XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[EMAG][STRUCT] Magneto-structural 2D transient analysis EM
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Nov 04, 2014 8:14 am  Reply with quote

Hello experts,
I need help in 2-D couple field analysis magnetic-structural. I explain my problem:
I have a rotating electrical machine on which I already performed a current fed transient analysis. It is a permanent magnet machine and I performed transient analysis to get the eddy currents and losses on the magnets (just in case you wonder why I am performing a transient analysis). I am using PLANE 13 for the entire model. On the magnets I have defined a local coordinate system for the radial magnetization. But now let's go to the problem.

I would like to perform a couple field analysis to get the deformation of the machine while it is rotating with certain electrical loads. For example I would like to see how the rotor and the magnets are deformed by the centrifugal and magnetic forces and verify that the airgap is thick enough for the rotor and stator strain. The problem is that I don't have a big knowledge of mechanical, so I don't know which material properties I have to define for:
-IRON
-AIR
-MAGNETS
-COPPER

I defined the following element types for the different parts of the machine:
et,1,13,4,0,0 ! Iron and copper UX,UY,AZ,TEMP DOF
et,2,13,4,1,0 !Air (same as et,1 but with extra shapes activation, according to the reference guide)
et,3,13,4,0,0,1 ! Magnets with coordinate system based on the element I-J side

I activated the TEMP DOF because I would like to take account of the thermal expansion of the magnets. Is it possible?
But now I really don't know which element types to use in the material properties. Can you experts please help me?
Thanks in advance.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Tue Nov 04, 2014 11:53 am  Reply with quote

Davide,

The main question is if you are looking to see the effect of strain on the magnetic field. If not, what I normally did was to use the forces from each magnetic solution and perform static or transient evaluation using those forces. Once you change the element types, then LDREAD is used to load in the forces for each load step, and run the transient. This is straight forward for the stator since it is stationary. For the rotor, the forces are changing as the rotor is rotating, and you can rotate the rotor also and apply the forces. If you need to include the rotor shaft compliance, that can be done with springs, or if the mass is being excited, model the rotor shaft also. I would try to keep the model simple but allow it to match as best as possible the dynamic characteristics of the shaft. The oscillatory nature of the forces could potentially excite the shaft.

You mentioned copper, so does this mean that you want to determine the deformation of the winding? That will be more of a challenge if it is a series of wire cross sections, because then, the deformation is affected by friction, and you will need to model contacts between them. You could model them as a homogenous cross section and derive some effective E's NUXY from mechanical tests. The conductors will need the JxB forces since this is a body force distributed over the winding cross section.

For the laminate and magnets you are using, you should be able to get the E and density from their data sheet. If NUXY is not listed, use NUXY=0.3.

No need to model the air in the main gap. In between the winding cross sections (when a slot has more than a single coil), I would model contacts.

If you have concerns about the temperature effect; you could as a starter, input the temperature dependent properties and specify a bounding value for the temperature using the BF command. What I have done in the past is to solve the magnetic problem, get the heat generations, then input those into a thermal model. Magnets will have some eddy current losses, but usually they are minor compared to the other heat generations. The laminates will have core losses which are dependent on the field and frequency. Core losses would be input as heat generations. In some cases, these can be dominate; just depends on the signal coming into the windings. The thermal modeling takes some consideration, since the peak temperature in the winding is sometimes outside the stack, and you have cooling on the stack surfaces and on the outside of the windings. You also have cooling in the air gap, and there are some effective K's for that. In some cases the design, due to high heat, may have cooling channels, and CFD was used to determine the cooling. If you know the mass flow rate, and the channels are simple, a simple energy balance could be used to determine the change in the bulk temperature along the channel and use some test determined film coefficients to solve the thermal problem.

Mike Yaksh
NAC International
Norcross GA


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Tuesday, November 04, 2014 10:14 AM
To: xansys@xansys.org
Subject: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Hello experts,
I need help in 2-D couple field analysis magnetic-structural. I explain my problem:
I have a rotating electrical machine on which I already performed a current fed transient analysis. It is a permanent magnet machine and I performed transient analysis to get the eddy currents and losses on the magnets (just in case you wonder why I am performing a transient analysis). I am using PLANE 13 for the entire model. On the magnets I have defined a local coordinate system for the radial magnetization. But now let's go to the problem.

