Autodesk Inventor Multibody Environment - Digging Deeper

and everyone my name is Dave Weitz liang technical director of envisage UK limited and welcome to another of our Friday morning webcasts the subject of this particular webcast is multi body modeling with an inventor I'm going to dig a bit deeper into it this time and may go over half an hour but only just hopefully this is based on inventor 2013 those of you who have got 2013 will hopefully notice new interface and new functionality I'm particularly I'm going to work entirely on multi body modeling I'm going to use two examples the first one is it's an electrical arrestor for a high tension power line it's made up of some plastic components some aluminium parts a ceramic disc and also it's filled with a part potting compound so it's actually filled with a liquid plastic or resin and I want to model this now what I've got here is I've got a part file now all but a multi body modeling is done within a single part on this particular part file contains two sketches I've turned the dimensions off at the moment but you'll see I've got two sketches in two different work planes you don't have to you can work from one sketch should you wish the whole idea is that I'm going to create a pseudo assembly if you like within this part file so the first thing I'm going to do is let's explain what we've got here first I've got a steel bracket a steel plate these will be bolted through I've got a ceramic disc I've got a piece of stud here I've got a plastic molding that I'm going to revolve and this area here is the is where the resin will be and the line there is the height at which I want the resin to fill so there's quite a lot here and to actually model this is separate parts would take a while and obviously then you've got to assemble it together and also if you change any sizes what happens if with the assembly should you change sizes because I'm working in a single part file all the dimensions can see each other all the geometry can see it see each other and I'm working within a single part file where all the parameters are available to me so it's a much easier way of working with a with an assembly within the part file those of you who've used invent in the past this will be alien to you but just think of this as a part file containing a pseudo assembly we'll worry about how it becomes an assembly later on so let's start working on this let's extrude the plate first of all so we'll just take the go to extrude I'll use the old dialog box so you can see more of what's going on and we'll take a profile here an extruded midplane I'll measure this off of the geometry I've got already and that'll produce the extrusion for me so that's my first part created we'll just turn the visibility of the sketch back on again and the next thing we'll do is create let's revolve the ceramic disk so we're going to revolve take the profile for the rectangle that represents this disk an axis to do the revolve now if we leave it like this as per a default in inventor Park modeling this will actually join this rotation to the previous part now I actually want this to be a new solid within my part file so within the boolean buttons that you get on revolve and extrude you've got a new button bottom now that says that is entitled a new solid if I click on that what you don't actually do is it will create this revolve and create a new solid body from that revolve and if you notice in the browser you've gone you a solid bodies folder that time's the solid bodies that are actually being created I would suggest you rename these because these will eventually become the part files within the assembly so rename these it'll save you a lot of time later on okay so let's just carry on very quickly on these we want revolve for the threaded stud again remember to add it as a new solid if you forget and do a join you can always go back to the feature and change it to a new solid later on anyway so you haven't got a problem there and we're sequentially modeling so it's listed as per normal in the browser but you'll notice that if you go and to one of the solid bodies within the solid bodies folder and expand that particular part out it will actually show you the features or feature that make up that particular solid body so you can if you want to on large part files we've got a lot of features in there you can actually expand the part out and see what it's actually made of in the browser so we're just rename this one then we'll move swiftly on with the others so we're building up these this multi body modeling model as we go let's just do the plastic component here those of you shrewd enough will notice that actually this will intersect with the stud at the moment there's no hole in this we'll worry about that in a minute again this is a new solid body this term it's called a casing but I'll actually turn the visibility off we can actually what you can do on these separate solids is turn the visibility on or off you can also change the properties you can't change the material properties only the colors the material properties you would change when you export it out as an assembly but let's just call this black cast then the the resin so we revolve the resin luckily it's found the rectangle where the disc was so we've got a little less work to do later on but it's still going to intersect with the plate and the stud again this is a new solid body and we'll just change we'll call that resonant and change the properties of that one as well the only reason why I'm changing the properties it's just a little bit easier to distinguish the parts when you're working on the on this multi body part you can change all this later when they become parts in their own right within assemblies and last but not least on this we'll do this final great so extrude this mid plane will measure the distance from another sketch because I need to do as a new solid body try again there we go okay so we've got our components here now we need to do a bit of boolean work on these models so for instance if we take a look to look at the resin this plate is interfering with the resin the stud at the end is interfering with the resin so we need to do a bit of work on this within the 3d model tab of inventor 2013 we need to go to the modify part of the ribbon this is compressed a little bit because of the rest of the resolution of our screen but we're looking for combine and what combined does it lets you do cuts or joins or intersects between two solid bodies within your part file so the base solid in this case is going to be the resin I'm going to choose to count and I'm going to cut with a tool body which is this plate here and I'm going to keep that tool body if I don't it'll actually delete that's all body click on okay it turns off the visibility of that plate or tool body to show us what's actually happening if I just zoom in on here you'll notice that it's now cut out the resin what I do is I just put a 1/2 view on here so you can see what's going on just put it out slightly okay and last but not least the stud work so just go back to that do another combine choose cut the base again is going to be the res in the tool body is the stud at the