Lesson finished
Lesson finished
Lesson finished
Lesson finished
Lesson finished
Unlock all 10 lessons of Crashworthiness Analysis using HyperMesh and RadiossFull course ₹40,000 · paid
Shell Element Formulation and Radioss Element Properties
A free lesson from Skill-Lync's Crashworthiness Analysis using HyperMesh and Radioss course, on Grow by Skill-Lync · Last updated 16 Nov 2026 · Session: “3.0 - 2D Element Formulation shell Part 1”
What will you learn in this free Crashworthiness Analysis using HyperMesh and Radioss lesson?
The instructor explains why shell elements suit thin parts, covering the 6 mm thickness guideline, the loss of normal stress results and the bilinear shape function. He then checks a model using energy error and rigid wall forces in HyperView and HyperGraph, and ends with beam and spring property cards.
- When shell elements are valid, and their limits
- SH4N and SH3N shell elements in Radioss
- Checking energy error and rigid wall forces
- Spring types and the beam property card
What comes after lesson 3?
Later in Skill-Lync's Crashworthiness Analysis using HyperMesh and Radioss course (paid): lesson 4, Materials Part 1; lesson 5, Hypercrash Part 1; lesson 6, Kinematic Conditions Part 1. The full course has 10 lessons (25 h 22 min of video); see the course overview or its price and syllabus.
Lesson transcript
Machine transcript of the lesson audio (lightly cleaned). Technical terms may contain errors; the video is the reference.
Part 1
Our next topic that is about element formulations. So during meshing exercises so far, we have seen three types of elements. First was 2D element, then we tried 3D element mesh, and then we did 1D mesh as well. We'll take a look at all of them one by one, their formulations, what exactly goes into them, when they are being considered in the solver, and what actually affects the stability of such elements. So while doing that, we'll also look for the reasons why those elements are used at all. So let's start with 2D elements. So quickly recalling about shell elements, we have been creating shell elements by taking the complete geometry of the component and getting to the mid-surface, and then after getting the mid-surface, we create the mesh on the mid-surface, and then we can apply thickness to it.
We have seen so far two types of shell elements, not sh4n, but shell, which is four-noded element, and then three-noded element, that is tria, which is in radius block format, called sh3n. So it is just the same thing, just that instead of four-noded, it is three-noded, so there is a slight difference in the keywords. As we have seen them already, how to mesh them, we'll quickly look at why those are used at all. We have used them by creating the mid-surface, then creating the mesh, but the general rule of thumb while creating the mid-surface, or doing anything at such, is that the thickness should always be less than 6mm.
Now, why exactly 6mm? Well, usually it is seen that if your thickness exceeds that particular limit, 6mm, then the accuracy of the result is largely affected. In case of thicknesses more than 6mm, then usually that component is no more called a thin shell or thin-walled component, and that is the basic point of the shell elements, that shell elements should be used only when we have a thin-walled component. Obviously, the thickness parameter needs to be followed pretty strictly. Then, the result types that you can get out of shell elements is pretty common.
You can get bending and shear deformations. It's just that the normal stresses can't be recorded using shell elements. In case your normal stresses are very important, then in such cases, it is recommended to use solid elements instead. Well, rest of the things are pretty obvious or pretty logical, that mass of the element is distributed over the nodes. So, if you have three-noded element, obviously the mass is going over only those three nodes. And then, because it is a 2D element, the deformations actually happen as per a bilinear shape function.
Obviously, the shape function, though it is linear, it has two different directions, and that is why. Now, when we are dealing with a large strain problem, there are few modifications that we do in the formulation, and that is what we are going to study. So, you will learn the meaning of this last point much more clearly when we get there. So, again, stressing upon why exactly we use 2D shell mesh. So, when deciding which kind of mesh to be used for one particular analysis, you always start with the basic.
How is the component and what is expected out of the component. If you are going to go for some drop test or some test which is dealing with the damage or which is dealing with the plastic strain in the component, but not with the normal stress. In such cases, 2D shell mesh can be possible. This possibility can be made into reality only after meeting some other conditions. Now, the other conditions, as I said earlier, the thickness should be less than or up to 6 mm. Well, so, in general, in such cases, because the normal stresses are not also gettable, the thickness of the component, the thickness change, that is not going to be very accurately calculated.
So, I know, so, we will study over the time that the thickness of the body, it is going to be applied as a constant thickness all over the shell element. And the change in the thickness over the body or over the component is not wide. So, that's why, if you can say that even with all the tolerances or manufacturing errors, if you can say that this particular component is going to have a fairly constant thickness, then you are looking at a component which can use shell element.
But, at the same time, during analysis, if that thickness change is not very important, then in such cases, yes, you can definitely go for shell mesh. Now, obviously, when the thickness is changing, you are looking at some particular failure. So, you can imagine if the thickness goes on decreasing and it reaches some stage where the stresses overcome the resistance or the strain overcomes the resistance put up by the thickness and then it finally breaks apart. So, in such cases, you will likely get approximately same results with shell mesh.
But, the thickness change over the time may not be very accurate. So, in such cases, again, solid elements can be the key. And, as I said, or as we have already observed, 2D shell mesh is much easier to create. And, the quality of 2D shell mesh, it's much more can be controlled by user than the meshing software. So, because you can control the quality well, there are obviously little less problems with the stability because now since the element shape is under control and the element properties you assign are under control, there is nothing much wrong that can go with the stability of the element.
Then, obviously, because it is using less nodes, it is going to use less disk space while saving the model or even for results because there are less number of nodes to handle and that actually results in faster post-processing as well. Shell mesh, the major cause for using shell mesh has always been the cost. Cost drives many, many decisions in all the industries. So, shell mesh has been proving a very good or reliable solution. But, obviously, in case where you really need a huge amount of accuracy without any chance of error, then they usually recommend going for 3D mesh.
So, applications of shell element. Now, in manufacturing processes, you have stamping dies. In case of stamping, your die will be of solid elements but the object that is needed to be stamped that is made up of sheet metal. Now, you can imagine the thickness is going to be very much consistent over the span. And, that's why shell mesh can be very well used. Then, obviously, automotive component or automotive bodies, you have more than 2,000 of components in a body. And, looking at the number of nodes, now, even if you try to use maximum number of shell elements, still, a fully retailed SUV car can go up to 4 million of node.
So, even after using shell mesh, so you can imagine what will happen if you started going for solid mesh. Then, in aerospace industry as well, shell mesh element or shell elements application is pretty common. And, then, apart from that, in automotive, the airbags, they are another example of shell mesh. Whereas, the dummy is a good example of 3D elements. So, since we were talking about time step just before starting this topic, let me quickly connect there and we'll see how the shell element time step is being calculated.
So, if you remember, our time step was actually delta t is equal to L by C, where this L was critical length and C was the speed of sound through the material. Now, the speed of sound through the material will be constant as long as you are using the same element. But, the critical length, that would depend on what kind of element type you are using. In case of shell elements, that critical length is calculated based on few formulae. Critical length can be usually the minimum height of the element.
So, to calculate the minimum height, there are easier formulae. Divide the area by maximum of the side and then that will give you twice of your height because since you have the area is equal to half into base into height, since you are trying to divide the area by the base, you have half the height and that is going to give you the critical length. Minimum length of all the sides of a triangle that can also be or all the sides of a quadrilateral that is quad element that can also become your critical length.
So, the critical length can be decided between L1 and L2 that is the minimum height and the minimum side and that can give you the critical length in the end. So, again, critical length, they can vary with your shell formulation, the shell formulations you will get to see very soon. And then, the R-glass control parameters. So, R-glassing is a concept, we will be studying very soon. R-glass is nothing but the zero energy deformation modes where your element is seen being deformed but there is no energy recorded for that particular deformation.
That means, the situation is already out of hand, there is an instability introduced in the system, so you want to stay away from R-glass. Numerical damping and membrane damping, those are, well, so they can affect the stiffness performance of your material and that can in the end, it can be accounted with the critical length and that is why it can in the end affect the time step. So, in radius, the shell element formulations that are mainly used are mainly the four types. If you have an out of them, three of them are mainly used.
For 400 elements, that is quad, at least for R applications in automotive, those will be the types. And then for 3-noded elements, there is one commonly recommended element formulation, that is core tria or core triangular element. And then for 4-noded shell elements, there is Q4, QBAT, and QEPH. With respect to them, there is going to be one entity called iShell. And depending on the number of iShell, this element type will be decided. So iShell is actually the thing that you need to control in order to select this particular type.
