Creo Parametric - Mold Design with Sliders | Camera Cover Demo

in creole parametric you can use the mold design module in order to come up with the manufacturing core cavity and sliders necessary to produce an object let's take a look at a more complicated example here i have a camera cover that i want to create let me show you a finished version of this let me go to the mold opening and so this is what we are going to end up with here i have the core here i have a slider here i have the cavity and then you can see the molding let's create this from scratch to start off with i will go to the new icon in the upper left hand corner you can also use the keyboard shortcut of control n let's change the type to manufacturing we have a number of different subtypes but in this situation we are going to use mold cavity let me call this my camera cover mold and you can enter in a common name if you want here i'm using the default template but i'm going to change the set of units here i have my default datum planes and a default coordinate system let me go to my properties icon i have that added to my quick access toolbar just so i don't have to go to file and try to remember where it is it's under prepare oh yeah there it is you know just put in your quick access toolbar right now my model is in inches let's use the change button i'm going to do it in millimeter newton seconds let me set that here it's asking me how to convert or interpret this but i don't have anything in here yet so it doesn't really matter and then close out of there now i've got the set of units that i want all right to start off with let's locate our reference model if i go to the drop down list you have a number of different commands here but i almost always use locate reference model and here we have a file open dialog box that allows me to select the part that i want and then use the open button then you have your choices of how you want to create the reference model i never use the same model option sometimes i use inherited but the overwhelming majority of the time i use merge by reference in other words it is a one-way associative merge of all the geometry from the source part the camera cover into this new model that will be created camera cover mode which is the name of the assembly followed by underscore ref you can change the name and the common name if you want but i am happy with that let me click the ok button and then we can preview how the model is located relative to the pull direction and right now it's not located the way that i want it's sort of sideways inside of here let's go to our coordinate system display i actually have a coordinate system that is oriented properly so in order to use that in the layout dialog box you can use the pick icon underneath reference model origin and orient it'll show the model in a separate window here the choice is set to standard which allows you to select an existing coordinate system and so i'm going to grab this coordinate system called main and then i'll hit the preview button again and now it's oriented the way that i want i've got the pull direction facing up i've got the top of the camera cover facing up as well let's take a look at some of the other different options that you have in here i'm just going to do one of these so i can address the slider but you could do this rectangular and here we have the number that you want in the x and y directions let's take a look at increasing the increments a little bit then i can hit the preview button and there you can see let me turn off the coordinate system visibility i do not need that anymore so here you can see how they're oriented and they're all oriented with a constant direction or orientation let's see what happens if we choose x symmetric and then preview and so now you can see how the parts are symmetric about the x axis and let's do y symmetric and preview that one so here you can see how they are symmetric about y but again i'm just going to do a single one let's click the ok button out of there now we get a warning hey please confirm setting the absolute accuracy value to this number here when you are doing a manufacturing model you have to use absolute accuracy which makes sense in general you should always be using absolute accuracy okay let's click ok out of there and we can hit done return out of the menu manager the next thing i'm going to do is apply some shrinkage to this part let's choose shrinkage and by the way there are two different choices in here shrink by scale or shrink by dimension i prefer using shrink by scale and let's again choose that here we have two different formulas that we can use we can use either one plus s for the shrinkage factor or one over one minus s depending on what your shrinkage values are for the coordinate system that we want to use for the reference once again i'm going to use that coordinate system mean i just turned off my coordinate system visibility turns out i need it again and i move my mouse over the model right now it's highlighting the mold default coordinate system i'll tap the right mouse button now that allows me to query select to the main coordinate system i will pick that here's an option for isotropic if you don't want to use isotropic you can uncheck that and then you can define different shrink ratios in the x y and z directions i'm going to use .005 and x y and z let me double click in there 0.005 and hit the enter key there's this preview button here i never use it because i don't know i can't see that much of a difference in the model let's hit the check mark and if i expand the reference part you can see that we have a shrinkage feature located at the bottom of the model tree you can see that we only have the external merge feature that brings in all the geometry from the reference model okay now that we have shrinkridge the next thing i will do is to find my work piece let's click on the let me show you the options once more from the workpiece drop down menu i almost always use automatic work piece but if you have pre-existing work pieces you can bring them in here's this option to create a work piece which is more work than automatic work piece so let's just use that automatic workpiece and you can see the bounding box that is just the same size as the reference model right now it's asking me to select a mold origin let's just