Solved: Interpreting my results

Thesunshines · ‎Aug 20, 2014

Hi guys,

I need a little help. I have run a simple simulation of a bolt under different loads. The UTS of the steel of the bolt is 530 MPa and each bolt is loaded with 265 MN. My results show three windows, one which is Stress Von mises, the second displacement and the third stress max prin.

Am I correct in thinking that the first is showing the areas of stress? Im confused since this appears to be up to 182 GPa.

The second is showing how far the bolt would be deformed and stretched and the third how the stress is mapped,how does this differ from the first one. I have been unable to find this information on the PTC site. Any help would be much appreciated.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

sdensberger · ‎Aug 20, 2014

Am I correct in thinking that the first is showing the areas of stress? Im confused since this appears to be up to 182 GPa.

You are correct. The first windows shows a fringe plot of the von-Mises stress throughout the geometry. Von-Mises stress is a scalar (ie no direction) quantity and yielding (ie permanent deformation) will occur for ductal materials when the von-Mises stress exceeds the Yield Strength of the material.

The 182 GPa value is the peak stress, which could very well be artificially high due to stress singularities; reentrant corners (corners with a mathematical 90 deg edge) will produce stress singularities, resulting in infinitely high stress at the edge. However, in the real world, there is no such thing as a perfect 90 deg edge; there is always some type of fillet present. There are also other modeling conditions that can cause singularities, and an analyst can spend a significant amount of time on a FEA model to ensure that any singularities are handled correctly and that converged results are obtained.

I also want to point out that it looks like Window1 is an animation, and that the stress fringe plot you see is for frame 5 of 8; this means the stress field you're seeing is essentially at 5/8ths of your applied load. Frame 8 of 8 will show the results for 100% of the load.

and the third how the stress is mapped,how does this differ from the first one

The third window is showing the maximum principle stress. The maximum principle stress is a vector quantity (ie it has a direction associated with it) and defines a the maximum tensile stress within the geometry. Material fracturing occurs typically when the maximum principle stress exceeds the ultimate tensile stress of brittle materials.

The second is showing how far the bolt would be deformed

Correct, but I have a feeling that something is wrong with your analysis, as the bolt is deflecting over 0.4 m (over a foot). It's possible that this value is right, but that would only be the case if your bolt is really big (around 2.25 m in length, which I doubt).

I'd be happy to review your analysis and provide feedback if you can post the model itself and a describe the situation that you're trying to simulate.

View solution in original post

ryankelley · ‎Aug 20, 2014

Hey Marcus - I've moved this post into our Simulation community so that others can offer their expert advice.

sdensberger · ‎Aug 20, 2014

Am I correct in thinking that the first is showing the areas of stress? Im confused since this appears to be up to 182 GPa.

You are correct. The first windows shows a fringe plot of the von-Mises stress throughout the geometry. Von-Mises stress is a scalar (ie no direction) quantity and yielding (ie permanent deformation) will occur for ductal materials when the von-Mises stress exceeds the Yield Strength of the material.

The 182 GPa value is the peak stress, which could very well be artificially high due to stress singularities; reentrant corners (corners with a mathematical 90 deg edge) will produce stress singularities, resulting in infinitely high stress at the edge. However, in the real world, there is no such thing as a perfect 90 deg edge; there is always some type of fillet present. There are also other modeling conditions that can cause singularities, and an analyst can spend a significant amount of time on a FEA model to ensure that any singularities are handled correctly and that converged results are obtained.

I also want to point out that it looks like Window1 is an animation, and that the stress fringe plot you see is for frame 5 of 8; this means the stress field you're seeing is essentially at 5/8ths of your applied load. Frame 8 of 8 will show the results for 100% of the load.

and the third how the stress is mapped,how does this differ from the first one

The third window is showing the maximum principle stress. The maximum principle stress is a vector quantity (ie it has a direction associated with it) and defines a the maximum tensile stress within the geometry. Material fracturing occurs typically when the maximum principle stress exceeds the ultimate tensile stress of brittle materials.

The second is showing how far the bolt would be deformed

Correct, but I have a feeling that something is wrong with your analysis, as the bolt is deflecting over 0.4 m (over a foot). It's possible that this value is right, but that would only be the case if your bolt is really big (around 2.25 m in length, which I doubt).

I'd be happy to review your analysis and provide feedback if you can post the model itself and a describe the situation that you're trying to simulate.

Thesunshines · ‎Aug 23, 2014

Shaun,

So if my bolt is made from high quality structural steel and I need to use the von mises and I can pretty much ignore the pronciple stress? I would need to load it until it reaches the yeild stress and not the UTS?

346gnu · ‎Aug 21, 2014

Marcus,

Your bolt seems a to be a very low grade, a lot lower than the more usual 8.8. Perhaps about 5.8. Is that correct?

Your stresss numbers look to be out by a factor of 1000. If your results really are reading GPa it is very broken. I think your results should be MPa

and you say your bolt loading is 265MN ,,, Mega Newton ... that's a big bolt.

Something is very wrong. Check your loads.

Example for you to compare

M20, grade 8.8. Tightened to 80% yield will require a preload of about 110,000N or 110kN with a 50kN reserve.

Regards

Charles

Thesunshines · ‎Aug 21, 2014

Hi Charles,

The bolt is big, 245mm with a 80 mm diameter. The UTS is 530 Mpa. Using the simple stress = force/area, then force = stressxarea

force = 530 Mpa x 0.502m^2 for failure

= 265 MN, which the the load that I used in my model. Have I used the wrong figure?

Regards
Marcus

Thesunshines · ‎Aug 21, 2014

Charles,

You may well have saved me from a huge miscalculation.

The area should be 100 times smaller 5.02x10^-3 m^2

and so the load is in fact 2.65x10^6

Such a basic mistake at the very begining!!!!

Thanks for that.

346gnu · ‎Aug 21, 2014

It's always the easy things that catch one out.

80mm dia is sizable. I rarely go beyond M24.

I think the stress area would be closer to 4.3*10^-3m^2 though and would be the value I would use as the fastener diameter in simulate

Impressive stats for the bolt ...

1.8 MN preload @ 80% yield

16800 Nm torque to tighten to this (making various assumptions about friction etc )

Hydraulicly tensioned presumably

atb

346gnu · ‎Aug 21, 2014

... that should have been 1.4 MN preload @ 80% yield