Fusion 360 Live - Late Design Changes

hello everyone and welcome to another fusion 360 live my name is Brad talus I'm going to be doing the presentation today along with my friend Angelo who's on the keyboard what we're gonna be talking about today is late design changes so I'm gonna show how you could go from a part like this to a part like this without having to start all over and you'll notice there are some differences like there's some curved surfaces on here etc so I'm going to show some tips and tricks on how you can instead of starting over how you can kind of manipulate the timeline to to reuse some of the work that you've already done I've included a link to the drawings there's actually two drawings the first one and the second one and I've also included a link in the description of the YouTube video to my outline that I usually put together that way you can follow after after this livestream you can kind of try and do it yourself so let's dive in like I said we're gonna start with this part here and then we're gonna transition it into this part be like you see here okay like I mentioned I have two drawings this first drawing here and then the second drawing is actually pretty simple it just has a couple dimensions on there that are important that we'll get to a little bit later so I'm gonna be using or referencing this drawing now I've thrown a couple little tiny curveballs in here for you that we're gonna run into and I'm gonna show you how we're gonna get through those for example this counterbore is dimension from the bottom of the park and you'll see that's gonna cause a little bit of an issue for us but we'll we'll figure out how to work through that okay so this part here is actually fairly simple right it kind of looks like just a couple circles and some tangent lines and that's how I'm gonna start out so let's go ahead I'm gonna create a new design and like I've mentioned in previous live streams I like to create everything as a component so I'm gonna say a new component and it's also it's right here or i can also say create new component it's the very first thing in the create menu so I'm gonna say new component and I'm just gonna give this a name I'll just call it part nine-to-five or something like that okay and that's gonna create a component for me I'm gonna go ahead and expand this open okay so the next thing is I want to make sure my units are set to millimeters so I'm gonna expand open my document settings right here click that little icon and say let's switch this to millimeters and then I'm going to start by creating my sketch and I'm gonna create my sketch on the top plane because according to the drawing you know most of the information is in this top view so I'm going to start by creating my sketch on the top plane okay again just referencing the drawing here I'm going to create a circle in the center so I just have to get near this little center point here my zero zero and the diameter is 50 millimeters so I'm gonna just type in 50 and hit enter okay then I also have the two circles on the side and what I'm going to do here is I'm just gonna randomly draw a couple circles I don't care what size I don't care where they are right now okay what I want to do now is dimension these but according to the drawing they are radiuses and you'll notice when I click on the dimension and they click on my circle it's wanting to do a ammeter if I right mouse-click you'll notice I have the option in when I'm doing my dimension to do a radius okay so I'm going to switch to radius and now you'll see it says R right so I can go ahead and say I want that to be 12 okay now I'm gonna pause for a moment here if I say create a circle you'll notice it's in diameter mode also if I right mouse click I don't have that option to specify a radius it's only when I'm doing the actual dimension that I get that option okay so that's why I just threw my circles on the screen I didn't care what size they were then I came in did my dimension and was able to do the radius now I want both of these to be the same size so I'm going to use the equal constraint so I'm gonna say equal I'll click on that circle I'll click on this circle and now you'll notice they're the same size and they have that equal constraint icon next to them I also want these to be lined up with my other circle so I'm gonna use the horizontal vertical constraint so if I say I want that point and that point you'll see it it jumps down and makes them horizontal with each other I'll do the same thing here and here and now they're lined up okay so quick way of doing that then the last thing I want to do is position these circles where they need to be so I'll throw a dimension from here to here I'll place that dimension and in this case according to the drawing they're 38 so I'm going to type in 38 and hit enter and you'll see how that moves and the lines have turned from blue to black now this one here I'm going to go ahead and throw a dimension on there also and I'll go ahead and place it now I've shown this before I could type in 38 or I can click on the existing dimension and it's gonna reference that dimension so that's what happens when I hit enter you'll see that it says FX which means it's a formula it's referencing that dimension so if I came over here and said I want that to be 48 you'll notice that that one also has to be 48 so it's a cool way of instead of typing in multiple dimensions and having to change each of them you can just select a pre-existing dimension okay I'm gonna go ahead and move this a little bit out of the way okay the last thing I want to do according to the drawing is I want to connect these lines to this circle so here you can see there's our 50 diameter circle here's the 38 that we did and the radius of 12 so just using all that information to create our sketch so I'm gonna go into the line tool and this