Wrap Feature Fun: Carving a Jack-O’-Lantern in SOLIDWORKS
The Wrap feature in SOLIDWORKS has been around since the early versions, but it just recently got a major enhancement. In SOLIDWORKS 2017, this feature gained the ability to apply the wrap to any surface, an upgrade from just analytical ones. I’ll show you exactly how this upgraded functionality can be leveraged to carve a pumpkin or work on any non-analytical surface to apply logos, engrave and emboss text and create natural-looking splits in geometry.
Picking Out the Pumpkin
Take a look at this pumpkin below that I modeled in SOLIDWORKS. Wrapping anything to the side of the pumpkin (which is a lofted surface between splines) would have been an impossible task with any release of SOLIDWORKS before 2017.
Using the shell feature, I first hollowed out the pumpkin with a few simple clicks – no scraping out the messy insides! Now that we have our pumpkin selected let’s get to the fun part of turning it into a jack-o’-lantern!
Carving (Wrapping) the Pumpkin
Just like in real life, our first step is to draw out the design. Here, I’ve selected the front plane to draw the classic, happy jack-o’-lantern. Once we have contours in place (we can have more than one contour, just make sure they are all closed), we can boot up our wrap tool.
Immediately, a refreshed Property Manager interface greets us. The wrap type should be familiar sporting the options to either emboss, deboss or scribe. Let’s select scribe. The enhancement comes in the form of the wrap method. Previously, this option did not exist. For the complex surfaces of the pumpkin, we will need to select the “spline surface” option, changing it from “analytical”. After that, the interface is just what we know and love. The source sketch is the sketch we drew our design on, the faces box should have all the faces that the sketch “projects” on and finally the accuracy (usually low is sufficient).
After hitting the check, we have our scribe lines. Now begs the question: Why did I choose to scribe rather than deboss greater than the thickness to punch a cut through? The answer is robustness. Instead of typing a deboss value that is greater than our thickness (which would work) we can future proof our model by having a feature that can handle end conditions to do the cutting for us. In this case, we’ll use the cut-extrude. That way, if we update the thickness or geometry of the pumpkin, it is more resistant to change.
We can start the cut by booting up the cut-extrude command, and it will ask for a plane to sketch on. Select the same plane that the original design sketch was created. We can now select the new faces and perform a “convert entities” in order to get that into the sketch. And from there, we can exit the sketch and perform a cut-extrude with the through-all end condition.
After reading through this, some of you may be asking: Couldn’t we have skipped the wrap feature and just use a cut-extrude > through all in the first place? Aren’t the results the same? And the short answer is no. Wrap is a powerful feature that considers the geometry and topology of the faces when it applies the wrap, whereas the cut-extrude by itself only projects the sketch in a linear direction. The best way to see the difference is to compare the two results side-by-side.
The image to the left shows the cut created with only a cut-extrude feature, and the image to the right shows the cut created with the wrap to guide cut-extrude. I turned curvature display on from the evaluate tab to make my point easier to see (radioactive green is a good look for these pumpkins, huh?). The picture on the left is the pumpkin with only the cut-extrude applied. Take note of the thickness of the eyes, which are completely black. This denotes zero curvature. Looking closer at the mouth on the left side, we see that it is this consistent green color. This indicates that it has a curvature, but it is unchanging throughout the face. From this, I conclude that the geometry is unnaturally consistent. Observe the same areas on the right-hand picture. The color is constantly changing which indicates a more natural application of the cut, adjusting with all the contours in the outer surface of the pumpkin. In the end, the wrap features helps the jack-o’-lantern achieve a more natural look.
Now, let’s check out the finished jack-o’-lantern below!
Setting the Scene
Now that we have a finished carving, wouldn’t it be nice to set it in the dark and light a candle? Well, that is more than a possibility in SOLIDWORKS! On the top of the Design Tree, click the Display Manager tab (it’s the tab with the beach ball) to see the appearances. On this page, click the third icon that has a camera over a checkerboard to activate the Scene, Lights and Camera options.
You will see options like these:
The first thing to do is right-click “Scene (3 Point Faded)” > “Edit Scene” to activate the Appearances, Scenes and Decals pan on the right-hand side of the screen. Scroll down in the Basic Scenes list until you find “Pitch Black”. Click it and hit the check to activate the scene. Things should be very dark now.
Right-click the Ambient light and select “Off in SOLIDWORKS” to darken things even further. Right-click the Lights folder itself and select “Add Point Light”. For the basic settings, check “On in SOLIDWORKS”. Set Ambient to 0, set Brightness to 1, and set Secularity to 0. The settings in the bottom of the pane define where the light is in the model. If you model the pumpkin origin-centric, you can set the coordinates to (0,0,0) (the approximate location of a flame). Hit the check mark. Your model should now look something like this:
Now that’s spooky! Optionally, you can take this even further and turn off all the lights except for the point light to achieve the jack-o’-lantern in the dead of night look.
Show Me What You’ve Got!
Now that I’ve shown you how to carve a pumpkin in SOLIDWORKS, just in time for Halloween, I would love to see what the community comes up with. Here are some more designs that I implemented using the technique discussed above:
Leave a comment below about what you’ve carved this season in SOLIDWORKS. Thanks for following along!
Author: Robert Maldonado, Application Engineer at DesignPoint
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