This is a multi-part message in MIME format.
------=_NextPart_000_007A_01BE63BE.7D7F8DC0
Content-Type: text/plain;
charset="iso-8859-1"
Content-Transfer-Encoding: quoted-printable
To show my gratitude to all those who answered my query, here
is a compilation of the answers I received.
Thanks very much to all who have responded, you've been
incredibly helpful and generous, especially Reinhard Buchhold!!
My original question was:
Dear MEMS Researchers,
I am currently in the process of using ANSYS FEA S/W to model a
pressure sensor's membrane. I have just created the structure of the
whole sensor, and found out that I have difficulty in mashing it. May I
know the reasons?
Also can anyone point me to anywhere where I can get some reference or
result regarding this tropic, so that I could use it as my reference.
Very Much Thanks in advance for any advice!
AJ Pang
*************************************************************************=
***********************
The advice are as follow:-
*************************************************************************=
****************
From: Shivalik Bakshi
To: ceeajp@cee.hw.ac.uk
Subject: Re: High Frequency Transducers
Hi AJ,
I used ANSYS to model a perssure sensor diaphragm some time ago so maybe =
I can help.
1. have you made a model of the whole sensor or just the membrane? In =
case you have modelled the whole sensor, you only need to model the =
membrane since the boundry conditions of the membrane are fixed.
2. Is it a 2D model or a 3D? The membrane can be easily modelled with a =
2D model using Shell 63 elements since the thickness of the membrane is =
negligible in comparison with the length and width.=20
One reference for stress in pressure sensor membranes is a paper by =
Kensall & White. I do not recall the deails though. It is prety old =
(1970's)
*************************************************************************=
************************************************************
From: Shivalik Bakshi
To: ceeajp@cee.hw.ac.uk
Subject: Re: pressure sensor
> ***Did U model the whole sensor? what is the dimension, the material=20
> did U used and what type of sensor did U model, was it piezo-resistive =
> or capacitive sensor. I was thinking of modeling a peizo-resistive=20
> sensor, but I don't know if ANSYS can do the calculation of the change =
> in resistance of the piezo-resistor??
No I did not model the whole sensor. It is not required because you are =
only interested in the stress distribution in the diaphragm.=20
Ansys cannot model piezoresistivity. Once you get the stress =
distribution in the sensor diaphragm, look up the Microsensors book by =
Sze. He explains the piezoresistivity coefficients that you have to =
multiply the stress with and that will give you a value of change in =
resistance. Look up the book by Sze. It explains everything.
> Do U have the material property parameter to the material that you=20
> used??
I used parameters for Silicon.
E =3D 170 GPa (approx)
Poissons Ratio =3D 0.22
> > 2. Is it a 2D model or a 3D? The membrane can be easily modeled=20
> with a 2D model using Shell 63 elements since the thickness of the=20
> membrane is negligible in comparison with the length and width.=20
>=20
> ***I used a 3D model and the element used is solid 95 with 20 node. =20
Just model the diaphragm and not the whole sensor. And you do not need =
to model in 3D, just a 2D will do. Even if you do it 3D, use the 8 node =
elements. They will give you good answers.
*************************************************************************=
****************************************************************
From: Trevor Niblock
To: "'ceeajp@cee.hw.ac.uk'" ,
"MEMS@ISI.EDU"
Subject: RE: High Frequency Transducers
You may find that you've the wrong mesh density at different parts of =
the=20
structure. In addition you may of modeled to much of the device. If it =
is=20
symmetric you will only need to model the section about the line of=20
symmetry. Don't forget that you can only use mapped meshing for =
uniformed=20
area/volumes.
The best FEA book (I've found) is by MJ Fagan: FEA Theory & Practice.
How are you assembling the model? You should try creating a *.log file.=20
You can then alter different aspects of the device to find errors.
With all FEA models you should validate the results by modeling a simple =
device that you can pre-calculate. Examples of diaphragms are given in =
the=20
above reference.
Trevor Niblock;
MEMS group, Rm. 2043, Building 53, ECS, Southampton University,
Highfield, Southampton, SO17 1BJ, UK.
e-mail: t.niblock@soton.ac.uk
URL: http://www.mems.ecs.soton.ac.uk/users/trevor/tn_hp.htm
Note: URL may not work in a microsoft browser.
The e-mail and any attachments hereto are strictly confidential and
intended solely for the addressee. If you are not the intended addressee
please notify the sender by return and delete the message. You must not
disclose, forward or copy this e-mail or attachments to any third party
without the prior consent of the sender.
