Author 
Message 
sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Fri May 17, 2013 4:57 am 


Hi all,
I am interested to find out the forces acting on iron in a dipole magnet. I made a symmetrical model (one quadrant) of iron and surrounding air. I selected Solid98 elements for iron and Solid96 for air. I made the complete upper and lower coils with Sourc36 elements. The infinite boundary are meshed with Infin47 elements.
I flagged the iron by making a component and then using FMAGBC command. I imposed the normal flux BC and issued the MAGSOLV command. During structural analysis in the next step I have to impose the structural loads obtained from magnetic analysis using LDREAD command.
But the the problem is that there are no results file (.rst) formed. Ansys is giving the error that no loads are found since rst file is not there.
I want to know why is this occurring? It is necessary to also model a half coil with coupled magnetostructural elements like Solid98 to create the result file?
Please clarify my doubt if anybody has done similar kind of problems. If anyone wants I can post the file also made using APDL commands. I am absolutely new to this field and hence have very little knowledge.
Thank you. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 10:24 am 


Sundeep
When you looked at the magnetics results, did you use an RMG file or an RST file? With the 96 and 36 and only the MAG dof for the 98 it might have put the results into an RMG file. So the LDREAD needs to use the same file as used to look at the magnetic results.
The forces are a result of the magnetic field and the iron. (You can compute the JXB on each element if the exterior application of the forces are not accurate). You can generate forces with a magnet. You do not need the 98 unless you have tetrahedral elements and you need a quadratic shape function. All my motor models were with the 96 and published numerous papers with the 96.
Mike Yaksh
NAC International
Norcross GA
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf Of sundeep.ghosh
Sent: Friday, May 17, 2013 7:58 AM
To: xansys@xansys.org
Subject: [Xansys] Force on iron in magnetostructural analysis
Hi all,
I am interested to find out the forces acting on iron in a dipole magnet. I made a symmetrical model (one quadrant) of iron and surrounding air. I selected Solid98 elements for iron and Solid96 for air. I made the complete upper and lower coils with Sourc36 elements. The infinite boundary are meshed with Infin47 elements.
I flagged the iron by making a component and then using FMAGBC command. I imposed the normal flux BC and issued the MAGSOLV command. During structural analysis in the next step I have to impose the structural loads obtained from magnetic analysis using LDREAD command.
But the the problem is that there are no results file (.rst) formed. Ansys is giving the error that no loads are found since rst file is not there.
I want to know why is this occurring? It is necessary to also model a half coil with coupled magnetostructural elements like Solid98 to create the result file?
Please clarify my doubt if anybody has done similar kind of problems. If anyone wants I can post the file also made using APDL commands. I am absolutely new to this field and hence have very little knowledge.
Thank you.

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Fri May 17, 2013 11:45 am 


Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards, _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 11:57 am 


Sundeep,
You can find the stress if you convert the magnetics model to a structural model (96 to 45) and use LDREAD. The reason for the 98 is to allow you to use updated forces to calculate the deformation, because the deformation is changing the field because some gap may be closing due to deformation.
The differences between the two force calculations usually indicated that the mesh was too coarse.
I looked at your model. Recommend
1) use bricks, not tets
2) really refine mesh
Mike Yaksh
NAC International
Norcross GA
Original Message
From: sundeep.ghosh <sundeep@vecc.gov.in>
Sent: Friday, May 17, 2013 2:46 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards,

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 1:27 pm 


Sundeep,
You can find the stress if you convert the magnetics model to a structural model (96 to 45) and use LDREAD. The reason for the 98 is to allow you to use updated forces to calculate the deformation, because the deformation is changing the field because some gap may be closing due to deformation.
The differences between the two force calculations usually indicated that the mesh was too coarse.
I looked at your model. Recommend
1) use bricks, not tets
2) really refine mesh
Mike Yaksh
NAC International
Norcross GA
Original Message
From: sundeep.ghosh <sundeep@vecc.gov.in>
Sent: Friday, May 17, 2013 2:46 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards,

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 1:27 pm 


Sundeep,
You can find the stress if you convert the magnetics model to a structural model (96 to 45) and use LDREAD. The reason for the 98 is to allow you to use updated forces to calculate the deformation, because the deformation is changing the field because some gap may be closing due to deformation.
The differences between the two force calculations usually indicated that the mesh was too coarse.
I looked at your model. Recommend
1) use bricks, not tets
2) really refine mesh
Mike Yaksh
NAC International
Norcross GA
Original Message
From: sundeep.ghosh <sundeep@vecc.gov.in>
Sent: Friday, May 17, 2013 2:46 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards,

