Partnering on 40+ Autodesk Fusion 360 CAD CAM Tips in 60 Minutes

SCOTT MOYSE: Thanks for tuning in today. So this is my recording of the class that I'm going to be presenting or presented at Autodesk University in 2023. So roughly 40 tips delivered over the next hour. So the four objectives we're going to be covering, so get some CAD techniques delivered, some tips and tricks, that can help improve productivity, but also, of course, into the CAM workspace as well.

We might learn about some new features that you haven't discovered yet. And there's some real magic available when you combine CAD and CAM together parametrically across milling and turning, so you'll get to see some of that. And then explore some of the power user knobs and levers in Fusion 360.

So what do I know? I've learned a few things over the years. I did nine years using Inventor and Vault Professional in the superyacht industry here in New Zealand. And I first started using Fusion 360 when it was a Labs tool which was probably 13, 14 years ago now. And for the last 10 years, I've spent my career working as a tech for CAD Pro in New Zealand and Australia using Inventor, Fusion 360, and also Vault, but these days, mostly Fusion 360 on the CAM side of things and develop post-processes for CNC machines.

As a little bit of a side hustle, I presented a class last year about that Grumpy Sloth mechanical keyboard project. And so any time I get to design and make real parts these days other than helping customers with their parts. So Autodesk required me to include this Safe Harbor statement. I'm not showing you anything that's under NDA today. Everything that I'm showing you is in the release product, so you're all good there. All right.

So the idea of this class was I've done a number of tips and tricks classes over the years. And it was suggested to me that it would be neat to demonstrate some of the prowess or skills that are available in Autodesk's partner networks. So there's a lot of solution providers, as we call it these days, around the world with a lot of embedded knowledge that's local to Autodesk customers.

So I reached out to a couple of friendly resellers. And so I'm from CAD Pro, and then we've got Design and Software International, DSI, a US-based manufacturing-focused reseller or partner. And then CAM Consult is a Netherlands-based partner and a man called Ian who runs that business. So I'll be presenting some of their tips through this presentation.

So in the top left-hand corner for each slide is who has contributed the tip. And so in this case, we've got Devon Dupree from DSI. A lot of traditional desktop applications, when you're in a command, if you press F1 on your keyboard, it loads up the help file. And so traditionally, that would have been local help and more recently, now, in the browser. But Fusion 360 works a little bit differently. If you click on the Black eye icon in the bottom left-hand corner of the dialog, you can expand out some additional information and get some tips in Canvas. But if you need to know more, you can click on the More information button, which will then load up a web-based version of the help which is far richer in content that you can then follow along with.

So this one's one of mine. We have tool paths like face and parallel as a surfacing tool path. There's an orientation setting on the Passes tab that defaults to zero degrees. Often with certain types of geometry, you end up having to measure or guess what that angle is to get the tool path to follow or flow or move along that path in a favored direction. So what the zero degrees actually represents is zero degrees relative to the x-axis.

So you can hack that by or take advantage of that behavior by using tool orientation and aligning the x-axis to a reference on the model. And so in this case here, with this 3D form, you can pick an edge on the model.

Now, if there's an edge that's not perfectly aligned or it's not a straight line, then you won't be able to select it. But you can create a sketch and then project that potential spline curve up onto that sketch, mark it as construction. And then draw a line between the endpoints, which gives you effectively a best fit curve or a best fit line to the curve. And then your tool path will align as best as it can to that geometry. So as you can see here on the right, the tool path moves in a much more favorable way than it does on the left. You're going to get a much nicer surface finish.

Control your wedgy. All right. So turn mill machines, most commonly when they have a y-axis, have got the x and y-axis linear rails don't sit at 90 degrees to one another, which means that your bounding area or your machining area in the xy range is not rectangular. And the post-processor, the Fusion 360 post-processor, will accept input as a property for min-max y-axis-- and I've just realized that I've made a typo with my label there. So the green is actually my y-axis.

The post will allow you to input a max y, min y, and then a min x. But so the post assumes that the boundary is rectangular. The reality on the machine is not. So the problem is with that is you can end up with overtravel alarms on the machine. So to add some confusion here, the way different machine tool vendors specify their min and max y-axis travel varies. Some will state the travel at the top end of the x-axis and some will state it at center, so at x0. And they can be sometimes symmetrical or asymmetrical.

