Fusion 360 Cylindrical Cam

in this video let's take a look at how we might model a traditional cylindrical or a barrel cam in this case for of shifter and if I rotate this part and look at it so we have a hole through the center some threads up here at the top that the the difficult part of the critical part in are these cam slots that are going around here and how to model those Camp slots and before I do that I'm going to go to a more simple model and we'll see how to set that up so here I have park going through here with a pin on it that would lock the pin is or so either this part is stationary or the part that goes into it is stationary and one translates rotates at the same time let's look at how I set this model up now I'm going to bring the history tree back to the beginning or the time line and if I look at my first sketch I have part of an arc the purpose for creating that arc then is to create a sheet metal flange because in fusion 360 we don't have a wrap command to wrap a profile around a cylinder we have to model it as sheet metal unfold the sheet metal create our pattern and then repo get back up so let's look at a couple considerations though so this is a critical consideration let's inspect this arc the length of that arc twenty nine point four five you need to remember that number that's just the arc from here around over to here alright and then I'm going to go to unfold my part now I used unfold not flat pattern coming in but unfold and I'm going to measure that length so I'll measure it and I see that it is now two point six one five so before let me bring this back over here so if I inspect just just this length right here that's the arc at now two point six one five where before we unfolded that it was two point nine four five it notices a lot shorter now than it was when we started with here's what happens when you fold a sheet metal part the material stretches on the outside of the band and it compresses on the inside of the band and so Fusion is calculating that stretching and it's it reduced the length of the part before the part is stretched or or bent the neutral plane where there is neither stretching or compression is generally not right in the middle of that thickness it depends on the material this thickness of the material the bend radius and the bend angle and perhaps a couple other parameters that determines that stretching kpac so if I go back to my sheet metal rules and I edit my sheet metal properties and my rules the default K factor is 0.44 so that means the neutral plane is 0.44 percent of the thickness from the inside of the bend radius in this case we don't want this to stretch at all because we're not making a sheet metal part but we're using sheet metal to kind of cheat and get around a limitation in functionality in fusion 360 so I'm gonna set my K factor to one so that would be out here zero would be here but that's the minimum radius of my cylinder and then that would be my maximum radius no I don't know if you saw that but the part just lengthened when I clicked on that so I could come back here so I want that maximum radius I want to keep actor out here the one I don't want this minimum radius so that distance of that art Clank long there is shorter than this one this is the one I want to use and again I measure that and it's two point nine four five and I go to my unfold again after changing the K factor and I inspect that and it is two point nine four or five so that's a critical step in getting the rest of this to work out correctly so the next step I do is I create my displacement diagram and so here I have created my displacement diagram certain distance from the edge if I look at the dimensions now normally we do these dimensioning in relationship to a number of degrees around the cylinder and so we could set up a pattern of points say 360 points for one point every degree along the length of that arc so that we could then define this relative to the angle but in this case I did it to a length to keep this one simple now when I did this let's back up for one minute my thickness of my follower or the distance of a slot from here to here is 0.25 so I did half of that distance of the pin that's gonna go in here is 0.25 I did half of that distance because this is the key what I need I really don't need this out here I really don't need that out there the only thing I need is the centreline travel of the tool that's going to cut this slot so that's why I did it - just to the centerline and one side or the other side it doesn't matter which side that we go to and then I extrude to cut that through the sheet metal part I then refold the part back up again now this isn't as simple as you might think well I'll just extrude cut through here and you know that wouldn't give us this shape here it's different can't just do a sweep either a sweep of a rectangle and I'll demonstrate why here in a couple of minutes let's turn off that and then the next step is ideally did everything on that sheet metal part except for the centerline this fact you'll remember now what it was this one of this when I guess it was this one this was the center line of our slot I delete everything except for the center line and actually now I'm confused about which one that is it was one thing that might be useful is to change the the color properties of your geometry the face that you want to keep let's go back here and I'll go to where I've extrude cut that and remember this was my sketch and I'll do it on this face because this is the this is my centerline of the slot right here so we'll go to the appearance and I'll put this on faces and I'll drag that to that pace and to this face and to this face okay so that's the centerline of my slot right there I go forward and so I've wrapped that around and hide that sketch now and I delete everything except for that centerline that's the tool path I then extended that slighting line you may or may not need to extend it I extended it on both sides slightly sometimes you might get an error where it will leave a sliver face