Products Mentioned

LTspice Production
LTspice® is a powerful, fast, and free SPICE simulator software, schematic capture and waveform viewer with enhancements and models for improving the simulation...
LTspice on Analog.com

Related Questions

Thread Details

  • State Verified Answer
  • Replies 4 replies
  • Subscribers 9 subscribers
  • Views 236 views
  • Users 0 members are here

Download the Latest Version of LTspice

Options
Related Content

        

            Post
             Go back to editing
        

    

    


    

    









		


















	
	
			
	
			
		
	
	
		

	    
	    
	    		
Follow-up on TPA3116D2 Simulation in LTspice

		
	
				

			

									
					    ReneOST
					
							

            
            			
				
									
											
			
			
				
    
			
			
			    	
			                    
                
				                on Nov 6, 2025 
				
			
			
		
    
		
		                     
				
        		
    
		    
		    		    
    
		      		            		        
    Category: Software
    
    		        		            		    
    Product Number:  LTspice  
    
    		        		        		        
    Software Version: 24.1.10
    
    		    		    
    
		    		    
		    			
    
			    
    Hello Mathias,
    

    Unfortunately, I have to reach out to you again regarding this topic. I’m now using the latest version of LTspice and trying to simulate the Class D amplifier TPA3116D2. With the alternate solver, the simulation does run, but as mentioned before, I still get unrealistically high output voltages of around 250 V — which obviously cannot be correct.
    

    Previously, the simulation worked fine with version 24.0.12, but now I can’t achieve any reasonable output voltage levels anymore, despite trying several adjustments. Our students are all using the newest LTspice version, and installing an older version is quite difficult to manage.
    

    Do you have any further suggestions or ideas on how to resolve this issue?
    

    Thank you very much for your help!
    

    Best regards,
     René
    

    TPA3116D2.LIBTPA3116D2.asytest_amp3.asc
    
			
    
			
									
		                             
                        

    
    
                                            
                 software
                
                                                    
                 LTspice
                
                                                    
                 24.1.10
                
                                
            
    
    
    
		
    

				
				        
        		
    
			
						
									
												
			
			
                        
                                    
                        
                        
                        
            
			            
						
						
			
			
			
			
		
    

        
        
        
    
					
    
			
    


    
















    
	
    
	
    
					



			


				
	









	
      
	

    • 
	

      • 

	

    • 
	
      



	
		
	
	



      
	
      
		
      
							
					
      
		
      
		    
		    		    
			
				
									
							        
			
			
			
      •  Analog Employees  
      
            
						
                            
            
            				
            
                on Nov 6, 2025 3:04 PM
            
            
												
						in reply to ReneOST
					
										
			            		
      
		
										0
					
	
      

		
		
      
		
      
                                
                                                            
      
					
      Hi  ,
      

      Without doing anything yet, running with UIC is highly discouraged. I'll take a look.
      

      mike
      
			
      

		
			
	      

		
		
	
      
	
      
		
      
			
		
      
	
      
	
      
		
						
						
				
						
				
				
		
		
      
			
		
      
	
      

      

      • 

	

    • 
	
      



	
			
		
	



      
	
      
		
      
							
					
      
		
      
		    
		    		    
			
				
									
							        
			
			
			
      •  Analog Employees  
      
            
						
                            
            
            				
            
                on Nov 7, 2025 9:43 AM
            
            
						
			            		
      
		
										0
					
	
      

		
		
      
		
      
                                
                                                            
      
					
      Dear  ,
      

      Please accept my appologies for not looking thoroughly enough into this matter. Your case reveales that there is a bug in the entire 24.1 line that causes some dependent sources with POLY(n) to be evaluated incorrectly. The next release will have this corrected. Thanks for insisting!
      

      Meanwhile, I can offer to just change the TPA3116D2.LIB as workaround. I can't post the file here (for copyright reasons) but the changes are simple:
      

      Replace line 304 with:
      VEBETA VBETA 0 1.852
      

      and line 306 with:
      bg1 d s i=v(d,s)*v(g)*v(vbeta)
      

      and line 435 with:
      BE8 RAMP NET112 v=62.5e-3*v(NET0141)*v(PVCC)
      

      

      In addition, don't use the .tran UIC flag. Instead:
      

      .tran 0 5ms 0 startup
      

      Run it with the gear integrator and optionally with
      

      .options itl4=40
      

      The latter makes the simulation a bit faster.
      

      However, even with these changes, I don't get a clean sinusoidal signal like on your screenshots. (Neither in 24.1.10, 24.0.12 nor in LTspiceXVII)
      

      Best Regards,
      Mathias
      
			
      

		
			
	      

		
		
	
      
	
      
		
      
			
		
      
	
      
	
      
		
						
						
						
						
				
				
		
		
      
			
		
      
	
      

      

      • 

	

    • 
	
      



	
		
	
	



      
	
      
		
      
							
					
      
		
      
		    
		    		    
			
				
									
							        
			
			
			
        
            
						
                            
            
            				
            
                on Nov 10, 2025 7:22 AM
            
            
												
						in reply to mborn
					
										
			            		
        
		
										0
					
	
        

		
		
        
		
        
                                
                                                            
        
					
        Dear Mathias,
        

        Thank you very much for your quick and extremely helpful reply.
         I applied the changes you suggested, and the simulation is now working correctly.
        

        The sinusoidal signal is also fine again — it was just an overdrive issue on my side.
        

        I’m glad that my case helped uncover a bug in the POLY(n) evaluation.
        


         Best regards from Switzerland,
         René Grabher
        
			
        

		
			
	      

		
		
	
        
	
        
		
        
			
		
        
	
        
	
        
		
						
						
				
						
				
				
		
		
        
			
		
        
	
        

        

        • 

	
      


      

	
			
      

      





		
      
		
      
			
        
				
      • 
					
												
						
						
						
						
						
						
						

																										
						
						

					
					
					
				
        •