I would like to perform a couple field analysis to get the deformation of the machine while it is rotating with certain electrical loads. For example I would like to see how the rotor and the magnets are deformed by the centrifugal and magnetic forces and verify that the airgap is thick enough for the rotor and stator strain. The problem is that I don't have a big knowledge of mechanical, so I don't know which material properties I have to define for:
-IRON
-AIR
-MAGNETS
-COPPER

I defined the following element types for the different parts of the machine:
et,1,13,4,0,0 ! Iron and copper UX,UY,AZ,TEMP DOF
et,2,13,4,1,0 !Air (same as et,1 but with extra shapes activation, according to the reference guide)
et,3,13,4,0,0,1 ! Magnets with coordinate system based on the element I-J side

I activated the TEMP DOF because I would like to take account of the thermal expansion of the magnets. Is it possible?
But now I really don't know which element types to use in the material properties. Can you experts please help me?
Thanks in advance.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Wed Nov 05, 2014 1:14 am  Reply with quote

Thank you Mike for your detailed answer. I will follow your tips and let you know.
Best regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Wed Nov 05, 2014 8:43 am  Reply with quote

Hello everybody,
I spent my day trying to perform the couple field analysis. I am missing something, most probably because of my lack in the knowledge of structural analysis.
What I did:
In a fist approach, I haven't considered the effect of the displacement on the magnetic field.
I started from a simple static analysis of my model. First of all, I perform a static magnetic analysis, that gives the espected results. Than I can see RFORCE and NFORCE in some parts of my model. In the external part of the stator yoke the RFOR are similar to a sinusoidal distribution of forces. Well, now:
1) I assign proper structural material properties to the model, for example to the stator iron (but I assigned similar conditions to the other parts):
MP,dens,1,Pesosp
MP,EX,1,211E9
MP,EY,1,211E9
MP,EZ,1,211E9
MP,NUXY,1,0.3
MP,NUyz,1,0.3
MP,NUXZ,1,0.3
2)I read from the previous analisys the reaction forces:
ldread,reac,last
3)I evoce the /solu and start the solution through "solve" command.

What I obtain is the displacement of the stator core, which translates in x and y directions.
I would had expect all the parts of the machine fixed, but with some elastic strain values in the output results, but I don't obtain anything but the translation a mentioned.
I am wondering:
1) if I have to model contact region for example between the copper in the slots and the iron of the stator yoke; and in general I am wondering if I have to model contact regions between the parts "structurally differents"
2)if I have to define some constraint equation concernin UX and UY dof.
3)If I can use a symmetric model instead of a complete model.

Kind regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Wed Nov 05, 2014 9:14 am  Reply with quote

Davide

If the properties are isotropic, only EX, NUXY is needed. The density is kg/m^3, I assume.

Usually I used the LDEAD, FORC instead. That seemed to work. You can turn on the forces to see them, /pbc,f,1

I am not sure what was in the static structural model. The stator needs to be restrained in some manner by springs since the frame has some measure of compliance. Same for the rotor. If you want to include the coils, you need to decide which way you want to go. One way is to allow the coil elements to be connected to the stator elements, which is what you have now. This will limit the motion of the coil, due to the stiffness of the stator. If you want to see the coil move independently, you need to use a contact between the two and model them separately. This means that the magnetic model needs to the same, and CP the AZ of those nodes. I would try the simple way first.

Typically, for dynamic problems, I modeled the entire stator. I thought it was then more straight forward to model the entire model for magnetics, and just bring the forces over by LDREAD. For larger models, I think I use a symmetric model, and then wrote some APDL to replicate the forces in the stress model.