*************************************************************************=
*********************************************************
From: Phil Rayner
To: ceeajp@cee.hw.ac.uk
Subject: Re: High Frequency Transducers
I have some experience with ANSYS which seems to like being=20
difficult to mesh. Circular membranes are especially tricky since=20
they have a singularity at the centre. I usually build up the model=20
by a point by point method ie place the points then join them to=20
lines, on these make an area. Then copy this area and=20
rotate/translate to the next point and join up to make areas top and=20
bottom. Finally make volumes that you can copy again and again.
Now when you mesh it will give a mapped accurate mesh.
Its not easy unfortunately, but is the most controlled way.
If you want any more help it would be good to see your model=20
shape ( by a screen capture)
hope this makes some sense
Phil Rayner
*************************************************************************=
**********************************************
From: James Marchetti
To: ceeajp@cee.hw.ac.uk
Subject: Re: High Frequency Transducers
Dear AJ Pang, =20
I recently read your posting at MEMS@ISI.EDU regarding your difficulty =
in=20
using ANSYS to mesh a pressure sensor membrane. I am curious, it this a =
capacitive or piezo pressure sensor? This answer might determine why=20
Ansys in solving the problem.
At IntelliSense corporation, we produce IntelliCAD, a software for=20
simulating MEMS devices. It can perform thermo-mechanical analysis like=20
ANSYS, but it can also perform electrostatic and coupled=20
thermoelectromechanical analysis which are MEMS specific phenomena. =20
Also, our meshing capabilities are specific for MEMS sensors and it is=20
compatible with Ansys. For example, if the mesh is generated in=20
IntelliCAD, it can be used in Ansys. If you are interested in learning=20
more, please visit our website for more information.
Please contact me if you can tell me more about your sensor or if you=20
have any questions. Thank you very much.
=20
=20
Sincerely, =20
James Marchetti,
Business Development Engineer
-----------------------
IntelliSense Corporation
16 Upton Drive
Wilmington, MA 01887 U.S.A.
(978)988-8000 x 17
(978)988-8001
jmarchetti@intellisense.com
www.intellisense.com
*************************************************************************=
**************************************************
From: Reinhard Buchhold
To: ceeajp@cee.hw.ac.uk
Subject: Re: High Frequency Transducers
Hi,
I have been modeling pressure sensors in silicon technology for a
while. These are my experiences:
- You should divide your model into sub-volumes which are
confined by 6 or 8 nodes. It does not matter how you define
these volumes (for instance from keypoints, areas or primitives).
- After this you should define the element sizes along the lines
(lesize).
- Opposite lines should have an equal number of line divisions.
- Then you should be able to mesh the volumes with bricks by
setting eshape,2.
- Solid 45 and 95 work good. You can also use Solid 46 for
considering anisotropy. However, this does not improve
accuracy very much.
If you are interested, I could send you some of my models on
monday. I doubt you will find any good reference for modelling
pressure sensors.
Best regards, Reinhard
*************************************************************************=
***************************************
From: Reinhard Buchhold
To: ceeajp@cee.hw.ac.uk
Subject: Re: High Frequency Transducers
Hi AJ,
I am modelling piezoresistive sensors. There is no direct corellation
between displacement and the change of resistance. You have to read out
the mechanical stress components in the resistor region. Based on these
you can calculate resistance or output voltage. Eshape,2 is a key which
sets element shapes to bricks (elements with 8 corner-points).
Enclosed you will find a file, which can be read in by a comman line.
It enables calculation of transfer functions for varying pressures.
