Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

help: TSMC BJT spice model

Status
Not open for further replies.

aindejeje

Junior Member level 2
Joined
Sep 29, 2009
Messages
21
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
1,416
Hello.
This is my first time doing mixed-signal IC design.
Im designing a CDP on Tanner and simulate it on T-SPICE.
and got the following error:

Fatal T-SPICE : Missing model declaration for "NPN"

I guess i need a BJT model for it.
SPICE model for TSMC (prefer 0.25um technology)
Can anyone help me?
 

erikl

Super Moderator
Staff member
Joined
Sep 9, 2008
Messages
8,112
Helped
2,685
Reputation
5,350
Reaction score
2,284
Trophy points
1,393
Location
Germany
Activity points
44,153
aindejeje said:
I guess i need a BJT model for it.
SPICE model for TSMC (prefer 0.25um technology)
Pls. find here SPICE Model Parameters for several TSMC 0.25µ processes!
 

    aindejeje

    points: 2
    Helpful Answer Positive Rating

aindejeje

Junior Member level 2
Joined
Sep 29, 2009
Messages
21
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
1,416
erikl said:
aindejeje said:
I guess i need a BJT model for it.
SPICE model for TSMC (prefer 0.25um technology)
Pls. find here SPICE Model Parameters for several TSMC 0.25µ processes!
thanks for your help.
but whats are the:
MM NON EPI
LO MTL etc
 

erikl

Super Moderator
Staff member
Joined
Sep 9, 2008
Messages
8,112
Helped
2,685
Reputation
5,350
Reaction score
2,284
Trophy points
1,393
Location
Germany
Activity points
44,153
aindejeje said:
... but whats are the:
MM NON EPI
LO MTL etc
These are all different 0.25µm processes (each process option has a unique name).
But meantime I discovered the files contain just S*PICE parameters for MOSfets, not for BJTs, sorry! :cry:
You should also specify, if you need a S*PICE model for a lateral or for a vertical npn. They can be quite different.
 

aindejeje

Junior Member level 2
Joined
Sep 29, 2009
Messages
21
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
1,416
erikl said:
aindejeje said:
... but whats are the:
MM NON EPI
LO MTL etc
These are all different 0.25µm processes (each process option has a unique name).
But meantime I discovered the files contain just S*PICE parameters for MOSfets, not for BJTs, sorry! :cry:
You should also specify, if you need a S*PICE model for a lateral or for a vertical npn. They can be quite different.
yeah.no BJTs :cry:
 

karthikvenkatesh

Newbie level 2
Joined
Jan 24, 2008
Messages
2
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,292
Hi erikl,

I am Karthik.
I am trying to simulate a circuit having BJTs in spectre.
I need 0.35 micron tsmc BJT model because my need in BJT that operates at 5v. I am not sure whether it is lateral or vertical BJT i need.
 

erikl

Super Moderator
Staff member
Joined
Sep 9, 2008
Messages
8,112
Helped
2,685
Reputation
5,350
Reaction score
2,284
Trophy points
1,393
Location
Germany
Activity points
44,153
karthikvenkatesh said:
Hi erikl,

I am Karthik.
I am trying to simulate a circuit having BJTs in spectre.
I need 0.35 micron tsmc BJT model because my need in BJT that operates at 5v.
Hi Karthik,
a 0.35 micron tsmc BJT model you can only get from TSMC if you sign an NDA, or through MOSIS, by a similar procedure.