Mike Yaksh
NAC International
Norcross GA


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Wednesday, November 05, 2014 10:44 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Hello everybody,
I spent my day trying to perform the couple field analysis. I am missing something, most probably because of my lack in the knowledge of structural analysis.
What I did:
In a fist approach, I haven't considered the effect of the displacement on the magnetic field.
I started from a simple static analysis of my model. First of all, I perform a static magnetic analysis, that gives the espected results. Than I can see RFORCE and NFORCE in some parts of my model. In the external part of the stator yoke the RFOR are similar to a sinusoidal distribution of forces. Well, now:
1) I assign proper structural material properties to the model, for example to the stator iron (but I assigned similar conditions to the other parts):
MP,dens,1,Pesosp
MP,EX,1,211E9
MP,EY,1,211E9
MP,EZ,1,211E9
MP,NUXY,1,0.3
MP,NUyz,1,0.3
MP,NUXZ,1,0.3
2)I read from the previous analisys the reaction forces:
ldread,reac,last
3)I evoce the /solu and start the solution through "solve" command.

What I obtain is the displacement of the stator core, which translates in x and y directions.
I would had expect all the parts of the machine fixed, but with some elastic strain values in the output results, but I don't obtain anything but the translation a mentioned.
I am wondering:
1) if I have to model contact region for example between the copper in the slots and the iron of the stator yoke; and in general I am wondering if I have to model contact regions between the parts "structurally differents"
2)if I have to define some constraint equation concernin UX and UY dof.
3)If I can use a symmetric model instead of a complete model.

Kind regards.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Thu Nov 06, 2014 5:34 am  Reply with quote

Thank you again Mike.

I followed you tips and I had some results. Of course I need to refine the models, but I think now I am into that kind of analysis.
I modeled the entire model and I used the FORC instead the REAC; I set the UX and UY of a portion of the lower part of the stator equals to 0. I did the same with the central node of the rotor. I didn't take account of the difference in displacement of the slots. I got deformed shapes and that's good. But now I am wondering about two points:
1)I moedeled the stator and the rotor separately and than I jointed the mesh through ceintf contraint equations. But the shape of the deformed stator mesh doesn't match the deformed shape of the rotor mesh. For example, it is possible that a part of the stator goes overlapping the rotor. Are the results plausible?

2)If I want to perform an analysis with an external PM rotor instead of internal. how can I set the UX and UY constraint to let the external "rotor ring" to deform correctly but keeping it's rotation around the pivot point?

Thanks in advance.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Wed Nov 12, 2014 1:26 am  Reply with quote

Good morning experts,
I performed some simulation with some good results...At least I got some results! By the way I didn't use the load transfer method, but the direct couplyng method, as far as with plane 13 I can have both AZ, UX and UY in the same keyoption(1).
My main question is that one: I used two separate mesh for the rotor and the stator, without merging them. I only coupled them with ceintf constraints for magnetic analysis. But now that I am performing a structural analysis, the two meshes deform themselves and one overlaps the other one at the end of simulation. I tried to add UX and UY to the ceintf équations in the boundary between them but it doesn't work. Have you got any idea to solve that problem?
Kind regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Wed Nov 12, 2014 7:37 am  Reply with quote

Davide
Usually when the UX and UY were connected by CEINTF, it worked. First I would list out the CEs and confirm that the CE indeed did get generated. The CE symbol shows up if any CE is generated. Maybe they did not get included. Sometimes it may be a graphics issue; use /DSCAL,,1 and replot. I would check the continuity of the flux lines across the interface also.

Mike Yaksh
NAC International
Norcross GA

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Wednesday, November 12, 2014 3:26 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Good morning experts,
I performed some simulation with some good results...At least I got some results! By the way I didn't use the load transfer method, but the direct couplyng method, as far as with plane 13 I can have both AZ, UX and UY in the same keyoption(1).
My main question is that one: I used two separate mesh for the rotor and the stator, without merging them. I only coupled them with ceintf constraints for magnetic analysis. But now that I am performing a structural analysis, the two meshes deform themselves and one overlaps the other one at the end of simulation. I tried to add UX and UY to the ceintf équations in the boundary between them but it doesn't work. Have you got any idea to solve that problem?
Kind regards.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Wed Nov 12, 2014 7:55 am  Reply with quote

Hello Mike and thank you for your answer.
Infact I think it is a graphical issue. I saved a "hard copy" of the displacement after issueing /dscale,,1. What I get is the overlapping of the rotor on the stator because its expansion while the steady state is reached. I activated large deformation with nlgeom,on. Should I turn on the Coriolis effects as well?
About the flux lines, I cannot check because once I try to plot them, the graphics freaks out. But from the results of a previous magnetodinamic analysis without structural, I can assure they are perfectly continuous.
About the ux,uy issued trough ceintf, I think they are taken from the program as far as I can plot them and they are perfectly distributed along the airgap nodes/elements.

