From scan to CAD. Two ways using MIRACO

I’ve broken these posts out from my showcase thread so that they are more easily found for those who are interested in how to do this. In the next two posts I will go through two ways you can go from scan to CAD. One is a quick and dirty method if you want to fit something to something else, the other is more involved and mainly for reverse engineering.

So, without further ado, let’s start with the quick and dirty method.
What we’re going to do is create a quad-mesh from our scan and then use the quad-mesh to surface conversion tool to make a brep editable solid in Fusion 360.

The controller for my drone (DJI Mini 4 Pro) only has mounts for a neck-strap at the rear.

This means it flops forward when not supported. I would like a way to hold it at it’s center of mass.


There are trays that mount to the controller but they increase it’s bulk quite considerably. Ideally I want something that mounts a strap here:

In order to create the part, we first need to create a scan of the DJI RC2 controller. It doesn’t need to be mega-detailed but we might as well show off Miraco while we’re doing it:

Getting it in to CAD
There are several ways we can get this model in to CAD. We could re-draw it from section sketches like I’ve shown before but for this project, we’ll use a different way.

Triangles to quads
I want to create a T-spline model of the controller in Fusion360. Unfortunately, the mesh to T-spline converter can only deal with quad meshes and the output of Revoscan (and all other scanning tools really) is triangles. We can covert the model to quads using a nice, free tool called Instant Meshes: GitHub - wjakob/instant-meshes: Interactive field-aligned mesh generator

Let’s load up our scan; click Open Mesh:

Our mesh is loaded and ready for conversion:

At the moment, our target vertex count is way too high at 100k. Fusion360 will have a fit. We want that around the 10k mark ideally. Move the slider to 10k:

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Next, hit Solve under Orientation Field

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Our mesh will have lots of pretty colours on it now.

Then, hit Solve under Position Field

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And now our mesh is all squares. Squares are good:

Hit Export and choose Pure quad mesh (this will ensure that all the facets are quads and that no triangles remain.

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Finally, Extract Mesh

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And save

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Now, over the Fusion360:
Create a new project, import your quad-mesh and orientate it so that it’s aligned with X, Y, and Z.

Next, under the surface tab, select New Form

Then hit Convert

We want Quad-mesh to T-Spline

Hit OK, and Fusion will chew on it for a while, then hit Finish Form

We now have a defined solid in Fusion that we can do all sorts of things with:

As you can see, we can cut it up just like a normal solid

OK, back together we want to make a copy of it

The new object, we want to scale it to make it bigger. I want something that will fit around the controller but follow the controllers lines. Let’s make it 1.1x bigger. Make sure to scale from the origin rather than a corner.

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Now, let’s cut it up and make the rough model that we want:

Now we have our rough model, let’s put it over the 1.0 scaled original model and then use that model as a tool to cut out from our new part:

We end up with this, ready for an attachment to be added:

A quick bit of CAD and we have our part:

This is what it looks like rendered in Fusion:

Let’s print it and see how it fits:

Like a glove:

Perfect. Exactly what we want.


Method two is more involved but much more accurate. This will get us a sub-mm accurate copy of our object that we can edit if we want to. This method is much more time consuming though.

What we’re going to do is import the mesh in the Fusion360 and then create section sketches through it to create profiles. We can then use these sketches to extrude our final model.

Let’s start. I want to replicate this object but the tolerances are pretty tight and the thread has to be accurate. A simple scan might suffice but I might want to edit it slightly.

Scanned in using Miraco

Over to Fusion 360. Let’s import the mesh and align it to X, Y and Z.

Create a mesh selection sketch


This has created a section through our object. But way, we can’t extrude from it yet. We need to fit lines to those sections.
Edit the sketch and use Fit Curves


We can draw lines, arcs, splines, circles to fit to our section.

Looks good. Back to the solid workspace, select the sketch and hit revolve.


Check it agrees with the mesh

Create another section sketch to capture the indentations

I’ve made it as a primitive here

Make a circular pattern of the new object


We want 8 indentations

Use the object as a cut tool to form the indentations

And fillet them

Make the threads - I measured these as 1" BSP threads

And here’s our finished model, ready for modification. Miraco has enabled us to replicate the object.

Let’s print it and see if it works. Looks good but does it fit?



thank you for these helpful tutorials! there actually is another great one from you I know about and I think it is good to have a link posted to it, too. I hope that is fine with you.

Great tutorials Andy ! Thanks for sharing !