SolidWorks LoftSweepExtract
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Today we're going to talk about a few different ways to create new features.
We're also going to talk about how to put an object into
a drawing so that we can use it for machining
or giving other people.
I have already taken this document and put it in
the ANSI drafting standard and I have chosen the units
to be inches. The first feature that
we're going to create is going to be a loft.
And for a loft I want two shapes in space that I am
going to connect with material. So the first thing I'm going to
do is go to my right plane.
And I am going to create a sketch
on that plane. I will put a
circle that has as its center
the origin. I'll make it
an arbitrary size, I would wanna choose a size for it
if this were actually a part.
I will finish that sketch, go back
into my isometric view and now I
need a second profile in space
to connect this one to. And the best way to put it
out into space is to use a 3D sketch.
So what I will do is go back to the 'Sketch' tab,
I will choose the right plane again,
and I will create a plane in the 3D
sketch. So I will click
and I will tell it that I want it to be, maybe
3.5 inches away from my
original plane. I will
choose 'Okay' and now
I have a plane that is 3.5 inches away
from my first profile.
I'm going to finish this and
create a new sketch on this new plane.
So I will click on the plane and I will
create a new sketch. I will
create a second circle that, again,
is centered around the origin.
And I'll make it a little bit bigger. It can be smaller, it doesn't
matter. Now I am going to go back
to 'Features', I'm going to
exit out of my sketch and I will
do a 'Lofted Boss Base'.
Now it already chose my big circle so I'm gonna choose the little circle
as the second profile
for my loft. I don't want to hit 'Okay' yet because
if you can see these lines that are
going from one profile to the next are twisting around.
And I don't want it to be twisted around.
So the way to take care of this is to
move these little green dots around so that they line up with
one another and go straight from one
circle to the other. This can be a little difficult to see
and to get to the correct place. So I am going to
use the 'Normal to' command
and I am going to
let that help me get these
one right on top of the other. When I am
successful with that I will
no longer see all of those lines going
between the profiles.
Now I can click 'Okay'. I will put
it back in isometric view and I have my loft.
The next thing we're going to look at is
the 'Dome' feature.
So I will click on 'Dome' and then all I need to
do is click on some sort of circular face
and it will start creating the dome for me.
I can change the
radius of the dome from really big to small.
I'll choose something somewhere in the middle.
And then I will hit 'Okay' and and it's
created a dome on the end of my loft.
Alright, we're in a new document, still with the same settings.
Now I want to show you
the 'Sweep' function.
So what I'm going to do is, again, create a sketch
on one of my planes. We'll go ahead and do the front plane.
Go to 'Sketch', create a sketch,
and I am going to create
an Allen wrench. So what I
want is a hexagonal profile.
And I will
place the center of my hexagon
and then I will decide how big I want my hexagon to
be. I am going to choose to make it
actually, only a quarter of an inch.
And then I will hit 'Okay' and I have this little hexagon.
I could've done a number of different polygons with any
number of different sides.
I will then hit 'Okay' and finish my sketch.
Next I'm going to
create a path along which SolidWorks is
going to create this sweep.
So what I'm going to do is, this time, click on the top plane
and I'm going to create a sketch,
and I'm going to make it so that I can see it
by using the 'Normal to' function.
And I am going to create
the shape of my Allen wrench.
So let's create it
Something like this
And then I will finish my chain.
Now I am finished inserting lines but
I don't want there to be this square turn here.
So I want to make that a smoother turn
and I am going to use a fillet for that.
So I am going to click on my two lines
And
I am going to change my fillet parameter, I'm going to make it bigger.
So maybe something like that.
And then I'll hit 'Okay'.
And now I am going to
finish my sketch.
Go to 'Features', 'Swept Boss Base'
It already chose the path for me, I am going to choose the profile.
It'll preview the sweep for me.
And I will hit 'Okay'.
And now I put this back into isometric
And now I can see my Allen wrench.
The last thing I wanna look at for features
is how to create a linear pattern.
So once more I'm going to create a sketch.
And I'm just going to extrude
a rectangle so I have a block.
Now I am going to create a sketch
on the face of this block.
And I am going to put a rectangle
on the block and I am going to use that rectangle
to cut out a hole.
Now if I want to repeat this rectangle so that I have more than one hole
I can use the 'Linear Pattern' function.
So I am going to leave my cut highlighted.
And I am going to choose 'Linear Pattern'.
Now I can choose up to two directions
So I can do a linear pattern going along this
axis and I can also do a linear pattern going along this axis.
Now I am going to change the spacing.
of my linear pattern so
I am going to put each of these about 3 quarters of an inch apart.
And I am going to
create maybe nine of them.
Now if I also want a pattern in the other direction
I am going to, in this case, go one inch apart.
And I am just going to make two of them.
