SOLIDWORKS Haunted House Using Surfacing & Weldments

Are you as excited about the cool fall weather and Halloween decorations as we are? This article walks through the use of SOLIDWORKS Surfacing and Weldments (which can be used with any tier of SOLIDWORKS Standard, Professional, or Premium) to create a spooky haunted house. Final touches were made in SOLIDWORKS Visualize to create the ultimate spooky season render (and a 3D print!). Finally, we’ve also included a STEP file for download and use.

Using SOLIDWORKS Surfacing

If you look around at everyday objects (e.g., the mouse at your desk), you can probably tell right away that it would be a living nightmare to reverse engineer using solid body modeling features (e.g., Boss Extrude, Revolve).

Most SOLIDWORKS users are quite familiar with modeling using solid body geometry, but there does exist an entire world beyond that: Surface Bodies.

Surface bodies are usually a means to an end – if you can entirely confine a bounded volume within a collection of surfaces, you can define a solid body. There is, after all, a reason why the Knit Surface command contains the check boxes Merge Entities and Create Solid.

The Haunted House model in this example can absolutely be created using solid bodies; however, Surfacing was used instead to highlight some of the interesting ways these geometries can be created.

Creating a Haunted House Model in SOLIDWORKS

First, I used a rough sketch of my idea to start forming the layout.

After creating surfaces to create the base of the Haunted House using the Extrude Surface and Trim Surface commands, the design begins to come to life.

All of the bodies in my SOLIDWORKS Viewport are Surface Bodies – evident by the blue outline on their edges, as highlighted below.

The blue edge color can be changed from the default via System Options > Colors > Surfaces, Open Edges. In any case, the color simply communicates that there are indeed Surfaces and they have open edges.

Next, it's time to focus on the roof, to make it a bit more realistic – and create some more solid bodies!

I’ll use the SOLIDWORKS Thicken command to add thickness to the roof, which can be located quickly via the Command Search, or by pressing the keystroke S in the SOLIDWORKS Viewport and typing Thicken into the search bar.

Once both sides of the roof’s surfaces are thickened (7.5 inches thick), I’m left with a gap at the apex of the roof.

After a quick sketch and Boss Extrude (making sure to keep Merge Result selected!), the main roof is complete.

A few more Thicken commands on the remaining roof areas completes the roof.

I've also added some keyhole windows (solid bodies, created with an Ellipse Sketch, a Boss Extrude thin feature, and a Circular Pattern to the top turret of the house.

As you can see, there are some surface bodies to deal with in the model. But the shape of the house is coming together!

Using SOLIDWORKS Weldment Profiles

At this point, let's shift gears to Weldment Profiles to add some character to the spooky Haunted House.

Looking back at the original sketch, there is a frame/border around the house.

I'll use a custom weldment profile to create this effect. (For a good primer on creating and utilizing your custom weldment profiles, check out our Create Custom Weldment Profiles in SOLIDWORKS guide.)

In this case, I created a 10" x 10" square profile with a 9" x 9" inner profile. This creates, in effect, a hollow beam once in use.

I saved my Weldment profile and followed the steps in the guide above to use it in my Haunted House. After deciding where I wanted to place these beams, I created a 3D sketch to outline where I’d like them placed.

Once satisfied with my 3D sketch lines, I can start creating my weldments/structural members.

This is accessed via the Insert > Weldments > Structural Member menu options.

Note the use of Groups within the Structural Member command. There are a few rules to what comprises a Group using the Structural Member command, but first, let’s define a Group: it’s a collection of segments in a Structural Member command that are related in some way; there are two kinds of groups:

1. Contiguous - segments that are joined continuously, or end-to-end; can be joined continuously so that the end-point is coincident with the starting point.
2. Parallel - discontinuous segments that are parallel (differing from the contiguous type, in that they are disjoint).

Because I have purposely designed this house to have a bit of a surreal edge to it (i.e., it’s drafted ever-so-slightly upwards), a number of Groups are comprised of just one Structural Member; they are neither parallel nor contiguous with another Weldment profile.

I can change the Corner Treatment of my Beams/Structural Members by selecting the purple dot defining a corner.

I want End Miter treatments on the corners of the main part of the house, so I pick the Group selections and define the Trim Order to achieve the corner treatment I need, and verify the end result in the preview window before clicking OK.

Want to learn more about Weldment Profiles? Check out our SOLIDWORKS Weldment Profiles & Weldment Tools Guide.

Final Touches

The keyhole windows have been included in the top turret of the house, but to add some additional spookiness, I'll include some “normal” windows with broken shutters.

I created two Boss Extrude features to make two window frames and a crooked shutter for the left window, then used a Linear Pattern to place the left-hand shutter on the right window. Using a Cut Extrude feature to “break” the shutter, I was able to create a dilapidated façade effect. And with a Mirror Feature across the mid-plane of the right window, my windows and shutters are complete!

To add the effect of a front porch, I utilized the Sketch, Split Line, and Delete Face features on all sides of the front porch to create a porch effect.

Two Boss Extrude features later, I have a front door!

Finally, I used the Thicken command to turn the remaining Surface Bodies into Solid Bodies.

Halloween Decorations

I was able to locate an STL of a skeleton and saved it as a .SLDPRT with a few modifications. I imported this into the Haunted House .SLDPRT file, and since this is a multibody part, I had to use the workflow outlined in: How to Transfer SOLIDWORKS Parts and Assemblies to a New Template.

Though this article focusses on changing templates, the workflow is great for inserting one .SLDPRT into another!

I used a little bit more creativity for an added spooky effect - a spider web in the corner of the porch, created with a 3DSketch and a few Swept Boss/Base features! Finally, a few SOLIDWORKS Appearances complete the picture.

A Note from the Author

I designed this SOLIDWORKS Haunted House with the idea in mind that it would be world-scale (i.e., it is nearly 50 feet tall).

I was able to use the Scale function in SOLIDWORKS to shrink this down to an appropriate size for my 3D printer. You can download the file here: Haunted House STEP File.

I’d say it was a great success!

Get in Touch!

Are you running into errors or unforeseen, unexpected behavior in the software? Email or phone Tech Support, or log into the GoEngineer Customer Portal to create a support ticket under the Support tab.

If you’re looking for your Account Manager or your Customer Success Manager:

1. Log in to the GoEngineer Customer Portal and locate your main Dashboard.
2. Your company’s Account Manager and Customer Success Manager (with their contact information) will be displayed front and center.

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