Product Simulation with Autodesk Nastran: Interpret FEA Results

hello and welcome to this webinar on results interpretation an overview my name is Mike Fiedler I'm a designated support specialist at Autodesk and I'm gonna work with you on today's presentation today we were gonna work with inventor now strand and we'll take a look at some of the tools that are available within the results environment and how you can really investigate the results of your analysis so let's go ahead over to inventor and take a look at what we're going to do today this is the sub-assembly that we are taking our parts from and for the model that we're going to work with today we're going to take a look at the arms and this crossmember here so I've already set that up let me go over to the inventor environment basically I just narrowed it down to this sub assembly and then I've already moved it into the inventor Nash Tran if you need to know how to get there it's from the environments and then you can access Autodesk Inventor - Tran and I've already set up this model and I'll explain what I have done to set it up so the first thing that I did was to find the material the material let me edit this and I want to use a a36 material so let's access the steel ASTM a36 scroll on down the list here there we go and we'll say ok to that and I've already added constraints and you can see I selected these cylindrical regions here and I assigned them pin constraints so the constraint type of pin is selected and I've fixed the radio and I fixed the axial directions and we'll say ok and I did the same thing in two other locations so there's mid-upper which is right here and then we have mid-lower which is here and they're all pen constraints where I allowed the tangential Direction movement and the reason that we have to do three different ones is because whenever you utilize a pen of constraint it's basically saying that we have some sort of bearing or axis that the model we're going to control the radial the axial in the tangential directions right basically these are three different axes if you imagine passing a cylinder through those regions that we have constrained we cannot use the same pin type of constraint for all three of those sets so I had to break them up into again three different applied constraints where the ones that I have chosen all would have the same cylindrical axis but no big deal doesn't take a whole lot of time to set up and then as far as the loads at the front end of this where the bucket would be I applied a minus fifteen thousand pound force load now when I had set this all up we'll take a look at the mesh settings the mesh settings that I did element size of two inch and I just generated the mesh in the settings maybe we could say to project the mid side nodes generate that mesh and now because it is an assembly we also have to worry about the contact so as soon as the mission is done here we'll take a look at that these are all the different contacts that are in the model and if I select one that highlights on the model and I'm leaving it at the default type of contact which is a bonded type of contact and I didn't specify any other parameters so what is controlling that analysis settings and we can take a look at the options tab and on the options tab we can see that it's a default of bonded and then a tolerance that it's using and it says you know if if some nodes or nodes in a surface or within that distance when we go through the the automatic contact to set up the pairs of contacts and what I had envisioned whenever I first ran this analysis was that you know I would just go ahead and run it and then whenever we start the presentation we can jump into the results environment and begin to take a look at the results of our analysis as it turns out this turns out to be a very good example of some issues that you might encounter so if you've gone through the slide deck that accompanies this learning material one of the things that I mentioned is potentially when you're going to review the results you could run into an issue where you don't obtain results on your analysis and that is actually what happens with this particular model as it is so you can see here the nest Ranson failed and there was an error shown there so where is that what I can do if I want to get back to that information I can go to the now strand output tab and you see here that we have a fatal errors an e5 thousand four error and stiffness matrix singular non positive definite and when this error occurs being that it's a fatal error I don't get any results so the goal today is really to focus on our results but with my analysis setup as it is we don't have any results and what I mentioned in these slides whenever you encounter a fatal error of the e5 thousand types generally what you can do or one thing that you can do is to run this as a modal analysis and then in the modal analysis or from the results of the modal analysis usually what you see is that some part moves by itself you know shakes free because it's unconnected to the rest of the geometry so that's typically what you'll see when you have an e 5000 error if you run a modal analysis and so what I did was I selected the analysis you can right click on the analysis and you can say that you want to duplicate the analysis right there so that is what I did let me activate this second analysis of ours and then I just change the analysis type that we're running if I go into normal modes here access normal modes when I access normal modes all I did was or I should say after I duplicated the analysis I access the analysis type and then I just changed it from a linear static to a normal modes or natural frequency analysis now in this one let me say ok to that or cancel out of that I make sure my material set my material set to the same material it does copy over the loads and constraints running a normal modes analysis it isn't going to