load on a circle and Axialsym model

[nikko801]

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

 

[xerf]

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.

 

[corus]

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

 

[nikko801]

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

 

[xerf]

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

 

[xerf]

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

 

[nikko801]

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

 

[nikko801]

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??

 

[corus]

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

 

[nikko801]

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??

 

[xerf]

"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.

 

[nikko801]

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

 

[nikko801]

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?

 

[nikko801]

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.

 

[bassmanjax]

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

 

[nikko801]

"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?

 

[bassmanjax]

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