Using Extrusion Templates in Fusion 360 Using Insert into Current Design

An F4U Corsair at Planes of Fame in Chino Ca.
Photo is mine.

As part of my Fusion 360 experience, I've been building different parts for a WW2 era Vought F4U Corsair.

Why am I doing it?  It provides me an opportunity to learn how a machine like this was put together, it challenges me to find ways to use Fusion to find creative ways to solve design challenges, and I flat out enjoy it!

And what's the point of doing it if it's not a least a little bit fun!

The planes I've used came via my subscription to Aircorps Library, who has done a marvelous job scanning and sharing plans for WW2 era aircraft.

And before you ask, sorry, I'm not sharing the plans.  I pay for my subscription with them, and I'm happy to support their efforts.  To me, sharing their plans without proper compensation would be tantamount to stealing their hard work.

But with that being said, here's what I've learned about how the engineers of the 1930s and 1940s who designed the Corsair, and here's how I was able to get Fusion to help me with my "recreation" efforts.

Many parts were created from extrusions,  These extrusions were in turn, machined to create various parts for different parts of the aircraft.

The "Make From" reference in the
drawing's title block

Due to this fact, the finished parts had a note to "make from", the "from" part referencing the standard extrusion.

Well the last thing I want to do is redraw the exact same shape for multiple parts!

So here's how I was able to use Fusion to make the extrusion profile available, and reusable, to multiple drawings.

It's actually quite simple.  The first step is to create the cross section of the extrusion in a Fusion 360 part file.  I opted not to extrude the part at this point in time.

A sample of the extrusion template

This part becomes my template for future use.

The next step is to insert the template into a new model file so I can create new parts from the template.

The goal of this is to insert the previously created sketch into a new model, and extrude this sketch to create a new part.



First start a new Fusion 360 file.  Once the file is open, browse to the location of your template, and choose "Insert into Current Design".

Choosing  "Insert into Current Design" to use the
template for the extrusion

This function links the extrusion profile into the new file.  Once the sketch has been inserted, the sketch can be extruded just like it had been created right in the part, instead of being linked in.

The part being extruded using Fusions std. Extrusion tool

Once the extrusion is created, you can work on the part just like any other Fusion 360 part.  You can add and remove material as needed to meet your design requirements.

That's the basics  of creating an extrusion template in Fusion 360.   At least that's how I've approached it.

So what are the advantages I found that drew me to this conclusion?

Well, for starters, I don't have to drawing the same shape over and over again.  That alone is reason to chose that route, at least for me.

Second, any new parts created from the template are linked back to that original template.  So in the event any changes have to be made to the template, the parts generated from the template will also update.

In the event that happens, it can be a lot easier to update several parts than have to transfer the same dimension to several parts, and run the risk of missing that one odd part.

So in conclusion, this is why I approached this file in this way.  You may come at it completely differently, or maybe just vary this process just a little bit.

It's up to you!  If you find a different approach, feel free to share  in the comments.



Disclaimer: The views and opinions expressed in this article are those of the author and do not
necessarily reflect the official policy or position of Planes of Fame Air Museum or AirCorps Library.

Hydraulic Fluid Fitting Models in Fusion 360

A project I've been working on, "here and there" has been a series of AS5174 hydraulic fittings.

Original created in  Inventor they were imported into Fusion 360 and added the gallery here.

They're samples I've opted to share in the event anyone can use them out there.

If they help you, let me know!

Have fun!

Using Attach Canvas in Fusion 360 to Find an Unknown Measurement

For the last few weeks, on my spare time, I've been creating models from scanned prints in Fusion 360.

Most of these prints are produced in the 1940s, and they border on artwork.  When an drafter nearly

80 years ago could accomplish with pen and paper was impressive.  They were certainly masters of their

craft!  You can see a sample of a similar drawing here. 

How can you find the missing dimension? 

But a challenge I encountered was one that even modern users of 2D drawings encounter.  Missing

dimensions.

In some cases, the missing dimension was a result of a drafting error, in most cases, the dimension

was referenced on a different drawing that was unavailable to me.

But it doesn't matter how the dimensions ended up missing, if they can't be found or derived.  Without the missing dimension, creating a model from the drawing becomes much more challenging.

