The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Modeling >> Semiconductor Devices >> Model for HJFET NE3514S02 transistor!!
https://designers-guide.org/forum/YaBB.pl?num=1273409182

Message started by RF_Designer on May 9^th, 2010, 5:46am

Title: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on May 9^th, 2010, 5:46am

Hello all,

I 'm looking for HJFET NE3514S02 transistor model !

Is there a way for that ? or in which way can we make it ?

Thank you in advance,

Nass

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on May 9^th, 2010, 8:39am

http://www2.renesas.com/microwave/en/parameter/low_gaashj_dp.html

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on Jun 16^th, 2010, 1:27am

Thank you,
I know the site and i had used the given model but it did not work in ADS..
Could you try if you have a time ??
Thank you in advance,
M

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by Geoffrey_Coram on Jun 16^th, 2010, 6:00am

It works for me ... what problem are you having? Does ADS give you an error? Do you not believe the answer?

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on Jun 17^th, 2010, 1:57am

Oh, Have your tried to create a component and then making a DC Bias in dorser to display the I-V characteristic curve??
Cause when you use the netlist in ADS is works but i mean after....
In attached the obtained model...
You can remark there is no ports...!!!
Pls, Could you check it if you have time...??

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 17^th, 2010, 2:04am

As I expected, simply you don't understand usage of netlist in ADS.

RF_Designer wrote on Jun 17^th, 2010, 1:57am:

In attached the obtained model...
You can remark there is no ports...!!!

It seems you don't understand usage of Agilent ADS surely.

There are two methods.
One is following. This is very simple and no symbol is required.
http://www.designers-guide.org/Forum/YaBB.pl?num=1266403928/17#17
http://www.designers-guide.org/Forum/YaBB.pl?num=1240322183/23#23

Second method.
Place port in your schematic and create symbol. But there is no model definition component in your schematic.

There is a Design Kit including this FET.
You had better use it since you don't understand ADS usage well.
http://www2.renesas.com/microwave/ads/nec_activelibraryv4.0.zip

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on Jun 18^th, 2010, 2:50am

How i don't understand usage of Agilent ADS ??
That attached figure is wrong ?? I do not think so..!! cause i have tried with the other component that active bias circuit it works but with this transistor does not work.
Could you check it pls ? (i.e , the second method)
I have never used Netlist include, and i do know if it gives the same results!!!
how can we use this netlist include ? is there a method ?
For the nec_activelibraryv4.0.zip, yes i know it and i used it in ADs but if you compare the s-parameters with the S2P you will find a big difference, i.e, the given paramters do not fit with the S2P file so that why i want to use the given spice model to ADS.
Pls, Could you give more information...
I appreciate your help.

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 18^th, 2010, 6:40am

RF_Designer wrote on Jun 18^th, 2010, 2:50am:

That attached figure is wrong ?? I do not think so..!!

That is a reason why I say you can't understand usage of Agilent ADS.

You can't understand what are necessary for FET component at all.

(1) There is no meaningful Net Label for FET symbol.
(2) FET symbol is "MOSFET_NMOS" in your schematic. This is wrong.
(3) Model refered by "MOSFET_NMOS" is unknown "x990x9".
(4) Even if "x990x9" is used, there is no model definition component for "x990x9"
(5) All values of L and C are unitless and factorless.
(6) If you want to use this as subcircuit, place port and create symbol.

You have to use followings if you want to make schematic.
http://edocs.soco.agilent.com/display/ads2009/EE+HEMT1+%28EEsof+Scalable+Nonlinear+HEMT%29
http://edocs.soco.agilent.com/display/ads2009/EE+HEMT1+Model+%28EEsof+Scalable+Nonlinear+HEMT+Model%29

RF_Designer wrote on Jun 18^th, 2010, 2:50am:

How i don't understand usage of Agilent ADS ??

I can't understand why you can say you are familiar with Agilent ADS, because you can't understand such easy things.