is really cool watch what happens I'm just gonna get near this circle I'm gonna click and hold and it's kind of hard to see but you can see that little tangency icon is at the end of my line so it's automatically creating a tangency constraint for me okay then I'm gonna come over to this circle and you can kind of see how it snaps to this circle and I'm just gonna keep moving around until I see that icon that tangency icon appear so it's basically creating a line that's tangent from this circle and being tangent to this circle over here and I can do that I can start over here just click and drag and you can see that tangency icon and all I have to do I'm still holding down my left mouse button I'm just gonna get near the circle and move until I see that tangency icon up here so it's a real fast way of creating these tangent lines so you can kind of see I just move over until it snaps to it and we can see that those tangent icons or constraints have appeared okay I'm gonna say that that's all I want to do again you've heard me say this multiple times I like to keep my sketches simple you know I might use multiple sketches to do something I could do a bunch of stuff on one sketch but I like to keep my sketches simple and start building my part from that and so what I'm gonna do here is say finish sketch and I want to extrude this now I'm gonna show you a neat little tip so typically you have to select the regions that you want to extrude so I'm having to click it looks like five regions to extrude well instead I'm just gonna draw a selection box around the whole thing because I want to extrude all of this all right mouse-click and there's my extrude command and notice that it's going to extrude all of my profiles so instead of having to manually click on them all I did was just draw a selection box around them and it selects all of them for me so I'm gonna go ahead and say extrude and I want to extrude this up eight millimeters according to the drawing so I'm gonna say eight you can kind of see that nice little preview notice I didn't trim any of the circles or anything like that I'm keeping it everything very very simple and when I did the extrude it actually trimmed everything for me automatically so fusion is smart enough to do that for us now I created that large circle I want it back again so again here's why I expand open my component is I can expand upon my sketches I'll just turn that sketch on okay now some of you might wonder what does this is a lock symbol mean next to my sketch a lot of people think that my sketch is locked I can't do anything with it what that actually is check this out if I were - let me let me just do this I'm going to draw a line like so notice it's a pencil right now it's kind of probably really small on your screen but that's a little pencil right there what that means is it's not a fully constrained sketch so you'll notice that there's some open areas this line is free to move we haven't constrained that at all or anything as soon as I finish my sketch or constrain it fully like so you'll notice that it switches to a lock symbol and that means that it's it's fully constrained so that's what that that little icon means okay when I did my extrude my sketch automatically turned off so I'm gonna go ahead and turn that back on I could rotate to the bottom of the part but I'm gonna click and hold my left mouse button for about a second and it's gonna allow me to probe through so the first thing it's hitting is the face then it's going to hit that profile and then the other face also so it allows me to probe through without having to rotate and I really highlight this because you know I have one of these really cool 3d connection mice that you can rotate and move around a lot kind of stuff in fact I'll show it here for those of you that haven't seen this it looks like this and allows me to you know rotate and pan and zoom and stuff but if you don't have one of these it's a little bit tougher to rotate around you might use the cube up here maybe you use the shift middle mouse button or whatever but instead of having to rotate I can just click and hold and select that profile okay all right mouse click and say extrude now I'm gonna start to drag and you'll notice an issue because the profile is cutting through my part fusion assumes that you want to cut through the part but in this case I don't I want to join I want to add this geometry and I want this to come up let's go up sixteen millimeters according to the drawing so I'm gonna come up sixteen from the bottom because that's where my sketch originally was and so you can see I used a single sketch to create a multi-layered part okay so there's the the basics of the part again jumping to the drawing real quick there's the sixteen that you see that I just did right there okay the next thing I want to do is to create this a large hole through the middle and these counter bores so you'll notice there's a symbol on here this little down arrow that means depth so five millimeters deep from datum a and so you're gonna see right here datum a is this bottom face and this counterbore is gonna be five millimeters from that bottom face actually I'm probably worded this incorrectly because I'm saying it's five millimeters deep I should say it's five millimeters from datum a so disregard that I might change that okay so let's jump back in here let's do the the larger hole first and I could use a sketch to do that but we have a really cool command called hole and I really like this command because it gives me a lot of power and watch what happens so what I did is I just clicked on the face I pre-selected it then I got a right mouse-click and about four o'clock it says hole I could also come up to the create menu and right about here just under halfway is the whole command or H is the shortcut key okay so I'm going to say hole and you'll