These will be written in an output file. A fully Wheatstone bridge,
a (100)<110> diaphragm and a piezoresistive coefficient p44 of
8.9*10^-10
are assumed. Good luck, Reinhard
/batch,list
/filname,ds40u
*cfopen,ds40u
*do,i,1,10
!i=3D4
/filname,ds40u
/prep7
*afun,deg
/com variable values
wdi=3D400e-6 !wafer thickness=20
cb=3D5.2e-3 !sensor width
da=3D20e-6 !diaphragm thickness
sb=3D0.6e-3 !bulk with at the
bottom
alp=3D54.7 !etching angle
ri=3D160e-6 !resistor length
a=3Dcb-2*sb-2*(wdi-da)/tan(alp) !diaphragm width
EMa=3D1.689e11 !youngs-modulus
nua=3D0.0625 !poissons-ration
dru=3D(1.6**i)*500 !pressure from below
/com material properties
si=3D1
mp,ex,1,EMa
mp,nuxy,1,nua
asp=3D5 !aspect ration
x0=3D0
x1=3Dsb
x2=3Dsb+(wdi-da)/tan(alp)
x3=3Dcb/2
y0=3D0
y1=3Dx1
y2=3Dx2
y3=3Dx3
z0=3D0
z1=3Dwdi-da
z2=3Dwdi
/com nodes for definition of the resistors
n,1,x3,y2,z2 !longitudinal
n,2,x3,y2+ri/2,z2 !longitudinal
n,3,x3-ri/4,y2,z2 !crosswise
n,4,x3,y2,z2 !croswise
/com structure
k,1,x0,y0,z0
k,2,x3,y0,z0
k,3,x3,y1,z0
k,4,x1,y1,z0
k,5,x0,y0,z1
k,6,x3,y0,z1
k,7,x3,y2,z1
k,8,x2,y2,z1
k,9,x3,y3,z1
k,10,x0,y0,z2
k,11,x3,y0,z2
k,12,x3,y2,z2
k,13,x2,y2,z2
k,14,x3,y3,z2
/com volumes
v,1,2,3,4,5,6,7,8 =20
v,5,6,7,8,10,11,12,13 =20
v,7,8,9,12,13,14 =20
et,1,solid45,,,,,, =20
allsel
vsel,r,volu,,1,3
vatt,1,,1 =20
allsel
esize,asp*da
allsel
r=3D6
s=3D6
t=3D16 !even number
lesize,5,,,r,1/8
lesize,7,,,r,8
lesize,9,,,r,8
lesize,11,,,r,8
lesize,4,,,s,8
lesize,2,,,s,1/8
lesize,20,,,s,8
lesize,16,,,s,1/8
lesize,12,,,s,8
lesize,8,,,s,1/8
lesize,25,,,t,-3
lesize,22,,,t,-3
lesize,23,,,t,-3
lesize,21,,,t,-3
lesize,18,,,t,-3
lesize,10,,,t,-3
lesize,all,,,t
vmesh,1,3
allsel
nsel,r,loc,x,0
nsel,r,loc,y,0
nsel,r,loc,z,0
d,all,uz
allsel
nsel,r,loc,x,x3
dsymm,symm,x
allsel
clocal,22,0,0,0,0,45,0,0
csys,22
nsel,r,loc,y,0
nrotat,all
dsymm,symm,y,22
csys,0
allsel
asel,r,area,,15
nsla,r,1
esln,r
sfe,all,1,pres,,dru
allsel
waves
save
fini
/solu
nropt,full,,on
nsubst,1
neqit,10
nlgeom,1
sstif,on
pred,on,,on
cnvtol,u,1e-6,0.0001,2,
antype,static
solve
save
fini
/post1
set,1
esel,r,mat,,si
lpath,1,2 =20
pdef,ll,s,y =20
pcalc,intg,ill,ll,s =20
*get,ill,path,0,last,ill =20
ill=3Dill/(ri/2)
lpath,1,2 =20
pdef,lq,s,x =20
pcalc,intg,ilq,lq,s =20
*get,ilq,path,0,last,ilq =20
ilq=3Dilq/(ri/2)
lpath,3,4 =20
pdef,ql,s,x =20
pcalc,intg,iql,ql,s =20
*get,iql,path,0,last,iql =20
iql=3Diql/(ri/4)
lpath,3,4 =20
pdef,qq,s,y =20
pcalc,intg,iqq,qq,s =20
*get,iqq,path,0,last,iqq =20
iqq=3Diqq/(ri/4)
s=3D(ill-ilq)-(iql-iqq) !effective mechanical stress
ua=3D5.0/2*(8.9e-10)/2*s !output voltage
*vwrite,dru,wdi,cb,da,sb,ri,ua
(3X,E15.6,3X,E15.6,3X,E15.6,3X,E15.6,3X,E15.6,3X,E15.6,3X,E15.6)
*vwrite,ill,iqq,ilq,iql
(3X,E15.6,3X,E15.6,3X,E15.6,3X,E15.6)
fini
/clear
*enddo
*cfclose
*************************************************************************=
***************************************
From: Reinhard Buchhold
To: ceeajp@cee.hw.ac.uk
Subject: Re: Pressure sensor
Hi AJ,
the part you are asking about is part of the post-processing routine.
