Difference between elastic boundary and rigid boundary

[Anonymous]

Hi,

I have a question concerning the BCs in the LSS. There's an "elastic boundary" and a "rigid boundary" boundary condition available. From the help, they seem more or less the same thing.

They both prevent translation/rotation in a certain direction...and they are both provided a spring stiffness, so what's the real difference between them?

Thanks

Björn

[xli · Accepted solution]

Hi, Bjorn,

They may be same in certain case. 

Rigid boundary element always applies on a DOF in coordinate axis direction, X, Y, or Z. It used to be with a default 10^10 stiffness, now you input a positive value. 

Elastic bounary element likes a rubber band that can be in any direction including coordinate axis directions.

-xli

[Anonymous]

Alright, so the elastic boundary element is like a rigid element, but it can be used in any direction, then. Thanks.

[xli]

Your understanding is correct. Both make same kind of Boundary Element (BE) for down-stream processor to deal with.

Here are some thing related in depth. A rigid boundary element always puts extra stiffness to a single DOF, kind of a constraint on that DOF. An elastic boundary element generally put stiffness on multiple DOFs (of that same node). If you rotate model making its direction as a coordinate axis, i.e. a LCS axis, then they are same.

In either case, all BE (rigid, elastic, and displacement) are not exact Boundary Condition (BC) though their engineering sense is a "constrained DOF". Numerically their related DOFs are still unknowns that need to be SOLVED from final linear system of equations. On the other hand, the DOFs with BC won't appear in the system equation, they are truly constrained DOFs, i.e. mathematically disappear from final linear system of equations.

Their numerical difference could be big in some cases while their engineering sense is similar. BE made the system ill-conditioned, i.e. more difficult to solve and could be totally inaccurate when ill-conditioning is too big; the BC made smaller system is easier to solve and yields more accurate solution. So if you can use BC then try to avoid using BE in general.

-xli

[Anonymous]

Hi Xli,

I am performing both static stress and transient stress (direct integration) analysis on a model of a single part.  I am attempting to simulate the real world assembly conditions by using Nodal Elastic Boundary and/or Surface Elastic Boundary.  For example, the part abutts a stationary metal bar when operational forces are applied.  To simulate the metal bar abuttment on the part I am using an Elastic Boundary with the stiffness set to Young's modulus of the bar.

Would this be a proper use of the Elastic Boundary, and would it yield accurate analysis results versus using a hard Boundary Condition?

Regards

[xli]

PSteven,

Surface elastic BE eventually produce nodal BE on all surface nodes. The original BE is designed to constraint the node in an arbitrary direction so that uses a very large stiffness as the default. When you use more realistic modulous, as far as the direction is not a problem for you this is OK to me.

Regards,

-xli

PS, actually model's numerical behavior will be better than using the default stiffness. And why do you not use truss elements (or another elastic part) representing abuttment? That is definitely better. 

[Anonymous]

Hi Xli,

Thanks for you comments.  I'm a novice and haven't used truss elements before.  Can you help me with the method?  In the model below, how do I add a truss to the nodes labelled for abuttment with the beam?

I found a post talking about selecting lines and then Draw->Pattern->Duplicate to create a new part which you define the Element Type as Truss.  Is there something further to do?  The static analysis didn't seem correct.

[xli]

Hi,

Since your mesh as example showed is uniform there, "drawering line and then combining copy lines" will work though a little bit time comsuming. I don't have your model, so I made a simpler and similar sample with steps to make truss. See if it helps.

results:

When you create the element part to host lines, i.e. trusses, you need to set up truss area and its material property.

-xli

[Anonymous]

Hi Xli,

I managed to add a truss to my Simulation model, and kept the default area.  The results seemed to reflect more closely what a real world prototype delivered, whereas using boundary conditions or elastic boundaries not so much.  What is the rule of thumb when selecting an area for the truss?

I also imported an assembly solid model that included the beam, which I modeled above using a truss, and some plastic bearings, which I modeled above using a fixed boundary condition.  The results of this simulation seemed to be better than the truss model above, however the bearings are not the same as a fixed boundary condition.

For the assembly, the beam was mated with the sidewall of the part, however the bearings were aligned and had a few mil separation from the part.  The simluation results specified Contact (Default: Bonded).  Is there anything that I should be doing to properly mate the surfaces of the different parts?

Regards,

PSteven

[John_Holtz]

Hi PSteven,

The truss element and elastic boundary element (1D spring in the version of software you are using) will give the same results as long as the input is the same. In this case, the input is the stiffness. For a truss, the stiffness k = A*E/L. The stiffness needs to represent the stiffness of the item they represent, whether that is a foundation or a beam against which your model abutts.