So the only true way to find out for sure what it is to go to your machine and move your tool to the zero-zero position in x and y for your active coordinate system. So most often, that would be your spindle center line. And then jog the machine over to max y then up to max x so we end up in the top right-hand corner. And then move as far as you can in the negative direction in the y until you hit your limit, and then take note of what that value is. So there'll be a coordinate relative to the origin.

Then move back to max y, all the way down to min x, and then across negatively in the y again until you find the negative y position at min x. At that point, you've found all four corners of the boundary, and you'll find that there's a straight angled line which chops through the rectangular boundary as defined by the limits set in the post properties. So you end up with this triangular area here, which the post will allow the toolpath to be output in xy coordinates. But once the tool reaches this area on the machine, you'll get an overtravel alarm, and the program will stop, which is not desirable.

So one way to stop that is to reduce your min y and min x to bring this corner up inside this boundary, but then you end up with a much smaller boundary area for x and y motion and the post will go into polar mode more often. So I include that sketch in my CAD/CAM turning template along with my spindle and chuck jaws and all the rest of it, and then create a patch surface off from those sketch profiles and color them. And add some sketch text to describe what the areas are.

And then when I'm in the manufacturing workspace, I can look straight down the spindle axis and highlight a toolpath and see whether the toolpath actually encroaches on that area or not. And then make a decision about how I want to handle it. And if you have a look in your turnmill post, most of them have manual NC actions that you can use to force a toolpath into polar mode or x at C mode, even if it could fit the toolpath within the xy boundary.

You can-- this is one of the bonus tips in the handout-- is to convert those manual NC action statements into operation post properties. So that in your milling toolpaths, this additional dialog will appear here, and you can choose which mode to use for milling on that particular toolpath. So in this case here, even though the toolpath-- because the toolpath fits in within the post-processes rectangular boundary, it will alarm the machine. We can force it to use polar mode, which means that the control on the CNC machine will be doing all of the polar coordinate calculations. Or we can do force x at C mode, which the post will effectively do polar coordinate calculations instead of letting the machine control do it.

However, because we are in an integrated CAD/CAM environment that's got parametric features, we can select the component and use the Move Copy command to rotate a part within that boundary. And we've got a nice visual to be able to do so. And luckily enough, this particular part does fit within that range. And then jump back to the manufacturing workspace and regenerate the toolpath, and we can now see that it fits. So what you're effectively doing is rotating the part around the c-axis and creating a c-axis offset. And so you could either do this in CAM or you could take that rotational value. And if your control supports it, add a c-axis offset into your work coordinate system offset table.

All right. So peer inside the abyss. Another kind of behavioral trait you can take advantage of is that when you generate turning toolpaths inside Fusion 360, it does so based off of a spun profile. And it basically creates a section sketch, and that sits on the xz plane of the setup. So in your template, in your CAD/CAM template, you can create a section analysis view on the xz plane.

So if you've set up your work coordinate system to match the model origin of your document and align perfectly, then you can just pick the origins xz plane. And then when you turn on the section view, it will section along the same plane as the toolpaths are being generated from. As a bonus tip here, if you can't select the plane you want, you can left click and hold. And a little dialog will appear, and you can pick the occluded or hidden objects from that list for your selection.

One of the really nice things that you can then do is if you are doing internal turning or clearing extra material from the bore of a part, it's often really handy to be able to look inside and see what's actually happening, check clearances with the boring bar, and so on. So you can turn on the section view in the middle of stock simulation, and it will section the stock as well.

All right. Chamfer any angle. So there are now quite a few different ways of being able to deburr or edge break parts in Fusion 360. And the Deburr command is the best one really it's super automated you can also do undercuts with it if you get your lollipop or chamfer mill tool set up correctly. But it is in the machine extension and not everyone has that. So if you do want to do edge breaks like in this o-ring groove here inside a bore, then you can just Google undercut chamfer CAD Pro and you'll find my blog post that details how to do this, or you can scan the QR code that's on screen at the moment.

The blog post fully details exactly how to do all of this longhand, but there's also a few toolpath templates that you can download. The one for HSM works in Inventor, CAM, and another one for Fusion 360. So if you download that and add it to your template library, you can then modify the tool to suit. And the cool thing about this is that I've just used trig to figure out what the radial and axial stock to leave needs to be to achieve the chamfer width size you specify in 2D contour.

