shell element material orientation aligned to surface

[Anonymous]

Hello, 

my part is meshed with shell elements and the material is defined with plys. Now I want to define the material orientation. The problem is that the orientation depends on the global coordinate system. My part has several surfaces and the orientation should be parallel to each surface. So the material orientation depends on the surface on which it is. The arrows on the right should lie on the surface like the left arrows. Is there a way to do this? 

Thanks. 

 

[John_Holtz]

Hi @Anonymous 

I cannot visualize which direction the arrows are pointing on the right side. 

Regardless of that, you select the faces that you want to orient when you use right-mouse-click on "Analysis > New > Material Orientation". So you create one Material Orientation for the face on the left and a different Material Orientation for the face on the right. In other words, the orientation of the lamina are measured from the Material Orientation (not the global coordinate system), and the Material Orientation can be defined using several different methods.

If you are still having a problem, be sure to let us know how you displayed the arrows that are shown in your image. Maybe you displayed them using a different method than what I know!

[Anonymous]

Thanks for the answer. 

I used already the function Material Orientation and tried all different methods. But the program always orient the plys like the red lines. So the E1 and E2 orientation is the same on all surfaces. The problem is still there when I make a seperate orientation for every surface.

I want a orientation like the green lines. So that there is a special coordinate system for each surface. 

In Abaqus you can align the ply orientation like this. 

https://abaqus-docs.mit.edu/2017/English/SIMACAECAERefMap/simacae-c-advlayupsorientations.htm

Hopefully now it is better explained. 

 

[John_Holtz]

Hi @Anonymous 

I suggest reading the Inventor Nastran documentation 🙂 New Material Orientation. I do not know what your model looks like because I do not have the full context, but I assume you want to do something like this:

 You just need to choose the "Type" of orientation that makes it easiest to define the orientation. I used "Curve Tangent" and selected the outside edge to define the orientation for each of the 5 faces.

[John_Holtz]

I spoke with @Anonymous  through a support case that she created. The confusion occurs because the arrows are a flat, 2-dimensional arrow instead of a 3D shape (like the arrows for a force load are 3D arrow heads). On some faces, the arrow head is flat (in the same plane as the element), and on other faces the arrow head is perpendicular to the element. It is hard to see in the software itself. (You can just make out the difference in the blue arrows on the left side of the pentagon in my previous reply.) This sketch here may help to explain what Inventor Nastran can show for the material orientation.

Figure 1: Sketch of the material orientation arrows. The arrow in A is drawn perpendicular to the face.

In reality, the arrow is just a symbol. The plane of the arrow head has no significance. If the software could show the orientation of material axis 2, it would look the like the following sketch. Axis 2 is always in the plane of the element and perpendicular to axis 1.

Figure 2: Axes 1 and 2 are always in the plane of the element.

Just to complete the topic, axis 3 is normal to the element. For composites, the bottom layer is on the negative size of axis 3, and the top layer is on the positive side of axis 3. Axis 3 can be displayed by right-clicking on "Elements > Normal Display > Vector". Axis 1, 2, and 3 follow the right hand rule.

Let me know if there are any questions.