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Bike Fender Part 4: Multi-Part Design
Advanced 3D Printing Class
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Using the basic shape from the previous lesson, I designed a couple of quick iterations with smoothed edges and interlocking parts. Remember that design is an iterative process, so you should never expect your first pass at a design to be perfect.

This class aims to help you develop the skills you need to make whatever you want. We're using the bike fender as an example project to teach you skills and tools that are useful for lots of different things.

Take the skills taught here, and make any project you like.

In this lesson, we're going to skip ahead to the final version of the design.


Version 1 is more graceful and slim


Version 1 is more flexible


Version 2 is more bulky and boxy


Version 2 is less flexible

Having done a couple of iterations of the design and test printed them, I can make some final decisions about the piece. Comparing the two clamp pieces in these photos, I like the narrower one (version 1) better from an aesthetic point of view. It's more graceful than the wider one (version 2), and the smoother curved surfaces are reminiscent of speed and streamlining, which is perfect for a bike from a conceptual point of view.

Version 1 flexes much more than version 2. This means it'll be easier to get it on and off of the seat post, but by nature, it won't be as strong as version 2. Version 2 has a solid wall where version 1 only has a 6mm deep member where it meets the upper piece.

The cutouts in the sides of version 2 help to reduce the amount of material used while keeping the structure strong, but since the whole purpose of the design is to prevent splashing, I think it's best to go with solid walls for the parts.


Design Decisions Based on Version 1

Version 1

In general, I wasn’t happy with the way the first version turned out. It was too bulky and didn’t match the slender profile of the saddle and the bike in general. I did a second iteration that was a bit closer to what I had in mind, but I made the mistake of making it too wide to fit on the printer. For the final design, I’ll match the profile I created in this second iteration and make a new piece that’s narrower.


Sketch > Create Sketch


Sketch new side profile based on first iteration

I create a sketch in the side plane and project existing geometry that’s going to help me match the side profile I already know I like.


Create > Extrude (Symmetrical)


New (thinner) mass

With the basic profile worked out, I extrude the mass using the symmetrical direction by 75mm, giving me an overall width of 150mm.


Create General Shape

With the base mass in place representing the side profile, it’s time to start working on the top-bottom profile.

Sketch on underside for clamp features

First, I create a sketch on the underside of the clamp part, then sketch out the sleeve thickness and the lines I’ll use to extrude the split in the clamp feature.


3-point construction planes match version 1


Modify > Split Body

I turn on the previous version of the fender as a reference. I want to keep the width of the clamp the same as it was in the previous version, so to cut the mass I create a 3-point plane from the Construct menu on both sides.


3-point construction planes match version 1


Split body to create slimmer profile

I use the mass I just made to provide the first two points (at the kink), then I use a point on the side of the previous version of the clamp to complete the plane.

With my two planes in place, I use the Split Body tool in the Modify menu. I repeat the same steps to create the tapered profile on the back end of my new mass.

Base form complete!


Refine General Shape

Now that I have my general shape worked out, I can continue refining the piece.

New slimmer profile sketched on bottom


Construction planes based on new sketch


Modify > Split Body

New slimmer profile

I Create a sketch in the bottom of the clamp feature and add a new, narrower profile by projecting geometry from the existing mass. I create 3-point construction planes again, use the Split Body tool, making the base of the clamp just wide enough to fit within my parameters.

Clamp feature details sketched on underside of clamp part

I create profiles on the top and bottom of the clamp feature because I’m not sure yet how I want to create the final profile of the clamp part. I might want to loft between the two profiles or extrude- I’ll have sketches to experiment with either way.

Profile extruded to create clamp features

I use the Extrude tool to add features like screw and nut pockets, tabs, and the split in the clamp.

{
    "id": "quiz-1",
    "question": "Why does the clamp have a split in it?",
    "answers": [
        {
            "title": "Because the clamp needs to be easily attached to the seat post.",
            "correct": true
        },
        {
            "title": "To keep it from warping while it's being printed.",
            "correct": false
        },
        {
            "title": "Because it looks better that way.",
            "correct": false
        }
    ],
    "correctNotice": "You got it!",
    "incorrectNotice": "Nope!"
}

Create Wall Thickness

I know I want a consistent wall thickness for the whole piece. There are a couple of different ways to make this work.