Fortunately Fusion 360 has a nice tool that makes finding this dimensions pretty simple, as long as

you have a single dimension, and the drawing is consistently scaled. 

How do you do it?  Here's how I was able to figure out what that phantom dimension.

Convert your drawing into an image file, a *.png, *.jpg, *.jpeg, and *.tif are all formats you can

use.

Now this image can be imported using the "Attached Canvas". icon.

Fusion 360 will want to know which plane you want to place the image on, and will also want you to browse for the image you want to insert.

Once an image and a plane are selected, you'll have an opportunity to scale the image, using either the handles or in the dialog box.  You can scale it here, but there's a step coming up where it'll be easier to scale the image accurately.  In my case, I used this yet to be seen step.

The Attached Canvas Preview

The drawing will import onto the Fusion 360 canvas, but it's not calibrated.  It's up to us to make sure the scale of the drawing  is 1:1. . 

I recommend re-positioning the attached image easier to measure.  Once that's done, locate the "Canvases" folder in the browser.  Right click on it, and choose "Calibrate".

This step gives you the opportunity to measure a known value on the Attached Canvas.

Choosing the calibrate option will allow you
size the imported image. 

Returning back to the situation I found myself in, The drawing I was reproducing had edges I with dimensions I could use, so I just picked an edge with a dimension, and chose the extents of the dimension for scale.

In the case of my drawing, the dimension I chose was 5 inches.  Naturally, the calibration the dimension on my canvas, but trust me!  It's 5 inches!

Calibrating the image using a known edge.

The image will resize according to that known dimension, and if the drawing with a consistent scale, measurements can be taken from any part of the drawing and a reasonably accurate measurement can be made. 

A measurement taken to obtain the part thickness

By using this method, the dimensions of the part can be obtained from the drawing, and the drawing turned into a 3D model.  

But of course, it's not all a walk in the park. There are some things to be aware of going in.

You've already seen me use the phrase "consistently scaled".  In other words, the drawing has to be created to some sort of accurate scale.  If it's sketched to different scales in the X and Y axis, it will be difficult, possibly impossible, to get good dimensions.

I've also used the phrase "reasonably accurate".  That means you can't quite get to the last decimal point of your measurement.  But you can get close enough to determine many measurements.

For example, if you measure .193 on a part that can be expected to be a standard thickness, then you might be looking at a thickness of .1875 inches.

But even if not perfect, this method can get you exactly what you need when no other methods work.

So give it a try!

Making a "Port Tool" in Fusion 360

The finished housing

Earlier this week I finished my sequence valve housing in Fusion 360.  And I learned a quite a bit doing it.

Many of my challenges were learning to use Fusion 360, partially because it's a tool I'm still new to, and there are different ways to do things in Fusion.

But the challenge I'm going to focus on is more one of process, than one of creating shapes in Fusion

The ports where fittings attach

One of the challenges I faced was how to easily model the 6 ports that were located in the housing.

They're all based on the AND-10050 standard.  That means that the ports are similar.  And when I say similar, I mean they're all similar geometry, varying only by size.

Take away the dimensions, and they're the exact same shape

I also recalled that there are special tools for drilling these ports.


In other words, where things can be standardized, they are as standardized as possible

So why do the same thing in Fusion?

We'll, here's how I did it, at least in brief.

First, create a new part in Fusion, locate the parameters, and entered the dimensions from the table found in the standard into the User Parameters section.

The user parameters

Why enter them first as User Parameters?  I can enter them in an orderly fashion, as they're seen in the table, and then enter them as I built, instead of trying to do both at the same time.  I think it's easier, personally.

The cross section for the "port tool".

Next, I built the port, using standard Fusion tools, and calling the user parameters I entered above.  In my case, I created the cross section for the port as a revolved feature.

It's interesting, at least I think, to point out that the finished "port tool" is a solid.  But I'll use this to remove material from the base casting that will be receiving the port I need.

The port tool, as a solid.

So what were the benefits I found to doing it this way?

First of all, I had a tool that was easily reusable and repeatable across as many places, and designs as I needed.

Second, since the AND-10050 port comes in multiple sizes, I could copy the port, change those user
parameters that I created earlier, and create a new port in a matter of minutes.

Inserting into the current design

And since there were several different port sizes in the casting I was reproducing, this proved to be a big time saver.

I effectively created a "template" for the port that I would use as a standard design feature.

