I recently ran in to a need to create a few structural brackets for framing up a new deck. I found that one manufacturer didn’t have 3D CAD models to download but they did have .dwg files that I could download and create a 3D model from. So I brushed off some cobwebs on how to use the built in 2D to 3D tools built in all version of SOLIDWORKS and thought I’d share my relearning with everyone.
Step 01 – Download the dxf or dwg that you need. For this example I’m downloading a dwg of a Joist Hanger from https://www.strongtie.com/ . Their download site is https://www2.strongtie.com/drawings/ at the time of this posting. If you look at the screen capture from their website they’ll give you a few options and I found that the top option includes the front, left, right and top views all in a single dwg.
Step 02 – Open the dwg in to SOLIDWORKS. Here are the settings that I use:
Setting 02 – Optional to have constraints added
Setting 03 – This is a good option to have on because your model creation will be easier if you have clean sketches.
Once you hit finish SOLIDWORKS creates a single sketch of the 3 different views. This sketch may need some cleanup. Lines that don’t connect to arcs, etc… A single sketch is created if all three views are only on 1 layer in the original dxf/dwg. When SOLIDWORKS finishes importing the model you will most likely see the 2D to 3D toolbar turned on on the left side of SOLIDWORKS. This 2D to 3D toolbar can also manually turned on.
Step 03 – Now we need to position the sketches in to the correct orientation by using the different ‘Add to…’ buttons on the 2D to 3D toolbar. We first start with the ‘Add to Front sketch’ button. While still editing the sketch that was imported, select all of the sketch entities that make up the front view and then click the Add to front sketch’ button.
Step 04 – Then we’ll go though and select the additional sketch entities that make up each of the different views and then click the corresponding ‘add to…sketch’ button. Top, Right, Left, …. as many as there are that pertain.
You’ll see that after the ’add to…sketch’ button is clicked, the sketch entities will then rotate to their new orientation. You can exit the original sketch and you should see something like the image below.
Step 05 – In this step we’ll use the ‘Align Sketch’ button on the 2D to 3D toolbar to align the sketches with the origin or the other sketches.
The way this button works is, you select 1 point on 1 of sketches and click the button and it will shift this sketch to align the selected point to be perpendicular to the origin. Or if you select 1 point of one sketch and 1 point of another sketch it will align theses point. It may be necessary to edit some of the sketches and add sketch points to assist with alignment. A trick that I’ll use is ctrl select two lines then click the sketch point button, this creates a virtual sharp sketch point, while editing the sketch.
With all of the sketches brought in from the dxf/dwg files and aligned, the last step is to create your 3D model. In the case this being a sheet metal part here are my basic steps for this part.
Step A – Start a new sketch on the front plane and convert entities of just the inside edges. Then use the ‘Base Flange/tab’ to extrude up to vertex.
Step B – Use the side sketches to create cut extrudes sketch/features that remove the extra material.
Step C – Complete the part using edge flanges, cut extrudes, tabs and forming tools.