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 1:27 pm 


Sundeep,
You can find the stress if you convert the magnetics model to a structural model (96 to 45) and use LDREAD. The reason for the 98 is to allow you to use updated forces to calculate the deformation, because the deformation is changing the field because some gap may be closing due to deformation.
The differences between the two force calculations usually indicated that the mesh was too coarse.
I looked at your model. Recommend
1) use bricks, not tets
2) really refine mesh
Mike Yaksh
NAC International
Norcross GA
Original Message
From: sundeep.ghosh <sundeep@vecc.gov.in>
Sent: Friday, May 17, 2013 2:46 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards,

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 1:27 pm 


Sundeep,
You can find the stress if you convert the magnetics model to a structural model (96 to 45) and use LDREAD. The reason for the 98 is to allow you to use updated forces to calculate the deformation, because the deformation is changing the field because some gap may be closing due to deformation.
The differences between the two force calculations usually indicated that the mesh was too coarse.
I looked at your model. Recommend
1) use bricks, not tets
2) really refine mesh
Mike Yaksh
NAC International
Norcross GA
Original Message
From: sundeep.ghosh <sundeep@vecc.gov.in>
Sent: Friday, May 17, 2013 2:46 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards,

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 1:27 pm 


Sundeep,
You can find the stress if you convert the magnetics model to a structural model (96 to 45) and use LDREAD. The reason for the 98 is to allow you to use updated forces to calculate the deformation, because the deformation is changing the field because some gap may be closing due to deformation.
The differences between the two force calculations usually indicated that the mesh was too coarse.
I looked at your model. Recommend
1) use bricks, not tets
2) really refine mesh
Mike Yaksh
NAC International
Norcross GA
Original Message
From: sundeep.ghosh <sundeep@vecc.gov.in>
Sent: Friday, May 17, 2013 2:46 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thank you so much for your reply. Yes the RMG file has been created. I followed your suggestion and read the force data from this file. Now no errors are showing and the program is working. Thanks a lot.
Regarding the use of 98 elements I want to clarify that I used this element since my ultimate objective is to find out the stress generated on iron from the magnetic forces. Solid96 does not have structural dof. So I can not get stress using this. If I am wrong please do rectify me.
Now I am facing another problem. The force results on iron from Maxwell ST and Virtual Work are varying greatly both in magnitude and direction. I can not find the exact reason.
Hence I am posting a small program which I prepared to clarify my doubt. Please have a look and indicate the errors in my program which lead to such huge variation in results from Maxwell and Virtual Work.
!*********************************************************
fini
/filnam,check,1
/clear
/PREP7
/title, Stress on Iron of Dipole Magnet
*afun,deg
d = 0.2 ! dist of coil from median plane
r = 0.12 ! coil mean radius
r1 = 0.1 ! coil inner rad
r2 = 0.14 ! coil outer rad
w = 0.04 ! coil width
c = 82000 ! current*turns*layers
a = 0.05 ! iron width
b = 0.5 ! iron length
s = 0.1 ! dist of iron from median plane
t = 0.2 ! thickness of air from coil and iron edge to the infinite boundary
!*************** Element type ************************************************
ET,1,98,10 !Air
ET,2,98,0 !Iron
ET,3,SOURC36 !Coil current element
ET,4,INFIN47 !For infinite surface
ET,5,98,0 !Element for Dummy structure for applying strucutural boundary condition
!******************* Material properties *************************************