Those benefits alone were enough to get me to bite on this method.

Now, all that was left to do was to open the design that needed the port, and insert the solid.

With a little magic from the move and combine command, I was able to subtract the port tool from the casting I needed, and end up with the right port.

But I'll save that one for a post a little later.

I hope this port helped, and if you have any tips on how you've tackled a similar challenge, feel free to leave a comment!

Inserting and moving the solid

Good luck!

Acknowledgements.

The print I used to create this valve body was provided via my subscription to AirCorps Library.  Thanks for the awesome work preserving vintage aircraft drawings!

A Friday Fusion 360 Tip - Going Off on a Tangent

My first try at the sequence valve housing.
After a few mistakes, I decided to try again. 

Just today I was working on a model in Fusion 360 of a small valve housing for the hydraulic system in an F4U Corsair.  Call it a self imposed design challenge.

This is actually my second try.  I had a first iteration, but I wasn't happy with it so I just decided to start again with a clean slate.

What can I say?  Life happens!  But I learned, and the new model will be better than its predecessor.

But in the process, I was cleaning some excess material with  the sweep command, and ran into something that left me with a combination of surprise, puzzlement, with a touch of frustration.  

The model path that I chose for my sweep wasn't complete.  The cut I was intending to make came up short.

The sweep coming up short, it should continue around the back
of the part.

I hope this isn't a bug.  I told myself.

I mean, I couldn't have made a mistake, right?  Right....  Of course not.....

Thankfully, I have years of 3D modeling experience behind me.  And when I say "years of 3D modeling experience", I mean "years of recovering from making mistakes building 3D models"!

So once my initial feeling of frustration passed, my troubleshooting brain kicked in and my experience told me to check the tangency of the sketch.

The arrow shows where I missed a tangent

Nothing will stop a path dead in it's tracks like a non tangent edge.

So I went ahead and checked the tangency of the path. Sure enough.  I had missed a tangent constraint.

You can see it in the image to the right.  On the left side of the highlighted area, there's a tangent constraint.  On the right, not so much....

So I added that in, and tried it again..  

Guess what!  It worked like a charm!  A small thing, but an important one.

So remember, whether your using Fusion 360, Autodesk Inventor, Solidworks, or another CAD tool, remember that one of the best set of tools you can have is a good set of troubleshooting steps!

Victory! 

And remember.... Watch those tangents!

Aircraft Maintenance Class - A Milestone Reached... But Why?

The instructional airframes that taught me many lessons.

June 16th 2017 marked a big date for me.  I completed the airframe portion of my aircraft maintenance curriculum.  It's been a long time in coming for sure!

In the 750 hours the FAA required of me, I've covered everything from safety wire, to hydraulic to safety wire, and everything in between.

Now I'm not racing through 18 hour days between work and school, I have time to answer a few questions I seem to be asked.

"Why are you taking aircraft maintenance classes?"

I know I'm supposed to have some sort of awe inspiring, motivational answer.

But the truth of the matter is, I did it because I like airplanes, and when the time came to expand my skill set, I decided to accomplish that by jumping feet first into something I've always liked.

And what resulted was an ongoing journey that has been difficult, exhausting, frustrating, and most of all, rewarding.

I learned many lessons that I've been able to apply to my work as a mechanical designer.

So that's my story.  I'm hoping to find a little time to blog about my ongoing lessons, as well as dive back into Fusion 360 and share a few of those lessons there as well!

The Amazon Web Service Outage of 2017

Earlier this week, Amazon Web Services suffered a service disruption.  For me personally, that meant disruption in Autodesk Fusion 360 (which I thankfully wasn't using at the time), and Fusion Lifecycle, which I was.  Fortunately, while Fusion Lifecycle was disrupted, it wasn't offline.

So, what happened?!?!

Several sites were affected.  My girlfriend sent me an instant message to let me know their CRM (Contact Resource Management) was down.  According to NPR, Gizmodo and Apple iCloud were affected.

The amazing, and perhaps disconcerting part of this is how easily the service was disrupted.  It seems that a technician was troubleshooting, and took off more servers than intended with a typographical error.

That's right, a typo, fat fingers as us techies call them, were the cause of the disruption.

Added to that, there didn't seem to enough redundancy, or possibly any, to absorb the lost servers while they were brought back online.

