E4 Autodesk Inventor 2021 - Basic Modeling 4

welcome back i'm chris secora and i'm going to step you through exercise 4 and inventor 2021. this exercise deals with what you see up on the screen there some of its review as far as making these revolve features that we see here for this hand wheel but what we're going to learn that's interesting here is the sweep tool now the sweep tool is the very first of the tools we're going to learn for free form design freeform design basically enables you to create pretty much all the other non-prismatic shapes that are out there like for example prismatic shape is just a box or a sphere or radius whereas free-form shapes are more organic in nature like if you wanted to design uh something that looked like a leaf or something or a car body or an airplane that's where we're starting to get into with sweeps and this is a very basic sweep but they're very useful so let's go ahead and we'll get started first of all go to new standard ipt and hit create go ahead and click on start 2d sketch select the xy plane now if you're wondering where we're going to get this information from as usual we're going to the vertani1 webpage verta n u x one dot com and from in here just go to the instructional manuals you'll see the autodesk inventor in the green there go ahead and click on that it'll bring up the the manual and here you could actually get to page 37 at the beginning you can see the dimensions that are right here we might do it a little bit different than what you see here but we'll still use the dimensions okay so let's start off with the rectangle and notice the rectangle i picked is just a two point so click on this origin when you get the green dot drag it up and make that one inch for the width hit the tab key and go ahead and type in three for the next one and now you could click on front here and it should give you what we're looking at here okay now what we're going to do is hit escape and i want to show you a new tool tool we haven't yet used we've used chamfers and fillets but we haven't used a sketch chamfer yet and so chamfer is found right over here sometimes you'll see fillet or chamfer hit the little arrow to the right of fill it if you don't see it and chamfer should be below it click on that now here you have the ability to set a distance distance angle the distance and so on and so forth we actually want this to be 0.25 we're going to leave it at distance to distance because this is a 90 degree angle it's going to come out 45 degrees so go ahead and select that vertex there and it should automatically put in the chamfer and you can see the dimensions and the fx means that they're tied together so if one changes the other one will update as well and it's not a bad idea to pull out some of these dimensions just from the standpoint of making it look organized and easier to read now we're going to go ahead and we're going to put like a little radius here a circle so go to the circle tool and locate yourself right about here notice i'm inferring to the 0.25 top edge of the chamfer and right in the middle that your y should be about 1.7 ish click drag it out and make it one inch and now let's go to dimension and dimension the center position of that to the bottom edge drag your dimension to the left to make it 1.75 now to locate it we could actually use a constraint here if you click on vertical constraints select the center point of the circle to the top vertex of the chamfer and that aligns it and should constrain it now you can see below here it says it's fully constrained now we haven't really talked about fully constrained too much in this uh previous exercises fully constrained means that you've added all the dimensions and all the relations necessary to where there's no more needed and essentially that is what you typically want before you go into production with something but initially though when you're just working on conceptual work it's all right to basically not put all the dimensions in but later on you might want to add those and relations and constraints so i'm going to go ahead and hit escape here i'm going to drag this dimension out a little bit now inventor doesn't make you trim this information out and we've learned the trim tool last week so we're going to leave it we're going to leave it as is now we're going to go to 3d model and we're going to go to revolve now let's click on the home button up here so we can see what's going on first of all remember here the blue line that's looking for selected profiles so click here here and here this negates us needing to select the trim and trim that stuff out now then click on select axis and you can use this right edge of the model as the axis and hit okay now in the book you'll see that i dimensioned with diameters and such and that's because i used a center line up as i'm seeing now not as many people are using the center line because it's just more efficient maybe to do it this way and but note that the center line as i showed you an exercise two is very crucial and your employer may or may not want you to use that's those center lines when you're revolving around just for the point of having construction geometry and understanding what's going on okay now we're going to go ahead and let's select a little okay and so from here we're going to go ahead and hit the little plus symbol next to the origins folder and find your x y plane click on it and then you could go right here to create sketch okay i'm just going to center a little bit with my wheel rolling in and out for zoom and what we're going to use next if you hit the little arrow underneath the line you'll find splines there's control vertex interpolation equation curve and bridge curve now the difference between control vertex and interpolation is basically interpolation is a much stronger control than the it's just easier to use especially those who are very artist it gives you these control handles that are easy to manipulate