## LS Dyna

Topics relate to LS-DYNA, Autodyn, Explicit STR and more

#### Material Coordinate System

TAGGED:

• Mehdi Saloo
Subscriber

Hello,

I have modeled a timber beam in LS-DYNA. In this regard, I used *MAT_WOOD which is a transversely isotropic material. I intend to define a proper material coordinate system so that the model can realistically behave. I have read LS-DYNA Manual regarding *MAT_WOOD, ELEMENT_SOLID_ORTHO, and other relevant sections. I will describe the steps I went through to define the proper material coordinate system for the model.

I would appreciate it if you could give me some advice.

Regards,

Mehdi

Step 0: FEM Model

Wood is an orthotropic material because it possesses different properties in three directions―longitudinal, tangential, and radial. A common assumption is that wood is transversely isotropic which means the properties in the tangential and radial directions are modeled the same (*MAT_WOOD). The parallel direction refers to the longitudinal direction (L) and the perpendicular direction refers to the radial or tangential direction (T).

For my FE Model, longitudinal direction (L) is along the global Z axis and transverse directions (T) are along the global X and Y axes. Therefore, longitudinal stiffness and strength properties (EL, XT, XC, …) should be assigned to the global Z axis of the specimen and perpendicular stiffness and strength properties (ET, YT, YC, …) should be assigned to the global X and Y axes of the specimen (see the picture 1).

Picture 1: The timber beam and global coordinate system (x, y, and Z)

Step 1: Material Directions for the Wood Material Model (AOPT=2.0)

I used the AOPT material axes option (AOPT = 2) and defined vectors a and d. The vector a is the parallel-to-the-grain direction (L) and d is one of the perpendicular-to-the-grain directions (T). Then, a x d = c and c x a = b, where a, b, and c are the principal material axes. Please see the following pictures. Please note that we have solid elements so far (see picture 5).

Picture 2: AOPT material axes option (AOPT = 2)

Picture 3: Display the material coordinate system for solid elements (Mat Dir: shows the material direction orthotropy defined by the AOPT)

Picture 4: Display the local element coordinate system

Picture 5: Solid elements for timber beam

Step 2: Setting the direction of orthotropy axis 1 of the material

On the following page of your website, it is mentioned that “In Element Tools > Element Editing, the Direction option sets the direction of orthotropy axis 1 of the material.”

As you can see in picture 6, it seems that this direction is wrong and should be along the global Z axis. Therefore, I changed the direction and set it along the global Z axis (Picture 7). After that, the elements for the beam changed to ELEMENT_SOLID_ORTHO as you can see in picture 8. It is also noteworthy to mention that the element direction does not change according to picture 9.

Picture 6: The direction of orthotropy axis 1 of the material

Picture 7: Setting the direction of orthotropy axis 1 of the material along Z axis

Picture 8: Solid_Ortho elements for timber beam

Picture 9: Display the local element coordinate system

• Reno Genest
Ansys Employee

Hello Mehdi,

What is important are the material directions "a", "b", and "c" and not the element direction. In your case, the material direction is independant of the element direction because of the AOPT option you selected. Here is an example:

In the image above, the material direction shows the "a" direction as defined  by the AOPT option. Note that you can set AOPT= to a negative number and the number represent a local coordinate system ID. The material directions a, b, and c will be aligned with the local coordinate system axis x, y, z.

The element direction is the direction from node 1 to node 2 as defined on the *ELEMENT_SOLID card. For the solid element 88 in the image above, node 1 is node # 128 and node 2 is node # 137 and so the element direction is from node 128 to node 137:

But, the element direction does not matter here; what is important are the material directions "a", "b", and "c".

For a regular  orthotropic material model, for example *MAT_002, the material directions for Young's moduli and other constants are clearly labeled:

So, the Young's modulu Ea  is in the material "a" direction for all element.

In the case of *MAT_WOOD, the parallel direction is the same as the material direction "a" and the perpendicular direction is material directions "b", and "c".

https://ftp.lstc.com/anonymous/outgoing/support/PRESENTATIONS/lsprepostcomposite.pdf

So, in your case, if the material direction "a" is aligned with the global Z axis, then the parallel direction in *MAT_WOOD correspond to the material direction "a" and global Z axis.

I hope this helps.

Reno.

• Mehdi Saloo
Subscriber

Hello Reno,

Thanks ever so much for your help, I really appreciate it.

According to the clear explanations you provided, I am sure that I defined a proper material coordinate system for my model via the AOPT=2 option. (Step 1: Material Directions for the Wood Material Model (AOPT=2.0)

The only thing I am still not sure about is Step 2 I did (Step 2: Setting the direction of orthotropy axis 1 of the material). According to your explanations, it seems that I do not need to do this step, however, I understood that this step is also related to the material coordinate system. Please see the following pictures.

I would appreciate it if you could read Step 2 as I explained in my previous post and give me some advice. As I mentioned before I understand that in Element Tools > Element Editing, the Direction option sets the direction of orthotropy axis 1 of the material. So, Vector-A is the direction of orthotropy axis 1 of the material. I wonder whether this direction (Vector-A) is the same as the material direction "a" for my model. If the answer is yes, as you can see in picture 6, it seems that this direction is wrong by default for my model and should be along the global Z axis (the material direction "a"). Therefore, I changed the direction and set it along the global Z axis (Picture 7). After that, the elements for the beam changed to ELEMENT_SOLID_ORTHO as you can see in picture 8. As you can see in picture 8, there are vectors A and D. I wonder if these vectors are the same as vectors A and D for the AOPT=2 option.

Regards,

Mehdi

• Reno Genest
Ansys Employee

Hello Mehdi,

The element direction is not the same as the material direction "a". All you need to do is make sure the material directions "a", "b", and "c" are correct for your material. Don't worry about the element direction; it does not matter.

By default, the element direction is from node 1 to node 2 of that element as defined on the *ELEMENT_SOLID card. So, the element direction has to do with the node numbering of the element. You can align the element direction to be in the same direction as material direction "a" using LSPP, but this step is not necessary.

The material models look at the material coordinate system (a, b, c) and not the element coordinate system.

Are the material axis a, b, and c in the correct orientation in your model? If so, then that's all you need. Your job is done as far as material direction goes.

Reno.

• Mehdi Saloo
Subscriber

Hello Reno,

It’s clear now. Thank you so much for your help, I really appreciate it.

Regards,

Mehdi

• Reno Genest
Ansys Employee

Hello Mehdi,

Sounds good.

Have a good  day!

Reno.