2D DWG into 3D SW Part
A Slick Way to Convert
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:
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:
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:
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:
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:
Insta-Part! With the possibility of some artifacts from the overlap, simply delete these using cut-extrude or delete face:
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:
This is a very quick way to translate DWG data into SOLIDWORKS parts. Of course, there are a couple disclaimers:
- These instructions assume the DWG was correct to start with.
- I did not include a step of fully defining the sketch entities, which would be necessary for editing the data if needed.
- This does not work with every geometry condition, but when it does its pretty slick.