Look up "2D to 3D" in the help. It is a little cumbersome to use, but you
can turn your 2D drawings into 3D models. If the drawing is of a very
simple part, you are probably better off just starting from scratch anyway
Simple rectangular parts are more efficiently created from scratch.
If you have hole patterns or complex curves, the importing can save some
I have in the past simply opened the dwg directly. Either into a part model
or a drawing file, depending on the DWG and how it imports.
Once in, I often found my self cutting and pasting accordingly.
For instance. - A simple block with holes on three faces. - Import the
three ortho views into a drawing. - (BTW ditch any annotations, they're
just clutter) - Start a new part model - create a sketch - from the
imported data copy one profile onto the sketch. - Extrude accordingly. -
Next select an appropriate face, create sketch and repeat with the
respective remaining orthographic views.
Bring along any holes, including the screw holes and use the centers with
the hole wizard.
Thank you for your help.
I don't want to use "2D to 3D". As you've stated "it's cumbersome".
I just want to bring the *.dwg or *.dxf of several trajectories,
profiles into SW model sketcher and do myself the loft protrusion. I
could be wrong but I don't think this is possible. I don't see any
option to import file into the model sketcher.
Oh, I see. It is not called an "import" per-say (until later anyway). Just
go File>Open and select .dwg or .dxf in the file type. Once you start
opening the .dwg or .dxf file, an import dialog will then pop up. In the
upper left hand corner you can select whether to import to a part (as a
sketch) or to a drawing. When you import it to a part as a sketch, you can
manipulate and use the sketch just as you can with a SW native sketch.
Hope that helps.
You're getting some answers regarding the 2D to 3D conversion, but if you
are looking simply to use geometry from AutoCAD to create sketches in
SolidWorks there are a couple of different ways. From AutoCAD, simply copy
(ctrl-c, edit>copy - choose your favorite method) the geometry you want.
Start a new part in SolidWorks and select a plane (you have to select from
the graphics window, not the feature manager), and paste. If you want fully
defined sketches you'll have a little clean-up to do. You might also use
tools>sketch tools>check sketch for feature to make sure you have clean
Please do not import all of the holes, cuts, chamfers, etc. from the AutoCAD
geometry. Use the SolidWorks tools to create features and you'll have much
better control of them down the road.
<end personal rant>
The other way is to open a drawing (.dwg) from AutoCAD and follow the
prompts to import to a new sketch. The drawback here is it grabs all of the
drawing views. Of course, as other have said, this is the way to start the
2D to 3D "converter".
Don't forget to sign up for SolidWorks World
Not a rant. It's sound advice.
In my previous post I had hoped to covey that one could preserve the
imported hole patterns for locating and then use the wizards. pretty much
the same applies for other features.
It has been so long that I in replying I was not selecting reply to group.
I will try one more time.
In 2004 we start a new part, select a plane, then under the Insert menu we
select DXF/DWG and browse for the DWG. This seems to work the best for us.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.