Guest
Hi all!
what boundary one should consider when analysing a pipe elbow for out of plane moment?
Thanks in advance
![[ponder]](/data/assets/smilies/ponder.gif "[ponder] [ponder]")
what boundary one should consider when analysing a pipe elbow for out of plane moment?
Thanks in advance
Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!
Extend pipe in both directions. Apply clamp BC continuously around one open end edge. Then, if using geometry-based BCs, apply total out-of-plane moment continuously around the other open end edge. Or, if using FEM-based BCs (BCs on nodes), divide total out-of-plane moment by number of nodes you have around that open end edge, then apply that value of out-of-plane moment to each node on that open end edge.
I would think the above will produce a slightly conservative analysis, which is probably exactly what you want. Notice that since you're applied load is a moment (and not shear force), it doesn't matter at what distance away from the centerline of the other leg you apply it (I think), since pure moments translate (theoretically) over any distance unchanged (and can even turn corners unchanged). Good luck.
I would think the above will produce a slightly conservative analysis, which is probably exactly what you want. Notice that since you're applied load is a moment (and not shear force), it doesn't matter at what distance away from the centerline of the other leg you apply it (I think), since pure moments translate (theoretically) over any distance unchanged (and can even turn corners unchanged). Good luck.
- Thread starter
- #3
Guest
Hi vonlueke!
Thank U.
Let me clarify my question.
If one is doing a linear static analysis,what U have said is good enough.
I am doing a nonlinear analysis TO FIND LIMIT MOMENT OF AN ELBOW by elasto-plastic analysis.
To nullify the so called "end effects",after a series of trails, I found that one must use a staright pipe of length five times the outside diameter of the pipe at both ends of the elbow.
I simulated pure moment at one end of the straight pipe by equal and opposite pressures on two halves of the cross-section of the pipe.
I applied clamped(fixed) boundary conditions at the other end of the straight pipe.
The problem with these clamped boundary conditions is that
the maximum stresses occur at the fixed end and yielding begins first at the fixed end.And that is not desirable as I want to find the limit moment of the elbow and not of the straight pipe.Yilding should begin first in the elbow when out op plane moment value is gradually increased.
How to achieve that?
I am using ANSYS 5.7 and in the nonlinear analysis ,large displacement option and auto stepping options are switched on.
Thanks in advance.
Thank U.
Let me clarify my question.
If one is doing a linear static analysis,what U have said is good enough.
I am doing a nonlinear analysis TO FIND LIMIT MOMENT OF AN ELBOW by elasto-plastic analysis.
To nullify the so called "end effects",after a series of trails, I found that one must use a staright pipe of length five times the outside diameter of the pipe at both ends of the elbow.
I simulated pure moment at one end of the straight pipe by equal and opposite pressures on two halves of the cross-section of the pipe.
I applied clamped(fixed) boundary conditions at the other end of the straight pipe.
The problem with these clamped boundary conditions is that
the maximum stresses occur at the fixed end and yielding begins first at the fixed end.And that is not desirable as I want to find the limit moment of the elbow and not of the straight pipe.Yilding should begin first in the elbow when out op plane moment value is gradually increased.
How to achieve that?
I am using ANSYS 5.7 and in the nonlinear analysis ,large displacement option and auto stepping options are switched on.
Thanks in advance.
On a copy of your model, delete current applied shear pressure loads and all current constraints; i.e., delete all current BCs. Extend pipe in both directions a distance of about ten times pipe outer diameter. Place a node at centerpoint of each of the two pipe open ends, and spoke each of these two open end centerpoint nodes out to the pipe perimeter using rigid bars or stiff beams. Place one clamp BC on one of the two open end centerpoint nodes.
Sketch a straight line between the two open end centerpoint nodes. Define a coordinate system aligned with this sketched straight line (if necessary). Apply a force load on one open end centerpoint node that points exactly at the other open end centerpoint node. Apply an equal and opposite force load on the other open end centerpoint node pointing exactly back at first open end centerline node. Make sure gravity (gravitational acceleration) is turned off in your model. Now run analysis. Hope this works.
