Modeling a Complex Part in Fusion 360 | Langmuir Crossfire Plasma Torch Anchor

today we're doing a deep dive into fusion 360 and we're going to model this complex part now there are a few techniques in use here that you may not have seen before so stick around and maybe you'll learn something new [Music] welcome back to cloud 42 i'm james if you saw last week's video then you know i made this which is a bracket to mount the torch lead down to the top of the motor here on my cnc plasma table the idea is that it will screw down to the top of the motor here and then provide a place to anchor the torch lead and the other cables that are flopping around so that they come up into a nice neat bundle and we can get some decent wire management on this now this is a pretty complicated part it's designed to fit the motor which is relatively straightforward but then it's got a bunch of compound curves it's got this curved rounded channel to fit the cord it's got curved slots through it for zip ties it's got more curves on the back it's opened up and skeletonized and has fillets around all the edges and a part like this is relatively complicated by the time you get it done but the tools used to model it are pretty straightforward so today we're going to go into fusion 360 and we're going to do a deep dive on modeling this part and we're going to walk through all the tools that are used to actually create this geometry now in order to get the part to fit the motor we need dimensions off of the motor and some of them are really easy just grab a caliper get the outside dimensions get the dimensions of these protrusions on the sides other parts of it like measuring the curves measuring the the radii of the fillets on this thing require a different tool this is a set of radius gauges and so on one end it's got leaves with outside radius radii on them and on the other side it's got leaves that have inside radii on the tip so this one is two and a half millimeters and so i can just sort of go through all the leaves and figure out which one fits and i can see that the two and a half millimeter fits nice and cleanly without a gap on the outside here and for the inside curve the five millimeter outside radius gauge fits nice and neat in there with no gaps so i know the radius of that is five millimeters the radius of these outside fillets is two and a half and so then all i need is the spacing for the screw holes and a really easy way to determine the spacing of screw holes is to take your caliper measure the inside diameter of one of the screw holes then zero it out then use the inside jaws to measure across two of the screw holes and that will give you a direct reading in this case 51.08 millimeters everything on this motor is metric these are m3 screws screw holes screw threads in there so i'm pretty sure this is all metric so this is a nominal 51 millimeters across between those two i will go ahead and measure the rest of the dimensions on this motor and then we'll go into the computer and walk through the design of this part this is fusion 360 and this is the model that we need to design this one's already done in fact you know i already printed it out you've seen it but i want to walk through how to model this let's take a quick tour of the features of the part the bottom is very simple this is just a base plate that fits on the top of the motor with four screw holes to allow it to be attached and then the main purpose for this part existing is this curved channel to hold the plasma lead so that the plasma torch will be down here the lead will be coming in from this side it'll follow this nice curved transition to vertical and there are some channels in here to tie down the plasma leads so that it doesn't move around so the channel itself is a compound curve you can see it's shaped to the shape of the cable to hold it securely and it also makes this curve so this surface is curving in two directions and then these channels underneath are for zip ties to anchor the cable down so i've come up here to inspect section analysis and i'll just choose a flat surface in here so we can cut the model and you can see that that zip tie channel is also curved and follows the the curve on that top surface so there's one in the middle there's one up here at the top and there's one down here at the bottom and you can see the geometry gets kind of complex but it's actually not that hard to create we'll walk through that here in the next few minutes and then the back support is a little bit wider just to clear the plastic block that's on the back of the motor there's a channel on each side to hold the other two cables that need to come up and similar curved zip tie channels to anchor them down and then i've just got a hole in the back here and a hole through the part both for aesthetics and to make the part a little bit lighter and use a little bit less material let me create a new design and let's jump in and i'll show you how i modeled this the first thing we need to design here is the base plate so i will start with a sketch put that on the x y plane and bring that up so we can look at it now i know that this is symmetric in two directions so i'm going to start with some construction lines that i can use for mirroring so hit l for line x for construction and i will just drag out and place a couple of construction lines now hit x again to turn off construction and now let's just sketch out the basic shape of the motor so this is one quarter of the motor and we need to put some curves on there so i'll choose the fillet tool i know these two are the same and these are 2.5 millimeters and i know this curve on the inside because i measured it is 5 millimeters in radius so now we have the general shape or at least the components of the shape of one quarter of the motor with the radii on there and the last thing we need is a hole for the screw so hit c for circle and i will just drag that out i know the dimension of this i'll hit d put a dimension on here of 3.4 millimeters and that's to create a clearance hole for