2021 Convert STL in Fusion 360 Tutorial
This workflow was released near the end of 2021 and still works the same. Yes, even in 2022! 😉
2019 Convert STL in Fusion 360 Tutorial
Please watch the video above for the most recent workflow to convert your STL files using Autodesk Fusion 360.
Thingiverse Demo Files
Here are the two Thingiverse files that I used in this tutorial. Special thanks to the following creators for originally uploading them.
File #1 – Hinged Box by zibi36
File #2 Fish Pen Pot by HEJHEJ
Split STL and Solid Files into Smaller Pieces
By the end of this tutorial, you’ll know how to use Fusion 360 to turn an STL or OBJ mesh file into a solid body. I’ll also be showing you several different tricks to help clean up your files after the conversion. I do have another tutorial where I covered similar steps, however, not only will this tutorial be updated to reflect the most recent UI changes, but I’ll also be sharing a few extra tricks.
You likely found this tutorial searching for steps to convert your STL files to a solid body. Many of you will find something you like on Thingiverse, or a similar website, with the intention to alter it before 3D printing. For this demo, I’m going to use two different Thingiverse files, which I’ll link to on this tutorial’s resource page at ProductDesignOnline.com/15… that’s ProductDesignOnline.com/15 [one – five].
The first Thingiverse file we’ll convert is this hinged box that I’ve linked to on my web page along with credit to the original author. This box is fairly simple, and I’ll use it to cover the overall process. Then, we’ll use a more complicated object, to cover common problems you may encounter, as well as some additional tips and tricks.
Once the file is downloaded, there are two ways that we can get the file into Fusion 360. The first option would be to upload the file in the data panel or the Fusion 360 hub.
I’ll click on the data panel icon in the upper lefthand corner. From here, we would need to select the blue upload button to select the STL file from our local machine.
The second method, which is quicker and more efficient, would be to use the insert mesh command. If I select the “insert” dropdown list, you’ll notice that we have an “Insert Mesh” option. The Insert Mesh feature will work with both STL and OBJ files. Additionally, you can access the insert mesh command from the shortcuts box, which is opened with the Keyboard shortcut letter “S,” as in Sierra.
After selecting the “Insert Mesh” command, your computer’s local folders will open up, where you’ll have to select the file from your hard drive. I’ll navigate to my downloads folder and then I’ll select the box STL file.
The reason I prefer this “Insert Mesh” option over the upload option, is the fact that we can now define the position of the model all within the Insert Mesh dialog.
Let’s take a look at all of the available options.
First, you’ll see that we can set the unit type. This is important to ensure that your model comes out the right size. You’ll want to double-check the file’s dimensions before you go to 3D print the file. You may even have to check the file’s Thingiverse page to see what units the original creator used.
Second, you’ll see that we have the “Flip-Up Direction” button. This button simply lets us flip the up direction from the “Y” axis being up to the “Z” axis being up. As in, we’re changing the direction of the model, not the orientation of our file or viewcube. This can be helpful if the original author modeled the file in the other orientation.
I’m now going to hit the eyeball icon next to the “Origin” folder, in the Fusion 360 browser. Looking at this mesh file, we can now see that its center point is not aligned with the center origin point of our file. This may or may not be important with your project. However, if you do need to fix this, then you can simply click the “center” button in the Insert Mesh dialog.
You’ll notice the model’s center point is now aligned to the center of the file.
Just below the center option is the button, “Move to Ground”. The model is currently centered on the origin point in all directions. I’ll look at the model from the front face of the viewcube so we can take a look at what happens. If I now click the “move to ground” button, you’ll see that the file snaps to the ground or the XY origin plane.
It’s important to note, that it will snap based on the lowest point of the model. This model has a nice flat base, but if you have any objects protruding out the bottom then those will be referenced first.
The last button that we have here is the “Reset Transformation” button. This will reset any changes that you’ve made and it will place the mesh file into the original imported location. If I select this, you’ll see the model is now away from our center origin point, as I originally pointed out.
Last but not least, you’ll see that you can toggle open the Numerical Inputs section, which allows you to define exact distances. This isn’t used all the time, which is why it’s closed by default. However, this can come in handy if you need to move the imported model around a pre-existing model or to a specified distance away from the origin point if the model will be inserted into a larger assembly file.
For now, I’ll click the “Center” and “Move to Ground” buttons and I’ll click “OK.”
Now that we have our imported mesh file, we’re ready to convert it to a solid BRep body. Then, I’ll show you a few ways to clean up the file’s mesh triangles.
