Fusion 360 - CAM Q&A

hello looks like we've got uh michael rudolph jasmine thomas david harrison some folks joining in uh actually pretty excited to go over a couple of i call them basics in fusion 360 surfacing specifically around selection and orientation or tool path containment this is a the part i wanted to start with was a part that a viewer sent in last week and had a problem with the parallel operation selecting the correct geometry to get a parallel tool path to machine this inside fill it so i wanted to go over kind of the right and the wrong and the good news is there's a really simple answer that solves a significant majority of the confusion and question around the correct setup for these three axis toolpaths and then i've got some updates and tips and tricks around the some five axis workflows a five axis camera part bracket that we were working on that frankly kicked our butt was pretty complicated part uh i thought i'd go over an example of how we're using our dual spindle lathe now and even go into some floor finish tips and tricks that we've been working on uh for an upcoming video um let me take a look here oh awesome got a lot of new folks here a lot of folks just uh joining in here uh albert parker marcelo andy thurlow albert ends leopoldo piotr gaston gt customizer uh von fondelli sorry if i'm getting any of these names wrong flowrider so how's everyone going i would love to also have some q a in this i'm not sure exactly how well that'll go because uh the inability for spokes to actually offer their model up but um happy to answer questions whether it's fusion 360 which is kind of the focus of this live stream or uh cnc machining in general uh i think julie's on here as well it was going to help chime in because it's quite difficult when you're doing these uh live streams to also be engaging with the uh chat window in the comments so i am going to hop into this sample part so the question was from a customer what why is my parallel tool path doing this when uh and this is a bullnose tool so instead of it being a complete ball end mill it just has a large corner rod and it's a great tool to surface in or machine in a chamfer like this and their confusion was that they have the correct chain selected so if you see this kind of neon green if we orient the model and we look you would think hey i've told fusion the machining boundary is that section so why is it basically machining a bunch of stuff and potentially the stuff i don't even care about and it's always helpful to look at the simulation and if we choose show points it makes it a little bit easier to pick a point and you can kind of snap to that location and you can see sure enough it's not what you'd expect because when the control point of the tool or the end mill is right here well it's actually machining fairly high up on the side of that fillet which means if i check a point say down here you can see it's working its way down nevertheless this is not a good tool pack it's not what i want so luckily the fix for this is pretty simple and i enjoy explaining it because when someone explained it to me it really clicked and made me appreciate the software a lot more so the first problem that i would do is i would stop with two chains when i'm troubleshooting the toolpath i like to keep it simple and focus down on the essence of the task at hand so i'm going to instead of clicking the x here which would delete both of them i'm going to hover over this and choose the little trash can to delete that so that gives me just one chain selection now tool center on boundary i'm okay with that but that's going to be the big thing we come back to in talking about the right workflow here i'm going to leave it at that for now but what we don't want is the additional offset uh the additional offset basically says that the file or the tool can go over or beyond that and that is what's going to cause it to do very strange things i'll click ok and generate it like this sometimes you'll even see it waterfall down the side of the part in fact i suspect if we do a tool outside boundary plus the additional offset it'll probably fall over the edge of this part and it didn't there but i've got an example i'll show later that really highlights that but let's cut to the chase what's the answer tool center on boundary zero additional offset would almost work but it's not still not cutting exactly what i want so my go to is to use what's called contact point boundary um is everybody um is uh can somebody confirm uh oh good julie's here let me see if i can make her oh she's a moderator already great um everybody else audio video coming through okay someone could chime in on the chat window just to make sure oh i forgot that you guys have the picture in picture uh let me make my uh let me make me a little smaller then i won't be hidden there so tool center on battery with contact point boundary so what where i think this is really confusing um and autodesk could probably do a better job of improving the workflow here is that contact point boundary really overrides the additional offset in the tool containment because what it does is it allows the tool to expand the area as needed to do the work it needs to do and rob lockwood who hopefully many of you have heard of is an excellent machinist who has a video that maybe you haven't seen because it's under the guise of hsm works and not fusion i'm going to go ahead and throw that in the chat window here though rob goes into a really lengthy detail uh showing the examples of contact point boundary um in the this this picture let me zoom out a little here in his video the example here is