I am currently working on the sizing of a finite element pressure vessel (according to CODAP).
To put it simply, the device consists of two half boxes (cubes) assembled by bolting with a rubber gasket.
My question is the following: how should we model the forces due to the compression of the joint (seat pressure, bolt tightening...)
The modeling and calculation are carried out using solidworks simulation static module. For the moment, I have applied the self-weight and the internal pressure but I don't see how to apply the compressive forces of the joint or even how to define these forces...
If the standard does not specify anything on this point, it is because it should not be dimensional.
A priori, I would say that you can just put rigid connections at the level of each bolt. It will then be necessary to check that the tightening to be applied to the bolts ensures a force at least equivalent to the reaction on each rigid bar (to validate the non-detachment).
Subsequently, the pressure applied by the seal is only the counterpart of the tightening force of the bolts.
It may also be necessary to check the deformation of the flange between the clamping points to ensure that there are no leaks. But it will also depend on the gasket technology used (flat or O-ring, with or without groove, etc.)
The construction code (CODAP) specifies the calculation method but only for circular flanges...
I was thinking of modeling bolt-type connectors (or solid-type contacts) between the bolt holes of my two flanges. Then I thought of applying the compressive force of the gasket (it's a flat rectangular rubber gasket cut identically to the flanges) at the level of the gasket span surface. However, I don't see how to calculate the value of this effort... Do I need the value of m and y (tightening coefficient and seat pressure)?
You calculate the necessary clamping force: seat pressure + pressure force on your equivalent section -> this gives you a minimum total force that you divide by the number of bolts and this gives you your preload effort per bolt.
On the other hand, it means that you will do a calculation with contact management (and that you must be able to have enough information on the material of the gasket to model it). At worst you can always model your gasket in pure PTFE.
Contact management can quickly make your calculation very long (but it can pass).
The big plus is that it will allow you to have the contact pressure all around your joint (you should have nice surprises in the corners).
Make sure you have fairly thick flanges because the pressure applied to the walls can deform them and cause your square flange to become uneven -> loss of seat pressure -> leaks in real life.
You'll quickly realize that it's not for nothing that the bridles are round, as soon as you get out of this geometry it can quickly be a hassle.
The easy solution: an O-ring in a machined groove. Your flanges are in metal/metal contact, you no longer have seat pressure and the 2 flanges deform together if you have enough bolts so your joint is always crushed whatever the pressure in your cubes.
1) If I have a joint seat pressure of 1.4MPa (for the example), I apply a pressure of 1.4MPa on my flange faces (in addition to my working pressure in the box...)?
2) Why model the joint and not only apply this seat pressure to my flange faces?
3) Currently, my two half boxes are "assembled" by a solid-type contact between the bolt holes and a "no penetration" type contact between the two flange faces. Is this modelling coherent?
- I calculated the compressive forces of the joint according to a "circular" flange (according to CODAP C6.5) with a diameter equivalent to my rectangular flanges
- I applied these forces to my rectangular flanges
- I calculated my chamber with these forces as well as the other loads (internal pressure, hydrostatic pressure...)
- I checked that the forces in the bolts were less than the permissible forces
Point 1: the seat pressure is a pressure to be applied to your joint to make it waterproof. You have to calculate with the section of your joint your seat force (the seat pressure x the section of the joint). Then you calculate the force equivalent to the pressure of your container (inner section of your seal x your calul pressure). With these 2 forces you find the force to apply on your flange (the maximum of your seat pressure and the pressure force + m x pressure x joint section). You divide this by the number of bolts and it gives you the minimum prestressing force to apply to each bolt.
Point 2: if you don't model the seal, you won't see what's going on there (and it's the critical place for the sealing). It all depends on what you're looking for. If it's just the pressure of the container it may be enough, if you want to be sure that your joint won't leak it's probably insufficient.
Point 3: if you managed to model like this, you didn't consider the thickness of the joint. The behavior of the mechanical parts should still be quite close to reality but you are still more rigid than in real life. When I had problems with the sealing on oblong/oval flanges, we noticed that the deformation of the boxes due to pressure discharged some bolts (the flanges were getting closer in these places). Your modeling will not allow you to see this kind of phenomenon since your flanges are welded to each hole. The best is to keep the contact option without penetration between the 2 flanges but to simulate bolt connectors at the level of each hole. This will allow you to have the effort in each bolt.
On the other hand, the fact that you are metal / metal between your flanges (without joints) means that they will surely not come off (you don't have the bending in the flanges related to the bolting forces). Putting a gasket in your calculation (even in a material that is not the right one: hence the suggestion of PTFE, but the SW material base also contains rubbers...) allows you to see the bending in the flanges related to the bolting forces. The results of the calculation will still be quite different from the one you got).
NB: if your joint makes the entire contact section of your flanges (i.e. it contains the bolting holes), you will have a big seating force but the result of your calculation will be very close to reality (or the calculation with the joint) because you will have no/little flex in the flanges related to the bolting forces. The contact over the entire width of the flanges will also limit the bending of one in relation to the other. (in my calculation I had a rather thin inner joint compared to the width of the flange, so it made a point of articulation)
In reality, I have a joint with a shore hardness of 70, so I don't have any seat pressure (y = 0 if shore hardness <75).
The joint is indeed a joint on either side of the drilling circle. The CODAP makes it possible to calculate (see attached image):
- HG: The compressive force of the pressure joint
- HT: The force resulting from the action of the pressure on the annular surface between the inner flange diameters and the reaction diameter of the seal
- HR: The force balancing reaction exerted on the assembled elements
- The HD force is already applied to my model through the pressure in the subwoofer.
It is these three forces (HG, HT and HR) that I applied to my flanges (calculated with an equivalent diameter). The objective is to validate the mechanical strength of the box.
I will try to calculate the device with the modeled joint so that I can compare the results.