For now, we can turn off the visibility of the origin folder by selecting the eyeball icon, in the Browser.
I’ll toggle open the “bodies” folder so we can work with the mesh body. If I right-click on the Mesh body, you’ll see that the option to convert the “Mesh to BRep” is currently not available. This is because we have to first turn off the design history, as mesh files are written in a format that Fusion 360 cannot process and record the steps in the timeline below.
I’ll right-click on the file name or the top-level assembly in the Fusion 360 Browser. You’ll then see at the very bottom of the list we have an option titled, “Do not Capture Design History”.
After selecting the option you’ll get a warning that “all design history will be removed and further operations will not be captured in the timeline”.
Watch what happens to the timeline as I click the blue “Continue” button.
Our timeline disappears, as we’re no longer recording the history of this design. We can now right-click on the mesh body again. This time, you’ll see the option “Mesh to BRep”.
The Mesh to BRep dialog will then open up, where we can choose to create a new component or a new body.
I’ll leave this set to “new body,” and I’ll click “OK” to convert the file.
You’ll notice this file converted very quickly, without any latency. The time it takes to convert your file depends on the size of the file or how many mesh triangles it’s made of. We’ll take a look at a more complex file later on, which will take much longer to convert.
In the bodies folder, we now have a solid body, along with the original mesh file that is automatically hidden after the conversion. If you’re certain that you no longer need to reference the mesh body then you can right-click on the mesh body and select the “delete” option, which will permanently delete the mesh body.
Let’s now take a look at some tricks to help clean up a converted STL file.
You may be wondering why your file has all these lines running across it. In short, stereolithography, or STL files, are made up of triangular facets. Each facet is created with three points representing the vertices of the triangle, along with a perpendicular direction.
Once we convert the file to a solid body, the small triangle facets will remain on the exterior surface of the shape. The conversion process essentially fills the exterior boundaries, making it a solid body.
This brings me to one key problem that you may face while converting mesh files. If you ever go to convert a file with the mesh to BREP command and end up with a surface body, then that means you have a hole or multiple holes somewhere around the model, which prevents the exterior facets from being filled. In such cases, you would have to use the surface tools to patch the holes, which I’ll be showing you a few tricks on in just a bit.
The first method and simplest way to start to clean up converted files would be to simply select a face and then hit the delete key on your keyboard.
I’ll select one of the large triangles in the lid of the box. Watch what happens as I hit the delete key. Fusion 360 will attempt to self repair the face, which, if successful, results in one solid face. The key thing here is that the facets need to be on flat planes. I’ll talk about curved surfaces in just a minute.
If I spend a few minutes just deleting one face at a time and letting it self repair, you’ll see I will end up with some pretty good results.
The problem with converting STL files always begins with the curvature of designs. Even this simple box shape has curvature on all of its rounded edges.
Lets first try to delete some of the faces of a corner. I’ll hold the shift key and I’ll select a few faces that make up this corner. Once selected, I’ll hit the delete key.
You’ll notice that the faces of curvature don’t self-repair very well. I’m going to hit the undo command so I can show you a neat trick. Watch what happens as I repeat these steps while under the surface tab.
After selecting the surface tab I’ll select a few of the corner faces again. Then, I’ll hit the delete key.
You’ll notice that our faces were deleted this time, as Fusion 360 still isn’t able to self-repair this curvature. Because some of our faces are now missing, we’ll end up with a surface body instead of a solid body, as I mentioned a minute ago.
At this point, we can revert the previous step and try to alter the solid body differently or we can proceed by repairing the surface body.
Let’s look at a few tricks to repairing the surface body, as I’ve found this is often the better route to take.
I want to first delete the rest of these facets that make up the corner. To select them all I’m going to click the “Select” dropdown menu and I’ll find the selection priority flyout folder. I’ll click the “Select Face Priority” option so I can only select faces.
I’ll also look at the “selection filters” to make sure the “select through” option is turned off. This will ensure that we don’t accidentally select faces on the other side of our mouse click.
I’m also going to use the paint selection option, so we can paint or drag the mouse over all of the faces, allowing us to quickly select them. In scenarios like this, I like to click on the closest face that I’m going to keep, or in this case the large face on the right.
Then, simply drag the mouse or paint over all of the faces to select them. Now we don’t want to delete the large face on the right, I simply used that as a starting point to ensure that I selected everything. We’ll need to hold down the shift key to deselect that face.
I can now hit the delete key to delete all of the facets. What we now want to do is figure out the easiest method to recreate a rounded surface to patch this hole.