Read documents of Agilent ADS surely.
http://edocs.soco.agilent.com/display/ads2009/Importing+a+Netlist+File
You can't use "Netlist Import" for ADS's syntax netlist.

"Netlist Import" function is valid for netlists of the following.
Spice2G
Spice3
PSpice
HSpice
Spectre

RF_Designer wrote on Jun 18^th, 2010, 2:50am:

For the nec_activelibraryv4.0.zip, yes i know it and i used it in ADs
but if you compare the s-parameters with the S2P you will find a big difference,
i.e, the given paramters do not fit with the S2P file

I will compare S-parameter calculated from "NE3514S02_v127.ads" with "NE3514S02v2_8-26_2_5.s2p" when I have spare time.

The attached figure is a method where subcircuit schematic is not required.

"NE3514S02_v127.ads"
Quote:

simulator lang=ads

define NE3514S02_v127 ( D G S )
parameters Noise=

"EEHEMTM1":NE3514S02_v127 _net125 _net127 _net126 Ugw=160 um N=1 Noise=yes _M=1

model EEHEMTM1 EE_HEMT1 Vto=-990.9 mV Gamma=39.57m Vgo=-346.6 mV Vdelt=0 Vch=593.2 mV Gmmax=84.53 mH \
Vdso=2 Vsat=711.5 mV Kapa=124.6 mS Peff=1.495 Vtso=-10 Is=28.39 pA N=1.633 Ris=5.777 \
Rid=1 mOhm Tau=2.861 psec Cdso=140.4 fF Rdb=1e9 Cbs=160 fF Vtoac=-1.005 Gammaac=42.32m \
Vdeltac=0 Gmmaxac=79m Kapaac=53.82 mS Peffac=14.47 Vtsoac=-10 Gdbm=20 uF Kdb=33.33 \
Vdsm=100 C11o=290 fF C11th=55.18 fF Vinfl=-1.058 Deltgs=2.939 Deltds=415.2 mV Lambda=50.75m \
C12sat=30.26 fF Cgdsat=12.72 fF Kbk=0 Vbr=15 Nbr=2 Idsoc=0.1 Rd=947.1 mOhm Rs=862.9 mOhm Rg=1.417 \
Ugw=160 um Ngf=1 Vco=-382.6 mV Vba=1 Vbc=301 mV Mu=1.836m Deltgm=354.5m Deltgmac=178.6m \
Alpha=300 mV Tnom=25 Rgtc=0 Rdtc=0 Rstc=0 Vtotc=0 Gmmaxtc=0 Gammatc=0 Vinfltc=0 Vtoactc=0 \
Gmmaxactc=0 Gammaactc=0 Xti=3 Kmod=1 Kver=1

L:Ld2 _net120 D L=7.1 pH Noise=yes
C:cds1 S D C=4.2 fF
C:cds S _net120 C=82.8 fF
L:Lg1 _net101 G L=1.98 pH Noise=yes
C:cgs S _net101 C=78.7 fF
C:cgs1 S G C=6.5 fF
C:cgd _net101 _net120 C=11.63 fF
L:Ls _net126 S L=100.3 pH Noise=yes
L:Ld _net125 _net120 L=561.6 pH Noise=yes
L:Lg _net127 _net101 L=583.5 pH Noise=yes

end NE3514S02_v127

NE3514S02_v127:Q1 d g s

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on Jun 18^th, 2010, 10:49am

Thank you pancho_hideboo,
1. pls, how you have gotten NE3514S02_v127.ads ?
In the Nec site they provide just spice file which is the same as you provide but without
In the beginning : simulator lang=ads
In the end : NE3514S02_v127:Q1 d g s

I don't how you have got it ?

2. The Nec technologies provides SPICE parameters. Before i thought that is the same to use Net list Import. Thank you for the remark.

Really, you are great... I'm learning from your knowledge.

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 18^th, 2010, 10:55am

RF_Designer wrote on Jun 18^th, 2010, 10:49am:

In the Nec site they provide just spice file

No, it is not SPICE Syntax Netlist. It is Agilent ADSsim's Syntax Netlist.