worry about the loads that's fine we're just looking for the natural frequencies but it's nice that it copies the material it copies over the constraints for me so there shouldn't be anything that I need to do otherwise for the set up what I can do is just go ahead and run the simulation okay so our normal modes analysis is finished let's say ok to that and here's an analysis being that we didn't have any fatal errors an analysis that we can review some results of alright so when we take a look at the results when it comes into the results environment by default the normal modes analysis is going to calculate for me ten different modes and the way we can access the different modes would be from the pulldown menu here and the results of the ribbon bar and when there is an issue with the model in a natural frequency analysis when there is and by issue I mean there's rigid body motion that is something is just translating or rotating about its axis basically unconnected to ultimately they constraints the ground of the model usually what happens is the frequency ends up being zero or very close to zero so in the normal modes analysis when it comes into the results environment it's showing me the last mode that it calculated MO ten which shows me a real frequency of twenty six Hertz but if we look at the first couple modes mode numbers one through five or six or seven in fact the first eight modes are all very low frequency so if I go ahead and I click on mode number one and allow it to show me what that mode shape looks like maybe again we're looking at mode 10 the bending of the arms first bending mode of the arms there you can see in mode number one something that we didn't see in the initial assembly right there's a a cylindrical part here and what we can see is that it's got some translation it's just moving out of the assembly and then I could take a look at mode number two so I can tell okay this part why is that moving it should be connected to the rest of the structure here but it doesn't appear to be and there's the second cylinder or cylindrical part of this assembly and it also is just translating so I can see that I have problems with both of those and then as I go through these different modes here that just kind of confirms what we are seeing but it doesn't hurt to go through the different modes and there's something that I talked about also in the slide deck whenever things are rotating they seem to expand and if we take a look at the displacement what we're probably going to see is some concentric pattern of displacement contours alright so there we could see that so those parts are just rotating so basically at this point I know that at least those two bodies are not connected to the rest of the geometry the contact is not there for those parts so that means that I need to do something to tidy up this model and when we go into what are we on fourth mode here now you can see that they're just basically vibrating free from the rest of the structure so again my constraints are here in this location here in this location here these two parts didn't have any direct constraints on them so the only way that they would be fixed to the rest of the assembly would be through the contact so I need to make sure that whenever I define my contact in this assembly that these two parts are are tied into the rest of it so what I did then was just go ahead and hit return and then again I right clicked on the modal analysis and I I duplicated that so let's go ahead over and take a look at this model and I'll tell you what I did so this one I renamed to modal redo and this is where we start to investigate you know how do we fix this assembly so that those parts are tied into the rest of the structure and basically what I did was I went back to the modeling environment and I hid this arm this pleat metal arm and then I could see where these cylindrical parts were supposed to tie into these gussets here right and then also tie into this bracket here and if we zoom in there hopefully you can see that right there you can see that there is a gap between them so with that gap in there that gap is larger than the tolerance again let me double click on the analysis and go back here to options so this bonded automatic bonded that gets done and this tolerance here is four thousandth of an inch but the diameter of these tubes is smaller than the diameter of these holes that it sits in both in the gussets here in the center and on the end plates if you will so that contact never got added those parts are that well the names of them are PK 40 6.25 o 107 and I also check that out when I was back in the modeling environment and when I came back and I expanded my list of surface contacts I can look down the list here so you can see everything is 40 6.25 zero one and again those individual part numbers are zero zero seven as I scan through this list here they just didn't exist in the list so from the automatic contact they were never picked up again because they were outside the the tolerance of what the program is going to create for contact pairs so what I did was I set up some manual contacts you can just click on manual and I selected the one entity being the cylinder and then for the second entity you know the the surface that I needed it made it to so I went through and I did that for each of those two tubes and if we edit that so you can see there's one of the pair's there's the tube there's the surface that it should be mated to and I used a offset bonded contact and then I gave it a activation distance a tolerance to utilize that is slightly larger than the gap between those two parts and then I did it at this location and then the two end plate locations so for each one of these tubes you have four different locations so that's right there and then the second four for the for the other tube and basically what I would do is I would just you know change my parameters