This symple circuit uses a model of MOSFET FDMS8622 and tests its working in Qspice. The same thing works as expected in LTspice but in Qspice the transistor is not truning ON. Can anybody give me some advice?
Thanks
.SUBCKT X1•FDMS8622 2 1 3
Dbody 7 5 DbodyMOD
Dbreak 5 11 DbreakMOD
Lgate 1 9 2.793e-9
Ldrain 2 5 0.004e-9
Lsource 3 7 1.014e-9
RLgate 1 9 27.93
RLdrain 2 5 0.04
RLsource 3 7 10.14
Rgate 9 6 1.05
D_D1 100 5 D_SG_cap
D_D2 100 101 D_SG_cap
R_R1 101 7 1.05
C_C1 6 101 27e-12
.MODEL D_SG_cap D (IS=1e-9 n=1 RS=5e-3 CJO=0.387e-9 M=0.549 t_abs=25)
It 7 17 1
Ebreak 11 7 17 7 110
Rbreak 17 7 RbreakMOD 1
.MODEL RbreakMOD RES (TC1=0.68e-3 TC2=-0.3e-6)
.MODEL DbodyMOD D (IS=0.8e-12 n=1 RS=10.389e-3 TRS1=2.5e-3 TRS2=1e-6 CJO=0.1e-9 M=0.41 TT=1e-9 XTI=2.75)
.MODEL DbreakMOD D (RS=8e-3 TRS1=1e-3 TRS2=1e-6 )
Rsource 7a 7 2.902e-3
Rdrain 5 16 RdrainMOD 30.5e-3
.MODEL RdrainMOD RES (TC1=7.0e-3 TC2=21e-6)
M_BSIM3 16 6 7a 7a Bsim3 W=0.67 L=1.15e-6 NRS=0 NRD=0
.MODEL Bsim3 NMOS (LEVEL=7 VERSION=3.1 MOBMOD=3 CAPMOD=2 paramchk=1 NQSMOD=0 TOX=1000e-10
.ENDS
X1 N03 N02 0 X1•FDMS8622
V1 N01 0 15
V2 N02 0 pulse 0 12 0 50n 50n 5µ 10µ
R1 N01 N03 15
.tran 100µ
.end
As you are a new user to the forum and cannot upload a schematic yet, it is not possible to pinpoint the exact issue in your workflow. Based on your description, it seems you can run the simulation and from your quote, you possibly imported it to Qspice correctly. Is there any chance you are confusing the gate, drain, and source? This model assigns Pin1 to Drain, Pin2 to Gate, and Pin3 to Source.
I expect that your model was downloaded from onsemi at the following link:
https://www.onsemi.com/download/models/lib/fdms8622.lib
Here is a symbol and an example created in Qspice to verify its basic ON/OFF operation.
Parent.FDMS8622.qsch (4.9 KB)
FDMS8622.qsym (2.3 KB)
OK, possibly I realized what the problem is. In FDMS8622.lib, it contains ; in its .model statement. If this library run with netlist (call through .lib directive), everything is fine.
However, Qspice auto generation symbol seems having trouble in importing it correctly. If you refer to your .model Bsim3 NMOS .... line, you can see all parameters after TOX are removed.
The quick fix is to remove these two ; from .lib and copy this subckt and re-import into Qspice.
Above message already with this corrected.
I can copy this for Mike to review… didn’t expect a subckt setup in this way.
1 Like
The problem is fixed by updating Qspice
05/11/2025 Fixed a problem pasting subcircuits onto a schematic to make symbols.
Thanks alot for the reply. I’ve just have updated Qspice and I see the same results. I would like to upload the actual circuit but for new users it seems that it is not possible.
José
Here is a reference how you can increase your trust level in this forum.
Understanding Discourse Trust Levels
I think may be Level 1 Trust level (basic member) will grant you upload file capability
Here are thing to do
- Entering at least 5 topics
- Reading at least 30 posts
- Spend a total of 10 minutes reading posts
1 Like
Did you regenerate your symbol from FDMS8622 subcircuit after update your Qspice?
Dear Kelvin,
You are right. I updated Qspice but did not regenerate the component. Now it works! Thanks a lot for your help. I’m designing a boost converter and I’m giving Qspice a try.
Thanks as well for the trusts levels link.
José
1 Like