MP,MURX,1,1 !Air
MP,EX,1,100
MP,PRXY,1,0.3
MP,EX,2,200E9 !Iron
MP,PRXY,2,0.3
MP,MURX,2,5
MP,RSVX,2,1.72E9 !O.m
MP,KXX,2,400
MP,EX,3,200E9 !Hypothetical material, having murx as air but strength very high
MP,PRXY,3,0.3
MP,MURX,3,1
MP,RSVX,3,1.72E9
MP,KXX,3,400
! Material 3 is introduced since fixed BC on top iron surface can't be specified
! since it is surrounded by air..see structural solution procedure at the end
!*************** Coil elements modelling (for current only) ******************
! Upper Coil 
wpof,,d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,2,3,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,2
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
! Lower Coil 
wpro,,90
wpof,,2*d
wpro,,90
csys,wp
*get,nm,node,,num,max
n,nm+1,0,0
n,nm+2,r,0
n,nm+3,0,r
n,nm+4,r,0
n,nm+5,0,r
TYPE,3
R,3,1,c,w,w,,,,,0.001 !Real constant for bar source 36 element
REAL,3
E,nm+2,nm+3,nm+1
E,nm+3,nm+4,nm+1
E,nm+4,nm+5,nm+1
E,nm+5,nm+2,nm+1
/eshape,1
eplot
!esys,0
csys,0
WPCSYS,1,0
WPSTYLE,,,,,,,,0
! Iron & Air Modelling 
block,0,a,s,s+b,0,a ! Iron
block,0,a,s+b,s+b+t,0,a ! Steel
block,0,r+t,0,s+b+t,0,(a+t) ! Air
vovlap,all
numcmp,all
!******************* Material Specifications ***************
vsel,s,volu,,3 ! Air regions
vatt,1,1,1,0
vsel,s,volu,,2 ! Dummy steel
vatt,3,1,5,0
vsel,s,volu,,1 ! Iron portions
vatt,2,1,2,0
allsel
/pnum,volu,1
/TRLCY,volu,1,3
vplot
WPCSYS,1,0
WPSTYLE,,,,,,,,0
!****************** Meshing ********************************
allsel
mshape,1,3d ! tetrahedralshaped elements
mshkey,0 ! free mesh
vmesh,all
allsel
asel,s,loc,x,r+t ! infinite boundary meshing
asel,a,loc,y,s+b+t
asel,a,loc,z,(a+t)
aplot
aatt,1,,4,,,
!mshape,1,2d
mshkey,2
amesh,all
!***** Making of components for calculation of coil forces ***********
ALLSEL,ALL
ESEL,S,TYPE,,2
EPLOT
CM,iron,ELEM
ALLSEL,ALL
ESEL,S,TYPE,,3
EPLOT
CM,coil,ELEM
ALLSEL,ALL
csys,0
/pnum,type,1
/number,1
save, model,db
fini
!****************** Solution *******************************
!************** Magnetic Field Solution ********************
/prep7
/title, Magnetic Field Analysis
KEYOPT,2,1,10 ! Selecting mag dofs of iron
KEYOPT,5,1,10 ! Selecting mag dofs of hypothetical material
/solu
ALLSEL,ALL
CSYS,0
FMAGBC,'iron' ! Force flag
allsel
asel,s,loc,y,0,
NSLA,R,1
D,all,MAG,0,0 ! Flux perpendicular condition
ALLSEL,ALL
magsolv,3,,,,,1
save, magneticfield,db
fini
!************** Magnetic Stress Solution *******************
/prep7
/title, Magnetic Stress Analysis
KEYOPT,1,1,2 ! Selecting ux, uy & uz dofs of air
KEYOPT,2,1,2 ! Selecting ux, uy & uz dofs of iron
KEYOPT,5,1,2 ! Selecting ux, uy & uz dofs of hypothetical material
/solu
csys,0
ALLSEL,ALL
allsel ! Symmetric BC at XY Plane
asel,s,loc,z,0
NSLA,R,1
D,all,uz,0,0
allsel ! Symmetric BC at YZ Plane
asel,s,loc,x,0
NSLA,R,1
D,all,ux,0,0
allsel
asel,s,loc,y,s+b+t
NSLA,R,1
NPLOT
D,ALL,UY,0 ! Fixed boundary conditions
allsel
LDREAD,FORC,LAST,, ,0,'check','rmg',' '
allsel
solve
save, stress,db
fini
!*********************************************************
Looking forward for your reply.
Thanks & Regards,

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Fri May 17, 2013 1:32 pm 


Hi Mike,
Thanks for the reply. I will try to refine the mesh as suggested by you to see the improvements.
I have a query. As you said the solid98 is used to update the deformation since it is a coupled element. I want to know how to do this magnetostructural analysis using Solid98 in a single step. I do not want to activate the magnetic dof for doing magnetic analysis and then structural dof to do structural analysis. I have tried to do so but could not find the solution.
I want to apply all the magnetic and structural dofs on solid98 together and then carry out the solution. Should I give MAGSOLV and then again SOLVE??
Please tell the direct solution technique.
Thank you. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Fri May 17, 2013 1:58 pm 