and then keep working with in this particular scenario within this particular analysis until we make sure that our model is all connected so I'll let this analysis run and we'll be able to see the differences in the outcome or the results of this particular modal analysis okay so the normal modes analysis with our additional contacts added in is now completed and we can take a look at the results of that analysis is oome out here a little bit and again we are starting at mood 10 let me go to the pulldown menu and we can see now if we look all the way down the frequencies will be sorted in ascending order so the first mode would be your lowest frequency your second mode you know a little bit higher the same or a little bit higher and so on as you go up through the modes so now we can see that mode number one is the twenty six Hertz which is the same frequency that we saw before for the arm so that's going to be my my first mode now because we eliminated those rigid body modes and when we look at the results of our modal analysis we expect to see more of a global level mode shape versus you know an individual part like we saw before so this tells me that my geometry is now connected together I don't see any parts flying off in the space if we again take a look at our mode shapes Wow I can tell by the frequency that it is connected but you know that gives me some confidence so we can see the first frequency 26 Hertz the second frequency is also 26 very similar frequency so that's just gonna be bending of the other arm I'll just toggle into that and see that so I hadn't intended to necessarily show moto analysis whenever I was first envisioning this particular webinar but it's good that the model ended up doing this so that I could show that moto analysis is a great way to figure out you know potentially where there are parts that if you have a large assembly you may not may not have initially noticed that there were parts that were unconnected so I wasn't the one that constructed this original geometry or you know if I were I certainly would have been aware of that coming into the model setup and I would say it's probably not uncommon that you know somebody provide you with an assembly and says here run this and maybe initially you're just presuming that all the parts are touching but as we know that's not always the case because there you know there could be interference there could be gaps as we saw here because ultimately later it's gonna get welded or maybe some other component gets fit in there some bushings or bearings that that weren't initially included with your model but anyway at this point we know that our assembly is all connected so at that point I'm ready to go back and perform my linear analysis so what I maybe would have done in a normal situation was just gone back to my my linear static analysis and made those changes there but I wanted to preserve that so I could show that to you so what I did was I made another copy of this particular analysis i just right-clicked again and said duplicate and that's that's not a terrible way to approach this and I'll tell you why because when we make a copy of that modal analysis then and I change it back to linear static analysis that carries over the surface contact so you know I added in those eight additional surface contacts and those just get copied over into my linear static analysis so saves me a little bit of work of of having to reset them up so that's a good thing and I'll show you that a moment there we go there's the different surface contacts that I have included there did that kind of quick there you can see the manual surface contacts that we defined versus the rest of the list here was created via the auto option so at this point the fact that my modal analysis runs and all my geometry sticks together if you will or connect it together that tells me that for this linear static analysis everything should just as well stick together and we'll run that and then finally we'll be able to take a look at some results beyond the modal results okay so my linear analysis has completed and we can get into the results environment and begin to take a look at some of the things that we want to take a look out typically once we get into the results environment so as we come into the results environment with a structural analysis the inventor Nash Tran is going to show us stresses and you know that's a decision by the the product team and I think the the thinking there is you know generally people want to come in they very quickly want to see what their stresses are are they below the yield of the material do they have you know high stresses in which case they know they they need to make some sort of change and if I go into the pulldown menu as I just did they're going to stresses I can take a look at the solid one me see so if one bee sees are generally comparable to the yield and yes we can make the the the quickest ershon there or presumption there that you know I'm using an a36 material I see that my stress is here are about six thousand seven hundred roughly we can also see that that's within a launched area might have a bit of a a stress concentration there but I can see that you know I'm well below the yield of this material so that's good but as I mentioned in the slides for this particular learning content was I would propose that one of the first things that you do is take a look at the displacements because the displacements with a linear static analysis we know that we want the displacements to be relatively small and they should be logical as well right so biological and small we'll talk about that a little bit first of all they are small relatively small displacements the overall length of of these arms is roughly about ten feet there's somewhere about four feet between the first and second hole there and then about another six between the the middle hole and the where it would attach to