Loading User defined code model.

[Fahim]

Hi,
I am new to the Ngspice/Xspice.

I am trying to create the new code model. I have created the interface and model file.

Can anyone please tell me the steps to load the new code model. he code is as below please let me know if the usage of new code model is proper or not

Small Signal Amplifier
*
*This circuit simulates a small signal amplifier
*with a diode limiter.
*
.dc Vin -1 1 .05
*
Vin       Input common             DC 0
R_source Input Amp_In         100
*
D_Neg 0   Amp_In              1n4148
D_Pos     Amp_In common            1n4148
*
C1        Amp_In common            1uF
A1        Amp_In common Amp_Out    Amp
R_Load    Amp_Out common           1000
*
.model 1n4148 D (is=2.495E-09 rs=4.755E-01 n=1.679E+00
+ tt=3.030E-09 cjo=1.700E-12 vj=1 m=1.959E-01 bv=1.000E+02
+ ibv=1.000E-04)
*
.model Amp Amplifier (gain = -10 in_offset = 1e-3
+                     rin = 1e6 rout = 1e1)
*
.end

Regards
Fahim

[Fahim]

The new code model is Amplifier. Thanks

[Holger Vogt]

Fahim,

please have a look at the actual manual
http://ngspice.sourceforge.net/docs/ngspice-manual.pdf
chapters 25.3 and  27.2 ff

Regards

Holger

[Fahim]

Hi Holger,

I have follow the same steps to create the model but its still not working and giving above error.

Could please let me know if there is any error in the code given above.

Regards,
Fahim

[Holger Vogt]

Fahim,

you have to be more specific:

What error message?

Correctness of usage depends on your new code model!
What are the new interface specifications?

Holger

[Holger Vogt]

Fahim,

please also have a look at the manual, chapter 2.1 on the gnd node!

Holger

[Fahim]

Hi Holger,

I am getting the below error.

Error on line 15 : a1 amp_in common amp_out amp
MIF-ERROR - unable to find definition of model amp
Model issue on line 22 : .model amp amplifier (gain=-10 in_offset=1e-3 rin=1e6 ro …
Unknown model type amplifier - ignored

Regards,
Fahim

[Fahim]

Regarding the ground model I have one common branch in my model which act as ground.

To check whether this causing the problem I deleted the port in the interface file and use it as gnd.

But still its giving me error.

[Holger Vogt]

Fahim,

you have to replace 'common' by 'gnd'.

The error message however tells you that your new code model has not been recongnized by ngspice.

The only way to help you may be that you decribe what you did 'step by step'.

Holger

[Fahim]

Hi,

I have changed the common with gnd also but still getting same error.

I had follow the below steps.

Step1: Created the new directory under ngspice/src/xspice/icm/xtradev as Amplifier.
Step2 : Copied interface and cmodel file in it.
Step3: did the necessary changes in it.
Step4: Added name of code model in the modpath.lst file.
Step5: Now to load the codemodel I created the release directory under the ngspice directory.
step6:  cd release
step7:  ../configure -enable-xspice -disable-debug -with-readline=yes
Step8: make
Step9 : sudo make install

[Holger Vogt]

as a short test, replace
.model Amp Amplifier (gain = -10 in_offset = 1e-3  rin = 1e6 rout = 1e1)
by

.model Amp gain(gain = -10 in_offset = 1e-3)

Holger

[Fahim]

I had use the existing model gain and it was running without any error.

Regards,
Fahim

[Holger Vogt]

next test:
to see if codemodel has been made, goto :
ngspice/release/src/xspice/icm/xtradev/amplifier
Is there a cfunc.c, cfunc.o, ifspec.c ifspec.o ?

Holger

[Fahim]

Yes its there.

Should I uninstall ngspice and then install it again?

Fahim

[Holger Vogt]

yes
try a
make clean
first. You may then do
make 2>&1 | tee make.log
instead of
make
, which gives you a make.log file in dir ngspice for analysis.

Holger

[Holger Vogt]

make uninstall

will remove the installed files.

Holger

[Holger Vogt]

correction:

make.log to be found in ngspice/release

Holger

[Fahim]

I checked the log in release but no error for creating .c and .o file.
make uninstall will uninstall the ngspice correct?

Fahim

[Holger Vogt]

just another idea:

ngspice internally sets all command lines to lower case letters before execution.
Please rename your code model accordingly:
Amplifier --> amplifier
and try again.

Holger

[Fahim]

I try it but still not working

Fahim

[Holger Vogt]

next step:

Could you please list your input files:
cfunc.mod and ifspec.ifs.

I will cheeck if there is something irregular.

I have easily been able to generate a XSPICE model 'amplifier' using the procedure described.

Regards

Holger

[Fahim]

/*ifspec.ifs*/

NAME_TABLE:

C_Function_Name:       ucm_amplifier
Spice_Model_Name:      amplifier
Description:           "A simple gain block"

PORT_TABLE:

Port_Name:             amp_in            amp_out
Description:           "input"           "output"
Direction:             in                out
Default_Type:          v                 v
Allowed_Types:          
Vector:                 no               no
Vector_Bounds:          -                -
Null_Allowed:          no                no

PARAMETER_TABLE:

Parameter_Name:     in_offset           gain        rin                 rout
Description:        "input offset"      "gain"      "input resistance"  "Output resistance"
Data_Type:          real                real        real real
Default_Value:      0.0                 1.0         0.0                 0.0
Limits:             -                   -           -                   -
Vector:              no                  no         no                  no
Vector_Bounds:       -                   -          -                   - 
Null_Allowed:       yes                 yes         yes                 yes   

[Fahim]

/*cfund.mod*/

/*=== UCM_AMPLIFIER ROUTINE ===*/
                                                  

void ucm_amplifier(ARGS)   /* structure holding parms, inputs, outputs, etc.     */
{
    Mif_Complex_t ac_gain;

    if(ANALYSIS != MIF_AC) {
        OUTPUT(amp_out) =  PARAM(gain) *((PARAM(rout))*(PARAM(rin)) + PARAM(in_offset));
        PARTIAL(amp_out,amp_in) = PARAM(gain);
    }
    else {
        ac_gain.real = PARAM(gain);
        ac_gain.imag= 0.0;
        AC_GAIN(amp_out,amp_in) = ac_gain;
    }

}

[Holger Vogt]

Hi,

I did not detect a princple bug, was able do generate a new code model 'amplifier' according to (MS Windows, MINGW compiler):

Step1: Created the new directory under ngspice/src/xspice/icm/xtradev as Amplifier.
Step2 : Copied interface and cmodel file in it.
Step3: did the necessary changes in it.
Step4: Added name of code model in the modpath.lst file.
Step5: cd 'ngspice directory'
step6: cd release
step7: ../configure -enable-xspice -disable-debug -with-readline=yes
Step8: make clean
Step9 : make
step 10: make install

However I changed line
OUTPUT(amp_out) = PARAM(gain) *((PARAM(rout))*(PARAM(rin)) + PARAM(in_offset));
(not input, gain multipled by resistance?) back to
OUTPUT(amp_out) =  PARAM(gain) *(INPUT(amp_in) + PARAM(in_offset));
all common to gnd in the input file,
and everything works well!

Holger

[Fahim]

Hi Holger,

I think there should not be problem with above statement because it is creating the .c and .o file without any error.

However I changed the cmod file but still it is not working. Could you please share the files.