Rigidity of GAP elements in contact
GAP element rigidity will depend on the material of the parts in contact... and also on the mesh size! Learn how to calculate it!12 December 2022
If you have a thermal load in structural design, the standard practice is to reduce the values of material properties. But that may not be enough!
While thermal load itself doesn’t cause stresses, it causes elements to expand or shrink… Stress appears when you block that deformation, and it can be huge!
In this post, we will tackle the most important things about thermal loads in structural design. And in the end, I will tell you how this knowledge allowed me to save a pressure vessel.
Let’s dive in!
When you heat something it extends. I don’t know if you had this “ball” experiment in high school. The teacher would put a metal ball on a string through a circular hole. And then would keep the ball over the candle to heat it. As the diameter of the ball increases, it can’t go back through that circular hole. That’s the idea!
If you would check, there were no stresses in the ball… it just got bigger.
And this is why in structural design, a bigger focus is on the material properties. As you know, when you heat a metal, it actually becomes weaker. On another hand, if you cool it, it becomes more brittle.
This is why many codes provide values of yield strength and Young Modulus of metals in higher temperatures. It would be lame to forget about that!
Firstly, we should take a look at what material properties we will observe. Then we can focus on how those properties change in elevated temperatures.
We usually think about “yield strength” as a measure of steel capacity, and there is a good reason for that! Normally, the stress-strain curve for steel shows a nice plastic plateau. We usually denote the stress level when this happens as fy. For sure, this is the very nice “measurement value” we very often use in design. In fact, it’s so cool, that we often “ignore the rest” of the stress-strain curve. We simply extend the plastic plateau to be longer:
But this is not all! I should mention that for austenitic steels we can’t really measure “yield strength”. Simply… because those steels do not have a plastic plateau!
Instead, we use a 0.2% or 1.0% proof stress (usually denoted as f0.2 or f1.0). We do that, simply because there is no “real” yield stress. But some folks call those values the “yield stress” anyway, and I’m not a fan of doing that.
Just so you know, this is how the stress-strain chart looks for those austenitic steels:
Before you ask, the code you are using should inform you which value (f0.2 or f1.0) you should use. Neither of those is “better” of course. It’s just a number we use to “describe” the material curve (and both do the same job!).
Of course, calling those “yield stress” is not accurate. Since proof stress of 1.0% means… that after unloading 1.0% of plastic deformations remain! So clearly, this is not the “stress when the yielding starts”!
Now, since you already know what we want to measure, it’s time to see how steel parameters change in temperature.
Normally you would see this information in tables. But I actually draw charts to show you how this looks (somehow I always understood things better with charts):
As you can see, as the temperature increases both the yield stress and proof stress decreases.
With a yield strength of S235, the thing is pretty obvious. You just reduce the yield strength in your material model, and move on! Since this steel has a clear yield strength I used the same values on both charts. Values for S235 come from an “old Polish structural steel code”. I literally had it near me when I was writing this.
It may seem that with proof stress thing is a bit more complex.
If you are using formulas for design, nothing changes. Firstly, you need to know if you need to use f0.2 or f1.0 in the code procedure. Then you simply take the reduced value, and things are fine! I took those values from EN 10028-7 (lots and lots of tables for steel grades used in pressure vessel design).
It’s a bit more complicated if you want to use the austenitic steel in FEA… You won’t model it with the bi-linear model. I guess you already saw, that it’s hard to find two lines on that stress-strain chart! So, you will most likely want a stress-strain chart to import into your FEA model.
The thing is, that you don’t have a chart showing the stress-strain relation for your austenitic steel at high temperature. You only have f0.2 and f1.0, which are only two points on the chart.
Luckily various codes (like EN 1993-1-4 or ASME VIII div.2) simply provide you with equations to help you. Those equations will allow you to “calculate” the curve, based on the data you already have. Realistically… you would do the same thing for normal temperatures as well. So effectively, it’s the same thing!
And at the very end, this is the chart for Young Modulus changes in temperature. I used the same codes as before, and I’m adding this just for the “completeness” of data. Of course, Young Modulus decreases as the temperature increases – no surprises there:
At this point, I think that the conclusion is obvious!
When you have a high temperature in your structure, you should reduce the strength of the steel you use in the design!
My professors said that the “limit” temperature when this becomes important in structural steel would be 70oC. But I’m not blind to the fact that EN 10028-7 provides values for 50oC as well!
And I feel that this is something, everybody is doing – or at least I hope so!
Sadly, this is not all!
I’ve recently done a cool pressure vessel design, and I will use this as an example here. It just fits perfectly (in fact the design motivated me to write this post!).
I will start a bit differently. We are about to wonder why people ignore the “not so obvious problems” in the first place! And then we will think about what to do about them!
As I wrote in the beginning if you heat something it expands. This doesn’t cause any stress in the element… as long as it can freely expand. And I think that this is the “base” for the common habit of ignoring the problem.
