Creating a Part by Projecting Geometry from Another Part in Fusion 360

One of the goals I set  for myself is to try to spend some time every week to build something in Fusion 360.  Sometimes, all I can do is create a patter of holes, or build a few sheet metal flanges.

But I always tell myself I'll try something new in Fusion 360.  

So far, so good!

One thing I've been trying is making different parts, some of which have been sheet metal.

I've got ribs that will support a sheet metal.  The component is an aircraft trim tab.  There are two ribs at each end of the tab.

The sheet metal forming the tab will wrap around the ribs and attached via rivets.  That means that the sheet metal will be following the ribs, so why not reuse that geometry instead of trying to recreating with a lot of "measuring and calculating".

The first thing to do is to assemble the ribs in their final position and orientation.

The ribs place and oriented, ready for sheet metal.

The next step is to create a new component in the Fusion assembly and activate it.  Select it as a sheet metal part and set your sheet metal rules.

If your not sure about creating sheet metal rules, my previous post here may help.

Create a new component

Now, create a sketch, and being projecting geometry from the existing parts.  

Now project the geometry that will be used to help define the new part.  I'd recommend making it construction geometry to make sure it doesn't accidentally add itself to your part. 

Creating construction geometry to build a part.

Now sketch out the profile required.  In this case, it's the shape of the sheet metal part. 

Projected geometry to form the sheet metal profile.

Now it's a matter of creating the sheet metal flanges to the distance needed to define the part.

The sheet metal part extruded.

Now continue the process of defining the part.  This includes other features, such as extrusions and holes.

Additional features can be created by projecting from another part.

Give it a try, it can make creating another part much easier than transitioning measurements! 

Bonus tip! 

Change your part opacity by right clicking on a component and choosing "Opacity Control".  You can make the part semi-transparent and make it easier to see underlying geometry! 

Try changing Opacity to make selecting through parts easier.

Acknowledgements: 

Trim tab created from drawings accessed via my subscription to Air Corps Library.

I've Got Great Designs in Fusion 360! But How Do I Find Them?

A valve housing I built, I'd hate to lose this! 

Lately, I've been posting about building models in Fusion 360, especially with the addition of sheet metal tools.  (Yay!)

But the most stunning Fusion 360 file in the history of stunning Fusion 360 files does no good if you're not able to locate it in the sea of slightly less stunning Fusion 360 files.

As I've started accumulating models, I found myself thinking; "How to I find a given file as I create more designs?" or, "What happens, if I misplace one?!?"

I haven't yet misplaced a file yet.  But it will happen some day, and I'll have to make sure I can find it again when I do.

Thus, I was led to the Data Management side of Fusion 360, to try a little simple searching.

The first thing I had to do was log into my A360 hub here.  That opens up the A360 hub, where I was greeted with a list of the projects I've created over my time using Fusion 360.

From there, it was a fairly simple matter of locating the search icon, typing in a file name, and letting the search tools do their job.

In my case, I picked a valve housing I had worked on.

Searching for the housing

When the file opened in my dashboard, I could see a thumbnail, what other designs this housing used, and where this file was used.  In my case, I'm not yet using this design elsewhere.  I can also access drawings created from this part.

Now there's quite a bit that can be done from this screen, so I'm not going to go into it all in this post. I'd be typing forever!

But I will point out two icons that are well worth looking at.

The first, is the View icon, which will open up the file in a viewer, the other is the Edit icon, which will open the file in Fusion 360 desktop, and the browser if available.

Just these functions alone helped as I was exploring alone, and there are more functions in the viewer. But like I said, I'm going to save those for later!  It's getting late, and I have to sleep sometime.



But remember to take advantage of the hub if you're using Fusion 360!

I think it'll help you out!

Restarting a Line in a Fusion 360 Sketch

My story of late has been building a few parts in Fusion 360 over the course of a few evenings.

Another sheet metal part I'm working on.

And with that practice, comes a few simpler tricks to help models get built a little bit more efficiently.


It's been a series of sketching, extruding, and now that Fusion 360 has a sheet metal module, it's included adding flanges.

Making these parts means drawing a lot of lines to build parts.  But part of drawing these lines sometimes means creating a line in one place, completing it, then creating another line in a different place on the sketch.

If I were using Inventor, I would right click and choose the "Restart".  That would finish the line being drawn, but remain in the command so another line could be started elsewhere.

It's a simple command, but one that I know I've found helpful.

But looking at Fusion 360 there is no repeat command.  At first blush, it would appear that it isn't possible.

But before wishing an overworked programmer a pox upon his soul, I thought I'd see if another tool might give me the behavior I was looking for.

And I found it!

All I had to do was right click and choose Repeat Line.  It's a slightly different command, but it did exactly what I was after.  It gave me the ability to finish the line command where it was, and restart it in a new spot.  And I didn't have to exit and restart the command.

