CREO: Creating a Simple Assembly & Creating a Part in an Assembly

okay so today we're gonna put together a simple assembly it's gonna be about six parts and we're gonna create a couple other parts just to finish off the assembly just to show how you can create parts within an assembly so this is the assembly we're making my ear it's a little pneumatic single cylinder engine this little wheel spins around in the back is a little piston that goes up and down as the wheel spins and we're gonna assemble it together in creo so first I'm going to select my working directory I've already navigated to the directory I want to be in but normally I would have never get it to it I'm gonna hit okay okay make sure I don't have anything in the background so I race not displayed there's nothing there someone hit new assembly MS 1 0 0 1 - 0 0 is the drawing number that I gave to my students so I'm going to hit OK and now I'm in my assembly looks just the same as any other part but first I'm going to assemble my main piece now my main piece looks like I'll pull my PDF over looks like this a little t-shaped frame where all the other pieces assemble - so I'll hit assemble I'll navigate to my t-shaped frame which is 1 0 0 1 - 0 4 I'll open it up and it'll put it by default in the center but I still need to find it right now it's pink which means it's not defined ok so what I'm going to do is I'm going to turn on my datum planes usually a good place to start and what I like to do is if these are off I like to turn on my tree filters to also have my features on so I can also see my planes and my feature as well as the different features under my part to create that I used to create the part as well so my first starting part a lot of people what they like to do is they go up here and they just hit fix now I don't like that personally because it takes a lot of assumptions into play and I'd rather actually define where my piece is so we can do this logically first I can take my assembly front plate and I can say okay I want my assembly front plane to be on the front plane of my part now I just selected the two planes Braille and do that just to show you the other way you could do it is what I could do is in my model tree I could select the assembly front then I could hit this little arrow and I could select the front of my part alright and now you can see that those two are on top of each other so a couple other things that are pretty handy when you're assembling something and assembly is if you can hold ctrl and alt and then middle click like you normally would spin a part you can kind of see what directions it's constrained in and which ones it's not so right now I'm on that front plane you can see that rotating but I can't move it backwards and forwards I can only twist it in this one axis okay which tells me that I'm kind of constrained in one direction which makes sense because we only made one constraint now if I use the right click instead of the middle click this is how you can move a piece around without rotating you can see it's just moving along this plane okay so if at any point in time you ever get lost and you're not sure of what constraints you have left that's an easy way to do it so the other thing I like to do is I like to have this placement open know when you're first constraining apart you can just keep clicking and it'll keep adding more constraints but if you're editing apart you have to actually click this new constraint option right here so if I click new constraint we'll just get in the habit of doing that now what I'm going to do is I'm going to make this right plane of my part and the right plane of the assembly aligned and this time I'm just gonna pick them I'm not going to use the model tree I like to move my mouse as little as possible to save a little time so I'll pick the two right planes now those are on top of each other now you can see I can't rotate it anymore I'm holding control and all and the middle mouse button nothing happens but if I hold ctrl alt and I use the right mouse button well look at that it can still move up and down that's why it's still pink right now maybe magenta is more accurate depends on your definitions of colors so we're gonna go ahead and hit new constrain again and this time I'm gonna take the top plane and I'm gonna assemble it to the top plane in my part now for my first part I usually like to use planes because I've modeled the part with the consideration of how other pieces are going to be assembled to it so if I line my planes up chances are it's gonna put my piece in the right place but the other thing I could have done is I could have assembled like the top plane to say the bottom of my frame and that would work just fine as well so you can see my parts turned orange now and that means that it's fully constrained very very important also you get a little clue right here where's fully constrained your parts need to be fully constrained now let me show you what would happen if it wasn't so if I hit okay now I'll just middle click do the same thing you can see this little white box that shows up now what we need to do in that scenario is we need to stop we're doing right away we need to edit the definition and add the constraint that's missing and a lot of times what I'll do rather than just hunt through the other constraints and try and make sense of it is I'll hold ctrl alt right mouse button and now I can see it moves up and down so that would give me a clue that I need my top planes to be assembled now I'm gonna middle mouse button click again that's just gonna automatically click this check mark anything that's blue gets selected by doing that okay yeah you know what why don't I turn my edges on to it's a little easier to see that way all right so I go back to my default orientation now I have my piece now from an assembly at this point you can use you can use the piece itself just to show the other option I'm going to turn my planes off so we only use the pieces so I'm going to say assemble okay and what I'm gonna assemble first is my wheel alright now my wheel lines up with this hole right here has a pin that goes through it okay and we're gonna use that hole later to create a piece but it also assembles to this side a little space so that we don't have any sort of friction okay so this is where that ctrl alt and right mouse button is handy I can move it over here and now I have it in front of my piece all right now the reason I did that is if I had just assembled these two middle things they're gonna be right on top of each other not the end of the world but I kind of like that a little bit so my first constraint is I want this hole and I can do this a couple of different ways