(P)Spice Model wanted

dc motor spice model

Hi friends,

i search a spice model for a "brushless dc motor".
I will use it to simulate a sensorless brushless dc motor control unit.

Thanks a lot

Regards

dc motor spice

Hi friend!

I have bee looking for the same now for a week . I have found several DC models but all are very much the same I need a tachometer output as pulses .. so i modified this model
This is one of the most complete that i found .. Now i trying to get the mechatronics lib from INTUSOFT i think that one is pretty good
If you find it .let me know ..

.SUBCKT MOTOR 1 2 3 4 5 PARAMS:RA=1M LA=1NH KE=7.06M KT=1 JM=1P
+ BM=1N KTC=1M KS=1G BKS=1N
+ CONV=.10472
* DC MOTOR WITH ARMATURE CONTROL
* NODE 1 IS POSITIVE MOTOR ARMATURE VOLTAGE
* NODE 2 IS NEGATIVE MOTOR ARMATURE VOLTAGE
* NODE 3 IS MOTOR SHAFT SPEED IN RAD/SEC RELATIVE TO SPACE
* NODE 4 IS MOTOR PLATFORM SPEED IN RAD/SEC RELATIVE TO SPACE
* NODE 0 IS SPACE REFERENCE
* NODE 5 IS TACH OUTPUT IN VOLTS OF MOTOR SPEED RELATIVE TO PLATFORM
* CURRENT OUT OF NODE 3 IS TORQUE DELIVERED IN OZ-IN
* UNITS : OZ,IN,RAD/SEC
* RA IS ARMATURE RESISTANCE IN OHMS
* LA IS ARMATURE INDUCTANCE IN HENRIES
* KE IS MOTOR BACK EMF CONSTANT IN VOLTS/RAD/SEC
* KT IS MOTOR TORQUE CONSTANT IN OZ-IN/AMP
* JM IS MOTOR INERTIA IN OZ-IN-SEC/RAD/SEC
* BM IS MOTOR VISCOUS FRICTION IN OZ-IN/RAD/SEC
* KS IS MOTOR SPRING CONSTANT IN OZ-IN/RAD
* BKS IS SHAFT SPRING DAMPING IN OZ-IN/RAD/SEC
* KTC IS TACHOMETER GAIN CONSTANT IN VOLTS/RPM
* CONV IS RPM TO RAD/SEC CONVERSION CONSTANT = 2PI/60
RA 1 8 {RA}
LA 8 6 {LA}
VA 6 7
EB 7 2 VALUE = {KE*V(9,4)}
GTM 4 9 VALUE = {KT*I(VA)}
CJM 9 0 {JM}
RBM 9 4 {1/BM}
LKS 9 3 {1/KS}
RKS 9 3 {1/BKS}
ETC 5 0 VALUE = {KTC*V(3,4)/CONV}
RTC 5 0 1G
RL 3 4 1G
.ENDS MOTOR

bldc spice

Hi,

such a model is included in Pspice Libraries (Orcad Version 9.2)
You'll find it in the model library mix_misc.slb
It name is simply BLDCM.
This model include all the parameter that are important for a BLDC Motor.

A simulation example is also include in ..\Pspice\schematics_sample\mixsim\motordrv\...

Bye reiniheini

pspice motor model

Have you ever tried to simulate this schematic ?

I always get the Error Message

I/O ERROR -- Unable to open stimulus file "motor.stm"....

spice brushless model

hi Vauxdvihl

yes, i`ve simulated this schematic...
Usually this file should be in the directory where the schematic file is.

But something seems to be happen with your file....

Try that one I enclosed to this post!

Regards reiniheini