Now I'm no expert on Internet architecture. I imagine I know more than some, less than others.  I'm not going to prognosticate on what Amazon could have, and should have done, or should be doing.

There are plenty of people smarter than I who can do that better than I can.

But what I will say, is what I learned, relearned, and what I can do in the future.

What I learned and (relearned)

• The cloud is a great tool, it's saved my class grades when I didn't print it out by mistake.  But the technology is new, and new technology is often developing systems, and developing systems can be prone to failure.  
• As a whole, the cloud is pretty robust, but when it fails, it can fail spectacularly.  Many can be affected, and word can get out quick!

What can I do in the future

• I can't make Autodesk, Amazon, or anyone else change their system, at least not directly.  But I've heard rumors that improved offline capabilities are on their way.  I hope they're true, and that after this outage, the efforts have been increased.  I'll be keeping my eyes out for that development! 
• To this end, I'll be doing a better job of backing things up locally.  That's right, in a 180 degree turn, I'll be working in the cloud and backing up locally.  Just in case. 

I won't be abandoning the cloud, what I will be doing is approaching it more cautiously, and more diligently.  

In many ways, the cloud is a new frontier filled with pioneers, and pioneers must face the hazards of a new frontier to pave the way for others.  

For my part, I'll choose to stay on that frontier, but I will make sure I'm planning ahead! 

On into the brave new world!

photo credit: NPS Park Cultural Landscapes Program Chilkoot Trail via photopin (license)

A Fusion 360 Event with Autodesk and Haas Automation

Today I had a great opportunity to see Fusion 360 at the Autodesk Fusion 360 FastTrack Event in Anaheim, Ca.

The best part?  It was held at the Haas Automation Outlet!  What better way to see the Future of Making Things then to go somewhere the future is being made! 

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 8:34am PST

The Haas Factory Outlet - There's magic inside!

The first thing I saw inside was a little bit of manufacturing heaven!  Cue the theme music from 2001: A Space Odyssey!

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 8:43am PST

That was amazing enough, but next came the opportunity to see a little Fusion 360 in action!  The attendees had an opportunity to see, and try, taking a part in Fusion 360 and build tool paths and G-Code.

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 8:57am PST

Let's do this! 

We also had the opportunity to talk among each other, get ideas, and ask questions.

Even better, we had the chance to talk to CNC machinists, and learn from there experience, which is invaluable.
I'm a far cry from being a machinist, but I have cut a few parts on a mill, and generally can create the shape I'm after if it's not too complicated.  But I learned a lot from listening to them, and will be bending the ear of our own machinists when I'm back in the office.

I remember the days of "Thou shalt not take heavy cuts with your tools!" and "Thou shalt cut radii that are divisible by 1/16th of an inch!"

So shall it be written!  So shall it be done! 

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 10:31am PST

But now, tools like adaptive clearing to remove more material more efficiently.  We were also taught that there's technology exists to keep the tool moving efficiently.  In effect, even though the machine is cutting a curve, the computer can compensate in such a way that the load on the machine is no different than cutting a straight line.

New technology, and a new way of doing things for the future of making things!

I answered a few questions, and came away with a few more.  But most of all, I came away exited with what I'd learned, and excited with what more I could learn going forward!

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 12:37pm PST

Here's a few videos I grabbed!  Enjoy!  And get excited about what's out there!

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 11:13am PST

A tool change, and back at the part! 

A post shared by Jonathan Landeros (@jlanderos1973) on Feb 22, 2017 at 10:56am PST

Finish him!

When is "O" a "0"? - A Lesson Learned!

So here I am.  I've finished my course in aircraft electrical theory, now I have a week off before I start off into hydraulic and pneumatic systems.

My mentor and my nemesis.  The electrical trainer.
The instructor didn't let us use lights so we couldn't cheat! 

That gives me a little time to work  in Fusion 360 again, and I took the opportunity to build 3D model of a spar for a PT-17 Steerman biplane.

A PT-17 Steerman
By USN - scan from Robert L. Lawson (ed.): The History of US Naval Air Power. The Military Press, New York (USA), 1985. ISBN 0-517-414813, p. 72. US Navy cited as source., Public Domain, https://commons.wikimedia.org/w/index.php?curid=8046360

The modeling itself isn't very difficult, but my goal was to focus on the process of designing in Fusion 360, instead of focusing on the design itself.

