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!

Using Sheet Metal Styles - Fusion 360 Style

So I've had a little more time to work with Fusion 360's sheet metal, and things are beginning to run a lot smoother. as I'm getting more familiar with the tool.

One of the things I've put a little of time into is sheet metal styles.  While making parts is the goal, and my favorite part of using any CAD system.  A solid foundation of sheet metal styles can go a long way to making sure your sheet metal parts are accurate and consistent.

Most of all, a good set of styles can eliminate a lot of repetitive work and make sure you spend most of your time modeling, instead of creating the same sheet metal for the umpteenth time!

To set up a sheet metal style, the first trick is to locate the style.  In Fusion, you'll find that in the Sheet Metal Workspace, on the Modify menu.

Finding your Sheet Metal Styles

Opening up the Sheet Metal Styles dialog box, you'll see two sections, In this design, and Library.   The styles located in the design are stored inside the current document.  But the library, those styles are available to any documents you want.

The Sheet Metal Styles dialog box

Fusion provided some defaults, but they didn't match what I needed, which in the case of this part was .032 ALCLAD Aluminum.

While Fusion doesn't provide us with this as an option, I do have a Aluminum (in), a generic aluminum, which I can copy to create my material.

You may have noticed that I've also got .051 and .040 ALCLAD already created.  I could have easily copied those as well.  But let's, for a moment, pretend they don't exist, and we'll start like I did from scratch, without any ALCLAD.

All you have to do is right click on the material you want to start from, in this case, Aluminum (in).  Choose "New Rule".

Creating a new rule

A new dialog box will appear where the parameters for the new rule can be entered.

The sheet metal styles dialog box.

Save the style, and congratulations!  A new Sheet Metal Style in Fusion 360.

The new rule is added to the library! 

Notice that since the rule I started from was located in the library, the new rule was also created in the library.  It's already a part of my library, and available to other parts.

But What if I Copied a Material That's Only Local in the Design? 

If you copied a material that's local to the design, just right click on it, and there's an option to Copy to Library, and the material can quickly be placed in the library so it can be available to other designs.

Copying from the local cache to the library

That's Wonderful!  But Now I Need to Change Styles! 

I poked around Fusion a little bit before I found this, mostly because I refused to resort to reading the instructions!  But to switch to a different sheet metal style, locate the Sheet Metal Style in Fusion's browser, and locate the Switch Rule option.

Switching Sheet Metal Styles

By choosing this you can select a rule located in your document, or in your library!

So have at it, and keep learning!

Fusion 360 Sheet Metal - My First Impressions

So I've had a little time to work with Fusion 360's sheet metal tools.  And when I say "a little", I mean "A LITTLE".

My first Fusion 360 sheet metal part

All I've had is a couple of evenings to create a few simple sheet metal parts.  They're no more than a couple of brackets, but they're also enough for me to start getting acquainted with the tools, even if it's sill a quick introduction.

But what I was able to do was to get a bit of an impression of how Fusion 360 works, and figure out where I need to learn a little more.

And when I say a "little more", I mean "a lot" more.

I've used sheet metal in Inventor on and off for around 17 years now, so it goes without saying that I approached Fusion from the perspective of using it like it was Inventor.

So I'll just cop to the fact that I can't help but compare it to Inventor.

What is the the kids say these days?  "Sorry.  Not sorry."

And while Inventor was similar to Fusion 360 in many ways, it was very different in others.

Here are just a few I've noticed so far.

Sheet Metal Rules

They're actually a lot like Inventor's sheet metal rules.  It's similar enough, that I could make the jump pretty easily.

Fusion's Sheet Metal Rules.  I've created my own rule here.

I miss the thumbnail images that Inventor has in its sheet metal rules dialog, but I could navigate it pretty well based on the information provided by Fusion.

Bend tables and equations aren't in Fusion at this point, but even when they were available in Inventor, I never knew anyone who used them to generate flat patterns.

I'm sure there are that do use them, I just didn't encounter them in my travels.  This may be one of those "future update" items.

I was able to create a new sheet metal rule in a few minutes, all it takes is copying another, similar rule and changing it to meet my new requirements.

The Flange Tool

In Inventor, the Flange tool created flanges from existing faces, that's it.  if you wanted to create a C-channel in one step, you had to use "Contour Flange".  If you wanted a flat sheet metal face, you had to use the 'Face" tool.

Fusion 360 combines those three tools into one "Flange" tool.

Using the Flange tool to create a channel

Using the Flange tool to create a sheet metal face.

The Flange tool creating a straight up flange.

Once I figured this out, I came to like it.  To me, it's a simple, easy to use approach, at least in my opinion.

After all, it's much harder to hit the wrong button when there's only one button!

I also like how Fusion implemented the grips to change the flange height and angle.  It felt like a natural way to form the part.

After a few minutes of figuring out how it ticked, I liked the way they went with it!

Unfolding

Creating a flat patter from a folded part was easy for me.  Fusion 360 asks for a stationary face.  In other words, which face the part will use as its "anchor" to unfold around.

Selecting the stationary face for a flat pattern

Inventor did this as well, but to me, it didn't always seem obvious that you could provide Inventor with this information, especially to Inventor newcomers.  Although later releases of Inventor did address this with the "A" face tool.

In any, case, the functionality is essentially the same, just presented differently.

The flat patterned generated in Fusion 360

What Can be Unfolded?

See this part?  You're not unfolding this one! 

The rule of thumb I was taught for Inventor was if you could bend the part in a sheet metal brake, Inventor could unfold it.  Formed parts with a lot of deformation, or flanges around bends, aren't going to unfold in Fusion 360.

The same seems to hold true in Fusion 360, based on my few minutes of testing.  But I expected that, so there really aren't any surprises here.  

I just had to see if maybe, just maybe, there was  the computer aided equivalent of the Holy Grail in the unfolding tools!

In conclusion.

After what was, at most, two hours of seat time, I was able to generate some pretty simple sheet metal parts pretty easily.

There's some room for growth to be sure, but I'm sure improvements will be made in future updates.

The functionality that I've seen so far, I like!

And I do have to reiterate that I have very little time with Fusion 360 sheet metal, so it's even possible there may be functions I haven't even discovered yet!

So at this point, I'll enjoy, and continue to learn the functionality I have, and look forward to those updates in the future.