And then for every type of iShell, there is a source or there is a description which tells you where it will be more suitable and what kind of integration scheme exists with that kind of element type. So as far as the integration goes, this is about the Gaussian integration that we talked about earlier. So you want reduced or full or improved integration, that is up to you. But usually the combination of integration that gives you the best result with minimum investment, that is usually selected. So from this picture, there is a clear choice for QEPH24 because they have reduced integration that is going to save time.
But they have an improvement in their formulation already that takes care of the accuracy. And that's why the cost increases a bit, but it doesn't increase by too much as good as fully integrated element. So let's take a look at all of them one by one. So what exactly are we doing when we are selecting different types of formations or formulations? Well, we were talking about reduced integration or full integration. So when you have a reduced integration scheme, you have one integration point on the whole surface.
Now as I mentioned in our preparatory session or the first ever session, the Gaussian integration points, they exist around the nodes. And what they do is, once you have nodal results calculated, the Gaussian integration points are going to help you with the internal details in the element. Now, having only one integration point over here, it is going to take feedback from all these four nodes. And then it is going to calculate some average or some value based on some formula that is again based on its location.
Now, because you have only one point to resolve all the results that you are getting on the four different nodes, there is a good possibility that you could introduce some error because your results between this particular point and this particular node, they may not be very accurate because they have been affected by other factors as well, which could be equal in quantity. So, obviously, this single integration, because there is less calculation to do, it is going to save a lot of time, but then again, it can introduce some error.
And then, obviously, the fully integrated element, which has four different integration points near every node, this method is definitely going to save a lot of time. But again, compared to the four point integration method, this is going to involve some errors. The one common issue with the under integrated element is that R glass is not controlled. So, R glass, as I mentioned, those are the zero energy deformation modes. So, in case, suppose you have this element being deformed by way too much, let's say this node has reached somewhere here and rest of the nodes are at the same location.
And this deformation has not been controlled or for every deformation, there is a stress that is being developed in the element and again, the area under the curve of stress and strain, that is the energy absorbed in the system. Now, because this node has moved in a remote location or somewhere else, and if these stresses have not been recorded, then obviously the energy won't be recorded. And that is why R glass is somewhere, is a condition where your node is moving, but it is not recording any stress.
And that is really a bad situation because if it is not recording any stress, then that stress won't develop any forces on the rest of the nodes. And that will simply break off the whole time step cycle that we studied earlier, how the time step works. So, further going on with R glassing, those are non-physical modes of deformation, under-integrated elements are very common examples where this could happen. So, in the picture that we see over here, there is first case where the element has deformed by way too much, and you see the rest of the elements are undergoing this instability mode now because this node hasn't recorded anything and the deformation type is really weird.
Whereas, if you go for any improved integration or QEPH integration or fully integrated element, you see that the moment of the node is pretty much under control and the rest of the body is also getting deformed accordingly. Whereas here, this node has by itself has moved so much upward that the rest of the body hasn't responded to that node's moment. So, again, this is fully integrated, this is improved Q4, that is the subtype of this, and then there is this QEPH. All of these are having very similar results, but the QEPH is better in terms of cost as well as accuracy.
If we really negotiate between our cost as well as accuracy, then QEPH happens to be a good choice. So, this R-glass can be controlled by two different methods. First is perturbation, other is physical stabilization. Now, let's see or let's look at them one by one. The perturbation method, in this case, it is actually a viscous method where when the R-glass deformation is happening, there is some damping applied. And because of that damping, the deformation will be stabilized and that way it will try to control the speed at which this deformation is happening.
Because when you apply damping, the damping is actually going to oppose only your velocity, but not the force. To apply that velocity, a force is getting generated, but it is only going to affect the speed at which this deformation is happening. And that is why, while this force is being introduced, it is going to add some stiffness to the element. And that stiffness, in the end, is going to cause this R-glass to be controlled. Now, because this force is being externally applied or applied by some other means and not natural FIA means, this force constituting to another energy type that is called R-glass energy.
That is why it is called an artificial energy or artificial form of energy because it doesn't exist in nature. It is neither kinetic, it is neither internal energy, but it is R-glass energy, which is actually a loss of both energy types. As per the energy balance, if you add your R-glass energy along with your kinetic and internal, then you might find a balanced system. Then there is perturbation method based on stiffness. Now, in this case, in this case, the stiffness is artificially added on the element.
And to add this stiffness artificially, it is going to affect the material properties directly and not by any other means. So, in case of viscous method, it is going to add a damping to that node. And that damping or that nodal damping is going to add some stiffness externally. Whereas in stiffness method, the stiffness is getting added right at the material level. So, because this change is happening at the material level, this can have a larger effect on your component. So, when we really compare between these two methods, because the viscous method is going to be applied only when it is trying to detect the deformation or R-glass type, there is a good chance that there will be a huge amount of artificial energy that is getting generated.
Whereas in this case of stiffness method, because it is happening at the material level, most of the R-glasses are getting controlled even before they arise. And that is why there is less need of the R-glass energy to be used to control those R-glass modes. And that is why if we really compare, the stiffness method yields a much better or much lesser R-glass energy. Stiffness method causes less energy to be spent in R-glass. Talking about the comparison, the point over here, that makes a lot of sense.
The viscous forms recommended for only high velocity or high strain rate problems. That is, when you have, now this high velocity or high strain, this high velocity is of the order of at least 100 or 100 to 1000 meter per second. This kind of high velocity is attainable only in case of explosives or only in case where you are firing a bullet into something. So, in such cases, you can attain such kind of high velocities. But for other cases, this QEPH or the other method, stiffness method, that works well enough to give you accurate or fairly accurate results.
With the stiffness method, there comes an R-glass coefficient and if you try to control that coefficient, that might just solve your most of the problem. Now, because you are increasing the stiffness at the material level, there is a chance that you will control your R-glass, but you will also affect the performance of the component by a lot. Because you have added stiffness artificially, in such cases, if the component, If the sound was supposed to deform by 10 mm, it might deform only by 8 mm, and that is a wrong thing. To take care of that, if you control the hourglass coefficient, it might minimize the stiffening effect, but because the stiffness is still getting applied at the material level, the hourglass is being controlled very well.
So, just coming out of the keywords here, the stiffness method is being used in the QEPH, whereas the viscous method is being used in the Q4 fully integrated or under integrated elements. So, obviously, because our problems usually are not the high velocity problems, the natural choice which we make all the time is the QEPH elements. So, when you open your HyperMesh window, such as the case here, if you have your mesh ready, what you can do is, if you go to the component in the entity browser, you will see that your component name is there, and after that, after the card image, always make sure that you are using a part card image with radius profile, and after that, it asks for material and property ID.
So, here, you can always right-click and say create, and for that, you can name something. Now, this naming convention can be based on your part name. In automotive OEMs or in many companies, they usually have a proper part number for some particular component. In such cases, this part number might come in this particular place. After adding the name, there are so many questions that it asks before finalizing the element formulation. So, let's look at some explanation for all of them, and then we can finalize one element card here today, or in this session, for 2D elements, and then we'll move on to 3D.
So, the key parameters that are being asked are just what we saw on the screen. First, we select the shell, and then from that, in the card image, again, we have to make sure that we are selecting P1 shell. To that, for these questions, or for these entities, I shell is actually the element formulation for 400 shells, the one which we just saw about Belich Chupoko, or QBAT, or QEPH elements. Then, there is ISH3N, which asks you for which element formulation should be used for 3-noded elements.
Now, we saw earlier that co-triangular elements with ISH3N2, that can be a good choice in such cases. And at any point of time, if you feel that you are looking for some more explanation on something, if you are in HyperMesh, you can always press F1, and that will take you to the help page. So, in this case, what I'll do, I'll show you another way of going there. You can click on help, and you can do HyperWorks help home. Then, on the HyperWorks help home, you need to click radius by scrolling down.
In many computers, it is likely that some content of this HTML document is getting blocked. You need to allow that content for all these links to work. So, I'll click radius for solver help. And then, here, what I'll do is, I'll type P1Shell with a slash, and that way, it is not giving me any result. And that happens many times. So, what you need to do in such situation is, instead of P1Shell, you can simply type formulation that we just saw for shell elements, slash shell.
And now, this is going to give me a lot of results. So, I'll go to this. Now, it is telling me, on the usual card for the shell elements, that there will be a part ID, there will be a shell ID, and then there will be four nodes. So, this still is not the one which we are looking for. So, what I'll do is, if you remember, in HyperMesh, when we tried to create the component, if I click here, it shows me this particular keyword, prop shell.
