Creo Parametric 8.0 - Part Modeling Enhancements (Video 1)

in creole parametric 8.0 there are numerous enhancements and in this video we are going to look at five of them first creating a multi-hole feature i'm going to click on the hole command and first off there's a lot different about the interface now you'll notice that there is a tab that opens up automatically also it is no longer overlapping on the model tree i'm gonna have an entire video on user interface changes but here we have a type drop down list and a new choice in here is sketched and so when i click on that we can pick on the surface that we want to sketch on and for the first one i'm just going to drop in a couple of holes let's create them on here and for the sake of this demonstration i'm not going to dimension them but here you can see we are creating two holes and let me just configure them a little bit everything else here looks good right now you can see that we are using an internal section for the sketch of course you can pick a pre-existing section and right now we are placing them on points but there are a couple of other different choices in here let me hit the check mark to complete this one let's create another set of holes and once again i will go to the sketched option and let's define a sketch on the same surface let me then instead of dropping in a few points like we have over here i'm going to sketch in a rectangle so let's make a rectangle make it about yay big let's throw in some dimensions and let's call this one 12 let's also do from here to here and then make that one 12 as well so that way if the block changes size then the rectangle will change size as well now when i hit the check mark we are getting points located at the vertices of those sketched lines and once again let me configure the depth option also you'll notice that the buttons on the dashboard look a little bit different they are bigger more prominent to draw your attention to them let me grab a bigger size over here and let's do our countersink counter or oops there we go and so you can see how we're creating them in here now another button that you have here allows you to place the holes on the midpoints of the sketch lines as well so i'm happy with that let's hit the check mark or the middle mouse button and so in that way we are getting multiple holes created within a single feature second in sheet metal mode you can now use the flat wall tool to place walls on multiple edges so let me select an edge over here i will hold down the control key and select this edge as well so you can see that the placement tab opens up and we have our collector that allows us to select the multiple edges that we want to place the walls on in the model let me just grab one more over here and so that way we've got our different walls configured and of course they are controlled by a single height value so as we drag one the other ones are going to drag up and down as well let me go with the smaller values seeing as i don't know how big that cut is inside of there and so then we can hit the check mark now there are a few other additional options that you get here when you are doing multi walls let me switch over to another part model to show them to you here i have a sheet metal part it has a sketch that is extruded once again let's create a flat wall and i will select one edge over here let me hold down the control key and grab another edge we now have automatic monitoring for those multiple walls that are created within the flat wall feature let's go to the miter cuts here's the option to create the miter cuts if i uncheck that well we're going to end up with overlapping geometry which would not be proper and for the three bend corner relief type here we have a drop down list with four different choices tangent open closed and rip let's leave tangent and the miter cut type is set to through all we could change it to ob round which in this particular case doesn't do anything or you could choose no gap so it closes that up let's change from tangent to open and now let's take a look at the corner that we have and with the open option we can have no gap or you could choose here we have through all and then you can configure the size of the gap or here we have operand which in this case again won't make any kind of difference because of where the ob round would be placed let's go to the drop down list and change this to closed so here we have closed with a miter but you can also choose no gap so at some point you would have to throw in some rips in different locations in order to be able to flatten this but you do have the option to have a filled in corner and also we have the rip option and with the rip option right now we're set to no gap but you can change it to one of the other different options and you have the ability if you have a gap to control the size of the gap so that automatic miter option is now available to you when you are placing a flat wall on multiple edge references third geodesic curves those are curves that have the shortest path not a straight path here i have a part model i use the warp tool in order to deform this surface let me show you that deformation i will go to the analysis tab and then mesh surface and then pick this surface so there you can see the topology of that particular surface now i want to create some curves between some points on the edges so let's go to the datum overflow menu here we can create a curve through points and first off let's select points on opposite sides of each other i will select one point and then hold down the ctrl key and select the second point so there you can see a preview of the curve initially it is a straight line on the ribbon and in the tab you have the option to place the curve on a surface you can also access that from the right mouse button and once you say that you're going to place the curve on the surface you need to select the surface that you want to use and so now it is following the surface but we also have an option for a geodesic curve you can select that from the placement tab also you have it right on the ribbon so take a look at what happens to the curve when we make it geodesic now it is going the shortest distance which instead of going right over the middle of the model it's going around the side that's good for the first curve now let's create another one and let's use the points going sort of like diagonal across we'll go to datum curve curve through points again and select one point hold down the control key and select another point let's put this on the surface and again you can see it taking sort of like a straight line path but not the shortest path so geodesic curve and once again it bends around going the side of that dimple all right let's take a look at one more example let's go to curve curve through points again and let's pick this point and this point over here let's once again specify that we want it on the surface and that we want a geodesic curve so again now it's going around that dimple once more so let's hit the repaint so that we no longer have the mesh displayed and that's how you can create those shortest distance curves on a curved surface the next one when you're doing multi-body modeling you can now use patterns of references as inputs to the boolean operations let me show you what i mean by that before i do that i'm going to drop in another body in here to locate it i need a coordinate system