Changing a elastic material to orthotropic? 1

[JLZmech]

I had a .inp model, where i want to change one material from isotropic to orthotropic.
So in the .inp i have write:
*ELASTIC, TYPE=ORTHOTROPIC
1.,2.,3.,4.,5.,6.,7.,8.,
9.,

Being the 9 variables i need for this material. When i run the program it says that i should give the directions. How can I write that? I just want to be x,y,z, -> 1,2,3

The section and everythin is the same, i just want to change the material and rerun.

Thank you.

 

[FEA way]

*Elastic, type=orthotropic is used when you specify elastic stiffness matrix terms directly. You can also use *Elastic, type=engineering constants to define orthotropic behavior easier (by giving E,v and G in proper directions.

When it comes to directions, use:

*Orientation
x_a, y_a, z_a, x_b, y_b, z_b, x_c, y_c, z_c

where point a lies on x axis, point b lies in x-y plane and point c is the origin of the coordinate system.

 

[JLZmech]

Okey, so I have this:
*Material, name=Orto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,

And what i should write is this if i want the local material tobe the same as the x,y,z global:
*Material, name=Orto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,
*Orientation
1,0,0,1,1,0,0,0,0,


Have I understand it correctly?

Or maybe this will be better,if I want local coord to be cylindrical:
*Material, name=Orto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,
*Orientation
*ORIENTATION, NAME=Orientation, SYSTEM=CYLINDRICAL

THank you

 

[FEA way]

Settings that match global CSYS are:

*ORIENTATION,NAME=RECT
1.0, 0.0, 0.0, 0.0, 1.0, 0.0
1, 0.0

In the first line coordinates of point c (local CSYS origin) are omitted since the default location is global origin. Second line concerns additional rotation settings. These values are default.

If you want an example, check "Elastic materials" part of the Verification Guide.

Cylindrical CSYS is sometimes useful as well. An example problem called "Thick composite cylinder subjected to internal pressure" in Benchmarks Guide features this since the geometry is annular.

 

[JLZmech]

Abaqus si giving me the following error:

***ERROR: in keyword *ORIENTATION, file "MedOrto1_1.inp", line 1028010: The
keyword is misplaced. It can be suboption for the following
keyword(s)/level(s): assembly, instance, part

This is what i have written, just like the example i have seen:
*End Assembly
**
** MATERIALS
**
*Material, name=AleacionTi
*Elastic
114000., 0.31
*Material, name=CromoCobalto
*Elastic
200000., 0.3
*Material, name=ResinaOrto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,
*ORIENTATION,NAME=RECT
1.0, 0.0, 0.0, 0.0, 1.0, 0.0
1, 0.0
**
** BOUNDARY CONDITIONS

So, for what i have seen, it's write in the correct place, that's why i'm not understandig the error.
Also, if i wante to use cylindrical coord, just global coord, will it be like this:
*Material, name=ResinaOrto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,
*ORIENTATION,NAME=Cyl,SYSTEM=CYLINDRICAL
1.0, 0.0, 0.0, 1.0, 0.0, 0.0
1, 0.0

 

[FEA way]

Since your model is defined in terms of assembly, you should place *Orientation keyword at the part, part instance or assembly level. It seems that you’ve followed the example that is not defined in terms of assembly.

Orientation with cylindrical CSYS is defined in such way that you only give coordinates of two points located on the axial axis (global Z). So it can be:

*Orientation, name=Ori-1, system=cylindrical
0.0, 0.0, 0.0, 0.0, 0.0, 1.0
1, 0.0

 

[JLZmech]

Okey, thank you friend, I'm understanding abaqus much better thanks to your help.
So I write:
*Orientation, name=Ori-1, system=cylindrical
0.0, 0.0, 0.0, 0.0, 0.0, 1.0
1, 0.0
inside the assembly and the asing it to my material in the material section? And if gives the same problem, write it inside part section?
This could be a solution:
*Tie, name=TORNILLOIMPLANTE-1, adjust=no
S_SURF-1, M_SURF-1
*Orientation, name=Ori-1, system=cylindrical
0.0, 0.0, 0.0, 0.0, 0.0, 1.0
1, 0.0
*End Assembly
**
** MATERIALS
**
*Material, name=AleacionTi
*Elastic
114000., 0.31
*Material, name=CromoCobalto
*Elastic
200000., 0.3
*Material, name=ResinaOrto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,
*ORIENTATION,NAME=Ori-1
**
** BOUNDARY CONDITIONS

 

[FEA way]

In case of independent instances orientations are defined in the assembly section but in this manner:

*Assembly, name=...
*Instance, name=..., part=...
*Node
...
*Element, type=...
...
*Nset, nset=Set-1
...
*Elset, elset=Set-1
...
*Orientation, name=Ori-1, system=cylindrical
...
*Solid Section, elset=Set-1, orientation=Ori-1, material=Mat-1
,
*End Instance
*End Assembly

*Material, name=Mat-1
*Elastic, type=engineering constants
...

