Replace a lost or broken battery cover using 3D printing

Introduction

 
This tutorial will help you to replace a battery cover using 3D design and 3D printing.
 
 
Finding a replacement for a battery cover can be a real nightmare. Most of the time you have to buy a whole new device, and if you can find the spare part, it is usually expensive and it takes forever to be delivered.
 
With this guide, you will be able to replace a broken or lost battery cover in a few hours at very little cost.
 
You will only need access to a calliper (or other measuring device), a designing software and a 3D printer.
 
In this guide we designed a specific battery cover but you can apply this method to many battery covers.
 

Examples of battery covers designed with this method from MyMiniFactory:
-Battery cover for Samsung remote control
-Battery cover for computer mouse

 
Let's begin!
 

Design preparation

 

In this section we are going to explain how we determined the measurements to take and the software tools to use. The design process depends on the shape of your cover, so you need to spend some time observing it.

 On this remote, we can see that the front and back section are not the same. The shapes are similar but the dimensions are different. So we should use a multi section extrusion: the loft tool on Fusion 360. We have to divide the cover into different sections and connect them to create the volume. We need to takes the measurements to draw each section.

Looking at the remote, we also notice that the cover should be curved. We need to take this curve into account when extruding the shape. We will use the loft tool with a guide line (called “center line”).

 

Part Design: the General Shape

 

To design the body of the remote, we will use the tool “loft”.

We need to:
-Divide the battery cover into different sections, measure the sections on the remote and draw them in Fusion 360. The more section you draw, the more precise is the design. In our case, the shape doesn’t change a lot so 3 sections are enough: the front section, the middle section and the back section.
-Draw the guide curve.
-Extrude the body with the loft tool.

 

Draw the sections
For each section, you can find a table with the measurements we took and how we used them to draw the sketches.

Table for the front section:

 

Drawing process:
-Select "Create sketch"
-Select XY plan
-Draw the sketch using lines and circular arcs ("Center point arc")
-Set the dimensions of the sketch
-Center the sketch (select the center of the curve and the origin, right click and select "horizontal/vertical")

Table for the middle section:

 

Drawing process:
-Create an offset plane (in "Construct" click on "Offset Plane", select the XY plane, and enter a distance of 31mm between the XY and the offset plane)
-Select "Create sketch"
-Select the offset plane
-Draw the sketch using lines and circular arcs ("Center point arc") - As we cannot take any height measurements, the curvature is an approximation of the shape observed
-Set the dimensions of the sketch
-Center the sketch

Table for the back section:

 

Drawing process:
-Create an offset plane (XY plane, 61mm)
-Select "Create sketch"
-Select the offset plane
-Draw the sketch using line and circular arc ("Center point arc") - As we cannot take any height measurements, the curvature is an approximation of the shape observed
-Set the dimensions of the sketch
-Center the sketch

 Now, we have drawn the three sketches.

Draw the guide curve
You now need to draw the curve that will guide the extrusion. It is not easy because we can’t take precise measurements of the curvature. We observed the side of the remote and tried to reproduce the curvature we saw.

Drawing process:
-Select "Create sketch"
-Select the YZ plane
-Draw the curve using "spline"

This step can take several iterations.

 We are ready for the “loft” tool.

Extrude the body

-Select the “loft” tool in the menu "Create"
-In “profiles”, select the three sketches
-In “guide type”, chose “centreline” (second icon)
-In “centreline”, select your guide curve.

 

Print and Test: the General Shape

 

Before designing the rest of the cover, we need to make sure that the body fit the device. So we are going to print it and test it.

Export your design as stl. (in the design tree right click on the body and select "save as stl").

Print it using your slicer and 3D printer.

Try it on your device.

If the shape is off, take new measurements and adjust your design. If the shape fits, you can go to the next step.

Before designing the rest of the cover, we need to make sure that the body fit the device. So we are going to print it and test it.

 

Export your design as stl. (in the design tree right click on the body and select "save as stl")

Print it using your slicer and 3D printer.

