Creating a surface part without surfaces
- Brad Tallis
- 1 day ago
- 4 min read
A common problem is making a part with a curve in one direction on the bottom and a different curve on the top. Many users try tools like the loft command. They might even think they need surfacing tools. This guide shows you a simpler way. You can create this complex shape using only basic modeling commands. This method is fast and easy to edit later.
Understanding the Design Problem
You need to create a part with two separate curves. Looking from the front, the bottom of the part has a curved profile. Looking from the top, the part also has a curved profile. This creates a unique, aesthetically pleasing shape. The challenge is to build this without using surfacing or complex lofts. The goal is to use simple extrude and sketch commands.
This approach keeps your model easy to manage. It also makes future changes simple. You can adjust the curves by modifying just a few sketch dimensions.
Starting the Model: The First Curve
Begin by creating a new hybrid design. Always start by making a new component. For this demo, you can name it "demo." Your first sketch will be on the front plane. This sketch defines the front view and the bottom curve.
Draw a basic shape. Use a center rectangle. For example, set the total length to 32 inches. Set the height to 2 inches. This forms the starting block of your part.
Now, add the bottom curve. Use a three-point arc command. Place the start and end points on the bottom corners of the rectangle. Place the third point to create an arc. You need to control the depth of this curve.
To do this, add a dimension. You must dimension to the arc's tangent point, not its center. Click on the top horizontal line of the rectangle. Then, right-click and choose "tangent" from the menu. Now, click on the arc. You can set this dimension to 1 inch. This controls how deep the bottom curve is.
A helpful tip: Turn one side of the rectangle into a construction line. This makes the rectangle and the arc a single, connected profile. It makes the next step easier.
Finish the sketch. Now, extrude this profile. Set the extrusion depth to 24 inches. You now have a solid block with a curve along its bottom edge.
Adding the Second Curve on the Top
The next step is to add the curve when viewed from the top. This curve will run in a different direction than the first one.
Select the top, flat face of the extruded part. Right-click and choose "Create Sketch." You will draw on this face.
First, project the edges. Use the "Project" command and select the top face. This brings purple reference lines into your sketch. They show you the boundaries of the face.
Draw the top curve. Use the three-point arc again. Place the start point on one projected edge. Place the end point on the opposite projected edge. Place the third point somewhere above the face.
You need to add constraints to control this arc.
Make the start and end points horizontal to each other.
Make the arc coincident with the point you placed above. This pulls the arc down to touch that high point.
Your sketch is almost done. It still needs a dimension to be fully defined. Add a dimension from the arc's high point down to the line between the start and end points. Set this to 2 inches. Your sketch is now fully constrained. Finish the sketch.
You now have a curved line on the top face of your part. This line is the profile for the second curve.
Creating the Final Shape: Two Simple Methods
You have a solid block with two sketch profiles. One profile curves the bottom. The other profile curves the top. Now, you must use these sketches to cut the final shape. There are two good methods.
Method 1: The Cut Extrusion
This method uses two profiles to remove material.
Select the profile on the front face (the bottom curve).
Hold the Control key and also select the profile on the top face (the top curve).
Start the Extrude command.
Drag the extrusion downward. For the "Extent Type," choose "All." This goes through the entire part.
Make sure the operation is set to "Cut."
Click OK.
This cuts away all material outside both profiles. It leaves you with the final double-curved part.
Method 2: The Intersect Extrusion
This method uses only one profile. Many find it faster.
Select the large profile on the top face.
Start the Extrude command.
Set the "Extent Type" to "All."
Change the operation from "Cut" to "Intersect."
Click OK.
The intersect operation keeps only the 3D geometry that is inside the extrusion profile. It removes everything else. You get the same result as Method 1, but with fewer clicks.
Finishing and Editing the Model
Your main shape is complete. You can now add finishing touches like fillets. For example, add a 3-inch fillet to the side corners. Add a 0.25-inch fillet to the top and bottom edges. This gives the part a polished look.
The real power of this method is easy editing. Your model is driven by two simple sketches. You can change the entire shape by modifying a few dimensions.
To edit:
Turn on the visibility for Sketch 1 and Sketch 2.
Right-click on a sketch and choose "Show Dimensions."
Now, you can change any dimension.
Change the part width from 32 to 48 inches. It updates instantly.
Change the top curve's height from 2 to 6 inches. Watch the model change.
Change the bottom curve's depth from 1 to 2 inches. See the shape update.
This is very efficient. You do not need to redo complex surfaces or lofts. All changes happen in the sketches.
Conclusion: Why This Method Works Best
Creating a part curved in two directions does not require advanced surfacing. You can do it with basic extrudes and careful sketches. This method is perfect for users who want more control. It is also great for those who want a simple workflow.
The key benefits are:
Simplicity: You use commands you already know.
Control: You define curves with precise dimensions and constraints.
Editability: Changing the model is fast and predictable.
This technique solves a common design problem. It proves that sometimes the simplest approach is the most powerful. You can create complex, organic shapes without leaving the solid modeling workspace.
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