SolidWorks 2012 and prior had two separate tools to create section views in drawings, Section View and Aligned Section View. Although these were very capable tools, there was two different workflows to create cutting lines for section views based on which tool was chosen. The two types of section views where not interchangeable. Both used sketches to determine the path of the section view cutting line. However, both tools produced very different results with the same sketch layout.
SolidWorks 2013 unifies these separate types of section views, along with half section views, into one tool called Section View. This new tool has expanded capabilities, being able to handle a wider range of section view types and scenarios. For example, you can now add arc offsets to your cutting line and get the correct display in the resulting section view. There are many other improvements as well.
When the new Section View tool is launched (without preselecting a sketch), a new user interface appears, called Section View Assist. Section View Assist allows you to rapidly generate cutting lines for your section views without needing to draw sketch entities. Four options for standard section views are immediately available: Vertical, Horizonal, Auxiliary and Aligned. Each of these can be previewed on any standard drawing view. Use Tab and Shift-Tab to cycle through the preview choices. Relations to geometry are automatically identified during the preview.
Vertical cutting line:
Horizontal cutting line:
Auxiliary cutting line:
Aligned (bent) cutting line:
To accept the cutting line placement and geometry relations, simply LMB click when the preview is at the desired location (more clicks will be required to place Auxiliary and Aligned cutting lines). The Section View Assist will then set the preview of the cutting line on the drawing view with any applicable geometry relations. Additionally, the Section View Pop-up appears nearby.
To accept the cutting line location, RMB click OK or select OK button from the Section View Pop-up. Then, just place the section view on the drawing sheet. In many cases, you can add you section view as easy as 1 – 2 – 3 clicks without the need to draw sketches.
Note: you can still create a sketch and preselect it prior to starting the Section View tool. This will allow you to bypass Section View Assist and use the same workflow as in SolidWorks 2012 to create a section view.
I was recently interviewed by Entertainment Engineering, an online magazine that covers technologies used in many types of entertainment devices and events such as movies, concerts, theme and amusement parks, electronic games, etc. The November 2012 issue focuses on the value of individual contributors and also of teamwork in the design process. Here’s the kicker, I’m quoted in the issue’s editorial article along side the great Steve Wozniak. Kinda cool.
The article for which I was specifically interviewed is called Teamwork Improves Section-View Options in SolidWorks 2013, which leads-off a series of interviews with various individuals from all over the engineering discipline. In my interview, I talk about the new SolidWorks section view functionality (now called Section View Assist) that has a whole new user interface that changes the way section views are created on drawings in CAD. This includes how I originally developed the concept which was then improved and refined via teamwork within the SolidWorks organization.
Section View Assist replaces the need to first create sketches before being able to create a section view. Instead, you can directly place cutting line on the original view and have the section view generated automatically. If you want to use aligned section view, you can add offsets to the cutting line directly in the Section View Assist interface (without the need to draw lines or edit sketches). Same goes to notch and single offsets. The new user interface saves time and steps. The improvement is nearly exponential. The more complex your cutting line, the quicker you can create it versus old methods using sketches.
With all the drawing improvements in SolidWorks each year, there’s often some small ones that don’t make it into the What’s New file. Last year, I covered several small enhancments in SolidWorks 2012 that weren’t in the What’s New. Well, it’s now time to start covering SolidWorks 2013. I’ll cover some of the bigger enhancements for SolidWorks, but I’m also going to cover some of these hidden gems too.
Section views are made of several elements, including a parent view, a cutting line, labels, and the section view itself. Both ASME and ISO standards have situations where the cutting line is not shown, such as with half sections or when the cut is obvious. Prior to SolidWorks 2013, hiding the cutting line required workarounds. In SolidWorks 2013, there is a very simple command now available.
To hide a section view’s cutting line, RMB click on the either the cutting line or the section view. Select Hide Section Line. That’s it.
Of course, the question now is, how are the cutting lines unhidden once they are hiding? Easy, RMB click on the section view itself and click on Show Cutting Line command.
The cutting line returns to the parent view as though it never went away in the first place.
In previous versions of SolidWorks, when you attempted to move the Section View letter by clicking on it and dragging, very strong soft snaps would often force the location of the letter to fall into one of two set locations around the Section View cutting plane line arrow. The snaps seemed even stronger if you were zoomed out a bit.
In SolidWorks 2012, users now have more intuitive control over the the placement of a Section View letter when they wish to move it. The two snap locations are not nearly so strong. It is still very easy to place a letter at one of the two locations by dragging and hovering the letter over the arrow tip or the bend in the cutting plane line. However, it is also much easier if you want to place the letter at a different location; particularly when you are zoomed out.
This improved functionality will help users that like their Section View letters to appear at alternative locations for style or maybe because of a very busy drawing with limited space.