It's a workflow in just about every CAD program that will allow me to use it.  I'm big on placing holes on lines and vertices of rectangles.

So if that's a workflow you're also used to, give it a try in Fusion 360!  It might be a way to make things run a little smoother!

Creating holes using lines, a trick I like using. 

A Few Minutes with Unfold & Refold in Fusion 360

The part for this blog.

My adventures with Fusion 360 continue.  Mostly, my tasks have been composed of taking 2D prints, and turning them into 3D Fusion models.  

These prints all hail from the 1940s, and it's fun, and educational to see how these prints adapt to new design tools that were beyond the science fiction of the day.

Naturally, with Fusion 360 introducing sheet metal, I've been jumping on the sheet metal portion of my self imposed task.

In creating the latest sheet metal part, I found a reason to try out the unfold/refold functions in Fusion 360.  It was exactly the right tool for what I needed.

The portion of the model in question is located on the end of the flange.  The channel is cut at an angle, and at first glance, that might not seem like much.  

But inspect the flange a little closer, and it can be seen that the angle was cut in the flat and then folded.  As a result, it follows around the bend of the flange.  

Thinking about it, that would seem to make sense from a "keep it simple, stupid" approach to manufacturing. 

But in Fusion, we design the finished sheet metal part.  The flat pattern is, in a sense, the result of the folded part we've designed.  

And the way I chose to design this part, was to create a C-Channel, and even though I tried to create the angle initially, it doesn't take long to see that I didn't get the result I wanted. 

The end of the incomplete channel.
That angle is all wrong

This is where the unfold and refold tools come into play.  Working in conjunction, they allow the part to be unfolded, a cut to be made, and then the part to be reloaded.

To get things started, choose the unfold tool from the sheet metal workspace.

Locating the Unfold Tool

This will bring up the unfold dialog box.  To unfold, choose the face that will remain stationary, then select the bends to unfold.  Alternately, the Unfold All Bends checkbox will unfold all the bends in the sheet metal part. I

In the case of my part, I'll need to unfold everything.

The Unfold tool in progress.  The bend in the lower part
of the image has already been selected to unfold, and is previewed.

The part will flatten out.  At this point, any features that need to be added can be added the part, in my case, I added the proper shape I wanted.

Once the cut is completed, it's a matter of refolding the part. All that's required is clicking the Refold Faces tool, and the part will be refolded

The Refold Faces Tool

Once refolded, you're free to continue working on your part! 

So give the Unfold and Refold tools a shot!  I've had pretty good luck so far, although admittedly my "seat time" isn't vast. 

But I have a lot more drawings to convert to 3D, so I expect I'll be testing it out quite a bit in the next few weeks! 

Getting a Diameter Dimension when Sketching in Fusion 360

It's been a busy week working with a little Fusion 360, as well as doing a little studying for my Aircraft Maintenance classes.

Because of that, this post will be a little on the simpler side, but I still hope the material is something that you all find valuable.

In my work with Fusion, I've had to create a few sheet metal countersinks already.  Admittedly, some of these parts will never unfold.  In fact, the part on the right wasn't even made using sheet metal tools!

But the part has sheet metal countersinks, and that's where this blog starts. The countersinks are made by dimpling the metal, since cutting a countersink would leave too little material and compromise the material strength.

The sharp corners at the bottom of this countersink are, to put it mildly, bad.

A better countersink for thinner material

That being briefly discussed, the dimpled countersink is created by using the revolve tool.  That's easy enough, but when creating the dimension for the hole diameter, Fusion only gives you an option for a radius.

But this dimension is a radius!?!

But what if there was a way to get a diameter?

If I took time out of my Sunday afternoon to write the post, you can likely guess there is.  Here's how you do it.

While in the sketch, start the dimension tool.  Dimension the geometry that represents the edge of the diameter, and the center of rotation.  But before just clicking geometry, here's a trick that helped me.

Pick a point on the diameter, for example, for my countersink, I chose a vertex where two lines representing my countersink geometry intersect.

Even if you could choose a line, take the extra time to pick the point.  I think it's worth it.

Next, pick your axis of rotation, just like normal.  At this point, you may say; "Jon, I still see a radius.  Thanks for nothing jerkface!"

But if you do, I'm going to give you a smirk and say; "Try right clicking!"

Selecting the diameter dimension

Now the option for Diameter Dimension appears.  Click on that, and you're off and running!

You may also be wondering why I made such a big deal about picking a point for the edge of the diameter.  I've found that by picking a point, Fusion picks the correct diameter every time.

I hate it when this happens

If I try picking a line, I sometimes get the geometry backward if I pick the geometry in the wrong order.  The trick if you prefer this method, is to make sure you pick the axis of rotation first.

So give it a try!  And good luck!