Simulation giving incorrect results

[cmosen]

Hey guys,

I've been trying to do a deflection simulation using Creo
2.0 Simulate which gave me really weird results. I
simplified it right down and still am having issues
however, I think there must be a setting or property
somewhere that I don't know about. The model is a 2000 x
225 x 1.5 mm stainless steel plate, with one of the short
edges (225 x 1.5) fixed in place using a displacement
constraint which is fixed in x, y and z direction. Then I
applied a gravity load acting perpendicular to the 2000 x
225 mm surface. My simulation gives me deflections in the
range of km's for some reason, and the deformed display
with no scaling shows an unrecognisable model.

I would have thought that the plate would simply have a
'drooping' appearance with a much smaller maximum
displacement. When I plot the undeformed shape it has the
contours in the correct place, i.e. deflection magnitude
slowly increasing, the scale is just way off.

I have also tried placing a small point load at the end
instead but it had similar results. I used the included
stainless steel material at first, and then tried a
custom one with the following properties set: Poisson's
Ratio - 0.3, Young's Modulus - 200 GPa, Density - 8000
kg/m^3

Does anyone know what my problem could be?

 

[Kaz Z06]

cmosen,


Did you select and edge for your constraint or one of the end surfaces of 225 X 1.5? If it let you use and edge and did not give you a warning and terminate, there is a problem with your install of the code. Did you run the analysis using shell or solid elements? I ran your problem using solids and constrained the small surface in X-Y-Z and got a max displacement of 4.1 m, not km. This result seems "reasonable" since the part is a long, thincanteleveredplate bending under its own weight in the weakest direction, AND we're assuming linear material behavior.


Now - here's a plausable scenario - I re-ran it using the Creo default units of inches (for USA installs anyway) and your same dimension values and got a result that does find displacment in the "km" range.Check your unit system just in case, otherwise there is no explaination. If this isn't the issue, maybe you can share the model you used for us to take a quick look at.


Cheers,


Kaz

 

[cmosen]

Thanks for getting back to me Kaz, this was on a computer
at work so I'll try post up the model tomorrow morning
(NZ time).

I selected the face not the edge. Would it really deflect
4.1m? That still sounds unreasonable to me as it is only
2m long, or is that a limitation of the linear analysis?
I'm fairly sure it is using solid elements.

Going file > prepare > model properties (those names
might be wrong, just going from memory here) shows that
the units are set to S.I, which would have been setup by
the systems staff so I would have thought that the units
all matched up.

 

[cmosen]

Okay so for some reason it won't let me upload the file

But still, 4.1 m sounds far too large to me as that would
mean there is significant deformation of the plate which I
don't think would happen under these conditions

 

[Ray Ellender]

Units.


Although these days it should be able to cope with mixed units, to be safe make sure that you are using a consistent force-based unit set. If your dimensions are in mm, change the model's units from mm-kg-s to mm-N-s. Then make sure the density is the correct value in tonne/mm3. (Typically 8e-9 for a steel). Then apply the g load as an acceleration of 9810 mm/s2 (or whatever it is in NZ!)


Constraints


Then as regards your constraints, if you want a built-in constraint, you must fix the rotations, otherwise you will get a hinge, which may well be what is happening. However solid elements don't understand rotations so you must make sure that the surface is constrained in translations (as opposed to an edge), which will prevent a hinge forming. On the other hand if you are using shells, then you should constrian an edge, rather than the surface, and constrain the relevant rotation as well as translations.

 

[Kaz Z06]

I've found that if you run the problem using non-linear, large deflection and mesh it using

 

[cmosen]

Unfortunately when I try these options, non-linear, LDA and thin solids, I'm informed that an advanced UI license is required so I'll have to see if anything can be done about that.


I guess it makes sense that LDA is necessary really as the deflections will be relatively large, if not 4 metres.