×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Error Flexion 3-point

Error Flexion 3-point

Error Flexion 3-point

(OP)
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

RE: Error Flexion 3-point

Hi,

Quote:

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

RE: Error Flexion 3-point

(OP)
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

RE: Error Flexion 3-point

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 ?

RE: Error Flexion 3-point

(OP)
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
"""""""""""""""""""""""""""""""""""""""""""

RE: Error Flexion 3-point

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.

RE: Error Flexion 3-point

(OP)
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

RE: Error Flexion 3-point

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources