msg error during a wb simulation

[xLOGANx]

Excuse me! Has it ever happened to any of you to get a message like this in the middle of a simulation?
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 at least 2 directions if solid brick elements are present. please see the troubleshooting section of the help system for more information.I press that, for reasons of excessive weight of the model, I had to transform some solid elements into surfaces (with the mid surface command). In addition, the model has an aluminum base bound by steel longheron bolts: I set the frictionless as a state of contact surfaces.

Thank you.

 

[Vmax]

Yes, it happens often.
typically happens because there is a local or global lability.
try with all bonded contacts and see if it turns, take a look at the results and see if something moves as it should not.
if it still gives you error verify the mesh that is probably a little too shady.
In any case, be careful with the solid-shell mixed models, they are very prone to being labile typically on the shell-solid or shell-win interface, but you should see it by looking at the deformed.

 

[jaccio404]

the best constraint configuration is the right isostatic? Of course, for certain particular situations!

 

[xLOGANx]

Thank you vmax. the trouble is that the simulation is interrupted on the birth and therefore it is impossible to see the result. However, since you suggested that I take a look at the contacts... I saw that many of these are wrong. I'll explain.
the aluminum base flows on steel guides and, by force of things, there are lights of 1 mm between the faces of the profiles. I do not explain why wb individuals a contact between these faces that are detached even if only 1 mm. I tried both to inflate the mesh and to change the value of the pinball region but nothing.

There is a way to make contacts only those that arise from faces actually in contact.

Hi.

 

[jaccio404]

I suggest you delete automatically generated contacts and set them yourself manually. always that your model is of such size to allow it! even to me the software sets the contact automatically when 2 parts are simply close!

 

[Vmax]

you can change the tolerance with which the surfaces to be held in contact directly from the contact group controls are automatically detected. or as jaccio suggests you can delete the automatic ones and do them by hand.

in any case the speech is that if you put all bonded contacts, even if they are overflowing, and the structure remains labile, there could be free components. I suggest you add one at a time and check.

 

[xLOGANx]

I'm sorry. first I thanked only vmax not having seen your post. In practice I have deleted all contacts and I am reinserting them by hand. :frown:

 

[jaccio404]

Don't worry. However, I have not yet understood exactly what changes, but I suggest you also set the most rigid element as target and as contact the most flexible one.

 

[stefano.garbin]

use the "contact tool".
click with dx mouse button on "connections" - > "insert" -> "contact tool".
for how to use search in the online guide.
this allows you to check immediately without launching the simulation as are the contacts (closed, open etc.)

 

[xLOGANx]

hi stefano, the analysis of the contacts I made it as well as you yourself suggested in another post. the problem is that some contacts are highlighted of red and others of orange; In reality, from model cad, there are neither gap nor compnetrations. and then why are these contacts highlighted as open when they are not?

 

[stefano.garbin]

Okay, let's do this one step at a time.
in the contact tool each contact couple takes 2 lines (see also written "contact" and "target"). start counting true row pairs until you find the first red or orange row. You've come to number five... go to the contact tree and find the fifth contact. see if it is defined well, if there are no gap or compnetrations and even if the mesh elements have quite similar dimensions.
if you don't correct the contact couple and repeat what I wrote to you.

Alternatively create a new modal analysis, convert contacts to "bonded" and see ways to vibrate at zero frequency. those are rigid motions of untied bodies.

 

[jaccio404]

Damn stefano, this is a schicceria!!! I never thought about doing something like that! on the card, however, stands!

 

[xLOGANx]

So, guys. First of all, thank you for the tips. the problem of some "red" contacts was mesh...or better the wrong value of the mesh elements. correcting these, the state of contact has changed from red to white.

some orange contacts remain. These contacts exist between a linear guide and rollers on which this flows. (if you want I place an image). even trying to change the mesh, the contact status does not change.

 

[stefano.garbin]

put the image so we understand!

 

[xLOGANx]

place 3 pictures, so explain what I did. in the first picture I highlighted the frame entirely in aluminium: is a welded and on it is housed a case that carries a weight of about 100 kg.
This frame flows on two profiles (aluminum section) connected to steel longherons (figure 2). I set the contacts of frictionless type to the longherone-profile interface to l.
in picture 3 you can see the guide (solidal to the frame) running on the rollers (mounted on the profile to l).

Moreover, I have inserted circular beams in the holes present on the profiles to l and the longherons: In this way, with a probe, I can define the forces agents on what then in reality are the vines.

Where am I wrong?