Creo Parametric 7.0 - Multibody Modeling (Part II)

the introduction of multi body modeling was one of the biggest enhancements to creo parametric 7.0 in a previous video I showed some of the basics of multi body modeling in this video we'll continue the exploration here I have a part and I used a single sketch in order to create five different extrudes in all those extrudes are their own individual bodies let me show you some of the effects of creating additional features let's say I want to create a whole and I'm going to create a whole in such a way that it is going to potentially intersect multiple bodies let's place it on this surface over here let me change to my offset references collector I'm gonna say that I'm going to dimension from this surface here let's hold down the control key and select this other surface over there let's see some of the different dimensions that we have on here let's try changing this offset dimension to 0.5 and this one should be a value of 6 just trying to put it in the middle of a bunch of different features and we have our depth drag handle let me right click on this and change this to through all if I go to the body options tab you'll notice how for some reason right now it just has selected body 5 it's only going through the part that it was initially placed on even though I have a thru all depth I can change this to all and in this way the whole would affect all the other individual bodies here you can see that we've got hole 1 in their body 2 isn't intersected so it doesn't have it so that's how you can control the extent of other different engineering features like holes but other ones in here do not support having multiple bodies so for example let's say that I go to create a round I will select an edge over here here we have the round tool from the mini toolbar and I'll drag this out let's change the dimension to make it big enough for you to see there we have our radius on here but there's nothing in here that allows you to control which bodies it is going to affect around is only going to a act the body on which it is placed can't have multi bodies involved in that so that applies to rounds and chamfers next let's take a look at what's called removing a body I have body four over here if I click on it from the mini toolbar I can choose to hide it if I don't want to see it let's bring it back for a moment you also have options to set it as construction so that it won't be contributing to your mass properties also you could use it to filter it out of a bill of materials but there is another option in here actually before we talk about that one you also have the ability to delete the body if I right-click on it sometimes though you don't have the ability to delete because there's geometry and features that are contributing to it so instead of deleting you can remove the body and that will consume it so when I choose to remove body we're going to get a dashboard here for a remove body feature you'll notice that shows what it's going to remove from here from the references tab you can choose additional bodies to remove but I'm going to click the checkmark in order to take it out of here and now we have that remove body feature and body for no longer appears in the list let's take a look at some of the model tree options that you have now if I go to the settings drop down I can choose tree filters and right now we have this new body tab for features types and consumed bodies are not displayed in the model tree let's hit the checkmark and then click the ok button and so now we do see body for and one thing to note is that these different bodies have different symbols based on their various different types sometimes so they look pretty close to each other but you know other times it's just really hard to tell so for example if I select say body 3 over here right click and then set as construction you'll see that again it has a slightly different symbol let me go to magnifier so there we have a construction body and there we have a consumed body and then we have our active body let's turn off the magnifier and then I'm gonna go back to body three over here and unset - construction so it becomes a regular body instead in addition to displaying consumed features in the model tree you have the ability to display additional columns of information and actually before I do that let's take one of our bodies and convert it to sheet metal to do that first of all that will help me if I hide some of these other different bodies in here okay so this first body I'm going to convert to sheet metal let's go to body right click and then convert to sheet metal from the references tab we need to select the driving surface and for the thickness right now it's using a thickness of 1 which is kind of ridiculous for sheet metal but let's just go with it and then bring the other bodies back display display display and the interesting thing is for some reason it brought back my feature number and future ID columns now let's display some of the other different columns that we have so I'll go to and actually I think this is the Tools drop-down not the settings drop-down as I mentioned a moment ago let's go to tree columns and get rid of some of the columns that are displayed in here under the info type we now have some additional columns that we can add in here related to body so we could choose contributing contributed body and also body category to be displayed in here let's click the ok button and so now I can see that we have information here so for example here in body one these are the different features that contribute to it but again we can see for the different extrudes and the different sections which bodies they contribute to and so for example this whole actually affects four different bodies in here so that sweat list multiple different bodies for body category there are four different types of body categories you have the basic solid which represents bodies two three and five and then we have over here sheet metal listed as well we go back to my tree filters interestingly consumed bodies went away there we have body four brought back in here so there we have our sheet metal our basic body the other two different kinds of body categories that you have our lattice for additive manufacturing and generated for bodies that are created as a result of generative design so there you have the additional information that you can display inside of here now I created a remove body feature and now this is showing up as a consumed body if I go back to the remove body feature and then right-click on it and choose delete and then get rid of that remove body feature now this is no longer a consumed body the symbol changed in the bodies folder to indicate it is the same kind of basic solid as the other ones next up let's take a look at three new config dot Pro options related to multi body so I'll go to file options configuration editor let's click the find button the first one I'm gonna search on is under a keyword boolean and hit the enter key there's this option boolean default operation and the default value is model-type if I go to the drop-down list you can see that there are four other options for this config dot Pro option the default for boolean operations can be add bodies merge cut or intersect but the default value is model-type which means that the actual default boolean operation will depend on whether you have a part or an assembly now if you take a look at the description in here and then I'll go back to the drop down if you have an assembly and you're creating a boolean operation the default operation that's going to choose is going to be a merge if you have a part the default boolean operation is going to be to add bodies but you can also cut or intersect and again this is just the default operation when you are performing a boolean operation when you're performing a boolean operation you can change within the tool what kind of operation that you're doing so for example I choose hey let's select body five over here and then I select that I want to do a body merge while I'm inside of here I can change this to an intersect to subtract whatever for boolean operations same thing in the let's activate when these other bodies over here oh actually let's go to the models have here's where I have my boolean operations command again you can change what is going to be your default what kind of operation that you are performing when you are inside of boolean operations the next new config dot Pro option let's go to file options configuration editor this time I'm going to do a find on a keyword let's use multi there is an option enable multi material body the default value is yes in other words each body can have its own individual material but for whatever reason if you didn't want that you could change that option to no so that you could not have different materials for different bodies and the last option that we will take a look at let's search on interference this one is related to visualization here we have this new option HLR which stands for hidden line removal advanced interference check for parts and what this means is the default value is yes so it's going to do a better check a more advanced check more accurate check on hidden lines for removal in a part when you are using that display mode the thing about this option as it notes in here is that the default value results in slower performance so you could turn off this advanced interference check for hidden line removal if you wanted better performance from your computer and updating on the computer screen the last new thing to mention for now for multi body modeling is a new option for exporting models in a previous video I showed if you go to file options and then data exchange and your different import profiles you have the ability to import multiple bodies in a part in your import profiles but also for your export profiles you can choose whether or not you want to export construction geometry if I go into my step export settings here we have construction bodies are automatically set to be exported when you export a step file but if you have those construction bodies that resulted in your part and you don't want those to be exported you can control their export by turning off this option for construction bodies I hope you enjoyed this video for more information please visit WWE windchill comm if you learned something from this video please give it a thumbs up and if you like this video please click the subscribe button to be informed when new videos are uploaded thank you very much

Channel: Creo Parametric

Views: 2,577

Keywords: creo parametric, ptc creo, creo ptc, creo parametric tutorial, creo parametric 5.0, creo parametric 6.0, creo 7, ptc creo 7, creo parametric 7, creo parametric 7.0, creo parametric 7.0 tutorial, creo parametric 7.0 multibody, multibody in creo, creo 7 multibody

Id: 59_4B6BMafU

Length: 12min 42sec (762 seconds)

Published: Tue Apr 21 2020