Showing results for 
Search instead for 
Did you mean: 
Showing results for 
Search instead for 
Did you mean: 

Creo3: Stress doesn't change regardless of load.


Creo3: Stress doesn't change regardless of load.


I'm trying to run a Creo 3.0 simulation of load on a disk. When I run the simulation, the stress remains constant regardless if my load is 100 psi or 0 psi. I've attached two images of the part.

The parts axis of symmetry is on the y-axis.

Constraints1: A pin constraint at the hole foxed in translation and rotation.

Constraint 2: A displacement constraint at the rear submerged face. Fixed on the y-axis, free in the x and z directions.

Constraint 3: A displacement constraint at the front on the small raised section, Fixed on the y-axis and free in the x and z directions.

Load: A pressure a applied on the outside back surface.

Material: I had to set my own material properties as it's a glass filled Noryl plastic part and the standard library doesn't have any anything.

When I run the simulation, the stress at the center is always 390ksi, regardless of the load.

Please let me know what I'm doing wrong, as I need to get this part redesign completed.

Thank you.


Is the stress the same everywhere, or only at one location?

Are you doing an anlysis with material plasticity?

If you repeat the simulations with forced displacements equal to zero, do you see the stress results change?

Sorry, I should have been more clear. The stress itself is distributed with the greatest concentration at the hole, as would be expected. However, I can set the pressure load to 0 psi or 100 psi along the outer surface and the stresses at the center hole are still exactly the same.

I'm not using material plasticity as apparently our simulate license doesn't support it. It's linear.

I've attached the Von Mises stress distribution that I end up with, which never changes regardless of the loading.


There was a similar post a week or so ago - I think the soluiton was to use large deflection analysis.

Also, if it is fixed in the Y axis on both faces, how is there ever any displacement to cause strain? With no strain there is no stress.

The back face you see is fixed across 90% of the diameter. However, the opposite face, against which the pressure force is pushing, is only fixed across about 30% of the face, so the edges can and do deflect with the pressure load in the Y-direction. It's just the small raised face on the opposite side of that shown above which is fixed, as shown in image d2.

I guess I really can't tell what areas are entirely fixed, but experience with this has shown that when analysis results are unexpected for simple cases it is always because the loads or the constraints are unrealistic.

Why are there any areas fixed in Y besides the pin, particularly both sides? Is the only load from displacement from the pin? What does an exagertated displacement look like - if the part doesn't deform realistically it won't have realistic loads.

Perhaps a stupid question, but... your picture says "mode1"... is this a modal analysis?

Yes, it's a modal analysis. It's the only analysis our license allows.

Hello Jason,

have you been able to figure out what was wrong? If yes, please let us know!

Otherwise, the limitations of your license remind me of something: Have you checked for messages telling you that some features are ignored for the analysis (we sometimes have/had such messages when specific features were not supported with specific analysis types or licenses)



I don't think modal analyses use a 'real' force value - it's more like a unit load, and I don't think that the loadset you apply are actually used (only the constraints).

As I understand it, stress and deflection values for a modal analysis are only indicative of the 'shape' - they are not absolute values. I believe this is true in any FEA system, not just Mechanica (sorry, Creo Simulate).

A modal analysis ignores all loads. The stresses that are displayed shows the stresses at a "normalized" displacement of "1". The displacement you see as a result from a modal analysis is the deformed shape during free vibration, i.e. there are no forces applied to the structure.

I find it strange that your license allows you to do a modal analysis, but not a static one. What kind of license is this? To tell from your geometry, it is possible that your problem can be solved in "Simulate Lite" which is available to all Creo users. Especially if you utilize symmetry in your model - the problem looks symmetric from what I can see in your pictures. Creo Simulate Lite has a limitation as for the number of surfaces in the model; for this reason it may be necessary to use symmetry and reduce the number of surfaces. From what I can see, it should be possible to use 1/12th of the model.

To activare "Simulate Lite" click Model Setup and check the "Simulate lite" box.