And it doesn't matter what the angle of your chamfer mill is, so you can use a 60 degree thread mill if you want to edge break. It will just take that angle value from the tool, and then do all the math to figure out what the offsets need to be. So you end up with a couple of clicks, and you get perfect undercut edge breaks all the time.

All right. Any CAD is a feature that's still not known to an awful lot of Fusion users. You have to go and enable it in your Fusion preferences. So if you go in the top right-hand corner of Fusion, click on your profile dropdown and go to Preferences. And then in the Design tab-- so in the Preview tab, you can then go and turn on Any CAD.

Now if you just upload third party files or generic CAD files, like SAT, IGES, STEP, to Fusion 360 through the Data panel, then it actually converts the file to a Fusion design. And that's not what you want to have happen to use Any CAD. So the correct way to upload those files is to do so through the Fusion Team Browser. So just go to your team site in whatever browser you use. Or you can download and install the Autodesk Desktop Connector, and then you can navigate through your team structure folder structure within your operating system and save files into it there.

So when it just uploads the files and treats it just like it would if you uploaded a file to Dropbox, Google Drive, OneDrive, whatever. If you upload another copy of the file with exactly the same file name, it will create a new version. So if your customers or supplier or internal team member sends you a new file, if you just upload it again, it will version it. So it will go from version one to two to three. And the effect of that then is that if Fusion is using it or see there's a new version available and prompt you to update it.

So yeah, you can do this with SolidWorks files, Inventor files, Catia, NX, Solid Edge, and STEP files. And once you do that, you'll see it appear inside the data panel. But it'll have a different icon. It may not always have a thumbnail until it's been opened and the thumbnail has been generated. But the file extension is still there as well.

So in this case, we can still see it's an Inventor IPT or a part file. And when you right click on it, you can choose Open or Insert Into Current Design, just like you can with a Fusion design file. But the difference is if you open it, it just creates a new untitled design document and then inserts a component link into the timeline down the bottom, which is very similar to a derive reference if you've ever done any deriving inside Fusion. I'll touch on deriving a little bit later on.

If you Insert into current design, it'll just Insert it like an additional component just like you would if you insert a Fusion design into another. And you end up with a component icon with a chain link on it in your browser. My preference, most of the time, is to use Open because it will create, and I just save the file name with the same file. So in this case, I'd name it Naca 0012 profile, and it'll be the Fusion 360 document version of the Inventor file.

And the reason why I do that is because I can then modify or add geometry to the component, whereas I can't do that if it's an inserted component. So I can defeat or I can create copies of the bodies. I can create a stock version of your pre-machined version of the model or whatever I need to do.

The huge benefit here is if you are using this within an assembly design of some kind, then you've got joints or you're creating sketches and building off of it or you're doing manufacturing and you're generating toolpaths on it, if the geometry changes, all of that updates. Of course, if you've referenced a pocket, so you've created a joint that uses the face in a pocket or you've generated a toolpath where you've selected that face in the pocket, and that face gets deleted in the newer version, then you'll get some kind of failure. And you'll need to act on that.

But if something changes or, again, in Fusion CAM, you've got some feature recognition, it'll pick up on those changes and just generate the toolpath. So you will have to do some work to fix things up. But the major gain here is that a lot of the things you won't have to redo, they'll just change and adapt. So it's a no-brainer time saver. Everyone should be using it as much as possible. You can always just suppress the link or break the link if it's causing problems later on. But as a starting point, it's kind of an insurance policy. It's going to give you a chance to save some time down the line.

All right. Fix your turn. So there are now a lot of simultaneous four-axis toolpaths in Fusion 360. But what's not super obvious is that now we've got all of the five-axis tilting from PowerMill in the HSM three-axis surfacing toolpaths. We can actually force it into four-axis mode. And so this is steep and shallow as a pure four-axis output. Fundamentally, steep and shallow is a three-axis toolpath that has five-axis tilting within it.

So the way you do it, so if we think about a vertical machining center where the tool spindle points towards the ground, and then you might have a fourth rotary axis on the table and we might call that an a-axis. And so we can have, just like you saw in that previous video, something turning around the x-axis. Then the way you set this up is the setup itself, you align the z-axis to suit the machine. So in this case, you'd point the z-axis towards the sky because it's pointing towards the tall spindle.