notice it gives me a little bit of a preview of what's going on here well I start out typically I start out by changing the hole to this simple hole okay now check this out I'm gonna grab and drag on this blue dot and when I do that you'll see a couple other little blue dots appear and I'm gonna point to it with a little arrow right there it's about seven or eight o'clock there's a little blue dots I'm gonna get near that and it's gonna snap to that dot okay well that's the center of this cylindrical face so I don't even have to dimension or anything like that I'm just saying I want this to go through the center of the part so all I have to do is get near that and it's gonna snap to it okay so I don't even have to do these references I want it to go all the way through so I'm going to say all and so you can kind of see how that changed and now it's going all the way through if it was just set to distance it might not go all the way through it might look something like this okay so I'm gonna say I wanted to go through all so it goes all the way through then I come in here and I see this little preview and I know that the diameter of this hole I want it to be 28 millimeters according to the drawing but it also has a small chamfer on it and this is kind of why I like to use the whole command because I can also do counterbored holes or I can do a countersunk holes so I'm going to say countersink and notice it's actually already filled in let me make this a little bit different I'll say 35 or whatever and you can see that it's gonna actually countersink that hole for me it's gonna put that angled chamfered edge right there well according to the drawing it's supposed to be 30 millimeters so I'm gonna type in 30 and I'll say okay now I could have created this sketch with a circle extruded that through and then use the chamfer command to chamfer that edge and that totally would have worked but notice this is one feature in the timeline instead of a sketch and extrude and then a chamfer feature this is all one and I can come back and change this very easily so instead of 28 I want it to be 20 I want this to be 22 for example or whatever so I want it to be a different angle for the chamfer etc etc I want it to be a counterbored whole instead of a counter so Nicole so you have a lot of power in here I can make it threaded or tapped is it flat or drill pointed etc so I really like the whole command in fact I'm going to use it to do these counterbored holes on the side so same thing I'm going to pre-select my face I'll say hole now it remembers my last size so it looks fairly large so again I'm gonna I'm gonna start by changing it to a simple hole and then these guys according to the drawing is a nine millimeter through so I'm gonna do nine for that and you can kind of see it gives me a little bit of a preview and then I'm gonna start to drag and you can see I have those two little dots now why - well this one over here is the center of this whole face it's like the centroid of that face this one over here is the center of this curved surface right here so once again I'm just gonna drag and drop it on that dot and it's in the correct location okay I'll say I want it to go through all it figures out the distance that it needs to go and now I'm ready to do the counterbore so I'm going to switch from a simple hole to a counterbored hole and you can kind of see it gives me a quick little preview what that's going to look like I can come in I can change the size or the DAP of this counterbore manually or I can come in here and say according to the drawing it's a 16-millimeter counterbore now here's what I was talking about notice the depth that it's asking for okay according to the drawing the counterbore needs to be 5 millimeters up from the bottom so this depth right here actually doesn't matter okay I'm just gonna leave it I'm gonna leave it some random number I'll go ahead and say okay okay and there's my counter board hole but if I were to measure from that face to that face we can see it's not 5 millimeters it's five point seven six eight okay so how do I fix that well cool little trick I'm going to select that face and I'm gonna press pull on it okay now when I do this it's gonna allow me to move this face up or down by default sometimes this is set to automatic so it's basically allowing me to move it a certain distance from where it was I want to do a new offset and what this is gonna allow me to do is I can click this little down arrow and I've shown this command before I love it it's called re anchor so I'm gonna say reinker to this bottom face and you'll notice okay if I can look at it from the side there's that four point seven four seven so it's basically saying this face and in fact I'll go ahead and move it here you'll notice it's now like six point three from the bottom of the part so if I were to type in five that face you know I started to pull it down then I'm referencing that face and I'm saying I want it to be five millimeters from the bottom of that face using that reinker command it's extremely powerful and the only reason I'm showing you this is because you don't know how you're gonna get the drawing you know maybe they said the the counterbore is 2.5 millimeters deep okay that's great but in this case the drawing was saying there needs to be five millimeters of thickness here before that counterbore so I was just showing you a couple different options so we used the offset command and at the re-inker command and if I were to measure that face to that face we can see that it's five millimeters now so that's perfect okay now I want to do the exact same thing over here well instead of you know redrawing recreating or whatever we can use a couple different commands and some of you might say oh just go ahead and mirror it to the other side and that would absolutely work so I could use the mirror