you know we've got this ball end mill and we want it to capture the top lip but not fall all the way over this part and he shows that once you have contact point boundary selected it kind of brings that tool right up to the right uh location it's a really elegant solution it's kind of a catch all save all if you will but the question you may be asking is well okay why the heck do we still have these little whisper cuts and that's the second solution that we need to go into here which is the additional offset so the way a lot of the cam operations work is they tessellate the model they take this beautiful perfect uh parametric solid model and they convert it into millions or billions of small triangles that's just how the graphics world works or the cam kernel the cam engine and so when it does that you end up with a shape that's not perfectly smooth or round but rather has juts and angles and though the resolution or the detail of that is subject to this tolerance right here under the passes tab and for this example i'm going to reduce that to 2 10 000 of an inch now if you have a huge surface area a huge part you may need to keep this a bit larger the value of it here isn't quite so important as is the relationship because if this value is two-tenths then back on the geometry tab i'm going to do a negative additional offset of three tenths so what i'm saying is my model resolution is plus or minus two ten thousandths of an inch of how it builds that tessellated model but my additional offset can never be more than negative three tenths and that usually solves this problem of giving us a clean tool path and sure enough if you look at this this is much more like what i would expect for it to do of moving back and forth we can even do a little simulation here that shows that tool path moving back and forth along that piece of geometry so in all respects or many respects rather that solves the issue however there's one more kind of major workflow uh that i think we could do to improve this 3d tool path which is very common in the high-end 5-axis or surfacing world i'll show it to you it's going to look like a fair amount of work and the reality is it is some work but it's super common even across different cam software packages um and it's just something that is uh kind of a if you want to go to this length it's worth it i mention it because once you figure out how to do it it's actually not that difficult so i'm going to hop back into the design space and what i want to do is take this surface i've already got one picked there i've already cheated we did this ahead of time for the customer but basically i want this instead of having it just be this narrow fillet range is i want it to go further left and further right that way we're surfacing back and forth across the full part kind of like if you've ever run a surface grinder you don't change directions on the part is anytime a machine changes directions or has any kinematic input it's going to cause some amount of imperfection because it's stopping a motor and moving it the different direction so what i'm going to do is go into the surface workspace create offset i'm going to hover over this the body here let me delete these other ones they're not acting up here create offset and okay this is a kind of a glitch it's picking the whole body i turn that off turn off chain selection now i can pick just that individual fillet click ok it doesn't look like anything happened but if i turn off the body you can see we now have a uh patch or what's it called surface model of that now there this looks like it has some meat to it or thickness but it's supposed to be a thick less or invisible if you will sort of service body it doesn't have anything it's just represented kind of graphically but now what i can do is take that modify extend and i can extend this left edge so whatever amount i need to and that's going to let us extend off the left side of the part now the right side is a problem so if i do modify extend here it's not going to do what i want luckily there's also a quick fix which is i already added this construction plane in when i was working with a customer but i'll do that again to show everybody construct offset plane i'm going to pick my uh models origins let's see what plane would this be the blue and the red is y sorry z x i think z x yep so that's the plane right there i'm just going to drag it anywhere to the left here so that it bisects or cuts my the fillet uh that i just made i'm going to pause here look at the comments and make sure we're all doing okay here okay and now i'm going to take and modify and split face or split body i believe either will work here we'll do split body i'm going to split this body with the tool that i'm using to do the splitting is that new plane i just created and it looks like they're not aligned it's just the view right here they are in line click ok and now i can hit click that hit delete turn my body back on just to see where i'm at so now modify extend click this drag it across and i want to go a little further perfect so now we have a new piece of model geometry that we can use to move that parallel tool path so that it's doing the linking moves or transition moves off the part the last thing we do to program this is i'll duplicate my parallel up so we'll do this in a new operation edit and under geometry we're going to change our machine boundary to be the selection of the new patch body and then you also under model need to add the model surfaces you can either select it by clicking on it or if you have a lot of patches or it's a complicated model you can expand your design tree and