Skip to main content
J
JouniAhola1-Visitor
1-Visitor
January 14, 2016
Question

How to constrain long profile?

  • January 14, 2016
  • 1 reply
  • 5810 views

Hello,

What is the best practise to create constraints for a profile? The thickness is 1-3mm and length 1000 to 6000. I am using family table and want to make sensitivity study.

I am using shell pairs and I create surface regions as constraints. This causes singularities to the edge of the regions and

the result stress von Mises is unreal.

Jouni Ahola

1 reply

M
mlindqvist1-Visitor
1-Visitor
January 14, 2016

There are different techniques.

1. Extend your model to also include what the profile is attached to. This might involve contacts (which need to be modeled with solid elements in Creo). Whatever it is your profile is attached to, this is elastic and can deform, which reduces stress peaks at the edge of your constrained surfaces.

2. Ignore the stress peaks at the edge of your constrained surfaces. The critical stress can be evaluated using for example the hot spot method, which extrapolates the stress from the "interior" to the edge where your non-linear stress peak is located. For example the IIW has documentation on how to use the "Hot spot method"

3. Use a beam combined with a weighted link, that connects a beam endpoint to your constrained surface. The weighted link allows some deformation of the target surface and you will get more smooth results.

In eihter case, you can still use for example the hotspot method to evaluate the stress level. This is OK according to some norms, I think also the Eurocode 3 standard allows evaluating welds according to the "hotspot method".

Here's a demo I did some years ago, on weighted links (in Swedish)...  Mechanica - YouTube

/Mats L

J
JouniAhola1-VisitorAuthor
1-Visitor
January 14, 2016

Thank you for the answer. I made as in your first answer. Now it looks better. I made an assembly, I will attach picture later. I need to test rigid links as well.

I can not ignore peaks, because I need Excel graphs for different height and length  of the profiles. I am going to make sensitivity study

and profile lenght is varying from 1000 to 6000mm. And even 12 000mm profile lengths.

Beam is one what I need to consider.

I noticed one rather strange thing. When I change the profile length from 1000-5999mm, I can use shell for meshing. But when the length is 6000 or more, Creo  automatically use solid surfaces for meshing???

M
MikkoHinkkanen15-Moonstone
15-Moonstone
February 2, 2016

For allowed relative deflection, you may use computed measure.

  • create parameter in Creo Parametric witch will have value of length of your beam (use relations)
    • length=d8
  • create measure in Creo Simulate for Driven parameter
    • length_parameter
  • create max_disp_mang_user measure in Creo Simulate
  • create computed measure relative_disp in Creo Simulate
    • max_disp_mang_user/length_parameter
    • you may Specify Allowables (0, 0.005), which will show on log

measure_relative_disp.JPG

###

Your loading height q has units of [N/mm]. If the length of beam will increase, so will the total force F=ql. This will lead to possibility to use another relation to capture the required force F for certain q (total load case).  Or use your imagination&calculator to get proper value for Force per unit area and use that as is.

You can use Creo Parametric parameters at Creo Simulate force dialog. Click RMB (Rigth Mouse Button) at force component definition, pick Parameter..


You can use feasibility/optimization to find what is the max allowable length for beam, when:

  • relative deflection must be < 1/200
  • stress must be less < max allovable
  • etc...
Terms & ConditionsAccessibility statement