How Turn/Mill Machines and Fusion 360 Help Rivian Increase Throughput

CHRIS COLE: Hello and welcome to how Turn/Mill machines in Fusion 360 help Rivian increase throughput. Before we get started, I'd like to draw your attention to the safe harbor statement. We will be making some forward looking statements regarding development. And just know that these are not promises or guarantees. Things are subject to change. So please don't base any kind of purchasing or investment decisions on the information you're going to hear today.

My name is Chris Cole I'm a senior solutions engineer at Autodesk. And I'm joined today by my colleague Michael Grenier who is also a solutions engineer at Autodesk. And we have the pleasure of being teamed up with Matthew Yates and Josh Postell from Rivian on this presentation.

Our agenda is we're going to go over Turn/Mill. So I'm going to start everybody off on a level playing field here. I know there are varying degrees of knowledge and expertise. So I'm going to start off with what is Turn/Mill. Give you some examples of what those machines are like and what they do. Then, I'm going to pass over to Michael and he's going to go through a case study of Fusion for Turn/Mill and talk about some future developments.

Then, we're going to kick it over to Matt, who's going to go over Rivian, who they are, what they do, and how they use Fusion. And finally, we'll go to Josh, who will talk about how Rivian uses Fusion specifically for Turn/Mill.

So first of all, what is Turn/Mill? Well, it kind of depends on who you ask. Because there is some varying terminology in the industry. In general, we're talking about multitasking machines, machines that can do more than one kind of operation. But in our case, we're talking about Turn/Mill.

And those are machines that, if you strip them down to their base, you're going to see a lathe. It starts as a lathe. And then functionality, like milling, is added to that machine. So it's Turn/Mill.

There are mills out there that have turning capability and we call them Mill/Turn. And then, we have Swiss machining that is a subset of Turn/Mill. I'll talk a little bit about that later. And just for fun I threw turnmill in there. That's one word, turnmill. Just for those of you who might use Feature Cam. That's another Autodesk application which has a Turn/Mill function where the part is actually turning in lathe. But you're using a live tool to cut that material. It's used for roughing and it can remove material very quickly.

So again, you might hear some different terminology. People even within Autodesk will call Turn/Mill and Mill/Turn-- they'll interchange those terms. But in our case, we're going with Turn/Mill as a milling machine-- or I'm sorry, a machine that's capable of doing both milling and turning. But it's recognized, at its base, as a lathe, either a vertical or horizontal.

So let's back up a little bit. Let's talk about what people traditionally do if they do not have multitasking machines. If you have a component like this, you'll have to do it in a couple of different operations. You might start on a lathe then take it to a mill to finish off the part. You might go the other direction or you might go back and forth.

But in essence, what you have to do is you do separate operations on separate machines. And you can see there on the slide, there are all kinds of different combinations of workflows. But the bottom line is it takes more than one operation. And that has pros and cons. First of all, it's pretty simple. You're using machines that with tribal knowledge that you already have. You're used to that workflow and knowing how to move things around your shop. No special tooling, no special equipment.

But it also has some cons. You need multiple machines. You need that tribal knowledge. It's slower. You have to move things around your shop. So more machines, which take up more of your floor plan. Moving machines or moving parts around like that can cause unintended errors. It's harder to maintain accuracy. And you could have more scrap.

And it's not the best use of personnel because you've got more than one person working on a part. Or worse yet, you might have one person going from machine to machine leaving idle machines behind. So the Turn/Mill advantage is you can do all of this on one machine. You can make the entire component without moving it around the shop.

There are special blocks on the machine, or tool stations, that allow you to run driven rotary tools, like endmills and drills. Oftentimes, they have a secondary spindle, like a sub-spindle, that will allow you to transfer the part and work on the other side of the part so that you can drop off a complete part into the part catcher.

There are all kinds of configurations in the industry to cater to what kind of work you do and what kind of work environment you have. The simplest being a single turret machine. These have power stations on the turret that can run rotary tools. And if they have a sub-spindle, they can address either spindle. So they can transfer that part.

If they have a y-axis, as you see there in the video, it allows you to create geometries that would not be possible if that tool had to stay on center of the part.

Moving up in complexity, we have multiple turrets, which do essentially the same thing but more turrets are in action. They can work together on a single setup essentially doubling your speed, or they can work independently on different spindles. Again, being more efficient and making the most of that production space.