the assembly as a whole so again roughly about ten feet in length and we can see with the given loads again somewhere around fifteen thousand pounds that my displacements are about three thousandths of an inch so nice small displacement so we haven't violated any of the basic presumptions of linear static stress which presumes a small displacement right and you know when I look at the displacements on the geometry the other thing that I see is I have a gradient rate going from a maximum displacement near where my loads are applied down to essentially zero displacement where my constraints are applied so you know that looks good to me too I don't see any one individual part which has some massive displacements on it which would indicate also that it's not connected to the structure if some component was able to just fly off in the space so that tells me that it's that it's all connected together now one of the other things that I mentioned in the slide deck was that by default when we changed to the displacements it's going to show me a total displacement which is a square root sum of the squares of the XY and z components so if you want to look at individual components you can certainly do that so I could take a look at say for instance the X direction along the x axis and because the total is a square root sum of the squares it's always going to be a positive value but when I go to one of these vector components then I'm going to get both positive and negative values so I can see that as I add this force in the minus y direction we have both some positive X movement if you look at the mini axis down here we can see that this end of it is kind of moving in the positive x direction and then the portion of the model are some nodes of the model in this region are moving in the minus X direction so that makes sense given the constraints and the loads that are on the model and with again any of those vector directions you're going to get positive and negative values presuming that the loads and the constraints that you have on the modeler are going to influence the geometry to do that of course if you have something like just a bar and you add constraints at one end and it hence I loaded the other I wouldn't expect the see both positive and negative values along the axis of that bar right so you know just taking a look at the y-direction again we can see that along the back end of it given the pen constraints allowing the rotation that we have the the back end of the arms move in a positive Y direction and then where we have the load we can see that we have a minus y Direction displacement so in this model that doesn't matter too much I just wanted to show you that you can look at you know vector directions and and when that does become important again given the the constraints that you have on it given the loads that you have on the model sometimes it causes these displacements in a certain vector direction and it could be relatively small but in something like say an electronics package where your deflections are coming from thermal expansion or contraction or something with some tight tolerances sometimes the displacement that results could cause some interference maybe we we don't have three thousandths of an inch clearance between this component certainly we do in this you know a front-loader model but in in some other assembly or product you might not have three thousandths clearance before this these nodes would would impact something else so it doesn't hurt to take a look at it and it's certainly doable the other thing that I would say is the one that we didn't explore here if I go to the next one over the pulldown menu if I want to change that from English into units to say something metric if you need to share your results with somebody it works in a different unit system you can very easy easily very quickly toggle it to a different unit system okay so that's enough with the displacements the next thing I wanted to show let's take a look at stresses and now stresses are going to be very similar in that when I go to stress and if I go to the pulldown menu here and I change this to a save one me see stress again the one me see stress is going to be something of a square root sum of the squares type of computation so the results are always going to be positive if we take a look at the lowest one me sees that somewhere right around zero and then my max is going to be six thousand six hundred and ninety seven all right and again that's because of a square root sum of the squares type of solution that it's doing calculation that it's doing but if you take a look at some of the other results that are here say something like a X normal stress so any of the normal stresses or principal stresses are going to yield both positive and negative stresses which would give me an indication of in the case of the solid x normal stress the tensile and the compressive load so here if we zoom in here you can see in the red area 6000 that's in tension and then of course given the load at the end that's going to put these elements into compression and if we take a look corresponding to the blue there I can see I have results that are somewhere around the negative end of the spectrum indicating that those those are in compression so that's maybe a good point or a good time for me to show some things about inquire and results it it's specific locations of the model and there's really two different ways that we can do that so one of the ways that we can do that is by going up to our ribbon bar in the results panel right here there's an icon that says probe and if I go ahead and I select that and I just move over top of the model you can see that the the indicator here is telling me with what the results are so if I just hover there it tells me what the element is that I'm hovering over the result type that I'm looking at is an X normal stress and then what the value is at 