Inserting a 3D Cross-Break in SOLIDWORKS

Article by Jim Peltier, CSWE updated February 23, 2017


A question we sometimes get in the SOLIDWORKS Sheet Metal course is how to insert a 3D cross-break. The functionality seems to be there in the SOLIDWORKS Cross-Break command on the Sheet Metal toolbar, but upon inspection, the cross break it inserts is merely cosmetic. In most applications, this will be sufficient, since the distortion on the actual component will be minimal.

Indeed, by SOLIDWORKS doing it this way keeps the geometry simple (lending itself to faster system performance) while not sacrificing too much in terms of functionality. After all, the cross break is still shown on the drawing in the bend notes, so the shop floor will still get it done.

Cross-Break command and result

SOLIDWORKS Cross-Break command and result

However, this does not dissect the top face and does not give me the slight pyramid shape that I would expect to see in the real world. Let’s say that was important to my design intent and I needed to show it. How can I go about doing this? I can’t use Sketched Bends for this, nor can I use an Edge Flange. This is due to the fact that I have two bend lines that cross each other. Well, luckily there is a way to do this without using bends or flanges.

What I need to do is use a Forming Tool to achieve what I’m try to do. I take a quick measurement of the rectangle I’m trying to cross-break (in this example, 150mm x 195mm). Then I create a new part and sketch the rectangle, 150 x 195, as shown below:

Cross Break Sketch

Cross Break Sketch

If this was a square, then I could just do a Boss-Extrude with the Draft option selected, but if I try this with my rectangle, I will not get all the faces converging on a single point. I could do a simple Boss-Extrude, then apply draft afterwards using the Draft command, but I’d have to use trigonometry to get the desired angle, and if my rectangle size changed, then I’d have to revisit all my math. Instead, I’m going to use the Lofted Boss/Base command. Of course, you’re wondering how I can do this, since I need two sketches. Well, I’m transition this rectangular profile into a single point, so I’m going to make a second sketch (on an offset plane, of course), that contains a single point. Behold:

Sketch point of second sketch indicated. It is on Plane1

Sketch point of second sketch indicated. It is on Plane1, and centred on the origin

Now I have two profile sketches (even though one of them is just a single point). Now I can crease my loft feature using the Lofted Boss/Base command. This gives me my very flat pyramid, which I will use as a forming tool to give me my 3D Cross-Break. If you’re not familiar with the process of creating a forming tool, please refer to this forming tool blog article which explains the steps well.

Please note: that the Forming Tool Stopping Face will be the flat base of the pyramid and there should be nothing selected for Faces to Remove.

Once you have your forming tool, you can switch back to your sheet metal part and use it. Be careful to locate the forming tool using the Position tab, as shown below:

I like to reposition the insertion point so I can select it (middle of image)

I like to reposition the insertion point so I can select it (middle of image)

Then, I apply Horizontal and Vertical sketch relations to the midpoints of the edges:

Right-click, Select Midpoint

Right-click, Select Midpoint

Once completed, the end result is shown below.

SOLIDWORKS Cross-Break applied

Measure angle between faces

If you’ve done this correctly, the faces should be split and you should be able to measure an angle between the faces.

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Jim Peltier, CSWE

Jim has been using SolidWorks since 2001, and has spent most of that time working in the design of industrial automated manufacturing equipment. He has been working as an Applications Expert at Javelin Technologies in Oakville, Ontario since July 2012 and is a Certified SolidWorks Expert (CSWE).