These are synchronized and are well designed for doing production type work where you're dropping complete parts off with every cycle start. And of course, they reduce that footprint, again, by doing a lot of functionality in limited workspace.

Taking it up one more notch we have B-Axis milling heads. These are milling heads which pivot around the y-axis of the machine, and effectively, take those tools from either being x or z-oriented or some fixed angle, you can hit any angle within that head's travel.

Some of those heads, depending upon the capability of the machine, can actually move while cutting creating simultaneous five axis toolpaths. And they can also be worked in conjunction with maybe a lower turret. So you really get the most of-- the best of all worlds.

Now, I talked about with Swiss lathes a minute ago. And these are specialized Turn/Mill machines that instead of using a turret, they use tool gangs, these linear tool gangs that you can see there in the photograph. They're known for being high production, high accuracy machines.

And now, not all of the tools can travel the length of the part. What they do instead is they stay in a fixed position very close to the spindle nose. And instead of the tool moving, the stock actually moves through a guide bushing using a sliding headstock.

This enables the user to create very precise small parts because the part stays fairly rigid relative to that tool. They are commonly found in the medical, automotive, and aerospace industries, and of course, they were invented for the watch industry in Switzerland.

Finally, we have Mill/Turn, and we mentioned these earlier. These are machines that are at their core milling machines, but they have some turning capability. They can turn one of the axes infinitely at an enough of velocity where they can create turning toolpaths. They always have a single chuck or a table and a single tool post or a spindle. And they're mainly used for larger parts that need some turning but are mostly milled, think of large housings.

The tooling can be fairly simple or specialized. But what's really critical here is the way they're mounted, of course, with these powered tool blocks. These turrets have limited space. So not only do you have the powered milling blocks, but you can have special turning blocks which can have multiple orientations of tools making the most of that workspace.

You can even have indexable mini turrets that are mounted on the turret that allow multiple turning tools to be mounted in a single position. When you have Turn/Mill machines that have spindle styled heads, those are going to have your typical tool changers and tool carousels.

The workholding on Turn/Mill machines are pretty standard. You have Collet chucks and you have jaw chucks, either soft jaws or hard jaws. The part support can be employed if you have parts that might flex or bend when being machined. So you might have a tailstock that can come out and fit into a center and hold that part stable so that it doesn't move under tool pressure or cutting pressure. And that will help improve accuracy and surface finish.

A steady rest actually cradles the part across its diameter, somewhere on its diameter, and holds that part steady, again, as it's being machined so that you don't get vibration or flex. You can even use steady rest and tail stocks in conjunction with one another.

The sub-spindle is not only for transferring parts, but it can be also used synchronized with the main spindle holding the part on both ends, again, to achieve more rigidity so you have more accuracy and better surface finish.

So what about programming these machines? Well, believe it or not, some people still program these machines manually, especially in the Swiss world. It might take a week to write a program. But when that program is going to run continuously for a year, it's not such a big problem.

But really, everybody's better off going offline in a Cam system where you can program faster, with more accuracy, you have access to more advanced toolpaths than you could write manually, you have all of these moving parts in these machines. So it's really important that you can synchronize that motion.

Not only can you synchronize it in the Cam system, but you can verify it virtually to make sure you have no interferences and no collisions. And you don't tie up the control by programming. So even if you can edit and run at the same time, you're wasting time by standing there at the control programming manually.

And better yet, if you have a program in a Cam system and you decide to go to a different machine, you might have to make some adjustments with tooling or synchronization. But then, you can just post it out for that other machine instead of starting over from scratch, which you would have to do if you wrote the program manually.

So Turn/Mill definitely has some different pros and cons. The best thing about it is you have a single machine that can produce finished parts. You can do a wide range of parts. You can do them faster in less space. You have better utilization of your workforce because a single operator can produce finished parts.

You can automate these machines with bar feeders and part catchers so you can run lights out running those parts around the clock. And they're available in many configurations depending upon the types of parts and the type of workflow you employ in your shop.

Now, the cons are these machines are expensive. And the initial investment in tool holding, maybe tooling specific for your applications may be expensive. It does take more skill to program and run these machines. And set up can be more complex.

So in some cases, if you're running very small quantities, it might not make a lot of sense to run it on a multi-turret machine when you're only making one part. So to take this one step further, I'm going to send it over to Michael and he's going to go through a case study where he contrasts all of these different applications. So Michael, I'm going to throw it over to you.