so let's create a coordinate system i'll locate it at the intersection of this axis and the intersection of that surface one thing that you might notice is that now coordinate systems are three colors they are red blue and green sort of like the 3d dragger they're no longer that simple brown color let's go to the orientation i'm going to use this surface to determine the z direction and i'll use this surface to determine y i need z going downwards let's use the flip button that looks good let's click the ok and let me make sure that my coordinate system display is turned on i'm going to turn off my notes i don't need that whole note and so i'm going to use this coordinate system to bring in some reference geometry let's go to copy geometry and let me grab a reference model and i think i've got the part that i want in session i've got a little helical insert that i grabbed off of mcmaster carr and let's use the coordinate system method to locate it that's why i create the coordinate system i'll click the ok button and we'll bring in the body geometry i'll just select the geometry from the part and so everything here looks good again while we're here you might as well take a moment to look at how the dashboard for the copy geometry feature has been revamped where you have the text for the names of the icons and so you're sort of like toggling between the different types and we've got the panel that's automatically open if you haven't taken a look at the options tab in a while back in creo 7.0 with the addition of multi-body modeling you get all these other additional options but what i'm showing now so far is stuff that you could still do in creole parametric 7.0 so there you can see the insert inside of the hole if you take a look in the model tree that is its own separate body let's select that coordinate system and then reference pattern it because it was located on a whole instance from a pattern and now that i pattern the coordinate system i can reference pattern the body and so now you can see that here we have a folder this is pattern three with eight different bodies and you can see the bodies inside of there by the way you'll also notice we have this design items folder i'll go into more detail about this in the user interface for creo 8 video but this is a way that you can access your quilts and bodies from a folder regardless of the regeneration order so we have our bodies that are patterned inside of here let's say i want to do a boolean operation we can click on the command and again the interface is slightly different now we are going to do a merge and for the body to modify i am going to select the main body in the part for the modifying bodies well let's select the entire pattern of features and then we can hit the check mark and there we have the body merge and you can see the different objects that we have in the model tree one other thing to point out now again i'll go into this in more detail in the user interface video when you go to your tree filters in the body quilt tab you have the ability to display consumed bodies and consumed quilts let me hit the apply button by default these options are not checked but if you check the options then you will be able to see let me hit the apply button you will be able to see the consumed bodies in your different folders oops let me click ok out of here and they will appear in a reddish color as opposed to the blue color of the other bodies and geometry that you have in your design items and the last enhancement that we will take a look at in this video is the ability to display snapshots of quilts and surfaces as they appeared in the past history of your model so for example here i have a surface when i click on it i can see the rough outline of what it looked like in the past and a lot of times when you're working on a complex part and you're trying to see those old features you would either have to use insert mode to roll back the history of the model tree or you would have to edit definition of the feature in order to see what it looks like now you have the ability to display snapshots now right now when i right click on it here you can see that we have the show snapshot option so that gives me an idea of what the quote looked like that was used to start off the model back at this point also when i right click on it i can also choose to copy the snapshot so that way i can make a copy of that surface in case i want to use it for something else in the model let me select that and hide it so that i no longer see it let's take a look at a couple more in here so again this is what the feature looked like back in the past let me show the snapshot okay that's what the surface looked like hey let's take a look at another one let's grab the one right below it and let's right click and show the snapshot so there i can see i'm getting an idea of the design intent of how this was built up by showing those different snapshots and they are going to stay visible while you are working on the model until you hit the repaint button then they are no longer going to be visible in the graphics area let's take a look at one more example of this let me go to a different part so here we have the exhaust manifold and here we have the design items folder you can see the various different quilts let me start off by selecting one of my initial surfaces here we have a surface that was used at the beginning again you can sort of see the outline when i right click and hold in this particular situation we don't have show snapshot something that you'll come across in older models is that you have to regenerate the model at least one time before you can be able to see those different snapshots because again this is a new feature in creo 8 this model is quite old let me just right click and choose insert here and then exit out of insert mode this is one way that i used to trigger a full regeneration i got that trick from martin newmaller let's go to this particular surface now i'll right click now we have the options to show the snapshot and copy the snapshot so that way i can see what it looks like and in addition to using the options from the features in the model tree you can also do it from quilts in the design items folder so for example let me grab say this quote over here actually before i show the snapshot let me change to a no hidden line mode a lot of times that makes it easier to see these snapshots if they're taking place in the middle of the part let me repaint the screen and then repeat showing the snapshot just so that is not overlapped by the original quilt that i had selected so that's a way of being able to understand your design intent in the model and again if you want to reuse that geometry you have the ability to copy the snapshot so there you have it five enhancements to part modeling in creole parametric 8.0 i hope you enjoyed this video for more information please visit www.creowindshield.com if you learned something from this video please give it a thumbs up and if you like this video please click the subscribe button and ring the bell to be informed when new videos are uploaded thank you very much

Channel: Creo Parametric

Views: 7,641

Keywords: creo parametric, ptc creo, creo ptc, creo parametric tutorial, creo parametric 7.0, creo parametric 7.0 tutorial, creo 8, creo parametric 8, creo parametric 8.0

Id: 9tsAAhDVtPM

Length: 18min 7sec (1087 seconds)

Published: Wed Apr 28 2021