Steel Structures Fire Test Simulation

  • 141 Views
  • Last Post 22 May 2019
swanpyae posted this 18 May 2019

Hi there,

I'm quite new to Ansys Workbench and I've been learning the program through youtube tutorials and threads from this forum. 

I'm trying to model a fire test simulation (Assembly as shown in Figure) to analyse the stress and strain performance on the connection plates under fire. I've got the geometry modelled (I only modelled half the assembly as it is symmetric and to simplify the model, I've only modelled the column, connection and half the beam with the 40kN loads). I'm a bit lost to model the fire conditions. Do I use transient thermal analysis? How do I model the temperature to simulate realistic convection through the beam and whatnot?

If you can help me out with the process and procedure of how you'd simulate it, it'll be much appreciated.

 

Swan

Order By: Standard | Newest | Votes
peteroznewman posted this 18 May 2019

Here is a Discussion from a member who was simulating a column under load while the temperature was raised.

Here is another discussion.

  • Liked by
  • swanpyae
swanpyae posted this 18 May 2019

Thanks Peter,

 

I'll have a crack at it.

swanpyae posted this 20 May 2019

Hi Peter,

I've got the test modelled (only modelled half of it since it's symmetric). I can't seem to successfully solve it. Keep running into errors (please see picture attached). 

I've modelled all the contact between bolts and nuts to bonded and every other contact friction (I specified the geometric adjustment to fit). I've modelled the boundary conditions of the column to be fixed at the bottom end and horizontally fixed at the top end to allow for expansion. The free end of the beam is modelled as frictionless support as it represents symmetric face.

 

I've attached my project file if you can have a look, it would be much appreciated as I'm kinda stuck.

 

Swan

 

Attached Files

peteroznewman posted this 20 May 2019

The above is an image because this website has a list of banned words that prevent content from posting. I couldn't guess what the naughty word was to change it, so I just did a snapshot as a workaround.

Here is an example of a bolt.

sweepable pieces

Plasticity.

swanpyae posted this 20 May 2019

Thanks for the reply Peter,

1) I'm working on 19.2

2) Can you relink the "example of a bolt" so, I can have a look at it for reference? Can you please explain how do I do the conversion as I'm not familiar with that?

3) I will add in tabular data for multilinear isotropic hardening based on temperature in Engineering Data.

4) Yes, I put that displacement 2 to help with convergence. 

5) I will try and solve Static Structural alone first

6) I will try that method of loading. Is it better to have a loading plate on top of the beam flange as shown in the test setup and put the load on the face of that plate?

7) So, in my timestep, step 1 should be when the Imposed Force is equal to 0 but the pretension load is applied. in step 2, the imposed force is applied. Is that correct?

peteroznewman posted this 20 May 2019

2) see previous post.

4) If the structure buckles to the side, that is a valid failure mode. Delete this constraint.

6) Yes, you could have a loading plate instead. Still use a Remote Displacement.

7) In step 2, the Bolt Pretension has to be set to Lock and the imposed Displacement is applied.

swanpyae posted this 20 May 2019

Hi Peter,

I've followed everything you said except step 2 which is slicing up the members to allow sweep meshing.

I've attached my updated project files. Can you please have a look as I am really stuck and don't know how to fix it.

I'm not sure my slicing is correct either. Also, i don't know how but the faces of the bolt threads are divided as well. I really appreciate your help so far Peter. 

Attached Files

peteroznewman posted this 21 May 2019

The example bolt I gave you is on the left compared with the mesh on your bolt on the right.
The head on your bolt is too small and you don't have enough elements on the face of the head.
The example has more elements than necessary, but one element is not nearly enough.

If you pick all six faces on the head (or nut) you can pull it to a larger size.

Watch out for the automatically created contacts when you update the Geometry.

You also have a contact that was near open. You have to fix the near open contact.
I duplicated the contact and made it a contact to the center web of the I-beam.

