Creo Parametric - Mold Design | Complicated Showerhead Mold (Video 1 of 5)

in creole parametric you can perform mold design that's coming up with the manufacturing components necessary to create a component using an injection molding process we're going to take a look at doing it for a very complicated part this showerhead component over here if you have traveled in hotels in the united states in the past 10 years or so you have most likely seen this component as part of a shower head you can see it's got some complexity with the geometry that's going to result in a little bit more of a complicated process in order to manufacture this and this is actually going to be the first of five videos rather than just jumping into the manufacturing process i want to explain what's going to happen over the course of these next videos here is a completed version of the mold casting for the part so in this first video we are going to start off the mold manufacturing model we're going to assemble the reference model create a workpiece and then we're going to create some supplemental geometry let me explain why let me go back to the model tree and i'm going to find the parting surface that we're going to use this is the parting surface that we're going to create in order to have a custom parting line to separate the core from the cavity so there's going to be some planes that we need to create we're going to need to create a curve for shut off for this and i'll explain that in a later video but we'll create that reference geometry in this particular video in this video we'll finish off with defining the mold volume using the automatic option and then doing a reference part cutout then in the second video we will define the inserts that are necessary for example we are going to create a plug up here and we we're going to create a couple of sliders the sliders are going to account for some undercuts in the model let me go back to the parting surface and hide it if i zoom in over here hey here's a little heads up there are some undercuts necessary in this particular model and then in the third video we will create the parting line and the parting surface then in the fourth video we'll create the splits between the automatic volume and the plug in the inserts and the core in the cavity and we will create the mode components and then in the fifth and final video we will create the molding and also do the mold opening analysis which you see right here so that's the process that we're going to go through also i want to mention that these videos are based off of a demonstration that ptc used to do for the mole design and cnc manufacturing packages it was called art to part and that was from back in wildfire 2.0 or so it's just got a high level of complexity which is why i'm going to show it here okay so we're starting out with our part first off let's create our new manufacturing model i will click on the new button and let's change the type to manufacturing the subtype will be mold cavity and i will call this the name of the part dash mold casting use your company standard be aware that this file is going to have a dot asm extension back in the day they used to have a dot mfg extension so you might still see some old manufacturing mold cavity models with that dot mfg extension you can enter in a common name if you want here's where we can choose a default template i'm happy with the one that ptc supplies and that default template from ptc gives you three default datum planes and a default coordinate system let's turn on the display of those different entities also if you take a look in the graphics area we have a symbol that indicates the pull direction for the model now that we have our model started out let's bring in our reference model if you go to the drop down list there are a few different options in here i'm going to use the locate reference model option and when i click on that command it opens up a dialog box let's grab the part that we want to use and here we have a dialog box that gives us a few different options we can choose the same model i never use that you could also merge by reference that's probably the option that i use the most in this particular case i'm going to use inherited because there is a datum plane from the reference model that i need to use later on if i use merge by reference i'm not going to have access to that datum plane and that data plane is going to be necessary for creating the parting surface just a bit of a heads up here we have a name for the reference model let's click ok out of here now i can click the preview button and from the preview button based on the pull direction this part is upside down from the way that i want it i need to change the orientation to do that i will click on the pick icon underneath reference model origin and orient it'll open up another window right now i can't see how this is oriented let's change to the dynamic option in the menu manager now i can see how the default workpiece and the coordinate system are oriented z is pointing down so in order to get it to be pointing up let's rotate about the y axis 180 degrees i will choose the y button let's double click in the angle field and enter in a value of 180 hit the enter key and i can see that this repaints and y is now pointing up i like that let's click the ok button out of there and hit preview once more and the pull direction is correct let's click ok i'm just going to use a single layout i'm not going to create multiple of these at the same time now we have a warning that opens it says please confirm setting absolute accuracy to a different value i'm happy with that let's click the ok button and now we have our model oriented let's turn off the display of those different entities for now the next step that we are going to do let's create our workpiece let me hit done return out of the menu manager let's go to the workpiece dropdown you could assemble an existing workpiece if you have one you could create one in here there's an option to mirror an existing part let's use the automatic workpiece option we can change the name if we want here we have our reference model selected it wants to know the mold origin i'm going to use the mold default coordinate system just pick it right out of the model tree then you have your different shapes you could use a rectangle you could use circular stock you could do a custom piece there's a drop down list with a bunch of choices in here you can also change the set of units right now the work piece will be sized exactly the same size as a bounding box to hold the reference part i want to make it a little bit bigger to account for these sliders and plugs and just to have some additional volume around it for the core and cavity to be secured here we have our dimensions so the x direction yeah x is sideways maybe i should have done that differently but let's make this bigger like a value of six you can see how the preview updates on the screen for the y value we want this to be a bit longer let's try a value of 10 