an m3 screw so that is the shape of one quarter of the motor of course the dimensions are not right yet we need to mirror this first so i will just select these parts now there's two ways to rubber band select if you select down and to the right then your rubber band box will cover parts and will select only parts that are completely inside the box so if i let go here you'll see that these line segments that were not completely inside the box did not get selected escape instead if i rubber band from the and up and to the left then everything that the box touches will be selected so those lines get selected when i go in that direction and that's what i want so then i will click mirror select this vertical line as my mirror line and now i've gone from a quarter of the motor to half of the motor i'll do the same thing i'll go across here select all of this now that's selected my mirror line i don't want that so i'll hit control and click that to deselect it and i'll do the same thing mirror about the horizontal mirror line and now i have all four sides of the motor but of course the dimensions are all wrong so let's put on some dimensions d for dimension i know between the screw hole center to center in this direction is 31.5 millimeters and in this direction is 51 millimeters and then i know the outside dimension of the sides of these is 38 and the overall outside of the motor is 56 and then i'll just put those same dimensions on the other direction clicked across there and i'll just click this dimension to link the value and do the same thing in the other direction on the large dimension here click here to link the value enter and finish and now we have the shape of the base plate that will fit the motor so i'll just click here hit extrude i want this to be five millimeters enter and we have the base plate the next thing i need to design is the upright rib that holds the torch lead and i've gone ahead and set up some parameters that we're going to use for this so that if it doesn't quite fit i can just tweak the design so i've got the torch lead diameter in here which is 13 millimeters i've got the cable diameter for the cables that come up the back that's five and a half millimeters and i've got the bend radius i want to use for the torch lead and that's 75 millimeters and i kind of just estimated this by playing with the cable to see how it bends but the point of having these as parameters is so i can come back later and modify them so i want to start with a sketch with a line that follows the center line of the torch lead cable so i'm going to click here to create a sketch and i'm going to put it on the yz plane now i i need this sketch to be able to take dimensions off of and intersect with parts of the base plate so i'm going to hit p for project and i'm going to select some of these lines and click ok and that puts these points into my sketch where those intersections occur and this will make life a little bit easier for me let me hit l for line and let's just sketch some lines in here i know i'm going to have a vertical face that comes up to the curve of the cable there i know i'm going to have one that comes up the back to there and then i'm also going to have a line that comes up like this so that i can uh have i can sketch this rib that comes up the back so i've got some lines in there and then i want to put an arc across here arc three-point arc and this will be the arc that follows the center line of the cable now let's go ahead and start putting some dimensions on this thing now before we can do this i would like this top surface on the back here to be perpendicular to this curve but you can't you can't make something perpendicular to a curved surface in fusion 360. so what i'll do instead is hit l for line and we'll just extend this line out now if i just move this back and forth you'll see the tangent constraint appearing now if i click this constraint is now here to hold that line tangent to the end of that curve the other way you can do this i'll put one at the other end is just draw your line at whatever angle you want and then come back later and select the curve and that line and select tangent and so now we have line extensions on the end that are tangent to the curve now let's start putting some dimensions on this now this is the center line of the cable and i want the outside edge of the cable to just come and touch the edge of this base plate so i hit d for dimension we'll go from this line to here and so i want this to be the torch lead diameter divided by two and i want exactly the same thing up here from here to here and i also want this to be perpendicular so i select those two and select the perpendicular constraint great now the width of this back rib is going to be the cable diameter and i want to go ahead and put this angle at 45 degrees and then the only other thing i think that's unconstrained here oh we've got to put the radius here this is the torch lead bend radius and then the last thing we have is this height and i am just going to pick a value d for dimension of 45 millimeters and now we have this sketch completely constrained now in order to actually extrude these sections have to be closed so i'll just go ahead and put some lines across here and now we have closed areas that we can extrude so now i can just click here get e for extrude i want to extrude symmetrically over a distance of the whole length and that distance i want to be the the torch lead diameter minus one millimeter i want this to be slightly narrower than the torch lead so that the zip ties will come around and grip well turn the sketch back on and let's go ahead and extrude this back area the same way and this will also be symmetric distance and i want this to be based on the measurements i took probably 22 maybe 23 millimeters okay so that gives us the rough shape now let's cut the trough for the torch lead so we'll create a sketch on this top surface right click create sketch hit c for circle and let's just draw a circle d for dimension this will be the torch lead diameter