And then within the toolpath itself, you enable tool orientation. You align the z-axis along the rotary. So now we're pointing parallel to the floor or the machine bed. That means that when the three-axis toolpath is being generated, it's looking down the new z-axis, and it's kind of like a waterline toolpath. So it will take slices of the geometry as you move down in the z-axis. Which means if there's any undercuts, the toolpath that you're using needs to support undercuts. And then some of them in the Passes tab, you'll have to go ahead and turn on the checkbox for it to go into undercut mode.

Then on the Multi-axis tab, you need to set the machining type to five-axis and the primary mode to lead and lean. Once you've done that, the Override Tilt Angle option will appear. Turn that on, and set the preferred angle to 90 degrees. That forces the tilt to stay at 90 degrees and then the turn, which is around the rotary or the a-axis, can then just turn continuously. Now this will work with a whole host of three-axis toolpaths now. So you've got a lot of options for simultaneous four-axis these days.

There are plans to make this more accessible. But at the moment, you basically have some switches that configure all these settings at the box. But for now, you can access this behavior by using these settings.

All right. So this one's from a good friend, Angelo, from DSI. A lot of people don't realize that the rectangular pattern tool doesn't have to be a rectangular pattern. It should really be called a linear pattern. So really all you're doing is inputting two vectors into it, and they can be at any angle between them. And so in this case, we've got a 60 degree angle. We've just selected two edges, and it's patterning along both of those. And now the cool thing is this also works, not just in the design workspace, but toolpath patterns as well. So you can use the same parameters effectively to mimic the same pattern across design and manufacturing.

All right. So stay the X down. Now, you can use this for x or y-axis. But a lot of the three-axis toolpaths in the Linking tab have their maximum stay down distance parameter which basically tells the toolpath how much it should stay down within a distance. So if it goes over that amount, it'll retract and reposition instead of staying down in the pocket or in the cut. So you can set defaults in Fusion. And by default, this is some other value. And in this case, we want it to always stay down for the full distance of the stock along the x-axis.

So if you mouse over any field inside Fusion 360 toolpath, be that an input field or a dropdown, you'll see an ellipsis, a vertical ellipsis, or kebab icon appear to the right-hand side. If you click on that and then select Edit expression, you can start typing in a parameter. So as you start typing, it will auto complete, and you can then just pick whichever parameter you want to use.

Now StockX, stock high, stock low are computed parameters from the setup. So based on whatever the stock definition was, these values will adjust. If the model size increases, for instance, and the stock size increases, these will get updated. So if you use StockXHigh minus StockXLow, you'll get the overall stock size in the x-axis. Set that as a default. The tool will always stay down in the job for as long as it can or will retract and reposition if it needs to avoid obstacles. But it will stay down as much as it can. It's the kind of thing that you have to decide on whether it's appropriate for your machine or not. But for a lot of machines, they would prefer to stay down.

OK. So it's OK to be picky. So if you're not using your selection filters yet, I highly recommend you get used to using them, and they're a huge time saver. The biggest trick with them is to remember you got them turned on or off. So you'll often find yourself in the beginning, find yourself frustrated that you can't select something on the screen, it's because you haven't reset your selection filters. But here you can choose which object which object type and whether or not to select through or not. So select through will select objects which are occluded by others. And then you can use your window selection to just select those object types in bulk.

As a bonus tip, when you window select from the top left to the bottom right-- and I'll just show you quickly in Fusion here. If you window select from the top left to the bottom right, then you'll see I'll get this orange color. And I have to window select everything in its entirety for it to be selected. Whereas if I go from the bottom right to the top left, it will select anything it touches.

All right. This is a neat idea from Devon at DSI. Structural drainage. So this is if you've got the Product Design extension, you can use the Volumetric Lattice command to select a modeled body and create a lattice that fills that volume. And you can then use the Offset command. And here, we just set our selections to faces only and then windows selecting across the center. I've accidentally picked up the bottom face. If I hold down Control and then select, it will deselect that one face. And I can choose a thickness to offset from. And we'll just pull that mesh inside. So I effectively have 100% fill around the outside of this for structural reasons. And then I have a lattice infill.

