Hi,
I have some trouble with the included colpitts 1Mhz schematics.
Why simulation works in LTSpice and in Orcad not works ?

Happy 2025
thx for help

 

Here schematics files

 

hi gmv,
Does Orcad require a RED dot to show an actual connection node, your diagram has missing dots??
The sim works OK in LTSpice.
E

 

hi gmv,
Does Orcad require a RED dot to show an actual connection node, your diagram has missing dots??
The sim works OK in LTSpice.
E

hi eric,
i double checked now all red dots are in right place

 

The schemes in the programs are different. Look at the value of C5.
Note: when calculating the oscillator at a frequency of 1 MHz, it is necessary to take the maximum time step of no more than 1% of the period. In this case, no more than 10 nsec.

 

The schemes in the programs are different. Look at the value of C5.
Note: when calculating the oscillator at a frequency of 1 MHz, it is necessary to take the maximum time step of no more than 1% of the period. In this case, no more than 10 nsec.

thx i fixed c5 and minimum step output is dampened

 

I wrote no more than 10 nsec. Make it smaller. Also try Reltol=1u . Also Trtol=1 how it is done in LTspice. Pspice has the disadvantage of dampening fluctuations. This is solved by reducing the time step and increasing the accuracy of the calculation.

 

See

 

I wrote no more than 10 nsec. Make it smaller. Also try Reltol=1u . Also Trtol=1 how it is done in LTspice. Pspice has the disadvantage of dampening fluctuations. This is solved by reducing the time step and increasing the accuracy of the calculation.

Sorry, set to 1n, Reltol=1u and Trtol =1


and i get

 

See
View attachment 339511

Yes in LtSpice it's works

 

You need to give an initial push. There are two ways. The first one: (I use it most often) to simulate turning on the power supply. This is the most realistic way. Second: set the initial current through the inductor. The final current has an amplitude of approximately 60 mA. To speed up the establishment of a constant level, I recommend reducing the flow capacity at the output of the oscillator.

 

You need to give an initial push. There are two ways. The first one: (I use it most often) to simulate turning on the power supply. This is the most realistic way. Second: set the initial current through the inductor. The final current has an amplitude of approximately 60 mA. To speed up the establishment of a constant level, I recommend reducing the flow capacity at the output of the oscillator.
View attachment 339520

View attachment 339521

Thankyou for all useful explanaitions

 

During the simulation in ORCAD, a poor transistor model was used - a very small value of VAF = 10. This greatly reduces the output conductivity and, as a result, the gain.
Yes, and some other parameters are different.
I have given the model below:
.subckt awb2n3904 C B E
+ params:
+ IC_VBE=1.10250E-36
+ IC_VCE=1.10250E-36
+ STATE=1
+ TEMP=0
+ AREA=1.0
+ STATE_FACTOR=0
+ IS=1.728E-16
+ BF=254.395
+ NF=0.85
+ VAF=10
+ IKF=0.0163741
+ ISE=9.97446E-15
+ NE=1.20863
+ BR=0.1
+ NR=0.891964
+ VAR=7.74046
+ IKR=0.163741
+ ISC=9.97446E-15
+ NC=2.84343
+ RB=28.3394
+ IRB=0.01
+ RBM=0.01
+ RE=0.00133911
+ RC=2.08353
+ CJE=4.56614E-12
+ VJE=0.4
+ MJE=0.245712
+ TF=4.81412E-10
+ XTF=0.9628
+ VTF=9.52193
+ ITF=0.0113328
+ PTF=0
+ CJC=3.72485E-12
+ VJC=0.4
+ MJC=0.236002
+ XCJC=0.8
+ TR=1.30399E-06
+ CJS=0
+ VJS=0.75
+ MJS=0.5
+ XTB=1.20888
+ EG=1.206
+ XTI=1.34879
+ KF=0
+ AF=1
+ FC=0.519152

LTspice:
.MODEL 2N3904test NPN(IS=4.639E-15 NF=0.9995 ISE=2.091E-14 NE=1.6 BF=160.1 IKF=0.12
+ VAF=98.69 NR=1.001 ISC=3.257E-12 NC=1.394 BR=5.944 IKR=0.06
+ VAR=19.29 RB=1 IRB=1E-6 RBM=1 RE=0.3614 RC=1.755 XTB=0
+ EG=1.11 XTI=3 CJE=5.631E-12 VJE=0.7002 MJE=0.3385
+ TF=3.001E-10 XTF=27 VTF=1.461 ITF=0.2723 PTF=0 CJC=4.949E-12
+ VJC=0.5969 MJC=0.1928 XCJC=0.864 TR=9.4E-8 CJS=0 VJS=0.75
+ MJS=0.333 FC=0.5582)

 

I took the NETLIST from both programs with models and calculated it in Qspice. With ORCAD on the top chart (red)- there are no fluctuations. LTspice lower chart (blue) the oscillations are present. Conclusion: programs should be compared with the same models, and preferably with the correct models.