SolidWorks Feature Based
0 (0 Likes / 0 Dislikes)
Today we're gonna talk about a few topics in feature-based modeling.
So I'm gonna start by creating a new part
and I am going to put a sketch on the front plane.
And I'm going to create a part that is cylindrical in nature
but has a complicated geometry
and this is easier for me to do
using revolution than extrusion.
So the first thing I'm going to do
is create a centerline that goes along the axis
of the part that I'm trying to create.
And I'm just going to put that along the x-axis.
I'll finish my centerline.
Then I'm going to use regular lines
to sketch out
the profile that I want to revolve.
Now normally at this point I would apply all of my dimensions
but I just wanted to show you a couple of dimensions because there's a trick
to dimensioning when you're going to be revolving.
So I'm going to open Smart Dimension
and then I'm going to dimension between the line on my
and the axis.
Now if I stay between the part and the axis
then I get the radial dimension.
If I jump down below the centerline
then I'm actually dimensioning the diameter
that will exist once I've revolved the part.
So I'll place another diameter here.
And then the other dimensions
that I'm going to wanna make will just be between the lines like before.
So I'm not going to bother modifying these dimensions I would modify them to be
the values that I want.
I'll finish my sketch and now I want to revolve
my profile. So I will go to 'Features',
'Revolved Boss Base', and
and this time it automatically selected the profile
for me. I may need to
manually select the profile and the axis.
This blank is where I select the axis
and then I will also select the profile.
So this looks like about what I want so I am going to click
my check mark to say okay. And now I can see what I revolved.
Now I want to create a hole patter on this face
and before we've created holes by drawing a circle
and using an extruded cut. This time we're going to use
the hole wizard.
So the hole wizard allows me to choose a wide variety of holes.
I can choose what standard I'm using,
whether the hole is threaded or not,
and the size of the hole. I'm going to use a straight hole
and I want it to be a quarter of an inch,
and I'm going to make it a through hole.
Now to choose my position
I'm going to click on the 'Position' tab and I'm going to click on the face
where I want to make the hole.
and then it's going to ask me to position it on the face
I'm going to place the around there.
Now it puts me in the Sketch panel
so that I can apply relations
or dimensions to put the hole where I want it.
So I'm going to add a relation
after looking at my face
between this point and this point
that makes them vertical to one another.
Then I'm going to dimension this distance
and I'm going to make it a little bit bigger
so maybe I'll make it 1.75
and that places my hole there.
Once I'm finished dimensioning
I can click 'Okay' for hole positioning
and it will create my hole.
So if I go back into isometric
I can see my hole.
Now I don't want just one hole, I want a pattern of holes.
So now I'm going to use 'Circular Pattern'
and I have to choose the feature I want to pattern
and then I have to choose
the circumference of something
that indicates the
circle I want to follow when I'm creating my circular pattern.
So I'm going to choose this circumference right here
and now you can see it creates a pattern
of holes. This has six, I could move it up
to seven or eight, I'm
going to leave it at eight,and I'm going to click 'Okay'.
Now suppose I wanted this to
a long pipe with flanges on either end.
One way that I could do that
is to use the mirror function.
So I am going to go 'Features',
'Mirror',
and I am going to mirror this part
around this plane
and the 'Features to Mirror': it already chose this circular pattern
for me but I also want to choose my first revolution.
So I choose that
and then I'm going to click 'Okay'
and now I have a mirrored part.
So this is my part
Now I want to take this part and put it
and put it in a drawing. So I will go to make a drawing
from part assembly, it's going to make me save my part,
again I'm going to have to browse
for the drawing template
and I will hit 'Okay', and now I'm in the OSU Title Block.
Now when I go to place my view.
This time I'm going to set down this left view
as my front view. And the reason that I'm going to do that is
to create a section view. So I'll place my left view down
and then I'm going to add
an isometric view
and that is it for my projected views.
And I don't like how big these are
I think they need to be a little bigger on my page so I am going to use
a custom scale, let's try 1:2
that's better.
Now I want to create a section view
based on this view so I will go to
'View Layout', 'Section View'
now I want to draw
my section line down the middle.
So I'm going to hover over one of the parts that I know is in the middle
and I'm going to go forward following the blue dotted line
and I am going to draw my section line straight down
and that will create my section view for me.
Now I have forgotten to change it
into ANSI so I'm going to do that.
So let's go back to ANSI
Alright. Now, not all my view have the right
hidden lines. So this view
should not have any hidden lines because it's an isometric
and this view should not have any hidden lines
because it is a section view and I don't show hidden lines on section views.
Now I will need to add my
centerlines to my views.
So I'll click 'Okay'
and I will go to 'Annotation'.
My centermarks have already been taken care of
except this centermark should extend all the way out
past the edge of this outer circle.
So I grab this little blue dot and I pull
it along until it goes out all of the way that it needs to go
and these lines would also come out
although they are obscured by the section lines.
Now I'm going to go to
'Centerline'
and I need to put a centerline down the middle of this part,
and I'm going to put centerlines for the circular holes.
So now I have all my centerlines
I have my views in place, I have a section view
and I would go through and edit my title block,
and set the page size and print.