command to do that well I'm going to show you another command that you might not think about that works also and that is to create a pattern and in this case I'm going to do a circular pattern so I'm going to say circular and notice it's asking for faces bodies features or components well I I could do faces but I'd have to manually select all of those faces and then what happens if we end up adding a chamfer to it or whatever so I'm gonna switch this to features I want to pattern the whole and I want to pattern the offset that I did because if I only said pattern this whole they wouldn't be at the same level because we made a change to it afterwards in time so I'm gonna select both of those I'm gonna select the whole feature and I'm gonna select the offset feature and you'll notice that selected all those faces for me I'll come in here and specify what's the axis I could select this circular face cylindrical face or I could pick on this axis since I created I started out kind of in the center it really doesn't matter in this case I'm gonna go ahead and select the axis right there and you'll notice it gives me a preview which doesn't make a lot of sense but watch what happens when I go from 3 to 2 so it's still doing a circular pattern if I can kind of see that light arc right there but we're only doing two of them I'll say ok and I now have that over on the right okay so mirror would have worked the pattern also worked ok the last thing according to the drawing is a one millimeter Filat which I don't have on this one that's interesting need to update my drawing so I'm going to add a 1 millimeter fill it to this edge and to this edge so watch what happens when I right-click and say fill it you'll notice it kind of finishes selecting that edge for me and that's because of this tangent chaining when I selected this edge it said is there another edge tangent yep right here there is it's gonna continue on is there another edge tangent yep there is so it selects that one also it's a pretty powerful option there I'll go ahead and say I want that to be 1 millimeter it fill it sit for me I'll go ahead and select this edge here in this edge here and you'll notice that it selects those edges now I'm gonna cancel that I've shown this also where I could select a face and say I want it to be 1 millimeter and it actually fill its all of the edges that that face is touching but you'll notice that it's also Philippine the circle here or the counter or and unfortunately because that this edge is part of that face I can't unselect it no matter what it always selects it okay so that's why I manually I said that edge and that edge and it chained it all the way around let's make that one and I said that edge and that edge and we get a nice-looking finished part okay so I'm done with this I'm gonna go ahead and save this I'll call this I'm sorry let me put it in the correct location um I'll just put it in here for now okay um I'll just call this a nine-to-five part save that guy and now you can see it's called nine to five part okay so I finished my design and maybe I have a design review with some of my fellow engineers and stuff and we decide that this part isn't quite strong enough and maybe needs to be mounted a little bit different so they want four mounting holes and they want it to be stylized a little bit nicer maybe with some curved surfaces and stuff because this parts gonna be visible or something like that and we've kind of came up with an idea of making it look more like something like this okay and you might look at that going wow okay so it's got some curved surfaces let me zoom up here you can kind of see the curved surface here a curved surface here but the part looks pretty much the same so I should be able to maybe reuse my existing design and modify it and that's what I'm gonna show okay so I'm going to start by creating a sketch on this front plane I want to curve these surfaces right here these flat faces and a lot of people like well how would you do that well I'm gonna show you a cool little tip I'm going to use surfaces in the surface menu to help me out with this but before I get there I need to create something that I can extrude so I'm going to draw a circle somewhere on the screen again notice it's in diameter mode okay so I'm just gonna place it I'm gonna place my dimension or start my dimension I should say and say I want that to be a radius of 240 now watch what happens when I hit enter my circle disappears and look what happened well if i zoom out you'll see that it's kind of way up here in space okay so I'm just gonna drag that down kind of closer to where I need it to be something like so okay now I want it to be lined up you'll notice that it's kind of off-center a little bit okay so I'm going to create a horizontal vertical constraint so I'm going to say I want that point there to be vertical in the same line as that point there and you can see it kind of shift over a little bit okay now I can zoom up just a little bit more and I'm gonna move this up so it's too long I'm gonna move that down just ever so slightly so you can kind of see what's going on here now according to the drawing this curved surface is three millimeters from the top okay so I need to dimension the top of this circle to be in line with that so if I go to my dimension tool you'll notice I can click on that edge but then when I click on this edge it wants to go like to the center right which is not what I want okay so here's another cool little tip I'm gonna say dimension I'll click on that edge then I'm gonna right mouse click and notice right here it says pick circle arc cent which is what it did by default or pic circle or arctangent so I'm going to click on that guy click on this circle in fact I'll click way over here and notice my result okay so instead of jumping all the way down to the center of the circle