Inruesh current handling?

[crutschow]

You simulation has problems.

You did not assign diode models to D3 and D4.

You diode models are 4A, not 35A, which will reduce the peak current

You must use a phase shift of 90 degrees on your sine source and UIC conditions on the transient analysis to get the maximum peak current by starting at the peak of the sine wave with 0V on the cap.

Your cap value is 3300µF instead of the 15000µF you originally stated. Is that intentional?

With the changes I get a peak current through the cap of about 87A with 3300µF and the 4A diodes.

Incidentally, the cap ESR is a maximum, not a nominal, so the actual peak current could be higher due to that.

Here's the modified file View attachment Charger2.asc.

 

[Mosaic]

I understand spice modeling more with each post....8).


The biggest diode I could find is 25A....modeled with 22.6 AC peak (16rms) shows around 150A peak with the .08 esr of the cap. At 40% more with a 35A diode we have 210A peak. About half of the single pulse peak of the bridge rating I will use. I might use a power Nfet with 5Khz PWM to pulse charge lead acid batts. The 12V batts may be as low as 3 V to start with. Batts with voltage that low will have an Int Resistance of upwards of .1 ohm, dropping to under .01 ohm at max charge (around 13.2v)

As I want to use a .01 ohm current sense resistor to control the PWM I need avg current as opposed to sampling the spikes, therefore the 15KuF cap may have to come after the NFet switching (in parallel with the batt). The adc will be fed by a Diff. op amp, both ref'd to a lm4040 4.096v precision source.

Lead acid batts. act like huge caps., so I am not sure if the 15Kuf Cap is really necessary to smooth the current flow to measure with the current sense resistor.

I may have to do a Pi filter on the input of the Diff op amp to block the 5Khz PWM.


I'm reworking the design to look at using Nfets with a FET driver chip to do the switching

 

[crutschow]

I might use a power Nfet with 5Khz PWM to pulse charge lead acid batts. The 12V batts may be as low as 3 V to start with. Batts with voltage that low will have an Int Resistance of upwards of .1 ohm, dropping to under .01 ohm at max charge (around 13.2v)0

As I want to use a .01 ohm current sense resistor to control the PWM I need avg current as opposed to sampling the spikes, therefore the 15KuF cap may have to come after the NFet switching (in parallel with the batt). The adc will be fed by a Diff. op amp, both ref'd to a lm4040 4.096v precision source.

Lead acid batts. act like huge caps., so I am not sure if the 15Kuf Cap is really necessary to smooth the current flow to measure with the current sense resistor.

With PWM you need an inductor at the MOSFET output to smooth the current and avoid high peak currents (otherwise the peak current is limited only by the various circuit resistances).

You might consider using a standard switching regulator PWM circuit, such as one of those listed in the LTspice parts list. It's easier to design than doing one from scratch.

The battery does act like a big capacitor so you don't need much capacitance to smooth the waveform after the inductor.

You will likely need some lag compensation from the current feedback to stabilize the circuit if you use PMW in a feedback loop.

You can simulate the loop with LTspice to determine its stability.

 

[Mosaic]

BTW how can I simulate the transformer secondary inductance for limiting inrush current?

Would you think using a linear regulator with a couple high current pass transistors , fed by the 15KuF cap would be a better solution? I concerned about the ripple through the current sense resistor causing wrong adc sampling.

 

[crutschow]

BTW how can I simulate the transformer secondary inductance for limiting inrush current?

Would you think using a linear regulator with a couple high current pass transistors , fed by the 15KuF cap would be a better solution? I concerned about the ripple through the current sense resistor causing wrong adc sampling.

The transformer inductance does not limit the inrush current. That inductance is the magnetizing inductance and is not see by the load current.

The linear regulator would be simpler but less efficient. Is efficiency a concern?

To get the average current, just filter the signal from the current sense resistor with a LP filter.

 

[Mosaic]

Sampling

Well...since i plan to have the ADC sample millivolt changes across the current sense resistor I am going to go with the linear approach. It simulates fairly cleanly. See the attached sim.

I created a fudged battery model with a large cap & voltage source to see how a constant voltage charge causes a current drop as the battery approaches the charge voltage. Also I sim'd the PWM feed to control the Linear voltage regulation.

The 'noise' in terms of the voltage drop across the current sense is around .2mV or 0.5% which will be ok as I can sample 16 times and then avg it out.

The 220Amp inrush surge should be ok with the 400Amp surge rated bridge:

https://www.newark.com/jsp/search/productdetail.jsp?SKU=10M6173

What do u think?

 

[crutschow]

I don't understand the purpose of D5 through D9.

Why are you going to the complexity of converting the current signal to digital and then back to PMW analog? Are you going to use a microcontroller to adjust the voltage output?

 

[Mosaic]

new design

Cruts: Thanks for all your help so far...I think i am improving with this.

Yes I am doing PWM control to make it a constant voltage or current supply.

The diodes were to prevent reverse polarity batt conn. I used parallel units to get the current levels up.

Anyway...I spent some time over the last couple of days working on a design to drive a MOSFET with opamp linear control.

Here it is....seems to be working. Used Pi filters on the adc inputs to clean up the millivolt noise. The MCU adc will be fed by another opamp diff. amp (not shown) so that the signal can be properly sampled given a 4.096V MCU ref.

 

[crutschow]

I'll take a more detailed look at in Monday.

 

[Mosaic]

Ok...cool

Here's another "transistorised" version with current limiting and really good regulation.

Which do u think is best? I am leaning towards the transistorised version as a darlington TO3 will be easiest to heatsink and it has the best regulation in the sim.

 

[crutschow]

If the bipolar venison does what you want and it's easier to assemble then use that.

Why do you want an adjustable gain at R3?

You could probably do away with L1 and L2 and just use an RC filter. You could increase the value of the R and/or C if you need more filtering.

I recommend a resistor in series with the base of Q5 to limit base current under overload conditions.

P.S. When you draw your schematics, use orthogonal (not diagonal) lines. All normal schematics (with few exceptions) are drawn that way. Connection lines at various angles makes the schematic hard to read and look rather odd.