Sketch a straight line between the two open end centerpoint nodes. Define a coordinate system aligned with this sketched straight line (if necessary). Apply a force load on one open end centerpoint node that points exactly at the other open end centerpoint node. Apply an equal and opposite force load on the other open end centerpoint node pointing exactly back at first open end centerline node. Make sure gravity (gravitational acceleration) is turned off in your model. Now run analysis. Hope this works.
I don't understand why the highest stresses are at pipe clamped end, as the bending moment is constant over the pipe axis.
If it's a matter of clamped edge, well why do you clamp it?
Just limit only the translational degrees of freedom and those end effects should disappear.
prex
motori@xcalcsREMOVE.com
Online tools for structural design
If it's a matter of clamped edge, well why do you clamp it?
Just limit only the translational degrees of freedom and those end effects should disappear.
prex
motori@xcalcsREMOVE.com
Online tools for structural design
- Thread starter
- #6
Guest
Thank U Prex and Vonlueke!
Let me clarify the point raised by Prex as to why the max stresses are coming at the fixed end.Let us not forget that the object of analysis is not a stariaght pipe but an elbow with straight pipes(of length 5D) attached at both of its ends.
Now when we apply a pure moment at one (say open)end of the elbow,because of the 90 degree bend angle,this pure moment becomes a pure torque (of magnitude equal to the moment applied ) at the other(i.e. the fixed) end.
And at the fixed end the stresses are higher even if only translational DOF are restrained and all rotational DOF are set free.It may be due to the OVALISATION that occurs in a pipe when it is subjected to a moment load.
I magine yourself holding an allen wrench and applying a torque to a nut.its other end fitted into the nut head is subjected to twisting moment and the max stress in the wrench occurs there only.
My aim is to claculate the limit moment of the elbow for OUT of plane moment.For that yielding should first start in the elbow portion and not in the straight pipe end.
Vonlueke's suggestion to use rigid elements or beam elements at the ends,presumably to increase the stiffness of the pipe at the ends,would be of no use here.That can not reduce the stress concentration occuring at the supported end.Also applying forces as he suggested would change the problem itself.
I have got one idea...to increase the yield stress of the elemnts close to the supprted end thus avoiding(or postponing)the yielding of the material at the supported end of the elbow.I got better results but they are still not 100%satisfactory.For your kind information ANSYS program has got into convergence difficulties after crossing some displacement limit,while analyising for limit out op plane moment.There was no such problem in the case of inplane moment.(well,in the case of inplane moment load,we need to model only 1/4th of the model due to double symmetry)
Further extension of this problem includes finding the limit out of plane moment when both out op plane moment and
CONSTANT INTERNAL PRESSURE are simultaneuosly acting.I am doing this analysis(using the trick mentioned above) but results are not satisfactory due to covergence problems.
Any suggestions are welcome with great gratitude!
![[pipe]](/data/assets/smilies/pipe.gif "[pipe] [pipe]")
Let me clarify the point raised by Prex as to why the max stresses are coming at the fixed end.Let us not forget that the object of analysis is not a stariaght pipe but an elbow with straight pipes(of length 5D) attached at both of its ends.
Now when we apply a pure moment at one (say open)end of the elbow,because of the 90 degree bend angle,this pure moment becomes a pure torque (of magnitude equal to the moment applied ) at the other(i.e. the fixed) end.
And at the fixed end the stresses are higher even if only translational DOF are restrained and all rotational DOF are set free.It may be due to the OVALISATION that occurs in a pipe when it is subjected to a moment load.
I magine yourself holding an allen wrench and applying a torque to a nut.its other end fitted into the nut head is subjected to twisting moment and the max stress in the wrench occurs there only.
My aim is to claculate the limit moment of the elbow for OUT of plane moment.For that yielding should first start in the elbow portion and not in the straight pipe end.
Vonlueke's suggestion to use rigid elements or beam elements at the ends,presumably to increase the stiffness of the pipe at the ends,would be of no use here.That can not reduce the stress concentration occuring at the supported end.Also applying forces as he suggested would change the problem itself.
I have got one idea...to increase the yield stress of the elemnts close to the supprted end thus avoiding(or postponing)the yielding of the material at the supported end of the elbow.I got better results but they are still not 100%satisfactory.For your kind information ANSYS program has got into convergence difficulties after crossing some displacement limit,while analyising for limit out op plane moment.There was no such problem in the case of inplane moment.(well,in the case of inplane moment load,we need to model only 1/4th of the model due to double symmetry)
Further extension of this problem includes finding the limit out of plane moment when both out op plane moment and
CONSTANT INTERNAL PRESSURE are simultaneuosly acting.I am doing this analysis(using the trick mentioned above) but results are not satisfactory due to covergence problems.