if you don't extend that a little bit and then I have the sketch for my cylinder itself so I extended @b into this cylinder and out of the cylinder to make sure that I don't get any kind of errors where it doesn't completely intersect that face then I do a thick and cut of that surface body so I thickened it mid playing 0.125 on either side to cut my slot I then created a work plane at the end of this curve I drew a sketch circle on that work plane this better turn that on so we can see it so I have it the work plane created at the end of this line I draw a circle and an extrude cut that circle to give me the end of the tool think of a how this is manufacturers so you'll have an end mill that moves along in this direction and the end mill just goes in a straight line it continues in a straight line while the cylinder rotates to produce the cut let's look at this in Autodesk Inventor where I can do a little bit more explanation of what's going on so we're here we have a pin and that pin is going to go into this slot I want to animate this to show how this works let's first let's look directly at it and in inventor I'm going to go to the dynamic simulation environment and so I've set up a 3d contact between this pin and the slot in the cylinder and the way I have this set up the pin can only translate it only goes in a straight line this part will rotate you could have it too just the opposite where this part is fixed in space and then this part translates and rotates anyways let's look at it it worked so we see the pin goes into the slot and it pushes against the slot which pushes the cylinder I'll play that again now I'm gonna stop this at a particular location now right in here someplace let me try that again where there is a high degree of change in the path that is where we can have some interference or where there should be no interference between the cutter and the past so let's just look and see how much interference there is so I'm going to go to the inspection tab and I'll analyze interference I'll select my first part I'll select the second part and I'll say ok and it says that there is an interference but let's look at how much that is saying that is it says 6.2 e to the negative 7 cubic inches so e to the negative 7 you would have to move this one and then 6 more decimal places so essentially that's just a mathematical error that going down to many decimal places but at that interference the major interference would occur in here in here if there was any interference now this is where if you tried to do a sweep of a rectangle along that path you would find me more interference so it doesn't give you the correct solution and let's look at why that is so I'm going to go to a section view of this and let's look at this view that in half section here and we'll go back to the dynamic simulation so notice the tangent point between this cylinder and this slot is right here at this time I will go back to the beginning and I'll play it again so right now the tangent point between the pen and imagine again this is an end mill cutter that rotating and it's cutting the slot the tangent point is if there's six o'clock in the 12 o'clock position as it goes down in a straight line then as we come up along here that notice the tangent point is here and on the other side it would be up in here someplace notice that this portion of the slot doesn't even appear to be touching it says it is touching but it's way up here where it's touching but if you did extrude cut with a rectangle it may come up here where there's actually a lot of interference there and so the tangent point is changed here it was down here so it was continued as it came up here that it was continuously variable that tangent point moving up here up here up here up here the same way on that side where it was cutting the slot and so I get up here and again when I look at it in section view it doesn't look logical that when we leave section view we'll we'll see that it is it is correct this is this this is what that cylinder is cutting let's reverse that section view so I'll go back to the View tab and I'll leave section view and I want to look at it from the other side so I'll do a section view from this side I've cut away the other half of this and again let's follow that pin so I'll go back to dynamic simulations and so our tangent point is here to 12:00 o'clock position and it stays longer as long as this straight line but then when it starts to curve that tangent point changes along that cylinder now there's some bouncing around in here depends on how many calculations I do on this as well and I can't remember whether if I kept a little bit of clearance in here or not yeah so let's look at it again one more time without it in section view all right let's up look at this again so I'll go back to dynamic simulation I'll play it again so remember it looked like there was a big huge gap in between the pen in section view but it's actually because the where the tangent point is located at it's continuously variable it is in contact and these they're both same size so it's in contact with both of these and at the same time I am set this up to do a thousand calculations along that travel the higher I set the calculations the more precise it would be but the slower it would be having to do all those calculations if I just drag this and I get this vector this force vector so the longer that vector is the greater the forces that I'm putting on that pin and now if I go too fast the computer can't keep up with the calculations I gotta be careful that I don't go too fast that and it's it's it works better if I have the computer driving it then if I try to do it by hand or I just need to go really slow so that it doesn't overrun the calculations and we can display all kinds of information about that motion too if I want to know so here's the acceleration of that the prismatic or the the straight-line motion of that pin can look at driving forces velocities accelerations positions so forth all kinds of information that I can graph as we're