How to create Grooved Surfaces
The Question
A customer reached out to me asking how to create "grooves" that ran along an axis of a part. I will explain a couple of different methods on how you could approach this.
Using the Pipe Command
The Pipe command creates a shape along a path. Select the part’s outside profile, then set the section size to 0.06. The preview shows the circular profile moving along the path and cutting the part.
Set the operation to Join when the pipe should become part of the model. Choose New Body when you want to keep it separate.
Pipe also supports three section shapes:
Circular
Square
Triangular
The circular shape is used most often in this example.
Build a Center Path with Midplane and Project Intersect
The first simple part needs a path through its center. In this example, the Origin sits off to the side instead of near the middle of the part.
Open the Construct menu and select Midplane. Pick the left side and right side of the part. Fusion creates a plane that cuts through the middle.
Grab a corner of the new plane to enlarge it if needed. The plane now clearly slices through the entire part.
Preselect the midplane and choose Create Sketch. Rotate to an isometric view so the intersection is easier to see.
Use Project Intersect. Its default selection filter is Specified Entities, which requires you to select individual faces. Hovering over a fillet shows where that face intersects the sketch plane, but a model with many faces would take time to select manually.
Change the selection filter to Bodies. Hover over the body to project its full intersection onto the sketch plane. Fusion creates a line wherever the body crosses the plane. This produces the same path as the outside profile, but places it directly through the center.
Pattern the Pipe Feature with 0.065 Spacing
Run Pipe again using the projected center path. Set the section size to 0.06 and choose Join.
Because the part has the same shape across its length, use the Pattern command. Change the object selection from Bodies to Features, then select the Pipe feature from the timeline.
The pattern needs an axis. You can select a horizontal line or an axis from the Origin. Drag the preview to see the result.
Change the distribution from Extent to Spacing. The circular section has a diameter of 0.06. A spacing of 0.06 makes the pipes touch, so use 0.065 to create a small gap, if that is what you prefer.
The pattern initially moves in only one direction. Change the direction from One Direction to Symmetric. Increase the quantity to 30, then set it to 31 to reach the edge of the part.
Fusion can create the repeated groove pattern quickly with this process.
Use Sweep for a Custom-Shaped Texture
The Pipe command limits the profile to a circular, square, or triangular shape. To make a custom profile, turn the sketch back on and create a plane along a path. Place the plane on a straight segment of the part, then create a sketch on it.
Draw any profile you want. The example in the video uses a eliptical profile. Make one point coincident with the matching point on the path, then finish the sketch.
Use the Sweep command. Select the custom sketch as the profile and the existing line as the path. Set the operation to Join.
Pattern the Sweep feature using the same axes as the Pipe example. Drag the preview to check the result. No measurements were taken for this example, so the correct spacing would need to be determined separately.
The example starts with a quantity of 30, changes the pattern to Symmetric, and then tries 40. The result creates a comb-like texture. This method can carry any chosen profile along the surface.
Create Paths for a Complex Recessed Part
The more complex part contains recesses and walls. A path through the center changes when it reaches those walls. One option would be to create three separate paths, moving from the center to a wall and then creating additional paths for the next wall sections.
That approach can work, but it takes time. An offset plane and Project to Surface can create the paths more efficiently.
Pattern Lines on an Offset Plane
Create an offset plane and lift it away from the part by a random distance. The exact distance does not matter for this setup.
Create a sketch on the offset plane. Project the body into the sketch, makin sure to change the selection to Body so Fusion projects the entire outline.
Draw a line through the center of the projected outline. Let the line snap near the center, then extend each end slightly beyond the sides of the part. The example exaggerates the ends to make the setup easier to see.
Create a Rectangular Pattern inside the sketch. Sketch patterns are not normally used in this way, but this case needs one. Select the line as the pattern object and drag to set the direction.
Set the spacing to 0.065, and choose Symmetric. When the quantity increases, the spacing does not change because the distribution is still set to Extent.
Change the distribution to Spacing, then set the spacing back to 0.065. Increase the quantity to 30, then set it to 31. The sketch now contains lines arranged symmetrically from the center.
Project the Pattern with Project to Surface and Along Vector
Create another sketch on any plane or face. In the example, the front face is selected, and the view is rotated to isometric.
Use Project to Surface. First, select the faces by drawing a box around the part. Next, select the curves with a crossing selection that includes only the patterned lines. The overall body outline may also become selected if the crossing area is too large.
The default projection type is Closest Point. This wraps the lines around the highest point of the part.
Change the projection type to Along Vector. Fusion then asks for a projection direction. Select the Z axis, shown as the vertical blue line in the Origin.
The straight lines now project directly down along the Z axis. They wrap into the recessed area, across the fillets, and down the straight walls.
After the projection, two sketches remain. Turn off Sketch 4, since it is no longer needed. The projected paths on Sketch 5 are ready for the repeated Pipe features.
Use Autodesk Assistant for Multiple Pipe Paths
The complex setup exposes a limitation in Pipe. The command asks for Path, not Paths, so it accepts only one path at a time. Holding the Control key does not allow additional paths to be selected.
The manual process would be repetitive. Turn on the sketch, select a path, run Pipe, set the size to 0.06, choose Join, and accept the feature. Repeat those steps for every single path.
Instead of that manual work, let's use Autodesk Assistant for the repeated operation. The command used is:
Use the pipe command to create a 0.06in diameter pipe on all of the sketch loop profiles on sketch 5.
Autodesk Assistant takes just under a minute to create the Pipe features along all the sketch profiles.
The new pipes appear as separate bodies. Keeping them separate makes it possible to inspect the result and remove unwanted geometry. In the example, one extra pipe is not needed. We will remove it.
Use Combine to return to one body. Select the main part as the target, select all the remaining pipe bodies as the tools, and choose Join. Fusion combines the geometry into one singular body.
Conclusion
This was just two ways you could go about creating a "textured" surface on a part. Experiment with the process and see what you come up with!
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