For this, 4 nodes which describe the edges of the resistors are
defined in the preprocessing prior any meshing. In the postprocessing,
a path is defined between these two nodes of each resistor. This
gives you the stress distribution along the resistors. After this, mean
values are calculated by dividing the integral value (from pcalc) by
the resistor length. So, you have 4 equivalent stresses which enable
calculation of output voltage by the usual equation. There is no need
to define electrical elements in the analysis. It is enough to simulate
the mean stresses and put them in the analytical equation. (The only
exception is for modelling Four-Terminal-Transducer, like the
Motorola sensors.)
Best regards, Reinhard
*************************************************************************=
******************************
------=_NextPart_000_007A_01BE63BE.7D7F8DC0
Content-Type: text/html;
charset="iso-8859-1"
Content-Transfer-Encoding: quoted-printable
To show my gratitude to all those who answered my query, here
is =
a=20
compilation of the answers I received.
Thanks very much to all who have responded, you've =
been
incredibly=20
helpful and generous, especially Reinhard Buchhold!!
My original question was:
Dear MEMS Researchers,
I am currently in the process of =
using ANSYS=20
FEA S/W to model a
pressure sensor's membrane. I have just created =
the=20
structure of the
whole sensor, and found out that I have difficulty =
in=20
mashing it. May I
know the reasons?
Also can anyone point me =
to=20
anywhere where I can get some reference or
result regarding this =
tropic, so=20
that I could use it as my reference.
Very Much Thanks in advance =
for any=20
advice!
AJ Pang
****************************************************************=
********************************
The advice are as =
follow:-
****************************************************************=
*************************
From: Shivalik Bakshi <
sbakshi@cs.sfu.ca>
To: ceeajp@cee.hw.ac.uk
Subject: =
Re: High=20
Frequency Transducers
Hi AJ,
I used ANSYS to model a =
perssure=20
sensor diaphragm some time ago so maybe I can help.
1. have you =
made a=20
model of the whole sensor or just the membrane? In case you have =
modelled the=20
whole sensor, you only need to model the membrane since the boundry =
conditions=20
of the membrane are fixed.
2. Is it a 2D model or a 3D? The =
membrane can=20
be easily modelled with a 2D model using Shell 63 elements since the =
thickness=20
of the membrane is negligible in comparison with the length and width.=20
One reference for stress in pressure sensor membranes is a =
paper by=20
Kensall & White. I do not recall the deails though. It is prety old=20
(1970's)
****************************************************************=
*********************************************************************
From: Shivalik Bakshi <
sbakshi@cs.sfu.ca>
To: ceeajp@cee.hw.ac.uk
Subject: =
Re:=20
pressure sensor
> ***Did U model the whole sensor? what is =
the=20
dimension, the material
> did U used and what type of sensor did =
U model,=20
was it piezo-resistive
> or capacitive sensor. I was thinking of =
modeling=20
a peizo-resistive
> sensor, but I don't know if ANSYS can do the=20
calculation of the change
> in resistance of the=20
piezo-resistor??
No I did not model the whole sensor. It is not =
required=20
because you are only interested in the stress distribution in the =
diaphragm.=20
Ansys cannot model piezoresistivity. Once you get the stress =
distribution in=20
the sensor diaphragm, look up the Microsensors book by Sze. He explains =
the=20
piezoresistivity coefficients that you have to multiply the stress with =
and that=20
will give you a value of change in resistance. Look up the book by Sze. =
It=20
explains everything.
> Do U have the material property =
parameter=20
to the material that you
> used??
I used parameters for=20
Silicon.
E =3D 170 GPa (approx)
Poissons Ratio =3D =
0.22
>=20
> 2. Is it a 2D model or a 3D? The membrane can be easily modeled =
>=20
with a 2D model using Shell 63 elements since the thickness of the =
>=20
membrane is negligible in comparison with the length and width.
> =
> ***I used a 3D model and the element used is solid 95 with 20=20
node.
Just model the diaphragm and not the whole sensor. =
And you=20
do not need to model in 3D, just a 2D will do. Even if you do it 3D, use =
the 8=20
node elements. They will give you good answers.