it's now going to the tangent point right there I'll go ahead and place that dimension and we know it used to be 3 millimeter so I'm going to type in 3 and we can see that sure enough it pushed that arc or circle in this case down to be 3 millimeters from the top kind of a cool little trick there okay just remember right mouse-click is your friend it has lots of helpful options in there so I've created my correct a sized circle radius of 240 I've made sure it's lined up perfectly in the center which it is and then I've positioned it where it needs to be and you'll notice the little lock symbol which means that this sketch is fully constraining which is good okay okay so I have this circle now here's where I'm going to jump over to my surface tab and under the create menu you can see that we can extrude surfaces revolve sweep loft etc by the way this ruled surface we just added this last weekend really really cool make sure you would check out the what's new if you haven't already if you go into the question mark what's new it'll bring up a web page which of course is on the wrong screen let me drag this over hopefully you can see this and you can see all of the cool enhancements that we've done and one of them is for example party-line in draft the new ruled surface see it in action so you can kind of watch these videos and stuff like that see he's actually dragging these edges just by kind of rotating them around and stuff like that it's pretty pretty so anyways I digress make sure you take a look at the what's new if you haven't already okay so I'm in my surface I'm going to say extrude and I'm gonna click on that profile I'm just gonna start to drag and you'll notice it's creating a thin-walled surface there's no like thickness to it it's not a watertight model I also want it to go symmetric because I want it I want this new surface to expand past my existing part and watch what happens when I say okay I get my original body which is this part here and then I get this open shell looking type body which is this surface right here okay now here's where the magic happens I've shown this in some of my other live streams I'm gonna jump back to my solid tab under modify is replace face okay now notice the pop-up that comes up replaces one or more part faces with a different face the new face must completely intersect the part okay and that's why I purposely made this larger than it needed to be if it was too small this wouldn't have worked okay so I'm gonna come in here and say replace face what's my source and notice it says faces so I can select multiple faces so I'm gonna grab that guy there and that guy there now you might be saying well what about all of the Phillips that are touching that face check this out what's my target face my target face is going to be that surface and look what it did I'll go ahead and zoom out a little bit I'll say okay I'll turn off that surface and it actually replaced that flat face with that curved so and it kept all of my Philip's for me automatically so let me undo and let me do that again so notice they're flat right there they got Phillips on them etc I'll say replace face I'll say I want to replace that guy and that one there the target face is gonna be this face here and you can kind of see it jump up in fact it kind of see the surface on that top surface there all now I don't need this extra little body anymore so I'm gonna turn it off okay so I'm just gonna hit the little eyeball next to it and turn it off also notice what happened to my counter bores if I say measure from that face there to that face there there's still five millimeters in thickness that was one of the requirements according to the drawing but the counter bore is now deeper due to the fact that we changed that surface so hopefully you're good finding that replace face is a pretty powerful tool some people might be like I don't have to go into direct modeling and you know pull on that face other people might be like I'm gonna have to create surfaces and extrude up to those surfaces etc the replace face command is extremely extremely useful okay so now what I want to do is let's take a look at our drawing here so you can kind of see this is the curved surface right there what I want to do now is maybe create this extra material you can get it's kind of hard to point out but you can kind of see this little wing right here or these little webbings or whatever term you want to use so I want to create those next and it's also kind of hard to see but they are also crowned right here the 240 radius so how would we do that well I'm going to use some information here to help me create that so a radius 20 circle that's 52 millimeters from the center so I want to create a new sketch on the bottom face here so I could go back to my original sketch but in this case things are changing this is way back at the very beginning I'd be a little bit nervous that you know none of these features would show up if I were to go back to my original sketch so I'm going to create a new sketch like so okay I'll I'll create a circle over here somewhere again don't care what size well to mention that right click radius place my dimension and that is supposed to be a 20 millimeter radius okay I know that it needs to be tangent to this guy so I'm gonna go ahead and click and drag with my line tool and you can see the tangent then I'm gonna get near here until I see that tangent icon there same thing here tangent until I see the tangent icon it's a little hard to see but it's right underneath my cursor it kind of snaps to it and if I were to move this circle now you'll notice that those lines stay tangent to it it's pretty cool okay so I want that point and that point to be vertical with each other boom it snaps it to be vertical and then finally according to the drawing the dimension actually comes off of the bottom of