SN74AHC1G126-EP: 74AHC1G126MDCKTEP

Ankit Jain

Part Number: SN74AHC1G126-EP

Hi,

I am simulating the behavior spice model of SN74AHC1G126-EP and observing one problem. When i am connecting the 3.3V source to OE pin with 10K in series, The voltage at OE pin is clamping to 550mV. When series resistance is changed to 1K the voltage at OE pin is 2.2V. Is this the issue with spice model? Please clarify.

I want to simply connect 3.3V power on OE pin through RC network to operate initially in high output impedance and then enable OE pin (Logic High) to pass input to output. But spice model is not working correctly on connecting series resistance.

Thanks

Regards,

Ankit Jain

over 3 years ago

0 Karan Kotadia over 3 years ago

TI__Genius 16725 points

Hi Ankit,

Yes it looks like it is a problem with the SPICE Model. Please give me some time to look at this and provide you with an updated model.

Regards,

Karan

+1 Karan Kotadia over 3 years ago

TI__Genius 16725 points

Hi Ankit,

I was able to find the problem. There is a ROEZ variable in the model which is to model the input leakage of the enable pin. Instead of having a 2200kOhm resistance, it has a 2000 Ohm resistance and so it was causing a resistor divider to occur. I have made the change in the attached file. You can also open the .lib file or .cir file and update line 51 from .PARAM ROEZ = 2000 to .PARAM ROEZ = 2200000.

SN74AHC1G126.cir

SN74AHC1G126.lib

Regards,

Karan

0 Ankit Jain over 3 years ago in reply to Karan Kotadia

Prodigy 70 points

Thankyou so much for your support and quickly resolving issue.

Logic

Logic forum

SN74AHC1G126-EP: 74AHC1G126MDCKTEP