Take a look at this pressure vessel:
As you can see, it stands on rather thin legs. Don’t worry it’s somewhere inside a building, so it’s not such a problem as you would think.
If I would heat the legs alone… the vessel would simply get higher. Literally, nothing else would happen (apart from the reduction of material properties of course!). But you don’t have to believe me – check for yourself!
This is an animation of von Mises stress in a model where only gravity and temperature of legs are present. This way I hope you can easily see what changes:
A thing gets a bit more complex when I would actually heat the vessel. This would be a “real” load case too. I’ve heated the legs, just to show you what would happen!
As the vessel increases its diameter (due to temperature expansion) you can see that this bends the legs slightly. However, those are not extremely rigid columns! Moving them “to the side” for a few millimeters doesn’t require a lot of force!
This means that while they “resist” the increase of diameter in the vessel… they don’t resist all that much! And as such, this small resistance will only generate small stresses in the structure. Stresses that we could potentially ignore!
I don’t want to discuss if those stresses are “big enough” to worry you or not. The reality is, that adding temperature load as “load” is not a common practice in structural design. I feel I have to admit that in many cases… for a good reason!
Simply put, if your structure can deform quite easily, temperature most likely won’t cause many issues!
Your structure will just deform a bit and generate some small loads in itself in the process. And things will most likely be ok!
If you are unsure if you can ignore temperature or not in your particular case… don’t ignore it! Just add that load to your analysis, and see how much things change. After some time, you will get a “feel” for this I’m sure.
You most likely noticed on the gifs above, that the legs have a zone, where stresses are suspiciously high. To be honest, there would be no such stresses in reality. I used this occasion to show you something as a side note.
When you load a portion of the structure with temperature (but not the entire thing), it is a bit complicated. There is a “border” between the “hot” and “cold” material. A place where both of those materials touch.
In such cases, the “hot” material (column in the first case) wants to expand. Of course, the “cold” material (very top of the column below) doesn’t. This will also produce significant thermal stresses, that you can easily see below:
Of course, you can observe the same phenomenon in the “other direction”. When you heat the vessel (and the very tip of the column) and not the columns themselves:
This is the source of those weird stresses you could see in the animations before.
I’ve decided to make the “temperature jump” on the column itself as you can see. It may seem that the place where the column connects to the vessel would be a more “natural choice”.
I did this to show you this phenomenon very clearly this way. I’m aware, that it would be less obvious in the connection area. But if I would be in a hurry in actual analysis, I would still go this route. After all, I perfectly understand that this “would not happen” in reality. And those “fake stresses” would not mix with the actual important stresses in the support zone.
Of course, in reality there would be a temperature gradient (so no “super sharp temperature drop”).
Loading your model properly (so including this gradient) would solve the problem, of course. But I think it’s worth knowing that simplifying thermal loads in FEA models may lead to such funny results. At least they won’t surprise you when this happens.
So far, you know, that most likely temperature won’t do much hurt if your structure can easily deform. Also, modeling thermal loads in a simplified way leads to problems.
So, why bother modeling the thermal loads, and bother with convergence and all that? I have to admit that in a reasonable amount of cases there is no point, but…
…I’m never a fan of “blanket statements” like “just ignore temperature load and live your merry engineering life!”. Because you can ignore stuff only based on your extensive knowledge in the field. Definitely not because you don’t know how to handle them!
Why? That’s actually simple!
Take a look at this second vessel. It will also be heated, the only difference is, that it’s welded to a steel structure that won’t deform. Let’s say this is because horizontal bracing is attached to each support point:
Let me mention one thing in case you want to be very accurate. I understand that we could consider some heat traveling through the supporting brackets to that supporting steel structure. It could potentially cause an extension of that structure, reducing the loads. But let’s ignore that to just discuss the “raw problem”. I don’t think that this effect would play a significant role though.
In the end, this leads to the assumption, that we have rigid supports for the vessel in the horizontal direction. The tangent direction isn’t as important – it all happens in the radial direction, to be honest.
This is what happens if we start to heat the vessel in this case:
You can see how the shell takes additional stress. But what is even worse it deforms to the inside! This would be a serious issue if the vacuum in the vessel should be considered. Such inward deformations really reduce the shell capacity due to circumferential buckling.
As you can imagine, the higher the temperature, the more deformations happen. This would lead to a lower buckling capacity in the end.
There is however a simple solution to this problem. You can provide the sliding support in the radial direction on each support. Welding of the brackets won’t be acceptable then – we will use bolts in long holes (in the radial direction).
We don’t have to model all that of course! We can simply assume that there is no radial supports on the brackets. There is no need to worry about modeling bolts and long holes, etc. And this is what we would get:
You can see that something is still happening near the brackets. They are restrained in the transverse direction and obviously more rigid than the “average” portion of the shell. But the effect is greatly reduced for sure.
Thanks to such FEA analysis, you can not only see that this “works”. You would also be able to check, how much the vessel expands. This would allow you to check how big “clearance” (movement possibility) you need in the support to make this effective.