that's good and now we need to add some height in the positive z direction for the cavity let's pump this up to 3.5 and for the minus z direction for the core let's change this to a value of two everything there looks good you can hit the preview button to see it in the transparent green color that is fine with me let's click the ok button and now we have our workpiece showing up on the screen i had mentioned that for the parting surface that we're going to create i need some additional reference geometry let's make that now first off i mentioned that i used the inheritance method in order to get a datum plane visible let's create a another datum plane right here inside of the reference part here we have the external inheritance feature i happen to know that there is a datum plane that i want to use let me turn on my plane display in the window i need this datum plane later on in order to define some extensions for an automatic skirt surface again i will get into that in the third video in this series but for now i'm just selecting an existing datum plane from the reference model inheritance feature let's create a datum plane right now it's suggesting some offset from there let's change that from offset to through just want to use that datum plane itself and i'm going to rename it to say exactly what it's going to do for me it's going to be used to extend the parting surface i will click the ok button so that is the first reference that i'm creating for something that i will need later on let's close out of the reference model window here we are back into the main window let me reduce my clutter by turning off the display of a couple of datum planes that i do not need in the default template for the manufacturing model we got a datum plane called main parting plane so this is a plane that you could use for parting if you had simple geometry but as i mentioned earlier we're going to make a more complex surface that's going to follow the basic contour of the reference model so i'm going to create a plane for shut off let's select the existing parting plane and then from the mini toolbar i can choose creates another plane let's drag it we're going to have it down here a little bit let's change the dimension to a value that i like that's good now i will click the properties tab and rename this to my shut off plane and then click the ok button there you can see it on the screen now we're going to create a sketch let me go to the sketch tab let me select the datum plane that i just created to sketch on and then for orientation let's have let's see as i orient this i'm going to have this surface face the right side of the computer screen i just know that i want to use this as a sketch reference later on that's why i'm setting up the sketch orientation while i'm here let's rename the sketch and call it the shut off sketch and hit the enter key now go into sketch mode and ah still didn't give me the sketch reference that i wanted let's go to our sketch references for some reason it gave me a coordinate system let me delete out of there delete those references i just want to create my sketch based off of these surfaces so i'm going to select all four of them let's close out of here now i will go to my sketch view and so now this sketch is going to be used for defining a shut off boundary for the parting surface later on again not going to make much sense now i'm just creating some setup geometry you'll see this more in the third video i'm going to sketch a rectangle and let's make it over here and i'm extending it beyond the part but having it go to the inside of the work piece at the front let's change some of these dimensions over here this one's good this one's good and i'll create a couple more dimensions let's dimension from here to here give that a value of one and last one let's dimension from here to here located there with the middle mouse oh i already have that one let's hit the undo button let's see which one do i want let's create a dimension from here to here middle mouse button and give it a value of one so that is good let's hit the check mark to get out of sketch mode so there i have the necessary geometry that i will use later on for setting up my parting surface the last thing that i'm going to do in this video is create the mold volume to do that here we have our mold volume command i will choose mold volume and we can create an automatic volume now it wants me to select surfaces i'll pick this surface here you can see that we get some previews for dragging it let me hold down the control key and grab this surface and i grabbed a bunch more surfaces doesn't look like the bottom surface is selected let's pick that so now those should be all the surfaces necessary to define the volume and it's going to be the same size as my work piece all right everything there looks good let's hit the check mark and now we have the ability to either trim to geometry or do a reference part cutout i'm going to do the reference part cutout to subtract the actual shower head itself there we have our reference part cut out feature everything is good with this mold volume let's hit the check mark lastly let me turn off the datum plane display to show you what we have let me hide that shut off sketch because i'm not going to need it for a while let's hide the reference model and the work piece i'm selecting them with the control key then i can choose hide from the mini toolbar now all that is remaining is the volume the mold volume that we've defined so far let's take a look at a cross section to see exactly what we have i will go to the view tab let me go to the section command and then planar and i'm going to pick this surface and then just drag it through here so you can see how the mold volume looks again it's hollow on the inside because these are surfaces it's interior and it's got the reference part cut out from it let's see what valley should we use for this now let's try value of three oh yeah three is good because i made the x dimension a value of 6 and that gets me halfway through let's rename the cross section in case i want to use this later on and hit the check mark so there is where we are going to end up with this first video where essentially we have our initial mold volume then in the next video we are going to deal with a bunch of our inserts we're going to have a plug up at the top and then a couple of sliders on the sides to deal with the undercuts then in the third video we are going to create our automatic parting line and an automatic parting surface then in the fourth video we will do our splits and create our mold components and in the fifth video we will create the molding and also do the mold opening analysis 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 hit the subscribe button and ring the bell to be informed when new videos are uploaded thank you very much

Channel: Creo Parametric

Views: 3,885

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: 8jRa4mvrF0s

Length: 17min 21sec (1041 seconds)

Published: Tue Jan 26 2021