3 pointing bending test of sandwich

  • 75 Views
  • Last Post 11 October 2019
Prashank posted this 07 October 2019

Hi

i am trying to simulate the 3 point bending test on honeycomb type sandwich panel according to ASTM-393 norms.

i am using solid core geometry with same orthotropic properties as that of honeycomb geometry core.

i meshed sandwich with shell-solid-shell elements.

To simulate the pressure pads i made a face on upper face sheet and then applied remote force. For roller supports i drew the center lines of rollers on lower face sheet and then fixed it by remote displacement.

 

By the above boundary conditions i got the bending stress in the face sheet close to the analytical value(~2 %) but the deformation predicted by ansys is about 23% lesser than the analytical one. Similarly the shear stress in core is 100 times lesser than the analytical.

in this discussion, peter suggested to use the 1/4 th of the model.

1. Ansys used Solid 186 elements to mesh solid core geometry. Will the honeycomb core behavior  be captured by the solid core with this mesh element. 

2. What is the advantage of using 1/4th model? And how i can use it.( i modeled the face sheets in ACPs and solid core in the mechanical model).

 

ANALYTICAL METHOD:-

sanswich height , d=13.1mm

core height ,c = 12.7 mm

sandwich width, b=42 mm

young modulus face sheet, E =6900 Mpa

shear modulus core, G= 18.616 Mpa

load p =400 N

Length of , sandwich = 130 mm

 

 

Deformation D= PL^3 / 48S + PL / 4U

where  

panel bending stiffness S = E(d^2-c^2)xb/12

 panel bending rigidity U = G(d+c)^2 x b/4c

 D =1.6485 while deformation by ansys is 1.25 mm

 

Core shear stress

T = P/ (d+c)xb =0.369 Mpa

while by ansys it is 0.00373 Mpa

Face sheet bending stress 

B.S = PxL / 2t(d+c)b   =119 Mpa 

( face sheet thickness, t=0.2 mm)

 

 

 

Order By: Standard | Newest | Votes
peteroznewman posted this 07 October 2019

The deformation plot looks odd to me for roller support. Why do the ends of the beam beyond the supports look flat instead of continue with the slope that the beam in the center has?  Please show the Details of the Remote Displacement.  Are the roller supports free to rotate about Y?

Prashank posted this 08 October 2019

Hi Peter Whenever I free the rotation about y axis, I get an error" During the solution the elapsed time exceeded the CPU time by an excessive margin. Often this indicates either lack of physical memory ..". I have pretty good system configuration ( 8 GB Ram, 8 cores). This error occurs for deformable ,rigid , beam condition. Then i solved the model for coupled but I am not satisfied with the results. Can you suggest me some alternative to solve this model. I am using ACPs and design modeller and I don't know how to use symmetry ( 1/4 th of model)

peteroznewman posted this 08 October 2019

You can create a rigid cylinder and define frictionless contact.

To use half symmetry, edit the geometry and cut the model in half at a plane in the center. In Mechanical, right click on Model and Insert Symmetry. On the Symmetry folder right click and Insert Symmetry Region. Now pick the cut face, and set the Symmetry Normal to the X axis. Insert another Symmetry Region and pick the edges of the surface bodies at the center and set the Symmetry Normal. Then edit the Force and divide it by 2.

  • Liked by
  • Prashank
Prashank posted this 08 October 2019

I edited the geometry to cut the modal in half for both face sheets and core. 

But in mechanical i cant find the symmetry region.

peteroznewman posted this 08 October 2019

Reread my post above, "In Mechanical, right click on Model and Insert Symmetry."

Prashank posted this 08 October 2019

Yes I did it.
I right click on the model , inserted the symmetry folder and then I when I right clicked on the symmetry folder I have only one option i.e pre meshed cyclic region. ( Screenshot in the previous post)

peteroznewman posted this 08 October 2019

I see now.  I don't use ACP-Pre so I don't know how Symmetry works there. Maybe it doesn't work in an ACP-Pre model.

Prashank posted this 09 October 2019

Hi peter

 i increased my mesh element size. Then i got the following error. This error point towards the core.

i set the remote displacement condition with 0,0,0 in translation and 0,free,0 in rotation.

peteroznewman posted this 09 October 2019

You must use two Remote Displacements, one for each roller support. Delete the one you have because on creation, it sets its coordinate system based on the edge selected.

  • Liked by
  • Prashank
Prashank posted this 10 October 2019

Hi Peter... Do the shear stresses in the homogeneous core equal to their counterparts in honeycomb core...? Are there any allowances to be considered...?

peteroznewman posted this 10 October 2019

No. The shear stress in the homogeneous core is an average value while the shear stress in the cell walls of the honeycomb change on each facet.

  • Liked by
  • Prashank
Prashank posted this 10 October 2019

Can you please explain it briefly how does the shear stresses in the homogenized core is avg of the real honeycomb when the area of homogenized core is at least 30 times that of the honeycomb core?

 Analytically i  found this to be contradicting .

peteroznewman posted this 10 October 2019

Did you average in the zero shear stress of all the air that is between the honeycomb cell walls?  There is probably 30 times more air than wall.

Prashank posted this 11 October 2019

Okey...

But if we consider the air in between the walls ( where the shear stresses are zero) and the face walls for AVG, then the shear stresses in Walls must be atleast 20-30 times higher than the average (0.471 MPa)..

Do you think the above statement is true?

If not , can you please tell me the reason.

peteroznewman posted this 11 October 2019

You can either model the walls of the honeycomb to get a very detailed representation of how the load is carried in the walls of the honeycomb cells, OR you can have a solid brick that represents the smeared behavior of the core when looked at from a high level of the sandwich and its bending properties. They are very different models that different questions can be asked of.  Trying to equate the shear stresses between them is an academic exercise that I am not interested in.

Close