Is it possible to simulate additional screw tightening by turning it through an angle (nuts)?
So, for example:
Thread M5:
thread pitch P = 2mm
angle tighten the nut = 60deg
delL = 60/360*2 = 0,166mm
Pre-tension can also be defined as prescribed displacement (*BOUNDARY) instead of force (*CLOAD). But it’s typically done once and then frozen so that actual (operational) load can be applied.
Hi Rafal,
I think it is possible. At least the bolt tension by turning. Need to try with pretension to see if pretension surfaces slip each other.
EDITED: It works and the two pre-tension parts keep tied.
May I ask you, why do you need pretension?. Is it to avoid too much turning and reduce computation time?.
If parts are assembled almost at its final position with threads very close each other , required tightening force should be achieved very fast with a small turn without need of pre-tension.
Maybe an initial interference fit between parts could provide the required pre tension.
That can be a lot of computing time but has shown to be converging easier than I thought.
In this case I have fix the bolt head and nut base. I’m just turning the bolt to see if it can pull the nut and it worked.
If you want to simulate tightening by actually rotating a screw with a modeled thread then it’s doable but avoided in most cases due to high computational cost. I’ve done such simulations for dental implants in Abaqus because pre-tension load is not supported in explicit dynamics and this kind of analyses was chosen due to complex contact conditions (the implant had quite tricky geometry). You have to be careful since there can easily be some snagging in contact between the threads. I wouldn’t advise this approach in place of pre-tension in most cases.
¿How could someone increase the tightening force of a joint but just after some operating condition has been reached?.
¿Is it possible to apply pre-tension two times?
EDITED: Seems it is not possible to pre tension twice.
*ERROR reading *PRE-TENSION SECTION: *EQUATION should be placed before all step definitions
*ERROR in calinput: at least one fatal error message while reading the input deck: CalculiX stops.
That could be one reason why this technique is useful.
it seems the load is too small when i tried to model of bolt with 10mm diameter and 50mm length.
case 1
case 2
case 3
multiple initial load by ten times larger,
Model without thread geometry, I’m considering the options:
x2 = x+P
After tensioning with the *PRE-TENSION command, use thermal shrinkage to shorten the bolt also by one thread pitch.
Modifying the contact so that after tensioning the bolt, the bolt nut is moved away from the contact surface by 1 thread pitch (is such a thing even possible?).
my previous example is a simple test, second step should not displacement boundary condition since pre-tension is a reversed action. Thermal induction can be used by equivalency, shrinkage movement will restrain due to geometry fit. Not really sure if this occurs for model with separation and overlap.
More generic model is something like below figures, it’s a couple force or displacement at end of bolt and nut surface. Sliding contact is assigned at their interfaces.
interesting example of bolt pretension by turn-of-nut method, coupling of rotation and translation displacement without threads in models (courtesy of Altair)
This seems to be the best option considering the fact that pre-tension can only be done once in an analysis. After all, thermal expansion is how pre-tension used to be simulated back in the days.
My small test in ANSYS:
and without mesh too. I think it is called SimSolid, and I have no idea how they perform the analysis without meshes and boundary conditions.
Their approach is explained here: https://www.inneo.co.uk/files/content/product-development/calculation-simulation/simsolid-technology-overview-whitepaper.pdf
it seems SimSolid share the similarity with traditional FEA including boundary conditions, only in mesh is different.
my example approach based on couple of force or displacement at nut and bolt end surface. However, SimSolid use advanced couple of rotational and translational at nut and bolt perimeter interfaces. Refned the model example at the same surface interaction, theoretically will yield in similar results.
I think the way to do this is explained here for Abaqus: Bolt Pre-tension Techniques in Abaqus - Learn FEA Second Technique: Translator Connector
to implement this, a translator connector has to be defined in CCX using equation or User-defined nonlinear equations which is not an easy task, but maybe worth working on it.
it seems Translator Connector of Abaqus in example link given could be similar to Tightening approach in SImSolid.