So, what I'll do is, instead of doing just oblique shell, I'll do a prop shell. And now, in this case, now, we have this prop shell component, and for that, we have an explanation for all the entities that are being asked on the screen in HyperMesh. So, I shall, we just saw, there is Q4, Q4 usable through 1 to 4 options, then there is QBAT, fully integrated shell element at 12, and then there is I shall equal to 24 for QEPH shell formulation. And then, for again, triangular elements, we saw there is option 2, which is good, and then there is option 1, with small strength formulation being applied right from the beginning.
So, I shall is going to ask you for the select, for element formulation for 400, ISH3N is for 300 elements. After that, this N is actually the number of integration points through the thickness. Imagine if you have very huge thickness, such as 10 mm or 12 mm, which is higher than the advised 6 mm thickness limit. If you have more than that, then, over the thickness, you have integration points, which are spread across the thickness. Now, these integration points are actually the reason why the solver is able to decide how much strain is needed to be applied in the normal direction of a shell element.
So, though we don't have any particular information on the thickness change of a shell element, the integration points, if they see any failure on any of the integration points through the thickness, then they'll consider that the element has failed or the element has cracked. So, this integration points through the thickness is very important parameter that needs to be set to maximum all the time. Not the maximum, but to a considerable number. Then, there is small strength formulation or large strength formulation. As we saw earlier, this formulation can help a bit with some of the instabilities.
And then, there is I plus and I thick, which are going to help with the yield or plastic strain results. So, I thick is all about under some load. If your thickness is going to change, then I thick needs to be selected in a way so that it allows the element thickness change. Otherwise, it will simply run into instability. So, this we saw earlier, Q4 is having four different options for high shell. And these four options differ only in terms of the algorithm for hourglass control.
Usually, option 1 of iShell or option 4 are usually preferred options, though they are very much similar to each other. So, in case you have, you don't have very complex of a load case, not many velocities are involved. In such cases, iShell equal to 1 or 4 can be very wise idea. Then, there is fully integrated elements. You have four integration points over the span of the element. And then, extra integration points. There will be no hourglass. Please don't get confused. The Gauss integration points can help you with hourglass.
Whereas, the thickness-based integration points are going to help you with the accuracy. This is about instability, the other one is about inaccuracy. So, again, QBAT may not be as flexible or as economical compared to iShell equal to 1 or 4. And then, one special thing about iShell equal to 4, that is, QBAT elements, is that they are the most accurate because you have so many integration points. And it also affects a bit for shear locking because the integration for shear is reduced already.
Part 2
After looking at the QBAT elements which are fully integrated, we can take a look at the reduced integration element, QEPH. Now the difference between the Q4 and QEPH, that is I shall equal to 1 to 4 or I shall equal to 24, is that the integration here, though it is still under integrated, there is an improvement because it has a physical hourglass stabilisation method within itself. So as we studied earlier, it has the stiffness method on perturbation and that is actually helping by changing the metal property a bit so that the hourglass will be controlled from the beginning itself.
That's why this can help with the hourglass deformations, hourglass issues a lot and this because it is still under integrated, the cost is still less and the quality or the quality of results or accuracy of the results has improved a lot. So that is why after negotiating between cost and quality, QEPH happens to be the best compromise or the best choice for all of us in case of automotives and as we stated earlier or as we saw earlier, QEPH can be up to 15% costlier compared to Q4 that is I shall equal to 4.
Then comes the triangular shell element formulation. So as long as we select ISH3N equal to 1 or 2, we usually get a co-triangle element with large loterations already considered. Now because a triangular element has only 3 nodes, there is no way that any node would run out of plane because those are only 3 nodes that are needed to form a new plane and that is why it becomes easier for the triangular element to deal with hourglass kind of loading. So obviously because it is 3 noded, the CPU cost is going to be low and among the 3 nodes, there is only one integration points result on the triangular element may be questionable may not be very accurate.
And that is why we have a reason that the triangular element that number should be minimized when we are trying to create the mesh. So, so far what from our discussion we have decided that because QEPH formulation that is I shall equal to 24 has improved under integrated form. So that's where it is good for cost and because of the physical stabilization method that is available for hourglass control, this QEPH can actually be a good element form that is yielding some good result. Then comes the triangular element or the element type needs to be taken as cotria which corresponds to I shall value 2 or 1.
Then we come to the integration point. So this integration point is nothing but the number of points over the thickness. Now in radius integration points up to 10 are allowed but so the usual idea behind the integration points is that the recommended number is always going to be 5 because in such cases it keeps one integration point on the surface of the 2D element and then there are two integration points on either side of the shell element.
Part 3
After deciding the number of integration points, N will go to the next property entity that is small strain formulation. Now the small strain formulation, most of the cases which we are going to run will stay the same. But there are very peculiar problems where the deformations are very small and those are the times when we might go for some other option. But right now, so in small strain formulation, we have couple of options, option 1 and 2. Option 1 is made for small strain from time equal to 0.
That means the strain computed will be based on the initial element shape. Whereas if you really consider a high deformation problem, you can say that the element size will be changing drastically. And because of that, the strain calculation should be very instantaneous. So if let's say during one particular time step, your element length has changed from 100 to 110. So in that case, you have 10% strain. But for the next iteration or next time step, if your length is going to change from 110 to 115, then in that case, your strain is not actually 15 by 100, but it is actually 5 by 110.
So in such cases, you need to keep it updated. And that is where the strain computation should be based on the current element shape or size. And then because the size has changed, the spatial integration points, the Gaussian integration points, their locations have also changed. And that will give a good enough reason for the calculation of stresses and strain inside the element. So your shape function is still constant, but the variables inside the shape function, such as the element size and length and maybe width, those have changed.
Then your location of Gaussian integration points have changed. And because of that, the whole style of calculations for the strain or stresses that has changed for that particular element. And that is why this large strain formulation or small strain formulation is very critical in most of the cases. So when I say it is default here, it means that if you keep this value 0 in the setting, then well, in that case, it will by default take the values too. And then in the cases of where the deformation is too high and that is and because of that, the time step has dropped drastically in the simulation.
And then we have set a limit. The time step cannot drop below certain value just to maintain the speed of the simulation. In such cases, the element will be switched to small strain formulation and then it will cause some errors in the calculation, but it will happen quicker than large strain formulation. But that happens only during the high deformation problem. So if your element size changes from 100 to 50, you can imagine the time and the drop in the time step because the time step is again dependent on the characteristic length of the element.
If the element size itself is decreasing, you know what could happen after that. So let's quickly look at how the stress competition is happening since we were discussing the small strain formulation. We have discussed before that the time step calculation or how the calculations are happening during each and every time step. You calculate forces on one particular node that gives you acceleration. Acceleration is in the end going to give you the displacement and that displacement is going to give you the strains. The strain is the cause for stress and stress is ultimately the result that we are looking for.
Or maybe the strain itself can be a good enough result for us. So to reach this strain value or in fact all the failure calculations inside the element are all based on the stress. To go up to that stress, obviously all these calculations are going to happen. And well, and in that case, because we are considering the one misses stress, the one misses stress formula takes care of normal stresses in two different directions as well as the shear stresses. And that's why the one misses stress becomes one good criteria to look at in the elastic materials or isotropic materials.
So as long as your one misses stress is smaller than yield stress, the compute stress is going to be used for internal forces of the elements. And that internal force is going to give the calculations for the next time step. So as long as your one misses stress is less than the yield stress, this style of computation will go on. After that, we reach or we enter the plasticity phase of the element or of the material. And then after that, because your elastic modulus, that is Young's modulus is changing, some of the calculations are going to change.
So since we have reached the plastic region or plasticity region, the strain needs to be updated through thickness. That is not just one thing, but the new elastic modulus, they need to be taken into consideration. So for all such purposes, there is a switch that is required in this case. As soon as our stress reaches the yield stress value, this I+, this particular entity gets activated or gets into its role. So as long as we select option 1 instead of 2, that is going to take care of all these changes.
So when we select 1, what will happen is it will update the strain through the thickness. So until now, we have seen that for shell elements, we take care of the thickness using a thickness value as well as the number of integration points over the thickness. So more the number of integration points, or better the calculation over the thickness. So because of that, once we have this I+, equal to 1, the strains will be updated through the thickness. So those number of integration points will come into place now.
