Tip:
Highlight text to annotate it
X
This video will show you how to define element properties
using Patran 2010
I'll be using this model in Patran
to show you how to create 1D,
2D, and 3D finite element properties using Patran
so I'll begin by defining the properties for my 1D elements
that are along this meshed curve here on the bottom
so from the properties tab under 1D properties
I want to define beam properties for those elements
so my action, object, and type are: Create, 1D, Beam
I'll go ahead and give this
property set a name
I can then click Input Properties
and I need to select my material that will be applied to these elements
Now I can click on the materials icon and see that I already have an existing material defined
in my database
if I didn't
I would need to go back
and define my material properties first
before I can then apply them
to the element properties
so I've selected my material
the next thing I am going to do is I'm going to define the section
the cross-section that I want to apply
along this 1D beam
so I can choose from a variety of different shapes here
but I can see that there is an I-beam
and that's the section that I want so I'll give it a name
and then define my height and width
and thickness values
to represent
my beam section
in this case I have a height and width of one
and all of my thicknesses are 0.25
once I entered
the appropriate values
I can then click calculate and display
to have Patran draw the section for me
this is the cross-section as it will be applied
to those 1D elements
so I can look at this and make sure that the dimensions are right
and I can see that they are, it's one unit high, one unit wide
with a quarter inch thickness
but also
looking at this the
[1D] elements themselves will be like coming out of the screen
so this section will always be applied
normal to
my elements
but what I still need to define is how
it will be placed rotationally
so I can look at this and see
the way this is defined
the web of my beam
is vertical
so when I apply this
section to my elements
I want to keep an orientation
that will [be correct]
I need to properly align my web
and that'll be our next step
so I can click OK
and now I need to define a bar orientation vector
so as I applied that I cross section
that I defined
along my 1D elements here
I want it to be oriented the same way as these other I beams
again with the web
oriented along the global Y direction
or lying in the X-Y plane
so for my bar orientation
I'm going to enter
this will define that X-Y plane
when used with the
X direction
which the element lies in
so the one orientation vector that I couldn't use
would be along the element
direction
which in this case is along our global X
so the with my orientation in the Y direction
I can go ahead and click OK
now I need to select my application region
so which elements in my model
will this property be applied to?
I'll apply it to all of the elements on that curve
I'll click Add,
OK,
and now I can click Apply and create my 1D beam elements
now if I want to view
these element properties and see that they've actually
been applied the way that I intended
I can go to display
Load/BC/Element Props
and scroll down and select a 3D
beam display
so I click Apply and now I can see
how those element properties are being rendered on my finite elements
so what we've done here is we've used the element properties in applying a constant
cross-section
to make up for the geometry information or the spatial extent
that was missing from the elements themselves.
and I can rotate the model and see that I did in fact
get that
beam orientation correct
if I could use a different orientation vector
like say one unit in the Z
this would be turned ninety degrees on its side
and would obviously provide different behavior.
So that's how you define your 1D element properties
now I want to define the properties for the 2D elements of my model
so for 2D properties
I want to define
my shell
so I'll create a 2D shell
I'll give this property set a name
and again click Input Properties
now here I don't have to worry about the orientation because all of my surfaces
already provide that information; all of these elements
already have a direction
they just need a thickness applied to them
so I need
to tell it what material to apply to these elements and again it will be our aluminum
and then also what thickness to apply
as currently currently these elements have no thickness
so my thickness value will be 0.25
now i can click OK and select my application region
and I'm going to select all of the surfaces
that form this
2D I-beam model
I can Add,
OK,
and Apply
and so now I have created my 2D element properties
that defined
the thickness
and material
for all of these
2D finite elements
so now finally I'm ready to define properties for my 3D finite elements in my model
so under 3D properties I'll select Solid
and this will create a 3D solid
I'll give this property set a name
and input its properties
now the only required property
for solid elements, because
remember they already represent the entire spatial extent of our model,
is what material to apply to them.
So in this case I will again select our aluminum material
click OK
and then select my application region
which in this case will be my entire solid
I Add,
OK,
and Apply and now I've defined my 3D element properties
SO as we've seen,
the more
complex
the spatial extent of the element is
like in the case of the 3D elements,
the less we have to define through our element properties
but here in this one model
we've shown you how to define
your 3D,
2D, and 1D finite element properties
so this should cover
most of the situations that you run into
in your finite element models.