- [Instructor] This video describes
how to convert SOLIDWORKS Weldments into FEA truss elements
together with the appropriate methods
for loads and band conditions.
We're going to recreate the F-game model
that we saw in the previous truss example.
That one used the alternative starting point
to solid geometry instead of Weldments.
So go to file open, and we choose rectangle.
If you have a SOLIDWORKS version 2018 or later,
than you can get this file directly
from the exercise folder.
Now this part contains a sketch,
which we'll use to create a Weldment profile.
If you're working with SOLIDWORKS version prior to 2018,
or don't have this SOLIDWORKS file available,
then you'll need to create this sketch
in a part from scratch using the dimensions shown here.
Note that origin of this sketch is at the centroid
of the rectangular section.
This forms the pierce point, or datum,
of the Weldment profile.
We're going to save the file as,
and then we're going to change the type
to a library feature part.
Now there's a specific location we want to save this into,
and that is the delivery folder
of your SOLIDWORKS installation.
I'm going to go to my delivery folder,
but yours might be slightly different.
So the folder we're going to
is wherever your SOLIDWORKS is installed.
And then the path is SOLIDWORKS Corp, SOLIDWORKS,
lang, English, Weldment profiles.
Now there are two folders underneath this,
ansi inch and iso, which are two profile standards.
We're going to select the folder ansi inch,
and we create a new folder called solid selection.
Now I've already done this, but you need to create that.
You may need to change your privileges,
so you can actually create a new file within this folder.
And you open up solid section once you create it,
and then you save this sketch,
which becomes a Weldment profile, within this hierarchy.
So I won't save it here, I'll just cancel out.
You can see I've saved that earlier.
Now that we've created the Weldment profile,
we can start to construct the truss assembly again.
So we're finished with the profile,
so we can close this.
We want to open up a new file as a part,
and we want to create a sketch on the front plane.
We choose a front plane.
We basically want to create three points,
which are going to be the corner points of the truss.
So I create a point, just drag the three points
in position like this.
We can go back and edit their positions.
Zero zero, we fix it there.
The next one will be the top point,
and this will be at 130 in x and 100 in y.
Again, it's fixed position.
The final point we want to modify
to be the right-hand base of the truss arrangement,
so it goes at 200 in x and 0 in y.
And we fix that position.
So our three points created, we just create a line
between each one of those.
So that's the first truss, that's the second truss.
Now we can save the sketch.
Now we can click on insert, Weldments,
and we're going to choose structural member.
Now the hierarchy runs standard, type, and size.
And we used ansi inch was the standard
that we saved our new type under.
The type was solid section, and size,
a little bit misleading name here,
but generally, the description of the section is rectangle
in this particular case.
Now we pick the two lines to form the two truss sections.
So the first line and the second line,
we check okay, and our new sections have been created.
In the feature manager design tree,
we can see solid section one and solid section two.
They're both formed from the Weldment called rectangle.
Now we're ready to open a new design study,
so go to simulation, new study.
Let's call it truss weldment,
and this is as opposed to the geometric-based approach
we used in the last video.
We want to carry out a static analysis, just check okay.
The study tree view now contains a cut list.
We expand this.
And within the cut list, there are two items.
We expand further.
The Solidbody one and the Solidbody two.
You look at the icons, you can see they're beam icons
indicating that they're automatically been recognized
as beam or truss-like members.
I right-mouse click in here.
I can edit the definition,
and it's by default gone in as a beam.
When it was a solid body, then we had to say
convert to beam.
Here, it's automatically a beam formed.
Now we're going to change this to truss.
Click okay.
And we do the same with this one.
Edit the definition, and set that up as a truss.
Now the icon has changed, so that truss-type icon
rather than the beam icon.
But let's find material to our bodies.
I'm going to use the material we set up
in the previous video under example materials,
truss benchmark, truss.
And the key thing is if you're repeating this,
we want to have Young's modulus equal
to one-eight to the sixth.
Click apply and click close.
Now we'll pause there, and we will set up loads
in band conditions and run the analysis
and check results in the next video.