Then if your element has undergone some compression or some excess tension, because of the Poisson's ratio, whatever the value is, the thickness or the shape of the element is going to change in 3D dimension. That is why the new thickness calculation is required. And that is why in this case, that will really happen. And now that is a considerable amount to calculate because you have reached a plasticity region. Until elastic region, you can very well say that the thickness has almost stayed constant, hasn't changed much.
But when you are reaching the plastic region, there is a good enough reason for us to look at those calculations, or for the solver to look at those calculations, not really as. And then the rest of the calculations are going to follow. If we check the radial return option, that is option 2, well, that process is going to be faster. Rest of the steps that are mentioned over here in 3 bullet points, those are going to be skipped. That's why, obviously, the calculations will be much more faster.
So, in this case, as it is highlighted by the green box, for I+, option 1 is always the best idea to look at. Now, if you keep it 0, it is going to go for option 2. That will give us a faster calculation method, but it won't be really very accurate. So, it is a good idea, usually, to set a shell card right away in the beginning by looking at some guidelines and putting all these values for once, and then you simply keep on copying that particular card so that you don't lose much information.
Then for I thick option, so, in this case, again, continuing from the plastic option, the initial thickness is used to compute the strengths and stresses in the initial phase. But once we reach the plasticity region, the thickness change can also be accounted for because in such cases, it is very likely that the thickness has changed a lot. So, in such cases, that change needs to be accounted for for calculations of strains and the stresses. And that is what exactly this option is doing. Obviously, as the instruction in that box particularly says, thickness change is being taken into account as long as you have I thick equal to 1.
If you have I thick equal to 2, it is going to give you faster calculations, but it will consider that the thickness is constant throughout the simulation and which may be realistic, which may not be very realistic. If you take option 1 and look at the results and if you take option 2 and look at the results, the change in the results may not be too much depending on your load case. But in critical load cases where, let's say, if you are doing something with the structure and some change in the results on the structure is going to affect how much energy is absorbed in the passenger compartment and then how much energy has been transmitted to the dummy in the end.
All such things are going to be crucial in the crash. That's why it's always a better idea to go for the most accurate option over here since the cost is not too high in this case. So, just to sum up all the recommendations that we have seen so far, iShell equal to 24, that gives us QEPH, 4 noded shell elements, which is best combination of cost and accuracy. Then, small strength formulation, number of integration points, ISH3N, that is 3 noded shell elements, that is trials. For them, the core triangular formulation is very important.
So, that does little modification to their formulation for large rotations. It's going to solve a lot of problems with the triangulation locking. Then, iThick option for thickness change accountability and then iPlus for plasticity region. So, with that, what can be done in Radios is that whenever we are creating any mesh, right away we create a property card or thickness card. So, since we have seen that even during the meshing stage, we just created a property card and we only assigned thickness. But apart from thickness, these are the rest of the things that are needed to be assigned in order to get the better results with our simulation.
Apart from that, apart from every plasticity card or every... Shell card. There is an option in radius that is called def shell. What it will do is when we define def shell, we can set all these values over here. What it will do is whenever some value is not defined for any of the shell cards, it will refer to whatever value here we have written in def shell. So let's say you have defined a new element card which has iShell equal to 0. Now if you have kept it equal to 0, then what will happen is when it is 0, it will try to point out to def shell and because you have iShell equal to 24 here, automatically it will consider iShell equal to 24 even for that particular card.
So it is always a good idea to define this just for safety purposes, but for element to element or for component to component when we are defining properties, it is a good idea to make sure all these options have been applied. Now in case of dummies or in case of specially formed elements such as let's say airbag, some of these options might change. Now in such cases, obviously you can't refer to value 0 because def shell is a global card. The property element property applied to airbag elements is very much specialized. In such cases, the specialized card will take care of those elements. Whereas as long as you keep 0 and def shell is properly defined, it will do the rest of the thing.
So based on that, once you are ready to run one simulation, the file that was shared earlier for the initial radius assignment, we are going to use the same file for the next assignment. Now that assignment will be conveyed in a separate slide or in a separate document as well during the assignment stage. But just to give a glimpse of it, this crash beam file, if you go to HyperMesh, go to import and wherever your file is stored, you say open and you say import and then when you hit import, you might see your file in this kind of format on the screen.
And then you will hit this button for shaded elements. So that will give us shaded elements. In your case, you might even see something like this. These are nothing but the contact surfaces, which is something for us to study in the later stages. But for now, it is a good idea for you to not get into that yet. We will go step by step. So here you can deactivate some of the things. So once you deactivate, it will be much nicer to look at these things as long as you don't have such things to pop out of the.
So you have this model open. What you need to do is as per the assignment, you only need to run the base simulation as it is. And then you are going to apply all these recommended properties in the element property card. And then you are going to run the same simulation. The idea here is to compare the result. What happens when you apply these properties and what happens when you don't have those properties? So if you quickly look at here, the properties, there is one prop shell, then there is another prop shell and there is another prop, then there is a spring beam card.
So the spring beam card is being used for all the weld elements. We'll look at it right after we study 3D elements and 2D elements. So for now, you can concentrate on these two. So here you have option to set all of these. Right now, they are 0. So whatever the default value is, they might be referring to that. And since there is no def shell card, there is no default value. So by default, if it says in the help documentation that 0 means 2, then it will refer to 2. And that is what we need to change right now.
So you will run the simulation as it is. How to run the simulation? There is a quick step. You can go to analysis, radius. And then here you can save this to a new folder somewhere, somewhere on the local directory, not on the shared drive or anything like that. Because radius instantaneously creates so many files during the simulation and you don't want to get into that mess to sync that whole folder with the with the network. You will select a new path or new file or you may want to write wherever you took it from.
In the export options, make sure that you have all selected. Because if you select displayed and by accident, if you had switched off some component out of your model, it may not get considered for your simulation and then it will mess up many things. Run options. Keep it analysis right now. Run number 1 is fine. And then here for options, this is how the by default settings would look like. But just to increase the speed of your simulation, you can use this option NT space 4.
And don't forget this minus symbol over here. So, what it is doing is NT is number of threads. So, it is much more like there are 4 CPUs running simultaneously to solve this problem. And then once you type this and make sure that the first run underscore 0000 dot rad is the path that is being saved as. And then you hit radius and it will start the simulation. If you are not able to run this, you can surely ask this question during our support hour. Once you make these changes, run the same simulation with maybe a new file name and make all those changes.
Quickly take you through what to expect from the simulation. You will be looking at some result types. Then you will make a brief presentation comparing the results from the default simulation and the changed simulation. Then you will have to tell me why there is a change in the result and what exactly is the change in the result. So, these are the points that you should look at. Obviously, you should open one dot out file. If it runs completely, then you should definitely open one dot out file and go to this part of the file.
You should check for energy error and mass addition at the end of the computation. So, energy error will be listed somewhere here as explained earlier and mass error will be somewhere here. And then there is some explanation for the energy error. Now, ideally, energy error should always go negative. But if it goes positive, then there might be something to worry about. But as long as it is less than plus 5%, that can be a considerably good result. If it exceeds plus 5%, then there is something really needed to look at.
You will look at the energy error and then make some conclusion whether it is an acceptable result or not. If the energy error is negative, there are so many implications out of that. If energy error is positive, there are so many options or so many implications out of that. You should ideally look at how the energy balance is or what is exactly the energy balance and then you should make some conclusion on that. So, I expect, I want you to try that specifically and then come up with an answer.
Make an attempt and then we will see what can be the ideal answer for that. So, in this case, if you don't know what are the implications of energy error, what I will advise is always, always use this entity. You go to help, you go to HyperWorks help home. So, it is going to take you to alter help and then you go to radius and then you can say energy error and try if anything comes out. So, it might give you some hint at how to check the results and so many things.
So, the purpose behind this is for you to take you through this process whenever there is a question in mind, always feel free to use this help documentation. So, if you really click on any of those, it is going to give you a lot of information on what exactly is going on in the simulation. So, always feel free to go through this stuff and come up with questions and in that process, you will end up exploring a lot more about the software and not just what we are learning in this particular class.
Obviously, after looking at the energy errors, you need to plot the rigid wall forces. So, for that, you need to open the T01 file in HyperGraph. So, to open that, I will quickly give you one simple idea how to use HyperGraph. So, when I switch my window to HyperGraph, this is where I can switch it from. This data will be raised but since I have written it out already, I am in good zone. So, once I switch this to HyperView, this is where I can open the animation file.