Do you think that the direct method is correct? I tried with the load transfer method, but I had problems with the overwriting of the .rst file, so I didn't be able to read any other load after the solution of the first loadstep.

Thank you in advance and kind regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Dec 02, 2014 9:53 am  Reply with quote

Hello Mike, hello experts

Here I am again asking for helps. I set up a a couple field analysis magnetic-->thermal--> structural through load transfer method. At first, I performed only static analysis. It basically works. I have two main questions anyway:

1)What is the best way to take account of air during the structural analysis? As far as I can use only structural element, I need to define young's modulus for it, which has no sense. I tried to exclude those elements during the solution, but I had PIVOT ERROR problem. Any suggestion?
2) Is it possible to read loads from two analysis (FORCE from magnetic and HGEN from thermal) and use those both into the structural analysis?

Best regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Tue Dec 02, 2014 11:51 am  Reply with quote

Davide
1) I typically put in low values for E which would not affect the response of the stator or rotor. The same procedure is followed for actuators, also.
2) You can use LDREAD to read in each loading from different analyses (model nodes/elements need to match). The magnetic solution produces a RST or RMS and the thermal is an RTH file. Just need to make sure that the thermal solution does not write into the same file that has the magnetic forces. The loading will be used if the degree of freedoms are active. If the model does not have a temperature DOF, the HGEN will not be used. If you mean to read in temperatures, they will be used for the properties and expansion.

Mike Yaksh
NAC International
Norcross GA

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Tuesday, December 02, 2014 11:54 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Hello Mike, hello experts

Here I am again asking for helps. I set up a a couple field analysis magnetic-->thermal--> structural through load transfer method. At first, I performed only static analysis. It basically works. I have two main questions anyway:

1)What is the best way to take account of air during the structural analysis? As far as I can use only structural element, I need to define young's modulus for it, which has no sense. I tried to exclude those elements during the solution, but I had PIVOT ERROR problem. Any suggestion?
2) Is it possible to read loads from two analysis (FORCE from magnetic and HGEN from thermal) and use those both into the structural analysis?

Best regards.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Dec 02, 2014 1:43 pm  Reply with quote

Thank you Mike for your reply.
I will follow your tip concernind the E values.
For the second point, I mean that I want to read and use together the reaction forces from the rst file of the magnetic simulation and the temperature from the rth file:

/COM "STRUCTURAL IS THE 3D ANALYSIS OF COUPLE FIELD LT METHOD
/solu
physics,read,structural
ldread,temp,,,,,,rth
ldread,forc,,,,,,rst ! or ldread,reac,,,,,,rst ??
allsel
solve
fini

Only a last question concerning the thermal analysis: is it correct to set the external nodes of the stator to a temperature of 20°C, which it is supposed to be the outer temperature? nsel,s,loc,x,stator_external_radius
d,all,temp,20
Thank you in advance.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Tue Dec 02, 2014 2:21 pm  Reply with quote

Davide
For the forces, I used LDREAD,FORC,,,,,,RST (since you are performing a magnetic static or transient, KIMG=0)

On a motor thermal model, I specified a film coefficient for the outer surface of the model. If you have liquid coolant flowing over the motor surface, the delta-T from surface to ambient is usually small and you could specify 20C.

