Orientation of composite material - C3D8 solid element

[khounlolei]

Hello All,

I would like to have some clarification concerning how to apply
orientation to composite material and then vizualise them. I know
there is different way to apply orientation:
- either defining a local CSYS and then assigning material
orientation with the local CSYS
- or using *ORIENTATION, DEFINITION=OFFSETTONODES with the local
nodes numbers in the input file.
I am using solid element C3D8 in ABAQUS 6.6 to model composite
material.

My questions are the following :
1- when you assign a material orientation to a section using a
defined CSYS-1, do you have to give the material properties of the
section in the global coordinate system, and ABAQUS will do the
transformation by himself, or in the local coordinate system (CSYS-1)?

2- And when you visualise the results (i.e stress and strain), does
ABAQUS give the result in the global coordinates or in the local
coordinates (CSYS-1) for the oriented section ?

3- Using the*ORIENTATION, DEFINITION=OFFSETTONODES instruction, is
there a way to define it so that one direction is always normal to
one surface (like a cylindric coordinate system, but for complex
shape such as an airfoil)?
Using the mesh stacking orientation tool, I am able to verify if my
elements are all oriented in one direction, for example the
longitudinal direction but then the local orientation of my element
seems to rotate randomly around this axis, and I have to change the
orientation locally to have all the "out of plane" direction of my
elements in the same direction.

Thanks a lot for your help and your advice !

Lolei

[BenZ]

1/In the new CSYS defined
2/In the CSYS, except for displacement components
3/OFFSET TO NODES is based on your element's connectivity. Itself is
based on how you have generated the mesh. To me the best way to
ensure a consistent connectivity is to manually extrude the mesh.

BenZ

Post by khounlolei
Hello All,
I would like to have some clarification concerning how to apply
orientation to composite material and then vizualise them. I know
- either defining a local CSYS and then assigning material
orientation with the local CSYS
- or using *ORIENTATION, DEFINITION=OFFSETTONODES with the local
nodes numbers in the input file.
I am using solid element C3D8 in ABAQUS 6.6 to model composite
material.
1- when you assign a material orientation to a section using a
defined CSYS-1, do you have to give the material properties of the
section in the global coordinate system, and ABAQUS will do the
transformation by himself, or in the local coordinate system (CSYS-

1)?

Post by khounlolei
2- And when you visualise the results (i.e stress and strain),

does

Post by khounlolei
ABAQUS give the result in the global coordinates or in the local
coordinates (CSYS-1) for the oriented section ?
3- Using the*ORIENTATION, DEFINITION=OFFSETTONODES instruction, is
there a way to define it so that one direction is always normal to
one surface (like a cylindric coordinate system, but for complex
shape such as an airfoil)?
Using the mesh stacking orientation tool, I am able to verify if my
elements are all oriented in one direction, for example the
longitudinal direction but then the local orientation of my

element

Post by khounlolei
seems to rotate randomly around this axis, and I have to change the
orientation locally to have all the "out of plane" direction of my
elements in the same direction.
Thanks a lot for your help and your advice !
Lolei

[jeffergj]

OFFSETTONODES is primarily useful if you have manually created the
mesh and so have complete control of the node order on the elements.
Don't count on an automatic mesh generator to order things in a
consistent way. Thats probably what you are seeing, adjacent elements
look to be oriented the same but internally the nodes are ordered
differently and so the 'offset' method gives a different material
orientation.

Post by BenZ
1/In the new CSYS defined
2/In the CSYS, except for displacement components
3/OFFSET TO NODES is based on your element's connectivity. Itself is
based on how you have generated the mesh. To me the best way to
ensure a consistent connectivity is to manually extrude the mesh.
BenZ

Post by khounlolei
Hello All,
I would like to have some clarification concerning how to apply
orientation to composite material and then vizualise them. I know
- either defining a local CSYS and then assigning material
orientation with the local CSYS
- or using *ORIENTATION, DEFINITION=OFFSETTONODES with the local
nodes numbers in the input file.
I am using solid element C3D8 in ABAQUS 6.6 to model composite
material.
1- when you assign a material orientation to a section using a
defined CSYS-1, do you have to give the material properties of the
section in the global coordinate system, and ABAQUS will do the
transformation by himself, or in the local coordinate system (CSYS-

1)?