So, H3D file is nothing but the animation file. HyperWorks 3D could be its meaning right now. I have that whole simulation loaded. So, the rigid wall which was defined in that particular case is now pretty much visible. I can use this particular button, plus or minus. If I hover my mouse over it, it will tell me what exactly it is going to do with the mouse clicks. If I left click on this particular thing, nothing will happen. If I do right click, it will hide that particular part.
But you see a rigid body defined at this end, which will be clearly visible now. Which may not be visible in HyperMesh until we switch on few components or entities. And then, apart from that, you can always go to preferences, option, and in visualization, all 1D elements should be, let's say, represented by a dot. And that dot size should be kept 0.05 because this size factor can be very crucial many times. If you go here, you will see this more like a weld. Now, I can always go back and change the size if I feel that it is too low to look at.
I can make it 3 times bigger. And now, I can see all those welds. Then, I will hit play button over here. Since I have already hit apply, it has loaded my model. But after loading the model, there is another step that is loading all the simulation steps. You will see the way these guys are deforming these elements. It is not really natural. This is not how I want to see this deformation. I can't believe that. I can't believe that at all. There will be such flat faces when something is deforming like this.
So obviously this mesh is very coarse for this particular application. But what happens if you change the element properties? So that is the purpose why we are looking at this particular exercise. Now, you can split this page into two parts using this particular option. And now in this case, once I click here, I'll go back to this button and here I'll go for hypergraph 2D. So it will switch this window to hypergraph 2D. Alternately, I can also make this window full screen or I could have also switched this whole window to hypergraph 2D.
No limitations as such. Now I can use this button over here to expand the whole window to full screen. Then I can narrow down the area spent in the non-useful things on the screen. So once this hypergraph window is open, this hypergraph, as the name suggests, it is going to plot all the graphs that you need. So I'll go to my folder where I have finished my run and all these files have been generated. So these A files, that is A, 0 something. So your simulation name A and then some number, these are all the animation files.
But these animation files have been combined into one H3D file. So if you really look at the size as well, every animation file was about 53 KB. Now the size depends on how many nodes or elements we had in the model as well as what all types of results we were requesting in the animation. So that decides the size of this animation file. Combined all of these into H3D. So I could have selected, so that is why I could select H3D as the single file. But apart from that, to run the animation, you can always select the first animation file in the series.
And if you hit open, then also it will load all the results. Now in this case, for time history outputs, that is the graphs, we need the T01 file. That is, which is for the time history plots. The name will be your simulation name, T01. Now this T01 is always constant, it always stays like T01, as long as it was your run 1. If you say run 2, then it could be T02. It will give us global variables, such as global internal energy, kinetic energy, then the total energy.
You can look at the energy errors, and then you will understand how these are behaving. So, the kinetic energy, which starts at a very high value, because you had initial velocity applied to your model, which is crushing into a rigid wall. Just to explain that case briefly, what I can do is, so what's happening in this particular case is, there is a rigid wall, and there is a rigid body, created on this end of the, this end of the crush can, or crush pipe. And then there is a mass applied to this particular rigid body.
So, initial velocity is applied at this end, because of that, this thing is getting pushed into, into this wall. Now, because there is a resistance, you see, and because of the shape, it is going to kink at this particular location, because once that load starts moving, there will be some bending in this location initially, and because of that bending, suddenly it will start buckling as well. So, if you go by this method, you see the kink that is getting developed here, and after that kink, there is still a lot of energy coming in from this end, and because of that, after this kink, this kink starts getting developed, and then it reaches the end of the simulation.
So, this is very much equivalent to a crash analysis. In simpler cases, your kinetic energy starts at a very huge value, because you have initial velocity, and you have huge mass. Your internal energy, that is, strain energy, starts at 0, because there is no deformation in the, at 0 second. And then, because the deformations are happening linearly, this goes on increasing linearly, and by the end of the simulation, by the end of 55 milliseconds, that you are supposed to run, though I have run for 60 milliseconds, you will see this graph constantly decreasing, this graph constantly increasing.
So, if you had run for more time, you could have seen that this graph reaches 0, and stays constant, whereas this graph reaches almost maximum value, and then stays constant. Almost maximum value, but not the exact maximum value, because there is some energy error in the simulation, and that is the energy error, that you will find out more about, once you read the help documentation. Obviously, there are plans of discussing that, in the later stages of this course, but it is a good idea for you guys, to start reading the such things, so that you will have a better idea, when we actually reach that stage.
Then, we are going to look at the rigid wall forces. So, our wall force, what we will go for is the normal force, and come back to this page, and delete these two graphs, if I don't need them anymore, and then I will hit new plot, don't start for new session, but hit the new plot, and that will give us a clean window again, and then are all forces. Why I needed clean window, because once I plot something, it is going to keep its title over here, and as soon as I get a new plot, this will be wiped out, and it will get us back to the original condition, or default condition.
So, we want the normal forces, that were applied on the rigid wall. In the initial stage, when the first impact happened, there was a huge force, and after that, because the internal deformation, inside the crush beam started, that force, or the opposing force, or the force that was being applied, onto the rigid wall, started decreasing. That is another case, that there was significant amount of force, that started getting converted, into frictional force. So, it will be a good idea, to also plot frictional forces here. Now, we see that it was zero in the beginning, but the frictional forces also, started developing over the stage.
Now, if you remember the simulation, there was some stage, where most of the pipe, was actually tackling against the whole rigid wall. And that was the time, when the contact area had increased a lot, and because of the contact area, there was more energy spent, in the friction, more forces getting developed, because of the motion of the, then there is a resultant force, that will combine both normal and tangent forces, and that is almost matching, with the normal force, because once you add these two quantities, there is not much change, that is seen on the resultant.
So, coming back to the presentation, resultant is the one, which we are interested in, as far as the presentation goes, but it is a good idea for you, to also look at, the normal forces, and you want to indicate, if there is any difference, between the two, between the two simulations. Then, you also need to plot, global variables, such as internal energy, kinetic energy, I showed you already, there is one more, hourglass energy, and total translation energy, that you need to plot, and you need to tell me, how their behavior is, this could be one sample behavior, but you need to compare, how the other behavior was, and then you also want to tell me, what was the maximum one misses stress.
Now, quickly showing you, how to plot the stresses, we will go back to this tape, and then I will, click this button, for this window, to go back to its original position, then I will go back to the first window, this is how I am switching the windows, within, or switching the page, within one hyper work session. Once I click here, I will again go for the full screen, and it will expand this plot. So here, once I am done, running the whole simulation, what I will do is, I will click this button, that is contour.
Once I click contour, I can either plot displacements, so, that is also a fun thing to look at, how the displacement is happening. So, initially it was all zero, then there is a contour, because, well, if you, clear the contour at this stage, and then, apply again, you will see, different contours, because, now the meaning of the red, color here, has changed. So, the displacement in this case, was, maximum was, 272 mm, remember the results here, you may not see any, unit, but, this is where, your unit system, that was applied to the, input model, will come into picture.
Because, all the distances in your model, were in mm, even this displacement, will be in the millimeters. Whereas, energy, um, Could be equivalent to what your unit system was. So that is something you need to find out. So once you keep running, you'll see that though the color stays red, the meaning of red has changed. So there is a way to keep this contour constant over the time. Now since I know that the maximum value is actually 820, what I'll do is we'll go to legend, edit legend, and put this value in.
This value as 820, hit apply. And now whether I move my simulation anywhere, I'll see this contour fixed at these values, whereas maximum will be shown at 820. So one application of this is that if I want to highlight any area that has displacement more than 800 mm, I'll put that value here. Or in fact, I'll put that value over here. So for that, I need to hit default. Then the second value is something that I want to target. So once I'm setting this value as 800, what I can say is that whatever is above 800 will be shown as red.
I'll hit apply. I'll hit OK. Now I see that the line between red and orange is shown as 800. So whatever is orange, it's still within 800. Whatever is above 800 is all red. When I move this, I finally see something in 800 region. Then I see red color suddenly and I see that these are the elements which have exceeded the imaginary limit of 800 mm. Now you see within this element, there is a contour. That is because the calculations happened over the shape function and Gaussian integration points.
And that is how it came up with that kind of plot. Now if the mesh was finer in this case, we might have seen better results or whereas if mesh wasn't finer. Now I see that there was some R glass behavior in this case as well. The way these elements have deformed is not really natural. So it is a good idea to look at the R glass behavior or see if we can improve on that particular deformation mode. Now perhaps you might get a better result. So that is something that you are going to try. Now this is how I plotted displacement. I'll go back to result. I'll hit clear contour.