I've purchased a subscription to a set of plans via my membership to AirCorps Library (A great resource BTW),.  They have a digitized copies of the spar, so I have a template to work from

The spar, being made of wood, has metal bushings pressed into it, and there lays the seeds of my error.

The spar modeled in Fusion 360, with the bushings assembled in.

The bushings are listed in tables, your typical "A" "B" columns with numbers.

But written in one of the columns was a suspicious looking "O".   It had to mean the number "0".  You know.  Zed. Naught.

An example of the "O" that got me. 

Confident in my conclusion of the figure's value, I modeled the bushing without a hole in it.

But as I my design progressed, I came to realize something.  That's not the number "0"!  That's the le letter "O".  As in a "letter O drill"!.

A letter "O" drill has a diameter of .316.  You can find it on any Imperial system drill chart.  Like this one here.

Fortunately, Fusion 360 did let me remedy that issue pretty fast.  But it did provide me a few moments of humor of what I saw, versus what the drawing meant.

Some of you may be thrown a mocking laugh, chuckle, or perhaps a guffaw in my general direction.  And I can't say I blame you.  Looking at the plans, the quotes around the letter should have implied it wasn't the number "0".

It also seemed odd to me that there would be a metal pin pressed into the wooden structure, but I shrugged it off as being a reinforcing pin.  It was only when I studied the assembly plans a little closer did I see that the bushing did have a hole in it.

I choose to blame it on the early hour of the morning (it was 5AM), and the coffee having yet to fully clear the fog in my brain.

So what have I learned?  And perhaps, what can you learn from my mistake?

1. It pays to know how something is built.  Even though I missed the mark initially, it did finally dawn on me that the drawing called out a letter "O" drill.  Had I not drilled my own holes, and known that drills can be called out by letters, I may have shaken my fist and accused the drawing of being wrong. 
2. Try to use your common sense.  I should have double checked the bushing against the assembly when I had my initial doubt.  It did clearly show the bushing as having a hole.  That might have tipped me off. 
3. Try to understand how the drawing is meant to be interpreted.  This drawing was originally made in the 1930s.  It's format is much different than the drawings I use at work today.  Things considered obsolete in 2017, like fractions and certain styles of notes, were the standard when this drawing was created. 
4. If you think that bullet 3 is a bit of a stretch, there are places that maintain drawings for decades.  Even at work we have drawings from the 1970s that look more like the drawing from the 1930s than the 2000s. 
5. You're going to learn something new everyday.  Embrace it! 

So there are my lessons!  Thankfully, it's a small error, easily corrected, and with a lot to teach!   

Learn from my mistakes, and keep an open mind to the lessons our profession has to teach! 

Making up Miles by Measuring Inches - My 3DConnexion CADMouse Anecdote

***Disclaimer!***

The pictures I'm using for this blog post are of my home laptop running Autodesk Fusion 360 with a CADMouse and SpaceMouse, both made by 3DConnexion.  Security at work limits what I images I can share from my work station.

Better safe that jobless!

*** End Disclaimer!***

It's likely we've all heard the quote "A journey of a thousand miles begins with a single step".  And I'm just as sure that millions of "bar-stool philosophers" like myself have used it in some sort of discussion or debate.

Earlier this week, the microcosm of my CAD station gave me a moment to reflect on that quote again.

Since I started at my new position as a mechanical designer about a year ago, I've had a 3DConnexion SpaceMouse Pro and 3DConnexion CADMouse.  What can I say, work takes good care of me!

My laptop running Fusion 360.  I need to program buttons for this too. 

At one point, I had all the buttons mapped, and I was happily using radial menus and hotkeys.

But then, our CAD stations were upgraded, and all my settings were lost.

For most of that time, I keep telling myself.  "I need to rethink what commands I use most frequently, and start programming them into my devices."

And for most of that time, I've told myself.  "I really need to finalize what commands are really important to me.", or "I'll do it tomorrow.", or the infamous, "Once things slow down a bit."

That's how nearly a year passed with all my buttons set to their default settings.

My CADMouse menu in Fusion 360

Finally, I told myself, "Jon, just pick a command and program it!"

So I did.  I picked a few commands, and put them into my SpaceMouse Pro and CADMouse.