3470 and I don't necessarily have to be right over top of an so it can interpolate from the nodes that are around it what the value is at that location and again you can see if I wanted to figure out is it in fact in compression and what is its value it's showing me that it's a minus 3458 in that area right and as I move it around or away from the the elements of compression we can see that value is reducing ultimately until we reach an area where it switches over to elements that are in tension now let me turn off that probe or the other way that you can interrogate is to go up to nodes all right if I right-click on nodes then I can choose query display and then I'm going to move over top of my geometry and the the node query is just going to give me results from nodes so if you're out in space somewhere between a couple nodes it might not give you a result but if you're on a note of the masher you're on one of the mid nodes it'll tell you what the result is at that node you can see that it's telling me specifically specifically the node number the coordinate locations of that node the translate translations of those nodes XYZ and then since we're on a solid x normal stress what the result is at that particular node so that one is is more useful if you're looking at specifically a specific node and and sometimes you know you might have forced a specific location I can go in and I could split a surface to make sure that I have a node in a specific location so if I know for instance that I wanted to get a value here that was maybe I don't know four inches up and four inches over from this hole because we're going to put a stress gauge on there then I could split this surface back in the modeling environment to make sure that I have a node at that specific location and then I could always do a nodal query at that location to figure out what the stresses are and then I can match that up between my finite element analysis and and what the experimental results show me or the physical testing results showed me so two different ways to go about that just wanted to show that as far as other results are concerned you know we took a look at displacement so we took a look at the stresses here I'm not going to go through all the stresses there's quite a large list of them what I will mention is you might also want to take a look at your strains and let me toggle over to a strand result here and go to the pulldown menu for just a second now when I go to strains when I go to the pulldown menu you'll notice that it's it's lacking in options and that's because the program by default doesn't output all the different types of strains should have turned that on but before we ran the analysis but it wasn't on so I did that intentionally so I can show you where that option is let me double click on the analysis type if I do want though the strain output again when I go into my analysis options we can check the box for strain which is not on by default we'll say ok and I do need to run the analysis with that option on so I'll let this analysis run we can take a look at that okay so that analysis is finished and we'll take a look at those results so I wanted to show this because sometimes people go to access the strains as far as interrogating the results of their model and they say how comes I don't have any value here and it's because you need to invoke that option before you run the analysis so pretty simple thing to do it's just a matter of remembering to do it before you run the analysis and then we can access all the different results there so I could take a look at for instance my X normal strains at this point and then everything that we took a look at just a moment ago you can do the same thing with the strains so I could use the probe tool I can go in and I could take a look at the nodal query so on and so forth so make sure that you turn that output on if that is a result of interest what else might we want do it might be interesting to take a look at the support reactions so as far as support reactions go so for instance maybe I'm trying the size the hydraulic cylinder that's going to be utilized that connects between the the main assembly and these connection points here for for lifting this this sub assembly so it's another good thing that I broke up the constraints into three different groups and I named them appropriately so this constraint group was called mid upper middle of the assembly and the upper constraints versus the lower constraints and as far as getting the reaction forces if you right-click what you do is just access SPC summation and you can see that it slicks all the faces that were involved in that constraint group and then it tells me what the total force is at that location 813 and the the loads in the X direction the Y direction is Z direction and likewise I can figure out what the moments are at those locations as well all right so then I could take that information and maybe that's what I utilize this is information to help size what that hydraulic cylinder is going to be and you can also select multiple to so if I select the first one I control select the second one I can do an SPC summation and then you get the total of the upper and the lower ones that I'm using there so in force I'm seeing a total reaction force of 4329 and then the component directions as well so SPC summation is a another good tool that you will probably utilize with some some frequency now the other thing that I won the shows for is interrogating results would be the graphs and as they're called and inventor and Astra and the XY plots but they're probably more interesting as I mentioned in the slides when we have something that is a either a time-dependent analysis such as a transient thermal or if we get into something like a nonlinear analysis where there are steps involved so the load is increased incrementally if you will so right-click on that analysis and we do