whoops wrong drawing sorry the dimension comes off the bottom here okay again I said I threw a couple curveballs in here just to let you learn some new commands so I'm going to right mouse click and instead of dimensioning to the center I'm going to say tangent I'll click on that circle there I'll click on that point there place my dimension and you can see that the dimension is tangent to that circle and according to the drawing here 52 millimeters so we can see that kind of pushes everything up the lines are turned black and my sketch has that little luck symbol next to it so I know that this is a fully constrained sketch so I'm gonna say finish sketch okay let's take a look at this guy now and I'm going to select these three regions right mouse click and say extrude you've seen me do this multiple times I hardly ever go up to the menus they're all usually in the right mouse-click it shows you the commands that makes sense so instead of having to figure out which command I let fusions show me which commands so I'm gonna say extrude I'm gonna start to drag up okay now I'm supposed to extrude up eight millimeters now notice what happened okay so I'm gonna have to say minus eight millimeters but notice what's going on right here we're gonna run into an issue here and this is the exact reason why I picked the design the way it is because this is what's going to happen to all of you all so it's not perfect every single time in fact I did a live stream a little while back where I called it stump the chump where I just randomly picked the drawing and kind of struggled through it and wanted to show different methodologies different ways you could do things well this is a prime example of that you go to make a change you want that to be 8 millimeters thick but my I get these weird faces so we're gonna learn how to fix this kind of stuff so I would be a little bit nervous that this could cost problems and I want to work almost like on this this flange as a separate body so I don't want it to calculate along with all these other Philips so instead of joining I'm gonna say make this a new body it's eight millimeters tall I'll say okay and now you can see that this is its own separate body from that guy okay it's in the correct location and everything but I'm gonna kind of work on it by itself until I'm happy with it and then I'll combine it with the original body okay so now I want to do the concave part and just like before it's the same radius it's the same distance so I'm going to create a sketch on this you know front face right here I'll draw a circle throw a dimension on there make sure it's set to radius and it's supposed to be 270 I'm sorry 240 and it disappeared so it's way up there so I'm just gonna drag that closer to where it needs to be like so and just like before I'm going to constrain it vertically like so can I see how that jumped across and I'm going to add a tangent dimension I'll click way up here like so now you'll notice it's not letting me sorry it's not letting me well there we go I can pick that point there I could pick that edge but you'll notice it's not letting me pick any of those points there so I could project it or I could just grab like this bottom line and I'll say three okay sorry for my little reminder that says keep open because I never know if my live streams are going to go longer or not so I always block off some time for that okay so I now have the circle it's perfectly centered and it's three millimeters up I'll finish my sketch now I could use the replace face again but I'm going to show you another method that would work in this case where I'm kind of machining some stuff away so instead of adding material that's where replace face really kind of shines is adding material but I could just split this body right so I'm gonna come in here and say split body what's the body to split well because they're separate it's only gonna affect this new little body this body three okay and it's not gonna split body one what is the splitting tool this circle and you kind of see it gives it a nice little preview it's almost doing like what I did earlier it's kind of creating a face and using that to split that body and now you'll notice I've got body three and body four well I don't need body three so I'm gonna right-click on it and say remove now I get asked a lot what's the difference between delete and remove okay so the best way I can kind of explain this is think of like an Ikea bookcase okay if and it has a bunch of shelves and I want to remove one of those shelves out of the bookcase I would say remove and I'm basically taking that and it's no longer part of my bookcase but I haven't destroyed it I haven't you know gotten rid of that shelf I've just removed it out of there if I said delete you can kind of think of it as we're trashing that shelf we're destroying it we're wood chipping it burning it whatever it is no longer there and I can't bring it back and if any of the my drawings or my models referenced that shelf and I deleted it it would cause downstream problem so I usually say 99% of the time you're probably gonna want to remove sorry you're gonna want to remove your part instead of deleting okay so I'm gonna say remove and what's cool is you'll notice it removed it it's no longer here however it did put it in my timeline so my self is still there I can always go back and get it and put it back in my design whereas if I had deleted it it might have caused downstream problems okay hopefully that makes sense okay I want this on the other side I could use the pattern command I've already done that for for this so let's use the mirror command in this case just to show that it really doesn't matter so I'm gonna say body I want to mirror that body what's my mirror plane let's do this face right there I'll say okay and now you'll notice I have three separate bodies okay so