Structure supported on springs and using gap elements

Structure supported on springs and using gap elements

Anonymous
Not applicable
1,100 Views
6 Replies
Message 1 of 7

Structure supported on springs and using gap elements

Anonymous
Not applicable
I have a very large structure supported on many springs. When the structure is loaded to its maximum weight the load shifts from the springs to ground after a 4 inch spring deflection. I want to model this in MES using 1D spring elements and grounded gap elements, where on one side of the gap is the structure and the other is ground. Ultimately, I should see the spring elements loaded to their expected force based on spring constant and displacement and remainder of the load as reactions on the ground plane. The structure was created in Solidworks and imported to MES so there is no "ground plane". Anyone know if MES has gap elements that can be specified between ground and the structure? If not any ideas as to how to model this in MES?
Reply
Reply
0 Likes
Accepted solutions (1)
1,101 Views
6 Replies
Replies (6)
Message 2 of 7

KubliJ
Alumni
Alumni
Accepted solution

Hi @Anonymous,

 

Unfortunately, gap elements are only available in Linear analysis.  I'm not sure you can model it the way you have described.

 

I assume the springs deflect for about 4 inches and then they bottom out and become a hard constraint? 

 

Or is it that they deflect 4 inches and then the structure comes to rest on a grounded plane?  And in this you have a hard physical stop on some places and others providing a spring force in other places.

 

Thanks,

James

 

 



James Kubli, P.E.


Please marked this as solved if your question has been answered.
Reply
Reply
0 Likes
Message 3 of 7

Anonymous
Not applicable

It is the second condition-

The springs deflect 4 inches and the structure comes to rest on a ground plane.  The total load is shared between all of the deflected springs and other parts of the structure resting on the ground plane.  The springs and "hard points" are not one in the same and are located in different areas of the structure.  There are almost as many hard points as springs.  Yes the structure must move 4 inches before the hard points make contact.

 

I first tried the analysis by imparting a spring force (equal to the spring constant x deflection) to the areas on the structure where the springs are attached and making the hard points fixed and roller constraints.  But honestly didn't like the results too much.  Some assumptions have to be made that may not be the most accurate, plus in the area of the reactions I was getting opposite reactions forces with nodes very close to each other which didn't make sense to me.  Based on the results I felt the reactions weren't correct because of the force reversal in such close proximity to each other I made the conclusion the force imbalance had to be balanced somehow and did it at the constraints.  It didn't feel right so I am trying to model it more like real world behavior but can't figure out how to do it in MES linear static analysis.  

Reply
Reply
0 Likes
Message 4 of 7

John_Holtz
Autodesk Support
Autodesk Support

Hi @Anonymous

 

It sounds like you should draw lines at the hard points and define the element type to  be "Contact". Under the Element Definition, the "Contact Distance" is the length of the element when it comes into contact. This needs to be some length greater than 0, so maybe you want to make the contact lines 10 inches long and indicate that they come into contact at a distance of 6 inches.

 

Another option that would work for some models is to define an impact plane which as an infinite plane that all nodes of the model can contact.

 

The third option is to draw brick elements to represent the ground at each hard point and use surface-to-surface contact with the hard points. Each brick element stop only needs to be one element, so they are easy to create by hand in Sim Mech.



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided, indicate the version of Inventor Nastran you are using.
If the issue is related to a model, attach the model! See What files to provide when the model is needed.
Reply
Reply
0 Likes
Message 5 of 7

Anonymous
Not applicable

I'm still a little confused as to the implementation of the 3 suggested possibilities.

 

1. Do all 3 of these apply to MES and not Linear Static Analysis? If not can you clarify which must be done in MES and which I can do in Linear Static Analysis?

 

2. I like this option "The third option is to draw brick elements to represent the ground at each hard point and use surface-to-surface contact with the hard points. Each brick element stop only needs to be one element, so they are easy to create by hand in Sim Mech."  because I can then determine the contact forces (reaction loads) at these elements.

If I have 4 hard stops on my structure that are 4" x 4" and they come into contact with the ground after structure moves down 4 inches (spring supported for the 4 inches) defined as brick elements, do I draw a 4" x 4" rectangle 4" below the hard stop as a new part and define as brick element?  That 'ground' surfaces would be fully constrained and surface-to-surface contact defined between structure hard stop surface and ground?  Unclear how to draw brick elements I guess?

 

3. If this is all done in MES unclear how to specify the "springs".  I don't see Spring constraints in MES like there are in Linear Static. I guess I am a little confused between using 1DOF spring constraint (in linear static analysis ) versus spring elements.  Would I  draw lines that define the free end of the spring connected to the structure and the fixed end is connected to ground? The fixed end of the spring is on the same ground plane as where the hard points contact.

Reply
Reply
0 Likes
Message 6 of 7

Anonymous
Not applicable

MESSpringDefn.JPG

An image showing the spring elements (green lines) with one end fixed and the other connected to structure.  I have constructed the springs as one (1) part, each spring is constructed on a different surface but all on same layer.  Eight lines represent each spring (part surface) with a spring constant of 800 lb/in.  When specifying the spring constant in the element definition does it apply to the entire part, each part surface ( each part surface has 8 lines) or each line that makes up each spring?  Or would I specify K = 100lb/in because eight lines make up each spring for a total of 800 lb/in?

 

Thesurfaces below the springs with the constraints are the surfaces that will come in contact with the ground after the springs deflect 4 inches.

Reply
Reply
0 Likes
Message 7 of 7

John_Holtz
Autodesk Support
Autodesk Support

Hi @Anonymous

 

  1. Sorry, I should have clarified that my original reply (with the 3 suggestions) were all related to MES. Four inches of displacement sounds like a large displacement, so I think you are required to do MES to get the large displacements.
  2. A brick element is an 8-node cube with 12 lines. So you would not draw just 1 rectangle, but draw 2 rectangles and connect the corners. (In reality, I would draw 1 rectangle and use "Modify or Copy" with "Join" turned on, and extrude the rectangle to create the brick.)
  3. It looks like you got your springs drawn (according to your second post). The lines need to be much longer than the 4 inch gap between the model and the hard stops. Basically, the length of the line/spring cannot go shorter than zero! In most cases, it is very difficult to get the length of the line down to exactly zero. This is what would happen if the lines for the springs were 3 inches but they needed to compress a minimum of 4 inches in order for the model to reach the hard stop. (Or another way to think of it is this: After the springs compress 3 inches, the lines turn around and get longer by 1 inch. At that time, the model reaches the hard stops.)

The answer to your other question about the spring constant is that it applies to each line.

 

Let us know if that works out.



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided, indicate the version of Inventor Nastran you are using.
If the issue is related to a model, attach the model! See What files to provide when the model is needed.
Reply
Reply
0 Likes