****************************************************************=
*************************************************************************=
From: Trevor Niblock <
t.niblock@soton.ac.uk>
To=
:=20
"'ceeajp@cee.hw.ac.uk'"=20
<ceeajp@cee.hw.ac.uk>,
=
; =20
"MEMS@ISI.EDU" <MEMS@ISI.EDU>
Subject: RE: High =
Frequency=20
Transducers
You may find that you've the wrong mesh density at =
different=20
parts of the
structure. In addition you may of modeled to much of =
the=20
device. If it is
symmetric you will only need to model the =
section=20
about the line of
symmetry. Don't forget that you can only use =
mapped=20
meshing for uniformed
area/volumes.
The best FEA book (I've =
found) is by=20
MJ Fagan: FEA Theory & Practice.
How are you assembling the =
model? You=20
should try creating a *.log file.
You can then alter different =
aspects of=20
the device to find errors.
With all FEA models you should validate =
the=20
results by modeling a simple
device that you can =
pre-calculate. =20
Examples of diaphragms are given in the
above =
reference.
Trevor=20
Niblock;
MEMS group, Rm. 2043, Building 53, ECS, Southampton=20
University,
Highfield, Southampton, SO17 1BJ, UK.
e-mail: t.niblock@soton.ac.uk
URL: =
http://ww=
w.mems.ecs.soton.ac.uk/users/trevor/tn_hp.htm
Note:=20
URL may not work in a microsoft browser.
The e-mail and any =
attachments=20
hereto are strictly confidential and
intended solely for the =
addressee. If=20
you are not the intended addressee
please notify the sender by return =
and=20
delete the message. You must not
disclose, forward or copy this =
e-mail or=20
attachments to any third party
without the prior consent of the=20
sender.
****************************************************************=
******************************************************************=
From: Phil Rayner <
p.j.rayner@cranfield.ac.uk=
>
To:=20
ceeajp@cee.hw.ac.uk
Subject: =
Re:=20
High Frequency Transducers
I have some experience with ANSYS =
which seems=20
to like being
difficult to mesh. Circular membranes are especially =
tricky=20
since
they have a singularity at the centre. I usually build up the =
model=20
by a point by point method ie place the points then join them to =
lines,=20
on these make an area. Then copy this area and
rotate/translate to =
the next=20
point and join up to make areas top and
bottom. Finally make volumes =
that=20
you can copy again and again.
Now when you mesh it will give a mapped =
accurate mesh.
Its not easy unfortunately, but is the most controlled =
way.
If you want any more help it would be good to see your model =
shape (=20
by a screen capture)
hope this makes some sense
Phil=20
Rayner
****************************************************************=
*******************************************************
From: James Marchetti <
james@intellis.com>
To: ceeajp@cee.hw.ac.uk
Subject: =
Re: High=20
Frequency Transducers
Dear AJ Pang,
I recently read =
your=20
posting at MEMS@ISI.EDU regarding =
your=20
difficulty in
using ANSYS to mesh a pressure sensor membrane. =
I am=20
curious, it this a
capacitive or piezo pressure sensor? This =
answer=20
might determine why
Ansys in solving the problem.
At =
IntelliSense=20
corporation, we produce IntelliCAD, a software for
simulating MEMS =
devices.=20
It can perform thermo-mechanical analysis like
ANSYS, but it can =
also=20
perform electrostatic and coupled
thermoelectromechanical analysis =
which are=20
MEMS specific phenomena.
Also, our meshing capabilities are =
specific=20
for MEMS sensors and it is
compatible with Ansys. For example, =
if the=20
mesh is generated in
IntelliCAD, it can be used in Ansys. If you are =
interested in learning
more, please visit our website for more=20
information.
Please contact me if you can tell me more about your =
sensor=20
or if you
have any questions. Thank you very much.
=20
Sincerely,
James =
Marchetti,
Business=20
Development Engineer
-----------------------
IntelliSense=20
Corporation
16 Upton Drive
Wilmington, MA 01887 =20
U.S.A.
(978)988-8000 x 17 <phone>
(978)988-8001 =
<fax>
jmarchetti@intellisense.com
www.intellisense.com
****************************************************************=
***********************************************************
From: Reinhard Buchhold <
buchhold@Rcs1.urz.tu-dres=
den.de>
To:=20
ceeajp@cee.hw.ac.uk
Subject: =
Re:=20
High Frequency Transducers
Hi,
I have been modeling pressure =
sensors=20
in silicon technology for a
while. These are my experiences:
- You =
should=20
divide your model into sub-volumes which are
confined by 6 or 8 =
nodes. It=20
does not matter how you define
these volumes (for instance from =
keypoints,=20
areas or primitives).