let's combine those into one so awesome come here and say combined now I don't show this all that often it's really cool if you hit the S key which stands for shortcut it will bring up shortcuts like your most commonly used commands and you can edit these or whatever but what's kind of cool is you can search so I can search for combine so you can see as I start to type in C om so there's the combined command okay I can actually run it from right here I can also add it to my shortcuts so instead of having to remember because I use the combine command all the time instead of having to remember it's in the modify menu and then come here I can just hit the S key and there it is right because I just added it to my shortcuts so really cool tip is using the s key to search for commands and then also add your commonly used commands that you don't want to have to go to the menu every single time for okay so my target body is going to be this guy that's what I want to join them to my tool body is going to be that guy and that guy and we want to join them together now if I said keep tools it would keep the original bodies but watch what happens I'm gonna say ok and we're back to one body now okay now I'm going to zoom up I still see a little issue here we might run into that just FYI so but let's keep moving forward so I have this all as one body now now what I'd like to do let's take a look at the drawing and it's gonna be a little hard to see but I have this curved surface here and then I have this webbing or whatever you want to call here I want to now create these other arms or whatever term you want to use but notice they're flat but we've already curved these guys so how am I going to do this so here is the power of going back in time okay excuse me so what I'm gonna do is I'm gonna create a circular pattern this is pretty cool so check this out I'm gonna say circular pattern okay I'm gonna make sure that my pattern type is set to features because I want to pattern some features when I want to pattern some features way back in time so I'm gonna pattern a bunch of this stuff way back here before we did some of these replace faces and stuff like that so I want to make sure I grab that extrusion and that extrusion I also want to make sure I grab the hole and I want to also pattern the counterbored holes and the offset and because I pattern it over there I'm gonna grab that pattern there so I basically I'm grabbing pretty much every single step I use to create my original part except for this sketch you know really pattern sketches so I'm doing the extrude I'm doing the the second extrude which is the the part that goes up a little bit higher then I did the hole through the middle and then I did the counterbore and the offset and then finally the pattern of that so I'm going to get both of those counter bores okay and this will make more sense as we go through now I'm gonna go ahead and say what's my axis I'll pick that that Center axis right there you can kind of see I get a quick little preview it's trying to do three of these well I only want two of them but notice what happens when I say - it's basically patterning it 180 degrees so that doesn't work I don't want three of them but if I say four you can kind of see the preview that I'm gonna get here okay so I'm gonna actually circular pattern this four times and I watch what happens to my bodies over here I'm gonna go ahead and say okay and you'll see that we get a result that looks like this but notice they're flat okay so I'm gonna go ahead and start turning some of these guys off okay now for whatever reason this counterbore didn't go through which is odd the hole did let me make sure I did that correctly one quick second okay let's try that one more time so I'm going to create a pattern circular pattern features I want to make sure I grab everything okay adjust is correct axis well maybe do that guy let's just see what happens with that quantity of four I'll say okay no I'm getting a weird result okay well I'll have to resolve out here in just a minute but basically because I now have a whole bunch of body if some of these don't matter like this guy right here I don't need two of them on top of each other so there's basically two right on top of each other you can kind of see the body eight and body six right so yeah that's interesting that it didn't do the holes this worked perfectly when I practiced it of course it doesn't work perfectly here so let me turn one of these guys off and we'll fix it so I don't need body six so I'm gonna go ahead and remove that out of there I also don't need body seven so I'm going to remove it out of there okay and typically this would be over here kind of surprised that it's not not one percent sure why okay but now I'm left with two bodies and we can kind of see that guy there and that guy there so let's turn off the one we don't need right now and let's fix this let's come in here and do a circular pattern again I could do features I can also in this case I could do faces so I could select all of these faces if I wanted to grab the axis again do two of them say okay let's turn that body back on and now I basically reused that geometry to help me over here okay now I want to combine these together so this is my target body my tool body will be this other one we want to join them together I'll say ok and I'm back to one singular body ok now I want to continue adding these Phil it's because we want these edges to be fileted and I've shown this before if I come into my Philip command and I click on a face it'll actually select all of the edges but watch what happens when I type in one I get an error message the Phillip chamfer could not be created and it highlights it in red and I I forced out of this earlier I said I'll bet you this is gonna cause a problem down the road and this is exactly what you might run into