Nonlinear models for "Ansoft Designer" and BJT are SPICE Syntax Netlist.
But others are not SPICE Syntax Netlist.

Agilent ADSsim can read Agilent ADSsim's Syntax Netlist and Cadence Spectre's Syntax Netlist directly.

RF_Designer wrote on Jun 18^th, 2010, 10:49am:

which is the same as you provide but without
In the beginning : simulator lang=ads
In the end : NE3514S02_v127:Q1 d g s
I don't how you have got it ?

I added these two lines
But "simulator lang=ads" is not mandatory.

If you create symbol having three ports, D, G and S whose content is empty, you don't have to append "NE3514S02_v127:Q1 d g s".

Again see http://edocs.soco.agilent.com/display/ads2009/Importing+a+Netlist+File

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 19^th, 2010, 4:32am

Red Curves : S-parameter calculated from "NE3514S02_v127.ads(EE_HEMT1_Model ; EEsof Scalable Nonlinear HEMT Model)"

Blue Curves : "NE3514S02v2_8-26_2_5.s2p(24. May 2006, VDS=2V, ID=5mA)"

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 19^th, 2010, 4:34am

Red Curves : S-parameter calculated from "NE3514S02_v127.ads(EE_HEMT1_Model ; EEsof Scalable Nonlinear HEMT Model)"

Blue Curves : "NE3514S02v2_8-26_2_5.s2p(24. May 2006, VDS=2V, ID=20mA)"

RF_Designer wrote on Jun 18^th, 2010, 2:50am:

I don't think there are awfully large difference between them although fitting of nonlinear model to S-parameter model is not so good.

Try to change Vds, Idrain or Analysis temperature slightly in simulation of Nonlinear model.

Generally I believe S-parameter model not Nonlinear model since former is a raw data without approximation due to fitting.

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on Jun 20^th, 2010, 6:44am

Thank you for the detailed explanation and sorry if i have taken up your time.
As you can see in the curve that you have done, when the frequency increase, the difference is more important espicially when you calculate the Roller fact for both methods. The same remark if you have used nec_activelibraryv4.0.zip...

Pls, how you have known the expression that you have added of the last line in the NE3514S02_v127.ads ? is always true for another component provided by manufacturer ?

What about BER? Do you have a good documents? i do know till know how can i proceed since i have just to work on RF receiver...!!! As you are familiar in that design, do you agree that in the RF receiver is important to simulate BER ?
Thank you in advance,
N

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 20^th, 2010, 7:04am

pancho_hideboo wrote on Jun 18^th, 2010, 10:55am:

Agilent ADSsim can read Agilent ADSsim's Syntax Netlist and Cadence Spectre's Syntax Netlist directly.

Sorry. Currently Agilent ADSsim can also read Synopsys HSPICE Netlist directly.
http://edocs.soco.agilent.com/display/ads2009/About+HSPICE+Compatibility

RF_Designer wrote on Jun 20^th, 2010, 6:44am:

The same remark if you have used nec_activelibraryv4.0.zip...

It is very natural result since "nec_activelibraryv4.0.zip" include completely same file as "NE3514S02_v127.ads".
It seems you also don't understand structure of Design Kits of Agilent ADS.

RF_Designer wrote on Jun 20^th, 2010, 6:44am:

As you can see in the curve that you have done, when the frequency increase, the difference is more important espicially when you calculate the Roller fact for both methods.

S-parameter calculated from Nonlinear model is suspicious for high frequency.
For example, S12 is very suspicious for high frequency.

Again I believe S-parameter model not Nonlinear model since former is a raw data without approximation due to fitting.

Again surely see http://www.designers-guide.org/Forum/YaBB.pl?num=1273408947

RF_Designer wrote on Jun 20^th, 2010, 6:44am:

Pls, how you have known the expression that you have added of the last line in the NE3514S02_v127.ads ?
is always true for another component provided by manufacturer ?

It depends on contents of model files.
Read documents of Agilent ADS.

