Unable to change the penalty multiplier in a critical buckling anaylsis

[ellard]

Hi,

I am getting an error message where my model is apparently poorly posed. Trawling through the Help pages, I have found an article which suggests changing the 'penalty multiplier' in the analysis and re-running it.

I have found out which menu this is supposed to be in

' If you find your analysis doesn't converge or is not performing as you expect, you can try a different Solution method to use with MPC equations (see Multi-Point Constraints). Click SetupLoadsMulti-Point Constraint and choose from the Solution method options. If you use the Penalty Method, the accuracy of the solution is controlled by the Penalty multiplier field.'  From (https://knowledge.autodesk.com/support/simulation-mechanical/learn-explore/caas/CloudHelp/cloudhelp/...)

but this menu doesn't seem to exist within my copy of Simulation 2015. Can anyone tell me where it actually is?

Regards

Ella

[Andrew.Sartorelli]

Hi @ellard,

That setting is only used in conjunction with smart bonding, which is off by default. Could you share the error message that you are getting when you run the model?

Thanks,

Andrew
______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[ellard]

Hi Andrew,

Thank you for replying. I thought I had switched the smart bonding on in the parameters section before I started hunting for the setting.

I have attached a screen shot showing the error message and the 'result' the analysis gives. Any advice would be appreciated.

Regards

Ella

[sebastian.sosa]

Hello Ella,
Looking at the picture you attached to your previous post, I think that, maybe, the error message you are getting is due to the setting of your problem and that you probably don't need to change any of the"default" setting for this kind of analysis (CBL) but modify your approach instead. From the picture I'm guessing this is some kind of pressure vessel and that you're trying to check for it's behaviour under external (or negative - vaccum - ) pressure. If this is correct, let me ask you: Did you fixed some part, surfaceS or nodeS ? if not, remember that CBL analysis needs a statically stable model. It needs to be prevented from rigid body motion in all directions and taking into account you're not using a half or quarter model (maybe this isn't a possibility for your analysis) applying boundary conditions might be difficult and hence the error message "poorly posed". (Note: I'm not saying that you should use "fixed constraints" on your model. This could result in an artificially stiffer model and thus you might get misleading results.... but again, I'm not familiar with your model/preblem... it might be appropriate) Hope this helps. If my guess is totally wrong, I apologize.
Best regards

[ellard]

Hi Sebastian,

Thank you for replying.

I have the model fixed as a simply supported beam, (mainly one end with no translation allowed, and the other end only allowing translation along the axis of a pressure vessel. Rotation is allowed at both contraints). I have used FEA analysis on pressure vessels before constraining them in this way and the analysis has been successful.

If you have any other suggestions that I could try I would be happy to give them a go.

Regards

Ella

[shigeaki.k]

Hello @ellard,

sorry for joining in mid-discussion. But following from @sebastian.sosa's suggestion, "...remember that CBL analysis needs a statically stable model.", are you able to confirm this by running a modal analysis on the model?

Regards,

Shigeai K.

[sebastian.sosa]

hi Ella,

I think that Mr. Shigeaki K. suggestion is a great one in iorder to detect any possible rigid body modes. It's not quite clear to me the settings of your model in terms of your boundary conditions and, as I sayed before, without really knowing your model/problem I really shouldn't give any particular advice about that. IF there is not any confidentiality issues with your study, I would suggest that you provide more information about your setup and some description of the physical problem you are trying to simulate (or even maybe attach the .arch file) and then maybe someone will be able to give you better advice.
Best reagards

[ellard]

Hi,

Thank you for replying.

I have completed the Modal Analysis and that seemed to run properly. I have attached the results here. I have been experimenting with the setup of my model, and I can get a static stress analysis to run, as well as a model analysis, just not the Critical Buckling analysis.

I am a little stumped now. I have run models similar to this before and never had a problem.

Regards

Ella

[ellard]

Hi Sebastien,

Unfortunately there is a confidentiality issue otherwise I would love to post more information.

Regards

Ella

[sebastian.sosa]

Hello Ella,

I understand about the confidentiality. I would just say that (again, knowing very little of your analysis) 0,04 Hz for the second mode seems a bit low for such a "sturdy" model (by sturdy I mean that there are no small "loose" or "long lean" parts visible) so there might be something there to check... but then again I could be mistaken. That's all I've got ... sorry. Best of luck.
If you reach to a point where you find yourself out of ideas, maybe you can think of simplifying your 3D model (taking out any compromising or confidential details) and sharing a little bit more with the forum to obtain other opinions.
Best Regards

[John_Holtz]

Hi Ella,

I agree with Sebastian that the low frequency seems odd. Seeing that the model is in mm, I wonder if there is a problem with the units and the input. For example, is the mass density correct? (Run the "Analysis > Analysis > Weight & Center of Gravity" to check the total weight) What about the other material properties?

What type of elements are you using? Is the Element Definition correct considering the units?

[ellard · Accepted solution]

Hi all,

Thank you very much for all your help. I have found the problem now. Well, I actually found two problems, the properties for one of my materials had not transferred from Inventor properly, hence the dodgy modal analysis numbers, and I had accidentally place a pressure on the interior of the pressure vessel which I couldn't see when checking. That was the reason the buckling analysis was failing and not the stress analysis.

Thank you for taking the time to post. I solved the problem a lot faster thanks to your suggestions.

Regards

Ella