Error Flexion 3-point

[moliPHD]

Hi friends,
I'm a new user of Ansys MAPDL, I'm trying to simulate a 3-point flexion on a sandwich plate, with an orthotropic heart, form honeycomb, and isotropic skins,i entered the properties of each type of material "orthotropic" and "isotropic", but Ansys didn't give me the solution and it gave me an error which is as follows:

"""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""
*** WARNING *** CP = 61.578 TIME= 22:54:34
Real constant 1 referenced by at least element types 1 and 2.

*** ERROR *** CP = 61.875 TIME= 22:54:38
The stress-strain matrix of material 2 is not positive definite, which
is required for real materials. Being positive definite means that
1.0 - PRXY**2*EY/EX - PRYZ**2*EZ/EY - PRXZ**2*EZ/EX -
2.0*PRXY*PRYZ*PRXZ*EZ/EX must be positive, but is equal to
-0.232529848. Consider reducing the Poisson's ratios.

EX = 1.25699039 EY = 171.492141 EZ = 1.50097534
PRXY = 5.47E-04 PRYZ = 0.32999577 PRXZ = 1.01537285
GXY = 307.804205 GYZ = 8.27121944 GXZ = 0.319477005.
"""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""

I checked the values of the properties of materials a few times, are all fair, I didn't understand where is the error,
Please help me find the solution.

Thank you so much

 

[0rel]

Hi,

PRXY = 5.47E-04 PRYZ = 0.32999577 PRXZ = 1.01537285

I'm not familiar with orthotropic materials but isn't the value of PRXZ false & impossible ? (> 1)

Regards

 

[moliPHD]

Thank you very much for your answer Mr. 0rel

concerning the value of "PRXZ", when i changed it to 0.5, Ansys mentioned this error
"" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" ""
  Real constant referenced by at least one element types 1 and 2.
"" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" "" ""
I clicked "yes", at the end it mentioned "solution is done"
what does mean this error?

here are the properties of each material

! isotropic materiel

ET,1,SHELL63
R,1,0.075, , , , , ,


MP,EX,1,69000
MP,PRXY,1,0.33


! orthotropic materiel

ET,2,SHELL63
R,2,0.075, , , , , ,


MP,EX,2,1.25699039

MP,EY,2,171.4921411

MP,EZ,2,1.500975344

MP,PRXY,2,5.47E-04

MP,PRYZ,2,0.32999577

MP,PRXZ,2,0.5

MP,GXY,2,307.8042053

MP,GYZ,2,8.271219444

MP,GXZ,2,0.319477005

 

[0rel]

It's just a warning, not an error, i.e. doesn't block the solve, but might lead to errors in your results.

Can you copy the lines where the mesh creation is done please ?

 

[moliPHD]

I meshed the entire plate (heart + skins), this is the code:

For example:
Heart:
"""""""""""""""""""""""""""""""""""""
ASEL,S,LOC,Y,hp+((1/2)*haut)
ESIZE,ray/4
AMESH,all
""""""""""""""""""""""""""""""""""""""""
skin:
"""""""""""""""""""""""""""""""""""""""""
ASEL,S,LOC,Y,0
AESIZE,ALL,ray/4
AMESH,all
"""""""""""""""""""""""""""""""""""""""""""

 

[0rel]

You don't give enough information.

Where do you tell Ansys which type and real to use for your areas ?

Try using AATT (see the help to use it) or
TYPE,X
REAL,X
MAT,X
AMESH,all
etc...

I think you don't set the real constant to use and thus, Ansys uses the last defined one.

 

[moliPHD]

ah, ok sir, sorry I didn't understand what did you want
Ok, if we take for example the area (59mm*24mm) localised in Y=0, this is the code of meshing of this area:
"""""""""""""""""""""""""""""""""""
ASEL,S,LOC,Y,0
AATT,1,0.075,1
TYPE,1
REAL,0.075
MAT,1
AESIZE,ALL,ray/4
AMESH,all
""""""""""""""""""""""""""""""""""""""
When I change the dimension of the area to (148mm*39mm) Ansys displays this warning
"""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""
*** WARNING *** CP = 307.641 TIME= 23:21:54
Shape testing revealed that 3 of the 9812 new or modified elements
violate shape warning limits. To review test results, please see the
output file or issue the CHECK command.
"""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""""
I simulate with Ansys MAPDL.
I don't understand why this warning didn't display when I use (59mm*24mm) like dimension of the area.

Regards

 

[0rel]

Try using,

R,1,0.075
REAL,1
or AATT,1,1,1

Number in AATT or REAL command is the real constant set, not the real constant value.


the shape warning will depends on the form of the elements. 3 out of 9800+ elements is almost nothing, just check they are not at the point of interest.