Fusion 360 CAM Tutorial for Beginners! FF102

hi folks let's walk through some of the cam for this part in fusion 360 and at the end let's walk through some other really good tips and tricks if you're brand new to machining welcome to another fusion Friday [Music] this video was inspired because our local makerspace called the ideal how that same state just got a tormach 440 which is awesome and it's really fun to see folks that are brand-new to machining and help walk them through that process so we've got this part modeled up let's say we went to machine out this cavity here on our tour Mach 440 we'll hop from model into cam first thing we'll do create a new set up click set up and notice what happened the transparent box is slightly bigger than the part so as I orbit around you can see it's got some extra material on the left the right the top the bottom and it would have it on the front and the back as well so why did that happen we move over to the stock tab the mode is called relative size box now fusion means well here and there's some cool features to this but if you're getting started I'm gonna recommend you switch this to fixed size box and again at the end of the video we'll talk about where to buy that raw material I want you to grab your calipers measure your raw material and let's say it was a piece of extrusion which it most likely is in this sort of size so the width is our X dimension that's left to right that's the dimension that we want our saw cut edge to be on and let's say it's a little bit longer than 4 inches and I'd rather be careful or conservative here and the Y is probably going to be pretty close to exactly being 4 inches the reason that we want the front and back sides in terms of a Y to be your extrusion edge is when we set that part up we want that clean and square extrusion edge to be what our jaws are squeezing against take a look and let's say it is one inch so we've got a little bit of extra material on the top and the bottom go back to set up and this is really important on terms of your work coordinate system this happens to be correct the Y is forward the X is to the right if it's not correct or you want to learn more about changing it again we'll have a video at the end click ok so we've got our set up one first thing we're going to do is we're face the part off 2d face and the face operation is really nice because it takes into account most of what it needs to know it's smart enough to just figure that out so we're gonna all we need to do is pick a tool we don't have any tools here so you can go into the samples library and go through and go down to say inch aluminum which is awesome I think it's really cool at Fusion has this or you can head over to the new NYC CNC website under speeds and feeds tormach we've got some NYC CNC fusion 360 to libraries and templates I checked my tormach aluminum library and I'm going to pick the superfly face smell which is a great way to deck down material click OK and the only thing I'm going to change is underpasses fourth tab over I want to make sure it doesn't take too much depth of cut so I'm gonna say the maximum step down is 0.04 inches there are some things we could do here a little bit more aggressively but I find when you're getting started it's much more rewarding to make a part successfully and then let's worry about pushing the machine and pushing the feeds and speeds and tooling later one last really good thing to check is this stock offset we can add about a quarter of an inch and that's just gonna make sure that the superfly gets all the way off the material and the fun thing is it doesn't really add much to our machining time so click OK awesome thing about fusion you can look at the color code of the tool path so yellow is what's called a linking move so that means it's going in or out of the cut but it's not actually cutting green is your lead-in or leave out so here is leading into this tool path and then it's leading out as it wraps around in blue is when it's actually in the cut if we click on this simulation button right here I like to actually turn stock off at first you can hit play and you can watch that tool move around our part possum you can turn stock back on and also watch how it cuts I'm gonna jump to the end of the tool path just to see what happened and you can see the CAD model kind of poking through here on the lines of our stock fact my turn if that transparent you can see we've decked it down to our part awesome next up 2d adaptive clearing we're gonna do the rest of this with one tool I'll come back to a recommended additional tool to consider purchasing but getting started let's keep it simple we're gonna pick a standard three flute quarter inch end mill for us this has always been tool 31 since the day we got started click OK here is that tool that we recommend it is a quarter inch diameter tool with a 3/4 inch flute length speeds and feeds we're gonna take all the RPMs we've got on that 440 which is ten thousand we're gonna go one thousandth of an inch per tooth we again can run that tool harder let's keep it easy so lead in I'll have match our cutting feed rate of 30 inches 30 inches rest that's okay geometry so where do we want it to machine I'm gonna pick that button really important I also need to click this these 2d tool paths are what I call dumb tool paths they'll go