choose body 8 click ok and there we go i really like the look of this tool path it's nice and smooth it's moving back and forth it's doing the transition moves off the left and the right side of the part so that is that's the majority of uh the way to tackle or improve that part there was a unexpected problem though when the customer applied that same methodology to the parallel tool path that surfaces across the numerous fillets across the top part of this if you take a look it's kind of a strange behavior it's a decent tool path there's nothing really wrong with it except you've got this section here which is instead of being blue is green and if you're not sure what that means go into simulation oh actually i just caught a there we go no that's okay and if you hover over the info tab you can see the feed rate and the movement of cutting so if we drag across this you can see that it's transitioning between a cutting feed rate and a transition or linking move now he's got them programmed the same way so they're really isn't a huge issue here but if you wanted to get super picky high-end machinists and high-end machine tools will have a slightly different finish because you've got this additional point there and excuse me every time you have a point basically converts it to a line of g-code so your machine tool your haas or hermela or tormach or whatever is going to see that as a point in uh again in the high end mold world five access world every time there's a point the machine may be doing something and that can manifest itself not necessarily as a problem in your tool path but it may mean that these blue lines are different than the green lines so in this case uh the reason that you have the linking move area there i believe is ironically a rare example of where contact point boundary kind of bites you because it sees that once it machined this kind of last blue line here uh the the face of the tool had already finished machining the rest of that part so you can almost think of it like a rest machining style strategy where the software realizes hey i don't need to machine this part anymore because it's already been cut so it's doing a linking move across it which again you may not want so i think if we turn that off here it fixes it just like so let me hop back to the comments here and see al's in there um okay how do i get 3d adapted to avoid a bore or an area awesome question uh the i think i have a template part open here mean when you start the tool path whatever operation it is fusion has no idea what you want it to do you have to start clicking uh generally 2d sketch geometry to build up that tool path so the classic example with 2d contour is if you won't do anything until you click a line and then fusion realizes okay john wants me to machine this contour or this line the 3d toolpaths are completely the opposite as soon as we created that 3d adaptive and picked a tool and clicked ok fusion went to work looking at the solid model and it's basically going to machine everything that it can you don't need to click anything you don't need to tell anything i'm getting an error folks that we're getting a low bandwidth and it may be buffering so can somebody chime in to see in the chat window if it's problematic yet or not and so the question is not only how do you constrain the tool path but in this particular question from mr squiggles how do you avoid an area well one of the best tricks is uncheck machine cavities and if you uncheck that it will no longer dive into interior pockets like this bore or this uh open face pocket right there really good and easy trick to do it the other thing that you can do which is quite simple is you can start choosing uh self selection so you can say i want it to machine here and here but nowhere else and you'll see it will just do work inside of this area and the area on the right oh get it in air i may have a rest machining on here try this here that should work maybe not let me turn off one of these and see if that fixes it well turn on stock contours i may have a height issue or something quirky in this uh setting here yeah i'll come back to that i don't want to get uh cut out um okay so the other example i wanted to give was uh and actually another shout out to rob lockwood was a really awesome way of improving and automating the way you handle lathe cam and this really works well for five axis work i would argue though it can be just as applicable for three axis certainly four access and for lathe work um but the idea here is you have a model your model stock and your fixture i'm going to throw the link in to this page here because if anyone's interested in this content it's worth going to watch if you just google nyccnc au 2019 it'll take you to this page which i'm going to post in the chat window right now and there's a number of great presentations uh on there i did one on our process of getting our first five axis um phil did one on making complicated five axis parts quickly which will blow your mind uh even if you don't do five axis work the way phil approaches stuff is is eye-opening uh lauren did a great one on some of the new stuff in fusion and then rob did one on this topic uh which is basically a badass way of automating this window machining template so if i change the size of this window you can see it's adjusting the thickness it's adjusting the height and you can even adjust the bottom offset of the part the taper of it and what you do is you then drop your part into this window and you're able to do work as i mentioned this is a great technique for five axis work because i can do work from both sides keeping it inside of