Mike Yaksh
NAC International
Norcross GA

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Tuesday, December 02, 2014 3:44 PM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Thank you Mike for your reply.
I will follow your tip concernind the E values.
For the second point, I mean that I want to read and use together the reaction forces from the rst file of the magnetic simulation and the temperature from the rth file:

/COM "STRUCTURAL IS THE 3D ANALYSIS OF COUPLE FIELD LT METHOD
/solu
physics,read,structural
ldread,temp,,,,,,rth
ldread,forc,,,,,,rst ! or ldread,reac,,,,,,rst ??
allsel
solve
fini

Only a last question concerning the thermal analysis: is it correct to set the external nodes of the stator to a temperature of 20°C, which it is supposed to be the outer temperature? nsel,s,loc,x,stator_external_radius
d,all,temp,20
Thank you in advance.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Dec 02, 2014 2:30 pm  Reply with quote

Thank you Mike, you are very helpfull to me. The only thing I can do is to appreciate and get better in these kind of simulations.
Very best regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Mon Dec 08, 2014 8:57 am  Reply with quote

Hello everyone again,
it was supposed to be easier, but it isn't, at all!
I am still facing problems with the couple field simulation of an electrical machine.
I tried two ways:

1)MULTIFIELD SOLVER and solution algorithm. I think I set upe well the model, but it becomes so heavy (from the computational point of view) that gave me memory errors. For that reason, I decided to try the load transfer method

2)Load transfer couple physics analysis. I defined three physics envirorment (magnetic, thermal and structural), with elements 13, 55 and 182. In these envirorment I wrote everything about the model, except the solution setting, which is a transient restart. Actually the solution is composed by a sequence of three transient restart. The procedure is the following:

physics,read,magnetic
/assign,rst,magnetic,rmg !and other esav, osav, emat, excetera.
antype,transient,new !START NEW MAGNETIC ANALYSIS
...flags for torque calculation, time stepping, parameters calculation for mesh rotation..
lswrite
lssolve
save,magnetic,db
fini

physics,read,thermal
/assign...(rth, esav, osav, full, emat)
antype,transient,new
...solution setting
lswrite
lssolve
save,thermal,db
fini

physics,read,structural
/assign...(rst, esav, osav, full, emat)
antype,transient,new
...solution setting
lswrite
lssolve
save,structural,db
fini

*do loop for transient restart analysis

resume,magnetic,db
physics,read,magnetic
!erase load and constraints
!mesh rotation
!apply new boundary and loads
Antype,transient,restart
lswrite
lssolve
fini
parsav,common,parm !parameters for the mesh rotation
save,magnetic,db

resume,thermal,db
parres,common,parm,change
!erase load and constraints
!mesh rotation
!Read loads from magnetic results rmg
lswrite
lssolve
fini
save,thermal,db

resume,structural,db
parres,common,parm,change
!erase load and constraints
!mesh rotation
!Read loads from magnetic rmg and thermal results rth
lswrite
lssolve
fini
save,structural,db

!calculation and storage of torque, calculation of new parameters for the rotation
*enddo

What I get is that it works till the second *do loop. After that, the structural analysis seems to not converge (I set cnvtol,u as convergence criteria). Actually the solution starts, but it doesn't keep going: after a first substep, the solution procedure goes over and a new cycle in the *do loop is performed, but once it arrives to the structural restart, it finds a corrupted .esav file, as far as in the previous loadstep the solution didn't converge. The error I get is the following:
*** ERROR ***
One or more elements have become highly distorted. Excessive
distortion of elements is usually a symptom indicating the need for
corrective action elsewhere. Try incrementing the load more slowly
(increase the number of substeps or decrease the time step size). You
may need to improve your mesh to obtain elements with better aspect
ratios. Also consider the behavior of materials, contact pairs,
and/or constraint equations. If this message appears in the first
iteration of first substep, be sure to perform element shape checking.

I tried rising the convergence value, giving a number to each written loadstep, checking th constraints and boundary condition...anything worked. So, is the procedure I am following the correct one? I am exausted!

One thing I notice is that during the transient restart, both the magnetic and thermal produce .esav files, but it's not the same for the structural...cannot understand why.

If you have any advice, plase tell me.
Thanks in advance.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Mon Dec 08, 2014 11:36 am  Reply with quote

Davide

I use the load transfer approach. I have to keep all the file names separately to do the restarts with the different DOFs. I do not use the LSwrite, LSsolve commands. The Physics write command writes out the element types and their options, material properties, loadings. I do not see a reason to do the Resumes on the data base and parameters.