Programming the menus for my 3DConnexion CADMouse

And nearly instantly, I started wondering why I hadn't done it sooner!

What were the lessons I learned? 

• Don't fall victim to "Analysis Paralysis".  I postponed making a decision until I had all the information.  The problem is, I had no hard stop to when I was done evaluating.  I could always "test a little longer". 
• Just start already!  It's not like the path can't be changed while keeping the destination the same.  
• We get so focused on the big goals, we forget the little steps.  Nobody knows that I customized my SpaceMouse Pro and CADMouse.  And there's really no need for them to.  But navigating my CAD system is much easier because I took a few minutes to do so.   

Conclusion?

Now, it's not like my 40 hour week suddenly turned into a 30 hour week, or that project that's going to take 18 months suddenly took twelve months because of my pre-programmed 3DConnexion devices.

But what did happen?

Things were just smoother, and dare I say a little more pleasant.  I wasn't reaching for my keyboard for commonly used hot keys, moving across a large monitor to get to an icon.

Now it didn't take my 40 hour week and make it into a 30 hour week, but it did make navigating my tools a little easier.

It's like having your favorite stations preprogrammed into your car radio.  It doesn't make a dramatic change in the lenght of your commute, but it does make the time you spend more pleasant.

Sometimes, it really is about the journey! 

Fusion 360 - 5 Updates on January 19th, 2017

Just a quick post on Fusion 360.  

Late last week, Fusion 360 received an update!

I won't spell it out here. Autodesk has already done that in their post explaining the update here.

Take a look at the new features and give them a try. 

Myself, I'm interested in the new branching preview they've added! 

Branching has been added! You can see it in the upper left corner of the screen.

I know I'm looking forward to some more features in the future!

Back in the Learning Saddle Again - In Classroom and Life!

A little update on the going on with me, and Inventor Tales as a blog.  

I'm back in class four days a week along with my day job as a Mechanical Designer, so things have gotten rather busy again.  

Which I'm afraid does rob time from my working with Fusion 360.

This time I'm studying DC electrical theory.  That means a lot of time in lecture and lab, right now I'm learning how to simplify series-parallel circuits. 

Then it means a couple of hours in the lab wiring circuits to make sure the concepts have really set in. 

The first, and simplest circuit I wired.  

That does mean slowing down my posts on my CAD products, yet again.  As my time is limited.  But I do plan on doing my best to share what I learn when I do have the time.

But one thing I can share, is a quick lesson I learned earlier this week.  One where my aircraft maintenance classes helped me in my "day job' as a mechanical designer.

It was during a discussion about how flared fittings are attached to a semi-rigid line.  

An example of a flared semi-rigid line I made in class.

The discussion related to the process of how it would be accomplish, as well as a few pros and cons as they applied to an aerospace valve.

And because of my aircraft maintenance classes, I've actually flared a 37 degree line myself. 

The tube in the flaring block.

Because I had taken these classes, I was better equipped to be an asset for my job.  

What's the lesson here?  Not all of you work with aviation applications, so a 37 degree flare may not apply to you.  

But the lesson I think you can take away is to keep your desire to learn alive.  And find something, whatever it is, that both interests you, and keeps you learning!

And I'll see about picking back up on those Fusion 360 posts soon!

And one last thing!

Here's a little video on the process of flaring a tube for an aircraft application!

A360 to Share a Fusion 360 Model - I Got the Feedback I Needed In Minutes!

There are many examples of people who have used computer aided design programs like Fusion 360 to create models for replacement parts that can no longer be located.

It's a fantastic technology, one that in my personal opinion is still in it's early stages.

This is my experience with a knob on the stove in our home. Now, this isn't a story of how I created a model, had it 3D printed, and how incredible the end product is.

There are many of those stories.  And their success is well deserved. 

I'm just sharing a step in the journey as I learn about the process first hand.  I may follow through and find success!  Or I may find, for some reason, it's not worth pursuing any further. 

But carrying that dose of reality. Here is the first step in that journey, building and sharing the model. 

Building the Model - The Easy Part! 

Building the model was a process of measuring the knob.  That meant pulling out my trusty set of calipers and carefully measuring the knob.  I had to make sure that the dimensions, particularly where it mounted to the stove were correct.  

