Tip:
Highlight text to annotate it
X
This video will show you how to constrain your model for a finite element analysis
using Patran 2010
Here in Patran I have a plate geometric model
that I want to constrain properly.
Now I haven't created my finite element mesh yet but that's okay because I can apply
my constraint to the geometry and then it'll be transferred
to the finite elements once they're created
so for my model I have two
flat plates here
that I want to constrain
so under loads and boundary conditions I'll select displacement constraint
my action, object, and type are: Create Displacement and Nodal
so I'll give it a name in this case
fixed
one
and I'll input my data
I can constrain translation
so by entering zero here
I'll be fixing the X, Y, and Z translation to be zero
now I could enter a non-zero value here
and that would apply an enforced displacement but that's really more of a load
I can also constrain all of the rotations
to be zero as well
for all of the points that I select
with this application region
so I click select application region
and here I can pick geometric entities to apply this constraint to
now I want to be careful not to select
two large of an application region. I could select this entire plate if I want
but that would make my analysis rather trivial because it would be fully fixed
nothing could move in any direction
so instead I want to just apply this at one point
so this bottom left of the my left plate
is what I'll use as my application region
I'll click Add,
OK, and now Apply and the blue markers indicate that I've constrained
all six degrees of freedom
for that point
so X Y and Z translation
and rotation about the X Y and Z axis
now that constraint alone is enough to fully constrain this plate
because it can't move
in any rigid body way
with that point
constrained that way
now the right plate is still totally free and we'll get back to that later
but because it's important to consider rotations in your model
I'm going to modify
that displacement and remove the rotational constraint there
so we're going to modify our Fixed [constraint]
and modify it's data
and to remove the rotational constraint, I'll just delete these zeroes
so that the rotations are again left blank
So I'll click OK and Apply
and now I can see that I am only constraining the 1, 2, and 3 or X, Y, and Z
direction translation
for that point
now this is not enough to fully constrain the left plate
because it can rotate about either axis
so I'll need to create additional
boundary conditions which I can do
I'll Create
Displacement Nodal again
and in this case
I'll create fixed_2
and input its data
Now I could constrain all three translations for another point elsewere on the plate
and that would help
but I have to be aware that I don't over constrain this plate
and unrealistically restrict its movement
so in this case I only want to constrain
the X and Z translations
of another point
so in order to do that what I'll do is I'll leave the value
for Y translation blank
so I'm entering [0, ,0]
so that I'm constraining the X and Z while leaving the Y blank
so I'll click OK
select application region, and in this case I want to apply this to this top point here
I'll Add, OK,
and Apply
and now my markers indicate that I've constrained the one and three or X and Z translation
the reason I didn't want to constrain the Y translation there
is that wouldn't allow this plate
to expand or contract
with load along this Y direction
and that might
be an unrealistic constraint
so the model would in effect be over constrained
so it's important to think about
your realistic loading situation
as you apply your constraints your model
now I still need to apply one more constraint to fully fix this plate
because currently it could retain about the Y axis
along this line
so I'll go ahead and create one more fixed constraint
in this case
I'll only constrain
translation is the Z direction
so
for my value
I'll leave two
both the X and the Y blank
and fix the Z to be zero
I'll click OK
select my application region
and I'll pick this point at the right edge of that plate
Add, OK,
and Apply.
So now my left plate
is fully constrained
With this combination
of translation constraints
I've removed all possible rigid body motion for this plate
and I've also been aware not to over constrain the plate
by restricting too many degrees of freedom
so finally another factor that I need to consider is this right plate over here
now if I need it to be properly constrained
I could either create its own set of constraints that apply to this plate if I want it to be a separate
object
or I need to tie it
properly
to this plate on the left
and I can
tie those two plates together as part of the meshing process
so I'll just quickly
create a mesh
on these
surfaces
I can see that now they've been meshed
but they're still two independent plates and if I were to run this model
I would get an error
Nastran wouldn't complete and I'd have an excessive pivot ratios error
that you often see when a model is under constrained
and that's because all of the nodes and elements on this right plate are free to move wherever
they want.
There's no constraint being applied there
so if I want to tie these two plates together
I do that
by Equivalencing the model
I can first verify
that they are two separate plates, I can see that there's a free edge between them
and I can Equivalence
the model to remove that and connect
the unconstrained plate to the constrained plate
again I won't
want to exclude any nodes from this so I'll leave this field blank
and all of the duplicate nodes will be removed
and that's what I can see here. There were six coincident nodes
that were shared
between [elements]
on the edge between these two plates
so now with those nodes being deleted and the elements tied together at common nodes
this model is now fully constrained
by the finite element mesh.
So again it's important to make sure
that you
have properly constrained your model and removed the appropriate
rigid body motion from your model
and you can do that by directly creating your displacement constraints
but even so you need to be aware of where and how and which degrees of freedom you are constraining at
different points in your model
and finally
you need to make sure that your model
it's continuous
so that your
constraints are applied throughout [the model]