Any suggestions are welcome with great gratitude!
Well your explanation of why high end stresses occur in the pipe does not convince me: at pipe end, as you say, there is pure torsion, and you, as any other FEM user, must be able to model that portion in order to get only the stresses that correspond to pure torsion (no ovalisation in a pipe in torsion, nor in bending!).
Of course if you restrain all the translational DOF's, the pipe is not allowed to change its diameter, but this should matter only when pressure is applied, as, if I'm not wrong, there is no change in diameter with pure torsion.
I don't remember at the moment if ANSYS allows this, but if you can restrain the end nodes only in the tangential (to pipe wall) direction and in the axial one of course, this should at least prepare you for the pressure calculation...
Personally I don't like all those tricks and technicalities that violate the rules for a correct mathematical model of a real thing: the risk is to lose the contact...
prex
motori@xcalcsREMOVE.com
Online tools for structural design
Of course if you restrain all the translational DOF's, the pipe is not allowed to change its diameter, but this should matter only when pressure is applied, as, if I'm not wrong, there is no change in diameter with pure torsion.
I don't remember at the moment if ANSYS allows this, but if you can restrain the end nodes only in the tangential (to pipe wall) direction and in the axial one of course, this should at least prepare you for the pressure calculation...
Personally I don't like all those tricks and technicalities that violate the rules for a correct mathematical model of a real thing: the risk is to lose the contact...
prex
motori@xcalcsREMOVE.com
Online tools for structural design
GoodWishes: My two previous posts, above, make no sense (as became apparent with your 2002-04-17 reply, above) because of the following question.
Definition question: Does the term "out-of-plane" moment mean the double arrowhead vectorial representation of the moment is (1) out-of-plane, or (2) in-plane?
Though it may seem to be a simple question, it would be interesting to get the answer to this question from various analysts. And where is a credible reference with this definition? Since my answer was 1, that's why my previous two posts do not apply to your current question. My apologies. In other words, I interpreted "out-of-plane moment" in your original post to mean "bending about an axis out of the plane of the elbow." So now I'll reread your and Prex's interesting comments.
Definition question: Does the term "out-of-plane" moment mean the double arrowhead vectorial representation of the moment is (1) out-of-plane, or (2) in-plane?
Though it may seem to be a simple question, it would be interesting to get the answer to this question from various analysts. And where is a credible reference with this definition? Since my answer was 1, that's why my previous two posts do not apply to your current question. My apologies. In other words, I interpreted "out-of-plane moment" in your original post to mean "bending about an axis out of the plane of the elbow." So now I'll reread your and Prex's interesting comments.
GoodWishes: I believe I have found your problem. You want to apply pure "out-of-plane" moment to the elbow, but then you're not doing it. Instead you're applying shear loads. True; your shear load creates constant torsion along the other leg, as Prex described; but it also has made your whole model into a giant, L-shaped cantilever. The highest moment on a cantilever is out-of-plane moment at its fixed support. I believe therein lies most of your ailments. Therefore, on a copy of your model, do the following.
Delete all current BCs (all applied loads and all constraints). Apply clamp BC continuously around one open end edge. Then, if using geometry-based BCs, apply total out-of-plane applied moment continuously around other open end edge. Or, if using FEM-based BCs (BCs on nodes), divide total out-of-plane applied moment by number of nodes you have around that open end edge, then apply that value of out-of-plane moment to each node on that open end edge. Now rerun your model. Good luck.
Delete all current BCs (all applied loads and all constraints). Apply clamp BC continuously around one open end edge. Then, if using geometry-based BCs, apply total out-of-plane applied moment continuously around other open end edge. Or, if using FEM-based BCs (BCs on nodes), divide total out-of-plane applied moment by number of nodes you have around that open end edge, then apply that value of out-of-plane moment to each node on that open end edge. Now rerun your model. Good luck.