So you could use this if you were 3D printing fixtures on your machine. It could be a nice way to allow coolant to flow out the bottom of the fixture or like a vacuum suction cup or something like that to create airflow. Yeah. It's a nice little feature. So you can then convert this graphic mesh into an STL mesh, convert the mesh into a b-rep body, and then do a combine Boolean to add it to your main body, if you want, depending on what process you're going to use for manufacturing it. So keep it stupidly simple.

All right. So this is a setting you have to turn on still, I believe. So if you again if you go into your Preferences. So in the top right-hand corner, go to your profile icon preferences. And then under Design, you'll find-- maybe they have just-- Fusion has just updated today. And it looks like it is no longer there, so it must be on by default now. But anyway, simplify and arrange.

So under the Modify dropdown, you'll have most of the way down, Arrange and Simplify. If Simplify isn't there, then it's because your timeline is turned off. So to get that turned on, you need to capture design history. So you right click on the top node in your browser, the very top node, and you'll find Capture Design History at the bottom of the context menu. Enable that and Simplify will appear in your modify dropdown.

It's kind of ironic that it works that way because, certainly from a manufacturing context, if you've been sent a step IDS SAP file, when you import those into Fusion and it converts them into a Fusion design, the history, the timeline is off by default. And it's often, in those cases, where you would want to use Simplify to de-feature and clean-up a model that somebody's sent to you for manufacturing. So another reason for using Any CAD because if you open one of those files, it creates a new design document and the timeline's turned on. Yeah. So if you don't see Simplify, enable design history.

And once you've got it going, it's a good tip from Devon here is for big complex models, just turn Select All off before you select the bodies that you want to simplify. So it doesn't try and find all of the features to remove in one go. Then you can just selectively turn on the features you want to remove and adjust the Feature Size slider to filter out, in this case, the holes, because I want to keep those in my model. A bit of a weird UI. You've got to click the red X to apply it. There's no OK or Apply button. But the good thing is it then stays open so you can do a different set of de-featuring.

All right. So simplify your machine. So if any of you are machinists and you've got 3D models of your machine and you're about to buy a machine and you've negotiated to have your machine model included in your purchase or your OEM just happens to supply them for free, then you can download and open them up in Fusion. Now invariably, they are way too complicated. There's way too many components, way too many geometry features in there that beyond what you need for machine simulation. So we need to simplify them.

So once you've got the model opened up inside Fusion, if the timeline is turned on, turn it off, and then go through and create logical machine components. So the component structure will be based off of how they need to structure it for manufacturing and assembly purposes. We need to structure the model to suit how we're going to build our machine.

So we go through and create a base component, XYZ components, for the linear axis, then all of the components you need for the rotaries, and maybe also one for the enclosure for the sheet metal worker in your machine. You then go through and set your selection filters to Bodies Only. Window select those bodies. Turn it on and off the original components as you go. So you're only selecting the bodies you want for this new logical component.

You cut and paste them into those components. And then using various modeling commands, clean them up. The goal at the end of the day is to have one water type body inside each component. You might need to turn on and off the timeline at various points as you go through and simplify your models inside those components. Sometimes, you'll use Remove Features, and then other times you can replace certain groups of bodies with a primitive.

And you want to turn off the timeline to clear out any features that you don't need anymore because you're not going to be modifying this stuff. It's just to clean up, and it's a static model at the end of the day. And another tip is to, if you delete a face or you've got a solid while you've got the Surface tab active, it won't repair the solid it. Will just leave a hole where you deleted the face. And you end up with an infinitely thin surface body. And then, again, once you've finished everything, just turn on the timeline so any additional modifications you make after that are captured and you can see them.

A good tip through all of this, as well, is to turn off Drag Components. So make sure that's not enabled because you can accidentally move components relative to their neighbors when you don't want them to. So then your linear axis might be in the wrong place for your machine. So there's a quick video highlighting that. So this is just an import straight away. Timeline's turned off, got complex set of component structures on the left. I'm just going through and creating all my linear axes xyz and then my B and C rotary components. I also had a base component, which is used for all of the parts that don't move.

And then I can set my selection type to Bodies and just control turn off the original components that aren't being used. So I can only see the ones that I'm wanting to move across. Cut and paste into the new components and rinse and repeat. And you can really see the effect of this when we get to the cover. So then we delete all the components we don't want. Then the cover, there's hundreds of bodies in there. Cut and paste, and you can see that in that complex web of components, all of the bodies have been removed because they now just sit inside the cover's component.

