Material file database (again)

[Bossbutteringbe]

Hello all - I'm new to this group but a seasoned Pro/E designer and experienced Mechanica user based on Ireland.

I have a job on which requires me to finally get to grips with the new elastic-plastic analysis functionality of Simulate 2 and apply it to a forming operation on a small 300 series stainless steel tube. Would anybody on here be prepared to share a material definition file for one of these steels, set up with stress/strain data for LDA? I'm not trying to freeload and would be happy to work collaboratively and reciprocally with one or more knowledgeable users who may also also be working to develop confidence in this powerful new functionality.

Many thanks

Tony

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.

[DenisJaunin]

Hi, Tony,

Here is a link on quaractéristiques of stainless steel.

I do not know if this is exactly what you want.

Cordially.

Denis

http://www.pxprecimet.ch/data/documents/fiches-techniques/FR/liste-complete-alliage.pdf

[ehaenen · Accepted solution]

Hi Anthony

Just as long as you understand that this is a typical engineering approach to AISI 304, that works well in Creo2.

There is a lot to be said on how to correctly make a material definition, but this one works nice with Creo (Creo likes smooth curves) and fits the 304 data for yield and ultimate (with true strain of course!)

Try it, let me know what you experience.

https://drive.google.com/file/d/0BxuTvot6TxcLelVEZTdVdkk1UkE/edit?usp=sharing

Erik

[Bossbutteringbe]

Thank you Erik.

To my chagrin I'm still having the traditional wrestle with PTC's installation to get Advanced Simulation running. I've added your sample file for 304SS to my materials d/b and will have a play once the elastic-plastic functionality is installed correctly. Rightly or wrongly I have the impression that this new functionality and other recent changes represent an upswing in investment in good old Rasna which helps keep the product relevant in my eyes. Elasto-plastic module seems a bit gawkish and I'm sure the user experience will gain more polish in the next few releases.

Hopefully this analysis job will work out and build the store of knowledge about how to get useful output in a sensible amount of analysis time. Will report in due course!

T

[Bossbutteringbe]

Eric here is an update about how I got on - and another question! (should I post this on a separate thread?).

I resolved my installation issues and familiarised myself with the advances in Simulate since Mechanica WF4.

I modelled my problem (the flaring of the end of a thin-walled SS304 tube) using bricks as far as possible, using an enforced displacement constraint, making the tubing workpiece short enough to avoid buckling modes, defining contacts with the mandrel by hand etc etc. and using 80 time-steps and single-pass adaptive converegence I got this:

Video Link : 4537

Not too bad I thought given the non-ideal nature of the way the mesh was generated using the available mapping tools. I should be able to define a composite measure for tracking engineering stress and strain as per Roland Jakel's "Basics of Elasto-Plasticity".

What is stumping me however is how to get the Include "Unloading function" to operate with my geometry, or to find a workaround. As Unloading seems to work with a single load reversal step, and as my part will be 'clinging' to the mandrel, Solver gives me: "Excessive motion detected at contact regions. Cutting load step size" during the final unload step, hunts for a workably-small load step and fails to converge. As a result I can't directly see the final plastic-only deformation of the flaring process.

Erik, if you or others have any thoughts how to workaround this (apart from manually subtracting elastic strain from measured engineering strain) I'd much appreciate it!

Tony

[346gnu]

Tony,

For simpler problems such as increasing the pressure inside a cylindrical vessel until the material yields, clicking the 'unloading in 1 step' button has given quite different and (my opinion) less trustworthy answers when compared to manually entering a number of time steps for unloading. The examples I have use a measured material stress-strain curve as an input.

In the case where parts form over/onto etc other, I would avoid the unload-in-one-step button and enter small time steps to withdraw your component using the enforced displacement constraint.

Also, would make for a more impressive animation showing the spring back as is withdrawn.

... I wonder how this will work with friction in Creo3.0?

Regards

[Bossbutteringbe]

Charles I'm working out how the Output Steps area on the Output tab of the Static Analysis dialog box interacts with the Time Dependence table function in Load Histories, which seems to be the only way to workaround the issues with Include Unloading where a displacement constraint is used. I'm doing this via short runs in a real problem and trying to take notes of how it all works. I hope to get there in the end, and can then explore parametric variations of the tube forming process parameters.

I agree with you about the upcoming friction model in Simulate 3.0 - this would be really useful for us right now!

[ehaenen]

Anthony

Absolutely beautiful, great work.

I've done something smilar, but not as spectacular.

Unloading has never worked for me (the automatic way). Same message as you got.

I use an excel sheet that generates cam profiles. I always set the amplitude to one (1) and use the result as a scale factor for my load or prescribed displacement. That way I also scale it back to zero again.

My third picture shows a graph of 2 such curves (The blue one preloads the rubber block in my example, the red one drives the punch)..

It works!

Erik

And yes , maybe we start a new subject on non-linear analysis in general. I made several really cool examples... I'm a great fan, hope they keep developing the capability.

[Bossbutteringbe]

That's really encouraging Erik, lovely work and you stoke my confidence that I'll get on top of the realities of an evolving product in a sensible amount of time. It is slightly unfortunate that PTC are almost silent on use of these new developments (quality case studies, tips etc). It would appear that this community fills that role, at least for the time being!

[rkannan]

dear anthony,

i have seen your video. thats very helpful to me. i am also doing nonlinear analysis in creo.. but my design studys are failed due to some mesh problem. if you dont mine plz give me your nonlinear creo model like that video,or give me some tips how to rectifie it. thank you.

[Bossbutteringbe]

Hi Raj.

We did some work last year using the Simulate 2.0 elastoplastic capability and evolved our own workflow. Your mesh problems will need to be resolved before you can proceed to any kind of analysis. It makes no difference whether this is an elastic or nonlinear analysis. For models that use a lot of idealisations this can be time consuming as you will know.

Based on our limited experience of Creo's nonlinear analysis capability I think you will need material models that approximate the materials you plan to use in the 'real' hardware. This stumped us originally as PTC dont offer any and there are issues around building material models that make for a stable non-linear analysis. We found that the best place to start is with authoritative stress-strain curves (must be true strain) for representative test pieces of the material you want and finesse the data to get a good curve-fit in the material modeller in Simulate 2.0.

The analysis should first be run as a linear analysis to check convergence and freedom from modelling errors. If that works it is safe to substitute nonlinear material models where desired and re-run the analysis using conservative load and approximate convergence settings. If that works, more refined versions of the analysis can then be run until you have obtained the insights you need. If it wont work, the material models probably need more attention. As always, build up more complex analysis models in modular fashion, dont expect to do everything at once.

We also recommend using User-Defined Output Steps for complex non-linear analyses as it can greatly help analysis convergence and (in combination with forced displacement constraints) also gives good control of unloading so plastic strain can more easily be seen.

Good luck Raj and seasons greetings!