I can turn the axes on and select it or I can just use the insert constraint which is just selecting a cylindrical surface and selecting a cylindrical surface that lines up okay and now those are lined up with each other now if I use that right mouse button you can see I can only move it in this direction apologize for the belt I am a teacher and we do have very loud bells here so now I can drag this along here because I've already constrained it in two axes really I haven't contraction strained it from a rotation but cRIO does assume that so my next constraint so I go to the placement tab my next constraint is going to be this surface having a distance to this surface now you'll see what creo does and it's usually pretty good about this if pieces are close together is it automatically assembled it as coincident now I don't want that so I want distance okay so my distance offset I'm gonna put about an eighth of an inch here okay leave a little space that might be too much so why don't we try a sixteenth that looks a little better okay so now that I have a sixteenth of an inch there and let's say it look like this oops let's say I type that in it went the wrong direction okay would have been as simple as before the number just put a negative sign hit enter it'll flip the dimension to the other side this flip actually flips the constraint okay so you can see the part flips back and forth now you notice it says allowance UMP shion's right now and that it's fully constrained what allow assumptions means is that right now this piece can turn this way but for most things that you assemble with an insert constraint for example like a bolt in a bowl you don't care about how it's rotated if you're assembling things that maybe have like threads or something on there like modelled threads which usually isn't the greatest practice slows down your model a lot but if you had something where the threads really really mattered and you wanted to make those threads line up well then you would need to have some type of rotate constraint so if I have that allow assumptions off you can see it's orange now very easy to fix okay I could say for example well you know a new constraint this plane needs to be oriented in the same way as this plane right down the middle okay and I could say they're parallel alright well now it's fully constrained as well so I can either use allow assumptions or do it that way both do the same thing so I'm gonna say okay now I've got my other piece assembled here okay now the third piece that I'm going to do is I'm going to assemble the two feet on the bottom here give us a little stability so if I had assemble and part number three is the feet okay now the way that my feet are assembled here is there's a little bolt that comes through the front okay and assembles through into this piece here so my first constraint that jumps out at me is that this hole right here needs to line up with this hole alright now I can see that the wrong direction right but I also need to look at what I have so I can see this surface here is all the way back so it's actually assembled in the right direction it just doesn't have all the constraints I need so I'll turn my datum planes off make it a little easier to see I'll add a new constraint by saying this surface is going to assemble to this one and then you can see because they're further away creo assumes well you know maybe they want a distance this is really really far apart but I can just hit my pulldown here and go to coincident what you should not do do not do this okay there's a lot of people who design things and they do this this way which is very terrible practice really really bad is type zero and hit enter now you may think well does the same thing was it matter well the issue is his creo is a parametric modeling program okay so all of these little dimensions these little constraints all this stuff is part of the parameters so when you put little zeros in here number one you can get some really weird results down the road when you go to redefine this thing but more importantly every single number gets recalculated every time you open the part at when it's not in session so you're better off just hitting coincident because then they just understand that those two surfaces meet up now okay now I'm gonna turn that allow assumptions back on because normally you should have that on all right but you can see mine can go like this right now so if I was really worried about that I could have that off and I could say well these two surfaces are parallel okay and that would orient it in the right way all right so that that one's okay now if I open up this part actually I don't even need to I can just hit this little arrow here I'll notice that these holes here were patterned so normally what I could do is I could do a little reference pattern that would jump it over to the other side the problem with that is since I also patterned this hole up here that's the same size if I was the pattern and create feet all the way through all three of those I can get around that though so if I hit pattern you can see there's my three dots right so if I hit okay now well I've got the foot on the other side but I didn't really want it there so in my pattern I can just turn off this dot and then I can hit okay and now I've only got those two all right now one thing to remember with a reference pattern and the reason that works is because it's a reference pattern it's referencing an initial pattern now you also have to notice which one of these circles has another little skinny circle around it okay that is your initial instance you can not turn this one off I can turn this one off I can not turn this one off okay so that's important to recognize because if the initial pattern is the one that you don't want then you won't be able to use that reference pattern or you'll have to go back and edit your feature the reason that's my initial one is because that's the first hole I made on that feature okay so now I've got those two feet in there all right and if we work our way down our next piece is a little crank plate okay that sits back here and rotates around to give some some movement or create a rotary motion of the piston that goes up and down okay so you know it's kind of hard to see but here's a little guy right back here in between these two farts okay so I'll go to assemble all right and I'll go ahead and open part number five and there's my little crank plate okay so my first assembly constraint is going to be this assembles to this okay if I move that in lines right up now for my next assembly constraint I'm going to say that this surface and this surface have a very small amount of space between them