it's grey, but i'm not touching

[ansyolitico]

Hello everyone
I'm using ansys for the first time to finish my thesis. I'm a donkey and I jammed.
I modeled my solid (a press) with solid works and I'm analyzing only a quarter using geometric symmetry and the distribution of forces. I have inserted everything by hand including various constraints of contact ( bonded and frictionaless) but when I start the resolution freezes by telling me

"an internal solution magnitude limit was exceeded. please check your environment for inappropriate load values or insufficient supports. also check that your mesh has more than 1 element in least 2 directions if solid brick elements are present. please see the troubleshooting section of the help system for more information."

I counterbalanced the various contact constraints with the contact tool and found two yellow and inactive seals...and I don't explain why. .

someone would tell me what I'm wrong... thank you

 

[ansyolitico]

Can't anyone help me?
Did I ask a banal question?

 

[cacciatorino]

Can't anyone help me?
Did I ask a banal question?

I think the real problem is the one indicated in the second line, that is, you have substantiated bodies.

Since you have contacts, you probably need to help with "soft spring" at least in the first load steps, but the solutor doesn't know what to do. Then of course you will have to use consistent measuring units, which are less trivial than you imagine, especially if you are also treating weight strength.

 

[ansyolitico]

I'm sorry if I ask you, but what are soft springs?

 

[gerod]

weak springs.
Before using the software it would be better to know a little theory and read the tutorials.

 

[ansyolitico]

as if I hadn't watched the tutorials.. It's more than two weeks I'm looking for tutorials and I don't find a cicca for my problem. .
on the manual does not write us on soft spring...intendo ilhelp di ansys...cerchero on the paper manual. .
even the tutorials say that the soft spring sets them by itself...boh.. .
Where do I look for tuturials?? ?

But I haven't been able to figure out why it gives me inactive contacts?

 

[volaff]

I don't know if it's your case but I recommend the following text including video:

"finite element simulations with ansys workbench 14 ".

If you're in the first weapons you'll certainly be able to help!

 

[Onda]

reduce the number of pieces as much as possible. uses bonded and mesh coarse contacts.
once it comes to convergence it begins to refine, if possible not to use frictionless but contacts with friction, are less erratic.
you probably have not properly bound components and that can't be "stop" only with contacts.
test with these settings and gradually return to a more labile configuration.

 

[ansyolitico]

I think I understand the problem
I have two yellow frictionaless contacts and correspond to the pull nut with the spacer on which it rests and the piston with the base on which it discharges all the pressure.
now both have a 7 mm offset between nut and spacer and 5mm between piston and base. I set the contact with an influence radius of 30 mm for each (exaggerated but to be sure).
suppressing both the operating pressure of the cylinder chamber and the pretension of the puller(s) and leaving only the weight force I can achieve convergence.
by going to see the results of the deformation known that both the nut and the piston penetrate in their respective supports as almost as if the contact constraint (frictionless) did not exist. ...someone could help me
Is there any options to set in the contact?

 

[cacciatorino]

I think I understand the problem
I have two yellow frictionaless contacts and correspond to the pull nut with the spacer on which it rests and the piston with the base on which it discharges all the pressure.
now both have a 7 mm offset between nut and spacer and 5mm between piston and base. I set the contact with an influence radius of 30 mm for each (exaggerated but to be sure).
suppressing both the operating pressure of the cylinder chamber and the pretension of the puller(s) and leaving only the weight force I can achieve convergence.
by going to see the results of the deformation known that both the nut and the piston penetrate in their respective supports as almost as if the contact constraint (frictionless) did not exist. ...someone could help me
Is there any options to set in the contact?

I'm sorry if I tell you, but I think you're going a little bit for a try. Now if the goal is to do realistic analysis, you need to know what you are doing, otherwise they come out of the completely unreliable results, and what's worse there is no way to know that these results are such.
the fact that a converged solution is not an indication that it is realistic: Maybe you should go back to the theory, otherwise the risk of taking fireflies for lanterns is very high.

 

[ansyolitico]

I'm sorry if I tell you, but I think you're going a little bit for a try. Now if the goal is to do realistic analysis, you need to know what you are doing, otherwise they come out of the completely unreliable results, and what's worse there is no way to know that these results are such.
the fact that a converged solution is not an indication that it is realistic: Maybe you should go back to the theory, otherwise the risk of taking fireflies for lanterns is very high.

Your colleague above just told me to change all the bonds above into bonded and to release them shortly at a time... is it not a go for attempts?
If you have to answer, answer if you know why you don't make unnecessary remarks. that already is frustrating not to solve problem... if you put us in. .


and in any case I have an analytical model (forms, integrals, aiosa theory and 3 years of study...I don't know what they are worth at my point)...and in fact, by tapping the results of this I'm not at all with that fem... so I distinguish both the lippies and the lanterns.

Now if there's someone who can tell me why a frictionless contact penetrates the contact surface makes me a huge favor. . .
If not avoid that you save me a useless mess...

thanks in advance

 

[stefano.garbin]

Hi.

contacts you see highlighted in yellow tell you that the contact surfaces are within the "pinball region" but are not perfectly in contact (i.e. there is a small gap).
Now, if you launch the simulation with a load too high, or with too many substeps, at the end of the first substep, the surfaces have already penetrated so much that the contact itself is no longer recognized.
solutions can be:
1-apply the load more gradually (e.g. if the bolt is preloaded with 1000, fima you make him make a step with 1 that closes the contact well, and then increases it to 1000)
2-increase substep number (analysis settings - auto time stepping = on - and games on the initial number and maximum number of steps)
3-in contact properties - geometric modification - interface treatment - you must select "adjust to touch", so ansys applies a small offset to the surfaces suitable to close the contact. Remember that sometimes it is better, always in the properties of the contact - advanced - update stiffness - select "each iteration" to make sure that the rigidity of the contact is updated at each step.

 

[ansyolitico]

Hi.

contacts you see highlighted in yellow tell you that the contact surfaces are within the "pinball region" but are not perfectly in contact (i.e. there is a small gap).
Now, if you launch the simulation with a load too high, or with too many substeps, at the end of the first substep, the surfaces have already penetrated so much that the contact itself is no longer recognized.
solutions can be:
1-apply the load more gradually (e.g. if the bolt is preloaded with 1000, fima you make him make a step with 1 that closes the contact well, and then increases it to 1000)
2-increase substep number (analysis settings - auto time stepping = on - and games on the initial number and maximum number of steps)
3-in contact properties - geometric modification - interface treatment - you must select "adjust to touch", so ansys applies a small offset to the surfaces suitable to close the contact. Remember that sometimes it is better, always in the properties of the contact - advanced - update stiffness - select "each iteration" to make sure that the rigidity of the contact is updated at each step.

for diana worksaaaa! ! ! ! ! !

You're a hottie!

I'd give you a kiss in your mouth, and with your tongue, you're a man, you're hurt.

You saved my tesin... thank you very much... if you're in a mile, give me a whistle I offer you a drink... you're too big

 

[volaff]

stefano garbin is the best of ansys in Italy!