this window frame and the cam can largely be pre-programmed now you'll still do a fair amount of time tweaking and adding surfacing operations and so forth but it saves you a lot of the busy work of kind of hey i want to do an adaptive from this side and from this side and the other two sides and the beauty of templates is it's always easier to delete operations you don't need than having to add them and oh looks like we've got a troll good let's kick out this guy it's interesting i've become much less tolerant of trolls we do what we do because we love it and we pay it forward i don't really care about folks that are interested in trolling anymore um i also wanted to note on this camera bracket part this is a really cool part i think we have to hold off on the full video for a little while with the customer but we did film it all but one of the new features here that i really liked is when you're doing a surfacing operation especially if you have a five axis machine or really only if you have a five axis machine sometimes you just want to say hey i want to come in with a tool from this angle you know i can see it in the software this is the approach i think i want the tool to come in at under the tool orientation window now literally align to view watch the blue origin click once it just updated your tool orientation to that view absolutely amazing in the past we handled this with what's called the the amish star globe which is a pre-defined sketch you can download off our website where we have kind of always reminded me of the disney world epcot thing or the death star where you've got all these different um schedule things and it lets you pick one that's i think every 15 degrees and there's nothing wrong with that approach it's worked well for us but the ability to do it from the visual orientation is an awesome plug-in in addition um i don't think we have time to go into the lathe part today but i will mention um we've got a video in the works on this it is a similar uh what i call the container method and so the container method which again i think was kind of a lockwood uh in the invention means in my lathe file i have my main chuck i have my stock i have my sub chuck and then i have a part placeholder so the key to understanding the container method is why do you have what's called a placeholder for the part well the reason is i insert my part that i want to make my chest pawn or plate spacer into this template file underneath this part plate placeholder and that that saves me the hassle in cam of having to define my setup model because my setup model is already picked as the parent component and anytime you put a component in as a sub component it just flows through so that may not sound like a significant thing but if you've been doing this the light bulb may have just gone off and you say oh my gosh this is a huge win what's even more amazing about this is another gentleman took it to the next level with these user parameters that automatically calculate the sub spindle parting and grabbing and part pick off so we needed to make a few hundred of these parts i didn't want to crash the lathe or have any stress all we had to do was update our stock diameter which is parametric one inch how far out of the chuck it's sticking two and a half inches some minor details about how far offset you want the parting to happen and then you do have to put in the part length which i wish you didn't have to but the 0.925 inches here just relates to the back to front dimension of this part then the parting operation and the pick off is already pre-programmed and it's a bit funny because the parting operation visually happens on the front side of the part which is not what you expect but that's not actually what happens because the part is pulled out by the sub spindle on the first prior two operations it's then parted off then we have a back side uh sub spindle oops oh here we go i don't have that on this one for some reason sorry oh we didn't even use the part pick here we just needed the sub spindle to hold onto the part because when you have both sides of the part being grabbed uh by both spindles if the part off is clean there's no need to clean up the back side there's no remaining nub and then the sub spindle dumps it into the parts catcher so super awesome kind of automated workflow that's been a game changer for us um i'd allocated kind of half an hour i'm happy to stay on though so let's see here uh what kind of questions do we have here i'll rewind here a second um not too many how many hours do you spend designing programming how many machining i don't even know where to begin answering that question um i would say i care more about the cam side and programming toolpaths uh like a lot of times especially on this camera bracket part i basically ran it unattended oh that's a good segue though the concern on a part like this is part collision cam pleat which is the software detection stuff that we use i think you can probably see the umc here in the background they just got bought by autodesk so that's a good little hint that i think some more infusion machine simulation stuff is coming which is a absolutely awesome and welcome improvement but for me there's definitely a fair amount of time spent programming what's your process for depth of cut on 3d contour undercuts i don't have a process we do have a video on it nyc cnc fusion undercuts 3d contour is the only fusion operation i believe that can do undercutting here we were using a lollipop tool which are not very rigid you've got a relatively thin shaft so you've got to take it easy i don't have a good rule of thumb to tell you