MICHAEL GRENIER: OK, Thank you, Chris. As Chris said, I'd like to go over in that next section over a case study. So I'll go over two things, actually. So we'll start with a case study, then we'll be looking into what's coming into Fusion as far as helping our customers program Turn/Mill machines.

So first of all, let's start with the case study. So what I've decided to put together is basically the programming of the part we currently see on the screen. So I want to go over three different methods of programming or manufacturing that part.

So the first one is to use what we call a more traditional method, which would be by using several machines to cut the part that would be in this particular case using a two axis lathe, then a three axis mill, and finishing it off by a four axis mill for those 0D holes.

On a second time, we'll go into a single turret workflow. So this one would be single turret-- dual spindle, sorry, where we can produce the part in a single run. So the user or the machinist would hit cycle start on the machine once and that would produce one finished part. And finally, we'll dive into a little bit more complex machine where we'll be using a dual turret dual spindle machine. So let's dive right in.

So here we've got our live setup sheet that we've put together where we can see the operations being cut on the machine. As you can see on the right hand side, I've got the machine set up time set to 30 minutes. So just take this with a grain of salt. That's 30 minutes, that's an average that we've decided to put there.

It doesn't really matter for the exercise today, but we've set it to 30 minutes for now. So as I said, we did do the two axis lathe on this part and we are moving into the three axis milling on the second side of the part. And then, to finish it off, we'll go install that part back on to drill those 0D holes.

All of those operations will give us a total machining time of about 100 minutes, if I remember correctly. So 102 minutes for the first part, in this case. 90 minutes setup time, which is obviously most of the time that we would be spending on this part.

But then, where I find it interesting is when we go into small production. So for this simple part, we would be thinking about 1,340 minutes, let's make it 1,300 minutes for hundreds of those parts.

Now, that was with a more conventional workflow. If we look into using a Turn/Mill machine with a single turret dual spindle, then we would be looking at a lot more-- not cycle time, but a lot more machining setup time. Simply because the machine is a little bit more complex. The way the tools are set up, you don't have a carousel as big as you would on a three axis milling. So most of the tools have to be installed and removed between jobs, which makes the setup time a little bit longer.

But then, the machining only got one machine to produce the part. Now, if we take a look at what that means, we can see we've got, again, 120 minutes in set up time. But only nine minutes in machining time, which makes the first part take about 130 minutes in this case. We can also look at the full production of that 100 parts, which would be close to 1,000 minutes. So we did shave about 300 minutes in this case.

And then, finally, if we look at the more advanced machine, well, it's actually the most advanced will be taking a look at today. This one has two turrets. So it's a similar configuration as before except that we've got a lower turret. So what that means, similar to what Chris said before, is that we can cut with those two turrets at the same time.

So we end up pretty much removing completely one of the setup in terms of machining time, which greatly reduces the total cycle time. The downside of that is setting up the machine is a lot longer because you've got two turrets to look for when you dry run the program. You don't want any collision or any problems. So that usually takes a little bit longer.

So again, I did set up the setup time to be 120 minutes. It's just an average. It could be between an hour and three hours, maybe even more depending on the part complexity.

If we go back to the machining time for that first part, we're thinking about 126 minutes in this case, and around 770 minutes for the full production. Now, if you're like me, I'm pretty sure you did not memorize all of those numbers. So let's take a look at this little table here.

We can see, if we've only got one part to manufacture, Turn/Mill may not be the best solution. Where if you've got a Turn/Mill, it might be a good idea to do it depending on how your tools are standardized on the machine. But if they're not, then maybe the traditional method is a better idea.

But then, as soon as we move into smaller production, low volume, then it makes sense to go into single thread dual spindle machine. And for bigger production, like aerospace or automotive type of production where we're thinking about hundreds of thousands of parts, then dual turret with dual spindle makes a lot of sense.

So we can see just on 100 parts here, we were able to save about 24% using a single thread machine and 43% using a dual thread machine. So for me, that's the kind of stuff that I like to think about when I try to compare different types of manufacturing methods.

Now, let's move into what Fusion offers to our customers in terms of programming technology. Fusion has been able to program Turn/Mill for a long time, so that's nothing new. But in the last year and also in the upcoming year, we've decided internally to focus our development effort on Turn/Mill specifically.

The important part here is where we've been focusing our effort. Because Turn/Mill, as Chris said before, is a big word. So it means-- or encompass a lot of different machines. For this year and next, we've been focusing on single turret dual spindle machines, single turret single spindle machine, and finally, B-Axis, whether it's single or dual spindle machines.