end here keep that okay on that and that's now cut out the stud work so what we can very very quickly do here is using the tools that we have in multi body modeling within the single part file were able to count one part from another and produce in this case the resin that's going to flow around the component or the components and of course from here I can work out the volume of this so that we can get the material quantities right so let's turn the visibility of these back on again well I will leave the a few on at the moment we'll just finish off this start here so let's take a sham from there and a thread choose ohm6 on this one and give it a thread length of 10 millimeters okay so there's our multi body model if I just finish off the section view you'll notice now we've got a complete pseudo assembly I just want to finish off by adding a hole between these plates it's important to note that within multi body modeling you are working on solids within this part file so when I drill a hole if I just create a sketch on this plate here I'm going to project some geometry from the back as well so that I can get the mid point between these two overlapping plates I'm able to project geometry from other parts within other solids within this part file so now I can just add a construction line between these two lines but my point on the midplane on the midpoint here I know that the hole is going to be in the middle now so when I drill my hole what's going to happen well if I drill the hole the hole we can pick up on this point tell me what size we want and tell it to drill through all now you got to be careful here because when you drill through all what's actually happening is it's only drilling through the solid body that you're sketching on you see the solid body that's highlighted in magenta or dotted magenta line type that hole is only drilling through that so in the dialogue boxes you will occasionally see a solids button this enables you to select other solids within this part file and in this case I want to select the plate at the back so the hole is drilled through both of these plates if you don't do that the whole line you drill through the plate that you actually sketched on okay so that's everything finished now we've got to get this out to an assembly and to do that we go to manage and make components from here we select the solids from our multi body parts that going out to the assembly the assembly by default will take the same the assembly that you're actually putting these into will take the same name as the part file so when you're creating your part file it's a good idea to give that the same name as the assembly or that the assembly will be given we got to next what this will now do is it will give us a list of the solid bodies that you've named originally in the part file it will give you a list then of the components that are going to be created you'll notice it takes the solid bodies name you can edit these here should you wish and then the templates now what I'm going to do here is the plate so I'm actually going to use a sheet metal template save me time later because I may want to do more work on the sheet metal when this goes out to an assembly you can scale as well this is quite useful if you're doing molds or anything like that way you need to scale this as it goes out to the assembly for shrinkage purposes click on OK this will then create an assembly containing all the part files that we've just produced as solids within a multi body part okay so now we have our assembly I can do further work on this so for instance well first of all let's look at the browser you notice everything is grounded we don't have to assemble these parts they're assembled in relationship to the multi body part that we created earlier so everything's grounded we don't have to do any work there you can unground them if you wish and reassemble later it's not a problem let's take this plate if I edit this because this was then created using a sheetmetal template I can actually go to the sheetmetal defaults here tell it this this is actually this was 2 mil thick I know I can do a further sheetmetal work on here so for instance I could actually add some bends to this component returned a lot I could do the same to the other plate should I wish let's go ahead and do that so we'll take that plate edit that one go to the sheetmetal defaults this was 2 millimeters thick as well it's important to give this the correct sheetmetal thickness if you are using sheet metal templates because in a minute I'll explain or dig a bit deeper in the properties that we're having produced by multi body models and then finally a word of warning really more than anything else these are all derived components all right so what's actually happening to these parts is if I just double click on one the stud for instance you'll notice that it's actually a derived component coming from the original multi body part so there's no features in this yet you can have features later should you wish like I have done with the bends on the part but they are not they are derived components they are coming through from the original multi body parts and are associative all these are associative to the multi body parts if we change the original part all this changes as well so a tip really first of all is if you want to find out what the multi body part is and you look at this assembly somebody else may have created this and look at these and thinking on these are all grounded so it gives you a clue that this is actually coming from a multi body part if you edit one of these it will show you then that it's actually a derived component coming from a particular part file you can then right-click on that and then you can open up that base component and that will then send you to the original multi body part that you can then edit and then update this afterwards we'll look at that later when it comes to things like bolted connections you need to be careful because let's just say this assembly you need to be careful because these aren't seen as holes because these are derived components there's no intelligence as such when it comes to holes so when we add Bolton connections you can't use by hole I would suggest to use concentric and if we then choose our start plane the circular reference the termination it will then be able to produce our fast and fast notes but one in so really the best way of working with this is correctly holes in the multi body model and friends as well remembering to set the solids as you go as I showed you earlier and then when we come to add our fasteners when we do a Bolton connection just remember that right sizing here you can't use by hole as a reference okay and then barb ulti connection in so usually I use the concentric option when you put voltage connections in okay so that's our assembly if we go back to our original part file and change this in some way let's go back to the original sketch let's change the depth of the resin so we just change the value of that so if that's put the depth of the resin up another 10 millimeters but it's a sketch the model will then change accordingly this is the multi body part so that will change accordingly and