Sundeep
Your model has both iron and a coil, which means that you need to use the DSP scalar solution. If you do not use the DSP, you will end up with some problems at the ironair interface.
The MAGSOLV will do the Biot calculation, and it will do the two step solution for the DSP and in each case it will use the SOLVE command. When the solve is issued, if the DOF is active, it should solve for the DOF. The 98 looks likes it was primarily set up for the RSP type solution, which is a single step solution.
For this reason, like for most motors and actuators, the loop was set up to do the magnetic solution with the DSP, then the structural. I have seen a lot of solutions over time. So, there must have been a problem with your APDL that did the solutions. Now, unless you are expecting some deformation which could affect the field, your solution would be a single pass through; one magnetic, one structural.
Are you passing DC current or AC current through the coils? Do you plan on looking at any transient fields?
Mike Yaksh
NAC International
Norcross GA
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf Of sundeep.ghosh
Sent: Friday, May 17, 2013 4:33 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
Thanks for the reply. I will try to refine the mesh as suggested by you to see the improvements.
I have a query. As you said the solid98 is used to update the deformation since it is a coupled element. I want to know how to do this magnetostructural analysis using Solid98 in a single step. I do not want to activate the magnetic dof for doing magnetic analysis and then structural dof to do structural analysis. I have tried to do so but could not find the solution.
I want to apply all the magnetic and structural dofs on solid98 together and then carry out the solution. Should I give MAGSOLV and then again SOLVE??
Please tell the direct solution technique.
Thank you.

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Fri May 17, 2013 10:58 pm 


Hi Mike,
I am passing only DC current. You are right that if there are not much deformations which can change the field itself, the solution should be a single pass through.
Since I am relatively new to this filed, I just want to know the procedures which should be adopted if suppose there are large deformations which will significantly change the fields.
I guess in such cases the solution must be carried out in the following way; first a bit of magnetic solution, then read loads to do structural solution, then read deformation to change magnetic field and so on. This way the loop should continue I suppose.
I want to know how this loop can be prepared. Please correct me if I am wrong in my thinking process. If possible can you kindly mention the APDL commands which generally people do to carry out such solutions.
Also please tell what elements should be used for such case. Whether 98 can be used or not since you think it was set up for RSP solution.
Thank you. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


mike.yaksh User
Joined: 05 Feb 2009 Posts: 291

Posted: Mon May 20, 2013 1:14 pm 


Sundeep
I will look for a previous model and send it to you.
Mike Yaksh
NAC International
Norcross GA
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf Of sundeep.ghosh
Sent: Saturday, May 18, 2013 1:59 AM
To: xansys@xansys.org
Subject: Re: [Xansys] Force on iron in magnetostructural analysis
Hi Mike,
I am passing only DC current. You are right that if there are not much deformations which can change the field itself, the solution should be a single pass through.
Since I am relatively new to this filed, I just want to know the procedures which should be adopted if suppose there are large deformations which will significantly change the fields.
I guess in such cases the solution must be carried out in the following way; first a bit of magnetic solution, then read loads to do structural solution, then read deformation to change magnetic field and so on. This way the loop should continue I suppose.
I want to know how this loop can be prepared. Please correct me if I am wrong in my thinking process. If possible can you kindly mention the APDL commands which generally people do to carry out such solutions.
Also please tell what elements should be used for such case. Whether 98 can be used or not since you think it was set up for RSP solution.
Thank you.

Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Tue May 28, 2013 10:08 pm 


Mike
Looking forward to hear back from you soon.
Thank you. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Wed May 29, 2013 9:28 pm 


Mike
You can take your time.
No problem.
Thank you. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Thu May 30, 2013 9:54 pm 


Mike
I have few queries related to the force calculation on iron through Virtual Work and Maxwell Stress Tensor methods. As suggested by you, I have made hex meshing on a simple model and observed the improvements. Both the methods (VW & MX) are giving near about same results. I want to know suppose there is a complicated model where hex meshing can't be done and one has no other choice but to use tet mesh, then is there any other way to get good results? Actually in my model of a dipole magnet, I had to use tet mesh owing to its complexity and I found huge difference between the results from VW and MX methods.
Secondly, I have another query. I have modeled a quadrant of the model since it is symmetrical. Do I need to multiply the force results by 4 in order to get the total force on the model or whether ANSYS automatically takes this into account and give the total force when I issue the FMAGSUM command?
Looking forward to your reply. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 


sundeep.ghosh User
Joined: 17 May 2013 Posts: 13 Location: India

Posted: Fri Jul 05, 2013 2:46 am 


Dear Users,
Has anybody carried out any development concerning my earlier post (dated 31st May 2013) under this topic?
Kindly give a reply. _________________ Sundeep Ghosh
Scientific Officer
Variable Energy Cyclotron Centre
India 

Back to top 




You cannot post new topics in this forum You cannot reply to topics in this forum You cannot edit your posts in this forum You cannot delete your posts in this forum You cannot vote in polls in this forum You cannot attach files in this forum You cannot download files in this forum

