## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Local coordinate system for each element of mesh and ICTE dependence.

• Łukasz Ruba
Subscriber

Hi,

I have a metarial with ICTE_x=25e-4, ICTE_y=-5e-4, ICTE_z=25e-4. Is it possible to create a local coordinate system for each mesh element, where, for example, the X vector will change discretely from -1 to 1 (like on image belowe)? I'm thinking of creating a CSV file in Matlab with three columns [x,y,z] and loading it into external data. And if it is possible, does that mean that in each element of the mesh ICTE will act on it through this local coordinate system?

Lucas

• peteroznewman
Subscriber

Create a solid beam, split it up with Planes and use the Share button to connect the mesh between the bodies.

Create five Coordinate Systems rotated to the correct and angle name them 1, 2, 3, 4, 5. You could click the face to define the origin instead of typing global coordinates, though the origin is not important, only the directions. It is more for visual checking that the correct coordinate system is assigned to the correct body.

Create five Element Orientation items and assign the correct body and coordinate system to each one.

Insert an Element Triad into the Solution to see that the coordinate system was used. I meshed this with 1 element per body, but you can have more elements in each body if you want.

DON’T TRY THIS WITH SHELL ELEMENTS!

I tried this with surfaces instead of solids.

A warning is issued:

Element orientation only works In-Plane for shell elements. As you can see, the Element Orientation was ignored.

• Łukasz Ruba
Subscriber

Thank you very much. I have tried that but I came across a few problems. I declare all local coordinate systems with the same orientatnion as in my other project without partition. Which means that all coordinate systems are without rotation - the same like global coordinate system. I did it to compare reasults between them.

Firstly, using this method I can't use linear mesh:

It only works when I use program controlled mesh generator and it looks like that:

For me it's quite important to have linear mesh because I'm generating the load in Matlab by coordinates on a strip. I set 'Protected' to 'Yes' but it doesn't work too. Is there something which can I do to use linear elements order?

Temperature results are similar in each case:

(Model without partition)

(Model with partition)

But I have a problem with deformation results:

(Model without partition)

(Model with partition)

Why both don't work approximately the same? Is it because of different meshes?

Lucas

• peteroznewman
Subscriber

Lucas,

Don't use Bonded Contact to connect the solids. Delete all the contacts, open the geometry in SpaceClaim and on the Workbench tab, click the Share button. Then you will not need any contacts.

In Mechanical, you can use Linear elements to mesh each of those solids. Use a Sweep mesh method, select the top face as the Source and in the Sweep number of divisions, type 4. You want at least 4 linear elements through the thickness. This should solve cleanly.

Another change you could make is to use a Coupled Analysis, so that the structural and thermal solutions are solved simultaneously in the one Transient analysis.

• Łukasz Ruba
Subscriber

Your advice was very helpful and thank you! Now I would like to ask if there is an option to set the orientation of an element using a mesh-dependent function (x,y,z)? Using the above method, I get a simplified orientation distribution model:

However, I would like to define the direction of the x-axis consistent with the direction of the normal vector for each mesh element:

Is it possible?