So to help our customers be more successful into programming those machines, one thing that came up several times when we were talking to those customers was the tool creation workflow. So obviously, we've been able to create tools forever.

But we've added the ability to dynamically see the tool being updated on the screen simply to help customers zoom, pan, and scale the tools so that they could focus on a very specific area of the tool that is important to them when they're defining it. So that's something that just made its way through within the software recently.

Another part that we've been working on as far as tool definition goes is the ability to import 3D models. Defining tools is important. Well, we've seen on the previous slide that, most of the time, we use stick tools for turret. But if we look at the Turn/Mill and B-Axis at Turn/Mill, most of the time, we will have much more complex tool holders that are used to define tools.

So the ability to import a 3D models allows us to define those tools perfectly. But we're also looking at, down the road, the ability to support or define tool blocks. So that would allow our users to define, in this case, a boring bar and assemble it with a tool block to eventually be able to see a full machine simulation. So seeing the full turret, the chuck, and all of the moving components being simulated on this green to avoid any potential crashes on the machine tool.

Now, one of the process that is the most stressful for me when I think about Turn/Mill is material control. I like to call that part ending. So that is how we control how we move the part from one spindle to the other, or simply, how we pulled apart from the main spindle to give us a little bit more clearance.

At this moment, our users are struggling a little bit with that part because there's a lot of manual work involved in transferring the part over to the sub-spindle. Well, we've been working a lot for the past year on a new operation that is called bar pull. So that's the only pieces that was missing to that puzzle.

Now that we've got that bar pull function or soon to be released function, we'll be able to program the full sequence completely within the software. So that will allow us to program from the sub-spindle coming in grabbing the part down to cutting off the part and moving to the sub-spindle and having the material be ready for a new part to be cut on the main spindle without modifying anything manually in the code.

So that's what we've been working on. That was step one within that project. Because step two is supporting more advanced sequences. Right now, we-- with that new bar pull function, we have all of the pieces, like I said, if we need to define that full workflow. But we want to be able to define those more easily. At least, we want to be able to define some of them for our customers.

So that all of they would have to do is to get into the software, select the sequence they want to use, and that specific sequence would include the sub-spindle grab, the bar pull, the cut off, and then, the return of the spindle back home if we were thinking about a cut off transfer in this case. We will have many different of those options or templates available for customers to pick from so that it's a little bit easier for them to start with.

Now, when we say Turn/Mill, there is mill in that word, which means that there's a lot of milling involved. Many customers will have or will do Turn/Mill on parts that are way more milling that than they are turn, which means that we need a lot of milling functions to be able to cut those parts.

One that customers have been asking for for a long time is polar machining. So for people who don't know what polar machining is, it's the ability to convert the C-Axis of the lathe or the Turn/Mill into a linear axis, which could be a y-axis in this case. Not all Turn/Mill do have a y-axis, which is why it's important to support polar milling or drilling.

In this case, as of today, what we're doing, the post-processor is deciding whether it's going to use one or the other. But it's great to be able to do that at the interface to get a proper simulation. One detail that is interesting here is that this function will also be applicable to milling machines. So we can think about a five axis milling machine where we would like to extend our travel. Because one of the axes may have more travel than the other. And we could use polar milling for that too.

Another detail where customers have been requesting for for a long time-- because they've had it in milling for several years now-- is the toolpath modification. So we're already able to modify a toolpath on a milling toolpath. By modifying, I mean trimming it, modifying leads and links, and that sort of modification.

So we can optimize our toolpath to make it just perfect and remove any undesired segment within that sequence. We never had that available for turning toolpath, but this is something that is currently being worked on. So bear with us. It's going to make its way through the software hopefully next year. That's what we're aiming for at the moment, if I remember correctly. But it's going to make its way through the software soon.

Now, one thing for milling customers, milling users that we've seen being greatly enhanced over the last, I would say, five to six years, is the amount of five axis strategies that we do support within Fusion. We've got many new toolpath that supports five axis simultaneous. We've got new five axis strategies that are available.

By five axis strategies, I'm talking about the way the tool moves around the part. Now, that was good for five axis milling or B-Axis type of Turn/Mill. But it didn't help too much for four axis Turn/Mill, so more simpler-- simple turn mill.

