Skip to main content
D
DamianCastillo1-Visitor
1-Visitor
October 24, 2012
Question

How are others calculating Welds in Creo Simulate?

  • October 24, 2012
  • 6 replies
  • 9856 views

I was wondering what different techniques are others using to calculate the effect of Welds on different components when running a Creo Simulate analysis.


If there is a partial solution or technique that does not give you 100% accuracy but at least provides some level of understanding on what you can expect from a weld joint during analysis, I would love to hear about it.


Thanks in advanced.


"Too many people walk around like Clark Kent, because they don't realize they can Fly like Superman"


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

6 replies

I
iceblink11-Visitor
1-Visitor
October 25, 2012
It depends: What do you want to accomplish with the analysis?

Are you interested in
1) the weld itself
2) material near the weld, or
3) is the weld only something that transfers the loads to your place of
interest?


As far as i'm aware:
1): Model the weld as accurate as possible using a solid model, then
see what happens. If stress gets high, use nonlinear material.
(Alternatively use the good old hand calculations for welds.)
2): Tricky business, start with weld features, but you may need to
create a more accurate model if the stresses get high. Always keep in
mind that material may be weakened locally due to the Heat Affected
Zone.
3): No problem, use weld features, they will do what you want.
Basically they create a connection between the parts for you, something
you can also model by hand, but the weld features make life a bit
easier.

Best regards,
Patrick Asselman

    D
    DamianCastillo1-VisitorAuthor
    1-Visitor
    October 25, 2012
    Patrick,

    We are interested on how the welds hold up under load. It seems most
    answers are the same. Model the weld as a feature and use hand
    calculations. The problem with this is that the welds would be very
    complex to model and the amount of time it takes to do it.

    Thank You,

    Damian Castillo
    CAD & Administration Manager
    Engineering Department
    Hensley Industries
    D
    DanMcCaherty1-Visitor
    1-Visitor
    October 25, 2012



    In Reply to Damian Castillo:


    Patrick,

    We are interested on how the welds hold up under load. It seems most
    answers are the same. Model the weld as a feature and use hand
    calculations. The problem with this is that the welds would be very
    complex to model and the amount of time it takes to do it.

    Thank You,

    Damian Castillo


    Wouldn't it be nice if it waspossible to define weld features that had SOLID mesh-able geometry as an option? Creating weld features in Wildfire 5 (and newer releases) is very quick & easy, but they still missed the boat on solid welds. I know that enhancement request has been in their pipeline for years, but it seems that there was never enough interest from the customer base to make it a priority.


    Dan McCaherty


    Caterpillar Inc.

      D
      DamianCastillo1-VisitorAuthor
      1-Visitor
      October 25, 2012
      Dan,

      It would be great for PTC to build solid welds into their software. I
      would imagine many industries can benefit from this. Not all companies
      are active in asking for more functionality from their software which may
      appear as a low interest in PTC's eyes.

      Things are made with welds and stress analysis software should be able to
      help you design things like this better and faster. This would be one
      more thing PTC can say they do above their competitors.

      On that note. Does anyone know of a software that can currently do this
      or is this a limitation across the board for most FEA solutions?

      Thank You,

      Damian Castillo
      CAD & Administration Manager
      Engineering Department
      Hensley Industries
      M
      MikkoHinkkanen15-Moonstone
      15-Moonstone
      May 5, 2015

      Design rules:

      A) don't weld it

      B) if you must, minimize welding

      If you are looking for full blown transient analysis of welding with contacts&friction, weld deposition and temperature depended material properties, consider yielding of material, possibility to consider tag welds and fixtures - in order to know residual stresses in structures and deformation during welding - which you would use as an boundary condition for actual utility load. Then you will soon find that there is maby 2-3 software that can do most of it, somehow.

      Then, on the other hand if you really look at hand calculation standard and the assumptions there is - you will quite fast notice that most, if not all stress concentrations are just neglected from computation - since weld material is hoped to have enough plastic reserve (yield before break) which will even out worst hot sports. Also the total stiffness of structure is very hard to handle in manual computations.

      If you just want to get a bit more accurate solution than your hand calculation you may use the FEM stress (components) from plates "near" welds and scale them with plate thickness and allowed stress (and some factor of safety) in order to find the throat size. Just be sure that you model the stiffness of welds correctly. This way the singularities caused by weld beads&plates can be omitted (and sometimes even the weld geometry as well).

      No guarantee.

      I
      iceblink11-Visitor
      1-Visitor
      October 25, 2012
      It is more or less a limitation of all generic FEA software.

      The problem is that most welds cause geometric singularities, such as
      sharp corners. The calculated stress in these locations will be infinite
      if you calculate using FEA.

      The obvious solution of course is to model the weld very accurately and
      have the singularities deform using material plasticity. This however
      takes a lot of work to model the weld correctly (and even then: how
      accurate is the welder?), and then when you are done modeling it takes a
      lot of CPU power to analyse.

      So in the end, most companies that I know model the welds as simple
      connections from one part to another, be it via rigid connections (mind
        M
        mlindqvist1-Visitor
        1-Visitor
        May 6, 2015

        Analyzing welds using FEA (and by other techniques) is a large and complex topic. Unfortunately there are no easy shortcuts.

        The international institute of welding (IIW) lists four techniques to analyze welds, in order of increasing complexity/difficulty of use:

        1. The method of nominal stress

        2. The hot spot method

        3. The effective notch method

        4. Fracture mechanics

        1. Using the method of nominal stress, you don't model the weld itself. The calculated nominal stress in the shell (or solid) elements is then compared to a series of standardized weld connections where the allowable nominal stress has been obtained through extensive testing. Advantage: simple to use. Disadvantage: you can only analyze weld joints that are identical, or very similar to the the listed/tested weld joints. The IIW method of nominal strress is very similar to that of Eurocode 3.

        2. Hot spot method. Same type of FEA model as in method 1: the weld geometry is not modeled. The stress at the weld toe is derived by linear extrapolation of the stress in the shell/solid elements to the location of the weld toe. This stress is called the hot spot stress. The allowable stress level, derived from testing is compared with the "hot spot stress". This is more general than method 1. but requires more work.

        3. The effective notch method. The actual weld geometry is modeled using solid elements. The radii at the weld toes/weld root are modeled with a standardized 1 mm radius. The stress at those "notches" are compared with a value derived from testing, I recall its 225 MPa for welds in steel.

        4. Fracture mechanics. This is only applicable for failure analysis and when you can measure the length/geometry of existing cracks. To my knowledge it is primarily used in nuclear, aircraft and pressure vessel engineering.

        The stress levels derived from testing according to methods 1-3 are called "fatigue classes" abbreviated FAT. That stress level is the stress evaluated using each method, that results in a fatigue life of 2 million cycles. IIW provides S-N the entire curves derived from testing, for all methods, as well as suggestions for fatigue life estimation using damage theory.

        These methods (1-3) by no means cover all cases and are not perfect. The effective notch method for example, has been proven to be non-conservative, at least for plates thicker than those used in the tests to derive the FAT-class for this method.

        As I said, analyzing welds using FEA is a large complex topic that can not be covered here.

        /Mats L

          M
          MikkoHinkkanen15-Moonstone
          15-Moonstone
          May 6, 2015

          I was referring to "The method of nominal stress" with my comment. Thank you for complete answer.

          More on fatigue: www.eurofitnet.org/FITNETBasicTrainingPackage.pdf

          Terms & ConditionsAccessibility statement