hexagon logo
Register Sign in
  • State Verified Answer
  • Replies 7 replies
  • Subscribers 3 subscribers
  • Views 150 views
  • Users 0 members are here
Options
Related

Generate Tapered BEAM Properties from Patran

shaheer.iqbal
This is in response to Tech Article ID KB8012044. I have some questions in order to understand this.
 
What does the station distances represents?
Do they need to match with my Grid Location?
 
Suppose I have cBeam (ONE bar2 element) between two grid points (GA and GB) (10 units apart) and I need to create a tapered beam
Will my input be
Station distance 0.0 10.0
Cross Section Area 1.0 2.0
Inertia 1,1 10
Inertia 2,2 10
Inertia 1,2 20
Torsional Constant 18
 
Does the above input means that at grid GA (station 0.0) an area of 1 with the above properties be created and at grid GB (station 10.0) an area of 2 with above properties be created?
  • 0
    If you look at the QRG for PBEAM it states that Station Distances (X/XB) is the "Distance from end A in the element coordinate system divided by the length of the element."
     
    So you need to put in your values in terms of X/XB. Think of it as a percentage along the length, from 0.0 to 1.0.
     
  • 0
    Thank you so basically the station distance are in terms of % which means if  my input is
    Station distance 0.0 1.0
    Cross Section Area 1.0 2.0
    It will create a tapered beam at the initial location with an area of 1 and at the final location with an area of 2.
     
    What if I enter multiple station distance such as
    Station distance 0.0 0.5 1.0
    Cross Section Area 1.0 1.0 2.0
     
    Does it mean that the 50% of the element length will be constant cross section (station distance 0.0 0.5) while the remaining 50% will be tapered cross section (station distance 0.5 1.0). will such representation be visual in the pattern?
     
    I am still struggling to understand the need of multiple station location (more than 2) and what is done in the background while solving for equations. Since I have only 1 element defined how is NASTRAN solving (splitting at that tapered section in between grid point)
     
    I hope I was available to make my self clear :)
  • 0
    Yes - 50%constant 50% tapered area. This is a rather fictitious example as changing the areas and not having the Inertias change too is most unlikely.
    Patran will only show the "cross section" using the end data - not the intermediate position section data.
     
    There is no need for multiple station locations. Think of it as a historical capability that was required back in the earliest days of FE when the size of the matrices(DOFs) you were solving was severely restricted by the computer power available. If you are introducing no external forces(constraints) at the intermediate positions then you do not need to model them to understand the force/displacement relationship (stiffness) between the end points. The ability to model a beam with changing section properties with just two grid points is a nice way to keep the number of DOFs in the model small. You can also think of this in a similar way to the use of "super elements", where you take a FE model and reduce its stiffness matrix down so it is only referencing the grids (DOFs) that connect it to other parts of a larger structure.
    So don't worry about wondering why you would want to use intermediate stations, you probably would not, these days you would just have grid points at the intermediate locations and multiple elements. The complexities of using multiple station locations probably outweighs any possible gain, these days computers are so powerful that I would not contemplate using this quaint feature.
    Edwin may well have additional input, and this is of course my personal perspective.
  • 0
    Thank you for a detailed explanation, those inertia number were not accurate and just to make the input easy. I  really appreciate you explaining this in detail. ​Yes I do not need multiple station locations and can use only initial and final station location as my grid length will be relatively small . I can capture the shape with this approach.
     
    One additional questions, when we define the beam we give a vector direction, suppose my beam length is x-axis I can define the vector either in y axis or z axis . When its an I beam, I can see the difference how my beam is oriented, in my case it will be a tapered beam, can you share some information on how to accurate define this vector so my y and z axis do not get swapped ?
     
     
  • 0
    For simple explanation: The orientation vector you define can be done using a grid (node) point or a vector. The cross product of the the orientation vector (either grid 1 to orientation grid, or orientation vector) and the beam x vector (element grid 1 to 2 vector) defines the y direction and the cross product of this Y with the X define the Z. The purpose of emphasizing the vector cross product bit is to get you to understand that the "orientation" vector does not have to be perpendicular to the element X axis. In fact it can be any vector that is not "co-linear" to the X axis.
    This means it is much easier to define one orientation vector that can be used for a group of elements even though the elements themselves are in different directions.
    Another useful "trick" is that you can use a coordinate system as part of the vector definition in Patran. So if you have a cylindrical silo storage tank with some I section reinforcement rings you can specify an orientation vector like <1 0 0 coord 1> . If coord 1 is cylindrical then Patran is using the radial direction (with respect to cord 1) at end A of each element as the element property orientation vector. Nastran will get multiple vector directions, each element around the circumference is different but it is easy to specify in Patran.
    Remember you can visualise the beam orientation in multiple ways - Display / Load BCs Elem props... and at the bottom of the form you will find "Beam display" options.
     
    To understand the Nastran input file please look at what Patran produces and correlate this with the description in the Nastran quick Reference guide.
  • 0
    Can anyone of you tell me what is wrong going with the model.
     
    So I created a rect beam section from the patran library ​with w=6 and h=1 and gave it to my beam element. I reviewed the beam orientation and it looked good (slide 1), however, when I uncheck this rect section and rather game geometrical input (identical to what was generated by the automatic beam section) it gives an incorrect beam orientation (slide 2)
     
    I am using the geometrical values pre generated by the auto rect section created by patran and use those as input for the second slide.
     
     
    Attached Files (1)
  • 0
    I suspect that you have the "Beam Display" option on the "LBC/Elem. Prop.Attributes" form set to the option
    "3D:FullSpan+Offsets+Equiv.A"
     
    When you use "properties" and not dimensions from a defined
    section, Patran does not have any geometric information for the cross section.
    In order to draw a representative cross section it can calculate a
    "rectangular" section that gives the same properties as those you
    input. This can either be done to give "equivalent Area" or
    "Equivalent I1/I2". Both are useful checks to give feedback about the
    data you input in relationship to the size of the geometry you are modelling.
    The area option always gives you a "square" shape(it only has one
    area value), the I option gives you a rectangle(calculated using the I1 and I2
    data) which will show the orientation of your section better.
© 2025 Hexagon AB and/or its subsidiaries. Privacy Policy | Cloud Services Agreement