Top profile sketch with 6mm offset sides

First, I create a sketch on the top profile of the clamp part with a 6mm offset from the outside edge.


Bottom profile sketch


Create > Loft (cut operation)

Then, using the profile on the bottom of the part, I can create a loft between the two profiles.

This gives me a consistent 6mm wall for the clamp part.


Create Hardware Pockets

I need a way to insert the machine screw into the clamp feature. It’s tight in there and I want to avoid a hole in the side of the piece if I can.


Sketch matches side profile of screw


Sketch extruded to create cavity

I create a sketch parallel to the back end of the clamp feature, then extrude a profile that’s the same size as the screw from the side. This gives me a cavity I should be able to use to wiggle the screw into place.

Modify > Fillet to round edge of cavity

I use the Fillet tool to make a rounded edge for the cutout I just made. This will make it easier to get the screw in and will make the piece more durable in the long term- sharp edges tend to chip and break eventually with just about any material.

Move > Rotate to test clearance

To test my design, I turn the screw on in the browser, then move it around a bit to see if I can get it into place with the cutout.


Create the Clamp Wall

My clamp needs a wall to align with the vertical part that attaches to it. To create this feature, I’m going to use the loft tool and keep the wall aligned with the kinks in the sides of the clamp.


Draw centerline between points


Offset in both directions by "t/2"

To loft, I need to create two sketches in different planes, so I start with a line connecting the two points representing the kinks, then offset from there by 1/2 of my thickness parameter, “t”.

Select centerline > Right-Click > Normal / Construction

I don't want two profiles on this sketch, so I select the centerline, right-click, and select Normal / Construction to give myself a single profile.

Repeat for bottom profile

In the bottom profile, I project the points that represent the bottoms of the kinks, then do the same offset operation I did in the last profile. This centerline also gets switched to Construction to make for a single profile.

Create > Loft (Join operation)

With two profile sketches of the correct width in two planes, I use the loft tool and select the “join” operation. This will create the wall I need for stability on the clamp part.

Modify > Fillet

With the wall in place, I fillet the inside corners of the clamp feature. I'm going to avoid sharp corners wherever possible, so in general I fillet edges as I go through the modeling process.


Sketch hole profile on wall


Hole profile on opposite side of wall

I want to hollow out the wall because it will save material and make it easier for the clamp to flex. Notice I’m still using the “t” thickness parameter for the offset here. Consistency means clarity!

Create > Loft (Cut operation)

I use the loft tool again to create this hole to ensure that my wall thicknesses and depths are consistent everywhere.

Modify > Fillet

I fillet these inside corners as well to avoid sharp edges. I use "t" or some multiple of "t" pretty much everywhere in the model. This ensures that if I change my mind about thickness later, I can update that parameter without worrying about it breaking the model.

{
    "id": "quiz-1",
    "question": "What's the point of using parameters instead of numbers?",
    "answers": [
        {
            "title": "It's easier than doing math.",
            "correct": false
        },
        {
            "title": "It's faster than typing multiple numbers.",
            "correct": false
        },
        {
            "title": "It makes it possible to easily change the whole design later.",
            "correct": true
        }
    ],
    "correctNotice": "You got it!",
    "incorrectNotice": "Nope!"
}

Create Fender Shells

Modify > Split Body

This design has to be made in multiple parts, so I use a 3-point construction plane to split the vertical part from the end part.

Modify > Shell

I select the 3 planes on the underside of the fender and use the Shell tool. Again, I use the “t” thickness parameter.


Modify > Fillet


Fillet outside to maintain thickness

I fillet the inside and outside edges of the bend in the vertical part to match the fillet I made on the inside of the clamp part.

Fillet clamp sides to match

To smooth out the kink in the side of the clamp part, I adjust the fillet radius by eyeballing it. These angles are different so I’m just adjusting the radius so that the lines match up.


Modify > Fillet


Fillet outside to maintain thickness

Finally, I repeat the shell and fillet operations on the end part of the fender assembly. I have to eyeball the upper fillet radius again because of the difference in angles.


Refine Design for Printing

Before I go any further, I need to check and make sure my design will fit in the printer’s build envelope in 3 parts. To do this, I use the Measure tool in the Inspect menu and select the longest edge on my biggest part, the fender end.


Construct > Offset Plane


Modify > Split Body

I see that it’s about 248mm long, and a quick glance at the printer’s specs tells me my maximum width is 230. This means I need to cut down the length of my end if I want it to fit in one piece.