So this creates a linear pattern
I am then going to hit 'Okay'.
And now I have a pattern of holes in my block.
Now what we're going to do is take this block and we are going to put it into a drawing.
So I am going to save it
because you have to save a block before you can put it into a drawing.
And then I am going to go up to the 'New' menu
and create a 'Drawing from Part/Assembly'.
The first thing its going to ask me for is my sheet format and size.
I will browse for this and I need
to go into the Class Drive,
go into FEH,
1282H,
templates and I am going to choose the OSU Drawing Template.
And I will open that and I'll
leave everything else the same and I will hit 'Okay'.
Now this 'View Palette' shows up
on the right side and I can use that
to insert my drawing.
Or I can go over to the 'View Layout' menu
I'm going to use the 'View Palette' this time.
And so what I'm trying to do here is to create a set of orthographic views.
I like what it's chosen for the front view and I
am going to use that for the front view but I don't
if I liked the top view better as the front view I could put that as
the front view it all depends on how I modeled my part.
So I'm going to drag my front view
onto my sheet.
And then as soon as I've done that it's going to
allow me to drag out additional views.
So I'm going to put a top view
I'm going to put a right-side view and
I'm going to put an isometric.
Don't worry too much about exactly where it places it, you can move it later.
Then I am going to hit 'Okay'.
I"m going to move my isometric around.
And this is — this is getting there. Now one
problem I have here is that these three views
all showed up with hidden lines, and I'm going to want to verify that.
If they all show up with hidden lines then I'm in good shape
If not I may need to add them in.
This view over here showed up with hidden lines as well.
And I don't want hidden lines in my isometric view because these are all through holes.
So what I'm going to do is click on this isometric view
And I'm going to un-check 'Use Parent Style',
Then I'm going to look at these different views here and I'm going to choose the one that doesn't show hidden lines.
It's called 'Hidden Lines Removed'.
If for some reason one of my principal views showed up
without hidden lines, I could do something similar
I could instead click the button that says
'Hidden Lines Visible' but for my isometric views I don't want hidden lines
And then I am going to close the dialog.
These are filling up the page pretty well.
Sometimes that won't be the case.
So if that's not the case then
I will click on this front view and I can change the
scale to use a custom scale.
So I can make it bigger, I can make it smaller.
1:2 is actually a pretty good scale for me so I'm going to use the sheet scale.
Here in the drawing I'm going to want to go back up
to 'Document Properties' and verify one more time
that my drafting standard is put into ANSI.
This is going to become extremely important
when we start dimensioning these parts.
Now I have all of my views
on my sheet, and
and the thing I have left is to change my title block.
So I'm going to
right-click on 'Sheet Format'
and choose 'Edit Sheet Format'. Now my
views are all going to disappear.
And that's okay, don't panic when they disappear.
Now what I'm gonna do is go down to each of these sets of X's
and edit them. So I'm going to
double-click on drawing title,
and I'm going to give it a funny title.
And I'm going to double-click on 'Drawn by'
and I'm going to type in my name.
The one thing that you're — that shows up on this title block
that you are not gonna have is a seat number
So you're just gonna double click on that and put in 'N/A'
And anytime I'm done editing text I can
either click the little check mark or I can just click out anywhere else on the sheet.
So you would go through and fill in the rest of these X's with the relevant information
Once I'm done I'm gonna go up to my upper right-hand corner
and I am going to finish editing my sheet format,
and all of my views will show up again.
Before I print this
I need to go to 'File'
'Page Setup' and make sure that I
choose 'Scale to Fit'. This is going to make sure
that my whole sheet shows up on the page when I
print it. Then I'll hit 'Okay' and
then when I'm ready to print my sheet I will just go up to
'File', 'Print', and print from there.
Now, we have
put this part here, on the drawing sheet.
But this hasn't forced us to create any centermarks or centerlines.
And we should do that. So I'm going to go back
to my original part and I am going to
add a hole that is a circle.
So I'm going to put a circle
somewhere here on the part. I'm going to
close that dialog, exit the sketch.
and create an extruded cut of that circle.
Hit 'Okay'. And now if I save my drawing over here
And I go back over to my drawing
you can see that my hole has shown up. So now
what I'm going to do is add in
my centermarks and centerlines.
I will go to 'Annotation'
and I will go to centermark,
and I am going to choose my circle here.
Remember we don't put centermarks on isometrics.
Once I have chosen all of the circles
that need centermarks, I am also
going to put on centerlines.
And so the side view of this hole
is over here, so I choose the two lines
that are the extreme elements of the hole
and I put the centerline between them.
Up here its a little harder for me to see which ones are
the hidden lines representing the circle.
I believe its these two so I add a centerline there as well.
So that is it for
lofting, creating domes, sweeping,
creating a linear pattern, and creating an annotated drawing.