So once that's done, you can go through and activate each individual component. And the goal is to get each one down to a single body. And in this case here, we can see we've got some sheet metal components. So we've turned on the timeline, and we're going to use Replace with Primitives to replace those bodies with a single cube effectively. It does end up adding the simplified primitive into a subcomponent, so we just need to cut and paste that out and delete the simplified primitive component. And then we've got three bodies that we need to combine together.

The last one is not combining, so there's a slight gap. So we use Push Pull to get an intersection so that when we combine them together, they actually join. This spindle housing's an interesting one. It's quite complex, but there's only one hole in it. So I create a sketch and project through all of the faces and then use the patch command to fill that up. And then you can use Boundary Fill to window select all of the different body surfaces and solids and just fill all the voids. And then go on to use the Featuring tools to get rid of any unnecessary geometry.

At the end of the day, the goal here is to reduce the number of faces that need to be converted into STL facets for machine simulation. So the simpler the geometry is, the more performant your machine model will be. Here now, I'm just using Select Through Faces, so I'm using Select Through because I want it to pick up on all those vertical faces and then just deleting them to get rid of those pockets.

All right. So this is a neat one from Angelo, again. Suppress the WiggleWiggle. So anyone who machines parts, complex parts, and certainly in a prototyping or job shop environment, low run type environment, as you get towards the end of machining your part, you need to still hold on to it in a rigid way. So in the design workspace now, there's this funky looking icon up here, and it's for automated modeling. So all that you need to do-- what it does is it just joins together different parts of geometry so you don't have to model that geometry.

At the end of the day, all we care about is having some geometry here to keep things connected, but we don't really care what it is because we're going to get rid of it in the end anyway. So it generates different connection types. So for every set of inputs you give it, it will generate six alternatives. Three of them have got smooth connections, and the other three have got sharp connections. And once they've generated, you can adjust the volume of the individual bodies using a slider.

So the idea here is to select the faces you want to connect, and then you can optionally include a body to avoid. And typically, the body to avoid will be material you want to remove and machine away in this context. Non-selected faces on the connection bodies are also avoided in addition to the selected avoid body. I've certainly seen it put material on those faces, but you can definitely see that it does try and avoid them most of the time.

All right. So you do not want to have meshy imports. So don't upload mesh files via the browser or data panel. Use the Insert Mesh command instead. It gives you the opportunity to set the unit type, which is really important when you've got meshes that have been exported from a product that don't write the unit type into the metadata for the file. So you need to make sure you get the units right. And once it's imported, you'll have a nice clean reference. It also allows you to Insert those from disk so you don't have to upload them first. So it's a much quicker way of doing it.

You can actually create a BREP, a proper solid, from an STL if it was originally created from prismatic source. So you use the Create Face Groups command to do this. When you preview, if you don't see the colors, like I didn't, use Shift F to display the groups. And just play with between the Fast and Accurate settings to get the optimal result.

Then you can use the Convert Mesh to BREP command using the prismatic method. It's important to use the prismatic method. And it will look at those face groups and build out a series of BREP faces so you get a nice clean model that doesn't have a whole heap of faceted noise on it. Prior to this, you'd have to go through and delete those individual triangular faces and have it healed a solid again. So this is just a much quicker and more intelligent way of doing things.

All right. So on the call that I had with Devon and Angelo from DSI, Devon pipes up and showed us this. It was a different model to this but a complex mold tool component or model. And asked us, I think he said, if you wanted to leave like 20 thou over the entire model, then how would you do that? So I'm a metric man, so how would you do this with leaving half a mil everywhere?

And none of the options we gave were going to work. There's no easy way of doing this with modeling tools. And the scenario is you've machined something or somebody sent you something that's been partially roughed out and semi-finished. It's gone off for hardening or some other kind of post-process treatment before final machine, and you need to get that back into your CAM environment and toolpath it in a meaningful way.

So the most stable object in your entire design document is the origin at the top level, so this here. It's there all the time. It never fails. It's available in all workspaces. And so you can take advantage of that with certain types of toolpaths. Well, actually with all toolpaths but with certain types of toolpaths, they'll react to it really well. They're super fast to generate. So it's a really low overhead for being able to go through and do this workflow. So you can use 3D pocket roughing and parallel surfacing, so the roughing and then semi-finishing, and they are insanely fast to generate. And if you apply a really loose tolerance to them, they'll generate even faster.

