses but caves. What yesterday was is interesting, indeed, and we should learn from it.

But progress means to improve.

Not to make the same mistake as before.

;-)

Regards, Sancho

I think if you look at the datasheet for a 1N4148 or MMSD4148, replot the forward voltage vs. forward current graph on linear axes and then work out dv/di you'll find that the slope resistance is about the same as the R_S Ohmic Series Resistance parameter of the 1N4148 model in CL.

This is the same value as the Rs Ohmic Series Resistance parameter of the 1N4148 spice model.

70*0.568 = approx 40V;

Add to that the forward drop for an ideal silicon diode described purely by the diode equation:

Vd = Is*(exp(eV/nkT)-1)

which is about 1V at 70A, and you get approximately 41V.

The reality bit is that a real 1N4148 would be destroyed very quickly if you passed that much current through it whereas the simulation model will let you carry on with the simulation.

If you don't realise that a 41V diode drop is a bit silly then you are in for a rude awakening when you build the real circuit with either the 1N4148 and it vapourises or with a big chunky diode and it draws much more current than your simulation led you to expect.

Some simulators (I think Multisim is one) allow you to set limits on device currents, voltages and powers though I haven't used it so I don't know what happens if a limit is reached or exceeded.

As I explained, in any simulator, you can set up monitoring of such things and indicate via a plot or a printout that a limit has been exceed.

So, instead of just saying that CL and spice are wrong, just plain wrong, wrong, wrongy wrong wrong, perhaps you could write a spec what CL should do?

Flash the symbol and print up a big sign saying "Silly user: that'll never work! Use a bigger diode!!"?

That could be fun ...

In the meanwhile, trillions of ICs and millions of discrete circuits seem to have been very successfully designed using spice without such amusing interactivity.

Maybe CL could be the first to break the mould?

:-)

Sorry, my point is completely different:

I see simulation to fulfill real behavior as far as possible.

There is no real flight simulator (your example ! ) for real pilots where you would not FEEL when you reach critical (low) speed with all alarm signs on, or where you wouldn’t even hear when you push out landing gear.

So if there is a model for an 1N4148 and there is no warning whenever the power dissipation is in excess of 500 mW (let alone 1000 W) the model / the simulation is simply incomplete.

Same with your argument of destroying components: Yes, this would be part of a simulation:

Of course it would be useful to acknowledge warnings but tell the simulator to proceed. It may be difficult now but the simulator must “blow” the (e.g.) diode but go on.

Now think about headlines about CL after 10 years:

1) CL was the 27th simulator copying the spice behavior!

2) CL was the first simulator introducing reality in electronic simulation!

You can decide.

But don’t forget, copycats are never leader in technology.

;-)

Regards, Sancho

OK but be careful what you wish for ...

https://www.circuitlab.com/forums/feature-requests/topic/jpu4kadn/adding-virtual-realism-to-cl/