playing at simulations and actually one of the things that we probably want to avoid particularly if this is a high-speed mechanism is any really sharp transition in the acceleration you want a smooth transition for a high speed application should I want to look at one more thing why we're here in Inventor and so I'm going to look at modeling this part in inventor versus how I just demonstrated modeling it in fusion 360 so I create my cylinder instead of a sheet metal part I don't need a sheet metal part to do this in Inventor I create a a work plane out here tangent to the part and then create a sketch and I said at that sketch I create this sketch on this work plane and I want to see why it's showing that it actually isn't fully constrained I want to find out why it's not fully constrained okay so I have a point in here that that point still has a rotation I was doing something earlier all there ative this line right here that line can still rotate and so these arrows when I just turned that on show me where that rotation was at and I'll put a constraint on that line and now it's fully defined it tells me down here it's fully constrained the degree of freedom arrows turned off and then I wrapped that around this curve and actually so this was my pin that I used to cut this with here's my 2d sketch and then I wanted to wrap that around the cylinder so in the 3d sketch I select a jet to a surface i selected a face i want to project to I want to wrap that to that surface and I select the curves that I want to wrap to it and so whatever my displacement diagram is I can wrap it around the cylinder instead of doing a sheetmetal fold unfold like we did in fusion 360 and then once I've done once I have a path I can tell this cutter to go along that path and cut my part I'll do that now I tell it to take that cutter and take it along that path and cut out my part so here's my fusion 360 Part D more complex part and I'm gonna send my timeline back to the beginning I'll go forward one step I created a work plane half the distance of the cylinder from the origin plane and then on that plane I put a canvas or a scanned image of the displacement diagram so this was a image taking from actual part and I'm going to edit this image and so I'll right click and say calibrate and then I need to select two points on this so this is a hole in the part and then this is the same hole after having gone all the way around the part there are other locations where you could find the same sort of thing so this point right here is the same as that point right there so I'm going to click in the center of this circle and I'll click in the center of this circle and right now tells me that image is 13.7 6-3 405 but I know the actual distance is the diameter 41 that's the diameter of the cylinder times pi will give me the circumference of the cylinder and so uh press Enter on that and that's rescales my image so now my image is one-to-one scale I might want to make some other changes on this so I'm going to edit canvas and I'm going to make that darker so that we can see that better I may want to move this so that the origin is in a particular location I might have made that too dark where I can't see the origin if I want to move this I can drag this and move that say maybe I want the origin right there or wherever so I put the origin in some particular location and then I may need to rotate this one way or another and I can also tell it that I need to flip horizontal or flip vertical if I need to say we have it mirrored backwards or some anyways once I get that done I then just create a new sketch and I lay out the distances for my displacement so I create a displacement diagram and I guess I can start to do part of that I've already done this and so I have it all laid out so I'm only going to do a portion of it but I have a line you know a straight line from here to here and then it's gonna go in a curve and so forth you get dimension these lines and to get our displacement diagram don't take the image too seriously so hopefully you have a physical part that you can go back and forth with your measurements between the physical part and the image because you're it's hard to tell from an image you're gonna always have parallax error some errors that make it difficulty to use the image anyways I went through that process and created a displacement diagram I'm gonna turn that off for now so I'll turn off the canvas and I'll turn off work plane and I'll turn off the visibility that sketch or I might just delete that last sketch all right so the next step I do then is I create the sketch for my sheet metal part like I did on the original that I have to do this in a particular way a sheet metal part has to have a great section to that sheet metal part and so I've got a straight section going from here over to here and then I have the curve that I'm going to lay out my slots on or at least a couple of the slots so then I create the sheet metal part and so let's go up here to our solid bodies and so here is our sheet metal part and the thickness of my sheet metal I have set to the depth of my slot so if I go to sheet metal and I set this to the rules I see I have it four point five millimeters so my slavi I'm gonna put is four point five millimeters if I edit this I have the k-factor set to one so that's important stuff all right then I unfold that portion of the cylinder where the slot is going to be I then create a sketch for my displacement of my first slot and remember one side of this will be the centerline so I'm gonna go half the distance and let's just look at the dimensions on that from Minnesota to show dimension so the thickness on this 3.03 so my total slot width is going to be six point zero six and any of these dimensions now can be changed so once we create a parametric model we can lengthen the slot could change your radius of the arc we can edit this slot however we need to edit it then I do an extrude cut just like I did on the first problems and then refold it and delete everything except for the surface