Intro to Fusion 360 for CNC Users

hey guys Winston at carbide 3d here for those that are looking to step up their CAD CAM game Autodesk's fusion 360 is usually the biggest name that comes up and for good reason it puts industrial grade design and manufacturing capabilities in the hands of common folk who aren't looking to write a check for several thousand dollars for a software license with its advanced feature set however comes a steep learning curve Autodesk has some great documentation and tutorials for those interested in learning how to use their software and there are some other pretty great resources on YouTube as well but it can still be pretty daunting to figure out if you aren't comfortable with carbide create you might want to hold off on diving into fusion for a little bit but for those of you who are fusion curious and ready today I'm gonna go through an example part I imagined designed in fusion 360 and fabricated in under 24 hours it won't be a super thorough tutorial because trying to cover all the basics of fusion would require a multi-part series but it should be enough to give you an idea of what the workflow looks like and if it's something you'd want to pursue further recently I bought a router table and put it together but found that it wasn't compatible with my Dewalt 6:11 palm router the router table was designed for tools with much larger mounting flanges but since I want to make the most of the tools I already have and I only intend on using my router for light duty work I decided I would make an adapter that would allow my 6:11 to mount to this router table I did some measurements and identified the set of holes my adapter would need to have to make this happen I need four holes in a square pattern to interface with a dwp 6:11 and the easiest holes to mount to on the router table side were these three that were in a triangular pattern the inner bore of my adapter needed to be 67 millimeters in diameter to allow sufficient clearance for the router to bottom out and I picked an arbitrary outer diameter from my adapter plate that was well under 8 inches so that I could cut this out on my know mat with a design in my head I fired up fusion 360 to create my model for those of you who are brand new to fusion 360 here's the 30 second tour fusions interface is segregated into different workspaces you have one from modeling one for cam sculpting simulation there's a bunch but you'll be spending most of your time in the model and cam workspaces within the model workspace which is where you always start tools for sketching are in this section tools for forming 3d shapes are here this might look a bit basic and dumb down but if you dig through the dropdowns you'll find all the tools you need plus you can customize the interface and pin your commonly used tools to the ribbon all the shortcut keys can be customized and you can even change the input scheme set 3d navigation around your model is to your liking I personally use the SolidWorks control scheme because I think it's blasphemous that the middle mouse button should do something other than rotate the model if you want to learn more about getting around the fusion interface I'll link to some tutorials in the description below from my router adapter I'm gonna start with modeling the entire plate first and I'm gonna sketch on the top facing plane so that my part is laying flat two circles to find the inner and outer profiles while I'm here I'll also sketch in the through holes for mounting the router these holes are in a pattern 61 millimeters square I'll use the rectangle tool to draw a square use the dimension tool to set the height and width and also turn it into a construction sketch so it won't get picked up when I choose which regions to extrude on the corners of this square I'll use the center point circle tool to draw in some holes these holes need to allow a number 10 screw to pass through freely so I'm going to make them four point five millimeters in diameter or about 0.18 inches I'm done with the sketch so I'll close it now I need to take this from 2d into 3d for that I'm going to use the extrude tool I'll select the shaded region I want and specify that I want it to be a quarter inch tall even though my project units are set to metric if I type in 0.25 or even 1 over 4 and include units fusion will interpret the dimensions correctly and make the actual plate thickness and equivalent six point three five millimeters the fact that you can type in mathematical expressions is really handy and I personally can't go back to using software that doesn't do this now the screws I have that go into the routers mounting flange are pretty short I don't want the screws to have to pass through the entire thickness of my quarter-inch plate so I want to counterbore these holes to do that I'm going to create a new sketch off the top face of my plate and use the circle tool to draw circles concentric to the mounting holes because the sketch is referencing the top surface of my plate it's already picked up the original holes so my new circles can snap to their center point these are going to be nine point five millimeters in diameter I'm going to close out my