and now we have a circle that represents that and i can just click this area and come up here and say create sweep and for the sweep path select this curve and i want to make sure we go all the way through the bottom so i'll go ahead and select the extensions on both sides it automatically defaults to cut click ok and now we have our curved surface for the torch cable now it's a fairly complicated surface because it is curving in two directions but all i did instead of trying to do this artistically or pushing and pulling or trying to make it the shape that i wanted i did it functionally i just defined where i wanted the cable to go with a sketch and then define geometry off of that path so that it will conform to the outside of the cable didn't actually model the cable i could have done that and then used it as a tool to cut but i find it just as easy to visualize it and make the cut with the sweep tool off of a sketch now we need some zip tie slots to hold the cable in place and that's actually a lot easier than it looks if you know a couple of little tricks so let me turn the sketch that has the center line of our cable back on and i'm going to create a construction plane so i'm going to say construct plane along path and i will select this curve as our path now where exactly do we want it i want it in the center so the distance here it distance type is proportional and the distance i will set to 0.5 and that will place that plane directly in the center so now i will right click on this and create a sketch and i'm going to come up here to my sketch tools under project and include i'm going to select intersect and i'm going to click this inside surface and click ok so now in our sketch you can see we have this purple line that follows the surface there now i'm going to hide the the body here for a minute just to make this easier to see and we're going to create a couple of offsets from this so o for offset i want my zip tie slot down in the surface i'm going to put it in a half one and a half millimeter so minus 1.5 and then i'm going to hit select this and hit o for offset again and i'm going to bring this in minus four millimeters so now we've got lines that are going to be down under the surface one and a half millimeters below the surface and four millimeters below the surface giving us a two and a half millimeter distance between them and hit l for line and i'm just going to enclose this and click finish sketch now let me bring back the body here as you can see we have this sketch with this area that is through the center of the through the center of our part to actually cut out the slot i'm just going to do an extrusion so i'll select this again hit e for extrude and we'll do the same thing we're going to do this symmetric extent type distance the whole length and i want this to be six millimeters because i know that's how much room i need for my zip tie okay and now we have our curved path cut through the part for the zip tie now that's one right in the center i also want them out on the edges as well so i'm going to go up here and say create pattern pattern on path and i'm going to select i want to pattern a feature and i'll come down here into my timeline and select that extrude and then the path is going to be this path and i want to do symmetric and i will set the extent now if i pull this out you can see that it's going to try to create two more of these now you can see the angle isn't following this so orientation is set to identical i want to change that to path direction and now those those duplicates of that feature will curve along the path so i'll just pull this down to about where i think it makes sense work it looks right on the top and bottom click okay and now i have my zip tie channels cut through the part now i'm looking at this and i think having those as thick as they are is just a little bit too thick so i can go back to my sketch here and i can change this from four millimeters to minus 3.5 and that looks a little bit more reasonable and along this path i will just pull these back a little bit so they don't intersect the other geometry turn off the sketch and there we have three zip tie slots in that channel and these will be there to hold the to hold the torch lead down and we can always go in here and say inspect section analysis and select one of these and kind of get an idea of exactly how those are fitting in there and those look great now to finish this up we need to put some curved channels in the sides of the back here that's pretty easy we'll just create a sketch on the bottom here and we will project this geometry down so we have a place to put it l for line i'm going to create a construction line so x that will be the center line across the bottom here and that will give me a way to position my circles to cut the channels on the side so c for circle and i don't want this to be a construction circle so i'll just put this in here let me put another construction line on the center here just so that we have a mirror and mirror that circle around that now i want this point and this line to be coincident so that that'll hold that on the center line and then i need to put some dimensions so i know this is the cable diameter because i'm making a channel for the cable and then i want the distance between these to be 21 millimeters because i know that's there's a plastic block on the motor that's going to interfere so i want those cables to be more or less touching the sides of it so i will right click and say pick circle arc tangent and i will dimension between those 21 millimeters and that gives me my positions for that and so now i can just select these pity for extrude and extrude those all the way up and now we have the channels for our cables now to put in the zip tie uh channels in this it's just as easy we can actually go back to this sketch here on the bottom and i can just offset this the same way 1.5 millimeters and 3.5 millimeters then we'll just select those regions and extrude and to for this extrusion we need to move it up the side