RF_Designer wrote on Jun 20^th, 2010, 6:44am:

What about BER? Do you have a good documents?
i do know till know how can i proceed since i have just to work on RF receiver...!!!

I can't understand meaning of this sentence at all.

RF_Designer wrote on Jun 20^th, 2010, 6:44am:

As you are familiar in that design, do you agree that in the RF receiver is important to simulate BER ?

I can't understand meaning of this sentence at all.
Create another new thread for your new questions with detailed decription and correct sentences using correct terminologies but without unfamiliar abbreviations such as "sof" and "pb".

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by RF_Designer on Jun 22^nd, 2010, 2:01am

I meant:
1. Do you have a good documentation on BER ?
2. For RF receiver, do you agree that it is important to have a BER parameter? how can we get it ? is it possible to get from simulation?
Also,
For the transistor part, is it important to have the layout of the transistor NE3514S02 or just S2P file is sufficient in order to use a co-simulation ?

Thank you in advance,

Title: Re: Model for HJFET NE3514S02 transistor!!
Post by pancho_hideboo on Jun 22^nd, 2010, 2:34am

RF_Designer wrote on Jun 22^nd, 2010, 2:01am:

1. Do you have a good documentation on BER ?
2. For RF receiver, do you agree that it is important to have a BER parameter?
how can we get it ?
is it possible to get from simulation?

Your questions are out of topic of this thread.

Create another new thread for your new questions with detailed decription and correct sentences using correct terminologies but without unfamiliar abbreviations such as "sof" and "pb".

RF_Designer wrote on Jun 22^nd, 2010, 2:01am:

For the transistor part, is it important to have the layout of the transistor NE3514S02
or just S2P file is sufficient in order to use a co-simulation ?

What on earth do you mean by "layout" and "co-simulation" ?

Again surely read followings.
http://www.designers-guide.org/Forum/YaBB.pl?num=1273408947/1#1
http://www.designers-guide.org/Forum/YaBB.pl?num=1273408947/4#4

Answer following questions.

pancho_hideboo wrote on May 9^th, 2010, 6:02am:

What conditions do you apply for simulation ?
Do you include package model and PCB model in simulation ?
Do you correctly do de-embedding in measurement ?
Do you correctly do calibration of reference plane in measurement ?

pancho_hideboo wrote on Jun 12^th, 2010, 6:45am:

RF_Designer wrote on Jun 10^th, 2010, 9:43am:

Not that, the simulations are done as following:
1. from layout i create the component

What do you want to mean ?
Do you mean that you use standard distributed component of ADS as layout blocks ?
Or do you mean that you invoke EM-Cosimulation of Momentum and SP-analysis in Agilent ADS ?

pancho_hideboo wrote on Jun 12^th, 2010, 6:45am:

RF_Designer wrote on Jun 10^th, 2010, 9:43am:

I hope that i clarified my problem.....

Your problem is very easy problem.
I think your problem is simply you can't reflect actual measurement conditions in simulation.
Show me reference plane location for actual measurement and simulation.
If you use SMA connector in actual measurement, how to treat it in simulation ?
Or do you use "Port Extension" in actual measurement ?

Your problem is simply you can't reflect actual measurement conditions in simulation.

I think both S-parameter model and Nonlinear model of NE3514S02 are for on-wafer DUT not for packaged device data.
And this HJFET can be provided as bare-chip.

Which do you use, bare-chip or packaged-device ?

If you use bare-chip, how do you mount this device on printed circuit board ?
(1) Normal mount with wire bonding.
(2) Flip mount with bumps

Artwork patterns of PCB(Printed Circuit Board) are very important in high frequency.
If you use packaged device, you have to include package model and foot print in simulation in addition to
Artwork patterns of PCB.

Even if you use bare-chip as normal mount with wire bonding, you have to include wire model in simulation.
http://www.designers-guide.org/Forum/YaBB.pl?num=1206929207/3#3

Such things are very very very very common in RF engineering.

It seems you are very beginner in RF engineering world.