sketch and go for the handy dandy extrude tool again I'm going to select the counterbore region and cut away three point five millimeters of material this should let my screw holes sit well below the surface while leaving plenty of meat in the plate to ensure that the connection is structurally sound lastly I need to model the holes for the router table side of the equation these holes are in a triangular pattern and the way I chose to make these was to draw an inscribed triangle using the polygon tool in construction mode I know my holes need to be about 58 millimeters from the center point so that's what I'll make the radius of the circle that this triangle is inscribed in then we'll just draw circles on the corners of this triangle these are point one three five inches in diameter so that they can be tapped for 832 threads another way you could do this is by drawing a circle and making a circular pattern that revolves around the origin in 120 degree increments I'll exit my sketch and extrude these holes all the way through my plate and as a finishing to add a level of polish to the machined part I'm gonna chamfer all the top facing edges just a little bit ten thousandths of an inch or a quarter of a millimeter that little change will make it so much more pleasant to handle okay now that we have a complete digital representation of the part we want a machine it's time to head to the cam workspace before you can do anything here you need to create a setup this tells Fusion what the dimensions of your stock are and where the origin point should be this is how fusion knows where it needs to remove material from because I modeled my part laying flat my default orientation matches how the CNC is going to cut the z-axis in blue is perpendicular to the front face I also want my origin in the lower left corner because that's where I intend done zeroing my CNC in the second tab I'm gonna say my stock is exactly as tall as my part if fusion thinks your stock material is thicker than what you modeled it's going to start the machining tool pads higher so it doesn't crash into the material above your part but in this case that would be a waste of time since there's nothing there with my setup defined I can begin applying tool pads let's apply a contour tool path to cut out the profile of the router clearance hole from the tool path menu I'll select 2d contour the dialog box that pops up is one of those things that might be a little overwhelming at first but when you step through it tab by tab it'll start making more sense in the first tab you pick your cutter and feeds and speeds I'm using a cheap 2 millimeter single flute and mill off eBay for this because I need to be able to pocket out a hole later that would be a tight fit for an eighth inch end mill but you could also use a smaller two flute like carbide 3ds number one 12 - Z 1/16 inch coated and mil for aluminum just at slightly slower feeds and speeds since it's more fragile I'll have links in the description box to videos showing how to add custom tools to your tool library for my cutter I'm gonna run at the nomadz max rpm of ten thousand and feed at 12 inches per minute when I'm easing into the material or plunging I want to go a little slower when exiting a cut I can go at regular speed if you have no idea how to pick these values you can plug in a plunge rate of 30 to 50% of your feed rate and ramping and lead in feed rates between 50 to a hundred percent of your cutting feed rate in the second tab you'll pick what geometry you want to cut I want to cut the inside of this hole so I'll pick the bottom contour here tab three is your Heights you're basically telling fusion what is safe elevation is for moving from cut to cut what height it should slow down and start cutting at and what depth it should stop at since I don't plan on using any clamps for workholding as soon as my end mill clears my stock material by just a tiny margin it's safe to move to the next cut so I'm gonna set my clearance and retract Heights to something small like 0.1 inches feet height is how far above the surface you begin slowing down in preparation for cutting top height is where the cut should begin bottom height is where you stop if you ever get lost here you can just hover your mouse over a field infusion we'll explain what that field does in tab 4 we can specify things like step down since this is aluminum I want to cut this in shallow passes so I don't overwhelm the end mill or the machine I'm going with ten thousandth of an inch per step down in tab five you can define how the cutter enters the material I've got lead ins and lead outs enabled so the cutter will sweep into the material instead of jamming itself straight into solid aluminum I'm also enabling this check box for keep tool down this tells Fusion to go from one step down straight into the next one instead of wasting time retracting and plunging every single time it goes around and that's how you set up one contour tool path you don't need to touch every single option to make it work you just need to figure out which ones are essential for what you're trying to do for the remaining features we can pocket out the smaller holes