use the mold default coordinate system here we have the ability to do a rectangular workpiece a cylindrical work piece or you can do a custom work piece here the units are in millimeters one option that you have is to apply uniform offsets from the x y and z dimensions of the model i'll enter in a value of 30 and hit the preview button to show you what that would look like once again let me turn off my coordinate system visibility one thing that i strongly recommend when you are working in mold design always make the screen as easy to read as possible it's really easy to make the screen cluttered also i'll talk about renaming your different objects in the model tree as well so here i'm using uniform offsets of 30. i tend to not like that because now we have weird dimensions for the workpiece i like to have something that's a little more normal so let's see instead of this 117 value let's use 120 for the x direction let me make this a little smaller 80 and then for the positive z for the cavity let's make that a little smaller and same for the minus z a little smaller is fine with me let's hit the preview button and that looks like a darn good work piece to me i will click the ok button and now you can see the work piece here in the model tree normally the next thing that i would do would be to create my main volume but i'm actually going to do the slider first just because it'll be easier for me to see to create my volume for the sliders i'll go to the mold volume command right now it's in volume split but i want to make sure i'm doing a mold volume and here in the dashboard we have the ability to create a slider and when i click on the slider icon it wants to or excuse me gives me the option to do something called calculate the undercut boundaries based on the pull direction it can figure out where you have undercuts in the model and we have two quilts that are highlighting right here exactly where i would have expected to need some kind of slider and it ended up creating two quilts right now they are excluded i'm going to use the control key to select both and then move them from exclude over to include then we can hit the preview button and there you can see the geometry for it here we have the ability to specify a projection plane let me show you what that does i will use the pick icon to select this surface over here and then when i go to the eyeglasses to preview it you can see that it extends that undercut to the reference surface but i don't want that because i'm actually going to create an extrude that's going to be a little bigger than that that's kind of small for the slider so let me remove the projection plane now if i hit the eyeglasses you can see that it's only the undercut volume i like that let's hit the check mark and so i've got my slider volume created in the model tree but you'll notice i'm still in the edit mold volume dashboard from here i can create a new sketch i'm going to select on this surface to sketch right now it's suggesting that bottom surface to face the bottom of the screen that is fine i will click on the sketch button to go into sketch mode and for my sketch references i'm going to grab the edges of that undercut volume i can hold down the right mouse button to get to my sketch references dialog box right now i've got a couple suggestions from creole parametric but i'm not going to use them because i'm going to use the edges to select them i need to query select which is tapping the right mouse button so i can grab them because right now my work piece is in the way let's hit the solve button and then close out of there let me go to my sketch view and you can see the references that i have for my geometry let's see i can get to the rectangle command from the right mouse button menu and let me sketch and try to make sure that i'm not going to lock into any unnecessary geometry yeah about that size looks good let's see let's change this dimension here 2.5 sounds good to me this one let's make this one a little wider let's use a value of 5. let's create a couple other additional dimensions let's use a value let's see from here to here i will also use a value of 5 and let's use a dimension from this sketch reference to this over here middle mouse button let's use a value of 5 once more i just want to make a little bit bigger than the actual undercut itself i'm happy with the sketch i can use the right mouse button to get to the green check mark to save the sketch and exit and so there i have my sketch now i can use the extrude command from the edit mold volume dashboard let's flip the direction and then i can right click over the depth drag handle to change this to to selected and i'll pick the surface of that undercut that's good and right now you can see that it's actually going to be interfering with the model a little bit but that's okay because i am going to create my automatic volume with a reference part cut out in a moment let's hit the check mark over here i'm going to deselect everything because i always like to change the names of the volumes let me go to the properties icon right now it is calling this mold volume one this is going to be my slider volume which i'll call it and i set my initial slider volume it's not going to be the final one let me just call it initial just so i can keep track of it and also let me change the names of some of these features so that i or someone else will not be confused later on when they are trying to understand my design intent and for this first slide or volume that's where i did the calculate undercut boundaries or i just like to call it cub all right so we've got our first volume created and i'm going to hide it because i don't need it at the moment now let's create a oh i didn't hit the check mark let's hit the check mark to complete the first mold volume now i can create my second mold volume let's go to the mold volume command this one will be an automatic volume i'll grab the top surface of the work piece you can see the drag handles if you want to make that volume bigger or smaller i'll use the control key to grab the side surface which grabs all four side surfaces and i always grab wait i'm confused how am i looking at this let me use the control key to grab this surface as well just to make sure that it is selected so that is my automatic volume if i go to the properties here that's