×
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

load on a circle and Axialsym model

load on a circle and Axialsym model

load on a circle and Axialsym model

(OP)
1) one question about how can apply the load: can we apply a pressure on a line with abaqus?how?I have tried but abaqus don't accept. Also if I want to applya line load on a circle how I can do?I have tried to do a partition with a circular line but when i apply the load abaqus doesn't accept the oad on the line!!

2) I have tried to modeled a circular plate subject to a circular load using the 2D axialsym shellsection    deformable model.I used for preprocessing abaqus cae but the program didn't work. I had one error in the mesh and anoter in the input file but I didn't find  the error. I report my steps:
a)I model the plate  drawing the sketch of a rectangular section
b)I define the material isotropic elastic
c)define of section:shell homogeneous with thickness of the shell like the plate that I want to model
d)assignement of the section at all te plate
e)partition of the plate i order to apply a pressure like with a ring
f)mesh  element type is a critical point and I'm not sure bout what element I have to choice (any ideas??)
g)apply boundary condition for axialsym and plate then load
H)create of job then submit

but the program said to me I have one error in the input (what??))

thanx nikko

RE: load on a circle and Axialsym model

The element type must be consistent with the type of section you assigned to the part.

I am a bit confused about what you are trying to do.

If the real 3D part is characterized by axis symmetry, your 2D model should contain half of the axial section of the part. When you say "circular plate", do you mean that the axial section you modeled is a thin rectangle ? At least this is the way I would model a circular plate buy taking advantage of axis symmetry.

If you have an inner partition then you cannot create a 2D surface based on the partition edges and neither you can apply loads which require surfaces as support. You can apply boundary conditions on these inner partition edges though.

RE: load on a circle and Axialsym model

If you have an error in the input then it will tell you what the error is in the dat file. It'd be better if you said what that error message says.

corus

RE: load on a circle and Axialsym model

(OP)
thanx for the replies

I try to explain better:

real problem: a ring apply a normal force on a circular plate with thickness of 500 micronmeter at radius  r

Model: 2D analsys of circular plate (thickness smaller then te other two dimension) with a circular load applied at radius r

My first question was about the load: I find out that I can apply a pressure if I use the partition on a ring surface, but I can't found how apply a load on a circle with abaqus cae. any ideas?!

second about the element type: what means consistent with the type of sections? I think in this case a plate can be modeled with shells , but when I have to choice the element type for the mesh I have not very clear what diference if a choice qudratic or linear and hybride etc..for my application that is static and with very small displacement probably linear element type is good?!
the thickness of the shell must be like the thickness of the  plate?

About the axialsym sure the section I modeled is a thin rectangle.

How can I read the file .dat?

thanx

 

RE: load on a circle and Axialsym model

You can read (ABAQUS's) .dat file using any text editor. It is a text file.

Other text files that may contain useful information are:
.sta
.msg
.log

RE: load on a circle and Axialsym model

As Corus said, providing the error message(s) could help figuring the problem.

RE: load on a circle and Axialsym model

(OP)
I have found this coments in the file .dat:

ERROR: 41 elements have missing property definitions. The elements have been identified in element set ErrElemMissingSection.
 ***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO INTERPRET SOME DATA.  SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION

RE: load on a circle and Axialsym model

(OP)
and after:


*Element, type=CAX8


P R O B L E M   S I Z E


          NUMBER OF ELEMENTS IS                                    41
          NUMBER OF NODES IS                                      208
          NUMBER OF NODES DEFINED BY THE USER                     208
          TOTAL NUMBER OF VARIABLES IN THE MODEL                  416
          (DEGREES OF FREEDOM PLUS ANY LAGRANGE MULTIPLIER VARIABLES)





          THE PROGRAM HAS DISCOVERED     1 FATAL ERRORS

               ** EXECUTION IS TERMINATED **
It's not veruy clear about the inpu error, is it possible is the same error of the element type for the mesh???
How I can decide the right properties for thus elements??

RE: load on a circle and Axialsym model

The properties you define for the 2D axisymmetric elements are the same as for any other element, ie. Young's modulus, poisson's ratio. They're not strictly shell elements as such as they have depth in the axial direction. I don't think Abaqus does thin shell axisymmetric elements. The loads you apply are defined as loads per unit circumference, or N/mm. The error occurs because you haven't assigned materials to the elements. 8 noded quadrilateral elements are fine. The only thing that is confusing is you say you have defined a circular line. How can that be on an axisymmetric model unless you're modelling a sphere?

corus

RE: load on a circle and Axialsym model

(OP)
yes sorry before I have not explained well. the load is a pressure on a piece of segment of the rectangle. I have defined the material properties (E and Poisson ratio) but how this propertis can create problem to the elements type I don't understand..or is it speaking about geometry properties??

RE: load on a circle and Axialsym model

"ERROR: 41 elements have missing property definitions. The elements have been identified in element set ErrElemMissingSection "

You did not assign a section the part.

In CAE->Property Module ->Menu -> Section ->Create
Category->Solid
Type->Homogeneous

Then use:
CAE->Property Module ->Menu -> Assign ->Section
Select part and assign the created section.

The element type you selected (CAX8) should be ok.

RE: load on a circle and Axialsym model

(OP)
I had already assigned the section part like you show above, this is not the cause of the error..

RE: load on a circle and Axialsym model

(OP)
one point:
under section property after I have defined the type of section solid homogeneus it ask for the shell thickness, I'm not very sure about this value. Is it reasonable the same value of the thickness of the plate. or different?

RE: load on a circle and Axialsym model

(OP)
I found the error some days ago but in these days I couldn't respond. When I define the section I defined shell section but he needs solid section.. my question is why if I have defined a 2D problem??
resume of the problem:

circular plate (small thickness) with circular load on a cicle  at r0: then axisymmetric problem.

I have modeled the plate in the modeling space axisymmetric with shell base feature. then why the section has to be solid??

Other question:

when you write an input file if you want to mesh like in this case the rofile of the plate then a rectangle:

(eg bias etc) have defined the node how you can fill. In particular. How you can choice choice the parameter of NFILL.
 
 

RE: load on a circle and Axialsym model

Quote (nikko801):

When I define the section I defined shell section but he needs solid section.. my question is why if I have defined a 2D problem??
resume of the problem:

Because an axisymmetric element is a 2D abstraction of a 3D model - hence it requires 'solid' element properties.

Regards

Martin

RE: load on a circle and Axialsym model

(OP)
"Because an axisymmetric element is a 2D abstraction of a 3D model - hence it requires 'solid' element properties.

from Martin"


This is a good point..I'm a bit confusing...

it' not clear if when you define the section then oyou have consequence on the kind of analysis
I mean the analisys with solid section is 2D or 3D?

Can you use shell 2D elements or continuum (solid) elements with solid section?

RE: load on a circle and Axialsym model

Axisymmetric elements (CAX3, CAX4) are classified in ABAQUS as continuum elements - so the properties are defined with the *SOLID SECTION keyword.  If you try and assign a *SHELL SECTION to axisymmetric elements, you will get an error, as you have already found out.  Axisymmetric elements have no thickness, as they are a 2D simplification of a revolved object.

I admit that it may seem confusing - *SOLID SECTION is also used to assign properties to 3D hex and tet solid elements.

Axisymmetric shells (SAX1) are different, as they do have a thickness in the x-y plane - hence their properties are set with the *SHELL SECTION keyword, with a thickness given on the data line.

Regards

Martin

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