Because we’re working with a surface model, you’ll want to work with the surfacing tools, which are all nested in the new Surface tab. If you’re new to Fusion 360 then you can remember this by looking at the color of the tools. You’ll notice the orange surface tools correlate to the orange surface body in the Browser.
The first trick I always try is the patch command, which lets us patch openings of surfaces. I’ll select the patch command in the toolbar and then I’m going to select the hole that we need to patch. Notice how it selects the entire outline of the hole, as I have the “enable chaining” option turned on.
I’ll click “OK” to take a look at the results. First off, you’ll see that the surface is yellow. This doesn’t affect the model in any way. Surfaces in Fusion 360 have one yellow side and one gray side so they’re easy to tell apart in comparison to solid faces. To switch it around we can use the “reverse normal” command in the “Modify” dropdown list.
Generally, I’ll make sure all the faces are aligned the same way as it’s easier to look at the surface geometry. Now that we’ve reversed the face we can see that we have some issues with it, as it resulted in irregular geometry. Looking at it from an angle, you’ll see that the path has this bulge and it doesn’t quite follow the rounded corner that we desire.
I’ll hit CMD + Z twice to undo both the “reverse normal” and the “patch” commands.
If you don’t get the results you’re looking for with the patch command, then I always recommend trying the loft command. This would be a pretty simple loft so I’ll activate it from the create dropdown list.
I’ll select both edges and you’ll see that creates a lofted surface from one edge to the other. We want this loft to follow this curved geometry, so we can reference it as a guide rail.
This, however, is where I see people often go wrong. They try to reference the geometry from the mesh file, which doesn’t work well because as we looked at earlier we get these choppy edges from the mesh triangles.
The key takeaway here is that you’ll often need to recreate simple sketch geometry to reference while you patch and repair your models.
I’m going to close out of the loft command for now and I’ll use the “Project’’ command with the keyboard shortcut letter “P,” as in Papa. What we want to do is project these two lines that touch the endpoints of this corner arc, that way we can redraw the arc.
With the project command active, we’ll first need to select the top face.
We can then select the two lines and hit “OK”.
We can now go to the create dropdown list, the arc flyout folder, and select the tangent arc. The Tangent arc is perfect in this scenario as we have our two tangent endpoints. I’ll select one endpoint and then the other. We can now finish the sketch and reference this tangent arc with the loft command.
I’ll reactivate the loft command and I’ll select both surface edges. This time, for the rail selection, we can reference our smooth tangent arc and I’ll click the “OK” button to complete the loft.
If we now inspect the corner you’ll see that we’ve successfully fixed it with smooth geometry. However, our model is still currently a surface body.
To get our solid body back we’ll have to stitch the surface bodies together.
I only repaired this one corner, so you would want to repeat this process to all areas of the model before you go to stitch them together.
I’ll select the “stitch” command in the toolbar. Then, I’ll select all of the surface bodies in the Browser and I’ll click “OK”. We now have some solid bodies in the Browser, which we can alter with the Solid modeling tools. In this scenario, maybe you’re looking to add custom text to the lid of the box or to create slots or storage compartments inside.
After altering your solid model, you could then click the Tools tab, select the 3D print icon, and resave your model as an STL to 3D print it.
Another option that you have while trying to repair your converted file would be to merge the mesh triangles.
With the paint selection tool still active, I’m going to drag over some of the facets that make up the hinge of this model.
Then, within the surface tab, we’ll need to go to the modify dropdown list. You’ll then see there is a “merge” option about halfway through the list.
If I click “OK” you’ll see that Fusion will merge all of the faces. Merging faces can be a lot quicker than recreating the faces from scratch with the surfacing tools; however, you won’t always end up with smooth geometry. You’ll see that this hinge does have a bulge in it similar to the rounded corner.
You’ll have to play around with these techniques as a lot of it varies from model to model. Sometimes the merge technique works quite well, but ultimately, it depends on how the triangles make up the model.
A lot of organic models will contain more facets, as more small triangles are required to define the contour. Let’s now take a look at a large file that is made up of a larger number of facets.
But first, let me know if you’re enjoying this tutorial by clicking that like button, and be honest, if you’re not liking it then hit the dislike button.
Making these concise and thorough tutorials does take quite a bit of my time, so help me out by commenting the words “ STL to SOLID” down below in the comments. This will help more Fusion 360 users discover this tutorial, and in return, I’ll be able to reach more people and continue to create more tutorials!
The second file I have is this Fish Pen holder, that I also grabbed from Thingiverse. I’ll insert the file with the insert Mesh command and I’m just going to center it as we did before.
