Difference in result using Fixed support and Displacement support with 0 in X, Y, Z

  • 111 Views
  • Last Post 05 June 2020
  • Topic Is Solved
khoojwn posted this 26 May 2020

Hello,

 

I am building a model of a railway track on a bridge and I have used springs with remote connections to "stiff beams" which simulate the bridge deck. I have tried applying fixed supports on the bridge and also displacement with 0 in all X, Y, and Z, but the deformation of the rail seems to differ. In both cases, all parameters remain same except for the support condition to be either fixed or displacement supports.

Using Fixed Supports

1st picture is with fixed supports.

 

Using Displacement Supports with X=0, Y=0, Z=0

2nd picture is with displacement supports.

What is the reason for this?

Thanks.

Order By: Standard | Newest | Votes
Aniket posted this 27 May 2020

This seems strange, Can you suppress the displacement constraint in the system and insert the fixed support in the same system, and see if that shows similar difference, just for a sanity check? APDL input file uses D, all, all command for fixed support which is exactly the same for displacement constraint.

-Aniket

How to access Ansys Online Help Document

How to show full resolution image

Guidelines on the Student Community

How to use Google to search within Ansys Student Community

 

khoojwn posted this 28 May 2020

Dear Aniket,

I am new to ANSYS so I do not know how to use APDL. I apply all these constraints manually via Mechanical. Those 2 pictures which I posted are from the same file. I had suppressed the displacement and applied fixed supports for the fixed scenario, and done the opposite for the displacement supports scenario. I also had the understanding that it should yield exactly same results.

Thanks.

khoojwn posted this 01 June 2020

Dear Aniket,

I tried rebuilding the model (to remove certain slices, etc, that I don't need) and I still encountered the same problem with this fixed / displacement support! The springs are connected between the rail and the beam via body-to-body remote connections, not direct connections. Could the type of connection affect the results for fixed and displacement support? I would really appreciate some help on this.

Aniket posted this 02 June 2020

Ok, Do you have any beams or shells in your model? Also, can you try to replace displacements with remote displacements with rotations as zero as well?

 

khoojwn posted this 03 June 2020

Hi Aniket,

 

my bridge is modelled as a beam. I've tried replacing displacement with remote displacement and it works! Does this mean I should use remote displacements for any displacement I want to apply on my model? It is strange that using displacement doesn't work the same way.

Aniket posted this 03 June 2020

From the image misinterpreted it as solid and this condition applied to end face. When you apply displacement condition to a face in a solid, it also constrains the rotations inherently, because to rotate, nodes must change relative coordinates, which needs them to translate, but again translations are constrained so the rotations are not possible.

For beams or shells, displacements when applied to a single node, it can rotate without changing their positions, when fixed support is applied, it also constrains the rotations (by d, all, all command I mentioned), but when you want to constrain rotations as well, you will need to do that using remote displacements.

-Aniket

How to access Ansys Online Help Document

How to show full resolution image

Guidelines on the Student Community

How to use Google to search within Ansys Student Community

 

khoojwn posted this 05 June 2020

Hi Aniket,

Thank you for the explanation. Since I am using a beam element, I will proceed with remote displacements =)

Close