- After this you should define the element =
sizes along=20
the lines
(lesize).
- Opposite lines should have an equal number =
of line=20
divisions.
- Then you should be able to mesh the volumes with bricks=20
by
setting eshape,2.
- Solid 45 and 95 work good. You can also use =
Solid=20
46 for
considering anisotropy. However, this does not =
improve
accuracy=20
very much.
If you are interested, I could send you some of my models=20
on
monday. I doubt you will find any good reference for =
modelling
pressure=20
sensors.
Best regards, Reinhard
****************************************************************=
************************************************
From: Reinhard Buchhold <buchhold@Rcs1.urz.tu-dres=
den.de>
To:=20
ceeajp@cee.hw.ac.uk
Subject: =
Re:=20
High Frequency Transducers
Hi AJ,
I am modelling =
piezoresistive=20
sensors. There is no direct corellation
between displacement and the =
change=20
of resistance. You have to read out
the mechanical stress components =
in the=20
resistor region. Based on these
you can calculate resistance or =
output=20
voltage. Eshape,2 is a key which
sets element shapes to bricks =
(elements with=20
8 corner-points).
Enclosed you will find a file, which can be read in =
by a=20
comman line.
It enables calculation of transfer functions for varying =
pressures.
These will be written in an output file. A fully =
Wheatstone=20
bridge,
a (100)<110> diaphragm and a piezoresistive coefficient =
p44=20
of
8.9*10^-10
are assumed. Good luck,=20
Reinhard
/batch,list
/filname,ds40u
*cfopen,ds40u
*do,i,1=
,10
!i=3D4
/filname,ds40u
/prep7
*afun,deg
/com=20
variable=20
values
wdi=3D400e-6 &nb=
sp; &nbs=
p; =
; =20
!wafer thickness=20
cb=3D5.2e-3 &nbs=
p; =
; =
=20
!sensor=20
width
da=3D20e-6 =
&=
nbsp; &n=
bsp; =20
!diaphragm=20
thickness
sb=3D0.6e-3 &=
nbsp; &n=
bsp; &nb=
sp; =20
!bulk with at=20
the
bottom
alp=3D54.7 &nbs=
p; =
; =
=20
!etching=20
angle
ri=3D160e-6 =
; =
&=
nbsp; =20
!resistor=20
length
a=3Dcb-2*sb-2*(wdi-da)/tan(alp) &n=
bsp; &nb=
sp; =20
!diaphragm=20
width
EMa=3D1.689e11 &n=
bsp; &nb=
sp; &nbs=
p; =20
!youngs-modulus
nua=3D0.0625 =
&=
nbsp; &n=
bsp; =20
!poissons-ration
dru=3D(1.6**i)*500 =
; =
&=
nbsp; =20
!pressure from below
/com material=20
properties
si=3D1
mp,ex,1,EMa
mp,nuxy,1,nua
asp=3D5 &nbs=
p; =
; =
&=
nbsp; =20
!aspect=20
ration
x0=3D0
x1=3Dsb
x2=3Dsb+(wdi-da)/tan(alp)
x3=3Dcb/2
=
y0=3D0
y1=3Dx1
y2=3Dx2
y3=3Dx3
z0=3D0
z1=3Dwdi-da
z2=3D=
wdi
/com=20
nodes for definition of the=20
resistors
n,1,x3,y2,z2 =
=20
!longitudinal
n,2,x3,y2+ri/2,z2 &nb=
sp; =20
!longitudinal
n,3,x3-ri/4,y2,z2 &nb=
sp; =20
!crosswise
n,4,x3,y2,z2 =
; =20
!croswise
/com=20
structure
k,1,x0,y0,z0
k,2,x3,y0,z0
k,3,x3,y1,z0
k,4,x1,y1,z0=
k,5,x0,y0,z1
k,6,x3,y0,z1
k,7,x3,y2,z1
k,8,x2,y2,z1
k,9,x=
3,y3,z1
k,10,x0,y0,z2
k,11,x3,y0,z2
k,12,x3,y2,z2
k,13,x2,y2,=
z2
k,14,x3,y3,z2
/com=20
volumes
v,1,2,3,4,5,6,7,8 &nb=
sp; &nbs=
p; =20
v,5,6,7,8,10,11,12,13 =
&=
nbsp; =20
v,7,8,9,12,13,14 =