- Thread starter
- #10
Guest
To Vonlueke: I have applied out of plane moment ( to bend the elbow in a horizontal plane passing through the center line of the straight pipe attached to one end of the elbow---when we imagine the elbow standing vertically before us)by equal and opposite pressure acting on the two halves(left half and right half from the end view) of the cross sectional area (and not by shear loads).
To Prex:case1
ipes and elbow without internal pressure,subjected only to out op plane moment at one end:In this case,as we know,only pure torque occurs at the supported end of the pipe.Even when all the rotational dof are set free at the end and only translational dof are fixed,yielding first commenced at the supported end and not in the elbow.The reason is that the von meises stress is higher at the supported end compared to that in the elbow(at a 45 degree section from one end of the elbow.)
(ovalisation of cross section occurs in the elbow but not in the straight pipe and it is not the cause of high stresses at the supported end.Sorry for mentioning it as the cause for high stresses at the end in my earlier post).
case II:same as in case one plus Internal pressure acting:
In this case,if we consider the effect of internal pressure alone, the deflection pattern of the elbow with straight pipes attached is similar to the deflection(springing action) of a rubber hose pipe when water is flowing through it under pressure.Now on such a deflection pattern we have to superimpose the deflection due to the out op plane momnet to get the total picture.
In this case even at the supported end the pipe has both rotational movement and translational movements(apart from the diametrical expansion of the pipe due to the internal pressure).When we try to restrict these translational movements of the pipe end,stresses raise and yilding first begins there. I agree with you that increasing yield stress locally etc are superficial things. But the question remains unanswered :How to get the limit moment of an elbow in this case?
Good Wishes
To Prex:case1
ipes and elbow without internal pressure,subjected only to out op plane moment at one end:In this case,as we know,only pure torque occurs at the supported end of the pipe.Even when all the rotational dof are set free at the end and only translational dof are fixed,yielding first commenced at the supported end and not in the elbow.The reason is that the von meises stress is higher at the supported end compared to that in the elbow(at a 45 degree section from one end of the elbow.)(ovalisation of cross section occurs in the elbow but not in the straight pipe and it is not the cause of high stresses at the supported end.Sorry for mentioning it as the cause for high stresses at the end in my earlier post).
case II:same as in case one plus Internal pressure acting:
In this case,if we consider the effect of internal pressure alone, the deflection pattern of the elbow with straight pipes attached is similar to the deflection(springing action) of a rubber hose pipe when water is flowing through it under pressure.Now on such a deflection pattern we have to superimpose the deflection due to the out op plane momnet to get the total picture.
In this case even at the supported end the pipe has both rotational movement and translational movements(apart from the diametrical expansion of the pipe due to the internal pressure).When we try to restrict these translational movements of the pipe end,stresses raise and yilding first begins there. I agree with you that increasing yield stress locally etc are superficial things. But the question remains unanswered :How to get the limit moment of an elbow in this case?
Good Wishes
- Thread starter
- #11
Guest
Some other readers correct me if I'm wrong here in saying: GoodWishes, it's very difficult to understand or visualize your applied load because of the words you're using to describe it. Everything else about your descriptions are clear, and you did well. But I cannot really visualize your applied loads because of your descriptions.
Therefore, could you please kindly redescribe your applied load on the elbow, except in the following manner. First, define for us three axes (x, y, and z). Orient them in any way you prefer. Thereafter, when you talk about forces, moments, restraints, etc., then you can use terminology such as "force in x direction", "restrain nodes against y translation", and most importantly, whenever you talk about moment, say "moment ABOUT the z axis" or "moment about the y axis". In other words, drop the terminology "out of plane." "Out of plane" is relative to which plane you're talking about. And whichever plane you intended to imply, even though you yourself know, might be misinterpreted by the reader. Then, also, whenever talking about a plane, you can say such as "an yz plane passing through the center line of the straight pipe attached to elbow end A", or "to bend the elbow ABOUT the y axis".
Whenever one says "moment ABOUT a z axis", it is more clear than "out of plane". And whenever you say "xy plane, yz plane, xz plane", everyone knows the orientation you're talking about. Therefore would you please be so kind to redescribe only your applied loads for us now? I cannot understand your applied loads yet, with the way you described them. Thank you. Cheers.
