what do you think the circuit of this load http://eko-eu.com/products/photovoltaic-evaluation-systems/i-v-tracers/mp-410-mppt-electric-load

 

what do you think the circuit of this load http://eko-eu.com/products/photovoltaic-evaluation-systems/i-v-tracers/mp-410-mppt-electric-load

And you think that $180 is expensive????

 

And you think that $180 is expensive????

yes , it's for me

 

yes , it's for me

I think that the electronic load you posted the link to will cost ten times what the resistor costs...

 

I think that the electronic load you posted the link to will cost ten times what the resistor costs...

i didn't ask how to buy it , i asked if i can do it .

 

i didn't ask how to buy it , i asked if i can do it .

Yeah parallel a few mosfets in a bucket of oil or on an extruded aluminum heat sink and operate them in linear mode.

 

Here is a simulation of a panel similar to yours. I am varying the resistance of R1, the load resistor, as the independent variable (X-axis) . The blue trace is the voltage across the load (comes to near 36V open circuit), the red trace is current through R1 (comes to near 7A short circuit), and finally the green trace is the power dissipated by R1. Note that for this particular panel, the MPPT of 148W occurs at about 29V, 5A, when the load resistor is about 5Ω.

The highest dissipation in R1 occurs at the MPPT, so you would need a 5Ω 150W resistor. Note that the rehostat linked to earlier wouldn't do that without burning up. As the resistance is decreased, the power rating must be derated, or you will overheat the part of the winding through which the current is flowing.

Next, I present a sim of a crude but workable electronic load for your panel. The panel model is the same as in the previous simulation.
Here the independent variable of the simulation is the position of the pot, U2. The dependent plots show the panel voltage (green), panel current (red), the power dissipation in one of the NFETS (blue), and the power dissipation in one of the source resistors (violet).

Note that the power in the source resistors R1-4 peaks at 5W each, so you should use 10W resistors. The power in the NFETs peak at 34W each, so you should use TO220 style NFETs bolted to a very large metal plate heat sink. Note that the drains of the four NFETs are electrically common, so no insulating kit need be used under the NFETs, but the heatsink plate will be tied to the Panel+.

The sum of the power dissipated in the four resistors R1-4 and the four NFETs M1-4 is the same as the peak power delivered by the panel...

 

Mike, where did you get that nifty LTSpice solar panel model? How can I get one? Did you make it yourself?

 

Next, I present a sim of a crude but workable electronic load for your panel. The panel model is the same as in the previous simulation.
Here the independent variable of the simulation is the position of the pot, U2. The dependent plots show the panel voltage (green), panel current (red), the power dissipation in one of the NFETS (blue), and the power dissipation in one of the source resistors (violet).

Note that the power in the source resistors R1-4 peaks at 5W each, so you should use 10W resistors. The power in the NFETs peak at 34W each, so you should use TO220 style NFETs bolted to a very large metal plate heat sink. Note that the drains of the four NFETs are electrically common, so no insulating kit need be used under the NFETs, but the heatsink plate will be tied to the Panel+.

The sum of the power dissipated in the four resistors R1-4 and the four NFETs M1-4 is the same as the peak power delivered by the panel...

why four NFETS and four resistors , as i saw in datasheet of IRF530 its PD equal 88 watt . ?

and how will i control the resistance and vary it with 1 ohm step ?
and why did you connect just R1 to U1 ? you said that you vary R1 and i see that it is fixed at 1.5 ohm.

 

why four NFETS and four resistors , as i saw in datasheet of IRF530 its PD equal 88 watt . ?

You need to learn about thermal derating. If you read the data sheet fine print, you will learn that it can dissipate 88W if the package is at 25degC. When you bolt it to a heatsink, the temperature of the heatsink (depending on its surface area) will rise.

How hot can it is allowed to get and still keep the IRF530 within its allowed dissipation rating is told by the 0.59 W/degC derating factor on the data sheet.
The allowed dissipation for this NFET at any case temperature is defined by a straight line equation Pd= 88 - 0.59*(t-25), where Pd is in W and t is deg C. Solving for 34W of dissipation, the max allowed case temperature is 116.5C, hot enough to boil water and then some.

Like I said, your heatsink area will be need to be huge, likely in excess of 1 square m., or you will need a blower, or you will need to immerse it in water or oil...

and how will i control the resistance and vary it with 1 ohm step ?

Are you wanting to vary the resistance with a micro controller or by just turning the pot shaft? Since in your original posting you bought a pot, I assumed the latter.

and why did you connect just R1 to U1 ? you said that you vary R1 and i see that it is fixed at 1.5 ohm.

R1 was being varied in the first simulation; not the second.
The configuration of the opamp and the NFET is a constant-current-sink. The opamp adjusts the gate voltage of the NFET to create a voltage drop across the source resistor R1 to create a current through R1 proportional to the pot position. I am assuming that the other three NFETs M2-4 have Ids vs Vgs curves similar to M1, so that they share the current equally...

In the second simulation, the 10KΩ pot-wiper is moved from 0% to 100% in steps of 2.5%.

 

Like I said, your heatsink area will be need to be huge, likely in excess of 1 square m., or you will need a blower, or you will need to immerse it in water or oil...