then we go to the assembly update the assembly then everything's updated in this within this assembly so that's the way to work with multi body parts what I'm going to do now is we'll look at another way of working so that's working with sketches within multi body parts initially what we're going to do here is have a look at something that I saw the other day that might be of interest where we we were looking at creating a mold now this is a part of your polyurethane component and we've got a part file that we've designed already and I want to stick this is quite large and semicircular polyurethane component that we want to make a mold for so I've got the part here initially and what I want to do is clad this with steel work and a plate so that we come in we can then inject the polyurethane foam within this mold so I can work from this part file and literally what you're doing really is working on the part so for instance I can sketch on this face here and perhaps put a piece of piping in here mr. steel pipe in for instance to help me produce a mold for this foam once I've got that sketch I can then extrude it extrude the profile again remembering to tell it that this is a new solid and because I can see everything else within this part file I can they'll tell it to actually extremely to face at the top here and that will correct me a new solid these changes properties and we worked like this as we clad this assembly the changes material okay and we work around this component buildings new solids as we go and then eventually we're going to get to something that looks a little bit like this so this is the multi body part where we've cleared it with steel work so we've got a number of solid bodies I've put the lid on yet but this is the steel work that we then weld together to make the mold for this polyurethane foam component I would have modeled the polyurethane foam apart scaled already so I may well have derived this so that I'm allowing for shrinkage remember these shrink so the mold needs to be a slightly bigger so you probably want to scale the part before you start working on the multi body part and then from this we've got the assembly now a word of warning here because these are because we're working on a single part initially the multi body part I can bring the properties across but things like length width and thickness aren't really much use to me because I was working on a single part and all these components might have different thicknesses and different and they will have different lengths and widths so if you wanted to put cutting lists out for your parts list your bill of materials and parts list it is important to actually get the information on the parts as they arrive in the assembly don't do all the work in the part file so on the assembly for instance if we take this plate I've already added some sketches to this plate which have created for the visibility in the zone I've created some sketches on this part after they've arrived in the assembly and then if we go to the the parameters what I've done is these reference dimensions that we've added because these parts are already designed and they're from a derived components the only thing you can actually do is add reference dimensions to these models so these are actually reference dimensions the part is driven obviously by the multi body part so all I can do is add reference dimensions so these also add their sketch to the side to get the thickness now a tip from me is use these parameters G underscore L capital letters for length width the width and thickness with the capital T for the thickness the reason why I do this is that if you work with sheet metal the thickness of the sheet metal part is always thickness with the capital T so we might not carry on with that throughout the assembly do you understand for steelworks if you is anything in the frame generator in Inventor the length is available to you as GE underscore L so that's what I'm using throughout my parts in my assemblies now I always use these parameters it's a good tip to work with so if I'm using sheet metal parts or still work or box section or anything like that these parameters will come across automatically in this instance because I'm at because this is a plate the only thing really I could have used from here is thickness if I had actually made that as a sheet metal part I didn't in this case so I had to add a dimension the reference dimension of the thickness remember to export these as well in the export column so they become available to you not only in the properties as custom properties all right they also are available to you in the Bill of Materials so that when we go into the Bill of Materials for this assembly these properties parameters are coming through as GM escorial width and thickness okay when we then create the drawing of these parts and bring a parts listing we can then pull across those parameters now what I've done in this case is I've actually corrected myself a class list style and the parts list style I've actually renamed you underscore L to length but in this way if you used you underscore L for the length width will be a name parameter that you create thickness as you would use in sheet metal then no matter what component you bring through whether it's box section sheet metal part or an hour component new designed you're going to get them in the correct columns so digging a bit deeper in in Inventor not only for multi body modeling this is a tip that can be used with just about anything that you work in in Inventor use these particular parameters so obviously the last thing we need to look at is what happens if we change component so let's go back to our original multi body part and we'll just change the sketch for this foam cars dimension we update the part that updates the assembly notice how quick it updates everything because you've modeled in a single part file everything updates extremely quickly then all you've got to do is go to the assembly and just do an update on the assembly and that updates all advanced so a very very fast way of working it's it's a must really if you're you're able to work from either single sketches or a single part file the the arrests are for instance was just a single there was two sketches it could just be a single sketch but multi body modeling is a superb way of working with you ideas of this tooling especially anything to do with wood timber excellent use of multi body modeling very very fast you're going to get the components out a lot quicker and of course there's a single part file that you go to to change everything you haven't got to remember to go to various parts within an assembly to update a most importantly of course within assemblies we're not using adaptive modeling which can slow an assembly down this is an extremely fast way of working so to that end I'll finish the webcast thank you very much for attending and hopefully speak to you again next week for the next one have a good weekend thank you very much

Channel: Dave Whiteley

Views: 9,739

Keywords: Autodesk, Inventor, 2013, MultiBody, Modelling, environment, cad, 3d

Id: hMISFIaDdPQ

Length: 29min 24sec (1764 seconds)

Published: Fri Jun 15 2012