Therefore, could you please kindly redescribe your applied load on the elbow, except in the following manner. First, define for us three axes (x, y, and z). Orient them in any way you prefer. Thereafter, when you talk about forces, moments, restraints, etc., then you can use terminology such as "force in x direction", "restrain nodes against y translation", and most importantly, whenever you talk about moment, say "moment ABOUT the z axis" or "moment about the y axis". In other words, drop the terminology "out of plane." "Out of plane" is relative to which plane you're talking about. And whichever plane you intended to imply, even though you yourself know, might be misinterpreted by the reader. Then, also, whenever talking about a plane, you can say such as "an yz plane passing through the center line of the straight pipe attached to elbow end A", or "to bend the elbow ABOUT the y axis".
Whenever one says "moment ABOUT a z axis", it is more clear than "out of plane". And whenever you say "xy plane, yz plane, xz plane", everyone knows the orientation you're talking about. Therefore would you please be so kind to redescribe only your applied loads for us now? I cannot understand your applied loads yet, with the way you described them. Thank you. Cheers.
- Thread starter
- #12
Guest
Well gp3..If there is a symmtry of load ,geometry and boundary conditions about a plane,and when we talk about such a load we loosely call it as inplane load.Here is the pic.xy plane is the plane of symmetry of the elbow.If 'Mz'(inplane moment) is acting then we need to consider only 1/4th of this model for analysis.
Fig.Elbow under out_of_plane(of symmetry)moment My
----|--------
| --|--------B <-- moment 'My' applied at B
|-| |
| | |
| |<--- straight pipes attached to elbow
| |
|A| <--supports at A
|Y
|
|--------X (Z axis is perpendicular to the screen)
The moment My applied at B causes bending in leg B and twisting in leg A.
AIM:
to calculate limit moment of the elbow under My alone as well as when My and CONSTANT internal pressure are acting.
comments and suggestionsa re welcome.
Thanks in advance.
GoodWishes
Fig.Elbow under out_of_plane(of symmetry)moment My
----|--------
| --|--------B <-- moment 'My' applied at B
|-| |
| | |
| |<--- straight pipes attached to elbow
| |
|A| <--supports at A
|Y
|
|--------X (Z axis is perpendicular to the screen)
The moment My applied at B causes bending in leg B and twisting in leg A.
AIM:
to calculate limit moment of the elbow under My alone as well as when My and CONSTANT internal pressure are acting.
comments and suggestionsa re welcome.
Thanks in advance.
GoodWishes
Goodwishes
I still don't see why you get higher stresses at pipe supported end under pure torsion, as torsional stresses are constant over straight pipe.
Isn't simply a matter of using a too limited number of supported nodes at the restrained end? Try refining the mesh only in the proximity of the end.
Another point is that in real piping, elbows are normally of a higher thickness with respect to connected pipe.
Still another point: when calculating pressure stresses you should restrain both pipe ends: no real piping subject to pressure just ends with an elbow and a cap!
prex
motori@xcalcsREMOVE.com
Online tools for structural design
I still don't see why you get higher stresses at pipe supported end under pure torsion, as torsional stresses are constant over straight pipe.
Isn't simply a matter of using a too limited number of supported nodes at the restrained end? Try refining the mesh only in the proximity of the end.
Another point is that in real piping, elbows are normally of a higher thickness with respect to connected pipe.
Still another point: when calculating pressure stresses you should restrain both pipe ends: no real piping subject to pressure just ends with an elbow and a cap!
prex
motori@xcalcsREMOVE.com
Online tools for structural design
- Thread starter
- #14
Guest
GoodWishes: That's an excellent diagram and description. Thank you. Now that you defined this coordinate system, we still need a redescription of the loads you are applying in your model to simulate My. Please give us a description of the actual applied loads in your FE model, using your new coordinate system for descibing the orientation of any planes, surfaces, cross sections, etc., in your description. Thank you. Cheers.
- Thread starter
- #15
Guest
To Prex
Mesh refinement at the supported end?!For your kined information,the OD of the pipe is 12"(324mm) and on its circumference I have 32 4noded shell(shell 181 in ANSYS) elements.I really dont thing further mesh refinement at supported end would work wonders and reduce stresses there.