what's going to call it i'm fine with that so there i have my automatic volume now i'm going to do the reference part cutout i will click on this command and it takes a look at the reference part and subtracts it from the current mold volume let me deselect everything and once again i will go to my properties i'm going to call this my main volume initial because later on i'm going to subtract stuff from it let's hit the check mark to complete that one all right so now that i have those two volumes created the next thing i'm going to concentrate on is going to be my parting line and parting surface let me turn off the display of the automatic volume so i can see inside of here and i still have the slider volume hidden again just make things easy to understand all right to create a parting line i'm going to use the silhouette curve command i'll click on this command and you can see that it finds all the different outsides of the part with respect to the pull direction via silhouette but it's also giving me some of the entities for the slider i do not need those let's take a look at this dashboard let me collapse the model tree navigator for a moment here's the references tab so automatically uses the surfaces of all bodies here's where you could do slide volumes inside of here here's this other option for gap closure here's where we have loop selection and you can figure out which of these objects correspond to the different things in here based on just moving your mouse over them you can see what is highlighting on the computer screen and based on the projection of this part it came up with 19 different loops mainly because they're all those little holes over here see these holes here you and just hover over them you can see how they're highlighting in sort of a greenish color as i'm doing that and so as i hover over these different ones let's see which one there it is loop number four is the one that deals with the sliders if i click on the word include i get a drop down list that allows me to change this to exclude and it's still showing them sort of like dashed out where they would be but again i don't need that particular loop over here another thing that you can do is change which side is being used for example if i go to the chains tab over here we've got all these different chains and here we have one this one is single single but some are using upper or lower for example this one here it's using the upper edges of this surface maybe because of how this one is created maybe i want it to be on the lower side instead you can see how it moved that chain from the upper edge to the lower edge see that all right let's go back to lower over here and i think that's everything that i want out of my silhouette curve let me go to the properties let me change this and i like to call it my parting line hit the enter key then hit the check mark now let's bring back the model tree just so you can see how we are currently organized let me zoom out over here now that i have that parting line created from a silhouette curve i'm going to use it for creating a parting surface let's click on the parting surface command be aware that there's also this command here for classify surfaces if you already have some surfaces in your model let's go to parting surface and here we have a number of different options in here like you could create a fill surface here's an extend option let me show you what the extend curves will do i'll click on that and it's automatically using this curve over here if i go to the references tab is it's in red it wants to know what the boundary reference is i can pick the work piece you can see how it takes those different edges of the part and just extends it out to the boundaries of the workpiece but that is not what i want because i created that parting line and i wanted to use it for making the other portions of the surface so in order to use that particular command yes i really do want to cancel let me go to the surfacing overflow menu and here's command for skirt surface this one is really nice the only thing is look at this this is a model dialog box this is the main way that features were created back in pro engineer 2001 and earlier for whatever reason ptc has decided not to update this command but let's take a look at it the way that these old interfaces work is that you have these elements up here with a status column and then these action buttons and you also want to pay a lot of attention to the message area right now it's prompted me to select or excuse me specify boundary reference which may be the work piece mold volume or mold component well in this case i am going to use the work piece which is the same size then it's prompted me to select a feature containing curves hey guess what that parting line that i created is a feature that contains curves i'll select it one thing about the old interface you're always using menu managers and hitting done and done return out of there so now i filled in this information oh yeah another thing about the old interface is that you did not get an automatic preview that was one of the best things to come about with wildfire 1.0 as you're creating features they were being previewed to you oops trying to slide things here and so now you can see what my parting surface looks like and that looks wonderful there's a bunch of other different options here in another set of videos i'll show using some of the options like the shut off extent and maybe even draft angle stuff like that but this is good let's click the ok button and here i have my skirt surface i'm going to rename this and call it my parting surface again just to help keep everything organized so i am happy with that parting surface all right so now i am ready to start doing some subtraction and for doing the subtraction i don't need the parting surface first i'm going to take out the slider so let me hide the parting surface and let me find my slider volume and show it and oh you know what i forgot to finish up this parting surface let me hit the check mark out of there it's always weird that the dashboard stays open even though the object is in the model tree but hey all you have to do is hit the green check mark all right so let's see now i'm going to start doing some splits let me go to the mold volume drop down here we have the volume split and for the