Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
Search
Need help in oscilation of UcD
|
raymond
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.
I post my schematic and graph under in the file name of U10155ray.rar. |
|
Please upload your .asc schematic file. The .asc schematic file is needed to troubleshoot your simulation.
toggle quoted message
Show quoted text
Howard raymond wrote: 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. |
|
raymond hui
I had upload my schematic in here and also in temp file under the name of ? . Thanks for the help,Howard.
toggle quoted message
Show quoted text
--- On Tue, 11/24/09, Howard Hansen <hrhan@...> wrote:
From: Howard Hansen <hrhan@...> Subject: Re: [LTspice] Need help in oscilation of UcD To: LTspice@... Date: Tuesday, November 24, 2009, 2:58 AM ? Please upload your .asc schematic file. The .asc schematic file is needed to troubleshoot your simulation. Howard raymond wrote: 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. I post my schematic and graph under . groups.yahoo. com/group/ LTspice/files/ %20Temp/ in the file name of U10155ray.rar. ------------ --------- --------- ------ Yahoo! Groups Links [Non-text portions of this message have been removed] |
|
Sorry I should have been more explicit. Except for the raw file, you need to Zip every file in the directory that contains your schematic and upload the zip file to temp directory. When I opened UM10155.asc LTspice says there were 5 missing symbols.
toggle quoted message
Show quoted text
Howard raymond hui wrote: I had upload my schematic in here and also in temp file under the name of . Thanks for the help,Howard. |
|
raymond hui
Really appreciate for your willingness to help me. I had zip my schematic in UM10155_4.zip under temp. I had modified some of the model because I imported some of the model into LPspice. I still unable to make the amplifier oscillate . My Vout is a pulse wave which has the value variate from 16mv to 33mv.? My pwm waveform is also very strange.
toggle quoted message
Show quoted text
Many Thanks, Raymond --- On Tue, 11/24/09, Howard Hansen <hrhan@...> wrote:
From: Howard Hansen <hrhan@...> Subject: Re: [LTspice] Need help in oscilation of UcD To: LTspice@... Date: Tuesday, November 24, 2009, 11:42 AM ? Sorry I should have been more explicit. Except for the raw file, you need to Zip every file in the directory that contains your schematic and upload the zip file to temp directory. When I opened UM10155.asc LTspice says there were 5 missing symbols. Howard raymond hui wrote: I had upload my schematic in here and also in temp file under the name of . groups.yahoo. com/group/ LTspice/files/ %20Temp/Um10155. asc . Thanks for the help,Howard. --- On Tue, 11/24/09, Howard Hansen <hrhan@...> wrote: From: Howard Hansen <hrhan@...> Subject: Re: [LTspice] Need help in oscilation of UcD To: LTspice@yahoogroups .com Date: Tuesday, November 24, 2009, 2:58 AM Please upload your .asc schematic file. The .asc schematic file is needed to troubleshoot your simulation. Howard raymond wrote: 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. I post my schematic and graph under . groups.yahoo. com/group/ LTspice/files/ %20Temp/ in the file name of U10155ray.rar. ------------ --------- --------- ------ Yahoo! Groups Links ------------ --------- --------- ------ Yahoo! Groups Links [Non-text portions of this message have been removed] |
Really appreciate for your willingness to help me. I had zip my schematic Many Thanks,Hi Raymond, I modelled the UM10155 from the datasheet - the tran waveform does start off as a smallish squarewave then settles into a nice sine wave after 20-30ms using the tran command below: .tran 0 100m 0 1u startup uic I didn't find a model for the output devices or one of the diodes, but otherwise my circuit is as the datasheet. Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.81/2524 - Release Date: 11/24/09 19:37:00 |
|
raymond hui
Hi Dave,
toggle quoted message
Show quoted text
Did you modified any of the resistance and capacitance value in the UM10155? What is the Vin for your simulation? What value that you gained in the Vout ? Thanks a lot for your information. Best Regards, Raymond --- On Wed, 11/25/09, Dave Allen <cdcat001@...> wrote:
From: Dave Allen <cdcat001@...> Subject: Re: [LTspice] Need help in oscilation of UcD To: LTspice@... Date: Wednesday, November 25, 2009, 4:20 PM ? >Really appreciate for your willingness to help me. I had zip my schematic in UM10155_4.zip under temp. I had modified some of the model because I imported some of the model into LPspice. I still unable to make the amplifier oscillate . My Vout is a pulse wave which has the value variate from 16mv to 33mv. My pwm waveform is also very strange. Many Thanks, Raymond Hi Raymond, I modelled the UM10155 from the datasheet - the tran waveform does start off as a smallish squarewave then settles into a nice sine wave after 20-30ms using the tran command below: .tran 0 100m 0 1u startup uic I didn't find a model for the output devices or one of the diodes, but otherwise my circuit is as the datasheet. Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.81/2524 - Release Date: 11/24/09 19:37:00 [Non-text portions of this message have been removed] |