And instead of displacement, now we want to plot one misses stress. I'll hit one misses. I'll hit apply. Now it will show me different stresses for each and every element. So one good thing to do in such cases is use the averaging method. Now you'll see continuous contours just left how we were seeing for displacement. So I'll start from the beginning. You see that there is a compressive force or compressive stresses being generated over here and that is why it is showing zero or not really zero but because it is compressive and the minimum value shown over here is 0.
It is going to show like that. But there are compressive stresses getting developed here. Whereas there are tensile stresses getting developed. We don't know yet where exactly they are. But a good idea to look at them is always hit clear contour, go back to original shape. Once you clear the contour and go back to original and then clear the contour, you'll see that it starts from 0 stage. Now, now it is truly at zero condition. If you hit or if you move the contour around, you'll see that this is continuously changing and the maximum value and the minimum value has been indicated over here.
Now to see continuously where exactly that is happening, you can go to this option over here, measures and then there is dynamic minimax or minimum maximum. Once you click that option, it will show you where exactly is the maximum result or minimum result on the node that has occurred. Now from this it is showing that the minimum value is at this particular weld element because it is undergoing very less stresses right now. Whereas you see that node number is changing continuously because the node under maximum stress has changed now.
Now you need to also see whether this maximum result came on the same node when we made changes to our simulation. So you can hit open report template, the one which we just saved template, hit open and we hit open. It will ask for all these files. So h3d file was used in this case. Now in your case, the change run where you will make changes to element properties if you have made those changes and if you have made or used some other name, simply select that h3d file.
So for example here, I will select the original file again because I don't have the other result loaded over here. Here as well, I will select that file again. And then here as well, the t01 file that it was needed. So that t01 will be selected over here. Now in your case, if your file name has changed, you can click this option and see if all these things are checked green. That means all the channels that we were using or all the output types that we were using, those are the ones that are loaded over here. If it is not all green, then try hitting this button select best match and it might just do the trick.
Then hit apply while keeping this option and bend or overlay or replace on. Right now in this case, it won't matter. But if you want to keep the result side by side, append option will do that or overlay option will do that. When I hit apply, hit clear button, close button. And now if you see the first window, whatever situation or condition it was in, it has loaded the same type of results. Now here also it has loaded the one misses stress. But in this case, I had done some changes by going ahead and back over the simulation time that hasn't happened here. So if I hit play, it will try to load all the steps again and then it will finally start doing that thing.
One thing you can notice is that if you have your animation as well as plots loaded side by side, it will try to run this kind of timeline and it will show you what was happening on the force when this kind of stress was happening. So this is one way of debugging few runs if something is going wrong. But usually I don't recommend doing this because right now this is a very light model. That is why we are able to do that. But in complicated models, your graphic memory being used for animation purpose is so huge that you won't be able to run them in sync on both sides. Otherwise the operations will be very, very slow.
Very slow. So not very recommended to do this. If you want to run the simulation, make it full screen and then run it and you will find that it is much way much faster. Whereas if you want to look at this only go to its full page mode and then look at this and then you will see that this is happening or this is moving so fast. And this is when the very light, light, very light model was being used. So this is about the result templates. The template itself means that you have used some process to look at the results on one file.
You want to reuse the same process to look at the results for another file. You should use a template. Now this is one of the best features that you can learn about hypergraph or hyperview. And this feature will be very useful for you in your all types of projects where you are trying to compare results for same model, but only some minimal changes. With this, we have completed exercises on shell property cards, shell element property cards. And next session will be about solid elements. That is 3D elements.
from the custom domains. And next session will be called 223 elements and search operations. Wow, yes.
Part 4
After shell elements, we move on to solid elements formulations. We start with the applications. Now, very typical applications are bushings in the solid assemblies where, now these bushings could be somewhere around your suspension, somewhere on the engine mounts, where all such cases, the behavior, the instantaneous behavior of that rubber element is very important. In such cases, bushings, which don't have constant thickness or the thickness is way too high, more than 6mm. In such cases, 3D elements have found a perfect application. Then, in electronics, in cell phone industry, if they are doing the drop test on your cell phone, in such cases, the cell phone body may be meshed in 3D.
Now, obviously, in such cases, minute details on the cell phone, such as the keys, well, in the recent days or in the era of smartphones, there are hardly any keys left on the cell phone. But, in such cases, if there are any keys, those are neglected and overall body of the cell phone is meshed. So, by approximating that, once you mesh it in 3D, the normal stresses, in such cases, and the normal strains, if they reach any plastic region for that particular material, usually, they consider that there will be a failure in such region.
So, let's say, if you drop a cell phone from 6 feet, if you see a permanent crack on the cell phone body, that is a plastic deformation. If the cell phone cannot come back into its original shape, obviously, that is a plastic deformation. And those are something that they would check for in their drop test. Now, in such cases, 3D elements find a good application. For biomedical purposes, obviously, because the studies or the level of study or the details of the study, way too high. And that is why biomedical structures, they usually have 3D elements.
And then, in the automotive world, obviously, the dummy and the seat foam, those are very critical components where 3D elements are being used. So, obviously, whenever you use 3D elements, there is a huge time that is going to be involved in solving them. The calculations for 3D elements right from time step are very different. That adds complexity to the problem. It adds somewhat extra load on the solver. Solve those equations and then get to the result. But in the end, the accuracy of the result may be higher than the 2D elements.
Now, as I explained earlier, from application to application, the difference between the 2D element result and the 3D element result may be very small or may be huge, such as in these cases. It depends on case to case which could be the best application for 3D element. In general, 3D elements can be used wherever you have thicknesses more than 6mm and you have continuously variable thicknesses. Somewhere in an application where you want to study the normal stresses, such as this case or this case. In such cases, 3D elements are very useful.
Now, this is the case where your thickness is neither constant and way too higher than 6mm. So, that's why it finds an application for 3D element. So, solid elements, as we have seen them during our meshing exercises, we have seen mainly tetra 4 elements and the brick elements. The one which we studied or the one which we made were first order elements. But they can be easily converted into second order, that is quadratic elements. So, tetra 4 becomes tetra 10, that is the element with 10 nodes instead of 4 nodes and brick 8 nodes gets converted into brick 20, that is brick 20 nodes.
As the name suggests, tetra 4 and the brick, they are linear formulations, whereas tetra 10 and brick 20 are quadratic formulations. And then, in the brick elements, since one of the exercises, we saw that we created the 2D mesh first and then we converted into 3D mesh over the thickness. In such cases, if your 2D mesh has any tria, that tria will get converted into a 6-noded brick element. And now, that 6-noded brick element is called pentahedron, which is, in solver's understanding, is more like a degenerated hexahedron.
So, for the solver, it is still a hexahedron, that is a brick element, but its shape has been morphed so that this node 5 and 8 have been deformed so much that they are meeting node number 6 and 7 respectively. So, obviously, not a good idea to consider it that way, but that is the way solver is going to consider that. That obviously tells us that these are the kind of elements that we want to avoid right away. So, it has been seen in many solvers, not just radios, but even other explicit or even implicit or linear static analysis, that whenever you are trying to use 3D elements, either go for brick or go for tetrafore, but try to avoid brick elements or the pentahedron element because those are the most unstable elements among solid elements.
Compared to shell elements, the geometry here is being defined by the volume enclosed by the nodes or node locations. Whereas, in case of shells, the plane defining the three continuous nodes was defining one side of the shell and the two common nodes out of those three and the other fourth node will define another plane and that will define the rest of the area of that element. Now, if those two planes or those two areas are not collinear or not in the same plane, then you run into warpage issues.
So, if you remember that correctly, in this case, warpage obviously doesn't exist because here we are considering a volume and not really a plane. So, in case of tetras, obviously, we had seen that there is a problem of tet collapse. That is, this node, it's way too close to the plane defined by other three nodes. The other way around, this node might be too close to the plane defined by these three nodes. So, such are the cases where tet collapse is a crucial quality criteria. We saw linear formulations, we saw quadratic formulations.
Obviously, they have their pros and cons. Linear formulations being very, very time sensitive or very economical in terms of time and memory consumption. They also have less integration points, larger time step because of that. That is why they are, they are economical in terms of time. Whereas, quadratic elements, there is better accuracy. But, for accuracy, we are paying in terms of time and memory consumption. Moving ahead, since we were mentioning about the time step calculations, this is just a glimpse of how critical or how complicated the time step calculation becomes.