anywhere you want so it's up to you to give it the areas that it wants the machine so by clicking this see how I put the red arrow on the inside so it's gonna machine everything inside of this square but we don't want it to machine our bean so by clicking on that it put the red arrow on the other side fusion gets this arrow correct almost every single time but if it didn't for some example you could click on it and it would flip it to the other side now one of things I like to do is just click OK there's more I want to edit here but I'd rather click OK for two reasons one I'm gonna give me a tool path and that's really nice to see that we don't have a problem or error the second thing is that by clicking ok it actually created the tool path which means I can now right click it and hit edit if I hadn't first clicked okay let's say I've gone through and spent a few minutes to change the bunch of settings and I accidentally hit escape or my computer freezes or fusion crashes I've lost all that work this way it's given me a little partial save Heights is good passes tab optimal load I like to start at 20% of the tool diameter so you can do math right inside a fusion I'm gonna say a quarter inch tool 0.25 times 0.2 for 20% and we're gonna leave let's leave 5 thousandths radial stock this adaptive is a roughing strategy so it's not a finishing strategy especially when it comes to the aesthetic and the precision of the sidewalls so by leaving 5 thousands radially radial think of radius or the side of the tool we're gonna come back and clean that up click OK and we should be good let's take a look at the depth of that pocket hit I on your keyboard and pick that line and see how that line is 0.5 inches that's right on the edge of being too much with a quarter-inch tool our rule of thumb that we talked about and our getting started for speeds and feeds video is no more than 200% so 200% of a quarter-inch tool would be exactly 0.5 inches so yes this would work but if it's your first part again don't break the tool so let's take that pass this tab multiple depths and let's say 0.25 inch that's gonna take it to depths of cut the other thing that's really great about this is that one of the most common causes for breaking tools especially when you're getting started is you accidentally chip weld meaning you don't evacuate the chips or you have a problem with the chips getting stuck to the tool that's a more common problem the deeper you go so by taking this in to depths of cut although you can see we got a problem there's actually three we're minimizing the chance that our coolant line or our fog buster has to be just perfect and better chance that we're gonna get a good recipe so why is that taking it in three deficit cut it's pretty cool actually take a look to edit our adaptive let's go back to that Heights tap I said it was okay it's not and here's why Fusion was to understand what's the top height and the bottom height of the work I have to go do if I orient this head-on and let's work from the bottom up here so the bottom height is the selected contour what does that mean well it's the geometry that I picked here so that's actually perfect that's where I want it to machine down to so what's our problem our problem is the top height the top height is the stock top remember when we set up our stock we told it it's a 1 inch piece of material so we've got about half that extra stock up above here so we just hold the adaptive remember it's a dumb tool pack that'll do whatever we want we told it that the top height is stock top and because we said hey you need to go quarter and step down it thinks it's got to start at the stock top well we just machine that down with our Superfly before this so let's change our top height to model top and watch what's going to happen this blue line is going to move down to here and if you didn't know what that blue line was if you orbit around you can see that's called top and it's a little confusing but the negative point 125 means how far off the stock it is fusion could do a little better job explaining those things I'll click OK and I bet you we're gonna get to depths of cut past now so 1 & 2 perfect little tip if you got 3 there sometimes what can happen is you need to say depth of cut could be just a hair more say 2 5 1 and that would help you get avoid that sort of whisper third cut at the floor so let's simulate it click on setup go back to simulate now I don't want to watch the face again we already did that so click on this go to next operation play so there it's doing a spiral move linking in and again one reason I really like the fog Buster versus flood coolant is you can use that air pressure to help blow the chips out of there and evacuating the chips is a really important role in what coolant does more so really for a lot of the newcomers to C&C then actual cooling the chip or the other benefit that coolant has which is adding some lubricity almost like a soap making it slippery when it cuts and this is what Fusion is really really good at called adaptive machining or high speed machine or trochoidal machine where it's moving the tool path to take constant engagements and what I love about it is it means you're never gonna dive bomb that end mil into a corner where it's gonna all of a sudden take a much much more aggressive cut that's how you either break end