a duplicate here let me move into that analysis activate that one and so I wanted something interesting to happen with this analysis and we saw from the results of that linear analysis that our results were somewhere around the 6000 mark between six and seven thousand so if we expand the material here after changing this to a nonlinear static analysis I'm going to change the material just right click on the material and say edit and I'm going to select the new material from the Autodesk material library not that you would ever design not that you would ever design the the structural portions of a front-end loader like this but just so we have some interesting output here I'm going to change the material to copper and when I change it to copper you can see the yield stress on this material is at 4829 right so it's lower than the stress results we get with these forces at the front end and so the other thing that we want to do or that I already did I went into nonlinear and I told it that I want it to be an elasto-plastic or by linear analysis of that way it's going to follow the modulus of elasticity up to the yield point and then it does have awareness of what that yield stress is at 4829 and then it's going to follow the slope defined by the tangent modulus and at that point we can go ahead and run that analysis okay so that analysis is finished let's say okay to that and now we have the results of our nonlinear static analysis and I wanted to a nonlinear static analysis because it is an analysis type that has multiple increments much like if you do a transient thermal analysis that transient thermal analysis would have multiple solutions over a function of time so when I set up my nonlinear analysis I told it that I wanted it to solve in ten steps so with that those for me is it breaks up that total load into those ten increments of course in the first increment you can see the load is point one or one tenth of that force is applied then the second increment the two-tenths of the load and so on and so forth so I can always roll back through the different increments and loads and see you know at the fourth increment for instance or forty percent of the load what are my stresses what are my displacements so that's one of the nice things with a nonlinear analysis you can kind of control the progression or the application of the load and see how the geometry responds at those different increments of load and a different way to toggle back and forth between the pulldown menu here of course is the previous and next buttons which is maybe just a faster way to do it otherwise you do have these same tools that we looked at with the linear analysis we can take a look at the probe tools we can take a look at the nodal query tools you still have these same pull down menus here so you can toggle through the different results but there's a couple other things I wanted to show beyond the fact that there are multiple increments when we get into the initial goal of running this is a nonlinear static analysis you'll notice that you have XY plots and it comes up with a number of default plots here for you so you have for instance a maximum displacement versus Luud scale factor and if I want to see what that looks like I can just select one of the default plots here and say show XY plot and it'll print that out for me so there is the plot right there if I wanted to I could also you know change this up a little bit as far as what they style the lines are the colors I can copy this information to a clipboard if I would like if you don't see a particular plot here of what you want to see with your analysis you can always right-click on the XY plot as well and say new and that's going to open up your XY plot dialog and the first thing that you have here is the choice between nodal information and element information so notable information if I come in and I select a node here and you can see identifies that node that would be utilized for certain types of data such as displacements and rotations and forces and moments you can see the information that it is able to plot by node and in the upper right hand corner here this is the span over which you want to plot it so I'm doing a multi-set plot where it's going to start at increment one and plot the increments 1 through 10 which are which would be the total increments from my analysis and I can say show XY plot and there I can see the displacement of that node over the 10 increments that I solved for on the other hand if you are looking for something like a stress then I would go into an element selection and I'm gonna select a element in that area where we saw the the max stress occurring and I'm going to do something like let's do a X normal and again multi plots or multi set and I can say show and there is a nice plot we can see of course we change it to a copper material we told it that that copper material is a bilinear material so once it reaches the yield point on the material then we can see how it changes slope once it's exceeded the yield of that material so XY plots nice tool something to keep in mind for certain analyses that you're gonna do okay so I would like to show just one more function within the results here and I can get there via a couple different ways maybe one thing that I do is just go to the results panel in my ribbon and I'm just gonna go ahead and click on the options here and that brings up this plot dialog and so with this plot dialog I can set up a couple different things first I can tell it which increment because again this was a nonlinear static analysis with ten outputs so I can choose which sub case I want to see I can tell it what result data I want to see from the contour options so maybe I want to see a displacement and then I can tell it again similar to like we saw before do I want to say total or specific along a specific x-axis I can also control the mid max as far as what the legend