- [Instructor] In this example,
I'm going to show you how you can take model items
from the part side of your solid works design
and import them directly into your drawings view,
which can be really handy.
For this specific part, I've got a simple sketch,
but I used the fully defined sketch tool up above
to fully define every point inside of this
and give me all the dimensions that I could possibly want.
It's a little bit overkill,
probably not what you would typically do in your designs.
You might use less dimensions to design this feature,
but just to show the point
that all of these dimensions already exist,
it's a lot of information
and we're going to easily drop it in to our drawing view.
Now if I switch over to a drawing that I already started,
all I've done so far is simply just drop in
a front view of this item.
I haven't done anything else,
it automatically gave me my center marks
and my origin point here in blue
cause I don't have that hidden up here.
So I'm going to go ahead and click hide so it hides all,
that leaves me only with my center marks.
And I'm going to go up to the annotations tab
and the command manager up in the top
and click on model items.
Now you can see while I'm hovering over it,
it tells you directly imports, dimensions, annotations,
and the reference geometry from the models that you select.
So I'm going to go ahead and click on that,
brings up this dialog box here on the property manager.
And you can see we have a bunch of options.
So starting from the top, the source.
I always try to use the entire model
because usually the views will give you the dimensions
based on that orientation
so it's a pretty safe way to go.
I'm going to import items into all of my views.
Now I only have one view,
but if I had a multiple views like in each direction,
I would use this as well to give me the most bang
for my buck.
Moving down, we have more options
for what in the dimensions you want to pull forward.
I want to pull forward any dimensions
that were marked for the drawing
and any dimensions that were not marked for the drawing.
I'm going to leave all of the other items here left out.
So hole call-outs, hole wizard information,
instances or number of counts for certain patterns.
Again, you probably won't use most of this,
but the ones that you might want to use
are going to be toleranced, dimensions,
not marked for drawing dimensions,
and then other dimensions that are also marked
for the drawing.
Moving down, if you had any annotations in that view,
GD and T call-outs, weld beads, you name it,
it's all available here to be shown
as well as any reference geometry.
Now I'll note that this can be a little bit much,
it can drag on a little bit too much information
so I suggest starting with the least amount selected,
see what that gives you
and then you can always run the tool again.
So I'm going to go ahead and drag down to the bottom here.
The last thing that it's asking me
is to select the view itself.
So you have to select a drawing view and once you do,
you'll see your destination view pop up right here.
You'll notice that I can add other views if I wanted to,
but I'm just doing a single view for right now.
Once I'm all set, I click the green okay
and automatically all of the dimensions
that were in that sketch that made my boss
inside of this part are all propagated into the drawing
and I can drag and drop them and place them
wherever I need to to make it more clear
as to what's going on,
but I didn't have to make any of these dimensions,
which might've taken a minute.
Now they're all just here
and I can just move them around accordingly
so that my drawing view makes sense and is legible.
So pretty handy tip, pretty easy to use
and the more information that you put in your part
as we get closer to model based definition,
this is going to be the trend,
but the more information, dimensional information
and tolerance information that you can put
in your part file, the more that you can leverage
inside of your drawing views
to quickly make these annotated dimensional views.