however for new users i find that the interplay to spline is actually easier to master initially for first day so we're not going to look at the control vertex but but note that that is probably what most professionals use for free form design but let's go ahead and use this spline interpolation move your pointer to the center and you'll see you can infer to the center but not really the center of the the hub in the middle so right about there just click now drag this out and maybe uh infer to this edge and you'll see the center point up here click on that then click on this point and now i'll start dragging it up and i'm just clicking and adding points and these control points are going to make my curve look interesting eventually when you get maybe about a half dozen six different control points that i've added and it looks similar to mine go ahead and hit ok now if you don't like what you see all you do is you grab these points and you could smooth out the curve or make it more dramatic however you want but you don't want it overly dramatic so just be aware that that can lead to some geometry that's difficult to sweep along you don't want it to tie itself in a knot per se and then have the solid do the same it will fail to actually merge in many cases so once you have that the way you like it notice i didn't use any dimensions just kind of visually just have a little fun with it get it how you like it and go ahead and now we're going to go to finish sketch and what we're going to do we're going to create a plane and this is my favorite plane tool because with this plane tool you could create a plane virtually at any any angle going anywhere and it's really it's just based off of a perpendicular plane to a curve so what you could do you could head over here on this uh plane tool up here and you'll see normal to curve at point that's the tool you don't necessarily need to select this in advance you could actually control select the end point where you want the plane and then the curve that it's attached to and then go to just the plane at the top and i'll create it but let's go normal to curve click on that point and then click on the curve and there's our plane so we just created a work plane and again that's my favorite because imagine you could draw lines anywhere and then say i want that a plane perpendicular to that endpoint so all right now that we have that let's go ahead and select it select the edge of it and go to create sketch now yours might rotate a little bit different than mine that's okay go to the circle tool and get to the center of that and when you get the little yellow dot click and drag out and we're just gonna make this point five now because i'm letting you have carte blanche on how that curve is looking if you have a very tight curve it may fail to sweep a half inch diameter circle so if you have that issue because i'm not there to actually see what you're doing my recommendation might be to either smooth out the original curve or just make this circle smaller so that you could get past it and maybe make it .25 or 0.125 if that fails and usually one of those will work just from my experience teaching this as long as i have just seen a lot of students have a little bit of a challenge there because we didn't use a dimension okay let's go to finish sketch we didn't really need to hit finish sketch but anyway let's i'd like to hide this work plane so if you remember from last exercise e3 if you right click on the edge at the four o'clock wheel there turn off visibility and then that hides it okay now we're ready let's go to sweep and it automatically had my profile selected for me apparently because that was the last thing i drew if yours doesn't have anything in here and if it's red click in there to get the blue bar and select that circle but now i didn't have to do that so i'm going to go click over here and you can see the blue bar is underneath actually i clicked on it a second time and turned it off so be careful it's like a light switch so make sure you have that blue bar underneath there and i'll select the curve and you should be able to see the curve sweeping along into the model go ahead and hit okay and that's a sweep and look at how it has that free form shape all right now moving along we want to pattern this so go ahead and you could select the feature right here on the surface or you could find it on the model tree over here go to circular and we're going to set this uh the rotation axis i'm going to select this hub what's really kind of neat um i always like to point out a strength that cad softwares have whenever i make videos for the different ones and this is one that i really like is it allows you to select any cylindrical face even if it has a radius around that so it's a complex face that should do it not all cad systems can do that all right so now we're going to go ahead and put in let's put in three instances 360 degrees hit ok and so we've just created our circular pattern and we learned circular patterns with the rib tool in exercise two so that's not really anything new that we've done there okay let's now move along to the x y plane and go over here and start a sketch now i'm going to click on front to center it go to the circle tool and find the midpoint of this edge over here on the left click and drag out a circle make it one inch type it in and now go to the spline tool hit the little arrow underneath spline and go back to line we're going to draw on at the origin here click and drag out a vertical line hit escape and that's so we have an axis of revolution now let's rotate this around let's go to 3d model and revolve so it automatically selected our profile again which is nice and it's just looking for the access so go ahead and select the center and hit ok all right now there are other ways to get an access center where you don't have to draw it you could show a sketch from an earlier sketch that was in there and use the edge and things