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SOLIDWORKS vs Solid Edge: How Well They Import Legacy Data from AutoCAD, Pt 2

By Elise Moss, June 12, 2014  

continued from Pt 1

I then selected the top view as the primary view, and the front view as the secondary one (see figure 20).

Figure 20: Selecting the top view as the primary view (and the front view as the secondary one)

Once again, the views were not folded correctly. As far as I was concerned this was the third strike - and out! But I could work with it. I selected the Extrude tool, set it to the Face option, and then selected the outside regions (see figure 21).

Figure 21: Selecting the parts of the part

...only to get the error that the profile was not closed (see figure 22).

Figure 22: Error message about the incomplete part

No problem, I did a quick run of the Clean Sketch tool and then re-tried the extrude operation. This time it extruded without any errors (see figure 23).

Figure 23: Part extrudes correctly

For the second extrude, I selected the inner region of the cylinder, then tried to select the horizontal line to designate the cylinder height, which was demonstrated in an on-line video I had watched (see figure 24).

Figure 24: Selecting inner parts of the extrusion

 However, Solid Edge wouldn't let me pick the horizontal line to set the extrusion distance. So, I went back to the video to see where I had gone wrong. Apparently, I was supposed to define something called keypoints.

I tried selecting just one of the endpoints of the horizontal line, but Solid Edge wouldn't allow the selection. I then added a vertical dimension to verify the height of the cylinder, because I couldn't rely on Solid Edge to set the proper height. I retried, this timepaying attention to the on-screen prompts. I pressed K for explicit point, then E for endpoint, then selected an endpoint on the horizontal line (see figure 25).

Figure 25: Specifying the height of extrusion

The cylinder extruded to the correct height (see figure 26).

Figure 26: The cylinder correctly extruded

I then went through my Feature Browser and unchecked the dimensions and sketches to turn off their visibility (see figure 27).

Figure 27: Hiding dimensions and sketches

...leaving me with the finished 3D part in Solid Edge (see figure 28).

Figure 28: The completed extruded part

So, I had a few fits and starts moving from 2D AutoCAD to 3D Solid Edge, but overall Solid Edge made the experience fairly painless. The prompt bar definitely helped, as did the on-line help.

The biggest obstacle I had came at the end: Solid Edge doesn't see my Dropbox or OneDrive folders. I store many of my projects up on the cloud and the ability to open and locate cloud-based files from inside the software is becoming more and more of a necessity.


Moving onto SOLIDWORKS and how well it brings in a 2D AutoCAD drawing: SOLIDWORKS doesn't have the CleanSketch or Create 3D tools - both of which I found useful in Solid Edge. And so the process to go from 2D to 3D is different in SOLIDWORKS. We would start by opening a new part file in the desired units, and then insert the DWG file as a new sketch.

To insert a 2D AutoCAD file into a sketch in SOLIDWORKS, highlight the destination plane, then go to Insert-> DXF/DWG (see figure 29).

Figure 29: Accessing DWG files in SOLIDWORKS

Enable import to part as 2D sketch, and then press Next (see figure 30).

Figure 30: Choosing how to import the AutoCAD drawing

Among the options, I enabled the "Add constraints" option to try to keep the sketch as clean as possible (see figure 31). Then I pressed Next.

Figure 31: Enabling constraints

I find it is helpful to locate the sketch so it is centered on the part origin, and so I select Define Sketch Origin (see figure 32).

Figure 32: Enabling Define Sketch Origin option in SOLIDWORKS

To redefine the origin, I zoomed into the preview window and selected the center point of the circle (see figure 33). Then I pressed Apply. Note the dimensions updated based on the selection. There is no snap to the AutoCAD elements, so I was basically eyeballing it.

Figure 33: Picking the circle's center without snaps

Sure enough, when I inspected the sketch it was off ever so slightly from the origin (see figure 34). I am not sure if it would not have been better to not bother defining the sketch origin, as I had to adjust the sketch position any way using the Move tool.

Figure 34: Checking the origin offset

SOLIDWORKS is able to define the two regions without any additional clean up required. I entered in the value and pressed Enter to create the first extrusion (see figure 35).

Figure 35: Extruding the sketch

For the second extrusion, I selected the outer circular region and then entered in the desired height (see figure 36). I definitely felt the loss of the advantage provided by Solid Edge and its keypoint options.

Figure 36: Extruding the inner cylinder

And so I finished the extrusion part in SOLIDWORKS (see figure 37).

Figure 37: The part finished in SOLIDWORKS


Both Solid Edge and SOLIDWORKS were able to read a 2D AutoCAD drawing and convert it 3D parts in a matter of minutes. The tools for going from 2D to 3D are more advanced in Solid Edge, so I would name Solid Edge the winner on this one.

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About the Author

Elise Moss has been teaching Autodesk and SOLIDWORKS software for the past decade. She is an Autodesk Certified Instructor and teaches at an Autodesk Authorized Training Center in San Francisco. She speaks regularly at SOLIDWORKS World and leads the Oakland SOLIDWORKS user group. Elise has a mechanical engineering degree. Moreā€¦

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