CONNECTION BEAM AND SHELL ELEMENTS

[FRANCESCA PISTORIO]

Hi everyone!

I have a doubt and I hope there is someone who can give me an advice.

I am modeling a MEMS gyroscope for my Master thesis and I am starting with a very basic structural design. My gyroscope is composed by a central mass suspended by for beams. Since the central mass thickness is smaller than other dimensions, I modeled it with shell181 elements, while beam are modeled using beam4 elements. Since these elelements have the same DOFs, can I connect them simply sharing the nodes at interface? I ask this because I have read on the 2.3 section of ANSYS APDL 2019 R3 guide ("Limitations on Joining different elements") that tt is inconsistent to connect only one node of a 3-D beam element to a 3-D shell element such that a rotational DOF of the beam element corresponds to the ROTZ of the shell element.

Moreover, I performed a modal analysis in order to obtain the eigenfrequencies of my structure. I noticed that, if I mesh the central mass with a coarser mesh, my result is closer than the analytical one. I can't explain this and I'm scared that it is linked to the previous concept.

I share  my APDL code (I hope it will be useful).

Thanks for the help.

Kindest,

Francesca

finish

/clear

/PREP7

!GEOMETRY 

E=166e3

densi=2332e-18

A1=500                 ! Weidth mass 1 (micron)

B1=500                 ! Hight mass 1 (micron)

T1=15                  ! Thickness mass 1 (micron)

tol=0

!Suspension mass 1

L1X=200

L1Y=200

w1=4

! Spring 

ET,1,beam188

SECTYPE,1,beam,rect

SECDATA,w1,t1

mp,ex,1,E

mp,dens,1,densi

mp,prxy,1,0.28

real,1

type,1

! First suspension

K,1,A1/2,B1/2,0

K,2,A1/2,B1/2+L1x,0

K,3,A1/2+L1y,B1/2+L1x,0

L,1,2

L,2,3

esize,40

real,1

type,1

lmesh,all

! Second suspension

K,4,-A1/2,B1/2,0

K,5,-A1/2,B1/2+L1x,0

K,6,-A1/2-L1y,B1/2+L1x,0

L,4,5

L,5,6

esize,40

real,1

type,1

lmesh,all

! Third suspension

K,7,-A1/2,-B1/2,0

K,8,-A1/2,-B1/2-L1x,0

K,9,-A1/2-L1y,-B1/2-L1x,0

L,7,8

L,8,9

esize,40

real,1

type,1

lmesh,all

! Fourth suspension

K,10,A1/2,-B1/2,0

K,11,A1/2,-B1/2-L1x,0

K,12,A1/2+L1y,-B1/2-L1x,0

L,10,11

L,11,12

esize,40

real,1

type,1

lmesh,all

LSEL,U, , , ALL     

! Mesh mass 1

ET,2,shell281

SECTYPE,2,SHELL

secnum,2

SECDATA,T1,

mp,ex,2,E

mp,dens,2,densi

mp,prxy,2,0.28

LSTR,1,4                      

LSTR,7,10

LSTR,1,10

LSTR,4,7

AL,ALL                          ! Creo area

esize,50

real,2

type,2

asel,s,loc,x,-A1/2,A1/2,-B1/2,B1/2

amesh,all

!Nummrg,node,0                    !Merges coincident or equivalently defined nodes.

! Boundary condition

Ksel,s,,,3

nslk,s

d,all,all

Ksel,s,,,6

nslk,s

d,all,all

Ksel,s,,,9

nslk,s

d,all,all

Ksel,s,,,12

nslk,s

d,all,all

/SOLU

nsel,all

antype,modal

modopt,subsp,4

mxpand,4,,,yes

nsel,all

solve

/POST1               ! List solutions

SET,LIST

SET,FIRST

[P.M.Deshmukh]

Can you explain it by ppt, it will be more clear to us.

--
You received this message because you are subscribed to the Google Groups "Ansys" group.
To unsubscribe from this group and stop receiving emails from it, send an email to ansys+un...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/44a5eee7-6a51-40aa-97c6-763e8e803546n%40googlegroups.com.

[FRANCESCA PISTORIO]

Thank you for the answer and sorry for the few details. I share a ppt and i hope it will be clear.

Kindest,

Francesca 

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/CALPsm4mYovd%3DfV1JKLO6F3fCWRt-j5%3DtyCHkRatpTdoJwbJZEA%40mail.gmail.com.

[Serkan Guler]

Have you tried to model all the legs with shell element as well? 

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/CABHJzB33ur%3Db%3DJsqpfvc-m-FhTo2oEejixxtkqhcfr78pUi3Bg%40mail.gmail.com.

