Knurl

SolidWorks Tips and Tricks sponsored by SolidWorks for the Sheet Metal Guy

 

Ever Need to Create a Knurl?

Knurled surfaces are very common in engineering design. However truly modeling a knurled solid feature takes up a lot of memory and slows down SolidWorks, especially with multiple knurled parts in your assembly. A couple other ways of dealing with a knurl is to apply a texture to the face or to add a crosshatch pattern in the drawing to make it look like a knurled surface.

 

With that said, the easiest way to add a knurl is to apply a texture to the face. SolidWorks has two knurled textures that you can add to the part to make it look like it is knurled. To apply a texture, pull down the “Edit” menu and pick Appearance – Texture. Pick the face in the graphics area that you want to apply the texture to, and then, in the Texture PropertyManager, under Texture Selection, pick Metal – Machined – Knurl 1 or Knurl 2, as shown in Figure 1.

 


Figure 1

 

Now, here’s how to physically create a knurl feature. Create a sketch of a 50mm circle centered at the origin on the Front plane. Next, extrude the sketch 50mm. Pull down the “Insert” menu and pick Reference Geometry – Axis. Pick the cylindrical face in the graphics area, and then, pick OK.

 

Figure 2

 

Start a sketch on the front face and create the square shown in Figure 3. The construction lines are used to constrain the square. It’s important that the points of the square are coincident to the circle.

 

   

Figure 3

 

Pull down the “Insert” menu and pick Curve – Helix/Spiral. Pick the front face in the graphics area, and then, pick the outside circle and pick Convert Entities from the “Sketch” toolbar. Exit the sketch, and enter the values in the Helix/SpiralPropertyManager, as shown in Figure 4.

 

   
Figure 4

 

After clicking OK, click Sweep Cut from the “Features” toolbar, or pull down the “Insert” menu and pick Cut – Sweep. Pick your square sketch for the Profile and the helix for the Path, as shown in Figure 5. Click OK.

 

Figure 5

 

Click Circular Pattern from the “Features” toolbar, or pull down the “Insert” menu and pick Pattern/Mirror – Circular Pattern. Pick Axis1 from the flyout FeatureManager design tree for the Pattern Axis. Set the Number of Instances to ‘36‘. Make sure that the Total Angle is set to 360 and that Equal spacing is checked, and click OK.

 

Figure 6

 

Now all you have to do is to mirror the pattern by clicking on Mirror from the “Features” toolbar, or pulling down the “Insert” menu and picking Pattern/Mirror – Mirror. For the Mirror Face/Plane, pick the Right plane from the flyout FeatureManager design tree. Pick the circular pattern for the Features to Mirror, and click OK.

 

Figure 7

 

To clean up the edges of the front and the back of the part, add a sketch on the Right plane, as shown in Figure 8. Exit the sketch and click Revolved Cut from the “Features” toolbar, or pull down the “Insert” menu and pick Cut – Revolve. For the Axis of Revolution, pick Axis1 from the flyout FeatureManager design tree. Click OK.

 

Figure 8

Figure 9

And there you have it, a knurled feature. But as you may have noticed, SolidWorks takes some time to complete these operations.

 

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