volume that i'm going to split let me see if i can grab the automatic volume yep there it is right out of the model tree but the weird thing is for the references that you want to use for the split surfaces you have to select it in the graphics area because these are surface references they're not a feature reference and here is where i'm going to select that slider volume that i just made visible all right creo parametric did some thinking now i can go to the volumes tab and we have two different volumes over here i'll click volume one and it's highlighting the main volume that has had the slider subtracted from it here's volume 2 which is just the slider itself and i'm going to rename this this is going to be my slider volume final that's what i'm going to use to create a component after i do the next split let's go to volume one and this is sort of like an intermediate volume we call it main volume intermediate can i spell today enter me d it and hit the enter key all right that's good let's hit the check mark out of here and now i can see the new main volume over here let me go back to this particular one let's hide it and let's see let me go to my parting surface and make it visible now let's do another split let me go to the volume split command this time i'm going to split this intermediate volume and for my split surfaces i'm going to use the skirt over here creole parametric is doing some thinking and it highlights the two other new volumes let's go to the volume here and here this particular one this is going to be my core let me call this what do i want to call it i'm going to call this my camera core final i like to be consistent in my naming so when i'm creating components i know what i want to use and this one is going to be the cavity camera cavity final and hit the enter key that's good let us hit the check mark and i've done my different splits i've got a bunch of different volumes visible on the computer screen it is starting to get confusing but the nice thing is when i extract my mold components it is going to automatically hide a bunch of different things and so here i have the different objects i just want to use the camera cavity final the camera core final and the slider volume final let me expand advanced and right now it is not using a default template for any of these parts let me select all and then use copy from and it goes to the folder where i have all my different default templates let me use my company's start part that is metric and set up for model based definition there you can see it's being used and let's rename some of these different parts here so this is going to be called cavity camera cavity final actually i'm fine with that name and camera core final let me call this my camera mold slider and hit the enter key and so that is oops and that was the common name let me call this the camera slider let me camera mold slider and i don't care about entering in a common name you should care but i don't all right so that looks good let's hit the ok button over there and now it's creating the individual parts you see stuff changing color on the computer screen let's now just make sure that anything that needs to be hidden is hidden let me go back over here and hide that one and so there you can see the different parts that we have let me see i can hide the parting line hide my parting surface and let me go to the view tab and be sure to save status so that when i save this model it remembers what i want visible and not visible next step that i'm going to take let's create the molding which is going to be the part that is going to be the result of this mobile design and for the name of the part let me call this my camera molding and i can enter in a common name if i want there you can see a preview of the geometry all right let's do a mold opening see what all this stuff looks like i will click on the mold opening command this is going to bring open the menu manager let's define a step and then define a move and the first thing i will do is grab the slider part and then you can hit ok or middle mouse button and now it's prompt me to select a direction i'll pick this surface over here let's use a value of 100 and then i can hit done beware you can also do a draft check and interference check as you're doing this so there is the slider let's define another step define a move this time i will grab the cavity and hit the middle mouse button because that's the only component i'm going to move now it's prompted me to select a direction let's pick that surface and go up a distance of 100 and then i can hit done or the enter key and it moves that component up oh my workpiece is still visible let me see if i can hide it there we go uh let's see next step and let me hide the reference model as well there we go when you see stippling on the computer screen that's how you know that you have multiple objects on top of each other let's define our final step define and move for this component okay and for the direction i'm going to tap the right mouse button to get to that surface i prefer to use surfaces let's use a value of 100 and then hit done out of here so there you can see the different components that i am using for defining the mold to generate this particular part let's take a look at them real quickly in their own separate windows here we have our slider part and that's what it will look like let's close out of here then let's grab our cavity take a look at it in its own separate window let's rotate this model and there you can see that just looks fantastic let's go back to the mold window let's grab the core and open that look at this look at this this is this is just a work of art all right let's close out of there and go back to the mold opening command to see the final result that we have over here and so that is how you can use the mold design module in order to create a mold with a core cavity and a slider i hope you enjoyed this video for more information please visit www.creowindchill.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: 8,168

Keywords: creo parametric, ptc creo, creo ptc, creo parametric 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 parametric 6.0, creo parametric 6.0 tutorial, creo parametric 7.0, creo parametric 7.0 tutorial

Id: rvMwe4hj2PY

Length: 31min 30sec (1890 seconds)

Published: Mon Dec 07 2020