I will only be online for one more night, then I am on vacation for several weeks.

swanpyae posted this 21 May 2019

Hi Peter, I will fix everything by what you've said and run the solver to see if it solves successfully.

If you don't mind me asking, will you able to solve it after you've fixed it? Will you be able to share the project file so, i can have a look.

For my research, as long as it runs and gives me results and data, I will be able to comment on the process and what can be improved. But i just can't seem to solve it successfully.

peteroznewman posted this 21 May 2019

There are too many nut and bolt heads that need fixing, so I am not going to fix them. When you have fixed them, and the contact between the Web Cleat\Solid to Solid, I will have another look.

swanpyae posted this 21 May 2019

Hi Peter,

 

I've refined the mesh on the bolts and nuts and fixed up the contacts (no more near open contacts). This is the error I'm gettng now.

Can you please have a look at what might be giving the errors? Thanks

Attached Files

peteroznewman posted this 21 May 2019

The elements are highly distorted. If you pick Solution Information, you can type a 1 in the Identify Element Violations. Then after a Solve, it will automatically show you elements that are highly distorted.

You must use even smaller elements around the nut and bolt head. Also, keep those faces on the Contact side, not the Target side. You can use Adjust To Touch on all the nut faces and bolt head faces to help it get started.

To get a solution, you could change all contact to Bonded, and suppress all the contact of the bolt shanks to through holes.

I am on vacation for a few weeks starting tomorrow, so I wish you good luck. Other members may be able to help.

swanpyae posted this 22 May 2019

Hi Peter,

I'm changing my I beam to sheet bodies for faster simulation. When I do the fritonal contacts between the solids bolt and sheet bodies, it is showing as oranged coloured closed contacts. Is that normal to have some penetration? (I did geometric adjustment of adjust to touch)

 

The simulation is currently running for some time now but it doesn't seem to be converging. How should I model the time stepping control in the analysis.

 

Thanks for your help so far Peter. I'm learning a lot about Ansys and simulation from you. Have a nice vacation. 

If everything else fails, my plan B is to simplifed the geomtery by having only the connected face of the Column I beam and have that fixed. And using sheet bodies for faster simulation.

Any suggestions on simplifying to get some results?

peteroznewman posted this 22 May 2019

Sheets have a Top and Bottom side, so if you have frictional contact between a sheet and a solid face, you have to make sure you picked the side of the sheet (Top or Bottom) that faces the solid face.  You also have to check Use Sheet Thickness.

Attach your .wbpz archive file and I have one last night to take a look.

swanpyae posted this 22 May 2019

Thanks Peter.

 

This is the simplified model with all contact bonded to analyse the effect of reduction in beam flange section. It's not solving as well. I'm archiving the one with the sheet bodies for you to have one last look. Really appreciate it.

Attached Files

swanpyae posted this 22 May 2019

Peter,

 

I hope this isn't too late for you. I was doing some refinement to the mesh and adding some contacts between the solid bolts and sheet bodies. Please find attached for archvie file

Attached Files

peteroznewman posted this 22 May 2019

On the solid model, suppress the large plate that is fixed on the back, and use the three faces on the back of the other parts that were bonded to the large flat plate and make them fixed instead.

The remote displacement is wrong. It should not be on the top face. It should be on the end face. If it is on the top face, you are requiring that the edge of the face be bonded (or fixed) and move down.  Can't do both, which is why it would not converge.

The symmetry region for the end of the beam had an X-axis normal when it needed a Z-axis.

swanpyae posted this 22 May 2019

I will do the simplified model with sheet bodies now.

 

Please see attached for the latest archive (I fixed some contacts) for the full model using shell elements. I'm getting elements distortion error in the bolts. Should I increase the mesh and probably use a ciruclar heads and nuts?

 

Attached Files

peteroznewman posted this 22 May 2019

Sheet model, the Symmetry region normal is X-axis but it should be Z-axis.

Remote Force Z coordinate is at 100 mm when it should be at 500 mm.

Displacement BC is duplicating the symmetry region constraint.

 

Close