So, if you remember correctly, for 1D elements, we saw that it was simple as L by C for delta T. But now, with C, we have various factors. The alpha is actually a product of kinematic viscosity and density as well as the velocity of sound through the material as well as the critical length. So, this alpha is actually a function of L, C as well as density. Critical length, the definition in this case has changed a bit. Element volume divided by the largest side surface, that becomes the critical length.
That is almost as good as how we saw the critical length for a tri element where we see the maximum, we see the area of the triangle and then we divide it by the maximum base of the triangle. And that gives us somewhat critical length or half, yeah, somewhat half of the critical length. Moving ahead, the calculation of C also changes a lot. In this case, C is not just E by rho, but it is L delta P by rho delta rho. Rho is again density, whereas P is actually the instantaneous deformation or it could be pressure as well.
So, for fluid materials, it is different. For solid elastic materials, the calculation comes to much simpler stage. Now, it is K by rho plus 4 mu by 3 rho. So, K is bulk modulus, mu is the lame moduli or lambda is also called lame moduli. And those are the other types of modulus that a material can have. So, moving ahead, in case of these time steps, I don't especially recommend you to or I don't really expect all of you to remember all of this. But these formulas are just going to give us a glimpse of what kind of complexity is getting involved now than compared to 1D or 2D elements.
So, we move on to defining the property card for solid elements. It is very similar to how we define for shell elements. Just here, in this case, where we were selecting P1 shell, now it is P14 solid. And in P14 solid, again, very similar things are going to be selected. There, in shell elements, we were selecting I shell. Now, here we are selecting I solid. And then there is small strand formulation, a special formulation for tetra elements, how we had one special formulation for triage. Then, how we had some formulation for plasticity and thickness.
This compression modulus or not really modulus, but a number for compression that is ICPRE. CPRE, that is one to look at. Then these QA, QB values, they are for hourglass damping purposes. And then these values are used, in this case, for C calculation. So, these values don't really matter a lot. Most of the times, even if you keep them blank, the solver will assume appropriate values. Whereas, in our case, the main things to look at is I tetra, ISMSTR, that is small strand formulation, and I solid.
So, again, I solid, just like I shell, we had so many options. Here also, we had some options. So, that is the most usual. The most ordinary solid element, 3D element, or hex element, that is brick 8, isolid equal to 1, which is default. So it has only one Gaussian point over the volume, so that's why the integration is really reduced. The cost is the minimum in this case, but then you know that the accuracy of the result may not be that great. Then there is HA8 element, isolid equal to 14. It has obviously a lot more accuracy compared to isolid equal to 1.
That's why the relative cost compared to isolid 1 is 2.5 times. Such is the case for HHC, where it is fully integrated. There are more integration points compared to the first configuration. And in this case, the integration points are actually 2 by 2 by 2, that is 8 integration points right away, corresponding to 8 nodes. Whereas for HA8 elements, the number of integration points really varies a lot, depending on the shape of the element, initial shape of the element. Then there is finally HEPH formulation, which is kind of optimized for reduced integration.
It still has one Gaussian integration points, but though it has one Gaussian integration points, as we studied earlier, the R-glass control algorithm in this case is much better. And that is why even though it has single Gaussian integration points, the element stays much stable. The relative cost is not too high, but it is a good compromise. So, in case of solids, I can't say, just like iShell, that you can, in general, select iSolid 24 all the time. It really depends from application to application. Usually, they either go for HEPH, that is iShell, iSolid 24 or iSolid 14, depending on the application, HA8 or HEPH are used.
Most of the times I have seen HEPH, but even usage of HA8 is quite often, not as negligible as in case of shells. For tetras, just like triads, there is a special formulation. For tetras, you can simply select iTetra equal to 1, and that will take care of it. Now, obviously, iSolid doesn't apply to it, so that's why it is not applicable. But one of the options for tetra will give you linear tetras, one single integration points, that is what we are looking for. Whereas for quadratic options, it will go for 6 degrees of freedom for integration points and much more.
So, this is very similar to HHC and HA8, something of that sort. Going ahead, just to summarize what I said in the previous slide about all these entities, iSolid is going to give you only the hex element formulation. iTetra is going to give you only the tetra element formulation. Smallstrand formulation in solid is again ISMSTR. iFrame, now instead of iPlast or iThick, in case of solid elements, we have iFrame, where instead of selecting the plasticity or thickness card formulations, we are going to select a co-rotational calculation formulation.
So, that is applicable for only hex elements, and it again depends from case to case. But usually, there is one good option, which will work for most of the cases. And if only it doesn't give us good results, or if it gives suspicious results, then only we think of using iFrame for other options. And then HKT, that is for tangent moduli estimation method. Now, because we are dealing with volumes, the tangent modulus becomes effective, and that's why IHKT comes into picture. So, we'll go over them one by one quickly.
As I mentioned earlier, it has single point integration, and it has 8 nodes. So, this single point integration point will be at the centroid of this particular, or center of mass of this particular element. All the results will be calculated based on that. Very inexpensive. For iSolid 14, the number of integration points can be huge. 2 by 2 by 2, or 9 by 9 by 9. This option can be selected. Because of so much detailing, there is no hourglassing, there are no zero energy deformation modes.
That is really a great part about this particular formulation. That is why there are applications where this is still being used, whereas this one, where the viscous hourglass formulation is being used, which kind of causes a permanent deformation in the calculation method, can create some issues in case of hourglassing. So, obviously, the iSolid 14 comes at a cost. The cost is really too high, 2.5 times the first one. HHC, the number of integration points is fixed, 2 by 2 by 2. Because of that, hourglassing is negligible, or there is no hourglassing, we can say.
And that makes it expensive. Then comes the iSolid 24. Improved and reduced integration, just like iShell 24. Single integration points, but the hourglass stabilization method here is based on the stiffness, and that is why it keeps the element stable, even in high deformation situation. So, obviously, depending on the result, the approach usually followed is, they will select iSolid equal to 24. They look at the results, and if the results don't have the kind of accuracy they were looking for, or kind of the variation they were looking for, they might switch to iSolid 14 or 17, and then they would finally make a conclusion.
But most applications where your solid elements are not undergoing huge deformations, iSolid 24 does the trick. If only in cases where you are undergoing huge deformations on some particular solid element, in such cases only, it will be a good idea to go for 14 or 17. Then we come to iTetra. We are looking for single integration points, linear formulation. So, for that, iTetra equal to 0 does the trick most of the times. If you have iTetra equal to 1, that is, in fact, going to do the same thing.
But in that case, the degrees of freedom changes a lot, and the number of integration points becomes 4. So, it is more suitable for 10-noded Tetra elements, that is, Tetra 10 elements. That's why it may not be recommended all the time. So, just to summarize, for default purposes, you always go for iSolid 24 and Tetra 4 equal to 0, that is, iTetra equal to 0. Then comes the next small strain formulation, just like how we did for the previous case. We want a large strain formulation, full geometric nonlinearities, which will be by default selected if you keep the value 0 for this particular entity.
And then there are other options available, depending on what kind of material and application there is. If you select small strain formulation equal to 10, that is, specialized for total strain calculations, especially for foam and rubber materials, where the strain or the way the strain is getting developed is way too rapid. And that's why you need a special kind of formulation in such cases. Then, the coordinate system. So, if you calculate everything in global coordinate system, obviously, in case of large rotations, can get confusing for the solver because this is a 3D element and it can bend within itself, by itself.
Those kind of bending behaviors are actually subjected to rotations of the nodes. For that purposes, it is actually a better idea for the solver to select a local coordinate system that is completely based within the element. And once it gets done with all the nodal calculations, then that matrix can be transformed into a global matrix. So, for the local or for more accurate and stable calculations, iframe equal to 2 becomes a good option to select. Iframe becomes 2 by default if you select isolid equal to 24 because it is default for HEPH elements.
Then, R-glass tangent modulus default, which is elastic modulus or numerical tangent modulus estimation, that is fine usually. It is really an estimated quantity. But, in case you have huge strings getting involved, such as the case of seeds or such as the case of foam or rubber materials, where you are undergoing high deformations, in such cases, you might have to use IHKT equal to 2, which will involve larger calculations because now the tangent calculus estimation is advanced. But, again, that is required for better results or accurate results.
So, for default purposes, whenever we are starting a simulation, always go for isolid 24, IHKT equal to 0, and then small strain, frame, and IHKT equal to 2 for default purposes. Once you get a set of results, that result itself will indicate you what to do with what particular part. So, obviously, whenever you have solid elements involved, there are certain parts where you expect large deformations and you should look at the results there and then you should decide whether to change these or keep it constant.