like that but i just wanted to show you sometimes i just better create a fresh one okay let's go to the fillet tool and set the fillets to 0.25 and proceed to select all these edges here and you can use the x-ray vision oops yeah i didn't really want it on that edge but that's okay suppose i'll just get the other one underneath it too and we can select these edges and we we won't select the bottom edge because i have plans for that all right so we've got some fillets in there now let's go ahead and rotate it to the bottom side now i want to show you the whole tool we've seen how to cut holes just by drawing a circle going to extrude and remove the material the whole tool here is actually very very nice i was just using it today and with some of the updates since the last time i used it it's getting up there it's pretty strong so let's try it the whole tool now notice you have simple hole clearance hole tapped hole tapered so like for national type thread and you have counter boards so let's go ahead and let's put a tapped hole in so select tap and then select counter bore now notice here you have libraries ansi and isil libraries metric and english let's keep it at a quarter inch and actually look at this the designation quarter 20 unc if you hit the little arrow uns you want unef so you have all the standards and this is why i was just like really impressed with this recently they did have this functionality in it before but never has it been so easy to use it's really quite nice and your classifications as well as the termination like let's go with the distance and the distance right now mine's defaulting 0.75 i'd like that the thread will have it go a half inch and the rest of these parameters pretty much that's just due to the selecting quarter 20 i didn't really change anything now go ahead and select where you'd like to put it now here's the thing you can put them anywhere just by clicking on points and then putting dimensions and to locate it but let's say you want to specifically get it centered first of all set it off center a little bit like right here just click and you can see a nice preview there now go ahead and grab that center point and drag it to the edge and actually there it is it just uh highlighted the center let's get it on center there and we can get the green dot release it and if you want to you can make any changes you want here too go ahead and hit ok and as we go up look at that it actually has a cosmetic thread that's it you can actually see it cosmetic threads are used generally they're just an overlay a texture that appears to be like looking like a thread and the reason you want to use those typically for common ones like this is uh you know unc quarter 20 is because to have real or true threads cut in there uses a tremendous amount of system resources and usually you have you can have hundreds if not thousands tens of thousands of little screws and holes and you don't want to have those as real geometry because each one of those is broken up into a collection of polygons each polygon takes up bytes of memory and so it really drags the system down so that's why cosmetic threads are desirable there is the regular thread tool so if you're making something that's a unique thread for example like for a bottle or something that's where you want to put in a real thread so you could get it in there and then mold it or whatever you need to do so anyhow that's that's it for that okay so that's exercise four now i usually do like you to enhance it you don't have to really enhance it much more i'm just going to go over here and select i just like to go with my chrome sometimes and maybe add a little surface that stands out a little bit differently than the rest of it so i'll go with dark green and then we could use this we could go to view turn on perspective and again i like to use like two lights or one light really gives it a nice shine and once you have that you could actually go over here to visual style go to realistic it even looks better and to make it really look polished click on ray tracing and again the longer you let it go and if you set it to draft or hide takes a long time i have actually 16 cores actually 32 threads running right now and it still takes a little bit of time there so now that we have that rendering we're just alt print screen and if you remember we've been keeping track those of you in my class imt110 i want you to go make sure you're using either microsoft office or this one here i'm going to go ahead and start that apparently i closed it without finishing it and you can see this is what your portfolio should start looking like i actually ended up updating a little bit and just going with the green and silver look just because i really kind of liked it but you could do whatever you want i really encourage trying different things now i'm going to ctrl v to paste that and now i'm going to go over here to the crop drag that in drag that one in i can drag that over so we have one of them done now the lab there's only one lab today for this week and the reason why is because it's a tough one and i suggest trying it on your own but feel free to watch my video here i'm going to start it up in just a second but okay let's turn off ray tracing so here we go let's take a look at what it looks like and i haven't modeled this at inventor in years so forgive me i'm gonna probably choke on it every so often trying to get it done but uh here i'm gonna go ahead and rotate this it's actually on page 46. i'm gonna rotate counterclockwise remember how to do that you have to download this first and then you can click on it to open it it opens up in the browser and all the different browsers have rotate differently like here some browsers you could right click and rotate if you want and that's just so you're not having to turn your head this is a hard enough print to read let alone at an angle okay so we could see this uses the same modeling theory that we saw