what's absolutely going to work the first time around should i finish the floor of a soft jaw asks west agenda so the reason i generally don't adaptive tool paths are not finishing strategies but they will they will leave imperfections or fastening around both straight and certainly curved edges but um so you need to come back with a 2d contour to clean the profiles but the floor tends to be quite good the only exception would be is if you're if you're roughing so hard that you're getting healing or deflection in the tool it may be worth coming back and cleaning it up is there a way to convert a tool path into a sketch no there's not um you can drive trace tool paths off of sketches though uh which i know is something john grimsmo does and i'm working on a video actually really excited about this how to machine a part that's larger than your x-axis travel which is a pretty common thing and so the video is going to talk about using our mod vise using super glue using fixture plates using regular vices using vacuum and then some tricks you can do to either handle it accurately or handle the blending of the part do i see solidworks stepping up their game to avoid losing customers look i don't know i can't i don't follow all the i like making parts i've tried to kind of avoid some of the drama around uh who loves what look if you love using bobcat god bless you not for me um my i think solidworks now offers a subscription which would be cheaper than the perpetual which you know cost me six thousand dollars that was not a fun check to write um and there's been a fair amount of drama around the fusion stuff um we've been a paying customer for a while and it seems like a lot of the paying customers are kind of happy to say hey let's make sure whatever we're doing here is sustainable um i think there's probably a mishandling of the publicity that fusion never was supposed to be free and a lot of folks were abusing it so um i i don't think anything i'm going to say is going to please the people that are upset i'm not sure what your next best option is for free or really low-cost software there's things i'd love to see autodesk do it differently or better and if anyone from autodesk is listening please dear god one thing i'd love to see is when you pick a chain or a body under these sort of menus within cam if that has been named in the design tree like if i've got a sketch that's called sketch one or it's called like oh i can't rename it here i rename it in the cad side um example two or you know protect one then reference that in the cam side so i know it's like talking to each other so i know hey when i chose that region that sketch it just doesn't just say sketch it says sketch one or design two um oh uncle phil thank you very much for the um the uh i forget what it's called but the contribution uh do i listen to within tolerance the only other podcast i've listened to is um hakko well machining podcast is uh oh shoot somebody tell me what it's called um the micro machining podcast with jo adam demuth and nick hakko i really enjoy that it seems that 2d adaptive now uses g2 g3 to the line segments for circular holes or you doing something asks posse cookie um i cannot give a good answer that off top my head except you may actually i think cj and some other autodesk people i saw in here they may be able to chime in it may be something where 2d adaptive i i generally wouldn't care when it's an adaptive but the smoothing setting here should be the tolerance with which it converts them which may make makes it do it precision microcast thank you are you planning to make more starting out videos for lathes yes i can't say anything more about that because i'm not allowed to talk about the lathe that we have hopefully you can't see it in the background i didn't even think to hide the thing but absolutely and i'll share that with the folks that are still listening um we've had some different opportunities come our way over the years and recently and i'll tell you it makes you think about what's important to you and what you want to do and um we've grown and we've got five access and bigger machines a bigger shop but i'll tell you the thing i care the most about is helping folks kind of go from nothing to something that's one reason why i still love helping folks with the the smaller machines the hobby machines the machines that you can bootstrap get that second job and afford because like anybody who knows how to wheel and deal could probably figure out how to get a loan on a big expensive machine that you couldn't justify that's fine and there's people that that's a good fit for but um i'm super glad that we have vince on board who's helping absolutely crush it to show what you can do with these smaller bench top machines we've got a new small lathe that i'm excited to put through its paces it just makes me excited um hey peter thank you uh very much for the donation uh we appreciate i'm not gonna say no but you don't have to donate folks it's it's appreciated but uh we do this because i love doing it um what is preferred cam for a big pocket oh great question this might be the best tip this whole video what is the preferred can for a big pocket the preferred cam for a big pocket is ready for this 3d pocket i don't want to take the time to pull up the example now but we had a guy in our class who works for one of the electric car companies and he had this huge huge suspension part and the adaptive operation was taking hours to calculate on a high-end computer and it does so because the adaptive operation has to do a lot of behind the scenes calculating we move that over to 2d pocket by the way