The problem is that when internal pressure is acting,at the supported end ,apart from the diametrical expansion of he pipe,there is tendency of the pipe to move sideways..and when we restrain this movement by clamping the end ,the stresses go up.
well..I have applied longitudinal stress(PD/4t)at the free end(End "B" and there is no necessity for restraining that end when internap pressure is also acting.
To gp3.
As I mentioned earlier..the out op plane moment at B ie My is simulated by equal and opposite pressures on the two halves(left and right half when looking from free end "B"of the pipe cross section.
Mesh refinement at the supported end?!For your kined information,the OD of the pipe is 12"(324mm) and on its circumference I have 32 4noded shell(shell 181 in ANSYS) elements.I really dont thing further mesh refinement at supported end would work wonders and reduce stresses there.
The problem is that when internal pressure is acting,at the supported end ,apart from the diametrical expansion of he pipe,there is tendency of the pipe to move sideways..and when we restrain this movement by clamping the end ,the stresses go up.
well..I have applied longitudinal stress(PD/4t)at the free end(End "B"
and there is no necessity for restraining that end when internap pressure is also acting.To gp3.
As I mentioned earlier..the out op plane moment at B ie My is simulated by equal and opposite pressures on the two halves(left and right half when looking from free end "B"
of the pipe cross section.OK, your mesh looks sufficiently fine, but you are still unable to explain why you don't get correct results.
And it says what it means: in a simple stress situation as yours, a correct mathematical model must give the theoretical stresses (so constant over straight pipe length, after any effects due to bend ovalisation have died out). As your model doesn't, it is incorrect in some way and you should try variants of it until you get the correct uniform stresses.
Concerning the tendency of the bend to straigthen up, well your example of a rubber hose with flow inside does not apply, as it's tendency to move is due to the dynamic effect of the fluid velocity and of the open end.
Also if you have only one end supported with only internal pressure applied, of course there will be no load at all at the supported end, so I don't see this tendency of the pipe to move sideways...
My suggestion is to restart from zero with a simple straight tube in linear analysis and simple loads (pressure separated from end moment): OK this is quite elementary, but you need to make sure you can get a correct behaviour from your model before you go on.
prex
motori@xcalcsREMOVE.com
Online tools for structural design
And it says what it means: in a simple stress situation as yours, a correct mathematical model must give the theoretical stresses (so constant over straight pipe length, after any effects due to bend ovalisation have died out). As your model doesn't, it is incorrect in some way and you should try variants of it until you get the correct uniform stresses.
Concerning the tendency of the bend to straigthen up, well your example of a rubber hose with flow inside does not apply, as it's tendency to move is due to the dynamic effect of the fluid velocity and of the open end.
Also if you have only one end supported with only internal pressure applied, of course there will be no load at all at the supported end, so I don't see this tendency of the pipe to move sideways...
My suggestion is to restart from zero with a simple straight tube in linear analysis and simple loads (pressure separated from end moment): OK this is quite elementary, but you need to make sure you can get a correct behaviour from your model before you go on.
prex
motori@xcalcsREMOVE.com
Online tools for structural design
GoodWishes: You say (and I'm paraphasing), "My is simulated by equal and opposite x-directed pressures on the two halves (+z and -z halves) of the pipe cross section at the (apparently) closed end B." Please correct me if I'm wrong.
If above is correct, your applied pressures do not precisely simulate a pure moment. They have some small degree of shear involved. Maybe it is giving you some surprises (?) and problems. Why not apply the My moment as a real moment at the closed end B centerpoint, if it's closed--or spoke it out to the perimeter, if not closed--instead of trying to only approximate a moment? Thanks.
If above is correct, your applied pressures do not precisely simulate a pure moment. They have some small degree of shear involved. Maybe it is giving you some surprises (?) and problems. Why not apply the My moment as a real moment at the closed end B centerpoint, if it's closed--or spoke it out to the perimeter, if not closed--instead of trying to only approximate a moment? Thanks.
Goodwishes,
I'm still a novice ANSYS user, but I'm wondering if you have considered these: First) Have you input your moment properly as a couple (+F, -F, at distance L)? Second) Are your constraints at pipe end placed on the end "area"? If so, you may be getting singularity error at nodes on the constrained face. ANSYS has to approximate something away from infinite strain and you should ignore this area for stresses (unless you've constrained properly for full symetry on this plane). Is it possible to batch mode your run and program to select and deselect this problem area at the appropriate times?
