Turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

** Community Tip** - Have a PTC product question you need answered fast? Chances are someone has asked it before. Learn about the community search.
X

- Community
- Creo (Previous to May 2018)
- Creo Modeling Questions
- Elastoplastic Curve Generation

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Mute
- Printer Friendly Page

Jul 02, 2013
08:11 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 02, 2013
08:11 PM

Elastoplastic Curve Generation

Can anyone tell me the right way to enter the elastoplasic properties of a material in Creo/WF 5.0? I have the true stress/strain curve entered. With the "Use best fit coefficients checkmarked the curves look good. However the Tensile Yield stress is at 0. If I try to hit ok it doesn't let me. It says I must have a value greater than 0. If I uncheck the box and put in the correct value the curve shifts way up. Any thoughts?

Solved! Go to Solution.

ACCEPTED SOLUTION

Accepted Solutions

Jul 03, 2013
02:24 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 03, 2013
02:24 AM

I never used this capability of Pro/E, but I see that the graph is a plot of **plastic** strain vs stress.

Thus it seems obvious that the curve starts **after** the yield stress point...

12 REPLIES 12

Jul 03, 2013
02:24 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 03, 2013
02:24 AM

I never used this capability of Pro/E, but I see that the graph is a plot of **plastic** strain vs stress.

Thus it seems obvious that the curve starts **after** the yield stress point...

Jul 03, 2013
04:31 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 03, 2013
04:31 AM

Hi,

Yes, only the part of the curve after yield should be used and should be true stress vs true strain.

This is to likely to change with Creo3.0

http://communities.ptc.com/message/195487#195487

Regards

Jul 03, 2013
08:58 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 03, 2013
08:58 AM

Ok thanks. It is true stress and strue strain. Should I also use the equation you mentioned to convert true strain to plastic strain?

Jul 05, 2013
09:30 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 05, 2013
09:30 AM

Paul,

The equation simply subtracts the linear part of the curve leaving only the plastic strain.

Regards

Jul 05, 2013
10:43 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 05, 2013
10:43 AM

Thanks Charles. I have gotten all the correct numbers in, manipulating the engineering stress/ strain curve to get true stress/true strain. Here is what I did:

I calculated the Ramberg Osgood Coefficient: n = (LN(eus/.2))/((LN(Ftu/Fty))

eus uniform strain

Ftu ultimate strength

Fty yield strength

Uniform strain can be calculated by: eus = 100(er-(Ftu/E))

er strain at rupture

E youngs modulus

I obtained an engineering stress strain curve using:

eeng = sigmaeng/E+.002*(sigmaeng/Fty)^n

I calculate true stress and strain

sigmatrue = sigmaeng*(1+eeng)

etrue = LN(1+eeng)

Then calculated true plastic strain

etrueplastic = etrue-(sigmatrue/E)

Does this seem correct? By the way all of this info can be found in MMPDS-01

Jul 17, 2013
12:11 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 17, 2013
12:11 PM

Paul,

I too have used the Ramberg Osgood relation, it seems to be generally accepted.

Could TAD D confirm or correct the following please?

the material curve input is interpretted one of 2 ways depending on whether the LDA check box is ticked.

(SDA = small deflection analysis

LDA = Large deflection analysis)

INPUT material curves:

The material curve input for SDA is interpretted as ENGINEERING STRESS vs ENGINEERING STRAIN

The material curve input for LDA is interpretted as TRUE STRESS vs LOGARITHMIC STRAIN

The axis labels on the input data graph do not vary and in CREO2 they are True plastic strain, True Stress (MPa).

OUTPUT Analysis results for the above are:

SDA results are in ENGINEERING STRESS and STRAIN

LDA results are in TRUE STRESS and LOGARITHMIC STRAIN

With SDA there is a generic assumption that the ENG and LOG strains (and other strain models) are about the same if the strain is less than 5%; therefore checking the LDA box 'doesn't matter'.

Thanks

Jul 23, 2013
12:58 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 23, 2013
12:58 PM

Hi Charles,

Yes, your statements in your July 17th post are correct. Concerning your last paragraph, it might be more accurate to say that as long as the strains, displacements and rotations are small, then an SDA and LDA analysis should give nearly the same results.

Tad Doxsee

PTC

Jul 23, 2013
05:14 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 23, 2013
05:14 PM

Fair point, my inverted comma's were too subtle.

Thanks

Jul 03, 2013
09:47 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 03, 2013
09:47 AM

Hello,

It would be interesting to find a tutorial on how to use this function in the material, with an explanation of functions and a concrete example.

Cordially.

Denis

Jul 05, 2013
07:15 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 05, 2013
07:15 AM

Hello,

See attached with some explanations on the subject link.

Cordially.

Denis.

http://www.qucosa.de/fileadmin/data/qucosa/documents/8714/SAXSIM_2012_Plasticity_Jakel.pdf

Jul 05, 2013
07:53 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 05, 2013
07:53 AM

Thanks Denis, I'd forgotten about the info available from here.

PTC, This information should be available via the knowledge base.

Why do users have to discover this? Why can't technical support point to these?

More advanced users need a different kind of support than that generically offered.

Thanks

Jul 05, 2013
09:04 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jul 05, 2013
09:04 AM

I agree with Charles !