Creo Parametric - Assembly Basics

let's take a look at the basics of modeling assemblies in creo parametric first I want to show a few different configure options so I'll go to file options and then configuration editor and the first one that I use is comp assemble starts and I have it set to moved in place and when you start placing components it's going to attach them to the end of your mouse so you can drop them into the approximate location in space before adding constraints there's another one called create temp interfaces and the first time that you assemble a component during your career parametric session it will remember how you assembled it and allow you to use that over and over again and another one is search path and if you're not using a data management system like windchill you could use this to direct it to different folders on your computer or your network where you might have components so let's cancel out of there to create a brand new assembly I'm going to click file new and change the type to assembly and this is going to be an engine so I'll change the name that's the file name you can also use a comma name if your standard naming convention is a bunch of numbers you want to use real words to describe what it is and here we have the option to use a default template I'm going to uncheck that just to show you what happens if I use my own custom personal template so this is going to give me a number of different things to start with first off if I turn on my datums I get a bunch of default datum planes and my default assembly are C's make default coordinate system if I go to my properties dialog box it also establishes what unit system that I am using and also you can have different predefined parameters and relations and also your layering scheme for how you want to organize the different objects and I have my default template setup for model-based definition so I have a bunch of different combination States in here as well so now that we have our engine assembly started with our default template it's time to start bringing in components so I will click the assemble button to do that you'll notice in the tooltip that in creo parametric 4.0 and later a is the keyboard shortcut for getting to that command so I will click assemble and in my working directory I'm going to start off with the left side of the crank case and I'll double click on it like I mentioned because that config dot Pro option I have turned on the component is attached to the end of my mouse and I can just left-click to drop it somewhere and you notice that we have this dragger on the computer screen that allow us to translate the component as we're placing it also you can rotate it to different angles and this is very convenient when you're trying to position it before adding constraints you can even do in plane motion with some of these other different controls for the first component though probably 98% of time or more you're going to align the components default datum planes with the default datum planes of the assembly and that's called the default constraint to get to the default constraint there's a drop-down list over here you could choose default but since it's so common you can also hold down the right mouse button in order to get to it and one of the biggest mistakes I see with new users creating assemblies is that they don't assemble the first component and at the end of the demonstration I'll show you what that would end up looking like so I'll choose default constraint and on the dashboard we notice that the status changes to fully constrained and the component color changes to orange to indicate that it is located in our model so that's good to finish off placement I can click the check mark or middle mouse button we'll do the same thing and to reduce screen clutter I'm going to turn off the display of my datums so there I have my first component placed here in the now let's place the second component so for this one let's click the assemble button this is going to be the right side of the crank case and again I've got it attached to my mouse and I can just drop it where I want to and then to help facilitate placing it correctly I can start using the dragger to position it approximately where I want and so when you are defining constraints you are going to select reference geometry from the component that you're assembling and reference geometry from the assembly in order to define its location and typically with static components we're adding enough constraints to remove all six degrees of freedom a component has three translational and three rotational degrees of freedom and so for this one first I'm going to select this cylindrical surface you'll notice that I have a little rubber band effect with this set of dash lines here stretching out and then I can use it to highlight what I want to assemble to and I'll click there and right now it's giving me a coincident constraint between those two surfaces and then I can start defining my second constraint maybe I'll pick this flat surface and this one over here and it says it's fully constrained because it's allowing assumptions it's not caring about the rotation angle but that's not correct that's not how I want it placed in here so sometimes when you have allow assumptions correct it's not going to give you the right thing so you can right click and hold and turn off some shion's you can also do that from a placement tab on the dashboard and I can tell creo parametric that I want to add another constraint I'm going to pick this cylindrical surface and that cylindrical surface and it gives me an oriented constraint and that looks correct for how I want it placed in the model and so again now that I'm happy I'm going to hit the checkmark to place it in there so two components in here next up before I start assembling more components I do want to mention that there are some assembly settings for your session if I go to file and then options here we have assembly and heroine of the top we have reference creation and backup control that's for external references in top-down design but I want to scroll down in here and show you that we have options for component dragging when we're moving it in here and also automatic placement options if you're using some of those different temporary interfaces here is the option for controlling that so again you can set these different things from configure Pro options you can also change your assembly placement settings during your session so let's cancel out of there now I'm going to assemble a