force or pressure

[stef_design]

hi guys, I have a doubt
If I have to apply a load in ansys wb to a surface, example 1000 n, do I apply it as a force or pressure bond?
They told me that:
- the pressure constraint is applied throughout the affected surface;
- if I want to use force I divide the force by the number of knots that form the surface on which it is applied, so as to apply a part of force for each knot.
Is that true?

 

[volaff]

If I don't remember badly... It's just like you said!

 

[Vmax]

It's not like that.
from the point of view of the calculation ansys wb reasons so: the boundary condition is always in terms of pressure. so even when applying a force he translates it into a pressure, so the force is still divided into the application area.
But there are differences if you impose pressure or force. what I say is true in general (then wanting you do everything and the contrary), we say standard scenario.
if you impose a force, also impose a direction of application that remains constant on All the surface of application.
if you impose a Press, impose a compression effort towards normal locale on the face, and then the direction is by default variable from point to point. you can also change the pressure module according to specific laws (e.g. hydrostatic).
There are other differences, like with forces you can't load multiple surfaces, but I would say that's the point.
the difference known on curved surfaces. Try.

 

[stef_design]

se imponi una force, also impose a direction of application that remains constant on All the surface of application.
if you impose a Press, impose a compression effort towards normal locale on the face, and then the direction is by default variable from point to point. you can also change the pressure module according to specific laws (e.g. hydrostatic).
There are other differences, like with forces you can't load multiple surfaces, but I would say that's the point.
the difference known on curved surfaces. Try.

hello vmax, if I understand correctly, in case you want to apply a load to a sup. curve is better pressure, in case instead of a flat surface I can choose also strength. Right?
Hi.

 

[cacciatorino]

hello vmax, if I understand correctly, in case you want to apply a load to a sup. curve is better pressure, in case instead of a flat surface I can choose also strength. Right?
Hi.

No, actually, the speech would be:

If, for example, you apply a direct force along the "z" axis, it will remain direct along z even if the surface on which it is applied moves into space due to the deformation of the solid under the outer load.

if instead apply a pressure, it will always be normal to the surface even if it is oriented in the space during the deformation resulting from the application to the load.

However, it seems strange that ansys does not foresee the application of nodal forces. I use code_aster and there it is possible to impose geometric relationships between a knot and a surface. at that point, the force (or the bond) applied to the node are transmitted to the surface transparently to the user. Try to look at the manual well or do a google search, I think you can simplify your life not little!

 

[Vmax]

what hunter says is still different: the follower-non follower loads.

what I said was much easier: if you have a pressure on a curved surface, the pressure acts at every point of the surface according to the normal direction to the surface at that point. instead if at the same curve surface apply a force according to a given direction, in each point of the surface will act a load that locally has the direction assigned regardless of the curvature.

from the practical point of view, if you perform a linear calculation, apply a force on a flat surface or even pressure with the same result, is equivalent. If instead the surface is curved is not the same thing.

 

[stefano.garbin]

vmax explained well.
But I would like to clarify a thing: in ansys the forces are applied to the knots.
the fact that wb makes you "believe" that you go to apply them to a surface is not properly correct. In fact, transparently to the user, wb "supports" a mesh of surf154 elements on each surface on which you go to apply forces or moments.
force or moment are applied to the "master node" (I don't know if the name is the right one) which then distributes them to all knots. among other things you can choose whether to stay rigid or flexible the surface of application of the loads.
I believe (but I must verify) that from version 14 wb can apply forces and moments directly on the knots.

 

[stef_design]

thanks a lot of guys for the explanations:finger:
next,
stefano:smile:

 

[stef_design]

I take the discussion. I have a doubt.
the first option that asks me the force bond is to select an application sup.
If I have any surface and I click at a random point, an arrow appears to me.
Sucessive steps are to introduce a numerical value and a vector direction.
but the arrow remains firm not at the center of the surface but at the point I clicked at the beginning to select the sup.

in terms of ansys reasoning, the force is applied homogeneously to the surface or is it dots and corresponds to the point I clicked to select the surface?

 

[stefano.garbin]

the force is "split" on the surface.
visually speaking the carrier remains at the point where you clicked.

 

[stef_design]

the force is "split" on the surface.
visually speaking the carrier remains at the point where you clicked.

Thanks stefano

 

[MatteoFEM]

I have a question, since the subject touches me. How do you create a master node in workbench? very kind