Thermal Stress Analysis Constraints

[Boghi1990]

Insulated main steam lines running from boiler stop valves to turbine main stop valves. The lines are 18 inches and 12 inches with 8 inch and 7.5 inch insulation thickness. The ambient temperature where this steam lines are installed is about 70F. Steam lines are warmed up during thecold start up, from 100F to 750F with a rate of 200F/hr.

The target of this FEA is to determine the thermal stresses caused ONLY by the temperature distribution in the pipe wall, which is determined from a transient heat transfer analysis. The temperature load is the only load applied in this thermal stress analys.

Attached snap shot shows the sections of the piping I am considering to analyse. I am thinking to use symmetry and slice the piping along its longitudinal axis. I will apply symmetry constraints to the cut out faces of the piping.

I am not sure what kind of constraints could I apply at locations labeled A, B as marked up on the attached snap shot.

I would appreciate any suggestions or advices regarding the type of constraints I needv to apply at thoe marked up locations.

Regards,

Bogdan

 

[TERIO]

Are you talking about stresses do to temperature gradients through the pipe wall thickness, or overall thermal expansion of the system?

 

[Boghi1990]

Hi,

The aim of this FEA is to investigate thermal stresses caused only by the temperature gradients through pipe wall thickness. The overal thermal expansion of the system has been analysed by a piping stress analysis(Caesar II).

I have run the transient heat transfer FEA model for the temperature distribution during the warm up process of the steam lines. I need now to set up and run the linear structural analysis. I am not sure how I could constraint the structural model at the locations(A & B) marked up in the snap shot.

Regards,

Bogdan

 

[rb1957]

if you want only the effect of thru-thickness gradients ... why not model a short straight piece, and apply your gradients to it ?

though it does seem a little "odd" ... to want 1/2 the answer ? but then i've been called worse before ...

Quando Omni Flunkus Moritati

 

[TERIO]

Assuming you are going to add these stresses to those from CAESAR II, then you probably only want to constrain rigid body motion. Also, make sure that your boundary condition is far enough from the area of interest (usually 2.5*sqrt(r*t)).

I'm not sure your what code your piping is designed to, but most don't specifically address the stresses due to temperature gradients. An exception is ASME BPVC Section III, NB-3600 for nuclear power piping. It gives simplified rules for evaluating these stresses based on the temperature gradients. It may be worth taking a look at.

 

[Boghi1990]

The piping system was analysed with Caesar II software and the pipping code was B31.1.The system is part of a coal fired power plant.

 

[TERIO]

B31.1 does not specifically address stresses due to through wall gradients (but it isn't a bad idea to look at them). Part of my point was that determining the stresses is one thing, but then once you find them what is your acceptance criteria (what failure modes are you protecting against)?

 

[corus]

As others have said, your section of pipe wants to be 2.5sqrt(rt) away from discontinuities, but personally I'd double that. Use symmetry, and at the free ends restrain one end axially, and at the other end restrain the free end by coupling the nodes so that they move parallel to the cut face, in effect giving you generalised plane strain conditions there. Generally, thermal induced stresses are classed as secondary and the stress range is limited to twice yield.

 

[Boghi1990]

Corus,

Thank you for your suggestions. If I use the symmetry plane (XY for example), the only constraint applied on the cut plane is Tz=0. One free end of the pipe (left end), is constrained only axially (Tx=0). I did not understand how to constrain the other free end (right end)? What does it mean "by coupling the nodes so they move parallel to the cut face"? Which cut face do you refer at ? If I use this should I constraint the whole face or only a node on that face?

 

[corus]

On the cut face, the nodes on that face are selected and the dof perpendicular to that plane is made equal to the dof of one of the nodes on that plane. In that way all the nodes displace by the same amount, and so remain plane.