Replace a Lost or Broken Battery Cover Using 3D Printing

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Introduction: Replace a Lost or Broken Battery Cover Using 3D Printing

This Instructable 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.

If one of the step is not clear, you can watch the video of the full design (step 8).

Interested links

Examples of battery covers designed with this method from MyMiniFactory:

Don’t hesitate to make a comment or ask us a question at the end of the page, we will be happy to answer you.

Step 1: The Tools

For this tutorial, we designed and printed a battery cover for a Polycom remote control (link). We lost the battery cover on this one, so we had to design it using info from the remote. It is faster if you have the original cover.

To design the part, you need to take several precise measurements of the remote. The most suitable tool is a calliper.

You also need a computer with a 3D design software. In our case, we used Fusion 360 (free for students and hobbyist). But you can use other CAD software like Solidworks, Catia, Inventor, FreeCAD…

Finally, you need a 3D printer, its slicer and some printing material.

Tools summary:
-a remote control or other device with a battery cover
-if you still have it, the battery cover of your device
-a calliper or another tool to measure
-a computer with a 3D design software (like Fusion 360)
-a 3D printer (with a slicer and 3D printing material)

Let's begin !

Step 2: 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”).

Every cover is different so the design process and the tools used can vary. If your cover has different features than this one, check this webpage (https://www.myminifactory.com/pages/battery_cover_help) and adapt the following method to your part.

Step 3: 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.

    Step 4: 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.

    Step 5: 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

    Step 6: 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.

    Step 7: 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!

    Step 8: Full Design Video

    If one (or several) of the steps were not clear, here is a video of the full design of the part with fusion 360.

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      1 Questions

      Would you make a replacement cover for my “Tens” stim device used for my back. Hum understand this was for instructional purposes but could really use the help.
      Thank you

      Yes, with pleasure !!

      I can design your part, print it (to check measurements) and send you the STL file.

      You can contact me on my email address : corentin@myminifactory.com
      Could you send me some pictures of your cover (on my email)? Perhaps I will ask you measurements and let's go for design !

      11 Comments

      OK. And where can I access a 3D printer at low or no cost?

      Try your local library first! It seems to be something libraries in the US are adding, try there first. My local library just asks you to pay for the plastic used in the print.

      Try to find a makerspace near you. Many of them offer printing services and even lessons.

      I built two for someone else and now they are letting me use one. That works for me. :-)

      Like a genius! have my vote!

      One of the reasons bought my Prusa 3D printer was to encourage/allow me to re-make broken parts around the house and workshop.

      This comprehensive instructable will be of great assistance and will put me further up the learning curve with Fusion 360.

      Thank you for your great instruction. I actually built a couple of 3D printers for our local university but had never got to use one or the software. this just may inspire me to get on with it. Thanks again. Terrific job.

      This is brilliant, I thought of doing this when my 3D printer comes! great post :) voted for you!

      Excellent explanations! Thank you for sharing!

      I still mostly feel like a fish out of water when designing things with tight tolerances like this, but you make it look so effortless. Need to up my game! :)