with exercise 3 last week so in this case it's a radius 0.75 at the bottom that's tangent on those edges and then it we have 23 degree angles off there and then 115 degree angle off of that and then we have a dome over the top of 1.5 and the distance between centers is 1.25 and distance between that corner and the bottom center is one inch so i'm going to drag this over and we'll build that right now so i'm going to go new standard standardipt create this is lab4 so i'm going to go now to start 2d sketch i'm going to go ahead and do it on the xz plane which is the top plane and i'm going to proceed with the line so i can mirror across and we'll get it to scale so i'm going to zoom out a little bit and let's see maybe about an inch and a half in height that's pretty good hit escape now i'll go to the line tool again down here about y point five and x minus point three ish click drag out a line about an inch long click drag out another one another about a half inch and look it's about 115 degrees remember that's almost exactly what the print says it actually is so click hit escape now go to mirror and it's looking to select these two pieces of geometry so i'm just going to window over now i'm going to go to mirror line and select that line we drew hit apply and done all right let's go now to the arc tools go to tangent arc and down below here click and drag this around and make sure you get the green dot to lock it in the next one is not tangent so we're going to go with a three point click here straight across get the green point drag it up and remember this is supposed to be 1.5 so we could actually just plug that number in right now if we want to all right i'm going to hit escape let's go to dimension now let's dimension from here to here and this is going to be 115 and then from here to here that's going to be 23 and then this bottom arc is .75 okay now mine's updating pretty well if yours doesn't update you might have drawn something over scale considerably or under scale and so it kind of locks up a little bit it doesn't lock up you just have to maybe try putting a different dimension or just grab a point and drag it and maybe get it more looking like what it's supposed to be anyhow let's move these out of the way here and i have that 1.5 let me get that escape here ah it's making it tough for me to grab that little point not sure why that's okay though we could grab it later all right now i need to add some of those other dimensions so i'm gonna go back to dimension this bottom center point to the top center point right up here actually let's make sure we get the proper center point i think you have two of them there actually oh boy it's hard because i this is why it's not a bad idea to use actually a center line in fact i'm gonna do i'm gonna hit escape i'm gonna click on this line and then change to a center line and then click off of it all right so now i could see that that's the point there and oh look at that i locked into it i didn't realize that okay let's see if we're going to have trouble with that maybe click here to here and this is supposed to be 1.25 all right it's not looking too good just yet but let's see if we can click on this vertex to this center point and that distance is going to be one okay it worked all right so i was getting a little nervous there like i said i haven't done this one in a couple years on this system but looks like we got it all right now we're going to proceed to extrude it and according to the print the extrusion thickness it's right here it's a half inch so let's oh and also there's 25 degrees of draft so go to 3d model extrude boss and we're going to go ahead and put in the distance 0.5 and the taper is to be 25 degrees okay now what i've forgot to flip i should put minus 25 degrees so easy fix i just go over here right click and there's edit feature and from here i could actually hit this reverse switch and there we go and put a little minus symbol in front of it so it's a negative now let's go ahead and go to the fillet tool and the fillet for this is called that on printed half inch select this edge hit okay now there is a chamfer that goes along this edge and we're looking at the print that's 30 degrees off of the 25 that's already based there and so i'm also looking at this let's bring this up the location is 0.181 off the bottom edge so 0.181 by 30. so let's go over here to chamfer and we're going to go distance to angle so 0.181 and 30. now select that top face and this edge and actually i believe it's supposed to reverse that let me uh let's do it again i think this face here and then this edge there we go all right now we could go ahead and hit okay so from there we now have our part ready to shell we don't really have to put those other features in just yet so let's flip it around and go to shell and let's look at the print again and the prints the typical wall thickness is 60 000 so 0.06 select this back face to open it up and hit okay all right looking good there now we're gonna we'll put in those uh cut outs select this face start a sketch and let's go counterclockwise get that line there all right from here i'm going to go to the line tool and i am going to use the center line just so i don't have that same issue where i can't tell the difference of what i'm looking at so i'm going to draw that hit escape then turn off the centerline tool that's the reason why i'm kind of avoiding it because this stopper you have to turn off but you don't really have to use it to begin with if you're an advanced user you're going to be fine okay so the next thing we need to do and see here [Music] i do believe actually i might have i guess we're okay i think i i should have centered this i didn't center it but let's uh we should be able to go back to that a little bit all right so now i'm going to take the line tool and right up here right in there i'm going to click and drag out a little angled line like so i'm going to go ahead and go to mirror