Is it possible to import *.DWG / *.DXF sketch into SW model sketcher?

Greetings:
I would like to avoid some redundant work to resketch by importing either *.DWG / *.DXF into SW model sketcher. Is this possible?
Thank you in advance for your time and help.
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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 though.
--
Seth Renigar
Emerald Tool and Mold Inc.
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in

Quite right.
Simple rectangular parts are more efficiently created from scratch.
If you have hole patterns or complex curves, the importing can save some time.
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.
JV
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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.
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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.
--
Seth Renigar
Emerald Tool and Mold Inc.
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John, 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 geometry.
<personal rant> 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".
Richard Don't forget to sign up for SolidWorks World
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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.
JV

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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.

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