you can do that by just right clicking and saying create divide operation choosing 2d pocket pulls all your tooling and settings over you want to check it but it eliminates a lot of the hassle work and 2d pocket calculates instantly now 2d pocket is not a constant engagement toolpath so if you took an end mill with a really deep cut and shoved it into a corner it's probably going to break so you want to be careful of that with either a reduced radial cut reduce axial cut or in his case he was using this is on a super high end machine so he was using a really open like a four flute two inch diameter uh hogging face mill so there was no way that was going to chip weld in aluminum uh it doesn't need to have that graceful adaptive high-speed strategy in the corners um am i going to have another open house look i don't know would i like to yes two things happen number one covid number two we basically lost our parking we don't have that much parking here and the factory that used to let us use our parking is owned by a different company now so uh without having a solution there i'm not sure how we're going to pull that off [Music] what is your advice for wood carving i'm not an expert on wood carving fusion could do some of it i definitely still see a lot of folks using the software that's very popular in the router world i believe vcarve is one of the leaders is there a quicker way to plunge mill than drawing points not that i'm aware of but the points thing isn't that bad and i believe dellcam which autodesk bought years ago three four years ago had a strategy and i don't know maybe a year ago autodesk finalized the i think they call it the porting over of the cam kernel which basically lets them use dell cam stuff in fusion and that's where we get the steep and shallow tool path so i suspect over the next year you'll see more high-end dell cam power mill uh feature cam type strategies come into fusion but i don't i'm just i'm speculating there any thoughts on rhino cad cam look i looked at rhino for a hot second back in 2009 when i was getting started and it wasn't for me uh fusion wasn't around then um but um the folks that i talked to everyone saw that use rhino love it but it's a little bit more uh it's really good i think it nurbs and it's it's takes a it's a higher learning curve that way like it or not the thing i love about fusion is the user base when we meet with people see other shops hire interns fusion is now just it's just common to know it and if they happen to know something like solidworks getting them up to speed on fusion is is not difficult jasmine says thanks for your videos really helping me start awesome love it do you like to use large face mills for rigid machines we do we use on a cat 40 especially a not dual contact we don't go beyond two and a half inches you could but you're starting to i think put a lot of ask a lot of that spindle and risk some long-term excuse me side effects how do you program high feed cutters asks kadar i would talk to your tooling rep or manufacturer manufacture usually they're no different than a really shallow adaptive style strategy or even a 2d pocket if you're not familiar a high feed cutter is they're kind of funny looking and you you might program one with only a six thousandth of an inch or a i don't know what that is look it up so i don't oops 0.26 inch two millimeter yeah like a 0.15 millimeter depth of cut but you may be moving forward it five or ten times faster than you would on a regular tool can we use fusion 360 for to make injection molds freshly i don't know we made one for our fixture plate plugs oops hope i didn't just close it no um it's actually pretty cool the injection now this is not the same as an injection mold that you would have for a lego brick but it's a real injection mold um and we made it um on our haas and took our time you know really spent our time with the tolerances and that has now made probably a half a million plugs and it's still going strong so fusion's not i would say not the limitation there a couple more questions then we'll wrap up here the thing i do find strange is the no rapids limitation asks garrett yeah some of the some of the things they did are i kind of get some of the things it's kind of like really um but again um i'm not seeing you know it's still fusion is still free to get be careful with that word to students there's still a hobby or startup license if you're a startup business that just doesn't want to pay for it for the first year um i think they're just trying to stop the people that were running real businesses and thinking well i'm just not going to pay for this oh here's a good one what is your best video to help me understand what the cut and depth of the cart for programming apart asks garage manufacturing so nyccnc.com i'll post this in the link go to speeds and feeds the basics we have a video called getting started if you're new to machining we give you some really good uh getting started you know no bs let's cut to it with some real advice that i would recommend watching um benny schwendermann asks i often get whisper cuts in in z when using 3d adaptive i'd watch the earlier part of this video to see if the negative stock to leave handles it fixes that otherwise the whisper cuts that happen in xy um spur cuts we have a video showing uh search for well i'll just put a link in the description the other way to handle the whisper cuts coincidentally that's the same thing we talked about earlier in this video which is it's an issue of carrying over rest machining with the tessellation with the stock to leave tolerance stack that builds up across them christian asks