 Okay I thought I was done with this model but several of you had some really good comments that I wanted to address. Specifically dealing with my decision of going with a circular hole here and the cutout for the pin. This brings up a great point which is that when it comes to 3D printing it's easy for us to bring in some self-imposed constraints that don't need to be there. When I thought about making the pin it was natural for me to want to go with a circular cylindrical shape because that is what I'm used to seeing. Traditionally this part would have been made on a lathe so the shape makes sense. Even though I'm no machinist my mind automatically pictured this shape because it's what I've seen. I haven't seen many designs that look like this. So I went with the cylindrical design. The problem was that the hole needed for the pin was going to be 3D printed in a vertical orientation. Weighing all my options I accepted that this was going to be the best orientation to 3D print the frame and I would simply have to do a bit of cleanup work after. Since printing holes in a vertical orientation doesn't give you the best results. Turns out there was one other option I hadn't considered and that's what I want to go into today. One beautiful aspect of 3D printing is that it removes a lot of the constraints that normally bound us but we have to consciously approach our designs with this awareness otherwise we subconsciously obey rules that no longer apply limiting our design freedom. So I'd like to shout out a few of you who helped me realize that this is exactly what I was doing. Brandon Owen 7563 first pointed this back in part three with this comment. Great tutorial I thought of maybe a slight tweak to the design to make things fit better together in print. Maybe changing the joint between the frame and the peg. Change from a circle to a triangle joint. Just so the frame prints better as the circle might distort too much printed upright. I didn't quite understand the comment at first thinking he was referring to making the shaft triangular. This was later clarified after Usafa at 1987 stated by the way for the design there is no requirement for the snapping section to be circular and thus printing with the bridging and needing to be cleaned up. That could easily have been a triangle that would have printed fine with no overhang issues. And finally quick bow who stated for the top of the hole modeling in a tear drop works pretty well. And I think that you are all correct. So in this tutorial we're going to look at some best practices of changing effusion 360 design without causing the entire thing to break. How to address the things that do break and some best practices along the way. All right here's our familiar design here of our rack in pinion. And if I turn this to the back well we see this is one I've kind of already started designing. I don't want to start here I want to start with the fresh design. Let me show you a quick tip here. If I open up my panel my data panel here and I click here where it says the version number so v6. I can click on show all versions and the first one I created here that I saved I'm going to open that and that's going to go ahead and bring me back to that version. And if I swing this back around you'll see that that is still a hole at that point. And you get this little flag up here telling you that you're not working with the latest version which is fine. If you click on it it'll restore it which I don't want to do. Okay so I've got my design here and just a little refresher on how I built this. You can see I have three components here. We've got our spur gear here and then our rack and then our base. And I'll activate the base and untie all the spur gear and the rack. And if you recall the base was made with two separate bodies. We have our pin here and then we've got our frame. So let's go ahead and rename those so it'll just make it easier to go back and forth. So pin here I'm going to call that and then I'm going to change this from body one to frame. Okay now that I've got those two let's do a quick look at how this was designed because that's going to sort of help determine what's the best way to go ahead and make the changes here. And then once we get errors if we do get errors we'll know you know have a little more insight into how to fix those. So first remember I started with a sketch here. I took this profile and then I extruded it out a symmetric extrusion to give me this shape. And then it looks like I came in with the sketch and that sketch there is on the back here where I made two circles. And then the next thing I did was create an extrusion. So that extrusion would have been for the pin here to give me that cylinder. And then another extrusion of that inner circle here to give me for the longer cylinder there. The next button there was the offset or the next feature here. And if we double click on that offset it'll show us what that was. So here what I did was I took this back wall in this front portion here and I offset those negative 0.2 millimeters in both directions. And the purpose of that was to give me some clearance here for the rack to move back and forth. All right so let's see it'll click cancel there and let's go one more. So this is a Boolean operation and with that that allowed me to cut the pin from the frame here to give me the shape here. And then if I go one more we've got another offset. In this offset if I double click on it you can see what that did was it gave me the clearance here for the hole. So that one was a negative 0.1 millimeter clearance to allow for the pin to fit there and give me a nice sort of friction fit. Okay now that we see how this design was built let's talk about the best approach here to change this circle to be a triangle. So the place you're probably going to want to start is that sketch where I created this circle. So let's go ahead and open that. I'm going to double click here on a timeline and that was that second sketch there. So I'll untaggle bodies and