Robot Structural Analysis Forum
Welcome to Autodesk’s Robot Structural Analysis Forums. Share your knowledge, ask questions, and explore popular Robot Structural Analysis topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

rotation of column (robot against ansys)

11 REPLIES 11
SOLVED
Reply
Message 1 of 12
Ruzeltje
1626 Views, 11 Replies

rotation of column (robot against ansys)

I have a construction modeled as given in the picture. All my connections are fixed in all directions including its rotations.

 

The only loads are its own weight and a small torque on top of the beam.

 

With this input a rotation occurs in the columns resulting in a displacement of 31 mm in the top beam.

 

A check of the same model in Ansys with the same type of connections results in a displacement of 1.7 mm.

When I remove the columns in Robot and replace this column with a fixed support the displacements are equal to the displacements in Ansys. Therefor I can conclude that there is a rotation in the column according to to Robot but there isn’t a rotation according to Ansys.

 

A rotation of the column (Hea 220) is not to be expected with the applied forces. In the actual construction there are displacements up to 10 mm, so there probably will be a small rotation in the columns.

 

My question is: What is the reason of the big difference between the robot and the Ansys model?

 

Further I’m interested to know if there is a possibility to limit the rotation of the column to get a more accurate displacement?

 

Thanks for the help

 

 

model.jpg

11 REPLIES 11
Message 2 of 12
Rafal.Gaweda
in reply to: Ruzeltje

Robot file please


Rafal Gaweda
Message 3 of 12
Ruzeltje
in reply to: Ruzeltje

Rafal,

 

I have included the calculation model to this post

 

Message 4 of 12
Pawel.Pulak
in reply to: Ruzeltje

Hello,

I have concentrated my attenttion on the right half of your model because if its symmetry.

RZ rotations in nodes 11 and 12 are very similar - so it is confirming your opinion that the flexural deformation of the beam 10 is relatively small and that the main source of the displacement in node 11 is the rigid body movement of the beam resulting from the torsion of the column 15 in node 12.

Such torsion rotation can be relatively easily calculated from the analytical formula knowing that MX torsion moment in the column 15 betweeen nodes 5 and 12 is equal to the bending moment MZ transferred from beam 10 in node 12.

It is illustrated in the screen capture below:

sc4.png

 

Please double check your model in Ansys whether it is really coherent with the model in Robot including:

1/ properties and orientations (weak/strong axis) of bars

2/ supports

3/ applied loads (including units)

 

---------------------------------------------
If this post answers your question please click the "Accept as Solution" button. It will help everyone to find answer more quickly!

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 5 of 12
Ruzeltje
in reply to: Pawel.Pulak

Thanks for the help. I understand where I went wrong in the robot calculation.

 

I have checked the ansys model and I found an important difference between the Ansys model and the Robot model.

In ansys the brackets inside the beams and columns are also modeled. Therefore the rotation is lower and therefore the displacements are much lower.

 

When I remove the brackets the displacements are still lower (aprox 10mm difference), where I would expect a higher displacement in ansys, because ansys considers the lateral buckling of the profiles where robot doesn’t.

 

I keep looking for the last differences between the ansys and the robot calculations.

But for now thanks for the help.

 

One extra question according to this problem. When I’m correct it’s not possible to insert the brackets in the robot model (except for the member verification check). For as far I know it’s not even allowed by the code to insert the brackets in the basic calculation of the stresses and displacements so I think I should remove them from the ansys calculation. Or is it allowed by the code and is there a possibility in Robot to model the brackets between the flanges of the beams and columns?

Message 6 of 12
Pawel.Pulak
in reply to: Ruzeltje

No, it is not possible to insert brackets in bar elements in Robot.

Generally torsion in bar elements in Robot is considered as free torsion - without preventing warping.

 

As concerns your Ansys model have you modeled it using bar elements with warping prevented (not available in Robot) or using shells to model webs and flanges of bars?

 

Regards, 


Pawel Pulak
Technical Account Specialist
Message 7 of 12
Ruzeltje
in reply to: Ruzeltje

The ansys model is a volumetric profile without preventing warping so this should be equal to robot.

Message 8 of 12
Pawel.Pulak
in reply to: Ruzeltje

But if you have modeled profiles using volumetric elements and these "volumetric profiles" were connected along webs and flanges  then this connections resulted in preventing warping.

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 9 of 12
Ruzeltje
in reply to: Pawel.Pulak

Ok, I assumed robot does the same on the location of the connection. Because of the type of connection. But when I understand you correctly there is a difference in the interpretation of the connection type. In robot it is rotation fixed but not preventing warping.

 

That would explain the last difference in my calculation.

 

Thanks for the help

Message 10 of 12
tony.ridley
in reply to: Ruzeltje

you are comparing a full on FEM analysis with simple "stick" analytical model.  not fair for Robot 😞

 

Message 11 of 12
Ruzeltje
in reply to: tony.ridley

You are right, there are some difference in the interpretation of a line model and a full model and it’s not fair to compare the 2. On the other hand it’s important to understand why there are differences. Normally I wouldn’t compare the two and simply trust on the robot calculation in combination with a hand check I did myself. Normally the results are in line with the actual construction.

 

In this case there is a big difference between the actual made construction, the robot model and the ansys model.

 

So that’s why I made the ansys model. I want to know where robot will be reprehensive for the reality and where there would be a difference.

 

I understand that there will be differences because of the different interpretations of the 2 programs. But in this case the results are completely different. So my questions weren’t intended to get the same results, but more to understand the differences between the two and the actual construction.

Message 12 of 12
Pawel.Pulak
in reply to: Ruzeltje

Yes, understanding the model and knowing the assumptions made is very important.

Huge majority of FEA software (including Robot) assumes free torsion in bar elements - no warping constraints.

It may result in significant dirrerences especially in case of torsion of short bars with warping prevented.

 

In my previous message I have asked you whether you have used in Ansys bar elements with warping prevented because I know that in Ansys some beam elements with the warping degree of freedom (the 7th DOF) are available.

 

Regards,

 


Pawel Pulak
Technical Account Specialist

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report