Now, we have been working-- we are working on four axis simultaneous. So that's basically just locking an axis on those five axis strategies. So once we release the ability to lock an axis, pretty much every five axis strategies will be able to be locked and convert into four axis, which is going to greatly increase the amount of strategies we've got for four axis as of today.

And the last thing that is coming into the software eventually is a better wrapping tool path. So we've been able to wrap for a long time. Most of our customers have been happy about it. The only problem I personally saw about our current wrapping strategy is that, most of the time, the geometry had to be already wrapped onto the 3D model, which was not always easy for customers working on Turn/Mill that were in the needs of engraving a part number or something like that on the part.

So having that geometry already part of the 3D model was not always possible. Now, there are ways in Fusion right now that we can draw a sketch-- a 2D sketch on the Fusion design side and use that sketch to convert it into a wrapping tool path. But it's not so easy and it's not everyone that knows about that. So we are currently looking on making this more accessible to everyone. But also, increasing the amount of options we've got within our wrapping strategy.

So that's what concludes my section. On that, I'll end it over to Matthew Yates from Rivian to talk about how they're using Fusion at their facility.

MATTHEW YATES: Thank you, Michael. My name is Matthew Yates. I'm going to give you a broad overview of Rivian and how our CNC and additive departments fall into the organization and how we use Fusion and our five axis milling process before I pass you off to Josh Postell who will focus on Turn/Mill initiatives he has been working on.

I'll start with a brief overview of Rivian for those who haven't heard of us. Rivian was founded in 2009 by R.J. Scaringe. We develop and manufacture our R1T electric pickup truck, R1S electric SUV, our electric delivery van, primarily for Amazon at the moment. We have headquarters in Irvine, California and an assembly plant in Normal, Illinois.

Our CNC and additive department fall under the prototype and special projects division of Rivian. We are located in a couple of different places around the country. I personally am out of Plymouth, Michigan. And we have another team that works out of Irvine, California.

Prototypes and special projects provide prototype parts. We build mules from the ground up including suspension and frame components. We also modify vehicles to support special projects such as the Maasai Wilderness Conservation Trust.

We provide production plant support in terms of assembly, jigs, and fixtures, rework or up rev production components, end of arm tooling, and emergency breakdown support as needed. For those who don't know what a mule is, in the automotive industry, it is a test bed vehicle equipped with prototype components requiring evaluation. So it could be a close representation of a vehicle or it might just be some of the physical components that make it function.

Under prototyping special projects is our CNC and additive department. Our additive department comprises multiple locations around the country, including Michigan, California, and at the assembly plant in Illinois, which allows us to provide just in time support for our production and engineering teams.

We use the latest equipment from Stratasys including their FBM, SLA, DLP, polyjet, and powder bed Fusion technologies. In this image, you can see Zach removing a 3D printed part from a Stratasys F900 FDM.

Our CNC department has five CNC machines, including DMU 95 and 65 full five axis machines. We have a Haas VF3 with a TRT210 axis trunnion. We have a DMG ALX2500 lathe with live tooling and a C and y-axis, and a large format for the three axis VMC for larger components.

We also have a small laser cutter processing sheet plastic components. And we are adding a large five axis laser for sheet metal parts.

We use all this equipment to produce a large array of components for upcoming projects. This includes assembly jigs and fixtures for the plant, frame and suspension components for new products made from 4143 hardened steel or 7075 billet aluminum. These components will only be used on the mules as we don't make any parts for the production vehicles.

We do, however, take on rework of production components, including machine and sheet metal parts. These components are occasionally reworked due to design changes as our product matures.

We also produce a variety of cases, covers, housings, or a general sample part for testing, and low volume sheet metal bending dies. We use a variety of fixturing to hold the wide assortment of parts we produce. From a simple plate with tapped holes for flat clamping of parts or a standard machine vise, to five axis centering vises or collet blocks for holding clinical features.

Five axis centering vices are most commonly used as our goal for every part is to complete 90% of the features in a single operation. This will often involve removing so much material that the part is left with a small tab on an insignificant surface, which can be broken off and machined or sanded down. As you can see in this video, this part is hanging on just by a thread of a tab that was left.

By all the pictures I showed in the previous slides can be mounted to a standard mounting plate. These mounting plates are attached to each machine, which allows us to quickly move the fixturing to any machine depending on the requirements and workload.