shows me if I want to specify that you can come into the the form options here and the form options allows me to control the displacement and this was something that I talked about in the slides as well so when you're doing a nonlinear static analysis it doesn't exaggerate the the deformed shape of the geometry it's going to set it to actual displacement at one time's the actual displacement or deformation of the model and then when I'm ready to have the program show me that I can just go ahead and click on the display button and then it'll display the output according to all the settings that I have checked okay so there we are so there's increment number ten it showed me displacement values and the actual displacement on my geometry okay there are other things that you can do in here you can create section views so if you want to show us such in view you click on the checkbox there you can tell what plane you can drag the planes around the slice through the model there's part view options here so I can click that select the part of that I can isolate the display of my results to the individual part you can get into vector options if you'd prefer to see things and vector form you have animation options here so you can tell it how many frames to output and then create the animation but I'm gonna do one last thing let me cancel out of this and let's say we wanted to go back and look at something with one of our linear analysis so let me right click on left click to highlight that analysis then I'm gonna right click and I'm going to say I want to activate that analysis so this analysis having already run it I don't want to have to run it again to review the results so I know that those results exist and this would come up you know when you toggle back and forth between the different analyses or maybe you save your work you go home you open it up a couple days later how do I get into these results if I right click on the results what I can do is couple different things here what I can do show in folder and if I do a show in folder that takes me to the results folder and specifically highlights the dot F n o file which is related to this particular sub case and analysis so I could find where that file exists so I know that that file exists the other thing I can do is I can just right click on results and say that I want to load the results and that will load up the results for that model I know that the results are available because they're no longer grayed out here and then what I can do is either just right click and say that I want to display one of those results types that are here for me the von mises displacement safety factor it'll take me right into that result type or again similarly I can go up to the menu bar and get into my results options again just like we did for the nonlinear static and whenever the plot comes up again just like we saw before I can go in and I can say ok maybe here I want to see a stress or a strain resolve let's do a stress result let's toggle to say that we want to avoid me see stress there it's telling me what the Max and mins gonna be and again I could adjust it if I want they will do that let's if I will say at the low end we want to see data min of zero and at the max end let's say 7000 and I'm gonna go into my deform options the form is already checked so that means it's going to show me a deformed or displaced shape now notice the difference here and the nonlinear static it was set to actual one one time because the linear static the displacements are going to be relatively small by default we're going to exaggerate them so it's setting it to 10 times a scale of the model the largest dimension in the model and so if you want to change it I'm going to leave it at that but if you want to change it to see the true deformed shape you can click on the actual button and set it to 1 but with with linear analyses we're always going to to scale it up and at that point I think I have everything set that I want to display so we'll go ahead and click the Display button and I'll say ok so there we go there's my we're in a von Mises stress i set the min range to be 0 the max range to be 7,000 even though the true max on my model is at 66 98 we're just adjusting the range of the legend so you can certainly do that there's one other thing that I don't think that I talked about in the slide deck and I guess that's the last thing that I can think of that maybe I want to show you maybe the final thing that you're going to do is prepare some images or you want to show somebody the model and you'd like to clean it up a little bit the last thing I'll leave you with is there's a number of options here under object visibility and that's where we can turn on and off the display of certain things so maybe I want to get rid of the min/max markers that's right here I can just uncheck that cleans up the model a little bit sometimes I like to get rid of the mesh the display of the mesh just makes a little bit easier to see the contours so we can turn that off and that'll clean that up and then lastly the the red lines here which show the initial position of the geometry that's your undeformed edges so we can turn that off as well and there we go so that's that we could also - things like turn off the the constraints and the loads if you also want to clean out those also but I think that's pretty good right there and you get the point so hopefully that helps the highlight you know some of the the major points of what you'd want to do in a results environment we showed you how to how to change different results types we showed you how to inquire on specific points on the model how you generate the XY plots

Channel: Autodesk Inventor

Views: 7,534

Keywords: autodesk, design, engineering, product simulation, fea, stress analysis, Inventor, nastran, learning, tutorial

Id: RxDSnI5CtwU

Length: 49min 28sec (2968 seconds)

Published: Thu Apr 30 2020