You could perhaps get 'incognito' SPICE models for a similar 0.35 micron process, but the simulation results ain't necessarily identical. If you intend to produce a chip, it's a must to use the original models from the very process.

karthikvenkatesh said:
I am not sure whether it is lateral or vertical BJT i need.
Which model is available depends on the respective PDK. A 'standard' CMOS process usually includes a vertical pnp BJT (beta ≈ 2 .. 5), sometimes additionnally a lateral pnp (beta ≈ 20 .. 50). In any case their collectors are connected to the substrate. If you need uncommitted BJTs (also npn ones), you have to select a BICMOS process.
 

karthikvenkatesh

Newbie level 2
Joined
Jan 24, 2008
Messages
2
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,292
Erikl,
Thanks for your comments which is very helpful.
What I did is, I browsed through MOSIS site, got IBM 0.35 micron BJT NPN model whose forward beta is 100.
My specification is beta = 20. So i changed that forward beta and used those parameters in spectre for simulation.
This BJT model is for Bandgap reference design.
Some say, dont dwelve a lot into all of the BJT model parameters. Just take the beta=20. Since the role of BJT here in bandgap is not gain oriented but just to nullify the temperature coefficient.


Thanks and regards,
Karthik
 

erikl

Super Moderator
Staff member
Joined
Sep 9, 2008
Messages
8,112
Helped
2,685
Reputation
5,350
Reaction score
2,284
Trophy points
1,393
Location
Germany
Activity points
44,153
karthikvenkatesh said:
... IBM 0.35 micron BJT NPN model whose forward beta is 100.
Probably from a BICMOS process.

karthikvenkatesh said:
My specification is beta = 20. So i changed that forward beta and used those parameters in spectre for simulation.
This BJT model is for Bandgap reference design.
Some say, dont dwelve a lot into all of the BJT model parameters. Just take the beta=20. Since the role of BJT here in bandgap is not gain oriented but just to nullify the temperature coefficient.
That's ok. Even simple diodes would work. BJTs beta > 1 achieve better accuracy, however.
Rgds, erikl.
 

cmos_ajay

Full Member level 2
Joined
Jan 30, 2007
Messages
123
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,296
Activity points
2,220
Hello,

Can you please send me the link to the BJT NPN model . Thanks in advance.

Regards.


Erikl,
Thanks for your comments which is very helpful.
What I did is, I browsed through MOSIS site, got IBM 0.35 micron BJT NPN model whose forward beta is 100.
My specification is beta = 20. So i changed that forward beta and used those parameters in spectre for simulation.
This BJT model is for Bandgap reference design.
Some say, dont dwelve a lot into all of the BJT model parameters. Just take the beta=20. Since the role of BJT here in bandgap is not gain oriented but just to nullify the temperature coefficient.


Thanks and regards,
Karthik
 

aadiltrikha

Newbie level 6
Joined
Oct 3, 2010
Messages
13
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Location
india
Activity points
1,380
open your tsmc technology file
probably u ll be having there pmos nmos parameters

now add this line there
.model PNPDIODE D IS=1e-18 n=1
and in interconnections use the above name PNPDIODE for refernce



lets see the image & work out example here sayeesh.png








now for this we are having fully defined cmos models but no BJT as 3 are used here D1,2,3
so if you are not using this circuit for layout etc then just u can add this line & it will serve your purpose of BJT
i am posting full t-spice for this circuit,
****************************************************************
.option scale=1u post
.dc VDD 0 6 1m temp 0 100 25

VDD VDD 0 DC 5
Vop Vop 0 DC 0
Von VDD Von DC 0
Vmeas1 Vmeas1 0 DC 0
Vmeas2 Vmeas2 0 DC 0

M1B Vbiasn Vbiasn Vd1 0 N_1u L=2 W=10
M2B n2 Vbiasn Vr 0 N_1u L=2 W=10
M1T vncas vncas vbiasn 0 N_1u L=2 W=10
M2T vpcas vncas n2 0 N_1u L=2 W=10
M3T n1 Vbiasp VDD VDD P_1u L=2 W=30
M4T Vbiasp Vbiasp VDD VDD P_1u L=2 W=30
M3B vncas Vpcas n1 VDD P_1u L=2 W=30
M4B Vpcas Vpcas Vbiasp VDD P_1u L=2 W=30

M5T n3 vbiasp VDD VDD P_1u L=2 W=30
M5B Vref vpcas n3 VDD P_1u L=2 W=30
RL Vref vd3 489k TC1=0.002