Try it on your device.

If the shape is off, take new measurements and adjust your design. If the shape fits, you can go to the next step.

 

Part Design: Clips and Feet

Now that the body of the remote is designed and fits the device, we need to add the clip and the feet.

-The feet (or rear pins) are used to align and block the cover
-The clip is used to attach the cover

The number of feet and clips can vary. In your case we had two feet and one clip.

We used the method described below because we don't have the original cover. If you still have it, take the measurements directly on the part.

Clip
The clips mechanism are usually quite standard, so we used another battery cover to design the shape. We then took measurements on the actual remote and adjusted it.

 

You can’t take all the measurements we need on the remote. So we had to guess and adjust some of them.

We were able to measure:
-The width (1)
-The position of the prong (2) & (4)
-The depth (6)

We had to guess and adjust 3, 5, 7, and 8.
3, 7 and 8 are not critical. We chose them to make the clip as strong as possible.
We also added filets where the feet connect to the body to reinforce attachment point. 

Here is a table with the measurements we took and how we used them to draw and extrude the feet.

The 3.5mm (hole width) is an estimation. We chose this value to make enough space for the clip creation.

 

Design process:
-Select "Create sketch"
-Select the YZ plane
-Draw the sketch using lines and circular arc
-Set the measurements of the sketch
-Extrude the sketch to make half of the clip
-Use the "mirror" tool to create the second half of the clip (in "Create", click on "mirror", Pattern type = new component, Objects = select the half clip you just extruded, Mirror plane = YX)
-Fuse the general shape and the clip to make only one body (in "modify", click on "combine" and select the the body and the clip).
-Add fillets (click on "modify", select "fillet" and select the edges you want to modify adding fillets)

Feet / Rear pin
Like the clips, the feet are quite standard. Most of them have the shape of an L.

 

 We were able to measure:
-The width (1)
-The depth (4)

We had to guess and adjust 2, 3, 5. As they are not critical, we chose them to make the clip as strong as possible.
We also added fillets where the feet connect to the body to reinforce attachment point.
If the two feet are symmetrical, you can design one and use the mirror tool to create the other.

Here is a table with the measurements we took and how we used them to draw and extrude the feet.

 

Design process:
-Create an offset plane (YX, 8mm)
-Select the offset plane created
-Draw the sketch
-Set the measurements of the sketch
-Extrude the sketch
-Use the "mirror" tool to create the second feet with symmetry (in "Create", click on "mirror", Pattern type = new component, Objects = select the feet you just extruded, Mirror plane = YX)
-Fuse the feet and the general shape to make only one body (in "modify", click on "combine" and select the the body and the feet).
-Add fillets

Print and Test: Clip and Feet

 

To test the clips and feet without printing the whole cover, you can cut the part with the clip or feet, print it and test it.

Cut the part you want to test.

To cut a part of your design:
-Select "Create sketch"
-Select the XZ plane
-Draw a rectangle which represent the part you want to remove
-Select "Extrude" then your sketch
-In "Operation", select "cut"
-Chose the extrusion length so it include everything you want to remove

Export your design as stl.

Print it using your slicer and 3D printer.

Try it on your device.

If it doesn’t fit and your part had overhangs. Try to clean the first layer that might be too thick.

If both the clip and the feet fits, your cover is ready. Otherwise, do the necessary adjustments.

 

 

Preparation of Printing / Conclusion

 

After the design comes the 3D printing time. It is the most fascinating part to me: when your project come to life.

You have tested separately the body, the clip and the feet and they all fit. So your cover should be working.

Export the full design in stl and print it.

You can print the part in PLA as we don't need specific mechanical properties.

For our cover, the best printing orientation was with the feet touching the platform (we had to use support). If your cover is different, the best orientation might change. Try to limit the support but keep in mind that the clip and feet have to be as precise as possible.

Test it on your device.

Congratulation, you have a functional battery cover for your device.
 
 
Now share it on MyMiniFactory!