Create Curvy Parts with Simple 2D Sketches

Most SOLIDWORKS users are comfortable with the process of creating machined parts. We start by deciding which geometry represents the overall footprint of the design and this gives us the starting sketch.

Figure 1. Starting sketch of a machined part based on the overall footprint of the part.

Things get a little more complicated when we’re asked to create models which will be injection molded. For today’s example, we’ll be working with a design that has no flat faces: a plastic kitchen ladle (or spoon).

Figure 2. Selecting a starting sketch is more difficult when there are no flat faces.

You might feel a little perplexed regarding where to begin on a model like this.

We’ll show you how to use tools such as Projected Curve, Trim Surface and Thicken Cut to perform a variety of surfacing commands on complex 3D models—and how the shape can be created by utilizing simple 2D sketches.

Start With an Image

When creating models of swoopy or lofty parts, it is helpful to have an image of the model (or something similar). I took some pictures of a spoon I had in my kitchen and used photo editing software to remove the background.

For more info on working with images, see the article “Using Photos in the Design Process.”

After cropping the images to create a new model in SOLIDWORKS and scaling the images to the correct size, they are positioned on the top and front planes.

Figure 3. Add top image and side image to a new SOLIDWORKS model.

Create Two New 2D Sketches

The 2D sketch is created on the top plane of the model. We’ll make a spline with four points and manipulate the spline to match the outer curve of the spoon.

Figure 4. Spline on top plane matching the curve of the spoon.

We’ll create another 2D sketch on the front plane and repeat the same steps to trace a new spline over the side view image of the spoon.

Figure 5. A spline traced over image of side view.

Once this is finished, we exit the sketch. We now have two 2D sketches, one on the top plane and one on the front plane.

Using Projected Curve

Whenever we have two 2D sketches, we can project these two sketches together to create a 3D curve. This technique is commonly used to generate a 3D guideline for a sweep or loft. We’ll do this with Curves > Project Curve from the menu.

Figure 6. Curves > Project Curve.

We choose the option for “Sketch on sketch” and then select the two spline sketches previously created.

Fiure 7. Creating a 3D projected curve.

The two 2D sketches are projected together, generating a 3D curve which will be used as a guide curve for a lofted surface.

Creating a Centered Guide Curve for the Loft

Since the model is going to be mirrored, the second guide curve is going to be created at the center of the model.  Once again, we’ll use the image to create a guide curve on the front plane.

When working with splines, it can be helpful to show curvature combs (shown in the image below). To view these curvature combs, click the right mouse button on the spline and choose “Show Curvature Combs.”

Figure 8. Centered guide curve showing curvature combs.

We’ll extrude this sketch into a surface body using the Extruded Surface command.

Figure 9. Extruded Surface command found on the Surfaces toolbar.

Extruding the spline into a surface will give us additional control during the lofting and help with mirroring this model smoothly across the center plane.

Figure 10. Creating a surface extrude from the centered sketch.

Creating Six Loft Profiles

Next, we create a series of loft profiles using 2D sketches. Having a 3D guide curve in place makes it very easy to lay out six loft profiles.  

Figure 11. Creating six loft profiles for the design, each a 2D sketch.

Creating a Surface Loft

Now that we have the six profiles, we can select the Lofted Surface command from the Surfaces toolbar.

Figure 12. Lofted Surface command on the Surfaces toolbar.

The six 2D sketches are selected in order as the loft profiles. Then we select the projected curve and the edge of the extruded surface (along with the center of the model) as the two guide curves.

Figure 13. Selection of profiles and guide curves for the lofted surface.

After selecting the second guide curve (which is the edge of the extruded surface) we will use the option of Tangency to Face as shown in the image above. This will enforce a condition where the entire loft will remain tangent to the extruded centerline surface and this will help ensure a smooth centerline transition when the model is mirrored.

Figure 14. The loft completed and mirrored.

The loft is now complete and after mirroring this lofted body, the model looks pretty good. We have successfully created a complex set of guide curves and a series of loft profile sketches, all using simple 2D sketches. Now, let’s add some final touches.

Using Trim Surface

Another tool commonly used in surface modeling is the Trim Surface command. Trim Surface is very similar to the Cut Extrude command that is used when working with solid geometry. We will use a 2D Sketch and the Trim Surface command to remove bits from the surface model.

Figure 15. The Trim Surface command.

We will round off the rear of the spoon and add a hole. Both features can be created with a single 2D sketch on the top plane and a Trim Surface command.

Figure 16. Sketch used for final trim on rear of handle.

Now we launch the Trim Surface command.

Figure 17. Use Trim Surface command to remove these areas.

We choose the option “Remove selections” and specify that that we want to remove the surface regions shown. When finished, we see the areas we specified are removed from the surface model.

Thicken to a Solid

Our surface model is looking pretty good, but it is still not a solid model. We can turn it into one with the Thicken command found on the Surfacing toolbar.

Figure 18. The Thicken command in the Surfaces toolbar.

We will thicken the model by adding 2mm of solid material to the inner direction of the surface model.

Figure 19. Thicken Surface to 2 mm.

The model is no longer a surface body. It has been transformed into a solid body.

Figure 20. The model is now a solid.

Using Trim Surface to Create an Indent Cut

To finish off the spoon, we’ll create some esthetically pleasing geometry—an indent along the length of the handle. We start by making a surface that is a copy of the top faces of the model with the Offset Surface command.  

Figure 21. The Offset Surface command on the Surfaces toolbar.

We will choose to offset the top two surfaces of the model by 0.00 mm.

Figure 22. Offset top two surfaces by 0.00 mm.

We create a 2D sketch on the top plane of the model representing the shape for the indent geometry.

Figure 23. Sketch for the indent geometry.

We use this geometry to trim the newly created surface offset, removing the outer geometry from the surface.

Figure 24. Trimming away outside area of offset surface.

Now we can take the newly trimmed surface and use it to perform a Surface Thicken Cut, found on the Surfaces toolbar.

Figure 25. Thickened Cut on the Surfaces toolbar.

Figure 26. Creating a thicken cut at 0.5mm in both directions.

We’ll do a thicken cut in both directions (the middle option) which made a cutting shape of 1mm thickness.  This is useful in surface modeling as it will help to avoid the slivers of material that end up around the edges of the cut if the cutting shape was flush with the top of the spoon handle.

Figure 27. Final model.

After adding a few fillets, we have a completed model—and are ready to create prototypes and share the design with the customer.


A design with no flat faces will often present a surface modeling challenge. But this doesn’t mean you have to make complicated 3D sketches. In this example, we saw simple 2D sketch geometry was used to create projected curves, loft profiles and trims. This geometry can be easily changed without breaking the feature tree. And the result will be a nice, swoopy, lofty model that will impress both your boss and your customers.

Learn more about SOLIDWORKS with the eBook SOLIDWORKS 2022 Enhancements to Streamline and Accelerate Your Entire Product Development Process.

About the Author

Toby Schnaars (AKA: TooTallToby) has been a SOLIDWORKS user, instructor and enthusiast for the past 20 years.  He has fielded over 10,000 tech support cases and has instructed over 200 SOLIDWORKS training classes.  He has earned the ranks of both Certified SOLIDWORKS Expert and Elite Applications Engineer (CSWE + ELITE AE). 

Toby regularly posts videos of SOLIDWORKS tips and tricks on his YouTube channel TooTallToby. 

Recent Articles

Related Stories

Enews Subscribe