here so for start we will select offset and we'll offset this maybe and i'll put in a number minus eight millimeters that looks reasonable and a distance of minus six okay and that now has given us channels for the zip ties and we'll just do the same thing and create another set of channels up near the top now we need to lighten this thing up a little bit so i'll right click here create sketch and i'm going to create an offset from this edge i have and i don't want to do chain selection so turn that off so we're only going to offset just this one line pull that down and i'm just going to do this by eye pick a value there that looks okay and then i'm going to put in some lines here to close that off and then i'm going to come in here with a fillet and put a fillet on this corner of i don't know was it three millimeters look good yeah that looks reasonable and put one there great and i'm going to put another [Music] fill it in this corner yeah that looks fine now right click extrude and we'll just push that all the way through and that looks pretty reasonable there and i'll go ahead and sketch up a rectangle here on the back create sketch and let's do a center point rectangle and i'll just come out here and touch these edges so that we get a guide and i'll just pick something that sort of looks reasonable right click extrude and push this in some amount that looks reasonable and that is all the geometry pretty much complete now the only difference between this part and this part is that i've gone back over it and added a whole bunch of fillets so there are multiple reasons why you'd want the fillets on here one is is just for aesthetics but another is for functionality i don't want a sharp edge along here so i will fill up that edge 0.5 millimeters and i don't want the cable when it comes out the front here to go across a sharp edge on the plastic so i'll fill at that maybe a millimeter maybe two yeah maybe a millimeter same thing here on the top where it exits and then the other reason to put in phillips is to avoid stress risers a section like this along the bottom here where we've got this you know nice tall part that's going to have some torque on it and we've got a nice sharp edge here that's a place where stress can cause a crack to occur over time same thing down here and so when we come in and put fillets in places like this those fillets then actually are smoothing that part out so that stress can't build up or concentrate in that corner now depending on exactly where these things are located and how close they are and what order you do the fillets in it can be complicated to get exactly the geometry you want so sometimes you have to mess around with the order should i fill at the end here first or should i fill up the side first or should i move this this zip tie hole a little bit so that i don't end up with a weird intersection and honestly that just requires some fiddling but once you do that you end up with a part that looks like this and we can just 3d print this and take it out and install it on the machine i'm printing this part in a carbon x carbon fiber reinforced petg just because i wanted the increased strength and stiffness in this application probably normal petg or even pla might work in this application but i think the carbon fiber reinforced filament is probably going to be a little bit more durable and last longer i originally designed this part as a part of a set of experiments for using some dissolvable support material on the printer but i needed this done and i was running into a little bit of trouble getting the support material to print right so i just decided to try without and turns out it printed okay there are a few areas on the part where there's a little bit of sagging in the overhangs again because i didn't really design the part to be printed without support but all in all i think it's going to be totally acceptable you can see the characteristic rough surface finish of the carbon fiber reinforced filament but all in all the print went okay and i ended up with a usable part interestingly now that the print's done you can see the ooze coming out of the nozzle back there as it's just sitting cooling down this turns out to be the biggest challenge on a printer like this in printing with dissolvable support but more on that in a future video well in the end i'm really happy with how this part turned out i really thought i was going to need dissolvable support material to be able to 3d print this because the overhangs under here and particularly the really shallow overhangs that are occurring when printing this bottom zip tie slot and in the end it just did not end up being necessary at all this printed just fine freestanding on the printer there's a little bit of hanging filament underneath this back edge if i knew i wasn't going to need this support material i probably would have just put a 45 degree angle on that same as we did here on the bottom but all in all i think this is a totally usable part and i'm expecting it to to wear and last a long time in this application probably never need to replace it well did you enjoy that video did you learn something new i i know i always learn new things when i watch people work in a piece of software and i love that because i pick up new things that i didn't know how to do before or quicker and more efficient ways to do things that i was doing in the hard way and without knowing it do you know of better ways to do some of the things that i did in this video if so jump down in the comments and let me know i love reading the comments on videos like this because i always learn something new well if you enjoyed the video please give it a thumbs up feel free to subscribe to the channel and like i said leave me some comments i'd like to know what you think thank you for watching [Music] you

Channel: Clough42

Views: 31,864

Keywords: Fusion 360, 3D Printing, CarbonX, Langmuir Crossfire, Plasma Torch Strain Relief, 3D Modeling

Id: _BZ7toLabQ0

Length: 28min 54sec (1734 seconds)

Published: Sat Dec 04 2021