All of our five axis parts are programmed from a common origin point, which is usually the top center of the turning. This allows us great flexibility and quick change over time switching between projects. It eliminates the majority of probing, raw stock in the machine, which can be a time consuming process.

We use Fusion 360 to program all of our CNC mills. We use Autodesk CAMplete for five axis toolpath verification on this equipment. We also use Fusion 360 to program our four axis lathe with some manual adjustments. Because there is not a great verification solution for this equipment, we have to be very careful and are always starting and stopping the cycle to make sure we are avoiding collisions and the machine is moving where we expect it to.

My co-worker Josh will follow up with some of the challenges he has faced with Turn/Mill. We have accurately modeled our physical tooling in the virtual environment within Fusion 360. This axis centering vice jaw positions are controlled with user parameters to position the jaws. We import our part and position it within the stock, then build a stock support, which allows us to reliably machine our part without fear of machining into the workholding fixture. The more accurate we are with the build up of our stock in Fusion, the more reliably we can verify for collisions.

We use CAMplete for a toolpath verification on the mills, which also checks for collisions and overtravels. Some might question why we use CAMplete when Fusion has built-in machine simulation. I personally prefer CAMplete standalone solution. I find it faster, more accurate, but most importantly, I can run it concurrently with Fusion.

For my workflow, I can post a CAMplete, fire for a couple toolpaths, send it to the machine and get the machine running. I can continue CAMplete's verification while the machine is running and still go back to Fusion and create more toolpaths.

If I use Fusion stimulation, I need to wait for Fusion to finish and I wouldn't be able to work on toolpaths concurrently or post and the machine would not be operating. The Fusion team are always working to improve the software and machine simulation, and obviously, it's been worked on by Cam engineers. So maybe one day it will work for me as an all in one solution.

So how does Fusion compare overall? So I've been around this industry for over 30 years as a machinist. I've use Cam software for 25 years. Not Fusion, I used a competitor's software. It got the job done. I use PowerMill for two of those years and then back to the competitor software after a job change. It wasn't by choice, but a competitor software was dominant in the area I lived in and to get my parts completed.

I worked for Rivian for one year and they used Fusion exclusively. I was apprehensive at first of using Fusion. I considered it more of a hobby software. And coming to Rivian I thought I would lean more to using PowerMill as it was an option presented during my interviews.

I picked up Fusion within a couple of weeks making some fairly complicated parts on the five axis equipment. I feel sufficiently near the majority of the function needed after a few months, but still found it lacking some of the newer toolpaths. Now after one year, they've included most of the functions I felt I was missing from previous software and made it more reliable. At this point, I haven't had a part I couldn't manufacture using Fusion 360.

And thinking back to parts I've made in the past, I'm sure I could produce those parts within Fusion. I do still have some trouble with larger files. Processing times for rest adaptive toolpaths can sometimes take 15 to 20 minutes, depending on the geometry.

I am missing some of the functionality that was in PowerMill. But I can honestly say there is nothing I'm missing from the competitor software. And overall, I find Fusion 360 a very capable and easy to use software and it provides great value. And now, I'll pass you off to Josh Postell to talk about how we use Fusion 360 on our Turn/Mill machine.

JOHN POSTELL: Hi, everybody. My name is Josh Postell. I work with Matt in prototyping special projects. And I'm going to walk you through some of my processes and how I utilize Fusion 360 for Turn/Mill.

So in prototype special projects, Matt talked about a little bit what we do. We make pretty much any physical prototype all over the car. This could be anything from suspension components to what you see on the screen, this little flashlight that sticks in the door.

One of the cool things with doing projects like this is it's such a simple project, but it's implemented into the car and kind of stays true to Rivian's goal of staying adventurous forever.

So heading over to our DMG ALX2500, the main reason I showed you that flashlight is because that's going to be the project that I'm going to walk you through how I made that. Deciding on what software to use when tackling mill through Turn/Mill, something that we realize is we already had a lot of our processes down for Fusion 360.

As you see on Matt's slides, we did all five axis milling off Fusion 360. So heading over to the lathe, it was a little bit more comfortable. I've also used Fusion 360 since 2015. So I'm familiar with it. I understand how easy it is and how intuitive it can be to tackle a new project and how everything's broken down. So I'm glad I did and made that decision. I have only been programming lathes for about a year now. So kind of shows how intuitive Fusion can be for learning new things.