for the fasteners contour outside the adapter plate and come back to chamfer all the edges these tool pads are all set up very similarly to our first contour and that basically replicates everything you would do in a more basic 2d cam package to cut this part out but as is this relatively simple program will still be way better than any G code you'd get using lesser software the way Fusion gradually spirals into the material or sweeps into the beginning of a cut will result in a lot less shock on an end mil which in turn reduces stress on your cutters your machine and you I know I still cringe every time I hear that horrible grinding noise of someone's Strait plunging an end mill into metal to create g-code from these tool pads we need to export it so after clicking the post processor button in fusion we come to this screen or this one if you're using Mac OS the fields are all the same the UI just looks a little different the one thing you must do to ensure your g-code will work on the shape OCO or nomad is select the carbide 3d post processor by the way if you've installed fusion prior to December of 2018 you'll want to download the updated carbide 3d post processor to prevent certain errors that may crop up when using more advanced tool paths an explanation of what that update changes how to get the new post processor and how to add it to fusion will be linked below now we can hit post or okay pick where to save the file and you now have G code ready to send in carbide motion and that's all well and good but because this is fusion we can actually do way better with just some small changes here's how I actually cut this part out first off anywhere I'm cutting for the first time I'll add a few thousands of an inch of stock to leave machining is a violent process and your first cut isn't going to be the most accurate by coming back later to shave off the last couple thousand get nicer finishes and better dimensional accuracy everyone who's cut something out in one operation and complained that it didn't read exactly what it should in calipers was doing it wrong the most accurate results come from a two-step process roughing and then finishing so here I'm going to take care to run a finishing pass afterwards with no stock to leave this is especially important in holes that I'm going to thread later because I need the tap to start in exactly the right size hole I'll even run a second finishing pass or spring pass to clean up anything that might have been missed because of tool deflection I'll also be repeating the chamfer tool path for the same reason also instead of tracing my inner and outer profiles with a contour operation to cut out my piece I'm actually going to be clearing out a wider channel than necessary so that aluminum shavings can't Jam the cutter listen to how gritty and ugly this cut sounds [Music] cutting aluminum should sound like a steady hum that gravely noise is aluminum chips getting snagged by the cutter and rubbing against the walls it stresses the cutter the machine and if you're using weaker workholding like double-sided tape the spike in forces and vibration can cause your part to rip off it's just not ideal so if you can't continuously blow out your cuts with compressed air or cooling using an adaptive tool path to clear a slot gives you a better shot at success I'll discuss these techniques more in a future video anyway that's enough fusion rambling for one video let's see how this cuts and what the finished part looks like I'm cutting this adapter out of mic 6 which is aluminum that's been cast and stress relieved in a way to ensure that it's super flat this particular piece is actually a scrapped Nomad table I'm holding it down on the Nomad with some double-sided tape after setting my zero to a millimeter inside the bottom left corner of my plate I ran my G code and watched the chips fly first the machine cut out the hole to allow the router to pass through then it milled the holes for the hardware and the last operation with this end mill was to cut out the adapter from my stock after the chamfer tool path all the top edges are way friendlier to touch it's a small detail that makes handling the piece so much more pleasant I would even say that it makes the part look higher quality than the router table itself but that's besides the point the bottom line is fusion 360 allowed me to design and visualize my part and gave me plenty of options to machine this piece in an optimal way to ensure accuracy and finish quality if you're looking to step up to machining more complex flat parts or even some proper 3d geometries fusion 360 can help you take your machining to the next level it's fully compatible with carbide 3d machines as long as you remember to select the correct post processor I'll have links in the description box to some general resources for those of you interested in adding fusion 360 to your arsenal hopefully this video gives you a good feel for what the fusion workflow is like good luck and have fun machining guys

Channel: Carbide 3D

Views: 80,554

Keywords: CNC, Carbide3D, Fusion360, CAD, CAM, Machining

Id: xRVVUteI1PY

Length: 13min 43sec (823 seconds)

Published: Mon Dec 31 2018