as you're doing parts like this and you're like well I want to fill it all the way around but because of this weird corner right here I have a feeling it's failing because of that well that's because it's kind of rolling over into this Philip so I'm gonna just click on that fill it and way back here in time it shows me which feature was used to create that Phyllis so I can select that right mouse click and say suppress now notice that that isn't you know rolling over into a different face so let's try our fill it again so I'm gonna say that face they're a size of 1 millimeter and voila that worked in fact I'll go ahead and do both of these at the same time ok so what just happened let me back up ok this is where messing with the timeline can sometimes help you and sometimes hurt you so I tried to fill up this edge and because it's going all the way around you can kind of see there's this little extra little slip what I would call a sliver face right here and mathematically it can't figure out what to do there so what I said well I want to solve it before this Filat is solved so I clicked on it I suppressed it I'm basically saying don't don't solve that fill it okay then I come in and say fill up this edge or this face I should say instead of selecting a whole bunch of edges I can grab the two faces boom boom I've just done I don't know how many fill its I'll go ahead and say okay okay now magically I should be able to unsuppressed this feature but notice what happens I get an error message and my Philip's went away why okay this is where it gets a little bit deep we're gonna be talking about going back to the future and forward and back in time and all kind of stuff so think about what just happened here I suppress this so this was no longer being calculated and I was able to add those Phillips but when I unsuppressed this it's like a recipe it starts at the beginning and it does the extrusions it does the holes it does the fill it's right here and continues on and then it tries to fill it that face but because this was created way back here in time it failed again right so it makes sense that I should have this maybe be after this guy so I'm gonna click and drag that fill it all the way to the end it's kind of hard to see but I'm gonna drop it there and notice what happens this works but the filler I just dragged is giving me an error okay so notice what we did here it used to be back here I think right about here before the sketch I just changed the past by dragging that feature all the way to the current location so now it's doing the recipe it's going along and it's able to create that fill it because it hasn't created this fill it yet okay but why did this one fail well if you right-click on it and you say review warning it'll actually tell you eight reference failures the edge references lost and it actually highlights in in red and hopefully you guys are figuring out what's going on here this Filat was created on edges before they were changed in time to a curb surface okay so unfortunately in this case it's looking for these edges in time but then we came along we created that surface we did the replace face etc so it basically lost it didn't know where those edges are anymore so I'm actually going to edit this Phillip feature in fact you'll notice there's no edges in here at all because it lost the reference to them but all I have to do is say it was that edge in that edge that edge in that edge and they were a radius of one and it allows it to be created I know this is a little little deep hopefully it's not confusing but we basically rearranged our timeline quite a bit we reused existing features okay we rotated them around we reused them back in time before they were curved to give us these guys here we were able to reuse the counter bores a lot kind of stuff we fixed an issue for whatever reason I don't know why it happened we were able to fix it by reusing that counter board hole and then I was able to fill it these edges by basically organizing when this edge rolled over onto this Filat and I that was what was causing the problem so we basically got rid of that fill it and then just reassociate Edyta to the edges that we wanted okay so the last thing is to add a couple more Phillips so on this edge here that edge there and that edge there notice I'm able to pick through I don't even have to rotate because I'm in the Filip command I'll say 1 millimeter fill it I also need to add that edge there and now I get a nice-looking casting so I'll do the same thing here now how did I know that I forgot an edge I'll show you I'll go ahead and click there and I noticed that that corner looked kind of weird I was like oh yeah I need to add in that edge and it recalculates and figures out how it would intersect and make that look really really nice I'll go ahead and say ok and we are done with our redesigned part so we went let's see from this guy to this guy without having to do a lot of recreation pretty much the only sketch I ended up having to do was was this guy here to kind of create those webs the rest of it was pretty simple so ok of course I thought this would be a shorter one I went 4 minutes over hopefully you learn something from this again the outline and the two drawings are in the description of the video so please feel free to get that a try I might actually throw this part over to Angelo and see how he would go about fixturing it and actually how he would add toolpaths to it so if you guys are interested in that keep an eye out for a future live stream I hate to put Angelo on the spot but hopefully he's willing to do that so with that I hope you have a wonderful rest of your day and have fun whew Janine you

Channel: Autodesk Fusion 360

Views: 8,644

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Id: l0YsxLeCQBk

Length: 67min 37sec (4057 seconds)

Published: Thu Jun 25 2020