Of course, you can always “guess how much “free movement” you need. If you would be not sure, you could then just add more clearance just in case. But FEA allows you to calculate this accurately. Especially since “adding more clearance than needed” is not always obvious, as you are about to see!
What youve learned so far is:
Thermal loads don’t mean much in structures that can easily deform – they will simply deform, and produce rather small stresses in the proces.
If you are not sure if your structure is sufficiently easy to deform – just add the thermal load in FEA, and see what will happen.
If your structure is “rather rigid” and won’t deform easily, make sliding supports that allow your structure to extend without issues. This greatly reduces potential problems.
In essence, I told you that most likely you don’t have to analyze thermal loads in structural design. All you need is to know that your structure “can easily expand under temperature”. And if this is not the case, just make the expansion possible with sliding supports. And in the end, remember that the material properties change in temperature.
All of the above is true. But, I have to admit, that this article could be much shorter if that would be the only takeaway…
… it gets better!
So far, we only needed FEA to check how much “free movement” we will need on supports. This essentially allowed us to ignore the thermal load in a rather rigid structure! Let’s face it – you could guess this. And if you don’t like guessing you could take the value folks in your company always use. In the worst-case scenario, you could even do some simple hand calculations to check this!
The fun really begins when you actually can’t have sliding supports!
It’s all cool to say, that you just make a “sliding support” and be done with the problem. Sadly, this is not always an option.
And this goes beyond the normal “structures have to be properly supported” argument.
I was hired once to analyze a vessel that got really bent during welding. As you can imagine such work is NDA protected, so I can’t really show you the entire model of that vessel. But I can show you a deformation around one of the brackets under load (and imperfection influence of course):
The problem was, that it was supposed to be vacuum certified! Clearly, the circumferential deformations due to welding were really a problem. Especially since they were bigger than allowable in the code.
Sadly, there were also thermal loads in the vessel, and this meant that the situation looked like this:
As you can see, there was no easy way to say, if the radial supports were good or bad for the vessel. Of course, things got even worse, when I did the initial verifications:
This is why I’ve checked the capacity of the vessel with 1mm, 2mm, 3mm, etc. gaps in the radial support. The assumption was, that vessel capacity was a “function” where both thermal effects and buckling impacted the capacity. I just wanted to see the “maximum” of that function. Obviously, I knew that on the “edges” (radial supports yes/no) the vessel is too weak. But I hoped that it may be still ok, somewhere “in the middle” (with semi-rigid radial supports).
I didn’t have a way to change the radial rigidity of supports easily. That would impact the elements that were beyond my influence (structure on which the vessel was supported). So instead, I decided to make the gaps in the radial direction. By making them “bigger and bigger” I could make the radial support “softer and softer”. It’s not a perfect way to change rigidity, but this is what I could do at least.
This actually works of course, as you can see on the chart below. It shows how the radial reaction force on one bracket drops, with the increase of the gap clearance:
So clearly, increasing the gap clearance in the radial direction makes the support “softer”. This is such a fun phenomenon. At the beginning deformation of the model (mostly due to thermal expansion but not only) are “free”. Thanks to the clearance they cause no reaction force. But when the gap closes, the rest of the deformation is “blocked” and this produces reaction forces, stresses, etc.
This means, that by steering how much initial gap I have, I could make the support more or less rigid. Well, at least if you would measure rigidity by the final value of the reaction force!
Quite to my surprise, the “optimal radial gap” was 3mm, and the vessel had sufficient capacity in that case!
The only problem left was to figure out the system that can block the radial movement so accurately. Of course, normal clearance in bolt holes was definitely not an option. But it wasn’t a hard task either. And finally, the vessel was “saved” from scrapping, saving my Customer a lot of money and missed deadlines!
Sure, oftentimes ignoring thermal loads in analysis makes sense. Something will just expand, maybe cause low stresses in the process, and effectively nothing will happen.
Other times, the solution will be simple! If the structure is rigid just as its supports, make sliding supports if you can! This way, your structure will expand nicely, and nothing will happen! You can of course guess or estimate the needed “clearance” – FEA can help you here as well.
But the use of nonlinear FEA shines in more complex cases! Structures are often super complex (duh!). There may be cases where you won’t be able to simply make sliding supports. This can happen either due to stability, or you will simply need that support to transfer loads! This is where analyzing the structure in detail becomes a necessity! And in those cases, you simply cannot ignore thermal loads! They may govern the design!
There are a few things I think you may want to remember from this article:
And a fun fact at the end. Did you know that the thermal expansion coefficient of the steel material also changes with temperature? This means, that the steel expands more (per constant temperature increase) the hotter it is. This is arguably not the most important thing, but it’s worth knowing I guess. If you need you can check the “cumulative average” thermal expansion from 20oC to a given temperature for various steel grades in ASME Sec. II – Part D.
Join my FEA Newsletter