How to get correct graph in this Pspice circuit when simulate it ?

[Ali Z]

Hi
I am studying a dc dc converter model. My friend drew this circuit and got this graphic.
I added his circuit and graph . But I draw same model , same numbers for resistors capacitors v pulse source ,inductor, diode but my graph is very different.
Actually my V pulse source looks like doesn't working . I added my Pspice design and graph . What is my mistake ?
Could you please help me ?

 

[stenzer]

Hi,

your graph shows only a time span of 1 µs, the graph of your friend 500 µs. Re-run your simulation for a longer time.

BR

 

[Ali Z]

I made time longer and got this graph . It shows maksimum 20 Amper . Again different then my firneds graph. I added my graph2 png file

 

[stenzer]

Hi,

the last graph looks like your boost converter is operated in Discontinuous Current Mode (DCM), where the current through your inductore gets zero during each switching period.

A possebility would be a too low inductor value, but is seems to work for your friend.

Try to connect a e.g. 10 k resistor right after your 4.7 Ohm resistor toward ground (one common resistor from the Gate of your IGTBs toward GND). This should ensure your IGBTs are turned off for sure (but I do not see any current flow through the IGBT during off period).

Also try to simulate up to 100 ms (as your friend), it might be that you are seeing some kind of start up behaviour.

BTW, your chosen diode might be quite on the edge with a nominal average current of 60 A.

BR

 

[Ali Z]

Actually I made step by step solution . I deleted all ıgbt and tested circuit and saw there is no voltage after diode . So I realised that my diode is not working and change that diode and ısaw voltage and added IGBT again . and now I saw a graph but this time very high ampers like 300 Amper . I am adding my new graph and its closer vision and circuit again. Can you check what is my mistake this time?

 

[stenzer]

Hi,

you have to watchout which kind of components you are using. Your diode is a varactor one, with a breakdown voltage of 60 V. You are aiming to boost the voltage (Vout > 201.6 V). So if you turn on your IGBTs, the voltage across the diode is too large and leads to an additional current flow accross the IGBTs. You migth choose R7000803 (300A, 800V, General Purpose Rectifier) as diode, which should be available in PSpice according to [1].

[1] https://www.pspice.com/discrete/diodes/general-purpose?page=13

BR

 

[Ali Z]

Hi,

you have to watchout which kind of components you are using. Your diode is a varactor one, with a breakdown voltage of 60 V. You are aiming to boost the voltage (Vout > 201.6 V). So if you turn on your IGBTs, the voltage across the diode is too large and leads to an additional current flow accross the IGBTs. You migth choose R7000803 (300A, 800V, General Purpose Rectifier) as diode, which should be available in PSpice according to [1].

[1] https://www.pspice.com/discrete/diodes/general-purpose?page=13

BR

I tried , graph is getting closer but amper value is again high. This a circuit of 27 kw boost converter . If dc value is 201.6 Volt so , current should't pass 134 Amper. But in my graph I see almost 360 amper values on igbt . What can else be ? I added my last graph when I changed diode , I used 300 amper 1200 volt diode. But maybe that 360 amper breakdown to diode I don't know. But in this circuit 60 amper diode is enough actually according to boost converter original design. İf you write your e mail , I can send you also my circuit to check it.

 

[stenzer]

Hi,

please do not send me private massages as I do not reply to them.

I'm not using PSpice at all (since ~20 years; I'm getting old ). I'm using LTspice very frequently, so I implemented your boost converter in LTspice. See the pictures below. There are no IGBTs available in LTspice, so I imported the provided SPICE model by Infineaon and created the symbol (I haven't but much effort in it).

According to your switching frequency with a duty cycle of about 70 %, your aimed output voltage is around 650 V. I increased the gate resistor from 4.7 Ω to 100 Ω, as the total gate inrush current has been in the range of a couple of amps. The higher resistance leads to an increased duty cycle of about 75 %, as it takes longer to discharge the IGBT gate capacitances. Consequently, the output voltage is about 800 V. As you can see, increasing the gate resistor leads also to a reduction of the switch on current spikes, as the IGBTs are turned on slower. This will most likely also increase IGBT losses during the on and off transistion, you should have a closer look.

In general, when running your simulation have a look at your output voltage and evaluate your signals when the steady state has been reached (aimed output voltage is met). As can be seen below, at the start-up the initial currents are very high, as the empty capacitor has to be charged also the output voltage is overshooting. You may introduce some prasitic components or more realaistic discrete components i.e. an inductor including a DCR.

BR

 

[Ali Z]

Hi,

please do not send me private massages as I do not reply to them.

I'm not using PSpice at all (since ~20 years; I'm getting old ). I'm using LTspice very frequently, so I implemented your boost converter in LTspice. See the pictures below. There are no IGBTs available in LTspice, so I imported the provided SPICE model by Infineaon and created the symbol (I haven't but much effort in it).

According to your switching frequency with a duty cycle of about 70 %, your aimed output voltage is around 650 V. I increased the gate resistor from 4.7 Ω to 100 Ω, as the total gate inrush current has been in the range of a couple of amps. The higher resistance leads to an increased duty cycle of about 75 %, as it takes longer to discharge the IGBT gate capacitances. Consequently, the output voltage is about 800 V. As you can see, increasing the gate resistor leads also to a reduction of the switch on current spikes, as the IGBTs are turned on slower. This will most likely also increase IGBT losses during the on and off transistion, you should have a closer look.

In general, when running your simulation have a look at your output voltage and evaluate your signals when the steady state has been reached (aimed output voltage is met). As can be seen below, at the start-up the initial currents are very high, as the empty capacitor has to be charged also the output voltage is overshooting. You may introduce some prasitic components or more realaistic discrete components i.e. an inductor including a DCR.

View attachment 175081

View attachment 175082

View attachment 175083

BR

I wanna inform you and all followers to follow this thread. First of all I wanted to go step by step on the circuit.
So , I deleted all IGBT and Vpulse and just Dc supply inductor diode capacitor and resistor left.
Later I checked every component measuring voltage and current. And then realised that there is no voltage after diode in my first image. So diode was not working well. I changed diode with your idea R7001203 . its 300 ampere 1200 volt diode in pspice library already. And then I saw my capacitor is not working well too . Because when I simulate just saw 160 volt on the resistor. Its basic capacitor. So I changed it discrete capacitor. When I simulate I saw 560 volt but this time it happen a green dot on the capacitor . İts writing an error when I click. Simulation is not working well on the capacitor like that.
Basic capacitors have simulation result but they are not working well shows 160 volt on the resistor(R1), but also these type of capacitors give error . What can I do ? Which capacitor should I chose?
I added image of error on the capacitor and other errors online drc part.
That errors on the online drc parts affect my simulation ? or these errors are just an error aboUt footprint ?

 

[stenzer]

So,

let me google that for you [1]....

"You have added parts from the "regular" Capture libraries, tools\Capture\libraries, rather than the PSpice libraries, tools\Capture\libraries\PSpice, hence the library parts have no PSpiceTemplate properties and will be ignored by the simulator."

[1] https://community.cadence.com/caden...311/warning-ornet-1119-no-pspice-template-for

BR