couple of cylinders on top of here so let's click the assemble button and I'm gonna grab cylinder dot PRT again let's position it approximately we are where we want it to be and for the first constraint I want to line up this cylindrical surface with a cylindrical surface over here and I recommend that you concentrate on the geometry that you want to align and also think about how you would assemble this in the real world alternatively rather than picking geometry first you can pick one of your different constraints that defines the relationship between the geometry when the most common ones is coincident so that will make two flat planar surfaces lie in the same plane or if you have two cylindrical surfaces or conical surfaces it will line up the axes similar to coincident is distance rather than making two entities lie in the same plane you can define a distance between them and go offset like the name implies you define an angle parallel you make them well essentially parallel to each other you just don't care about the distance vary can similar to distance except you're not specify a numerical value normal makes them perpendicular to one another you can see tangent in here so you know we have about a dozen different constraints but again rather than picking the constraint first I typically start focusing on geometry so I'm going to pick this cylindrical surface over here and this cylindrical surface over there then I'm going to pick the two planes that I want to line up so I'm gonna pick this surface over here I want to pick a surface on the underside you could either use query select tapping with the right mouse button or if you click on this button on the dashboard you can display the component in what's called an accessory window and you can resize it and that's very convenient cuz allows you to rotate the model in its own separate window as opposed to doing it in the main window and so let's pick this surface over here right now creo parametric thought I wanted an angle offset that's not what I want I actually want them to be coincident so there it moves it into the right place and because I turned off assumptions it keeps assumptions turned off if I turn assumptions back on it says hey that's all that you need to assemble it but the problem is I'm not sure that the holes are lined up because I haven't controlled the rotation angle so what I'm going to do in order to facilitate picking the holes I want to line up here you'll notice for the second constraint we have a checkbox with a constraint enabled by unchecking that I can then translate it which can help me and now I can add my other constraint I can say let's line up this hole and this hole over here gives me that oriented constraint now I can go back to that constraint that I disabled and re-enable it and now I've got the component in the correct location so that's good I will hit the checkmark and so I've got my cylinder in there one second because all my colors are the same colors the background screen I'm going to file options and then system appearance graphics let me change my background color to a little bit of a grayish color for some more contrast alright so for assembling the cylinder again rather than hitting the assemble button and then defining my constraints I can repeat this component because I want to use essentially the same constraints as before and so I can click on the component and then hold down the right mouse button and here we have the repeat command and I'll list the different constraints I'm going to select all three constraints and then click the Add button and first it's highlighting the cylindrical surface and then a flat surface in front of the hole that I'm gonna line up and so that's very quick and easy for getting this component in there again and I could continue adding the cylinder as many times as I want using this repeat component dialog box but I only want it in there one other time all right so let's click the ok button and let's do a few more constraints or excuse me components in this assembly and I'm gonna create a stub assembly and place it so the next component is going to be the cam cover and for this one let's select flat surface over here and flat surface over there and I'm gonna turn off the display in the sub window oops I turned off the display in the main window in the sub window over here let me make sure that for moving it around if I hold I can also use the control in the Alt key ctrl alt and right mouse button for translating it to moving it approximately where I want it to be so for this one this has some curved surfaces in it and so I'm going to define a new constraint oops there we go move it approximately I want we're going to define a new constraint and let's choose the edge from the selection filter because I know I only want to pick edges I want to line up say this edge and this edge over here and let's see let's drag it down approximately and again because I have curved surfaces here I'm not picking the flat surfaces usually if you have a choice between surfaces or edges you want to pick surfaces and so let's pick that edge there and I'm going to use the selection filter again to change this to edge there we go and now I've used edges to line up where that component should be that's good let's hit the check mark over here and another component in this one will attach the blower to the cam cover and again let's position it approximately how I want it to be and let's pick this cylindrical surface and line it up with that over there let's pick this flat surface and open up it in its own sub window helps me pick this surface over here right now suggested normal that's not what I want and you can also double click on the 3d note in the graphics area to access the constraint it also lists the geography that you're using and from here we can say hey I want to use a coincident constraint instead and right now it's in here but it's rotated incorrectly so let's right mouse click and hold again turn off assumptions and I'm going to add a new constraint and this one I'm gonna close this little window over here I'm gonna take this surface and this surface and rather than angle offset and I can double-click on the note and so let's just make those parallel that's good that's how I want it in here so I will hit the check mark and my engine is starting to come together and before I put in the next components I'm going to create another assembly and then place it in here as a sub assembly so let's create new and this is going to be for my carburetor and air intake