Skip to main content
K
KG_76810274-Participant
4-Participant
October 26, 2023
Solved

Creo Simulate 8.0.8.0 Determine Max Force up to Yield Point

  • October 26, 2023
  • 2 replies
  • 3319 views

Howdy PTC folks!

 

Do y'all know how to run an analysis that can determine what the maximum force load (up to the yield point) can be for any particular low carbon steel part given a specific geometry, and force location/direction. 

 

Surely there is a way to do this, right? I've seen tutorials on how to optimize certain features of the design like material thickness or other dimensions, but what if I just want to know how much of a load a particular part can handle? The only way I know how to do it is by running multiple simulations and increase the load incrementally each time until the von mises stress gets close to the yield strength. Which is very inefficient IMO. 

 

Thanks for any help on this!

Kevin

 

 

 

KG_7681027_1-1698336721303.png

 

 

 

Best answer by ChrisKaswer

The load will be increased as a percentage (0 - 100% is from time 0.0 - 1.0). So time 1.0 will be the application of the full load, 0.5 time will be equal to 50% of the load you applied, and so on.

 

I hope this makes sense,

 

Cheers

2 replies

C
ChrisKaswer16-Pearl
16-Pearl
October 26, 2023

If you run the analysis with geometric non-linearity turned "on" ("Calculate large deformations"), you can have it run load steps. The results can then be used to find which load you hit the material's yield. Here is an example of the analysis set-up dialog box you'd see when this is active:

ChrisKaswer_0-1698345983923.png

I hope this helps!

K
KG_76810274-ParticipantAuthor
4-Participant
October 26, 2023

Thanks for the quick response! I tried the different load steps, which does increase the max stress as you move from 0 - 1.0. But, still not exactly what I'm looking for. Also, can you explain what is happening between time 0 to time 1.0 that is causing the stress to increase? The load remains constant, correct? 

C
ChrisKaswer16-PearlAnswer
16-Pearl
October 26, 2023

The load will be increased as a percentage (0 - 100% is from time 0.0 - 1.0). So time 1.0 will be the application of the full load, 0.5 time will be equal to 50% of the load you applied, and so on.

 

I hope this makes sense,

 

Cheers

    S
    SweetPeasHub17-Peridot
    17-Peridot
    October 26, 2023

    You cannot put all types of parts into the same FEA method. The image shown is complex to analyze and is likely infinite stress at the sharp inside corners where the high stress is appearing. If you keep refining the mesh and the P-order the stress will go up and up and up for the same load. This is why those types of sheet metal parts have stress relief cutouts at those corners.

     

    If you don't have that type of issue then simply run a linear analysis and scale the results linearly. Linear is a good assumption for many metal parts especially if you don't go past yield.

     

    Scaling example for a linear static analysis:

    First run with 1N load.

    Find the PartStress produced.

    YieldStress / PartStress = K  (scaling for the load)

    1N * K = new load that produces exactly yield.

     

    That said, sometimes I run a non-linear material to allow some yielding that stress relieves those difficult areas. Certainly low carbon steel can take quite a bit of yielding (like 20% strain) before failure, which is why it can be bent like your image. But, also the material has changed after bending unless it is heat treated, so that needs to be considered too.

     

    Hopefully that gets you a bit further along regarding your general question on FEA analysis for stress!

     

     

      Terms & ConditionsCookie settingsAccessibility statement