Hi Dave, Did you modified any of the resistance and capacitance value in the Best Regards,Hi Raymond, Vin is set at 1.8v 1Khz out is 48v peak to peak approx with 30-0-30v power. I haven't checked this is the correct gain figure as I only modeled it out of curiosity. You did remember the enable link between J3 and J4 and a 4R load between J10 and J11 ? Having checked again the tran only settles around 50ms and takes an age to get there. There's a little of the switching waveform at the output - much more before the output choke! I haven't downloaded your version to check, but I can upload mine, such as it is. Sorry, won't be today though. Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.81/2524 - Release Date: 11/24/09 19:37:00 |
|
raymond hui
--- On Thu, 11/26/09, Dave Allen <cdcat001@...> wrote:
From: Dave Allen <cdcat001@...> Subject: Re: [LTspice] Need help in oscilation of UcD To: LTspice@... Date: Thursday, November 26, 2009, 1:07 AM ? >Hi Dave, Did you modified any of the resistance and capacitance value in the UM10155? What is the Vin for your simulation? What value that you gained in the Vout ? >Thanks a lot for your information. Best Regards, Raymond Hi Raymond, Vin is set at 1.8v 1Khz out is 48v peak to peak approx with 30-0-30v power. I haven't checked this is the correct gain figure as I only modeled it out of curiosity. You did remember the enable link between J3 and J4 and a 4R load between J10 and J11 ? Having checked again the tran only settles around 50ms and takes an age to get there. There's a little of the switching waveform at the output - much more before the output choke! I haven't downloaded your version to check, but I can upload mine, such as it is. Sorry, won't be today though. Regards Dave Hi Dave,The J3 and J4 is? grounded in my schematic. Is it correct? Yes. I connected J3 and J4 with a 4 ohm resistor.? When you can upload your version ? I would like to have a look on how it simulate? Many Thanks,Raymond [Non-text portions of this message have been removed] |
|
Raymond, I agree there is something wrong in the model of a UM10155 you uploaded to the Temp folder. For an input sine wave with a 1 volt peak amplitude the output amplitude should be approximately 46 volts peak to peak. Instead I was seeing a peak to peak output in the millivolt range. Just as troubling was the very low amplitude of the signals at the gates of the power MOSFETs. I will keep looking to see if I can find the problem and will post message is I find the source of the problem.
toggle quoted message
Show quoted text
Howard raymond hui wrote: Really appreciate for your willingness to help me. I had zip my schematic in UM10155_4.zip under temp. I had modified some of the model because I imported some of the model into LPspice. I still unable to make the amplifier oscillate . My Vout is a pulse wave which has the value variate from 16mv to 33mv. My pwm waveform is also very strange. |
|
Dave,
toggle quoted message
Show quoted text
I'm not sure what else is wrong but C6 and C8 are probably not correct. regards Robert --- In LTspice@..., raymond hui <rcch87@...> wrote:
|
Dave,regards RobertRobert, Raymond I've uploaded the UM10155 file from my machine as UM10155.asc in the temp folder - I've checked, it oscillates with or without input. I'll leave the rest as an exercise for the reader! BTW - the component refs on this schematic <don't> match the datasheet. Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.82/2525 - Release Date: 11/25/09 07:31:00 |
|
--- In LTspice@..., "Dave Allen" <cdcat001@...> wrote:
Hello Dave,Dave,robably not correct. I miss the model BF824 and BF721 to run the simulation. Please provide(upload) the model. Best regards, Helmut ---------- |
|
Dave,
toggle quoted message
Show quoted text
I also modified the circuit to get it oscillating reliably. my changes are also in the temp directory. regards Robert --- In LTspice@..., "Dave Allen" <cdcat001@...> wrote:
Dave,regards |
Hello Dave, I miss the model BF824 and BF721 to run the simulation. Best regards,Hi Helmut, Strange that - they're in my standard.bjt file! .MODEL BF721 PNP(IS=5.35E-16 ISE=9.81E-17 ISC=1.00E-13 XTI=3.00 BF=1.40E2 BR=1.00E-2 IKF=2.41E-2 IKR=1.00 XTB=1.5 VAF=1.49E2 VAR=9.18E1 VJE=3.00E-1 VJC=3.00E-1 RE=1.85E-2 RC=2.22 RB=1.99E1 RBM=2.41E-2 IRB=1.10E-2 CJE=4.20E-11 CJC=1.65E-11 XCJC=1.00 FC=5.00E-1 NF=8.73E-1 NR=9.84E-1 NE=1.03 NC=2.00 MJE=4.13E-1 MJC=7.00E-1 TF=1.11E-9 TR=0 PTF=0 ITF=3.00 VTF=9.99E5 XTF=5.76E2 EG=1.11 KF=1E-9 AF=1 VCEO=40 ICRATING=800M MFG=SIEMENS) .MODEL BF824 PNP(IS=2.948E-16 ISE=1.879E-14 ISC=2.21E-15 XTI=3 BF=42 BR=1.5 IKF=0.05266 IKR=0.05 XTB=1.5 VAF=35 VAR=33.62 VJE=0.7113 VJC=0.4038 RE=0.1038 RC=4.2 RB=1 RBM=0.5 IRB=1E-06 CJE=2.453E-12 CJC=3.237E-12 XCJC=0.0464 FC=0.8618 NF=0.99 NR=0.9809 NE=2.469 NC=1.25 MJE=0.3218 MJC=0.3117 TF=2.602E-10 TR=1E-32 PTF=0 ITF=0.1748 VTF=2.773 XTF=9.349 EG=1.11 KF=1E-9 AF=1 MFG=PHILIPS) Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.82/2525 - Release Date: 11/25/09 07:31:00 |
|
Robert, Thank You for fixing the UM10155 schematic to get the circuit to amplify an input signal. So Raymond will know what was done I will mention you eliminated C6 and C8 and corrected a wiring mistake. The wire going from the emitter of Q12 to the anode of D3 was connected to the wrong terminals in Raymond's schematic. The problem with C6 and C8 seems unusual. Dave Allen version of the UM10155 power amplifier includes C6 and C8 and he says his version works. This seems to imply it makes a difference as to what type of transistors are used as whether C6 and C8 are required.