and I'm not going to use the default template I'm going to use my own personal I accidentally chose to create a park let's cancel out of there come let's do file new change the radio button to assembly and again this is the carb air intake and I'm using my own personal default template let's hit the assemble button and first off we are going to start with the manifold and again for the first component most time you can just use the default constraints and let's hit the checkmark and it's located in here now for the second component I'm going to assemble the carburetor and for this one let's see take a look at how I want to assemble it in here gonna select let's do yeah that looks correct let's select this cylindrical surface and this cylindrical surface and right now it's giving me coincident let me turn off the display in the accessory window and I'm gonna use ctrl + Alt + left drag it to drag it up over here and for the next constraint let's pick this flat surface oops and that flat surface over there and it looks like I have it oriented incorrectly yeah looks like I got the wrong holes lined up alright no problem let's go and I deleted that first constraint over there and so and disable the constraint so I can get to the holes and say for the new constraint let's pick this cylindrical surface there that cylindrical surface and actually before I enable that constraint let's do another new constraint I'm going to line up this surface here and this bolt surface now I can go back and able that constraint there I have it placed the way I wanted to so again sometimes when you're assembling you're like hey I accidentally accidentally picked the wrong stuff you might delete constraints and then put it in the correct one that you want or change the references that you're using all right last one that's going to go into this carburetor assembly let's assemble the scoop and for this one let's see let's have a pointing say this direction and again I'll pick a cylindrical surface there cylindrical surface there and let's pick a flat surface there flat surface there and we just have assumptions turned off so let's do a new constraint and let me disable the first one I really like this disabling so I can actually the first ones good let's disable this one so I can translate it up and for the new constraint that surface that surface make it oriented in the correct direction go back and enable that coincident constraint hit the check mark and now I've got my carb air intake created let's hit the Save button for this one to put it into my working directory and now let me close this window back to my engine window let's hit the assemble button and this time I'm assembling a sub assembly another assembly into my main assembly I'll click the Open button and let's put it right about over here and then rotate it so we get it approximately the way that we want it to be and so for this one we're gonna line up the surface of these cylindrical surfaces first this surface and that surface over there let's add in a new constraint by the way the reason I'm clicking new constraint is a lot of times if you pick cylindrical surfaces followed by cylindrical surfaces kuroh parametric might think that you're trying to make changes to the first constraint but I like right-clicking and choosing new constraint to make it explicitly known to creo parametric that I am trying to create a second constraint that is also using cylindrical surfaces let's pick that surface there and that surface over there and I'll just go to picking a flat surface and some choosing a different kind of surface I didn't need to do new constraint so that's good now we have our carburetor sub assembly in there so let's hit the check mark and that is all the components that I am going to place in here and so there are a few other things I want to point out about assembly modeling first off if I expand these different components in here I have what's called a placement folder that will allow me to access the constraints right from the model tree let me scroll down over here so for example if I go to the cylinder component over here again we have a opes one too far we have a placement folder and we can see that we have three different coincident constraints and as you click on them they highlight on the computer screen and as I showed in another tips and tricks video you can also use the repeat command right from individual constraints which can be a lot faster than using the repeat command like I did it in this video here all right and at the beginning of the video I mention that one of the biggest mistakes that new users and creo parametric make is that they don't use the default constraint or any constraints for the first component let me edit definition of the first component that's placed in here and I am going to go to the placement tab and delete this default constraint and hit the check mark and now what you'll notice is that the first component has an empty box next to it meaning that it's under constrained in this case completely unconstrained and all the components that are assembled to it have a double box next to them let me try to blow this up and so you can see in there the box next to another box in the case that it is assembled to an under constrained component so again if you see this in your model tree the most likely cause is that the user did not assemble the first component and again the overwhelming majority of the time you should be able to use the default constraint for the first component now you'll notice those little glyphs as they are called went away from the model tree and the last thing that I want to mention is from the tools tab there is a bill of materials command and we can do it for the top level or an individual sub assembly you can choose which other components you are including but just gonna go with the default and by that we can see this bomb report be generated in the embedded browser I hope you enjoyed this video for more information please visit

Channel: Creo Parametric

Views: 29,945

Keywords: creo parametric, ptc creo, creo ptc, creo parametric tutorial, creo parametric 2.0, creo parametric 2.0 tutorial, creo parametric 3.0, creo parametric 3.0 tutorial, creo parametric 4.0, creo parametric 4.0 tutorial, creo parametric 5.0, creo parametric 5.0 tutorial, creo assembly, creo parametric assembly, creo parametric tutorial for beginners, creo parametric 3.0 tutorial assembly, assemblies in creo, creo assembly constraints

Id: bYKbYLfpk6k

Length: 24min 4sec (1444 seconds)

Published: Thu Feb 28 2019