Tip:
Highlight text to annotate it
X
This video
will show you how to create loads
for your finite element models
in Patran 2010
Now that I have a model in Patran
with finite elements defined
I'm ready to
define some loads to be applied to these three blocks that I have shown here
notice that
I've already applied a boundary condition
to constrain the bottom face of each of these blocks
from translation in all three directions
so looking at loads
some of the options I have
are a force
pressure
temperature, inertial load, distributed load,
or a total loading
and I'll show the differences between some of these
here as we create loads on these blocks
but no matter what type loading you decide to use in your model the process in Patran
is really
pretty similar
I'll start by creating a force
which is commonly a point load
applied to an individual node
so our action, object, and type are Create Force Nodal
and i'll begin by giving a name for this particular force
which I'll call force
then I click input data
to enter the vector information to define the direction and magnitude of this force
so
for our force value
I want to apply 100 pounds in the negative Y direction
So I'll enter [0, -100, 0]
and leave the remaining moment
fields
and phase fields blank
so I'll click OK
and now I need to select an application region
for this load
So what I'm going to do
is select
the entire top face
of this first block
so I'll change my filter here to
surface or face
and I can select
that top face, click Add, OK,
and Apply
now remember I mentioned that a force
applies
a point load
to the selected nodes
so in this case every node on this top face is going to see a load of a hundred pounds
Now some of you might be realizing this might not be what you
what for your model
but will demonstrate that in a little bit
so the process is similar to go on and create say a pressure load
this case I'll be creating an element uniform
pressure load which means the pressure
across each element will be the same
you can very well have an element variable where the pressure varies across an element
so again I'll enter a name
in this case creatively I'll call it pressure
our target element type is 3D
but you could apply a pressure to a 2D surface if you had one in your model
I'll input data and
in this case we just give it a magnitude for the pressure because it's always considered to be
normal to the surface you select
I'll select 100 in this case pounds
per square inch
So I'll click OK,
select my application region
and in this case off what the top face of the middle block
then click Add, OK,
and Apply
The red arrows indicate that I've applied a pressure to this surface
Finally I want to a look at another option
for creating a total load
on a surface
and the way this works is the total load value that you enter
is distributed across all of
the the entities that you select to add up to a total of the value you defined
so again I need to give it a name
and select my target element type,
input my data
(this is a vector load)
and I'll select my application region as the top face
of this last solid
so I'll click Add,
OK,
and Apply
and the blue arrows indicate that a total of a hundred pounds
it's being applied all across that whole surface
So next I'll analyze
this simple model and we'll view the results
Now that I have my results file attached I can create a quick plot
to show how
these different loads cause our model to behave
I'll plot my stresses and displacements
and we can quickly see that the pressure leading
was significantly higher than either of the other two
now this is because
we have a ten by ten block
so there is
hundred square units of area there
each of which
got a hundred pounds of pressure applied to it
resulting in a
significant amount of force
being applied to this part of the model
now over here with our Force loading
we had each of these nodes along the top
each receiving 100 pounds
resulting in a higher total load
being applied to it and
some
significant visible deformation there
when compared to the total load here
where 100 pounds was distributed out over the entire top face
resulting in significantly less force being applied than either of the other two options
So really the point here that you want to get is to make sure
that the load and boundary condition
that you choose
really reflect
the actual loading the you're going to have in your model
I just wanted to touch on a couple other
types of loads that you can create in Patran
%um
an inertial load
by default applies to all of the elements in the model with mass properties
so you don't need to select an application region
You also have a distributed load which is like a load per unit length
and then you can group your loads together in load cases
so say you have a loading situation where loads A, B, and C are being applied and then a different situation
where you want just B and C applied
you can group those and then run
your seperate load cases for separate analyses
so the basic process for creating any of these
loads
is
pretty much the same, you'll enter a name
define your data
and usually if necessary
define where
the load will be applied by selecting your application region
Finally the last thing I want to show you is that you can modify
your existing loads in your model
by selecting Modify from your LBC actions
and then choosing the type that you want to modify
and any of the existing
loads that you've defined in your model
you can select here
and then modify their data or their application region as necessary
so hopefully this just gives you a brief introduction showing you how to create loads
this will let you create the types of love that you're looking for in your finite element model