We use a Collet chuck system. So this is a quick change Collet chuck. It's all standardized sizes. So we have half inch, 3/4, 1 inch. This can make ordering material a lot easier instead of having to order specific size or trying to get as close as possible. It just makes things a little bit more streamlined.

Using the centralized work coordinate system, you can see on that picture our z-0 is actually the front of the collet. This is going to save me time every single time I'd throw on a new part. Working in prototyping, I might make two, three, four different parts a single day. So having to pick up 0 on every single part does start to add up in time.

This also having a template set up in Fusion 360. I can just throw in my model and I don't have to worry about creating a fixture for every single job. I can already have my environment set up right away.

Heading into parameters, so on top of having a template, I have parameters set up to be able to change my stock diameter and stock stick out length. So again, I don't have to model my stock. I can just go ahead and type in what I'm going to be throwing into the machine.

I've noticed, too, this also reduces the risk of error just because whatever number I type in there, if I type in 3 inches for stick out length, I just need to make sure that's what my stick out length is on the physical machine. I've had it happen multiple times where I go to pick up z and then I mess up a number somewhere or I change an offset and I go to run the part and it doesn't line up. So having everything based off of one coordinate system can save you.

Having even more automation, so having templates set up in my main template file. So everything I start from comes from the single file. I have toolpaths ready to go. All I have to do is click my setup, select my model, and now I already have a rough template for my roughing toolpaths.

You can see this is a recurring theme, which is just having templates set up to save time and just having to make one or two selections. This is crucial in a prototype space. If I spent all day making a new file for every single part, it would be my entire day.

Now we have our fixture in place with our stock. Go select the model. And now, I can have all of my toolpaths automatically generated. So all my parameters and geometries selected is based off of my stock. So it's either model front or stock front, stock ID. And this is going to be able to make it. So I don't have to even open those toolpaths. I can just go ahead and click Generate and get roughing.

Similar on a mill, this saves a lot of time because roughing isn't very accurate. I just need to get some toolpaths laid down so I can start running the machine while I go back and fine tune those finishing toolpaths or some of those pockets that you see on the side there that isn't automatically generated.

Getting into the more advanced operations that Autodesk is currently developing, such as operating the sub-spindle. I use even more templates in NC Commands. So when I select one of these templates, it imports a variety of toolpaths, including a lot of pass through NC Commands.

Different combinations is going to give me a different result. If I just need to use a sub-spindle as a tailstock, there's only going to be one command in there. If I'm doing a bar pull function, there's going to be multiple.

Because of all the pass through NC code, I have to manually do a lot of this math myself and then actually open up the pass through NC code and change parameters to what I need them to be. This is not ideal. There's a lot of error that can happen here just by even messing up one number.

If I have to change something, I can't just move a certain parameter. I have to actually go in, do the math again, and then, see what else that might have changed down the line.

So there's two main functions that I use a sub-spindle for currently, bar pull, as Michael touched on. So I can machine a part, have the machine part it off, and then, have the sub-spindle come in, grab the part and pull it out so that way the stock is left exactly where I need it to be for the next part.

And then, I just go ahead and loop that with a M98 command and I can have 10 parts out of one piece of stock instead of having a bar feeder. Not having a bar feeder saves space, but it's also cost effective if you can just utilize your sub-spindle if you're making a few parts.

I can also, as you're going to see with this flashlight, grab the part, cut it off. It'll actually pull the stock out a little bit more so the stock will be-- the stock remaining will be ideal for the next operation. Return home and then switch to G55 and use backwards tooling in the machine to drill and tap the holes in the backside.

Currently, there's no good way to simulate this. You'll see in the next slide. Once you start using pass through NC Commands, Fusion doesn't know what's going on. So even though I have it programmed to come in and grab the part, pull it out, Fusion doesn't understand that. So if I simulate anything past that point, it's actually going to be machining places where the model doesn't line up.

Again, with all this handwritten math in here, there's a lot of error that can be had. One wrong number can mess up everything. And without the way to simulate that, you can't really tell until you go and cut the part.

Here's a quick video. You can see our Collet chuck set up in there. Notice too we are running this dry for video purposes. So the finish isn't going to be exactly what it would be if we were running with coolant and you'll see some pictures at the end.

We have all of our Collet standardized. So this is 2 inch stock and everything is going to be based off that. Sub-spindle transfer, it's going to pull the part out a little bit. It's going to come in, cut this off, and then return home. And it's going to begin roughing a separate part. This is going to be the end piece of the flashlight.