Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Normals of 3D elems using MAT9

hi,
i am not sure how to check the 3D elems normals and how the normals are combined with the right use of the MAT9 material card for anisotropic materials. Can I check if the material is defined in the right way respective the anisotropic way/alignment of the elems in 3D?

Thanks for your time

Find more posts tagged with

English

HyperMesh

Accepted answers

All comments

Rahul_P1

Hi Tobias,

Please refer to the scripts below @ http://www.altairhyperworks.com/Script-Exchange.aspx

if your concern is about the orientation of the angle, you can also check the script below, which allows to change the direction/orientation of HEXA elements.

Thanks and regards
Prakash Pagadala

Rahul_P1

Hi, thanks for your advice! I think Skript #382 'Show and adapt element orientation' is the right way for me.
To proof my line of thought:
I can edit the elems orientation with this tool, so that I can assign MAT9 in the right direction. My material is a nomex honeycomb with a high compressive modulus G33 (Ezz) and two shear moduli in G55(Gzx) and G66(Gyz) direction. Right?

And if I create a 3D hex mesh the Z direction of the elements are the origin 2D element normal?

Rahul_P1

Tobias,

OptiStruct do not need their normals defined for 3D elements because the stacking sequence is physically modeled and the normal is defined based on of the material orientation. You just have to make sure that you have all of your material orientations defined properly and material data within the MAT9 card and you should be fine.

to make sure the material orientation, card edit the PSOLID property and check the CORDM is defined/updated to material coordinate system

also, Have you considered using MAT9ORT for orthotropic solid elements?

Thanks and regards

Prakash Pagadala

Rahul_P1

I thought with these skripts I set the material orientation of the 3D elems. I know there is a material orientation in the composite panel for 2D elems, so how does it work for 3D?

The PSolid sheet looks very blank.

translating my MAT9 into MAT9ORT would be:
G33 --> E3
G55(Gzx) -->G31
G66(Gyz) -->G23
Or am I wrong in this point?

//edit: and works MAT9 /MAT9ORT also for 2D (composite Core)?

Rahul_P1

Hi Tobias,

For shell the MCID is assigned to the element. for solids the MCID has to be assigned to the property. You can use use macro 1064 to create a property for each element with an orientation system as described above.

Just change the cordm options from blank to user, then click on the cordm word in the card, it will then change to a yellow coordinate system selector, now choose the coordinate system.

You should also be able to review the orientations after this

Rahul_P1

Tobias,

the conversion from MAT9 to MAT9ORT or the otherway is different. below picture is from the card of MAT9ORT. the G11 in the picture is the C11 of the stiffness matrix of orthotropic material (assuming C as stiffness and S as the compliance matrix notations).

Thanks and regards

Prakash Pagadala

Rahul_P1

hi,

I have the following data provided and tried to fill out the MAT9 Card. But the calculations are wrong.

With the Datasheet, i filled out the green arrays. G_xy is assumed to be small (2), E_xx and E_yy are chosen so that the different nys are in a realistic range Ny<0.5.

The inversion of this matrix provids me the stiffness and so the MAT9 card. But my calculations do not fit. Is it easier to work this the MAT9ORT card?

Thanks again

Rahul_P1

Tobias,

since you have all engineering material data (E1, E2,G12..) you can directly input them in the MAT9ORT, this will converted to MAT9 while solving.

Rahul_P1

okay nice

would you agree that my material card is correct with the provided material datasheet?

Rahul_P1

Yes, if the following is true:

XX is the 1 direction (MAJOR), YY is the 2 direction, ZZ is the 3 direction and so on..

Thanks and regards

Prakash Pagadala

Rahul_P1

the model does not show the stiffness that there need to be for this material. Unfortunately I have a huge displacement. Regarding this I think that there is a problem with my directions.
lets review:
When I create a 2D mesh and create with elem offset a 3D solid, the 3 direction is the thickness. So in the material card the 3 direction (in my example at the page before) is with 734 MPa a bit higher, than the other two directions with 500. In this example is the global coordinate system like the solid coordinate system. Is it nessassary to define a System by node reference, assign all the nodes and assign this system to the property?

Rahul_P1

yes, the system defines the direction. create a system and assign the same in the property and check if that works.

since there is no system assigned the solver considers the nodal reference system which may not be the same for all the elements.

Thanks and regards

Prakash Pagadala

Rahul_P1

it worked with MAT9ORT, thanks

Altair Forum User

When I try to use the script #1064 I receive an error message. Probably because I don't know what the instruction

'You have to source oribyline.tcl. It opens a tab with the function shown in the video.' [https://connect.alta...w.html?kb=99445]

means. Could someone please explain this to someone who has basically no experience in scripting?