The element distortion would not occur in the laminates or rotor, but probably in the air and it could occur if the interface was not permitting it to slide. Since the structural is a transient, need to check how it is being restrained, since it would not pick up a singularity as in a static analysis.

Mike Yaksh
NAC International
Norcross GA


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Monday, December 08, 2014 10:58 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Hello everyone again,
it was supposed to be easier, but it isn't, at all!
I am still facing problems with the couple field simulation of an electrical machine.
I tried two ways:

1)MULTIFIELD SOLVER and solution algorithm. I think I set upe well the model, but it becomes so heavy (from the computational point of view) that gave me memory errors. For that reason, I decided to try the load transfer method

2)Load transfer couple physics analysis. I defined three physics envirorment (magnetic, thermal and structural), with elements 13, 55 and 182. In these envirorment I wrote everything about the model, except the solution setting, which is a transient restart. Actually the solution is composed by a sequence of three transient restart. The procedure is the following:

physics,read,magnetic
/assign,rst,magnetic,rmg !and other esav, osav, emat, excetera.
antype,transient,new !START NEW MAGNETIC ANALYSIS ...flags for torque calculation, time stepping, parameters calculation for mesh rotation..
lswrite
lssolve
save,magnetic,db
fini

physics,read,thermal
/assign...(rth, esav, osav, full, emat)
antype,transient,new
...solution setting
lswrite
lssolve
save,thermal,db
fini

physics,read,structural
/assign...(rst, esav, osav, full, emat)
antype,transient,new
...solution setting
lswrite
lssolve
save,structural,db
fini

*do loop for transient restart analysis

resume,magnetic,db
physics,read,magnetic
!erase load and constraints
!mesh rotation
!apply new boundary and loads
Antype,transient,restart
lswrite
lssolve
fini
parsav,common,parm !parameters for the mesh rotation save,magnetic,db

resume,thermal,db
parres,common,parm,change
!erase load and constraints
!mesh rotation
!Read loads from magnetic results rmg
lswrite
lssolve
fini
save,thermal,db

resume,structural,db
parres,common,parm,change
!erase load and constraints
!mesh rotation
!Read loads from magnetic rmg and thermal results rth lswrite lssolve fini save,structural,db

!calculation and storage of torque, calculation of new parameters for the rotation *enddo

What I get is that it works till the second *do loop. After that, the structural analysis seems to not converge (I set cnvtol,u as convergence criteria). Actually the solution starts, but it doesn't keep going: after a first substep, the solution procedure goes over and a new cycle in the *do loop is performed, but once it arrives to the structural restart, it finds a corrupted .esav file, as far as in the previous loadstep the solution didn't converge. The error I get is the following:
*** ERROR ***
One or more elements have become highly distorted. Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere. Try incrementing the load more slowly (increase the number of substeps or decrease the time step size). You may need to improve your mesh to obtain elements with better aspect ratios. Also consider the behavior of materials, contact pairs, and/or constraint equations. If this message appears in the first iteration of first substep, be sure to perform element shape checking.

I tried rising the convergence value, giving a number to each written loadstep, checking th constraints and boundary condition...anything worked. So, is the procedure I am following the correct one? I am exausted!

One thing I notice is that during the transient restart, both the magnetic and thermal produce .esav files, but it's not the same for the structural...cannot understand why.

If you have any advice, plase tell me.
Thanks in advance.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Dec 09, 2014 6:40 am  Reply with quote

