Thermal bolt pretension 2

[jfymsam86]

Hello everyone
I modeled a bolt connection (a Beam welded to an Endplate and connected to the Column flange with 4 bolts (A490, 1.25”)) under cyclic loading (general-static) in ABAQUS 6.11. I defined interaction setting. (Units: cm, kg). After analysis, bolts got narrow, because I didn’t pretension them. Now I’m going to define negative thermal pretension on face of bolts (about 70% of capacity of them) according some articles. They define orthotropic thermal expansion coefficent only in axis of bolt. In this case, first step is applying the pretension, and second one is for cyclic loading.
1) should I define the first step by Coupled temp-disp.? How can I stop it for second step?
2) Software wants me to define Conductivity, Density, Specific Heat, Change the elements of end plate and column to Coupled temp, etc.‼ Is my way to pretension right? Or there is a better way for it?
3) What’s the difference between pretension by “Bolt Load” or “Thermal Load”?
Which one is better?
If someone can tell me the the best way (step to step) I really appreciate it.
Thanks a lot.
J.fymsam

 

[corus]

You don't need a coupled temp-disp analysis to define bolt loads. The pretension you're wishing to define is by using differential thermal expansion, and you merely have to define the temperature of the bolt relative to the rest of the structure. If you apply a negative temperature then the bolt will contract (relatively) and you'll effectively apply a pretension to the bolt. Don't forget to input thermal expansion in your properties.

 

[jfymsam86]

Hi
Thanks for your reply
I did this process: Mechanical>Expansion>orthotropic: alpha11=alpha22= 0, and alpha33(axes of bolt)=2.1e-6.
And then: Create load>Surface Traction>Vector (0,0,1).
Did you mean this path?
But about magnitude! Is it Temperature or Pretension Load??
Pretension for A490 1.25” (138.7 Kips) is about -61696.5 kg ‼?
What’s the relationship between Load and Temperature in this case?
Thanks a lot

 

[corus]

The thermal load is defined in the load module, 3rd icon down, I forget the name of it. Or you can simply define a pretension load as you said. For a thermal load you're defining a displacement, d=alpha x T x L, given by the thermal expansion alpha. So if the stiffness, K, of the bolt is AE/L then F=Kd or F=AEalphaT

 

[jfymsam86]

Thanks again Corus
Sorry, but I didn’t get my answer. In load module, 3rd is pressure and 5th is surface traction. If the surface traction is true, my question is about the magnitude of that. Because in fact in my problem there is no heat! So I should calculate the T from F=AEalphaT and put in the magnitude? So it’s about 1863 C ‼?
Is it true? (the picture attached)
Moreover I used the Static-General for both steps.
I really appreciate

 

[jfymsam86]

Amm, this is attached file...

 

[jfymsam86]

Hello everyone
My model has a beam=430 cm ,and a column=550 cm. The setting for interaction is:
Tangential, penalty, friction coeff.=0.2, hard contact.
And others are in attached file.
But each analyze interrupted after about 10 hours (about 50% of analyze) with error because of small (about 1e-5) increment and below warnings:
For contact pair (assembly__pickedsurf5625-assembly__pickedsurf5533), adjustment was specified but no node was adjusted more than the adjustment distance = 2.22000e-16.
THE SYSTEM MATRIX HAS 23 NEGATIVE EIGENVALUES. EXPLANATIONS ARE SUGGESTED AFTER THE FIRST OCCURRENCE OF THIS MESSAGE.
MATERIAL CALCULATIONS FAILED TO CONVERGE OR WERE NOT ATTEMPTED AT ONE OR MORE POINTS. CONVERGENCE IS JUDGED UNLIKELY.
Excessive distortion at a total of 77 integration points in solid (continuum) elements.
The strain increment has exceeded fifty times the strain to cause first yield at 99 points.

Thanks a lot beforehand If someone can help me.
J.fymsam

 

[corus]

If I recall, the temperature is input via the predefined field icon. You want the bolt to compress so the temperature should be negative, what ever its value.

As for the 2nd problem, you'd be better posting that as a separate question if you want more responses.

 

[jfymsam86]

Hi
yes, I got it, but in help the units of magnitude is F/L^2 that is stress. If I put the real value of stress there, its too big too software! if I put the lower value, in odb, model hag=s movement instead of traction!!!
sorry its a little stickler to me.

 

[corus]

In the predefined field option select the step rather than initial conditions. This will show you temperature in the window that opens. The units of temperature are deg C or deg F. If you're trying to input a bolt load then in the Create Load option there is a bolt load option in the window. I've not used that before but the units for that are Force.

 

[jfymsam86]

Hi Corus
Thanks for all of yyour favour

Sincerely yours
J.fymsam

 

[jfymsam86]

Hi
Bolts are A490 and 1.25 in. So A=7.91 cm^2
Pt-bolt= 138.7 kips= 62900 kg
E=2.05 e6 kg/cm^2
I’m going to define 70% Pt = 44000 kg
I defined orthotropic expansin as:
0, 0, 2.1e-6
So AEalpha=34.08 and then T= -1290 degrees
So in predefined load I assigned -1290 for surface of shanks in the first step.
(Direct specification> constant through region> Ramp> and propagate for 2nd step)
But they provide the Force only 8000 kg instead of 44000 kg at the end of the step (according to free body force)‼
What’s my fault?
thanks