And then you can set up one toolpath from each direction, so effectively, six different toolpaths. And if you set the tool orientation based off of that or at those origin planes, then it doesn't matter. You can take the model out and dump a new model in and it will still generate and just react to the new model that you've put in there. And instead of having sketches for boundaries, you just use the bounding box. And the bounding box is whatever-- it just reacts to whatever the model definition is in the setup.

So the end result here is we end up with six toolpaths for roughing, six for finishing. And we'll just go through and remove all of that stock and leaving half a mil of material over all faces. So now after that is you just store those inside a stock prep folder, and when you go to post-process, you just don't output all of those toolpaths. You only output the toolpaths following that. That means any surfacing toolpaths you do after that will be done based on a more realistic stock condition.

All right. So if you've done much looking around online for productive ways to toolpath your parts and come across any of Rob Lockwood's classes in the past, you'll probably be familiar with the container method. So that revolves around using components as containers. But sketches are containers, too. And so as long as you use your construction geometry appropriately, because if you've got geometry in your sketch that you don't want to have participate in any kind of machining, if you set it to construction, the CAM will ignore it, unless you explicitly select the construction geometry from the graphics area.

So with that in mind, when you want to use sketches for machining, if you select the sketch object from the browser instead of the sketch from the graphics area, whatever you put in the sketch will become part of that selection. So that means that toolpaths, boundaries, and if you're using toolpath modifications in the machining extension, you can then trim using those sketches. And they will just react to any new construction sketch geometry.

So here we can see that this had some additional material welded onto it for a repair. And then Insert uses that same sketch boundary, and then we can generate a steep and shallow toolpath using that same boundary. But if we go and edit the sketch and add an additional geometry-- and again, it doesn't matter what it is-- it will react to it. So we'll trim this up, regenerate the toolpaths, and you'll see it react to that new geometry. So a super powerful workflow to keep in your back pocket and just have that template saved away.

Have a repair job, just bring in the model, generate the tool paths, done. They're really, really slick workflow. Some of you might not use that often, but when the opportunity comes up, really, really incredible.

All right. So don't patch and trim. So with a really common thing, workflow with this sort of work, is to go through and patch all of those individual holes. But if it's a single phase, you can just use Offset by 0 mil. And then use the new Untrim command. And in this case, we're going to use the internal edges only. And it just deletes all those internal edge loops. So instead of having dozens of individual patch shifts is we've now got a single surface we can use as a model override in your toolpath. And it will stop the tool from dropping down inside all those holes. So yeah, it mainly works really well for single faces. If you've got complex geometry, a patch is the way to go.

All right. So round peg, square hole. So earlier this year, the Fusion team released the ability to have if-then conditional statements in parameter expressions. So you can actually use unitless parameters as a Boolean switch, if you want. So zero being false, one being true. With just using an if-statement as an example, the condition is the first argument. And then based if that condition is true, whatever is in the true section, the true argument becomes the value. Otherwise, whatever the other condition is true, else is whatever that value ends up being.

So in this case here, we've got length formula. So if CircularStock is one, then use width for the length. So we're making it the width and the length equal to one another. Otherwise, use length, so it will become 50 mil.

So if we just have a quick look at this. When we open up the Parameters dialog, if I change this to zero, you'll see it changes to a rectangle. One goes back to a circle. And the problem with this is that the fillet feature will fail because it now has a radius of zero mill. If that's at the end of your timeline, probably not too much of a big deal. But now, as of the September release, we have the ability to use configurations. So we can combine all of this stuff now.

And I'll just bring my timeline back even further. I've got configuration table in here. And I've just created a theme by using my circular stop, stop that Boolean parameter, and the fillet. And so if we want to use circular bar, then the parameter is one, and we don't suppress the fillet. If we want rectangular bar, then the circular stop Boolean is zero, and we suppress the fillet. And then we can include the length and width values. So now, when we close that, we switch between rectangular and round bar, you'll see that the fillet feature gets suppressed or not.

Now one of the neat things, a few features of discovered, is if we-- I'll just come back to here. I'm using this in the context of stock between two vise jaws. This could be a number of different things, though. If I want to create a joint between this component-- so my component drag is turned off-- between this component and this body, I can use a joint. So the important thing to remember here is that this is still the same body, it's just converting from a rectangular to a circle because of the fillet.