ANSYS simulation of beam with variable Modulus of Elasiticity (E)

[nzaza]

Hello all,

I need help in how could I model a beam which has a variable modulus of elasticity along its length (lets call this the x-direction).
Originally the modulus of elasticity was obtained as a function, but I could settle for breaking the beam in little bits and assigning a different value to each of these sections. I have not been able to overcome this issue. I am not very proficient with ANSYS workbench so maybe there lies the issue. Any input is greatly appreciated.

Thanks

 

[assafwei]

Hi,

If breaking the beam is good enough this is easy to perform, regarding modulus as a length function, I dont know ANSYS good enough to answer this.
You can split the beam to small pieces using design modeler (how many splits depends on you), then create an equivelent number of materials with different modulus and assign each material to each part of the beam. Don't forget in design modeler to create one part from all the pieces (by selecting all the pieces right click on with the mouse and choosing "form part") this will assure that you have a continuous mesh and that the part will be analysed as one part.
This is the easiest method that I can think of, but maybe you should wait to the more experienced ANSYS users with a better answer.

Best regards.

 

[Stanum]

I would use following macro, commented part is not very efficient if your model is large, but it gives a more precise result.

finish
/CLEAR,NOSTART
/units, si
/filname, mat_mod_change
/title, mat_mod_change
/OUTPUT, mat_mod_change_1, txt, , D:\ANSYS files
/PREP7

a=5
b=2
c=4

nus=0.34
kolt_X=20
*dim,Es,table, kolt_X, , , X, , , 0
*do, i, 1, 20
Es(i,0)=i
Es(i,1)=(i**5)*100+150e9
*enddo

!element type
ET,1,186

!geometry creation
block, 0, a, 0, b, 0, c

!mesh
ESIZE,0.2
MSHAPE,0,3d
MSHKEY,1
VMESH,all

!material properties
!*get, elem_count, elem, 0, count
!*do, ii, 1, elem_count
! *get, elem_num, elem, 0, num, min
! x_loc=CENTRX(elem_num)
! MP,EX,ii,Es(x_loc,1)
! MP,NUXY,ii,nus
! MAT, ii
! emodif, elem_num
! Esel, u, elem, , elem_num
!*enddo

kolt=20
x1=a/kolt
*do, ii, 1, kolt
esel, s, cent, x, x1*(ii-1), x1*ii
MP,EX,ii,Es(x1/2+x1*(ii-1),1)
MP,NUXY,ii,nus
MAT, ii
emodif, all
*enddo

 

[Reitzel]

Just make the Young's modulus temperature dependent and apply a temperature. That way you avoid slicing the beam and thus having discontinuous stress across edges all over your model. Just keep in mind that the environment temperature (found by clicking your static structural inside ANSYS Mechanical) is 22 degrees celcius per default. This means that at 22 degrees celcius nothing happens. Example: You want your Young's modulus to be 1 at x=0 and 0 at x=L. Then you specify, that for 22 degrees celcius the Young's modulus is equal to 1, and for e.g. 23 degrees celcius (this value can be anything else than the environment temperature) the Young's modulus is equal to 0. Just remember to delete the coefficient of thermal expansion from the material definition.

 

[nzaza]

Excellent information I appreciated greatly. It kind of works now.
Maybe I will have to create another thread for this but how do I simulate a two-span beam. Simple one with extra support in the middle equidistant from both ends.

Thanks a lot!!!

 

[Reitzel]

Just model it like you modelled your one span beam?

 

[nzaza]

I got the two span beam. But the solution with temperature is not working. Eventhough it was the simpler one to implement. It is not letting me solve the model. What could be the mistake that is producing this mistake? I am almost sure that I deleted the coefficient of thermal expansion.

Any other advise?

Thanks greatly

 

[Reitzel]

Check the solution information for more information regarding the error.