Respectfully, DarrellW
I'm still a novice ANSYS user, but I'm wondering if you have considered these: First) Have you input your moment properly as a couple (+F, -F, at distance L)? Second) Are your constraints at pipe end placed on the end "area"? If so, you may be getting singularity error at nodes on the constrained face. ANSYS has to approximate something away from infinite strain and you should ignore this area for stresses (unless you've constrained properly for full symetry on this plane). Is it possible to batch mode your run and program to select and deselect this problem area at the appropriate times?
Respectfully, DarrellW
- Thread starter
- #19
Guest
Thank U all..Prex,gp3 and DarrellW!
Let me state it clearly all over gain !
(i) Out of palne moment only:
When I applied only OUT OF PLANE MOMENT(My at B)..I got good results and there was no problem anywhere,even at the clamped end.In this case the maximum stresses were in the elbow at a section 45 degrees from one of its ends.
(ii)Out of plane moment(My at B)+ internal pressure :
one end clamped and at the other end axial stress(pd/4t)applied.
There is nothing wrong with the model.
Due to the internal pressure ,the ELBOW tries to straighten up(I can see the deformed shape)in its own plane.(though there is no dynamic effect due to velocity of fluid etc.That was only a crude anology I had mentioned.).Remember that the elbow is more flexible compared to the straight pipe.
This causes the supported end to move(in the same plane of the elbow--XYplane in the figure above).Restrainign this end movement is one of the causes of stress concentration at SOme points at the supported end.Even freeing the ROT dof didnt help(as expecteD.)I took several static runs with different support conditions before proceeding to run nonlinear analysis.The internal pressure is the culprit here.
Gp3.. U r right.the exact moment simulation would be t to apply linearly varying pressure from top to the bottom of the cross section(just like bending stress distribution in a beam under pure moment).I have applied constant,equal and opposite pressures(+x And -X on +Z and -Z sides of the cross section.).at a slight distance away from the end ,this too simulates pure moment.very near to the end B ,it will not be a pure moment.As the distance of elbow is 5D away from the end,its oK.Th eproblem is not due to the moment simulation technique.The end B is not physically closed in the model..but the effect of closed end is simulated by applying Pd/4t longitudinal stress at end B.So it is as good as a closed end.
If one is interested in stresses in the elbow ..this model is perfectly ok since the the elbow is away from the two ends of the pipe.(to be precise at a distance of 5D from either end.)
My problem is different.I want to go to Yield stage and find the limit moment of the elbow.As yielding is first beginning at the supported end(in the load case of internal pressure+ My at B) I am in a dilemma.When I applied only Out of plane moment, yilding first began in the elbow and the result was OK.But when Internal pressure is also acting,I am getting into trouble.
DarrellW..
I applied Y direction restraints (Dy=0) and ROZ=0 and ROX=0 at the supported end "A". Dx and DZ should be made to zero at atleast some points to avoid rigid body motion and I applied Dz=0 and Dx=0 at some nodes at an interval of 90 degrees along the circumference.This condition gave better results(low stress concentration)(In one case I fully fixed the end "A" ieI amde all 6 dof=0. In this case I got comparitively hihgher stresses).I did make several trails like this.
Thanks for your suggestion regarding batchmode operation.Instead of selecting and deseleting this area..I tried a different route by locally increasing the yield stress of the material and I got a better result.I would have got correct limit moment of the elbow but for the convergence problems in ANSYS in the Out of plane limit moment analysis.
It seems ANSYS has got an inherent limitation..after some displacement had reached(in out of plane moment case),there were convergence problems in ANSYS.
well..thank u all once again for your enlightening suggestions!
I will look at this problem from different angles and will post the results here.
GoodWishes
Let me state it clearly all over gain !
(i) Out of palne moment only:
When I applied only OUT OF PLANE MOMENT(My at B)..I got good results and there was no problem anywhere,even at the clamped end.In this case the maximum stresses were in the elbow at a section 45 degrees from one of its ends.
(ii)Out of plane moment(My at B)+ internal pressure :
one end clamped and at the other end axial stress(pd/4t)applied.
There is nothing wrong with the model.
