2D DWG into 3D SW Part

Categories // 3D CAD, Tips & Tricks

A Slick Way to Convert

This article is also located in our DASI Blog 

Created by: John MacAurthur, Application Engineer - PDM Manager 

So I’ve shown this in a number of my training classes over the years, but I thought it was about time to put it into a blog.

There are many ways to convert DWG files into SOLIDWORKS, but I’ll show you my favorite:

Open the file in SOLIDWORKS, and select the DWG or DXF file. Make sure you choose Import to a new part:

SOLIDWORKS Import to a new part

If the data is clean, you can use it as is, but if there are many unwanted layers you can choose not to import them:


Click finish and it will bring in all 3 views into one plane in SOLIDWORKS. You’ll need to use the 2D to 3D toolbar, box select the lines that represent each view and click on the relative view button:

SOLIDWORKS 2D to 3D toolbar

This will line up the Front and Top, and the Front and Right, but not the Top and Right. CTRL-select a couple sharp corners and click on the Align Sketch button:

Align Sketch

This will get the 3 views into the correct orientation and location on the correct plane. Next, you’ll extrude using the contour selection tool to extrude the areas where there will be material:


Next, reorder the tree so the extrude is before the other two sketches, and repeat the extrusion process with the Top and Right view, clearing the merge result check box:

Convert 2D files to 3D in SOLIDWORKS

This will result in a jumbled mess of 3 bodies. However, you can use a handy tool under Insert - Features, called Combine. Be sure to set this tool to the common option, which will leave geometry where the 3 bodies intersect:

SOLIDWORKS Combine bodies

Insta-Part! With the possibility of some artifacts from the overlap, simply delete these using cut-extrude or delete face:

SOLIDWORKS cut-extrude

If you’re importing a sheet metal part, you can use Insert Bends and choose a fixed face:


And then, with your K Factor or Bend Allowance set, you can get a flat blank by clicking flatten in the sheet metal command manager:

Sheet metal command center

This is a very quick way to translate DWG data into SOLIDWORKS parts. Of course, there are a couple disclaimers:

  1. These instructions assume the DWG was correct to start with.
  2. I did not include a step of fully defining the sketch entities, which would be necessary for editing the data if needed.
  3. This does not work with every geometry condition, but when it does its pretty slick.