There are multiple approaches that probably vary widely depending on your preference and objective.  Perhaps consider the following.

Put a circle approximately the size of a large washer (or slightly larger) on the interface surface.  Put an anchor node at the circle centerpoint so you'll get a node exactly at the bolt centerline.  "Shell-coat" the circle with shell elements, assigning a very high modulus of elasticity to these shell elements to simulate the much higher stiffness in the bolt grip region.  Mesh the solid elements, which will follow the shell-coat mesh on the interface; or preferably extrude shell elements and a copy of the shell-coat elements, if possible, to create better solids.  If bolting to ground, put a constraint (clamp) on the node at the circle centerpoint; release constraint torsional degree of freedom (dof).  Read constraint reactions to get bolt forces.  If bolting to another part, create a matching shell-coat circle on other part and run a very stiff, very short beam between the two centerpoint nodes, releasing beam torsional dof (and omit the above clamp).

Toggle modulus of elasticity of shell-coat elements (and beam element, if any) to a very high value (but not so high as to cause singularity and solution failure).  When shell-coat elements (and beam, if any) are stiff enough, you'll see (in displacement display) near parallelism between bolted surfaces, locally in shell-coat circle, thus roughly simulating (approximating) the average heel-toe prying resistance of the clamped plates (regardless of direction of prying moment).  If interface plates are nonparallel at shell-coat circle in displacement display, it means your shell coat (and/or beam, if any) is not yet stiff enough.

For any decent bolt pattern footprint (i.e., more than one line of bolts resisting moment in that direction), prying moment on individual bolts is often negligible and bolt loads can be read directly, ignoring moment reactions or beam moments.  Good luck.

ABAQUS has special facilities for putting bolts in models. The facility enables the bolt to be given a pre-tension. The bolt is modelled explicitly.

TERRY

OK pals, I'll follow your advices. Thanx for answers...

Does anyone know if Nastran for windows has a similar capability ( model bolted connections)?
thanks
mzl

Nastran does not have the capability that ABAQUS does (in fact ABAQUS states that they have a patent on this capability).
Brad

You can create a very simple bolt model for NASTRAN! Create first one Beam element with the screw dimension. Create both end double rod stars! (This means you need to define from the screw's end rod elements. The first star is the rod elements between the center and the hole's edge. The second is a little bit larger the size of a large washer. The stiffnes should be high. Important things: Try to create approximatelly simmetric stars!) Now you can add a unit temperature load on one end of the beam bolt and zero on other side. You should give only for beam element alfa value! Calculate the result from the temperature load! Check the force inside the beam element! Modifiy the temperature! Know it is ready for further calculation!

Irwin

Irwin,
I have used that approach in Nastran, and if one only has Nastran, it is the best approach available to them.
However, there are three severe limitations to this approach:
1) It does not allow one to directly input the actual load or length changes in the bolt for most models.  All it is doing is describing the thermally-induced strains.  For statically indeterminate structures, one must iteratively tweak the value of the temperature differential or alpha in order to arrive at a number for force/deflection in the bolt.
2) If the model undergoes temperature changes downstream (for instance, an engine analysis which first concerns bolt-up, then cyclic temperature changes due to engine heatup), this approach fails, as it is relying on the constant initial temperature change to drive bolt forces.
3) It falls apart if one is concerned with nonlinearities in or around the bolts.

Your approach does work, but if one has ABAQUS at their disposal, the Nastran approach is archaic by comparison.

Brad

Hi:
    I have been seccessfully using brick elements in ABAQUS with temperature effect to model bolts.  My entire model was a steel structure assembly with concrete which has a total of 60,000 DOFs.  
    These bolts were modeled using approximately 600 8-node brick elements per bolt.  The temperature effect was used to apply the required pre-tensioning force in these bolts.  Gap elements were used on the interfaces between bolts and other elements.  However, these gap elements had converging problems sometimes.  Another option is to use an user predefined thin layer elastic element with super high stiffness in compression but very low stiffness in tention to allow seperation between elements.  If you need to pretension the bolts, you have to set at least two steps of loading.  The first step is to decrease the temperature inside the bolt to produce a tension force in the bolt shaft and of course a compression force to other elements between bolt head and nut.  You have to calibrate the temperature to get the right pretension force you need.  The second step is to load the structure as the way you want it to be.
    I know there is a pretension option in ABAQUA which allows you to model the bolts with tension force.  However, it only allows the force to be applied along the bolt shaft. In another word, if you need to displace the entire structure, changing the loading axis of the bolts, you will confuse the program and errors may occur.
    I hope these will help and good luck.

shp6:
I have never experienced the problem which you are stating.
The pretension does indeed limit itself to the axis of the bolt (technically to the normal of the defined bolt cross-section).  This is the definition of the bolt pre-load.
However, this does not limit the bolt from carrying lateral forces, nor does the introduction of such forces 'confuse' ABAQUS.  

The mechanics of that situation may be complex enough to lead to convergence difficulties, but there is fundamentally limitation to this capability such as what you suggest (and I state this from a basis of a lot of experience in using this specific functionality).

Your approach is essentially the ABAQUS version of the Nastran approach, and limitations 1) and 2) (from above) still apply. If somebody has ABAQUS, I would strongly encourage them to use this built-in feature, which is VERY robust.

Brad

Well...Brad...I guess you are right with your models.  However, I do have problems with the pretension option in ABAQUS when I need to move my bolts with my entire structure.  I thought that is the limitation of this option.  I do not want to argue with you about this issue and what I mentioned before just want to express my experience and share with you guys.  Someone should probably try both methods to see which one is more suitable for his own models.  Actually, there are a lot of methods I tried in my models but these two are the ones actually work best.  Good luck.

spirit,
ansys5.6 and ansys5.7 have pretension element(prest179)
which can be used to model the pretension section.
u can find about these in www.ansys.net

jagadeesh!

I tried this ANSYS element, I had lots of bad experiences! (I used in 5.6 or 5.7, I do not know.) I made a simple beam model, and I tried this pretension element on it! For me it seemed, that is uncorrect! May be I made a mistake, or in the newer version it is better!

Irwin