Rb Vr vd2 52k TC1=0.002

D1 Vd1 0 PNPDIODE
D2 vd2 0 PNPDIODE 8
D3 vd3 0 PNPDIODE 8
.model PNPDIODE D IS=1e-18 n=1

** Start-up Circuit
MSU1 Vsur Vbiasp VDD VDD P_1u L=2 W=30
MSU2 Vncas Vsur Vpcas VDD P_1u L=2 W=30
MSU3 Vsur Vsur ns1 0 N_1u L=10 W=10
MSU4 ns1 ns1 ns2 0 N_1u L=10 W=10
MSU5 ns2 ns2 0 0 N_1u L=10 W=10

.include tsmccmos_models.txt

.end
**********************************************

Hope it ll be helpfull :) :roll:
 

aadiltrikha

Newbie level 6
Joined
Oct 3, 2010
Messages
13
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Location
india
Activity points
1,380
open your tsmc technology file
probably u ll be having there pmos nmos parameters

now add this line there
.model PNPDIODE D IS=1e-18 n=1
and in interconnections use the above name PNPDIODE for refernce



lets see the image & work out example here View attachment 70821








now for this we are having fully defined cmos models but no BJT as 3 are used here D1,2,3
so if you are not using this circuit for layout etc then just u can add this line & it will serve your purpose of BJT
i am posting full t-spice for this circuit,
****************************************************************
.option scale=1u post
.dc VDD 0 6 1m temp 0 100 25

VDD VDD 0 DC 5
Vop Vop 0 DC 0
Von VDD Von DC 0
Vmeas1 Vmeas1 0 DC 0
Vmeas2 Vmeas2 0 DC 0

M1B Vbiasn Vbiasn Vd1 0 N_1u L=2 W=10
M2B n2 Vbiasn Vr 0 N_1u L=2 W=10
M1T vncas vncas vbiasn 0 N_1u L=2 W=10
M2T vpcas vncas n2 0 N_1u L=2 W=10
M3T n1 Vbiasp VDD VDD P_1u L=2 W=30
M4T Vbiasp Vbiasp VDD VDD P_1u L=2 W=30
M3B vncas Vpcas n1 VDD P_1u L=2 W=30
M4B Vpcas Vpcas Vbiasp VDD P_1u L=2 W=30

M5T n3 vbiasp VDD VDD P_1u L=2 W=30
M5B Vref vpcas n3 VDD P_1u L=2 W=30
RL Vref vd3 489k TC1=0.002

Rb Vr vd2 52k TC1=0.002

D1 Vd1 0 PNPDIODE
D2 vd2 0 PNPDIODE 8
D3 vd3 0 PNPDIODE 8
.model PNPDIODE D IS=1e-18 n=1

** Start-up Circuit
MSU1 Vsur Vbiasp VDD VDD P_1u L=2 W=30
MSU2 Vncas Vsur Vpcas VDD P_1u L=2 W=30
MSU3 Vsur Vsur ns1 0 N_1u L=10 W=10
MSU4 ns1 ns1 ns2 0 N_1u L=10 W=10
MSU5 ns2 ns2 0 0 N_1u L=10 W=10

.include tsmccmos_models.txt

.end
**********************************************

Hope it ll be helpfull :) :roll:

---------- Post added at 16:50 ---------- Previous post was at 16:35 ----------

.model PNPDIODE D IS=1e-18 n=1
i have defined here in which n=1 just defines level of bjt model i.e. =1 so only is that is breaking point of bjt i am mentioning here which you can vary,.
also try to not be completly dependent on model technology files of companies, like sumtimes u want to implement your design <<innovatively>> or tech file are not having that parameter value,, so always just put .model command , edit , set level, make ,edit or add parameters accordingly ..
the above mentioned tsmc models is for 1micron tsmc technolgy for that BJT with IS=1e-18 i have used ,, but for 0.25u which u are using definitly value will be different , which is headache :) beacuse when i added resitor RL Vref vd3 489k TC1=0.002 TC temp coefficient was very hard to find ,, so process goes like that ,,
also switching to bicmos is very helpfull :)
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top