have i ever used power mill no a friend took a power mill training class and on day two they were still doing the work coordinate system set up so i'm a fusion guy when machining large deep pockets do you pause in to deal with ship material we don't have to do that but if you need to absolutely no question about it oh peter belafonte mentions i think this was about the mold question that they make carbon fiber lay it molds infusion all day long uh and that works fine uh vision forge hey john unrelated but are you releasing some lathe videos proven cut for late i have a new machine i'm trying to learn it so um i don't have any well we've got a couple late videos on the haas coming out um i've got some small lathe stuff that'll happen in the next few months and then and this is super exciting um although i will absolutely say i'm not trying to turn this video into a sales pitch for us that's not what this is about but we run proven cut it's a paid feeds and speed service and literally uh last week we've we published or we uploaded the first lathe recipes i don't think they're actually public yet but we built the whole back end out to support turning and we've got that underway so we are super excited to get proven cut turning recipes on proven cut 1620 garage new to milling would you recommend aluminum or steel if you are getting started i would absolutely recommend aluminum go easy lightweight radial depth of cut light light with the cut and light depth of cut keep your feed per tooth up watch that video i linked in there about getting started though do you have basic parameters for your tools in your tool library in the umc infusion each material so you select the tool and it has settings you know it works michael now we have a lot of tools set up which you can kind of see behind me but i don't have material specific speeds and feeds uh that are ready to go per se but we don't cut material that's hypersensitive you know exotics and canals titaniums where you've got a narrow band so like on a surfacing tool uh a 316 ball end mill for surfacing i'm actually probably going to run similar fuses speeds between aluminum and steel i may tweak it a bit but it's not like one's going to immediately kill the tool bobby says thank you for all the videos thank you sir um kadar threw my through 400 currency my units my way i have no idea how much money that is but i thank you very much i saw i use solid cam in solidworks for my shop asks dad what is your inspection room equipment like we are probably that's probably a 2021 thing for us we have a whole video the past four months we've completely overhauled this shop it's its own story in its own video that we're nearing the end of filming it's been a four month process but we've built our own erp system a new coolant system new machines new processes qc etc we have a spironi right here and a mitutoyo height gauge right there which are definitely key parts of it we also this year have spent a lot of money buying dedicated product or product or machine things like micrometers thread gauges go no-go gauges which hand tools i love you know deltronics gauge pins and go no gauges are really good for the work we do parker engine setting up the s tools system what does that look like in your tool library do you put the s number in the name description uh yes but um someone convinced me that maybe it is worth get changing the s number to match the t number and just updating the tool number in the atc and the haas it's a trade-off that i think i was wrong on um and it solves some other problems long term if i'm missing a question and somebody really wants it go ahead and ask it again because otherwise i think we're going to wrap this up here in a second biscuits and gravy how do you make a spiral in bobcat i don't know in bobcat infusion you can probably do with the helix command but i would google it on youtube if we don't have a video on it i would think somebody does what parameters should i look for to reduce the side of my g-code file luckily asks uh or snitchy virginia uh that is a great question and the answer is uh generally smoothing smoothing will consolidate points and like i mentioned earlier every time you have a point you have a line of g code so taking three or four points and turning them into one will reduce four lines of g code to one that will reduce your file size by in that case 75 the other trick if you have a really limited memory is reduce the number of step downs like on an adaptive strategy every time you're doing a step down you're adding a whole other layer of those codes in size um do i have videos of programming five access yep um if you you look on youtube or um on nyccnc if you go to library and most of nyccnc is free and public-facing there's some pro-member content as well but a lot of it is free and open if you check five axes you'll see lots of examples there vision forge we're going to post this video yeah i think it actually just stays live or after we're done you can re-watch it mark says love your channel learned a lot i thank you mark um tad says he was asking about the metrology tools he has a feral arm laser and vision systems vision systems are interesting fair arms are not nearly accurate enough for what we do fair arms are those kind of arms you can freewheel around to touch points my general understanding is those are only accurate to say two to five thousandths of an inch which is um 0.12 millimeters that's we work in dimensions it's generally way tighter than that um do i need a very good pc for fusion 360. we've got an article on that too nyc cnc fusion computer we update this article every week or two