Are you wanting to vary the resistance with a micro controller or by just turning the pot shaft? Since in your original posting you bought a pot, I assumed the latter.



R1 was being varied in the first simulation; not the second.
The configuration of the opamp and the NFET is a constant-current-sink. The opamp adjusts the gate voltage of the NFET to create a voltage drop across the source resistor R1 to create a current through R1 proportional to the pot position. I am assuming that the other three NFETs M2-4 have Ids vs Vgs curves similar to M1, so that they share the current equally...

In the second simulation, the 10KΩ pot-wiper is moved from 0% to 100% in steps of 2.5%.

how could you vary R1 in first simulation i think it's also constant as both of two simulations have same configuration .
yes , i want to vary the resistance using pot.
you said that FETs dissipated power is 34 watt , how did you assume that ? from simulation and how to control that ?
and i got that varying the pot will vary current of FETS consequently its resistance , am i right ? if so what is the range of variation .
finally which resistors will be the load .

 

how could you vary R1 in first simulation i think it's also constant as both of two simulations have same configuration .

It is a simulation, therefore I can vary anything I want to...
Note that in the first sim the value of R1 is {R1}. The statement .step param R1 0.1 30 0.5 reruns a DC solution for all values of R1 from 0.1Ω to 29.9Ω in steps of 0.5Ω.

yes , i want to vary the resistance using pot.

Then use a linear 10K pot.

you said that FETs dissipated power is 34 watt , how did you assume that ? from simulation and how to control that ?

Look at the blue trace on the second simulation plot again. That is the dissipation in the NFET M1 (Watts) as a function of pot position. You cant "control" it; it is what it is...

and i got that varying the pot will vary current of FETS consequently its resistance , am i right ? if so what is the range of variation .

Yes
At any given pot setting, the effective resistance of the electronic load circuit is V(panel)/Ix (Panel voltage=green trace/Panel current=red trace).

finally which resistors will be the load .

At the worst case (near MPPT), 20W is dissipated in the four resistors R1-4 and 136W is dissipated in the four NFETS, for a total panel power output of ~150W

 

mah, isn't your goal to map out the I-V curve for your panel, so that you can calculate where the maximum power point is? This isn't that hard and I think you're getting buried in complexity.

You need just two things, a load that can be varied and metering of voltage and current.

Folks have told you over and over that the simplest load you can use is light bulbs. They are purpose-built to dissipate heat and provide visual feedback while being incredibly cheap and convenient. Another option is a heater element immersed in water.

There are a number of ways to control the load. One you may not have considered is to use an inverter with your panel and a simple light dimmer controlling lights on the AC side. You'll still take all your measurements on the DC side; voltage across the panel leads and current either directly with a current sensor or by voltage across a low ohms shunt resistor in series with the panel.

Or you could build yourself a constant current DC power supply using your panel (using an op-amp to watch the voltage across a shunt resistor). This simple circuit requires the power transistors to dissipate up to half the power of the load. 75W would need a good heat sink strategy but it's not unreasonable. An inexpensive control pot would allow you to smoothly control the overall current.

edit - Aww nuts, I see Mike has already described exactly this scheme, more or less.

 

I reran the second simulation, this time I plotted the effective resistance of the electronic load as a function of pot position. I asked LTSpice to plot the expression V(Panel)/I(Panel). It is easier to read the effective resistance if it is plotted on a logarithmic scale...

 

Mike, where did you get that nifty LTSpice solar panel model? How can I get one? Did you make it yourself?

Yes. I have worked with enough panels so I was able to just cobble it up on the fly:

It is just a piecewise-linear approximation that sorta-kinda has a IV curve that looks like most panels...

Isn't hierarchy wonderful? I can hide the complexity of the panel model in a simple two-terminal box.

 

Folks have told you over and over that the simplest load you can use is light bulbs. They are purpose-built to dissipate heat and provide visual feedback while being incredibly cheap and convenient. Another option is a heater element immersed in water.


edit - Aww nuts, I see Mike has already described exactly this scheme, more or less.

I need to vary the resistance around 10 ohm at mpp with sensitivity
0.2 ohm , how could i do that with light bulbs ?

 

Use the current control scheme Mike showed earlier - where voltage across a known shunt provides feedback for the control op-amp. The light bulbs are merely an inexpensive alternative load to use instead of costly resistors.

Don't think of it as controlling ohms - you'll control current and let the circuit provide whatever ohms are needed to do the job. You can calculate the effective ohms based on current and voltage drop.

 

I need to vary the resistance around 10 ohm at mpp with sensitivity
0.2 ohm , how could i do that with light bulbs ?

More like 5Ω.

 

Use the current control scheme Mike showed earlier - where voltage across a known shunt provides feedback for the control op-amp. The light bulbs are merely an inexpensive alternative load to use instead of costly resistors.

Don't think of it as controlling ohms - you'll control current and let the circuit provide whatever ohms are needed to do the job. You can calculate the effective ohms based on current and voltage drop.

ok i will use light bulbs instead of resistors but should i take their operating voltage into account i think that automotive light bulbs work on 12 Vdc .

 

More like 5Ω.

do you mean the sensitivity is 5 Ω ?