okay very very small amount of space okay now I could put that right up against there really isn't a big deal if I was to do that because there's plenty of space here for this little guy to move around if it needs to now the other constraint I'm gonna apply is I'm going to add another constraint to say that I want this surface and this surface to be parallel okay now I could also change the angle offset and then I could start typing in numbers and I could rotate this thing around right but for now I'm just gonna make them parallel I can go back and edit that later if I need to all right so now those pieces are all lined up and the next thing I need to do is I need to assemble part number two okay which is my cylinder all right so the way my cylinder works is this hole lines up with this threaded hole okay and that's where it rotates around I have a little bushing I'm going to assemble that that rotates around okay now the other thing that matters here is that this right here rotates with the bottom pin here because there's a little piston that moves around and we're not going to model that piston because this is just a simple assembly that we're just getting used to how to assemble pieces but if I modeled that then I probably would have assembled the piston first and then assembled it into this bore but the interest is saving time I'm gonna say that this surface and this surface are parallel okay so they line up now the last thing I need to do is this thing pretty much sits right up against this surface here so I'm going to pick these two surfaces and I'm going to say they're coincident okay now I have that feature assembled and then the last feature I have of the six parts that the students need to create is this little bushing this bushing goes right in here and that surface sits right up against there this coincident alright and for that one I don't care how this thing's rotated it's completely symmetric radially so I'm going to allow assumptions on there all right now normally what would happen is we'd have a little bolt that assembles through there into this piece okay now in the interest of saving time and keeping this video short what we're gonna do is we're gonna create the pin that goes from this side and assembles over to this side okay now the first thing I'm going to do is I need to know how long that pin is so I can go to analysis measure hover over this surface it gives me a whole bunch of information hold ctrl and pick the other surface now it's telling me that it's point eight seven three long okay so that's awfully close to seven eighths alright so maybe what I'll do is I'll create a pin that seven eighths and it'll just sit flush with here and maybe stick out a little bit on the back of that one okay so here's how you create a model within an assembly now the first thing I'm going to do is I'm going to say create create a component in assembly more you see that message right there that's going to give me this create component okay now what I'll call this thing is dowel pin okay and I'll hit okay now it says do I want to copy from some existing stuff do I want to locate datum planes things like that and what I'm going to say is that I want to locate some default datum planes and I must say sorry jump the gun I want to locate default datum planes and I'm gonna hit OK okay now what I need to do just turn on some datum planes all right I think it accidentally backed me out of there alright let's try that again delve in and you know why don't I just hit create features it's another way I can do it okay so now I'm going to create features I'm creating my dowel pin you can see there's a little green star there I'm gonna say I want to create a revolve and I want to create that revolve on this plane that goes right down the middle it's gonna zoom me in now for my references I'm gonna turn on some axes okay for my reference is I'm gonna say I want this axis right down the middle of this hole I want this surface over here and I want this surface over here middle click a few times so it goes away and now just like I'm creating a normal revolve I want to center line and then these dolphins going to be around so I'm gonna make a little rectangular section now what I could do is I can go right up to this length here but I'm just gonna do that just so I get it dimension so I'll say it's 0.875 alright now if I had turned this to have hidden lines oops missed it hidden lines the other thing I could do to make sure this dolphins the right size is I could say this line is in line with that hole there okay now I don't even have a diameter on this thing now it is an eighth of an inch because that's something that hole is but now I can hit my check box I'll turn my shading back on and you can see there is my dowel thing all right rotating around I'll hit my check box maybe I want to throw a few chamfers on here make it 45 degrees 101 fine and okay now I've got a little dowel pen there now to go back to my assembly all I need to do is right-click my assembly and hit activate now my dowel pins not saved yet it's there we can see it in the hole however it does not save until I hit save up here save object pops up I hit OK now if I go and hit open okay look at that there's my develop it I can open them right up alright modify it as much or as little as I like alright and that's how we assemble this together so we use a couple different constraints okay we use some datums use surfaces surfaces tend to be the best once you have a base component the reason I like them personally is because now if I move any of these holes for example if I open my frame up and I changed my design and I say well you know this actually needs to be not quite that much this actually needs to be 2 and 3/4 up here I regenerate this I close it you can see my holes moved I regenerate my mass M my assembly that everything moved with it ok so it can be a little bit of an advantage if you model things properly it really shouldn't matter either way ok you spent some time paying attention to how am i modeling this what's the orientation notice the orientation of this part when I modeled it it's exactly the same as it was in the assembly and considerations like that can save you a lot of time down the road okay so I'll put up another video I'll put up another video about making a drawing for this but that's how you assemble a simple assembly this is six parts will seven now I guess eight if you want to count these as two different parts they're seven different parts one of which we created in the assembly okay

Channel: Mr. Mez CAD

Views: 18,841

Keywords: cad, creo, ptc, modeling, assembly

Id: 2FIeVIzpzRs

Length: 24min 45sec (1485 seconds)

Published: Tue Oct 31 2017