If you want to understand it better I suggest that you prepare simple analysis in CAE (no need to define loads and BCs, finish on mesh and assembly definition), write input file and review its content (or use Model—> Edit Keywords). Such approach can be very helpful, not only in this case.

 

[JLZmech]

Thank you, I will try it today and let you know how it went. The examples you told me had being very helpul.
Also I would like to ask another thing not related to this topic, Do you know any example that shows how to change a mesh size writing in the .inp? I whant to change teh size of an orphan mesh, a with Abaqus/CAE it is not possible.
The mesh is 0.5 global size and curvature control 0.25, minimum saize control by fraction of global size 0.1. What i want is to change the global size to different values. Is it possible?

 

[FEA way]

You can't change size of orphan mesh elements like you would do with native mesh. Only operations available in Edit Mesh toolbox are available in this case so you can for example manually edit nodal coordinates and do another local changes. But there is different way to remesh orphan part. Import it to CAE, convert to geometry (use Geometry Edit --> Face --> From element faces) and generate new native mesh for this geometry, this time using different size settings.

 

[JLZmech]

It isn't working is giving me some error. In the .inp i have the section assignments with the geometry i want, is it possible to do something with this? So i can recover that geometry.

Or is some way to remesh in the .inp? A mesh of around 300k element?

 

[FEA way]

I'm afraid that the only way to do it is to import your model to CAE and then recover geometry and mesh it. I did it several times with different models. Sometimes it's more difficult than usually because you may have complicated geometry. In such cases you have to select less element faces for conversion. Try using "by angle" or "by feature edge" selection options, it usually helps a lot. When you create faces for whole part remember to delete orphan mesh and use Create Solid --> From shell to convert the surface (shell) part to solid body.

If you do all of this and still keep getting error messages, can you show them here ? They usually tell you what's wrong with geometry.

 

[JLZmech]

Okei, i will let you know. Talking about the main topic, i changed the orientation and the program gave me this error:
***ERROR: THE *ORIENTATION OPTION REQUIRES DATA CARDS
Do you know that could this means?

 

[FEA way]

This probably indicates that there are no data lines beneath the *Orientation keyword in your input file.

 

[JLZmech]

Well I'm not understanding it, maybe a problem with the computer. This is what i wrote, maybe you can see the error:

**Orientation=ResinaOrto
*Orientation, name=Ori-1, system=cylindrical
** Section: Corona
*Solid Section, elset=SET-5, material=CromoCobalto
,
** Section: Tornillo
*Solid Section, elset=SET-6, material=AleacionTi
,
** Section: Cuerpo
*Solid Section, elset=SET-4, material=AleacionTi
,
** Section: Implante
*Solid Section, elset=SET-3, material=AleacionTi
,
** Section: Hueso
*Solid Section, elset=SET-2,orientation=Ori-1,
material=ResinaOrto
,
*End Part

*Assembly=....
* End assembly

*Material, name=AleacionTi
*Elastic
114000., 0.31
*Material, name=CromoCobalto
*Elastic
200000., 0.3
*Material, name=ResinaOrto
*Elastic, type=ENGINEERING CONSTANTS
12700.,17900.,22800., 5000., 5500., 7400., 0.18, 0.31
0.28,

*Boundary=...


Thank you.

 

[FEA way]

Take a look at this part (I removed the comments for clarity):

*Orientation, name=Ori-1, system=cylindrical
*Solid Section, elset=SET-5, material=CromoCobalto

So there’s no data line below *Orientation keyword and this causes error. It should look like that:

*Orientation, name=Ori-1, system=cylindrical
0.0, 0.0, 0.0, 0.0, 0.0, 1.0
1, 0.0
*Solid Section, elset=SET-5, material=CromoCobalto

 

[JLZmech]

Oh, i thought that by writing cylindrical Abaqus already use the general cylindrical coordination so It isn't needed to give the coordination yourself.

Thank you i Will give It a try.