convergence problem

[saclovitzky]

Hello,

I've tried to model a 15mm thk steel plate with 203x203UC46 steel column section(pls. see attached file).

The steel column is offset from the center. But I encounter some convergence problems.

Any particular reason why it is happening?

Any help will be greatly appreciated.

[Rafacascudo]

change mesh size to 5cm and nonlnear parameters to the picture below

[saclovitzky]

Thanks@Rafacascudo for this,the convergence problem is gone.

Also, the tensile force on the anchor bolts(near steel column) are 10x higher if using the non-linear analysis(pls. see attached screenshot)  compared to static analysis(pls. see attached static model).

It seems to me that the tensile force coming from non-linear analysis are quite outrageous(am I correct in saying this?).

[saclovitzky]

Also, I've attached two steel plates model,where the bolts arrangement is symmetrical and the result can be checked manually.

Again, the non-linear analysis result is not as expected compared to static analysis(pls. see attached files and screenshot).

Any particular reason why the result from non-linear analysis is way off.

[DennisVDijk]

hello @saclovitzky,

I think your elastic soil value is way to stiff. your support are anchors so they have a spring value too + uplift Z-.

this is what you want, i guess:

model attached. 

i hope this will help.

[Simau]

Hi @saclovitzky 

As soon as there is a possibility of uplift, you must use only non linear analysis. Indeed, as soon as the plate detaches from its support, the vertical forces in the local supports are nul.

Comparing NL and L analysis when uplift exists has no sens
As pointed by @DennisVDijk  in your model, the rods are also nonlinear supports because when the plate rests against its support, the forces in the rod are zero.

@DennisVDijk   said "I think your elastic soil value is way to stiff"

I think @saclovitzky is trying to set up concrete parameters.

[saclovitzky]

@Simau thanks for this, but using your suggested support,I also encounter convergence issues, can you fixed the file?

[DonBAE]

review this video from AISC: https://www.youtube.com/watch?v=x_P1EezPXGI

flexibility of the plate will significantly impact the anchor tensions.

[Simau]

Hi @saclovitzky 

Use "Pinned but uy UZ-" supports

Model attached

[saclovitzky]

@Simau Thanks for this.what really bothers me is the result,the anchors are symmetrical with the moment at the center(between the achors of the opposite sides).

when a moment acting at the center of the supports ,it produced equal compression/tension reactions(couple);ie, M =15 kN.m, c/c distance =0.48m,then, 15/.48 =31.25 kN(31.25/2 = 15.63 kN/bolt), but since the support nullifies the compression(-z),only the uplift will show(in this case,the linear analysis produced 65 kN/per bolt! ).

In my opinion the result is not acceptable.did I miss something here?

[Simau · Accepted solution]

Hi @saclovitzky 

Your verification is not correct (You forgot reactions at finite element nodes).

So that you can see all the reactions (at the anchors and in the finite elements), I've used  surfacic support instead of soil parameters directly to the plate.

Redo the check with all reactions (at anchors and other nodes)

Model attached

[Stephane.kapetanovic]

hi @saclovitzky,

Let me add a few more thoughts to your discussion. No, I don’t think the reactions can be symmetrical.

Another key point is that the load application isn’t a true point load, it’s the 203x203UC46 section that transmits rotation to the plate. As such, even the forces in the rods should be evaluated by including at least a small portion of the column, to reflect both its stiffness and its ability to distribute loads.

It’s also worth noting that you're assuming the concrete provides uniform pressure (if there is any concrete shim). This overlooks how the plate interacts with the support. It’s possible that the compression zones are primarily located beneath the column flanges, and not at all where they are currently assumed.

Some time ago, I developed a small program (AutoConnect) "based on the Eurocode" that transforms the base of a fixed column into a finite element model. You might find it helpful to explore something similar to see where it leads you.

Best Regards

[DonBAE]

before we all give potentially inaccurate advice which base condition do you have from the below choices A or B

In A there is a grout layer between the concrete base and the base plate so compression support is provided by the concrete through bearing in B there is an air gap beneath the base plate so compression must be developed through the anchors.

[saclovitzky]

Hello @DonBAE , pls. see attached

[saclovitzky]

@Stephane.kapetanovic ,thanks for your time in doing this.I'm just wondering is there any simple modelling other than solid modelling that I can resort to(simplified model)?

[Stephane.kapetanovic]

hi @saclovitzky 

This is a plate-and-shell model, not a full solid model. The results are obtained in just a few minutes. In your case, you should move the column to the edge of the plate and add the two small gussets. To achieve this, you need to start with a bar model and add a fixed column connection. AutoConnect will then be able to export the forces by cases, although you can also adjust them manually if needed.

Best Regards