consist of measuring units

[enrico1979]

Bye-bye.

I have a problem with measuring units used with patran.
I press that amount a parasolid ( created with pro and, set in mm) and I wondered if for the module of young I had to insert 2e5 (which I think right, as with the mm and n the relative coherent unit are the mpa)
If so, however, I obtain not similar results, provided both mathematically, with sheet and pen, and using the simulate of creo parametric.
Can you tell me where I'm wrong? ? ?

 

[Onda]

Bye-bye.

I have a problem with measuring units used with patran.
I press that amount a parasolid ( created with pro and, set in mm) and I wondered if for the module of young I had to insert 2e5 (which I think right, as with the mm and n the relative coherent unit are the mpa)
If so, however, I obtain not similar results, provided both mathematically, with sheet and pen, and using the simulate of creo parametric.
Can you tell me where I'm wrong? ? ?

often when it amounts a parasolid in patran amounts it in inches instead of millimeters. always check that the measuring unit is correct.
2e5 is good for steel. it is right to use mm and mpa. forces in n., accelerations in mm/s^2 and masses in tons!!, denista' in ton.mm^3

 

[enrico1979]

hi wave apologies if you stress

but I checked the dimensions of the componmente in patran (from geometry>show>distance and the distance between the 2 extreme points is right, that is the measure is to be in mm).
fixed for steel the module of young 2.5 and 0.3 that of poisson, I continued the analysis imposing newtow as a unit of measure of force. relative to the mass and density not included values of any kind assuming to neglect them (I think it can be done, or at least in ansys, from which I come this option is contemplated).
I carry out the simulation and in the post I get the results to say little exaggerated (where ansys says a voltage of 85mpa, patran gives me a value of the voltage of 1.3e4 (13000) I do not know what, I think mpa, but it would be absurd even if from the units used the output of voltage should be in mpa ).
you have the slightest idea what can induce such strange results (as you will have understood I am trying to learn such software and the evidence made is on a beam - square boxed 1000mm long and section of side 100mm, often 5 mm -a shelf loaded on the free end with a f=5000n )

 

[Onda]

If the beam is isostatic, the elastic module does not change the result of stress.
If the very high values are located at the disaster, it's easy that it's a problem of constraints

 

[Lorenzo_Z]

is the force applied the same? what order do you get?

sometimes putting a total load or a point load on n nodi has different moool effects.

control the values of strength, it can only be that.

Hi.
Lorenzo

 

[enrico1979]

Hello there

As you understand, it's all but a patran expert.
then the force was applied by me ( 5000 n ) to the end surface
not bound by the beam (I used the button that allows to select the surfaces and I selected the end section) . the deformed values do not remember them as the file I preferred not to save it (but I assure you that even in this case the orders of magnitude were far out of the real results, calculated with ansys and hand-held-treated of a supported beam and wrong is really difficult -).

 

[Onda]

Hello there

As you understand, it's all but a patran expert.
then the force was applied by me ( 5000 n ) to the end surface
not bound by the beam (I used the button that allows to select the surfaces and I selected the end section) . the deformed values do not remember them as the file I preferred not to save it (but I assure you that even in this case the orders of magnitude were far out of the real results, calculated with ansys and hand-held-treated of a supported beam and wrong is really difficult -).

when applying a force to the surface, Patran applies the force to each knot of the surface.
the simplest method is to create a rbe3 and apply the force to the dependent node (single) of the rbe3.
Consider that the rbe3 must be created by binding 1a3 independent nodes and by binding 1a6 the dependent node.

 

[Onda]

Maybe I was a little cryptic.
Patran applies the same force to each knot, in practice multiplies the force by the number of knots.
If you want to continue applying the force to the surface you have two possibilities: either count the knots and divide the force for the number of knots, or use the utility load/bc resultant that calculates the result of the force applied, the product of the force inserted for the number of knots and then divide the force to apply for the number of knots.

 

[enrico1979]

Thank you wave.

to be honest I imagined something like this (from the interface we noticed how the force at least was applied to the 4 corners of the section) but to be sincere I did not want to believe it (I come from the world of ansys, and the worckbench mechanical has no such problems even if I think it can be considered less reliable).
I will see to solve by following your advice, even if such a thing and the little material available (I talk about documentation and tutorials ) make me a moment reluctant to learn a software that I think ostico (the classical of ansys is perhaps even worse but I have about 15000 pages of documentation and more than 300 tutorials on which I can count )

I'll let you know

thanks and good work

 

[Onda]

basic with patran normally work directly on the fem entities and not on those cad.
when you get used to working well.
there is a lot of documentation, even on the net. Just look.
the software is ostico, however it is a reference in a certain type of industry (airboating / space).
to you choose whether to use this or other.

 

[enrico1979]

hello wave

I preferred to make a test with uniform load applied on the upper surface of the beam and finally the voltage and deformation values that I get match perfectly with those obtained with ansys.
this and your advice prompt me to investigate the software (and parallelly I will try again with ansys so as to perfect both-- maybe a little ambitious but will not fail)

Hello and thank you

 

[Onda]

if you apply force on a rbe3 having node dependent in the center of the load surface the results should be exactly the same as ansys.

ansys if I am not mistaken by applying a force on a surface the blade so that the resulting is in the center of the surface.
On the other hand, by applying force on knots, you do not know a priori the center of force applied as it depends on the density of mesh.
the way, to bypass this problem is to use a rbe3 with central knot at the desired point. is nastran cure then apply forces to knots in order to get the correct result

 

[enrico1979]

hello wave

Sorry to stress you. especially thanks for the precious rabbits.
from what I ask you would seem that anyway I do not follow them (you told me of reason for fem elements and not fall), but if instead of the force I use a total load on the terminal section of my blessed shelf beam, I solve the problem related to the need to impose an euiripartite force for the knots that are on the section in question? ?
At the level of result we are ( matchano that is a beauty with ansys) your perhaps to me is escaping something, but can I generalize, that is to use the total load every time I intend to apply a force to a surface?