select that line to mirror and the mirror line is the center line hit apply done let's go to tangent arc bottom here and put that in and then the top one here and now we should add some dimensions to that so the bottom arc is to be point one the top arc is 0.2 and the distance between the centers on that one is a half inch and now look at this i went a little too quickly here so i want to get that aligned so i want it to be tangent actually so i'm going to select tangent select that curve and this one that will smooth it out so if that ever happens to you i just went a little too quick i think and i didn't get the green dot like i'd hold now we need to center the dimension there's actually a bolt circle and that bolt circle is 0.835 and so essentially if we want to do that we could we could go to circle and turn on construction and highlight this edge until you see the center and there it is and 0.835 is that right yep 0.835 and hit escape and turn off that tool turn off that tool now actually i'm going to go ahead and click on this with the right mouse button and change the construction because it didn't make it a center line like the center lines are explicit now okay and so in theory oh you know what i was wrong on that i'm sorry we're looking at this one right here which is a radius of 0.7 okay so technically we didn't need that one here's what we can do instead let's just go at a dimension since it's a radius it makes it easy actually we could click here to this center point and again that was point i just want to make sure 0.7 okay there how it's located could have probably even made that tangent to that top edge but i'm not sure if that when i designed this years ago that wasn't my intention all right now i'm going to go ahead and cut that through now we could do a circular pattern of sketches i'm going to show you a couple different tricks here let's go to 3d model extrude select that profile and these profiles reverse the direction it should cut make sure it's set to through all and hit ok now that we have that as we look at the drawing here there are 24 degrees off center from each other and there's two on this side two on that side so let's go ahead and select that extrusion go to circular and the rotation axis select this right here all right now you know we could go around and turn off individual ones let me just show you here if we went with um 24 degrees oops i didn't want that right click add a feature i didn't want to hit enter so we have 24 degrees and let's just go with three actually it's just that's per one so we actually have two there oh darn it i keep hitting enter edit feature sorry about that i had to right click edit feature okay so we see that there we have actually we have fixed oh no we don't want to fix i'm sorry i want rotational and if we double this to 48 now in that theory we can change it to 3 there and then we've got it all right hit ok now if we want to get them to the other side now we could have gone all the way around with an array and figured that out but um i want to show you also you can mirror these over too so if we select the extrusion hold ctrl select the circular pattern go to mirror in theory we should be able to select our right plane which is the x y plane all right and the let's see did it get it i'm not seeing a preview no it didn't take so let's edit that all right so the features we've got to select this there we go okay we just need those two selected and hit ok all right there it is now we could continue on with the boss on the front here start a sketch i'm going to rotate this vertically go to the circle now to wake this up i just tap the edge but don't click find that center point drag it out point eight six eight is point eight six eight let me look 0.835 so double click on that point three 0.835 all right and then that's 30 thousands in heights i'm going to extrude so 0.03 now we want to put a cut out on there and there's a little there's an array of little holes you know here's what we're going to do with that select this face start sketch let's get that rotated a bit again okay and we're going to look at that print and we can see it's a rectangle of 0.1 vertical and by .05 wide it's centered and it's located the base of it's located 0.371 from center so let's try that let's go to use a point center get right over here and let it float drag it out and let's make that point one hit tab by point zero five hit escape now we go to dimension and dimension this bottom edge if we select this we should be able to get to center there we go and click and then this is to be 0.371 and then it's located now we could hit 3d model extrude zoom up and select those two profiles flip the direction through all and hit okay now let's put some fillets on here now the radius is called out on here probably zoom up to see it on a side view there's a 100 thousandths on the inside and then there's a i believe a 30 thousandths radius yep around the outside of that so let's go ahead and put those in so let's get this fill it in first it's supposed to be 0.03 select this edge here hit okay now we want to keep it separate from this next one so now i go back to fill it this one's going to be 0.1 and it's going to just be this edge here it's going to give us a really interesting looking effect when we're done and hit ok right now we want to pattern that hole and that fill it so let's select fillet 3 and extrusion four holding control go to circular rotation axis you could select this face and again because inventor does it that way it's rather unique actually it's a very nice feature to be able to select that filleted face that's rounded as a axis of rotation now the placement let's count how many we have there i don't think i have it on the print and we have 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15. hit okay all right this next feature there's no dimension for because it's just a logo you're welcome to make your own logo you don't have to do the