Post by khounlolei
2- And when you visualise the results (i.e stress and strain),

does

Post by khounlolei
ABAQUS give the result in the global coordinates or in the local
coordinates (CSYS-1) for the oriented section ?
3- Using the*ORIENTATION, DEFINITION=OFFSETTONODES instruction, is
there a way to define it so that one direction is always normal to
one surface (like a cylindric coordinate system, but for complex
shape such as an airfoil)?
Using the mesh stacking orientation tool, I am able to verify if

my

Post by khounlolei
elements are all oriented in one direction, for example the
longitudinal direction but then the local orientation of my

element

Post by khounlolei
seems to rotate randomly around this axis, and I have to change

the

Post by khounlolei
orientation locally to have all the "out of plane" direction of my
elements in the same direction.
Thanks a lot for your help and your advice !
Lolei

[jeffergj]

You can specify a material coordinate orientation for the isotropic
elements as well if you want all stresses displayed in the 'laminate'
coordinate system.

[khounlolei]

Thanks a lot !

Another small clarification for my question 2:
If I have a model with oriented material (composite) and isotropic
material (aluminium mould), when I visualize my result, will ABAQUS
give them in the CSYS for all the assembly (mould + composite) or in
the CSYS for the composite and global coordinate system for the mould
(isotropic material) ?

Lolei

Post by BenZ
1/In the new CSYS defined
2/In the CSYS, except for displacement components
3/OFFSET TO NODES is based on your element's connectivity. Itself is
based on how you have generated the mesh. To me the best way to
ensure a consistent connectivity is to manually extrude the mesh.
BenZ

Post by khounlolei
Hello All,
I would like to have some clarification concerning how to apply
orientation to composite material and then vizualise them. I know
- either defining a local CSYS and then assigning material
orientation with the local CSYS
- or using *ORIENTATION, DEFINITION=OFFSETTONODES with the local
nodes numbers in the input file.
I am using solid element C3D8 in ABAQUS 6.6 to model composite
material.
1- when you assign a material orientation to a section using a
defined CSYS-1, do you have to give the material properties of the
section in the global coordinate system, and ABAQUS will do the
transformation by himself, or in the local coordinate system

(CSYS-

Post by BenZ
1)?

Post by khounlolei
2- And when you visualise the results (i.e stress and strain),

does

Post by khounlolei
ABAQUS give the result in the global coordinates or in the local
coordinates (CSYS-1) for the oriented section ?
3- Using the*ORIENTATION, DEFINITION=OFFSETTONODES instruction, is
there a way to define it so that one direction is always normal to
one surface (like a cylindric coordinate system, but for complex
shape such as an airfoil)?
Using the mesh stacking orientation tool, I am able to verify if

my

Post by khounlolei
elements are all oriented in one direction, for example the
longitudinal direction but then the local orientation of my

element

Post by khounlolei
seems to rotate randomly around this axis, and I have to change

the

Post by khounlolei
orientation locally to have all the "out of plane" direction of my
elements in the same direction.
Thanks a lot for your help and your advice !
Lolei

[Harrycha]

In the Field output window, there is an option that says "include local
coordinate directions when available". That means, I think, for composites
the values are oriented in material's principal axes whereas for isotropic
it is in global direction (if you have not assigned any CSYS for it). You
can easily check this out using simple example.

[Alex Bogdanov]

2. You can always transform results to user defined coordinate system
in viewer if you have doubts about default coordinates.

3. If you wish mesh stack direction were out of plane, prepare your
model as if you are going to use continuum shell elements (i.e. make
all mesh concerned with composites swept from one surface to another)

[MSD. Jacob]

Hi all...

Following up with your discussion: Please help me to the follwing doubts
1. how to read stress and strain in local CSYS. I am bit confused in
that part. Please advice me in details.
Tks in advance
Jacob