- [Narrator] While it's not the preferred method
of receiving data,
Solidworks does give us the ability
to import DWGs and DXFs directly into our part files.
Here you can see some 2D data
that I've downloaded off of McMaster-Carr
of a stainless steel ball valve.
Let's go over to Solidworks
and see what happens when we import this
into a part, and use it to rebuild it into 3D.
Let's start by going to my Open dialog and finding the part.
Now, you see here I've downloaded
both the DWG and the DXF file version.
I'm going to start by choosing DWG.
Like other geometry that we import,
we want to go down to the dropdown menu
and select DWG from the dropdown
so we can see any options
that might be available to us with that file.
Unfortunately for DWG files, there are no options.
Unlike STEP files and other 3D data,
this is just simply opened and converted.
This makes sense because when we think about it in the end,
2D data is simply points and lines,
and there's not really much to be done.
I'm going to go ahead and click Open.
When we do that,
it brings up a whole other prompt
for importing DXF and DWG files.
For this example, we want to drag it into a part.
So, from this menu,
I'm going to choose Import to a New Part,
and I'm going to do so as a 2D sketch.
Now, it is possible to import 3D/2D data.
This is something like an Autodesk Revit file,
or something else that's not typical 3D,
but uses 2D geometry to build a 3D model.
Solidworks handles this a little more poorly
than 2D sketches,
so typically, I always go with a 2D sketch,
and then if I have to build up the geometry around it,
I use the different views to do so.
Click Next.
Now, for a DWG and a DXF, this will be the same process.
So, when you come to this next part of the file,
you see your preview here
of the geometry that you're bringing in.
You have the option to
change the preview to a white background,
if that's easier to see,
depending on your layers and colors,
but this is quite a simple example,
which just has black and white lines.
I'm going to switch back to the black format,
which I'm used to seeing it as in Draftsight,
as you can see there.
On the left, we have things such as units.
Again, you want to select
the proper units for your drawings
so that everything is scaled correctly.
This becomes especially critical
when you're converting from 2D to 3D data.
While it's good to steal geometry,
and increase the productivity,
you want to make sure that
you're not doing it with something that's wrong.
You can also add constraints or import the dimensions
if you like,
I typically choose not to do either.
Also, if your DWG or DXF file has many layers built into it,
you can select the many different layers be brought in.
This drawing only has one layer attached to it,
so I'm going to use that All layers button,
or I could use select layers and just turn the one,
but you can see, as I turn it on and off,
what the effect is.
Essentially, if I turned it off, I would import nothing.
So I'm going to keep that on, and select All layers.
You also have the ability
to import each layer into a new sketch.
And if you're bringing in
something like a layout of a facility,
this can be extremely handy
when trying to separate out the information.
Moving to the next tab, we have more options.
It's trying to make continuous lines throughout the sketch,
so it asks me if it would like me to
Merge points that are closer than a certain distance.
I leave this set to the default,
and just let it go through the process.
If you have a complex 2D geometry
that you're trying to bring in,
you may need to merge overlapping entities.
Often with 2D data, you'll find items
such as lines that are overlapping due to the construction,
and you don't want to have overlapping lines
in your final 2D output
because it can lead to headaches,
such as not being able to figure out where a contour's open
when you're trying do an extrusion.
You also have the ability to remove entities from the model.
So, if I click on Remove Entities
after selecting a line,
it'll delete it.
Again, select a line, Remove Entities, delete it.
You can also undo it if you don't want to do it,
but you can see how you can quickly clean up a model
before you even bring it in.
Again, I can set the location relative to the origin,
I leave it as the default and hit Finish.
One of the options that typically comes up is this one,
to Enable the Explode Blocks option.
This is what you will want to do.
Blocks are a feature of 2D geometry,
and being able to explode them
gives you the ability to dismantle a block
so you can convert its geometry, or edit it appropriately.
So I'm going to click Yes, and there we go.
As you can see,
relative to the origin that was set forth in Draftsight,
I have all of my 2D data.
Now, if I want to,
I can go right ahead and make an extrusion from this,
for example,
and simply choose the contours that I want to use.
You can see that you can select any closed contour,
just as if it was native geometry.
Drag it out, create an extrusion,
or any other feature that I like.
You will notice that as I drag around,
Solidworks has a little bit of trouble handling it
because there is a lot of geometry in here.
So, if you don't need any of the geometry in this drawing,
my suggestion is to get rid of it as soon as possible.
For example, if we zoom in here to look at this notation,
that's all line segments and automated geometry.
I'm going to get rid of that.
Just by selecting it and hitting Delete,
we get rid of that geometry.
You can also scan from right to left,
selecting more geometry to delete.
My border is also unnecessary.
I'm going to select that and delete,
and you can see how I quickly clean it up
to the base geometry that I need to convert
or export any other information.
If we go up to our Sketch Tools,
we can see all the options available to manipulate this.
But even more critical is our Sketch Settings,
where we want to have some things
like Automatic Relations and Automatic Solve on or off,
depending on the size of the drawing.
Sometimes with these options on,
it's too hard for Solidworks
to handle the automatic relations it's trying to create,
so if you're running into issues,
go to Sketch Settings
and turn these options on and off
until you get what you want.
New in the Solidworks 2017 is the Shaded Sketch Contours.
What this means is if
you have a closed sketch contour that you made,
it'll fill in and shade it, so that you know.
I typically keep this off right now.
So as you can see,
it's pretty simple to bring 2D geometry inside of a part,
and then start working with it.
It's basically just line segments.
The process for doing a DWG and a DXF
being brought into a part file are exactly the same.
So feel free to follow the same steps for both file types.
Once you're done,
you will want to exit the sketch
and then save the part file
before you move on any further.
Now I have 2D geometry
that I can go back into and edit at my leisure.