The process of modeling took only about two relaxed hours on Friday morning, which for me is a day off. That part was pretty easy. 

The stove knob modeled in Fusion 360.

But now I've finished my model and it's only about 9AM.  I'd like to share the model with her, but she's just started her day at work.  

So how do I share the model? 

How do I share the model quickly, easily, and effectively so I can get feedback as soon as possible?

My Answer - A360

In a previous post, I mentioned that Autodesk 360, or A360, mirrors your Fusion 360 projects.  Now was time to take advantage of that for collaboration to a fuller, if not completely full form. 

I opened the model in A360 and opened the file in the A360 viewer.  I clicked the share icon to start the sharing process. 

The knob in A360.  Notice the "Share" icon in the upper right.

After selecting "Share" the sharing options will show up.  

In my case, I made sure the file was shared.  Then I copied the link to my instant messaging program, and sent it to my girlfriend.

After a about 30 minutes, she had taken a look at the model in her internet browser, and had given me a few thoughts on what I had done.

First circle completed!

Thoughts on Collaboration

While very tech savvy, my girlfriend isn't a CAD operator.  But with just a link, she was able to view the model in all it's 3D glory.  I didn't have to take half a dozen screen grabs, and wait for an email.  Points to A360 for that.  The online view did all it needed to do, and it did it quickly, and efficiently. 

My total turnaround time was less than 3 hours from starting to build the model, to having my girlfriend's feedback. 

On another note...  If your aware of Autodesk's Live Review you might be wondering why I didn't use it. The answer for that is a simple matter of logistics.  With my girlfriend at work, I had to accommodate her schedule, which meant sending her a link that she could use at her convenience.  Sending a link was the best tool for this task. 

Next Steps?

The next thing to do is look into getting the part 3D printed.  The main question is will it be cost efficient.  There's no sense if the cost to make a new knob is 20% of the cost of a new stove.  

But that's what I'm trying to learn by going through this process.  

I'll keep you posted on this part of my journey!  You're learning along with me!   Or at least that's my hope! 

And if' you'd like to look at the Fusion 360 model yourself.  Here's a link!  Feel free to have a look.

Autodesk A360 and Your Own Private Wiki

One thing I've learned from my aircraft maintenance classes, as well as from my various aviation mentors, is that the information surrounding a design can be every bit as critical as the design itself.

For example, aircraft have extensive logbooks recording all maintenance and inspections that have been performed on the aircraft.  At any time, your friends from the Federal Aviation Administration (FAA), can drop in and say.

"We're from the FAA, we're here to help.  May we see your aircraft maintenance logbook?"

A typical aircraft maintenance logbook.  This is not to be lost! 

Needless to say, if you don't have an accurate and updated logbook, you may feel a few beads of sweat on your forehead.

The point of my little anecdote is that when working with an aircraft, product, or design, the information that drove your design in a given direction can be every bit as important as the design itself.

That information may come in the form of spec sheets, vendor quotes, or meeting notes.

What would you do if you were asked, "What information drove you to make the decision you did?

In my experience, these documents are often misplaced or even worse, lost forever.  Meeting notes get thrown out, spec sheets get dropped in "a network drive somewhere", and vendor quotes are left in "an email from a few months ago".  

As I've taken a deeper dive into Fusion 360 and Autodesk A360, I've found that A360 provides a nice tool that can help with that very thing.

A360 has a "Wiki" folder that let's you create documents letting you keep the information you need with your project.

The "Wiki" folder hidden in A360.

It's a special folder where you can add information and add links to whatever information you deem important to your project.

Here you can create multiple documents, share them with other members of your team, and allow them to comment, and update the documents.

A sample of my A3t60 Wiki.  I only have one page started

In my initial test, I created a Wiki page with links to important documents that I might need.  These references are documents from the FAA, links to important technical documents, and helpful instructional videos.

The Wiki page I created for my Fusion 360 project.

Now is that all you can do?  Hardly!  Personally, I've only just waded into the shallow end of the pool.

But it's something I intend to make further use of, and if you're using Fusion 360, I think that it's worth taking a look at what this Wiki folder in A360 can do for you.

After all, if you don't record it, it's like it never happened in the first place.

So what do you think you could use this Wiki page for?

Share your thoughts!  In the spirit of collaboration, let's all learn together!