Thank you Mike for you suggestion; I followed your guide and I am not using nor .db files and lswrite/lssolve anymore. I am keeping file names separate during the restart procedure, but I am pretty shure I am missing the point of physics envirorments.
As you know, during the restart procedure, the rotor mesh rotates. Should I update the physics I have written in the previous step? That's the point I cannot understand, and that's maybe the reason why I fell into save/resume commands. I think that physics envirorments don't take account of geometry, but only of material propertier/element types/loads/DOFs. However, after the first rotation of the mesh, when I load the thermal physic, Ansys give me an error: shape testing revealed that 7 of 7970 new or modified elements violate shape error limits.
If I skip this error, after a couple of iteration in the *do loop, I have the same convergence problem I was talking about in the previous post, in the structural analysis. I really can't understand why. I also issued the command upcoord,-1,on to see if it's a problem of large deformation mesh. I set this parameters for air:
MP,dens,13,1
mp,NUXY,13,0
mp,EX,13,1
MP,EY,13,1
MP,EZ,13,1

I hope to solve my problem ASAP.
Best regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Dec 09, 2014 8:01 am  Reply with quote

Sorry for the double post:
I was thinking about the air distortion: yes, in the 4th loadstep it begin becoming highly distorted...but I let the interface to slide only during the magnet analysis...How should I constraint that part? I only use ceintf,ux and ceintf,uy and the program seems to accept them.
Regards.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Jan 06, 2015 3:06 am  Reply with quote

mike.yaksh wrote:
Davide

On a motor thermal model, I specified a film coefficient for the outer surface of the model.

Mike Yaksh
NAC International
Norcross GA



Hello everyone.
In the previous days a made some couple field simulation with quite good results. Anyway, regarding the thermal part, I am still imposing a temperature in the outer part of the stator yoke, cause I can't define a film coefficient. Have you any idea to suggest me regarding the definition of a film coefficient in a couple field analysis?
I mean, I have a forced air cooling, which requires the definition of a convection coefficient. What I would do is to design an air layer outside the stator (plane55 with keyopt(9)=0) and assign to that region a temperature of 20°C. Then I would design the stator with plane55 as well, but I have no idea about how to set the keyopt(1).
Another couple questons:
1)would it be better to consider the stack lenght through the keyopt(3)=3 and setting up the proper real constant?
2)Is there a way to consider the effects of air turbulence in the airgap?

Thanks in advance.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Tue Jan 06, 2015 8:21 am  Reply with quote

Davide,
If you were to apply a film coefficient for the forced convection, then it would be applied to the model surface. There is no need to model the air outside the model for the thermal. Most heat transfer books have sections on forced convection and the corresponding h's. The h will vary along the surface, or you could input the minimum value which would provide bounding temperature. The h's are also dependent on temperatures, since they depend on the air properties, which depend on temperature. It is easy to implement an h dependent on temperature through the HF property. If the h varies with position, I would have to define a temperature dependent HF for each element along the surface.

On Keyopt(1), most text will refer to a film temperature which is the average between the surface and the ambient. I have seen from natural convection tests, this tends to be conservative, and keyopt(1)=1 gives better agreement. With forced convection, the Delta-T to the ambient is less, and the difference might not be as great as for natural convection.

I either solved the thermal problem as a 2D or a 3D. If it was done as a 2D, I did not bother with the thickness option, since I assumed that the heat generation and the h's did not vary in the axial direction. I have solved 2D magnetic problems since it was a good fit, but did a 3D thermal due to fins on the motor end.

For the air gap, which has been of interest since the first motor, and there has work done on this. This is an old paper around that have means to compute an effective thermal conductivity in the air gap. I have use this, but did not see much effect on the stator coil winding. On the rotor side, when we had a heat problem we did not rely on the air gap to solve the problem. The only time, I have seen otherwise, was in a sea application in which water flowed between the rotor and stator.



Mike Yaksh
NAC International
Norcross GA

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Tuesday, January 06, 2015 5:06 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM


mike.yaksh wrote:
Quote:
Davide

On a motor thermal model, I specified a film coefficient for the outer surface of the model.

Mike Yaksh
NAC International
Norcross GA




Hello everyone.
In the previous days a made some couple field simulation with quite good results. Anyway, regarding the thermal part, I am still imposing a temperature in the outer part of the stator yoke, cause I can't define a film coefficient. Have you any idea to suggest me regarding the definition of a film coefficient in a couple field analysis?
I mean, I have a forced air cooling, which requires the definition of a convection coefficient. What I would do is to design an air layer outside the stator (plane55 with keyopt(9)=0) and assign to that region a temperature of 20°C. Then I would design the stator with plane55 as well, but I have no idea about how to set the keyopt(1).
Another couple questons:
1)would it be better to consider the stack lenght through the keyopt(3)=3 and setting up the proper real constant?
2)Is there a way to consider the effects of air turbulence in the airgap?

