I would like to get a better understanding of how the Fictitious Clearance works. If my geometry contains a gap of 2 mm and I apply a fictitious clearance of 1 mm. Will the solver force the gap to 1 mm or 3 mm?
Do bonded contacts have to physically touch?
Global contact setting
[German Workshop] Step-by-Step (Session 2) - Nichtlineare FE-Analyse einer Flachdichtung
Import Separate Solids into SimScale
basically when adding a Fictitious Clearance to a contact surface, we add a layer of a fictitious material (with no additional stiffness) with the defined clearance as thickness. On an algorithmic point of view, when it comes down to compute the (signed) contact distance, the solver removes from the actual geometrical distance the fictitious clearance and the result will be used to evaluate the contact state (open/closed) and the contact forces.
So, if your geometry originally has a gap of 2mm and you apply a fictitious clearance of 1mm, the solver would compute a remaining gap of 1mm. After moving one part for 1mm the contact will become active and contact forces will start acting. Using an exact contact algorithm (Lagrangian), the gap will never be smaller than 1mm.
Does this explanation makes sense to you?
Roller bearing - Dynamic analysis
Comparative simulation of two beams producing nonsense result, or failing to simulate
that makes sense.
So if my geometry contains an overlap of 2 mm and I apply a fictitious clearance of 1 mm, the two surfaces will move a relative distance of 3 mm to produce a final gap of 1 mm.
I created more runs using “Fictitious Clearance”, for example: https://www.simscale.com/workbench?publiclink=dc509247-35c2-40f5-85fb-b93c64056a34, or https://www.simscale.com/workbench?publiclink=dc733a48-9048-4869-88aa-8da225260178
In these simulations I modelled different bolt connections with pretension. I wanted to set a gap (pretension) of 0.1 [mm] (1E-4 [m]) between the bolt head and the compressed part. The Fictitious Clearance was set 0.0001*t, while the simulation time was 1 sec. After the calculation I checked the results and I have seen pretty similar results in both cases; the displaecement between the bolt head and the top of the compressed part is almost the same: 4.2E-6 [m] and 4.1e-6 [m] respectively, which is much much less compared to the value what I would like to see (1E-4 [m]). There has to be something what I misunderstood here with this Fictitious Clearance option, please help to eliminate the problem!
Please see below the result plots of two independent runs showing up the same phenomenon:
Thanks in advance for your support!
the problem lies not in the definition of the fictitious clearance, but in the contact type. You are using a penalty contact, which always has penetration of the contact surfaces. A higher penalty coefficient will decrease the inter-penetration, but it will never vanish.
In your first example you have a run called 1srhighpenalty, where I assume you increased the penalty coefficient to see if it has an influence on the results, Unfortunately you forgot to change the value for the contact Bolt-Plate, which has only a value of 1e11, which is not much compared to the stiffness of the involved materials (steel E=1e11).
The penalty value should be about 5-50 times as high as the materials Young’s Modulus.
Increasing the penalty coefficient should improve your results drastically. On the other hand the convergence might become harder and some high value it won’t converge at all.
To check the contact clearance/penetration you can add the contact results global field in the global fields to your run. It has a component called “JEU”, which is the contact clearance on the slave side.
Finally you could try the augmented Lagrange contact type. It does not have contact penetration at all, but is hared to get converged, especially if friction is activated.
Thanks a lot for your hints! It is right what you mentioned, I tried it and the results became different, however I didn’t checked yet what are the exact values.
Do you have ideas what kind of options do I have to modify or influence to get convergence with Augmented Lagrange in frictional contact?
And what can I check in the log file to learn something about my model conditions?