Due to the internal pressure ,the ELBOW tries to straighten up(I can see the deformed shape)in its own plane.(though there is no dynamic effect due to velocity of fluid etc.That was only a crude anology I had mentioned.).Remember that the elbow is more flexible compared to the straight pipe.
This causes the supported end to move(in the same plane of the elbow--XYplane in the figure above).Restrainign this end movement is one of the causes of stress concentration at SOme points at the supported end.Even freeing the ROT dof didnt help(as expecteD.)I took several static runs with different support conditions before proceeding to run nonlinear analysis.The internal pressure is the culprit here.
Gp3.. U r right.the exact moment simulation would be t to apply linearly varying pressure from top to the bottom of the cross section(just like bending stress distribution in a beam under pure moment).I have applied constant,equal and opposite pressures(+x And -X on +Z and -Z sides of the cross section.).at a slight distance away from the end ,this too simulates pure moment.very near to the end B ,it will not be a pure moment.As the distance of elbow is 5D away from the end,its oK.Th eproblem is not due to the moment simulation technique.The end B is not physically closed in the model..but the effect of closed end is simulated by applying Pd/4t longitudinal stress at end B.So it is as good as a closed end.
If one is interested in stresses in the elbow ..this model is perfectly ok since the the elbow is away from the two ends of the pipe.(to be precise at a distance of 5D from either end.)
My problem is different.I want to go to Yield stage and find the limit moment of the elbow.As yielding is first beginning at the supported end(in the load case of internal pressure+ My at B) I am in a dilemma.When I applied only Out of plane moment, yilding first began in the elbow and the result was OK.But when Internal pressure is also acting,I am getting into trouble.
DarrellW..
I applied Y direction restraints (Dy=0) and ROZ=0 and ROX=0 at the supported end "A". Dx and DZ should be made to zero at atleast some points to avoid rigid body motion and I applied Dz=0 and Dx=0 at some nodes at an interval of 90 degrees along the circumference.This condition gave better results(low stress concentration)(In one case I fully fixed the end "A" ieI amde all 6 dof=0. In this case I got comparitively hihgher stresses).I did make several trails like this.
Thanks for your suggestion regarding batchmode operation.Instead of selecting and deseleting this area..I tried a different route by locally increasing the yield stress of the material and I got a better result.I would have got correct limit moment of the elbow but for the convergence problems in ANSYS in the Out of plane limit moment analysis.
It seems ANSYS has got an inherent limitation..after some displacement had reached(in out of plane moment case),there were convergence problems in ANSYS.
well..thank u all once again for your enlightening suggestions!
I will look at this problem from different angles and will post the results here.
GoodWishes
I suppose that, together with the pd/4t axial stress, you also apply pressure to the inner face of the model.
However this pd/4t stress might be partly incorrect and give rise to spurious effects at pipe end. The best would be to cap the pipe ends and to apply only pressures to the model. Anyway to be sure that your pd/4t load (stress) is correct, you can check that at supported end there is no net (resultant) reaction load in the opposite direction to the pd/4t load. If you have such a reaction then you should adjust the pd/4t value in order to get a zero reaction.
Moreover, as I already told in a preceding message, in my opinion the pipe should be capped and supported at both ends when calculating pressure stresses: I know that it would then be impossible to superpose the twist and pressure effects in the plastic analysis, but, you know, plastic analysis is not so simple as it appears when reading code manuals!
prex
motori@xcalcsREMOVE.com
Online tools for structural design
However this pd/4t stress might be partly incorrect and give rise to spurious effects at pipe end. The best would be to cap the pipe ends and to apply only pressures to the model. Anyway to be sure that your pd/4t load (stress) is correct, you can check that at supported end there is no net (resultant) reaction load in the opposite direction to the pd/4t load. If you have such a reaction then you should adjust the pd/4t value in order to get a zero reaction.
Moreover, as I already told in a preceding message, in my opinion the pipe should be capped and supported at both ends when calculating pressure stresses: I know that it would then be impossible to superpose the twist and pressure effects in the plastic analysis, but, you know, plastic analysis is not so simple as it appears when reading code manuals!
prex
motori@xcalcsREMOVE.com
Online tools for structural design
- Status
Similar threads
- Locked
- Question
- Locked
- Question