mils or cause them to clog up or you can the part out of your workholding or you can stall the spindle so adaptive is great because I have the confidence to set up a tool path I'll take a simulation but when I run it after I start watching it for a second to make sure it's okay I'll usually walk away now if you're brand new sit there and enjoy the show adaptive is really cool when we started this about 10 years ago it was a very expensive or more complicated endeavor to get into software that was capable of doing this and I love that nowadays it's there for anybody to take advantage of it pretty cool so one of things I'm noticing let's pass forward here so I can pause it and scrub along it's leaving those corners did it clean them up here I think it's gonna clean them up that's actually awesome perfect it did come back and clean them up so see again it's taking these little nibbles to make sure it doesn't take too much in one pass perfect you can jump all the way to the end and take a look that looks good what do we have left to do well remember that 2d adaptive is just a roughing strategy we need to finish the toolpath and awesome trick in fusion right click onto the adaptive create derived operation 2d milling and 2d contour is the operation we want I'll click it and I'll just click OK let's see how she looks it's perfect with one exception because I added the multiple depths it brought those over but otherwise the cool thing about the derivative operation or create derived operation is it carries all your settings over I don't want the multiple depth of cut here no problem taking it in one depth and actually we want it in one depth to give us a better surface finish but one things I love about it is it saves you from having to remember the settings or add the tool back or re select lines really nice one other little pro tip right click Edit you ever seen a machined part where that has a little trough line of following around it where it came back and did a clean up it's less likely to have that if you're using the same tool as you did to rough it but we don't always do that so a good tip to get into habit of this will make use of this stock to leave will check that we don't want to leave any radio stock that's the but on the axial let's leave one thousandth of an inch that's about one quarter the thickness of a piece of printer paper so it's pretty darn thin and what that does though is it prevents the bottom of the tool from touching our floor especially if we have a very slight miss measurement and the height of our tool and it makes your parts look a little better and it's not going to affect your tolerance or functionality whatsoever click OK and we're done so again simulate fast-forward last tip I like to do is see this light bulb up here turn it off what that does is that stops your CAD model I'm going to put on the transparency here it stops your CAD model from what I call back filling or back stopping your simulation sometimes the simulation looks like it was perfect but your tool actually cramped or crashed through your part but you don't see it because your CAD model was there to kind of make it look like it was ok so toggle that off now we get a view either transparent or not of what our part really should look like when we're done awesome so what's that new website we've had we're really excited for this we got started in this about ten years ago I didn't know what an end though was her bridge port was and we love doing what we do on our YouTube channel we love trying to pay it forward and we love sharing our knowledge with folks so we've created this new NYC CNC website and our goal is that I shouldn't have to explain the website to you because hopefully it's obvious this is what I will call a Minimum Viable Product the site is not done yet we've got a lot more content to add I would say that our fusion 360 content is probably the best off right now we've got fusion 360 training examples in CAD and cam and some of the other environments and one of the things that I love the most is not just the machining side but let's talk about business let's talk about entrepreneurship how to come up with ideas how to execute those ideas how to grow those businesses we're gonna have a lot more here on getting started with tormach and other machines but guide to buying raw material if you want to machine this part and you're brand new where do you buy that piece of aluminum we've got a video here as well as links to walk you through where we recommend buying pieces of aluminum whether new or drops under speeds and feeds tormach we've got videos already on different tools different materials with speeds and feeds examples we're also going to make some of the content exclusive to folks that subscribe you can join here on the subscribe button all the NYC CNC tool libraries all the cam templates as well some of the more advanced entrepreneurship and business topics so we appreciate the folks that have helped us get to where we are and we love doing what we're doing folks thanks for watching take care [Music] [Music]

Channel: NYC CNC

Views: 480,767

Keywords: tormach, fusion 360, how to, cnc, machine shop, nyc cnc, DIY, machining, milling, CAD, cnc machining, cnc milling, fusion 360 CAM beginner tutorial, beginner

Id: Do_C_NLH5sw

Length: 16min 35sec (995 seconds)

Published: Thu Oct 19 2017