[FRANCESCA PISTORIO]

Yes I have tried and it works. However, the crucial point is that I would use beam elements since suspensions are actually beams. This is a simple initial structure but if the model becomes more complex, I think beams are computationally more efficient. So I hope to find the way to link beam and shell together (if it is possibile)! 

[Serkan Guler]

I understand your concern regarding computation. You should try to combine the shell and beam with CP command or MPC184 element. 

On Sat, 22 Aug 2020, 21:32 FRANCESCA PISTORIO, <francesca....@universitadipavia.it> wrote:

Yes I have tried and it works. However, the crucial point is that I would use beam elements since suspensions are actually beams. This is a simple initial structure but if the model becomes more complex, I think beams are computationally more efficient. So I hope to find the way to link beam and shell together (if it is possibile)! 

--
You received this message because you are subscribed to the Google Groups "Ansys" group.
To unsubscribe from this group and stop receiving emails from it, send an email to ansys+un...@googlegroups.com.

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/CABHJzB2kEq%3DbpfDvxS5ySKZqBrQUKWr8EuD9kEr25KC1_udvXw%40mail.gmail.com.

[Francesca Pistorio]

Dear Serkan,

 

thank you so much for your suggestion. I have tried to use cerig command between the node at the interface and the two adjacent shell element nodes. I wanted to couple the ROTZ degree of freedom of the interface node with the in-plane traslational dofs of adjacent shell element nodes. I share you a piece of my APDL code:

The master node is the node at the interface between beam and shell elements, while slave nodes are the adjacent shell element nodes.

 

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

nsel,s,,,master_node

nsel,a,,,slave_node1

cerig,master_node,slave_node1,ux,uy,rotz

 

 

nsel,s,,,master_node

nsel,a,,,slave_node2

cerig,master_node,slave_node2,ux,uy,rotz

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

 

In this way, I managed solve the problem relating to the frequencies calculation when refining the mesh. However I noted that now the vibration mode shapes are inverted respect to what I expect (I simulated using all shell elments and solid elements in order to make a comparison).

Any insight about this?

 

Kindest,

 

Francesca

 

 

Inviato da Posta per Windows 10

 

Da: Serkan Guler
Inviato: sabato 22 agosto 2020 21:04
A: an...@googlegroups.com
Oggetto: Re: CONNECTION BEAM AND SHELL ELEMENTS

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/CAGxMoBS%2BqMzZM%3DVDLrZwiC7foQq3ZOqY5pxWgWsD4MZnvObGjA%40mail.gmail.com.

 

[Serkan Guler]

Dear Frencesca,

I am happy to help you. Please try to use code written below for defining coupling between the nodes. I wrote the code for all DOF however you can use what you need. Let me know any problem with this issue, good luck.

Best wishes,    

!======= CODE BEGIN =======

n=1      ! arbitrary Constraint Point number 
n1=11   ! master node 
n2=12  ! slave node

cp,n+1,ux,n1,n2
cp,n+2,uy,n1,n2
cp,n+3,uz,n1,n2
cp,n+4,rotx,n1,n2
cp,n+5,roty,n1,n2
cp,n+6,rotz,n1,n2

  !======= CODE END =======  

Francesca Pistorio <francesca....@universitadipavia.it>, 23 Ağu 2020 Paz, 14:16 tarihinde şunu yazdı:

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/BEC43572-BF1B-4D50-8981-6EC9550D6131%40hxcore.ol.

--

Saygılarımla/Sincerely

Dr. Serkan Güler

İskenderun Teknik Üniversitesi
Mühendislik ve Doğa Bilimleri Fakültesi
Makine Mühendisliği Bölümü
31200 İskenderun-Hatay- TÜRKİYE
Telefon: +90 326 613 5600/ 4611

=============================

Dr. Serkan Guler

Iskenderun Technical University
Engineering and Natural Sciences Faculty
Dept. of Mechanical Engineering
31200 Iskenderun-Hatay- TURKEY
Phone: +90 326 613 5600/ 4611

[Francesca Pistorio]

Dear Serkan,

thanks for the help, now my simulation seems to work!!!

 

Kindest,

Francesca

 

Inviato da Posta per Windows 10

 

Da: Serkan Guler
Inviato: domenica 23 agosto 2020 14:30

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/CAGxMoBSfmxsBrYifbzRwSy3o9Ekeu8Rzt%2BrZdUvj7qjV_%3D9Qhw%40mail.gmail.com.

 

[Serkan Guler]

Dear Frencesca,

You are very welcome. Sounds are good. Happy that your model is working. Please feel free to ask any questions. 

Best wishes,

Serkan

To view this discussion on the web visit https://groups.google.com/d/msgid/ansys/A282CE45-F8D0-4EBA-83BA-E0A567BCB155%40hxcore.ol.