So, even in case of solid elements, all these things can be set using a def solid option where you can set all of these for once and then just like I mentioned earlier, for every solid property, you can either give it a local value 24 or if you keep it 0, then it will refer to def solid card and there it will go to by default value that was 2. Same goes here for iframe. Now, because it was 0 here, it will go for the default card, def solid, and iframe was equal to 2 for there.
So, it will go for 2. But even in cases where isolid was equal to 14, this will be applicable. Whereas for isolid equal to 24, iframe, whether you keep it 0 or 1 or 2, whichever, it will go for 2 in the end. And then come the rest of the things. So, for foam materials, as I mentioned earlier, there could be different options to be selected. So small-strand formulation becomes 10, frame and HKT becomes 2 each. And then Isolid is still 24. It might need a change depending on what kind of deformations we see.
Usually the dummy elements might need Isolid equal to something else. So for foam materials, single-point integration with viscous for hourglass formulation is fine. So here are the recommendations for foam materials. For rubbers, these are the recommendations. So you can definitely refer to these whenever you are trying to model a material for foams. So that concludes our solid element cards. Really it was quick because there are only 4 things to discuss. And all of them have a reference to shell elements. If you understood the shell element card properly, then this is pretty easy to pick up from there.
And that is how the rest of the radio studies will be. Once you understand this process well or these parts well, then rest of the parts are actually going to refer to these things again and again, the speed at which you can learn radios, rest of the radios will increase. Then we come to 1D elements, which we can continue in another video. Thank you.
Part 5
In radius, there are particular forms of 1D elements that we commonly use, beam, truss, and spring elements are the main 1D elements, the deformable 1D elements that we use. And then in the rigid arena, there is one single rigid element that we use, which is equivalent to RBE2 formulations of usual cases. If you have studied static analysis, then usually people get confused between RBE2 and RBE3. So, yeah, in this case, the rigid element that we keep referring to corresponds to more closely with RBE2 than RBE3.
So, moving ahead, if you recall during machine exercises, what exactly we did with all these element types, those are pretty easy to pick up, pretty easy to understand for their element formulation. Because there is no complexity such as R-glass or calculations during high strain or higher deformations. But these are only 1D elements. The calculations are as simple as they can be. So, for truss element, for example, the calculations are so easy. If you look at the time step, for truss element, all the time steps are actually quite resembling to the formula L by C.
Where L was your characteristic length and C was your speed of sound through the material. So, delta T for truss element becomes L of T by C. Well, L of T really, for truss element, it actually is the cross-sectional area and then the characteristic length. Then C, the calculation is simplest, E by rho. The one which we have remembered all over the time. What I would recommend here is you should really remember this kind of formula, E by rho, which is pretty handy to remember. And then it will give you a quick idea where if you change a material from A to B, you will know its values in terms of Young's modulus and density.
So, how will it affect the time step in general? You can gauge that based on this particular formula. If the C is increasing or decreasing, then you can see the effect on delta T. And then you can predict what will happen to the simulation if you keep the L, that is mesh size, same. For beam elements, again, it becomes very much similar, L by C. Only in this case, you have the cross-sectional area. The cross-sectional area has its own formulas to calculate from. Too many details to look at.
Don't worry about them. I have included those just for curiosity purposes who are really curious to know how this A came from and what this F1 and F2 values have come from. But I won't really push for you to remember all of this. But just in general remember, for 1D elements, because those are the simplest, L by C and where C is equal to root of E by rho. That are enough details to remember. For spring elements, the things change a bit. You have a mass assigned to it.
And then there is stiffness, which is pretty much local. And the stiffness can vary over the time, over the deformation. So, the time step calculation really depends on that. And then there can be a damping as well. So, if you have a spring damper combined into one single spring, there is a special formula for time step calculation. And as it mentions in the slide as well, the K and C values will depend on the spring type. If the spring is linear, these values will stay constant.
Whereas, if the spring is non-linear, then K has its own formula, C has its own formula depending on their curves and the type of loading. Then there are multiple direction springs that you will be able to define in radius. Where for one particular spring element, it is not just the linear stiffness, but the bending stiffness will be available to determine or apply. Apart from bending stiffness, the torsional stiffness, and rest of the stiffnesses, that time step in such cases, wherever you have multiple modes of deformations combined into one, the time step will be the minimum value of each direction.
And that is pretty much simple to understand and pretty much logical. For rigid bodies, the computed master node has its mass and inertia. And then you select few options in the rigid body formulation that will decide whether the slave node mass is to be shifted to master or they are supposed to be maintained at slave. And that is going to affect the time step calculations. But in general, whether you make that change or not, because there is no deformation that is going to happen in a rigid body, the time step is going to be huge.
Because the solver knows that as long as it is able to calculate the motion of master node, all the slave nodes need to be applied the same motion or same rotation throughout. And then it saves a lot of calculation for the whole element or rigid body element. Because of that, rigid bodies are the easiest for the time step calculations. So coming back to the truss elements, now we are going to go into more details into the cards. For every slide until now, you have seen a title prop type 2 or prop truss.
Those are the, these are the text that you will see in the starter input file. Whenever, whenever HyperMesh writes out any file, you will see these kind of details in the file. This is more like the code syntax. So when we say a truss element, thing about truss is that you can apply it a force only in one direction. It has only local N1 to N2 direction, whatever is going to happen, it is going to happen only in this direction. Rest of the, rest of the directions are not really computed for and that's why they don't really happen.
As long as you have a cross sectional area defined for the, for the truss, it is going to behave well and good. And that area will be used for any inertial calculations that are required in a bigger body. Then we move to beam elements. Now beam elements as we saw earlier, it can be defined with three, three nodes. And because of that, the orientation becomes a thing to look at. And apart from that, because you have an orientation, there are three different axes, three different directions and only common thing between them is the area or the cross section.
The moment of inertia really differs from all, in all three directions and that really affects the time step calculations a lot. And also rest of the calculations or the understanding of the whole problem. So obviously beam gets defined with three nodes to start with, but after that, the small string formulation comes, then there is a damping factors, but right after that, we have a cross sectional area. Now this, instead of this area, you can always define your length and width of the cross section and it will calculate the area by itself.
And then there is a inertia values depending on what area is calculated on this case. Then we come to the springs. In springs, there are so many types, it can get confusing. To keep it simple, just keep looking at these pictures over here. If there is a linear elastic spring, you'll have infinite deflections or deformations in the spring possible. And because of that, the stiffness of the spring will go on increasing or decreasing accordingly. Non-linear elastic springs, because they are elastic, once you unload them, they are going to come back to zero-zero situation.
Non-linear elastic spring can be defined with a curve or a graph, which will tell the solver how to follow the path for that particular spring. Then there are elastic springs with isotropic hardening. The hardening really changes the stiffness a bit in the non-loading region. Because it has hardened, there is a permanent set, a permanent deformation that has happened in that case. And because of that, while coming back in the unloading curve, it might follow a different path. Same goes with the rest of the formulations. So mainly in our case, we'll be keep using linear elastic or non-linear elastic springs.
Because those are the two which we can completely control and model them the way we want. So while defining the spring, the card of the spring element property is going to ask for any mass and mainly the stiffness. And then the spring behavior flag, H, that is going to tell us what type of spring we are going to refer. So if you select H equal to zero for linear or non-linear elastic springs, it is going to do simpler things. Now for H equal to four, it is going to follow this kind of path, which is more practical in a professional world.
And then there is a function ID. So when you have H equal to four, this curve and this curve needs to be defined by a function. So that is why a function is or a curve is getting loaded over here. Then we come to type 13, that is beam type spring. And those are actually the most critical type of springs that you will have to study. Now in case of type four spring, we only had this kind of complexity, whether to choose it linear or non-linear.
And then we in the end found out that a same spring behavior flag refers to both of those. Whereas for spring beam, because we can define it with two nodes or three nodes, the degree of freedom also changes a bit. It is not constant. It depends on what kind of property you apply to that particular spring beam. And then it will start behaving that way. So with this spring beam, obviously there are a lot of details that are going to be calculated, such as bending, shearing, because now you have multiple degrees of freedom to each node in the beam.
The beam is going to bend by itself or the beam might extend or undergo tension. And because of that, the failure parameters sometimes are added and many times it is pretty common for analysis engineer to look at the elongation and the strings and the forces inside a spring to get a clear idea of what is happening with the system currently. So this is all about element property cards. We'll soon start applying all of these when we go on in creating models. For now, we might shift our focus to materials in radios.