one i did i did like kind of looks like a death star i suppose i didn't put any dimensions on it just like that and then extrude select that and i'm going to have it cut down but i only want it to cut like 0.01 just barely recessed okay let's flip it around this side let's get the inside now select this face start sketch there's two concentric rings on the print an id of one let's uh find that center there it is i just woke up that center and well the one the od x is 0.6 and the id is 0.1 you could do an offset i suppose i'm sorry 0.0.5 and then go to 3d model extrude select that profile and let's look on the print what that's called on right here if we follow this line it's 0.13 okay now the boss says select this face start a sketch this one in the center is much easier so i'm gonna go circle and i have to wake up the center point now normally i should have actually had that locked in there you can see we could get by without it but it is sometimes nice to lock into the origin and i'm gonna show you how i could go back and fix that if you wanted to so i'm going to click here and these are 0.125 if i'm correct let's again look at the print another 0.175 three of them and then there's a recess in it point one deep by point one diameter and there is draft on those and i don't think i called out the draft but we could put the draft on that's fine we'll put like one degree so hit escape it's 0.175 let's draw another one over here we're just going to eyeball that one i'm just going to draw this one out click and then i'm going to hit escape and control select these two and go to equal that makes them both equal so i didn't have to add another dimension because we want them all to be the same now i want to get that over to the other side let's go to line and go ahead and draw just a vertical line there to mirror across i'll go to mirror select this and then mirror line select that and apply and done now we could go to 3d model extrude boss select those three and let's look at what the print calls out for the height of those 0.375 oh and i wanted to add draft so here's what you could do click on this right click and edit feature and the taper as they call it here let's just add like one degree and actually flip it so it's one degree minus one and again the reason for draft is so it can pull out of a mold easier now select this face here start a sketch and there's these bosses that are a hundred thousands by a hundred thousand so we could draw those in i suppose right here point one and then i'm gonna make these equal so now i could go to equal click on that click on that click on that click on that so again they're all the same go to extrude select those and they get recessed actually so flip the direction make sure it's set to cut and it's only 0.1 deep and we're not going to add draft on those all right now all that's left if you want to add those ribs and here's how i'll show you how to do that i don't have any specifications for the ribs other than maybe the thickness we'll talk about that select this face right here and that's the floor of that recess go to create sketch and we can have a little fun with this let's go to the line tool and we could put one in right about there notice i'm not touching the lines we'll put one in right about there and then here you could right click great line rather than always going back to that and over here hit skate okay now we want to get these over there so we could actually use this line as our mirror so go to mirror select these two entities here and here go to mirror line select that and hit apply now let's try i'm going to rotate this and we're going to go to 3d model rib and you can select these now they're really thick now there is actually a rule of plastics that goes along with this now those deactivated because it's too thick um there's a sixty percent rule the overall wall thickness uh on this i recall was about sixty thousand so let's say it was a hundred thousands point one you should make the ribs on it sixty percent or less than sixty percent of the wall thickness and the reason why is because that those masses of plastic as they intersect vertical ribs with the flat face will actually cause sinkage when it cools and it will sink make little sink marks on the nice flat side so it's not flat anymore so if you've ever seen a poorly designed part that's why someone didn't reduce this so the overall wall thickness correct was a 60 000 so i could look at the print make sure but i'm pretty sure it was so we'll make it like 0.003 i mean you know we can make it we'll just make a point or we'll get within range point zero four okay we could also add draft to those too okay or taper okay and hit okay now i got really sloppy with those i should have actually centered them but again i didn't have any specifications right off the bat but there it is that is our part that's a tough one and that's what you're gonna see in industry you'll actually get better drawings hopefully actually sadly actually i used to get really really bad drawings from customers but um not all the time but that's it for exercise four and lab four be sure to save this and remember do your alt print screen i'd like to see if you could give it to me either side is fine whichever side you'd like for your portfolio let's say i chose this side here i really kind of like the inside let's go with that and then we could go to default and i'm going to go with chrome polished and then i use i usually like to add a little bit of an enhancement on some of these faces and let's go with the green darker in there and then we go to view and you don't have to do this part all these little details i'm doing realistic ray tracing and instead of the default ibl like i like one light or two lights sometimes looks better okay and that concludes this exercise

Channel: vertanux1

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Id: J_Ndr6vDuKI

Length: 45min 23sec (2723 seconds)

Published: Thu Aug 06 2020