Just looking at this file you’ll see that we have a large number of triangles that make up this shape. As you work with more mesh files you’ll start to get an idea of what shapes will be harder to convert.
I’ll turn off the design history for this model and I’ll try to convert this STL to a BRep solid body.
As you’ll see, I got a warning message and the conversion was aborted as the number of facets is too high for Fusion 360 to process. In some scenarios with a large number of facets, but fewer than this, you may still get a warning message, but it will give you the option to proceed with the conversion.
Either way, I would recommend that we don’t proceed and we attempt to lower the number of triangles. There are two approaches that we can take when this happens. We can either split this model into sections and then convert each section one at a time, or we can reduce the number of mesh triangles.
You can click that link in the upper-righthand corner to watch my other tutorial on splitting both mesh and solid files into smaller parts. I’ve also put the tutorial on the resource page.
If your file is extremely large, then you can split it up into sections, and then follow the steps I’m about to show you.
Let’s take a look at how to reduce the number of mesh facets.
You may have noticed that I have a Mesh tab in my toolbar. To see the mesh tab, you’ll have to turn on the mesh preview. Select your user name. Select Preferences. Then, select the preview tab on the left-hand side.
From here, you can turn on and apply the Mesh preview. Note, it’s in preview mode, as the functionality of the Mesh tools is still being worked on.
Under the mesh tab, we will find a “reduce” feature in the toolbar, or in the modify dropdown list.
We’ll first have to select the mesh. It’s important to note that you can either select certain areas of the mesh, or you can select the entire mesh body by selecting the body in the Browser.
Then, we can change the “Reduce Target” to the “Face Count” option, as we want to lower the overall number of facets.
Above that, we have the “reduce type.” Adaptive means Fusion 360 will adapt the surface triangles how it best fits the overall shape; whereas, the uniform option will force all of the triangles to be the same size. Generally, you’ll want to use the “adaptive” option, to ensure the object is closest to its original shape.
We then need to define the number of facets to be used. This model has over 100k facets, and Fusion 360 doesn’t allow more than 50,000. Ideally, we would have no more than 10,000…and you ultimately want to aim for the lowest amount as possible, without ruining the shape. You may even find that after you reduce the mesh triangles that you need to undo and try a smaller or larger amount.
For now, I’ll type out 5,000.
Lastly, we have the option to check “Preserve Boundaries”. This option controls whether Fusion 360 is allowed to modify any open boundary edges. This is particularly useful if you split your mesh files in half and will have two separate bodies meeting at open boundaries that you wish to merge later on.
We don’t have an open boundary with this model, so I’ll leave this unchecked and I’ll click “OK”.
If I now right-click on the mesh file to convert it to a BRep, you’ll see the option is not available. You will have to be in the solid modeling tab to access the option. This is another common problem that I see users face, as they wonder why the option is not available for them, even after they’ve turned off the design history.
I’ll select the Solid tab, then right-click on the mesh body again, where this time I’m able to select “Mesh to BRep”.
After clicking “OK” it looks like the model converted without any issues.
Another important thing to note is that some very complex STL models may have so many triangles that Fusion 360 won’t be able to reduce them without the software crashing. If you run into this, then I suggest reducing the mesh file in Autodesk Meshmixer, which is also available to download for free.
Most of the mesh functionality in Fusion 360 was derived from Meshmixer. So you should be able to use Meshmixer’s “reduce” command by following the same steps I just described. I’ll also add some helpful Meshmixer links to the resource page.
Now that we have a solid body we can clean up the file using the procedures I covered earlier in this tutorial.
I can simply use the delete key, or I can merge faces using the surfacing merge tool.
One important thing to note, when you’re working with very organic shapes or models, you’ll often find that there is simply not a way to completely get rid of the mesh triangles. If you’re looking to get rid of them completely, then you’re better off recreating the shape with the t-spline sculpt tools, or in some cases, the surfacing tools.
At this point, you have a solid body that you can attach to another solid body, customize with your name or design, cut a hole out of, or alter the design for your individual needs.
If you made it to the end of this video then let me and the community know by commenting below what type of 3D printer you have and what you like and dislike about it.
Last but not least, I want to give a shoutout to this week’s Patrons that joined us in the Product Design Online community. Special thanks to Kenneth Chang and Kaizen Z for supporting all of the Fusion 360 content that I make!
As always, I truly appreciate you taking the time to watch this tutorial. Click that thumbs up icon if you want more free content and click on that playlist in the lower right-hand corner to watch my “Learn Fusion 360 in 30 Days” series.
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