Problem with pre-tensioned bolt 1

[JulesVerne77]

hi,

I`d like to perform a nonlinear analysis in ABABUS with pretensioned bolts (made of solid brick elements). The model was created with I-DEAS-Preprocessor.

I defined a pre-tensioned section and a pre-tension node for each bolt. The pre-tension nodes are not attached to any element in the model, they are free in space.
In a first step I applied a defined pre-tension force (CLOAD) by means of the pre-tension nodes.

And now my problem, when I run the analysis, a "numerical singularity solver problem" occured at one of the pre-tension nodes. I assume a rigid body motion in the free DOF of the free node. I`ve read the ABAQUS manual a thousand of times, but I didn`t forget anything. No additional boundary condition is necessary in the first step when I use the CLOAD command. But then a rigid body motion of this node will cause an solver problem..

Has anyone any experiences with pretensioned bolts?
Below I added some lines.. please help me..


*PRE-TENSION SECTION, SURFACE=PRE_TENSION_SURF01, NODE=1000001
*PRE-TENSION SECTION, SURFACE=PRE_TENSION_SURF02, NODE=1000002
*PRE-TENSION SECTION, SURFACE=PRE_TENSION_SURF03, NODE=1000003
*PRE-TENSION SECTION, SURFACE=PRE_TENSION_SURF04, NODE=1000004

*STEP,NLGEOM
*STATIC
0.5,1.0
*CLOAD,OP=NEW
1000001,1,18000.
1000002,1,18000.
1000003,1,18000.
1000004,1,18000.
*END STEP

*STEP,AMPLITUDE=RAMP,NLGEOM,INC=100
*STATIC
.2,1.,.001,.2
*BOUNDARY,OP=MOD,FIXED
1000001,1,1
1000002,1,1
1000003,1,1
1000004,1,1
...
*END STEP

 

[brad]

As I don't see boundary conditions in step 1, I'll ask the obvious question--do you have boundary conditions or other constraints which keep your model from undergoing rigid body motion? If you do not, then this is almost certainly your problem. Even if the forces are entirely internal (as is the case with pre-tension section), you must resolve any rigid body motion if you expect to solve this.

Brad

 

[JulesVerne77]

sorry brad, I forgot to mention it above.. yes sure, I have sufficient boundary condition for the model in step 1 (but no additional boundary condition for the pre-tension nodes)..
When I run the analysis without the pre-tension definition, there is no problem.. but when I add these lines above, I got the solver problem every time.. but is the answer to constrain the only DOF of the pre-tension nodes in step 1? I don`t think so..

 

[brad]

The easiest recommendation is to put a dummy step 1 in which a small displacement is added to the pre-tension nodes (this would precede your current step 1). Modify your current step one by adding boundary, op=new and redefining your current bc's (hence removing this pre-tension nodal displacement). Keep the pre-tension loads loads defined as is.

Without getting into a lot details, I suspect if everything else in your model is kosher, this will work.

Brad

 

[barryodonnell]

Hi

Is the bolt free, i.e. has contact been modelled between the bolt-head & component etc. and the frictional forces generated assumed to remove the rigid boby motion. I have had this problem previously analysing bolted asemblies, use soft springs in the inital preload step. These can be optionally removed in the 2nd step (i.e. *MODEL CHANGE) when the frictional forces are fully developed.

Barry

 

[DickButkus]

Check for duplicate boundary conditions (such as symmetry on one face, and displacement on an adjoining face) and of course, rigid body motion. When you define pretension section, you've set up a surface just like contact. Be careful what you do with the nodes on the pretension surface. Try not to let these nodes participate in other boundary conditions.

You may wish to contact your local ABAQUS rep. They will sometimes run your deck and tell you how to debug it.

Best regards,
KF9RI

 

[garyyang]

Hi,
Does anybody know what is the philosophy of the PRE-TENSION? How is it formulated in the solver? I am quite confused with something in the manual: " When a pre-tension node is not controled by using the *BOUNDARY option, make sure that the components of the structure are kinematically constrained; otherwise, the structure could fall apart due to the presence of rigid body modes?". What does it mean "to FALL APART"?


thanks

Gary

 

[brad]

Gary,
Without getting into the math, the easiest way to conceptualize it is a cutting-plane across the pre-tension surface (or through the beam). This then "splits" the bolt into two parts. The reference node enforces constraints consistent with axial strain/deflection (if everything is done right).

My suggestion about a dummy step and boundary comes out of this realization; there is a potential for one side of this "split" bolt to be unconstrained. Please do not take this description completely literally; it's intended to basically the phenomenon.

Brad

 

[brad]

that would be "basically CONVEY the phenomenon".