I'm just going to show the current sketch. Now when you need to make a change to a sketch and you don't want it to break the rest of your design you want to avoid deleting sketch entities. So you can come in and delete for example sketch dimensions and sketch constraints and give them new constraints and those will translate fine. Your design will be updated and it will work great but when you go ahead and delete like if I delete a circle or any other sketch entity then I'm causing trouble. So here I'm kind of faced with a dilemma. The only way for me here to change the circle to a triangle is to just delete it and make a new triangle. I can't edit the circle and make it a triangle. So unfortunately this is the way I'm going to have to go. So I'm going to grab the circle here hit delete and I'm going to come in with a polygon circumscribe polygon. Start it at the origin there start dragging it out hit tab give it three for three sides and I'll go ahead and hit enter here. I'll take this top edge here make that horizontal for now and I'm going to hit D for dimension and let's go ahead and make this 30 millimeters. All right now I'm going to create an offset of this so I'll go to modify down to offset select the triangle and I'm going to go to five millimeter offset and click okay. Okay now that I have the sketch that I want I'll click finish sketch and there are a couple things here I want to point out for example if I untie all the frame you can see that fusion was smart enough to know that okay I took that circle that was there I changed it to a triangle so it went ahead and changed the shape here of the model to a triangle not only that but if we untie all the pin and bring the frame we can see that it carried that over it says okay since that pin has been changed to triangular shape I'm going to assume that you want to discard out here to also be triangular. So those stay intact but not everything is as it seems because if I go back to this extrusion here that made the pin you can see that in the dialog box here it says missing profiles normally it would highlight it yellow telling you that something's off here but I have a good idea of what you're trying to do so I'm not going to break anything but here we don't see that and it's not until you open that profile that you see that it has missing profiles at easy to fix we can just bring that sketch back into view and then just tell it which profiles we want so in this case I'm going to click here in the circle and it will go ahead and update those profiles we'll click okay and there we have it. So in cases like that where you have to delete a shape and remake it expect to go back to the extrusion that reference that profile and remake those selections. All right let's keep going forward and see what else we need to fix here. Now here I have to make a few more changes I want this cut out here to go all the way through so I'm going to go back to the edit feature there and for that distance instead of negative three millimeters I'm going to say distance to object and my object I'm going to reference the front of my frame and click okay and now that cutout goes all the way through. All right you keep seeing this error here this is referencing this last offset here it's not an error after every change I make it's just every time it goes back to the model workspace it tells me I have an error and we're going to address that in a few minutes. Okay next I'm going to bring the pin in and I want to add this outer profile here to my body there so I'm going to create a new extrusion here e4 extrude I'm going to take this arrow and drag it out and let's go negative three millimeters and hit enter okay so now we have this shape here and I want to bring up another point here so if I go back to the frame you'll see that the cutout is not what I want it to be so I really want this shape here to be cut out of this frame the problem though is that this extrusion I created it at the end of the timeline so it was created after this Boolean operation and that Boolean operation is what cut the pin from the frame so there's a couple ways I can address that one way is I can I can try to select this combined feature here and that Boolean operation and have it reference the extrude feature here problem with that though is that the extrude feature was created after the combined feature there so it grays it out it doesn't allow me to select it so we'll just say cancel there and so the only option here instead of deleting and remaking things is taking advantage of your timeline properties here now watch this keep an eye here on this cutout and if I take this extrude feature and drag it back in time and I put it before that combined operation notice how this updates and Fusion knows okay if you're telling me that that feature there was created before the combine then that means by the time we get to the combine this is what this is going to look like because that pen shape has changed and this is what you want it to be so even if you create things after the fact in some cases you were able to bring them back by just dragging them and this will update your design so again much faster and efficient to go this route than to delete this and try to remake that combine operation okay let's make a few more changes here I don't like how sharp these corners are so I could come in and fill it this and then go back to the pen and fill it that as well but let's do it a different way so here I'm going to go ahead and add some fillets here so f4 fill it and I'm going to select each of these edges so three on the outside three on the inside I'm going to do a two millimeter fill it there and click okay now here we've kind of have the same situation if I go back to the frame bring that you see that the pen is filleted but the frame is not now what I could have done is actually drag this timeline here back to before the combine again and done to fill it there I can say go here and make the fill it but because I didn't do that I can use that same