Instead of fixing the nodes/surface where the bearing are, and instead of trying to model the bearings, why don't you use a pin constraint? ("Setup > Constraints > Pin Constraint"). This is meant to simulate a shaft held so that it can rotate about its own axis. Or if the bearing do not prevent bending/rotation, then you can create a "Mesh > CAD Additions > Joint" at each bearing, create a "universal" type joint, and restrain the node at the center of joint. The universal joint would act like a ball and socket at each bearing. Two points of restraint leave the part free to rotate about the axis through the two points while allowing bending like a simply supported beam.

[xli]

Hi PSteven,

Making modeled support as uniformed as possible probably is a rule. The first and an easy way is to use total area there devided by number of trusses you need. Basically truss area is the factor of stiffness to contribute in surpporting. But this way is kind roughly done.

If you have to consider FEA modeling more delicately, actually this average-area way sounds like putting a uniformed support but actually not exact. Considering corner truss should get only 1/4 of a unit area, and edge trusses should get 1/2 than 1 unit for an interor truss. Then you may get more unifrmed axial force in those trusses.

A more close-to-real-world way modeling is using another solid part to replace the truss part. And use contact between them. Then you won't have to consider averaging area etc. But model becomes nonlinear and may have other difficulty depends on geometry and loading etc.

For the assembly you have question, can you post a picture here if possible? I am not exactly understanding your structure and what you want from text your descriptions. Sorry about this. Thanks for sharing your story with us.

-xli

[Anonymous]

Hi AstroJohn and xli,

Here is my assembly solid model.  I added the loads and constraints, defined the materials and then ran a Static Stress w/ Linear Material Models simulation.  I'm doing this in reverse and trying to match results with prototypes.  Which perhaps is an easier way to learn (to trust) modeling!  My question is whether I have to do any type of surface to surface preconditioning for the simulation, or whether it "just happens" automatically.  One comment: the beam is a partial beam and is not the full extent I'm using in the prototype, so the modeling results would reflect this difference.

AstroJohn, the pin constraint may be appropriate for this situation as well.  I will play around with it and see how it compares.

Thanks for your help!

PSteven

[John_Holtz]

Hi there,

I like your approach: simulation something that you are familiar with and has known results so that you can learn how to model, etc. I think you will learn a lot from this one model, which in some respects looks so easy. It is about to become more complicated.

For your first question: does contact between parts happen automatically? The answer is yes. The type of contact between parts is determined by the last branch in the browser: "Contact (Default: Bonded)". Bonded means the nodes on adjacent parts are connected together, and this simulates a full weld or fully glued condition. If all parts (or a majority) have the same type of contact, change the default. To define a different contact type between parts, either select the two parts, or the two surfaces, or some combination of the two. Right-click in the canvas and choose "Contact > X".

Item 5 from the figure: 0.002" clearance between bearing and shaft.

In a linear static stress analysis, parts need to be in contact. So the mesher will remove such small gaps. The bearing and shaft are connected together (based on the type of contact defined).

Item 2 from the figure: BC Ty Tz Ry Rz.

I suspect the boundary conditions are not doing what you want.

• Brick elements cannot be restrained with a rotational constraint. The processor ignores that part of the constraint. So the constraint on the bearings is really just Ty Tz.
• I am not sure if you wanted the bearings free to rotate, or whether the shaft was meant to rotate inside of the fixed bearings. If you wanted rotating bearings, the bearings are not free to rotate in your setup. One way to think of it is that solid bodies do not rotate, not in real life and not in simulation. What happens is all of the points translate to a different location, and this gives the "illusion" of rotation. Yes, it is silly to think of it like that in real life, but simulation follows a stricter set of rules. Hopefully, the figure below shows why the bearings are not free to rotate.
• If you wanted the shaft to rotate inside of the bearings, then you could define surface contact between the bearings and shaft. But then there would be nothing to prevent the bearings from translating in the X direction. So IF you use surface contact between the shaft and bearings, you should change the constraints on the bearings to Tx Ty Tz.
• Mathematically, it is much simpler to use the pin constraints and forget the bearing entirely.

I think that is all for now.

[9msl1]

Hi

I was interested in your conversation.  I'm trying to create 1D springs for use in the Mechanical Event Simulation Software (MES) to create a spring boundary condition for my component.

Unfortunately, these components (as far as I'm aware don't show up in MES.  Could you let me know how you were able to create these elastic boundary conditions? 

Thanks!