- [Instructor] When working in large assemblies,
it's always a good idea to try to reduce
the file size of the assembly as much as you can,
by swapping out components that you're finished
designing and working on with dumb solid bodies.
Let me show you what I'm talking about.
Your exercise files will be in a similar folder to this.
I'm looking at the Wheel Loader.
So you can see here, this is a 3200 kilobyte file.
I'm going to go ahead and open it.
And I'm going to open it, and I'm going to open it Resolved.
All right, not too bad to handle.
Let's take a look at the Assembly Visualization.
This will give us an idea
about the performance that we have.
So if we go over to Performance Analysis,
we can see that this component
is causing the most rebuild time.
So there's a lot of features in this,
pretty extensive.
If we switch back to our assembly,
we can see that it takes 4.15 seconds to rebuild.
Now we want to limit that rebuild time as much as we can,
and also limit the open time as much as we can.
So let's try to swap this out for a dumb solid,
such as a parasolid, instead.
So, how am I going to do this?
Well, first I'm going to save my part.
Turn off Assembly Visualization.
And I'm going to open up the part
that's giving me the most grief here.
So we want to maintain all of the geometry inside this part,
but we don't necessarily need
all the functionality of this feature tree.
So I'm going to go ahead and save this as a copy,
and change it to a parasolid part.
I choose a Parasolid xt version for my dumb solid,
because this is going to give me the best chance
of having all of my geometry maintained.
If you use a stp file or an igs file,
for example, this software format is older
and not as maintained as thoroughly as the parasolid,
and it can have errors occur sometimes.
You might lose a face, you might not have
two faces stitched together properly.
So a parasolid has the most data.
But if you want to have the smallest file,
you might consider using an igs or stp file,
if it's a low-detail part.
But this part has a lot of detail,
so I'm going to go with the parasolid file.
I'm going to save this is Rear Body Parasolid.
You can see it saves pretty quick.
I'm going to close this file.
And now I'm going to open up that parasolid.
You can see that it's populated right here.
It's about 2,200 kilobytes.
The original file was 3,700 kilobytes.
Looks like we've already got a reduction.
I am going to run Import Diagnostic on this part.
We see here the errors that I was talking about
have come up.
I've got a couple faces
that aren't stitching together quite right.
So let's go ahead and use the repair tool.
I'm going to attempt to heal all.
All right, and it was able to fix those faces
and give me solid bodies.
Now I'm being asked by FeatureWorks,
because I used SolidWorks Premium,
if I want to proceed with feature recognition.
Here I'm going to say No.
We went through this whole process
so we could get rid of all our features,
so we don't want to go and put them right back
into the feature tree.
Now, when you import a parasolid into SolidWorks,
if it was created in SolidWorks,
using the feature recognition feature,
might be able to restore a majority of the feature tree.
So sometimes it is good to use it,
but here we're trying to increase our performance.
So we're going to say no.
All right, part looks good.
Got all our lines.
Got all our bodies.
I'm going to go ahead and save this, as a SolidWorks part now.
Now if we go to that folder, we can see now
that our part is down to 1,456 kilobytes,
so even smaller.
We're going to switch back to our assembly,
and now switch that component out.
So I'm going to right click and go to Replace Components.
If, when you right click on a component in your assembly,
you don't see this option, what you want to do
is go down to the bottom and hit Customize Menu.
And here you can turn on and off the different options,
so make sure that that's clicked on.
So I'm going to right click, go to Replace Components.
Because I have this open in another window,
it populates this window automatically.
If I had multiple parts open, or assemblies,
they would all be dropped in here.
I'm going to select that component, hit OK.
You can see it dropped it and replaced it, no problem.
I'm going to save this.
And now go to my Assembly Visualization
to see how we did.
Go into Performance Analysis.
We can now see that that same part,
it can be a little hard to see,
now has a 0.1 second rebuild time.
And because it hasn't opened yet,
it doesn't have the open time here,
but I can assure you, that will be less, as well.
So we've increased the performance of this assembly
just by swapping out one of the parts
with a parasolid.
Now you can do that with the sub-assemblies,
once they're complete.
And you can go back and forth.
Because this was created originally by the same body,
if I want to replace this component again
to do work on it,
I can simply find the Rear Body,
select it to replace, and drop it back in the assembly.
It'll have all the same line and edge entity numbers,
because they were created
from the same original SolidWorks file.
So you can swap these in and out, as required,
if you need to go back and some work on this part.
So that's a good way to speed up your assembly performance.
Always consider using dumb solids,
because they drop all the functionality of SolidWorks out,
and just give you that base geometry that you need.
Always remember when you're done, to Save.