that is my centerline surface and then I create a new sketch for the next path so again I use that same technique of part of a straight line and the curve that will encompass that path I go a little bit beyond that so I have some extra material and then I do my sheet metal flange again I unfold that and actually I split this face up here at from this point on the original cam so that I have the same reference point on the cam I projected this point up split that face and then when I unfold it I have a reference point here that I can use that reference is the same point on my first flat pattern and then do the sketch and then do the extrude cut then to the next step I did this one down here so these two profiles start and end in the same place so I have those two sketches connected together with construction lines and I guess I could have done both of these in the same sketch and then just one extrusion one extrude cut but for editing purposes it may make it easier to not have too many dimensions on the screen at once and so I did it as two separate sketches and two separate extrusions I then refold my model and this is the second sheet metal body now I'll delete everything except for the the centerline of the first side let's back that up so I have two slots in this now so I need the the centerline of one of these this is the centerline of the first slot that we did and then I need to centerline for this slot the centerline for that slot and so I get the second one actually I think I already had the third one they just don't have a visible yeah there's that there's a third one up there yeah so when I back here when I did that delete I deleted all the faces except for the centerline for this one in the center line for that one then I sketch my circle for my cylinder that I'm gonna cut these out of and I copied these surfaces we'll see why in a few minutes that I had a copy of each one of these surfaces offset distance zero okay so I offset each one of these SERPs is a different distance zero to give me a copy of those surfaces and originally I didn't think I had to do this I don't recall why I ended up doing that well I know why I did it but I thought I don't think I should have had to and I don't think I had it in there originally and then I extrude cut one of those surfaces you know this surface and I extrude cut I mean not extrude cut I do thicken that's the key you do thicken midplane the thickness of your slot picking me playing the thickness of your slot the machining purposes you're going to want this curve right here to define the path of your cutting tool and so that's why I put these these copied offset surfaces at distance 0 in here so that those could be used later when generating a CNC code in a camp right then in the next step I put the top and bottom of the hub and I could have put those in originally before as part of that original extrusion here and and put a fill it in here did a work plane here someplace and we'll look at that work plane notice all of my sketches are fully defined so I created a circle the cylinder is rotating at is is being cut when it gets to that last spot it actually leaves a little bit of a flat there half of this will end up being a planar surface so I do it extrude cut so that the planar face right there because the rotation stopped in the same way at each end of disc did the same thing at each end of the slot and so I have that one and have wherever the next one is here and this one and this one again there's a planar face right there planar face right there right there it's not cylindrical like this face because the cutter stopped there or they had the drum stopped rotating as the cutter was cutting the slot and then continue cutting away from my piece of stock put my hole in here it's read it hole put some champers on here there's a large camp for small chamfer sand fill 'it's a chamfer on the threaded hole the hole cutting through the side here and the hole cutting through this side right here so that is cutting cam slots or cylindrical slots in fusion 360 using a trick with the sheet metal tools I'll take a look at briefly how I did part of this in Inventor and so I'm going to go up to my first sketch and so if I turn on the visibility of the sketch so here is the centreline path of my three slots I'm going to turn on the visibility of the original image so here it was the image used to lay off those paths and turn that off again and then do a wrap of the 2d sketch around the park to get the paths as they they go around the cylinder and then you can go and continue to finish rest of the camp I've turned off the visibility of my 3d sketch one final thought on the design of cams so normally when we're laying out a cylindrical cam like this we specify the slot in terms of the angle going around the camp and so for this distance I had it calculated as 41 millimeters that's the diameter of the camp times pi that gives me the circumference times the angle I want out of a total of 360 degrees going around the cam neck converts that angle into a linear dimension that we can then wrap around the cylinder and then if we're using a cam generation tool like the Autodesk Inventor cam generator we we set our angles that we want and what we want to what motion we want to occur in between the angles we can put in the radius of the cam the depth of the slot that we want you know all of the information that we will use to generate the cam itself and just specify the lift over certain displacement and Pratap's all we want to do is look at just the the graph of of just the the lift we might also want the acceleration curve and we want to probably avoid sharp changes in acceleration like that and we can specify the motion laws where it changes from say a linear motion to a harmonic motion in between the various segments of the cam

Channel: The CADWhisperer

Views: 5,838

Keywords: Cylindrical Cam, Fusion 360, Autodesk Inventor Professional, Sweep Solid, JD Mather, The CADWhisperer

Id: Wekmai5MqFM

Length: 27min 59sec (1679 seconds)

Published: Sat May 09 2020