about the what we're seeing as tips and tricks and recommendations and options most of fusion doesn't require an insane computer there are certain things in the cam side or simulation side that will benefit from things like solid-state drives and ram and graphics processors but the only thing you need is a 64-bit in in most computers nowadays are are 64-bit andy thurlow had a question here which i recognized his name i'm looking at a used 2012 hos vm3 8 000 hours tsc probe side tool changer would you be okay with that if it's a tight budget it's about one-third the cost of new so it's impossible to answer this question on the spot without knowing more a couple things i'd add haas is running pretty crazy sales right now so make sure you factor that in terms of what new versus use cost um you can if you're friendly with your hfo or maybe offer to pay them just as a goodwill gesture hopefully they don't really charge you if you get the serial number you ought to be able to get a crash report or a service report on that machine always ask why someone's selling it there's situations like a company's upgrading or or closing where hey they're selling it that's a great reason there's others also situations where they're selling it because it's been run into the ground or as a problem machine my general ethos is i don't have nearly have nearly much a problem buying a used machine if it's not my primary main machine you know if it goes down if i can't get parts so forth 2012 haas parts are going to be readily available so again maybe think about making sure you have a budget and if i remember you work at a school so make sure your school will be able to fund a repair cost you know if you have a spindle go out that's eight grand it's either eight grand or the machine's going to the scrap yard there's no in between there how do you deal with end mills that are used but not worn out um great question uh so we don't um if an end mill is good we use it if not it gets put in the scrap bin um sometimes we'll put it back in and like write on a piece of tape or stick a thing in the box but um or it just needs replaced it's just kind of a cost of doing business dope i used uh peter peter did get crushed with an old fidol but that's different than a 2012 haas nick brown i messed something up how many times can i undo show us where to fix that because i can only go one step back well if you're talking about fusion every time you save it revs up a version so like these are all recent files but if you expand the file you can look at the old versions those don't ever go away so that's a great um way to solve that oots of all okay last few questions um usually how do i motivate my guys to keep machines maintained in the shop clean um so that's not a situation where i would use the term motivate because motivate to me would be like hey let's think outside the box or let's um have a better attitude keeping the shop clean or machine maintained that's your job and that's part of what you need to do something i've seen shops do when they're trying to implement this is do that in the beginning of the day because at the end of the day everyone's rushing to finish a part or rushing to get out the door or go home so as your job as the shop leader the boss is that's not something you're going to motivate to it's something you're going to do and it's not something we're going to discuss further you're going to wash out the machine you're going to mop the floor we're going to get this done clean that's it um drives the spindles aren't cheap but we said about her yeah uh does the camp post work perfectly right off the box are you happy with it um only problem we had with camplete post was a couple of like the quirky like peck tapping and one of the like um through air coolant didn't work which they got fixed the service was great support was great am i happy with it i mean it does what it needs to do it's cumbersome software it was it's hard to learn it requires a lot of clicks um platter would have hit the side of the spindle those are the crashes that get you it's not the like hey you just programmed your part into the device everyone can see that if they're looking so i'm glad we have it um yeah well hey folks uh i actually really enjoyed this we've got a really good turnout and uh i think we'll ought to do this again if you guys want you can always reach us through nyccnc.com we've got our products over at saunders machine works like i said proven cut's kind of our new thing we have online fusion training if you go to nyccnc.com this is a paid class but if folks are looking to learn it there's a ton of free videos here but we also have a online course which you guys are welcome to take a look into and i tell you what phil nope and james will you do me a favor and save those questions for the next uh live stream we will absolutely dive into that happy to talk about it um tom lipton said something on a video a while back that really stuck with me which is the trades have been good to me uh i love that i get to do this i love that we get to share this journey with you hopefully everyone's a little better off from the content you've learned here or elsewhere on youtube or in the online machining community so thank you guys for chiming in take care see you soon

Channel: NYC CNC

Views: 11,217

Keywords: tormach, fusion 360, how to, cnc, machine shop, nyc cnc, DIY, machining, milling, CAD, cnc machining, cnc milling, learn cnc, john saunders, manufacturing entrepreneurship, provencut, chip rag, CAM toolpaths, workholding techniques, fixturing

Id: VdJyVmjQ7Jo

Length: 51min 49sec (3109 seconds)

Published: Wed Oct 21 2020