- [Instructor] Now you may have just been taking this course
in order to practice your SolidWork skills,
but maybe you actually want to build this frame
in real life.
If so, then we need to somehow transfer these virtual parts
into the real world.
So let's have a look at the model.
If you're starting fresh at this point
and using the exercise files,
then unzip the chapter six files to a new folder
and open the assembly file for chapter six.
So to make this frame, first we need to cut out
all of these tubes to the correct length.
So let's have a look at this top tube, for example
going to zoom in, going to click on the tube
and press open parts.
Now to measure the length of the tube is reasonably easy.
We can just start sketch on the right plane,
then we can get a center line
and draw two vertical center lines, one at each end.
Then we can zoom in, we can select the line,
also select an outer curve of the tube,
and then we can add a tangent relation, like so
and that will move the line to the outside of that curve.
Can do the same on this end.
So select the curve, select the line and add a tangent.
And then we can just use smart dimension
to measure that distance.
So we can find out the distance like this,
is reasonably easy to find that out.
However, if we look at the model in 3D,
we've also got these curved notch areas at both ends.
So we need to cut these out at the correct angle
and if you don't have a specialized tool for this
maybe something like a milling machine,
then this is potentially really difficult,
but we're going to have a look at a way,
you can transfer these notch cuts onto a paper template,
and you can then use these
to cut the tube perfectly by hand.
We'll demonstrate it with this top tube
but the process is the same for all of the tubes.
Essentially, we need to flatten the tube out.
To do this, let's start a sketch on the same plane
the tube profile is drawn on.
So for me, this is the front plane, going to start a sketch
and go normal too.
So you should just be able to see the two profile like this.
Then we need to draw a very thin cut through the tube.
So zoom all the way in, get the center rectangle,
just start at the middle of the tube at the top
and draw something like this.
We need to make this a very thin curve.
So it's almost so thin that we can just ignore it.
So I'm going to make mine nought 0.1 millimeters
and then for the height can be any height really
as long as it cuts all the way through.
So I'm going to make mine 10
and then you might just need to zoom all the way in,
select the center point of the rectangle
and then also select the origin
and just make those vertical,
and that should fully define your sketch.
So we're cutting all the way through the top section
of the tube there.
Now use this profile to cut a slice
all the way through the tube.
So I'm going to go to features, extruded cut.
I'm going to go to through all
and then you might need to flip the direction
so we're cutting all the way through like this.
So now it's quite hard to see, but if we zoom in
we've got a very thin slice all the way through the tube.
This now means that we can unroll or flatten this tube.
To do this, go to the sheet metal tab.
If you can't see the sheet metal tab here
then just try right clicking on any of the other tab names
and then go to toolbars and then just select sheet metal.
So go to the sheet metal tab
and the tool we want is called insert bands,
it's this one at the end.
Select that tool, we can keep all of the options as default.
Just make sure you're in this first box
and then zoom all the way in
and choose this upper edge and then just press okay.
Now if we zoom out, it looks like nothing's happened.
If you look here on the left
we've got a load of extra new features.
These indicate that this is now a sheet metal part
so we can now flatten this tube.
To do this, just go up to the sheet metal tab again,
and choose flatten,
and now that part is flattened out.
If we look from the top,
we can see this is basically an unrolled version
of that tube.
If we look at the ends
you can see we've got this wavy shape.
This is basically a flattened version of that tube notch.
So if I press flatten again to fold up,
you can see that curve when we flatten
is actually the same curve there.
So we can actually print this shape out on paper
and then cut it out with scissors, wrap it around the tube
and then we've got a perfect template
to cut that notch out in 3D.
So print this out, we can add it to a drawing
by going to file, make drawing from par.
Then for this drawing we only actually need one view
that top view.
So open the view pallet here on the right
and just drag in that top view
and it should look something like that.
Let's make it a one-to-one scale
so click on the view and then here on the left go down
and change the scale to one to one.
And you probably find that it's way too big for the paper.
So let's drop out this middle section
cause we don't actually need that to go all the way
along the tube.
To do this, you can go to the view layout tab
and then choose break view.
Then select the view and choose the cut direction.
In this case, it's this one, horizontal break
and then zoom in and let's just make a cut, say here
and also here.
So we're going to cut out everything between these two lines,
like so, and if you need to,
you can just drag and adjust these lines later on like so.
So we can now print this out a hundred percent scale
or one-to-one, we can cut it out from the paper
and then we can take or glue it around the end of the tube.
And then we can cut that notch out using hand tools,
maybe like a file or maybe a rotary tool,
something like a Dremel
and you can use the exact same process for all of the tubes.
If you want to look at this process in more detail
then if you open the chapter six exercise files
there's a SolidWorks drawing file in there
called top tube notching template.
And if you open that,
you'll be able to take a closer look at how this all works.