; =
=20
et,1,solid45,,,,,, &nb=
sp; =20
allsel
vsel,r,volu,,1,3
vatt,1,,1 =
&=
nbsp; =20
allsel
esize,asp*da
allsel
r=3D6
s=3D6
t=3D16 &nb=
sp; &nbs=
p; =
; =
=20
!even=20
number
lesize,5,,,r,1/8
lesize,7,,,r,8
lesize,9,,,r,8
lesize,=
11,,,r,8
lesize,4,,,s,8
lesize,2,,,s,1/8
lesize,20,,,s,8
lesi=
ze,16,,,s,1/8
lesize,12,,,s,8
lesize,8,,,s,1/8
lesize,25,,,t,-3<=
BR>lesize,22,,,t,-3
lesize,23,,,t,-3
lesize,21,,,t,-3
lesize,18,=
,,t,-3
lesize,10,,,t,-3
lesize,all,,,t
vmesh,1,3
allsel
ns=
el,r,loc,x,0
nsel,r,loc,y,0
nsel,r,loc,z,0
d,all,uz
allselnsel,r,loc,x,x3
dsymm,symm,x
allsel
clocal,22,0,0,0,0,45,0,0csys,22
nsel,r,loc,y,0
nrotat,all
dsymm,symm,y,22
csys,0
=
allsel
asel,r,area,,15
nsla,r,1
esln,r
sfe,all,1,pres,,druallsel
waves
save
fini
/solu
nropt,full,,on
nsubst,1neqit,10
nlgeom,1
sstif,on
pred,on,,on
cnvtol,u,1e-6,0.0001=
,2,
antype,static
solve
save
fini
/post1
set,1
esel,=
r,mat,,si
lpath,1,2 &nb=
sp; &nbs=
p; =20
pdef,ll,s,y &nbs=
p; =20
pcalc,intg,ill,ll,s &n=
bsp; =20
*get,ill,path,0,last,ill =20
ill=3Dill/(ri/2)
lpath,1,2 &nbs=
p; =
; =20
pdef,lq,s,x &nbs=
p; =20
pcalc,intg,ilq,lq,s &n=
bsp; =20
*get,ilq,path,0,last,ilq =20
ilq=3Dilq/(ri/2)
lpath,3,4 &nbs=
p; =
;=20
pdef,ql,s,x &nbs=
p; =20
pcalc,intg,iql,ql,s =20
*get,iql,path,0,last,iql =20
iql=3Diql/(ri/4)
lpath,3,4 &nbs=
p; =
; =20
pdef,qq,s,y &nbs=
p; =20
pcalc,intg,iqq,qq,s &n=
bsp; =20
*get,iqq,path,0,last,iqq =20
iqq=3Diqq/(ri/4)
s=3D(ill-ilq)-(iql-iqq) =
!effective=20
mechanical stress
ua=3D5.0/2*(8.9e-10)/2*s !output=20
voltage
*vwrite,dru,wdi,cb,da,sb,ri,ua
(3X,E15.6,3X,E15.6,3X,E15.6,=
3X,E15.6,3X,E15.6,3X,E15.6,3X,E15.6)
*vwrite,ill,iqq,ilq,iql
(3X,E1=
5.6,3X,E15.6,3X,E15.6,3X,E15.6)
fini
/clear
*enddo
*cfclose
****************************************************************=
************************************************
From: Reinhard Buchhold <
buchhold@Rcs1.urz.tu-dres=
den.de>
To:=20
ceeajp@cee.hw.ac.uk
Subject: =
Re:=20
Pressure sensor
Hi AJ,
the part you are asking about is part =
of the=20
post-processing routine.
For this, 4 nodes which describe the edges =
of the=20
resistors are
defined in the preprocessing prior any meshing. In the=20
postprocessing,
a path is defined between these two nodes of each =
resistor.=20
This
gives you the stress distribution along the resistors. After =
this,=20
mean
values are calculated by dividing the integral value (from =
pcalc)=20
by
the resistor length. So, you have 4 equivalent stresses which=20
enable
calculation of output voltage by the usual equation. There is =
no=20
need
to define electrical elements in the analysis. It is enough to=20
simulate
the mean stresses and put them in the analytical equation. =
(The=20
only
exception is for modelling Four-Terminal-Transducer, like=20
the
Motorola sensors.)
Best regards, Reinhard
****************************************************************=
***************************************
------=_NextPart_000_007A_01BE63BE.7D7F8DC0--