toggle quoted message
Show quoted text
Howard RobertTalty wrote: Dave, |
Robert, Thank You for fixing the UM10155 schematic to get the circuit toamplify an input signal. So Raymond will know what was done I will mention you eliminated C6 and C8 and corrected a wiring mistake. The wire going from the emitter of Q12 to the anode of D3 was connected to the wrong terminals in Raymond's schematic. The problem with C6 and C8 seems unusual. Dave Allen version of the UM10155 power amplifier includes C6 and C8 and he says his version works. This seems to imply it makes a difference as to what type of transistors are used as whether C6 and C8 are required. HowardGood morning, The UM10155.asc file in the temp directory is the one I uploaded yesterday. This is as per the datasheet except that I didn't follow the circuit references exactly! The models of BF824 and BF721 were posted in my reply to Helmut yesterday ... though for some reason I have them in my standard.bjt file. I never downloaded Raymond's original circuit so C6 and C8 don't register with me. The 100u 100n combination? Reservoir for the gate switching? I was originally interested in the circuitry driving the output devices as this gives a rapid discharge of the gate capacitance. Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.83/2528 - Release Date: 11/26/09 09:10:00 |
|
raymond hui
Thanks, Guys. I"m able to oscillate my amplifier.In my case, C6 and C8 need to eliminate in order for my amplifier to oscillate . In this model, it is impossible to perform DC and AC analysis. Am I right? In order to calculate THD and IMD, what steps and analysis that I need to do ?
toggle quoted message
Show quoted text
Regards, Raymond --- On Fri, 11/27/09, Dave Allen <cdcat001@...> wrote:
From: Dave Allen <cdcat001@...> Subject: Re: [LTspice] Re: Need help in oscilation of UcD To: LTspice@... Date: Friday, November 27, 2009, 3:38 PM ? >Robert, Thank You for fixing the UM10155 schematic to get the circuit to amplify an input signal. So Raymond will know what was done I will mention you eliminated C6 and C8 and corrected a wiring mistake. The wire going from the emitter of Q12 to the anode of D3 was connected to the wrong terminals in Raymond's schematic. The problem with C6 and C8 seems unusual. Dave Allen version of the UM10155 power amplifier includes C6 and C8 and he says his version works. This seems to imply it makes a difference as to what type of transistors are used as whether C6 and C8 are required. Howard Good morning, The UM10155.asc file in the temp directory is the one I uploaded yesterday. This is as per the datasheet except that I didn't follow the circuit references exactly! The models of BF824 and BF721 were posted in my reply to Helmut yesterday ... though for some reason I have them in my standard.bjt file. I never downloaded Raymond's original circuit so C6 and C8 don't register with me. The 100u 100n combination? Reservoir for the gate switching? I was originally interested in the circuitry driving the output devices as this gives a rapid discharge of the gate capacitance. Regards Dave ---------- No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.709 / Virus Database: 270.14.83/2528 - Release Date: 11/26/09 09:10:00 [Non-text portions of this message have been removed] [Non-text portions of this message have been removed] |
|
Howard,
toggle quoted message
Show quoted text
I don't think my corrections are optimal. maybe there is some purpose in having such oversized bootstrap capacitors. All that I could see was an excessive transient load on the gate voltage regulator circuit. Raymond, you should be able to run transient simulations as is. to see the distortion you do an FFT of the audio bandwidth filtered output signal, usually a 4th order LC filter at 30khz is required. remember to run the simulation with Alternative solver .options plotwinsize=0 max step size appropriate for the number of FFT points I'd use about 11msec simulation, start saving at say 1msec and use FFT with no window and 65536 points. The power supplies need to be done correctly with the appropriate capacitors and filter inductors. BTW you also need to add series diodes to the voltage sources because Single Ended classD amps result in "supply pumping" with effects distortion. I think most commercial versions of this circuit add a first order integrator stage ahead of the amplifier, which gets some "noise shaping" but even without an integrator this you should get a 3rd and 5th harmonic at about -90dB. regards Robert --- In LTspice@..., Howard Hansen <hrhan@...> wrote:
|
to navigate to use esc to dismiss