UcD Oscillation Matter

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Hai.. Guys. I'm doing on UcD class D amplifier based on Philip UM10155 . I'm having problem in oscillate the UcD amplifier in order to simulate the desire sine wave . My Vin is 5V sine wave , with the frequency of 1K. My output is only 1.1 V. Can you guys give some advice on the way to oscillate the amplifier? Really appreciate if you all can help me.
 

Attachments

  • graph2.JPG
    graph2.JPG
    210.3 KB · Views: 473
  • Schematic2.JPG
    Schematic2.JPG
    427.9 KB · Views: 468
I think there is an error in the scheme.

Thanks for the useful advice. I managed to oscillate the amplifier. Really thanks for your help. Do you know any reason that caused my Vout is only simulate 30mv to -210mv sine wave?
what device and parameter that I need to change in order to get desire output waveform?
 

Attachments

  • Graph2.JPG
    Graph2.JPG
    245.7 KB · Views: 376
  • schematic2.JPG
    schematic2.JPG
    276.4 KB · Views: 345
If you are not getting rail-to-rail waveforms at the junction of the output fets and the filter inductor, it is not oscillating.

Change the MEG OHM resistors to xxxxK. LTSPice interprets M as milliohms, I think. That is R14 and R15 on the original schematic.
J3 has to be tied to J4, grounded, to work. Read section 6.1 about enabling the amp.

Any errors flagged from the models? There is a Class D folder on the Yahoo pages for LTSPice users with complete Class D amps ready to go and very easy to simulate. Similiar to UM10155.
 
If you are not getting rail-to-rail waveforms at the junction of the output fets and the filter inductor, it is not oscillating.

Change the MEG OHM resistors to xxxxK. LTSPice interprets M as milliohms, I think. That is R14 and R15 on the original schematic.
J3 has to be tied to J4, grounded, to work. Read section 6.1 about enabling the amp.

Any errors flagged from the models? There is a Class D folder on the Yahoo pages for LTSPice users with complete Class D amps ready to go and very easy to simulate. Similiar to UM10155.


Really thankful for your advice.
The rail to rail waveforms are sine waves? Yes. I changed the to xxxxK but it didn't bring any effect at all. I had also tied j3 and j4 and grounded them.
There was no error. Just some warnings.

Instance "m:u5:2": Length shorter than recommended for a level 3 MOSFET.
Instance "m:u5:1": Length shorter than recommended for a level 3 MOSFET.
Instance "m:u4:2": Length shorter than recommended for a level 3 MOSFET.
Instance "m:u4:1": Length shorter than recommended for a level 3 MOSFET.

Do the warnings matter?
 

Attachments

  • schematic3.JPG
    schematic3.JPG
    288 KB · Views: 106
  • graph3.JPG
    graph3.JPG
    184.4 KB · Views: 116
The warnings tell me that you have some problems with the models U5 and U4, the MOSFETS. Where did you get the models? Did you add them correctly to LT Spice??

When you added them to the schematic, did you right click the mouse on the symbol for the NMOS and do a "pick new MOSFET"?? Choose the STD30NF06L or PHM21NQ15T to get you started. These models are included in the standard download of LTSpice. Once you get things working you can change models.

The waveform at the left hand terminal of the inductor, L1, should be a square (rectangular) wave not sine wave.

I see about 100's of millivolts after the filter of 200Khz to 500Khz on the output of my simulations. Plus I see the audio I put into the input, amplified of course. What frequency do you think your circuit is oscillating?
 
The warnings tell me that you have some problems with the models U5 and U4, the MOSFETS. Where did you get the models? Did you add them correctly to LT Spice??

When you added them to the schematic, did you right click the mouse on the symbol for the NMOS and do a "pick new MOSFET"?? Choose the STD30NF06L or PHM21NQ15T to get you started. These models are included in the standard download of LTSpice. Once you get things working you can change models.

The waveform at the left hand terminal of the inductor, L1, should be a square (rectangular) wave not sine wave.

I see about 100's of millivolts after the filter of 200Khz to 500Khz on the output of my simulations. Plus I see the audio I put into the input, amplified of course. What frequency do you think your circuit is oscillating?



I get the model from npx. I inserted the Mosfet by cracking it in the sub and sym which I learned from Forum.

I had simulated it with PHM21NQ15T. The result is the same like the previous model.The waveform at the left hand terminal of the inductor, L1, is a square wave.

Can I know how you perform your transient analysis? What V(input) that you put?

I set my Vinput as sine wave which has 1V amplitude and frequency of 200KHz. I get my Vout value which variate between 20mV and 28mV. Does this meant that my signal is not amplifier-ed?
 
I had simulated it with PHM21NQ15T. The result is the same like the previous model.The waveform at the left hand terminal of the inductor, L1, is a square wave.

Good!



I set my Vinput as sine wave which has 1V amplitude and frequency of 200KHz. I get my Vout value which variate between 20mV and 28mV. Does this meant that my signal is not amplifier-ed?

You should be using audio frequencies. 200Khz is too high. I use 1.4 volts (peak) and frequencies from 100 hz to 20Khz.


When you set the input voltage source to zero, what do you see on the output?? When I simulated this design, I saw 100's of millivolts of DC offset, which is too high. There is no pot to adjust the output offset. Plus there is no real current limiting either. This design is incomplete, IMHO, and should be built and used with care.
 
There's another problem with your schematic: bottom end of C8 should connect to the node common to D6 anode, R24, U6 collector, U4 source etc., not to U8 cathode.

For frequency domain modelling, you can build a small-signal equivalent circuit, which can be helpful in terms of designing additional active loop-compensation. See Bruno's paper on the amplifier.

For modelling distortion, you could try a time-domain FFT analysis.

There aren't many components in the amplifier and PCB layout will play a significant role in its performance, so better to build it and measure it in real life ;)
 
my imd

Hai..guys. I had successfully simulated my thd with .four . My thd is around 0.03 which is almost the same with the manufacture datasheet. I had simulated my IMD. But I had problem on how to determine the value of my IMD. I inserted a series voltage supplies , 9.5KHz and 10.5KHz in my Vin. Both of my sidebandsi amplitude is below -100db. My amplitude in the graph at 9.5KHz and 10.5Hz are both -33.dB . The rest are mostly below -100db. So can I know the way to determine my IMD?
 

Attachments

  • IMD2.JPG
    IMD2.JPG
    135 KB · Views: 188
  • IMDcircuit.JPG
    IMDcircuit.JPG
    289 KB · Views: 197
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.