Prestressed bolt with contact

[n3l3]

Hi all
Im modelling a prestressed assembly with a bolt (taht is attached), the bolt is prestressed with a temperature field over the beam that represents its body.
I´m using 3 contact interfaces, betwen the clamped parts, and the bolt heads and each clamped part.
I dont get errors in the firs step (the pretensioning with the temperature field)

Abaqus has finished the job in some cases in the next static loading steps for some specific dimensions of the part "sector", but when I change the dimensions of the part, "sector" I get an "aborted" error. (The principal dimension I change is the main clamped body depth in the X axis)

Indeed I get a lot of warnings like this:

overconstraint checks:slave node SECTOR-1.19 has prescribed displacements tangent to the master surface. this could make the friction constraint for these contact slave nodes redundant; hence the friction formulation is changed from *friction,lagrange or *friction,rough to the default fenalty method (friction coefficient of 1.E+03 in the case of *friction,rough).

My knowledge of abaqus is starting to finish here, so would be nice if someone can give me some tip.

Thanks a lot.

 

[rstupplebeen]

I looked into your model and I think I have a solution. I have not found the root cause though. I deleted all steps except for the first one. Then made an amplitude similar to your loading that was changing in the different steps. Then I linked the load to the amplitude and solved. I am not sure what this 'fixed' though. I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[n3l3]

Yes it helps. But unfortunately the prestress is not working on the bolt. (At least as I have done) Is like now it works but forgets the predefined field.
would be nice if u pass me your example.

Any way thanks a lot , right now i´m traying to make it work properly in by the way you told me.

 

[portliner]

I copied your CAE and made some changes. It run through all steps.

1. The hole in the "sector" enlarged to 67E-3, the screw is 66E-3.
2. Reduced the model by using two symmetry planes, requires a flat rigid surface.
3. The rod was replaced by solid cell adding to the "cabeza M36"
4. The flat contact surfaces between the M36 and the sector was TIED
5. The contact between sector and the introduced rigid surface of type "surface to surface" and zero friction.
6. Partition of the "sector" to get good shaped elements and reduce the numbers.
7. Second order elements.

 

[n3l3]

Thank you for your help.
I have lernt new useful things with that model.
(the diameter was a mistake, thx = ))
i dont know if the results are ok, because of the tie in the head, and the no friction in the plate, maybe thats two ideal, anyway, im working in it.
thanks a lot!!!!