Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

[SOLVED] help with multisim simulation

Status
Not open for further replies.

andreas157

Newbie level 6
Joined
May 14, 2012
Messages
11
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,362
help with multisim simulation (sim error)

hi, i'm trying to simulate this pfc rectifier in multisim. simulation won't start because of convergence error. tried convergence assistant but also hints on multisim forums with no result :roll:. Tried virtual transistor and diodes. I tried max timestep 1e-3. Nothing. So i guess i'm doing something wrong :-?

Pulse generator is 40kHz. It's a boost converter attached to a three phase recifier. The topology is fine itself. Runs in simulink (timestep 1e-6) but i need a more accurate spice simulation (power losses, efficiency etc).

i got this:

------ Checking SPICE netlist for Design1 - Κυριακή, 10 Φεβρουαρίου 2013, 2:36:17 μμ ------
======= SPICE Netlist check completed, 0 error(s), 0 warning(s) =======
Error message from simulation: doAnalyses: Timestep too small


schematic is

thanks.
 
Last edited:

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,854
Helped
14,119
Reputation
28,495
Reaction score
12,800
Trophy points
1,393
Location
Bochum, Germany
Activity points
277,754
You shorted part of the rectifiers by incorrect grounding. If the DC bus is grounded, the star point must be floating (respectively connected to ground with a high ohmic resistor to help simulation convergence).

It's not actually a PFC rectifier by the way, because the input currents of a three phase bridge can't be sinoidal.
 

andreas157

Newbie level 6
Joined
May 14, 2012
Messages
11
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,362
well, it is actually a pfc converter, the boost converter is meant to work in dcm so that the inductor currents become spikes with a sinusoidal shape (input voltage reference). Filtered out they become a nice sine with a thd of about 10% :)

hmm. i removed the rectifier's ground. now simulation reaches 4ns and then stops again.
 

BradtheRad

Super Moderator
Staff member
Joined
Apr 1, 2011
Messages
13,804
Helped
2,738
Reputation
5,473
Reaction score
2,648
Trophy points
1,393
Location
Minneapolis, Minnesota, USA
Activity points
103,031
1.

Try installing small 'token' resistors in the same wires with the capacitors.

2.

Try installing a token resistor inline with the pulse generator to your mosfet's gate.

3.

Try running an individual ground to components, rather than joining three ends together and then to a single ground.

4.

I see two places where there is a red dot on a wire close to a node, but not on a node. It looks as though wire ends are overlapped rather than directly joined.

- - - Updated - - -

The power-carrying loops might as well be a short circuit during the negative half of the AC cycle.

I have not been able to create a boost converter powered by AC sinewaves. (Although it is possible with a buck converter.)
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,854
Helped
14,119
Reputation
28,495
Reaction score
12,800
Trophy points
1,393
Location
Bochum, Germany
Activity points
277,754
well, it is actually a pfc converter, the boost converter is meant to work in dcm so that the inductor currents become spikes with a sinusoidal shape (input voltage reference). Filtered out they become a nice sine with a thd of about 10% :)
Yes, not bad for this simple circuit.
 

andreas157

Newbie level 6
Joined
May 14, 2012
Messages
11
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,362
the same topology runs ok in orcad. same values, same simulator options (reltol, max step size), even with an output volage pi controller.
i just wanted to use multisim wich is easier to use and most of all, does not crash unexpectedly. But it is weird that simulation does not start...
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,854
Helped
14,119
Reputation
28,495
Reaction score
12,800
Trophy points
1,393
Location
Bochum, Germany
Activity points
277,754
Different circuit simulators have different weaknesses regarding convergence problems. I'm not presently using Multisim and thus can't help with it's specific issues. There are some general points how to avoid respectively find workarounds for popular convergence problems with semiconductor components. I wonder if you have set realistic rise and fall times for the gate driver, at least none are shown in the schematic.
 

andreas157

Newbie level 6
Joined
May 14, 2012
Messages
11
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,362
:-D and it's sooooolved! Thanks for that. Rise/fall time were too low. Just increased them and everything is fine! Thanks again!
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top