I offset a construction plane from the end of the part by 20mm, which gives me a length of about 228mm, which will fit within the build envelope. I use the Split Body tool with the construction plane.

Modify > Fillet

I use the fillet tool on the corners of the fender end and the clamp part to get a rounded profile.


Select > Right-Click > Break Link


Sketch > Fillet

Sketch > Fillet

The sharp corner at the seam between the vertical part and the end part bugs me, so I create sketches on the side planes to make a rounded seam. I want to use the line I projected from the end part in my sketch, so I select the line, right-click, and select Break Link so that I can edit the line.

Create > Loft (New Body operation)


Separate body for later use


Create > Loft (New Body operation)

I use the profiles I just created to make new bodies using the loft tool. When I loft this time, I use the New Body operation.

Create > Mirror

There’s no point in creating these sketches a second time for the other side, so I just take the new bodies and mirror them along the center plane of the model.

Modify > Combine

With the new bodies in place, I use the Combine tool in the Modify menu to create monolithic pieces. The Combine tool allows you to add, subtract, or intersect parts that are touching or crossing.


Modify > Fillet (big radius for sharp corners)


Modify > Fillet (small radius for all edges)

Modify > Fillet (match radius of other filleted edges)

Now that I’ve got my basic forms in place, it’s time to start filleting all the sharp edges. I use “t/2”, which equals 3mm for the corners, and "t/4” which equals 1.5mm for the edges. Of course, I could use number values here, but if I want to change the thickness of the whole model by changing the “t” parameter, the proportions of all the parts will stay consistent.


Fitting Features

My clamp part attaches to the seat post with screws and nuts because it’s not a permanent attachment on the bike. The other parts don’t need to be disassembled from each other though, so I’m going to add some fitting features that will keep them in place while I epoxy them together later.

I’m just going to make a simple ridge / trough connection for these parts.


Sketch ridge profile


Extrude by "t/2"

I start by creating a sketch on the flat connection surface on the vertical part, then offsetting the lines. I don’t want to go any thinner than 1mm with the width of the wall because I’m worried it will break off easily. I extrude this profile by "t/2" or 3mm. This ridge / connection isn't doing much structurally speaking, just giving me a feature to align the parts.

Fillet edges for easy fit


Offset female profile by .25mm


Extrude into lower part, cut operation

Next, I create another sketch on the clamp part to create the trough. I project the geometry of the ridge onto this new sketch, then offset the profile by +.25mm. I know this is the clearance I need from the fit test piece I made before.

Fillet edges for smooth fit

I fillet all these edges to ensure a perfect fit. Sometimes with sharp edges, distortions in the plastic due to heat can become a problem for parts that need to fit together. With that profile finished, I extrude into the clamp part by "t/2” as well. This edge also gets a small fillet to ensure a perfect fit.


Print Parts

We've been through the printing process before, so here's a quick recap of how it's done step-by-step.

1. Export the three bodies of the fender assembly separately as STL files.

2. Open Simplify 3D and import the parts one-at-a-time. Double-click on the part to open the modify window so you can rotate and place the part.

3. Go Place Surface on Bed in the Edit menu and click the top surface of the part to get the proper placement. Double-click the part to get the Move / Rotate / Scale controls, and rotate Z by 90º.

4. Go to Edit > Place Surface on Bed and click one of the facets that's in plane with the bottom of the model.

5. In Edit Process Settings, increase the Infill Percentage to make the part more robust.

6. Click Prepare to Print for a full preview of the tool path.

7. Click Save Toolpaths to Disk for a .g3drem file that can be put on the Dremel’s SD card for printing.


Recap

In this lesson, we concluded the Bike Fender project by executing the final iteration of the design. We used a previous iteration as a guide for the overall form of the final design, integrated hardware, created features to allow us to insert the hardware, and designed fitting features to make assembly easy once the parts are printed.

What next?

If you want to learn about some useful finishing techniques, check out my follow-up instructable, 3D Print Finishing.

We hope you've enjoyed this 3D printing class series and that you'll keep going with digital design and fabrication. If you want to round out your high tech skill set, I'd suggest moving on to the Laser Cutting Class, the CNC Class, and the 3D Scanning Class.

CLASS PROJECT

Share a photo of your finished project with the class!

Nice work! You've completed the class project