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Solid Edge ST6 First Looks: 2D Drafting Enhancements

By Jeffrey Heimgartner, November 8, 2013

In this First Look article on Solid Edge ST6, I focus on new enhancements to 2D drafting functions using Extended Views and Break Lines. These two functions are used when creating 2D layout drawings of 3D models and assemblies.

Siemens PLM in their What's New in Solid Edge ST6? Fact Sheet describes the two new functions like this:

I was pretty excited to test out these two new functions.

Extending Views

No matter how good or how detailed our 3D models and assemblies are, 2D shop drawings are more often than not still required. They contain clear, concise details of how to make our product, and how it goes together. Even today, 2D drawings are needed for fabrication and manufacturing shops to build and assemble our products. Creating 2D views that show dimensions, details, sections, and so on are a must.

To test the new functions in Solid Edge, I used the 3D model of a trolley assembly (see figure 1). First, I created a set of 2D drawings from the 3D model:

Figure 1: 3D model of a trolley assembly

  1. To create a new .dft drafting file, I picked the appropriate selection from the New dialog box, and then selected the View Wizard command from the ribbon's Drawing Views pane.
  2. I selected my trolley assembly file, and then clicked Open.
  3. Here in the View Wizard pane, I could control options, such as View Layout, View Orientation, Fit, and Scale (see figure 2).

Figure 2: View Wizard settings

  1. Using the View Wizard, I easily brought in the standard front, top and side views, as well as the isometric view. The wizard perfectly aligned the views, as you can see in figure 3.

Figure 3: Standard drawing views created with the View Wizard

While the View Wizard helped me get perfectly aligned views right from the start, there may be older drawings or drawings imported from other CAD systems in which the views are not aligned. Other times, I may want to change the scale of a view or its location on the sheet. Solid Edge ST6 contains tools we can use to maintain proper alignment between keypoints in two associated views, even when the geometry is scaled, cropped, cut away by break lines, or otherwise modified. Drawing view alignment is associative by using true keypoints to align drawing views.

  1. By right clicking on a view and then selecting Create Alignment, I set up two alignments: first with Drawing View Centers option, and then later with keypoints.
  2. When I set up the alignment based on Drawing View Centers, Solid Edge ST 6 asked me to "Click on the alignment drawing view" to create the associativity.
  3. When I set up associativity through the keypoints option, Solid Edge asked me to "Click on a keypoint in the current drawing view".

After I set up my desired alignments, Solid Edge applied changes I made to a view position (or scale) to the other associated views.

Adding Break Lines

To test the break line features in Solid Edge ST6, I began with a simple three-view drawing of a long bar. It has some gear features and holes at either ends, but the middle portion is long and detail-free. As you can see in figure 4, the views fit quite nicely at the scale of 5:1. However, I wanted to increase the scale to 10:1 to make the details at either end larger.

The change in scale made the drawing twice as big, and too large to fit the sheet. To make the drawing still fit, I used the new break lines function in Solid Edge ST6 to remove the middle portion of the bar.

Figure 4: Drawing views at 5:1 scale

  1. I right-clicked on the view to which I wanted to add the break lines, and then chose Add Break Lines.
  2. From here, I controlled all the aspects of the break lines, such as how I wanted the break lines to appear: visible, hidden, phantom, dotted, and so on.
  3. Solid Edge ST6 also allowed me to specify the break line gap, the height, and to select from several different types of breaks. These included straight break, cylindrical breaks, linear and curved short breaks, and long breaks.
  4. After I chose my desired settings, Solid Edge ST6 prompted me to "Click in the drawing to place first break line."
  5. After doing so, I was prompted to select the location of the second break line.
  6. After selecting Finish, the break lines were added to my selected view (see figure 5).

Figure 5: Break lines added to the front view

After I added the break lines in the front view, it was time to add break lines to the top view. This is where the Inherent Break Lines option comes in handy: it copies and applies break lines from a source view to another view, either principal, section or auxiliary view. The resulting break lines are inherited and are associative to the source drawing view.

  1. To accomplish this, I right-clicked the other view, and then chose Inherit Break Lines.
  2. Solid Edge prompted me to select the alignment drawing view, the break lines were added to the top view using the properties supplied to the first break line command.

The result can be seen in figure 6.

Figure 6: Inherited break lines added to top view

Changing the Drawing Scale

Now that break lines have been added, I had enough room to scale up the drawing views to even larger details of the part's ends. To do so, I selected one of my drawing views and changed the scale from 5:1 to 10:1. As you can see in figure 7, all three drawing views were scaled correctly, due to associativity.

I was them able to dimension and notate the features on the ends of the part more clearly, with the larger scale.

Figure 7: Broken views at 10:1 scale

Conclusion

Drawing creation is still required after modeling to produce the documentation manufacturing shops need to fabricate our items. The quicker we can model, assemble, and create shop drawings, the quicker we get our parts built.

The tools available for Extended Views and Break Lines in Solid Edge ST6 definitely help us handle this aspect of drawings quicker and easier.

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About the Author

Jeffrey Heimgartner has over 20 years of industry experience. He manages Advanced Technical Services for CapStone's CAD division. He has a bachelor's degree in Industrial Technology with an emphasis in CAD from Wayne State College in Wayne, Nebraska. More...

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