- [Narrator] Here I want to talk about
making our first solids.
We're going to be using the Pad operator.
You'll notice that with Pad,
you will have the universe,
which is called pocket.
Pad creates and adds material,
pocket removes material.
You also have, shaft and groove,
which we'll be discussing in the next lecture,
and whole, and various other options
with ribs and slots and such.
So for every positive polarity feature,
you have a negative polarity feature.
Now, you see we have our sketch.
I'm going to go ahead and select our Pad icon,
select my sketch,
and automatically based off of this sketch,
you can see here my sketch profile,
my length of 20, it determines the vector direction.
Remember when you pick a sketch,
you're picking the planer face or an actual plane.
The normal off of the plane becomes the vector
for the pad direction.
You can use by selecting more
a different direction, but by default
it is normal to profile.
So if you have a tooling direction that you need to use,
then you can come and specify
whatever that tooling direction is.
Now here, I have my first limit.
It is up to a dimension, I can enter in the value
that I need, and preview.
I also have the capability of going
in the opposite direction for the second limit.
So for this I'll just type in 15,
and preview.
As you can see, I'm going 15 in the opposite direction,
and 15 in my limit one direction.
If I enter in any negative value,
and preview that, you'll notice that it goes
in the opposite direction.
So this is a negative 15.
I also have the ability to pick
where it says limit one, limit two, and drag
the size or location that I need.
Next, I have what is called myriad extent.
With myriad extent you'll notice that the length
on the second limit disappears.
And that's because it's taking the first limit
and saying, go that far.
So I can't change the second limit
any longer.
Just the first, and you'll see that it is now symmetrical.
Once I have the size that I want,
I simply select okay, creates my pad.
Now note, in the tree, the sketch is nested
underneath the pad.
This is indicating a parent/child relationship.
The sketch is the parent, the pad is the child.
I'm going to go ahead and create another sketch.
So I plane, and this time I'm going to draw
an open profile.
I'm going to exit out.
With this, you'll notice now
pocket is active, I can select pocket,
and with this, I have the ability to specify,
just like the pad, the direction, the length,
the size, preview that, and you'll notice
that I didn't have to create a closed off profile.
I wanted to talk about an open profile
here right away because some people get confused.
Typically speaking when you're making a solid,
you need a closed profile, but because as a pocket,
the system knows it's going to be removing material,
remember the pocket is the negative,
the pad is the positive,
it also knows that it's going to be removing material
from a side.
So in this case, if I remove material from the
incorrect side I can simply reverse side,
preview, and it's removing material
from the other side.
I also have the same capabilities
with my normal profile direction,
I can do myriad extent.
If this does not extend out beyond the complete part,
preview, you'll notice that it will remove
material based off of the depth you specified.
So, the pad and pocket are very, very powerful operators.
One thing to take serious heed of at this point
is that the first sketch I used is a closed profile.
The second sketch I used is an open profile.
One I made the pad with, one I made the pocket with.
Now I can make a pad with an open profile,
and this is why I wanted to be very specific
about using an open profile at this point.
Because when I go in and make my pad,
with an open profile, let me go ahead
and do a couple of undos here.
Go back to this, I'm going to double click on it,
I'm just going to simply delete these two curves.
And exit out.
Now I have an open profile.
When I go and I make my pad,
you're going to get an error message.
Now, just as a warning, sometimes these error messages
are a little cryptic, and the reason being is
this is a Dassault product.
It's originally written in French
and it's translated to English,
so some of the messages can be a little confusing at first.
Once you understand what the system's
asking for you, you'll fly through it.
It's not that big of a deal.
But in this case, it's saying you must use
thick option in order to use an open profile.
Whenever current features the first solid feature of a body,
do you want to use the selected sketch anyway?
So it's a little cryptic, so if you do want to use a sketch
just simply select yes.
And remember, as an open profile,
you're trying to make a solid, you cannot make a solid
off of a curve unless you have thick turned on.
So that message is letting you know,
yeah you can use this open profile,
but you have to turn on that thick function.
And what that does is it,
and this is again where it gets a little cryptic,
a little odd, it activates the thin pad perimeters,
so you're turning on thick, to get to the thin pad.
So, again, it's the phrasing of it.
It's, again, initially written in French,
translated to English, so it loses a little bit.
Again, once you've used this several times,
you go through it, you don't have anything to worry about.
So here, you have a direction for your thickness
in one side, in a direction,
and your thickness in the other side.
As you can see I'm taking that pad,
making a solid out of an open profile.
Just by adding thickness to it
in either direction.
If you want, maybe you're making a wall,
that is some sort of a rib, plastic part,
whatever that may be, and you have a constant thickness
to either side of the sketch,
you can turn on neutral fiber.
You'll notice that thickness too disappears,
so that 18 millimeters now as you see
is balanced across that sketch.
Nine in one direction, nine in the other direction.
Select okay, and there is my solid.
So don't be afraid of open profiles.
You can use them, again, the messages are a little cryptic,
but it's just basically asking you to make sure that
you're turning on your thick function.
Also, as a note, I'm going to go back
into my sketch one,
and I'm just going to close off this profile
and I'm going to leave the thick function turned on,
just exit out, and you'll notice that it updates fine.
No problems.
So yes, you can use the thick option with open
and closed profiles.
You just end up getting a solid wall
or ring, as we have in this case.
Now if I go back in the pad,
by double clicking on it,
and turn that off, you'll notice in this case it works.
Because we have a closed off profile.