approach where again let's look at the back of this I'm going to take that fill it operation and just drag it back before the combine and notice how that adds the fillets to the frame there so again if I take that fill it drag it back to after the combine we get sharp edges and I drag it to before our edges are now filleted as well because again we're telling it to assume we did the fillet on the pen before we did the combine and this is the result you would get so a lot more efficient than coming back and adding the fillets there another thing I'd like to address is this pin here and sort of how it bumps out a little bit more than the wall of the frame here now the reason for that if you recall we did an offset on this back wall and that's right here at this point where we took it in 0.2 millimeters and the extrusion on the pin happened here before the offset so the way I'm going to address this one is I'm just going to go to that offset feature and it's going to tell me the faces that are selected I'm going to say you know what just add one more face to that and I'm going to command or control select the pin here may be easier to untangle the frame there and just click and grab the pin there and you see it's going to add that to the number of selections so it says there are three faces now instead of two and I'll click okay and now when I bring the frame into view you can see they are now even okay so that addresses that and let's finally address this little error here that's been screaming at us the whole time to get a little more information on that error we'll right click and go to review warning in here we see it says the face references lost try editing this feature to reselect the lost faces so same type of deal we lost some faces and if I orbit it'll actually show you where if things those faces should be right when this was a circular hole these were the faces that were offset since this offset is the last feature on the timeline we can actually just delete it and create a new one and it wouldn't affect anything because if there's nothing after it then that means nothing is relying or referencing that feature but I'll show you how we can just go ahead and edit it if I double click here and bring up that feature I can simply go ahead and make my selections here and so number of faces was set to zero because it didn't know what we were referencing and I can go ahead and continue selecting and if you start getting weird stuff like this especially with the offset face tool and as you select more faces it'll kind of act weird it's trying to put an offset there I'm just going to set that to zero so it doesn't change my design and then I'm going to make my selections first here sometimes you may need to hold command or control now it's going to be quite a few more selections here then we need it for the circle because the circle was just one loop here we have all these fillets that we have to select so I'm going to go ahead and select those so I should have 12 six for one six for the other here I'm going to enter that clearance of negative 0.1 millimeters it's going to make it just slightly bigger and there we have it so you see we lost our error there and if I double click to select it we have our 12 faces with a negative 0.1 millimeter distance for an offset and here if I bring the pin in you can verify that offset if I zoom in you can see you have a little spacing in between those two if I bring the timeline back see how it's gone and I bring it after the offset it's there okay so that takes care of updating this design so that now we have a triangular pin there instead of a circle before I forget I'm going to click on this pin here because I made this mistake last time I forgot to add an offset to that so modify offset face and I'm going to do a negative 0.3 millimeter offset on that just to give me enough of a clearance there so that the spur gear will be able to spin around that all right I can already hear some of you saying hey that triangle you've got there that's not the best way to orient it because now you've got a bridge here so we need to flip this upside down so that the narrower side is facing up now this allows me to show you how making changes should work in fusion so in this case it would be as simple as going back to that sketch and let's untangle the body here and I want to flip this triangle so the pointy side is facing up now the way you don't want to go about this is to delete the triangle and remake it and in this case we don't have to do if I go in and try to move this it's not going to let me well that's because we have a horizontal constraint here all I have to do here is delete that constraint now it's going to let me move this by just dragging one of the points and when I get it close I'm going to grab my vertical constraints here and I'm going to constrain that point to the center origin here and that's it now watch what happens when I click finish sketch the model updated so that the pin is now facing this way you know the pointer side up and not only that it went ahead and changed the frame as well so that extrusion is facing the correct way right because it'll update everything cleanly down the timeline so when it's done right it's a beautiful thing the way it works to make a simple change like that and having it travel down your timeline and updating all the other features that rely on that shape okay that's the way I would approach this design here to go from a circular cutout here to a triangular cutout all right let's 3d print this and see how much better it is okay let's go ahead and 3d print this and see how well it fits all right I know this was a bit of a long one but I hope you found it informative if you're getting value from these tutorials consider becoming a patreon supporter link below I've also got some great resources below including my free fusion 360 constraints cheat sheet along with links to my fusion 360 online courses including my weekly live class where you can get live help with your designs