Thanks in advance.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Tue Jan 06, 2015 8:53 am  Reply with quote

Thank you Mike,
I will apply convection coefficient using SF,all,conv,... command, then I will map the coefficient using MPDATA,HF,...
I will neglect the thickness and the heat exchange with the air in the airgap. I will only apply the CE's to tie togheter airgap nodes.
I didn't received the paper you were talking about converning the airgap heat exchange, but it's not a problem since I will neglect that aspect.

Just another question concerning a magneto-structural CF probelm: is there a way to consider the displacement effects on the resulting torque during a couple field analysis performed with physics envirorments? I would think to use ldread,ux and ldread,uy just before every magnetic transient restart, after every structural transient restart...But I don't think that the magnetic physic is bale to read displacements...

Thank you very very much.
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Tue Jan 06, 2015 10:01 am  Reply with quote

Davide

It depends the solution method. If you are using plane13 with displacements and AZ, then NLGEOM,on should take it into account. If you doing the cycle of EMAG, structural, EMAG..., then you could return to the preprocessor long enough to use UPCOORD,1 on the stator side. I do not think that I have tried that with a restart on a transient before. You might have more deformation due to an off centered rotor. I used to run solutions where the rotor was off centered which generated large forces to pull the rotor more off centered. They were usually a series of static analyses and was not concerned with restarts.

Mike Yaksh
NAC International
Norcross GA

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of davide.rossi
Sent: Tuesday, January 06, 2015 10:54 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [EMAG][STRUCT] Magneto-structural 2D transient analysis EM

Thank you Mike,
I will apply convection coefficient using SF,all,conv,... command, then I will map the coefficient using MPDATA,HF,...
I will neglect the thickness and the heat exchange with the air in the airgap. I will only apply the CE's to tie togheter airgap nodes.
I didn't received the paper you were talking about converning the airgap heat exchange, but it's not a problem since I will neglect that aspect.

Just another question concerning a magneto-structural CF probelm: is there a way to consider the displacement effects on the resulting torque during a couple field analysis performed with physics envirorments? I would think to use ldread,ux and ldread,uy just before every magnetic transient restart, after every structural transient restart...But I don't think that the magnetic physic is bale to read displacements...

Thank you very very much.

------------------------
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France






+-------------------------------------------------------------+
| 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 xansys-mod@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 xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
davide.rossi
User


Joined: 30 Jul 2014
Posts: 29
Location: Italia - L'aquila / Francia - Amiens

PostPosted: Wed Jan 07, 2015 1:41 am  Reply with quote

Thank you Mike,
I already tried both nlgeom,on and upcoord, but with a factor equal to -1 to cancel the large displacements which used to cause errors during my simulations, but I have problems with both of them:
1) If I use nlgeom,on I get very large displacement if the air elements, which causes the mesh to deform to much and somme errors to occur after some loadsteps. Regarding this point, as you previously suggested, I modeled air with "softer" properties compared to the other materials which the machine is composed. In detail:
! air
MP,dens,2,1
mp,NUXY,2,0
mp,EX,2,1E5

Do you think they could be ok?

2)If I use upcoord,-1 in a couple field multiphysics environment I get mismatching meshes between emag and structural loops. That's because the upcoord,-1 command cancels the displacement. Now I will try with upcoord,1 and I'll let you know. Actually, while I perform a structural analysis, I get deformed shapes both in radial and in tangential directions. I am afraid that if I upcoord,1 the mesh would move on in the tangential direction, which means that I would lose my synchronism. I am interested only in the radial displacement. Anyway, I will try.

Thank you very much!
_________________
Davide Rossi
Grantholder in electrical engineering
ESIEE - Amiens / UPJV
Amiens - Picardie - France
Back to top
View user's profile Send private message Send e-mail
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
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


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron