cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Community Tip - Help us improve the PTC Community by taking this short Community Survey! X

Plasticity and fasteners

346gnu
12-Amethyst

Plasticity and fasteners

NOT SUPPORTED !

Was this the case before the fasteners became beams, I haven't time to test?

Ansys it is then

13 REPLIES 13

Correct, you can't use beams in models with plasticity. You will need to model the bolts using solids, which may be prohibitive. Or use Ansys...

I have requested having the possibility to include beams (+links) in large deformation models/plasticity models, but had no sucess yet. I would think it is relatively easy to implement this. As long as the beams themselves stay in the linear region and do not bend like fishing rods, they should be able to undergo "rigid"-body rotation and be included in large deformation/plasticity models. In statically indeterminate load cases with contact, deformations may be "small" but you still need large deformation analysis for correct results. Being able to include beams in such models would be great. It is often you have designs that rely on friction and contact, where pre-loaded bolts are  present, and where you need to include large deformations to get correct results, even if deformations appear small.  I hope PTC's staff reads this...

346gnu
12-Amethyst
(To:mlindqvist)

We don't often carry out plastic analysis. 99% of problems are linear enough. Use is mostly when a component cannot be redesigned to reduce stresses and therefore we need to know if it will actually rupture.

 

These components tend to be buried in an assembly and the loads to which they are subjected are complex and any attempt to carry out a single component analysis will give results that are simply wrong.

 

... This is where we could use sub-modelling to great effect and would be immediately much much more useful than being able to use 128gb RAM,  buying light speed SHDD's and CPU's that require their own substation ...

 

The plastic material properties are limited to specific volume regions of a component. The rest of the model has linear material properties. Making the complete component plastic would be onerous.

 

I found that it isn't possible to work around using solids and preloads either. Preloads not supported for models with plasticity.

 

One discovers this after applying a preload to a model with plastic materials applied (or vice-versa). The moment of discovery is when the attempt is made to set up a static analysis.

 

A warning should be presented during the model build and not lie in wait to ambush the work.

 

I did check the help files. The help files ...

 

The overview should have a list of limitations as a MAJOR heading in the overview and therefore UN-miss-able.

 

Nothing in the help is immediately obvious or maybe I use it the wrong way.

 

Then the work around using solids with contact/interference. Just keeps failing insufficiently constrained. (tangential dofs were constrained). Using contact/interference eliminates anything to do with temperatures.

 

I had already filed a brief support call re volumetric preloads not recognising a prismatic volume if extruded up to surface rather than as a blind protrusion but this insufficiently constrained frustration will take many hours to build and reproduce in a model I am allowed to submit and will have to wait for some down time.

 

So I have tested a simple component with a volume region and a temperature load in the volume region (to shrink and gets rid of contact interferences) I am still able to define an analysis with plasticity and ran it.

 

The question is whether I am confident to invest more time here or to actually move the study to ansys as suggested earlier where I have certainty of outcome. (the reasons for remaining in Creo are at the request of the client; I will bend this soft rule if I have to in order to get the answers out of the door)

Good points Charles...

Just to demonstrate, I make a quick test with a model that requires large deformation analysis, in a pre-loaded structure, but where deformations may seem small.
A bolt maintains a pre-load on a wedge that holds a component. An external load is applied to the part held by the bolt/wedge arrangement. I want to include the effect of shear/bending of the bolt; this is why it is necessary to use large deformation analysis - the problem is statically indeterminate.

The load is applied in two steps, first a pre-load to tighten the bolt, then the external load is applied. This is accomplished by using different time functions in the analysis form.

In a contact analysis like this, even though deformations are seemingly small, they are significant in comparison to the stiffness of the structure. This is a typical example where I would like to be able to include beam elements in a large deformation analysis, to model the bolt. In this simple example, it worked fine with a single solid bolt, but if there are many of them, and/or the model is otherwise complex, some component has material nonlinearity etc, I don't want to model bolts like this. I want to be able to include beam elements.

This model contains 3970 elements, took about 15 mins on my laptop (64 bit, 16 GB RAM, 2x2.7 GHz) It was made in Creo 3.0.

/M

(Statically indeterminate at Wikipedia: Statically indeterminate - Wikipedia, the free encyclopedia)

community1.PNG

community0.PNG

346gnu
12-Amethyst
(To:mlindqvist)

Mats,

I agree.

But also you cannot use a preload on your solid fastener and have elasto-plastic properties in one of your parts (internal rounds on the outer component seem potential locations for plastic material behaviour).

Give elasto-plastic material properties to one of your components and try and define an analysis ...

It seems to be working! Convergence is slower, I have a sharp edge-surface contact that might make the plastic convergence problematic, but as I write this it seems to be moving forward. (need to punch out, so I can't wait for it to finish) Check out my model. I use Creo 3.0 M030...

With rounds added, to avoid edge-surface contact, the model ran to completion. I'm out of office right now and we're having issues with our VPN so I can't access the license to review results 😞

346gnu
12-Amethyst
(To:mlindqvist)

Mats, (& forum)

I looked at your model and you have done as I have done which was to resort to the ancient art of preloading by 'shrinking' using a temperature load.

This avoids preloads which are disallowed when considering large deformation and therefore elasto-plastic materials.

I have the additional complexity of an initial interference.

I have attached a model to illustrate this.

This model will run if large deformations are not used. Analysis1.

The model will fail if large deformations are switched on. Analysis2.

The full interference is entirely resolved in the time=0 step causing the large deformation solver to fail. I cannot gradually introduce the interference.

Possible errors/causes reported in the logs:

  • To close to or beyond a buckling mode
  • Loads may be too high and thus mesh should be refined, reduce the load a inspect the deformed shape
  • Static instability
  • Exceeded the material limits

The model is constrained ok. It's unlikely to be unstable or buckle.

Material limits are not applicable as linear properties are assumed at this stage.

So load/mesh combination is not good and I am guessing that this will be at the 'L' shaped contact. I would also further guess that I would need rounds on the 'L' to begin to make this work. The fastener also has corners at it's change of section between head and shank  As mentioned above I cannot step the load when there is an interference so I am left with mesh as the only thing to play with.

As a result I cannot begin introduce non-linear materials. (there is a volume region with suppressed non-linear material property applied). Analysis3.

I chose the location for the volume region where there is no possibility of the material becoming plastic or material limits being exceeded.

None of the above considers friction (although I have infinite friction applied under one end of the fastener so I do not have to make springs) and I am not worried about mesh quality or whether the numbers for the fastener are sensible at this stage.

bfn

Charles

346gnu
12-Amethyst
(To:346gnu)

I have a work around for the interference.

The parts need to be offset so that there is no interference at all.

I now need to understand how to adapt the preload calc as this means the fastener is initially tightening on a gap

This means I can use plasticity with a preloaded structure that has initial interferences.

It a right faff though and I can imagine arrangements of components where this method won't work

So much better if preloads/initial interferences can be made to work with large deformations and/or being able to sub model.

rjakel
4-Participant
(To:346gnu)

 

Hi Charles & all,

 

unfortunately, like you recognized, there are still many limitations in combining different nonlinear functionality in Simulate. You may find some useful information for your problem in my recently created blog “Rolos Simulate Sources”. Simply download the following presentations from there:

 

Basics of Elasto-Plasticity in Creo Simulate – Theory and Application (my last Simulate presentation I wrote as PTC employee)

 

Analysis of Bolted Connections in Creo Simulate - Theory, Software Functionality and Application Examples (my first Simulate presentation I wrote as Altran employee)

 

In this presentation about bolted connections, you’ll find an example about a centrically loaded fastener that undergoes significant plastic deformation (slides 41-51). I had to spend significant time to get that finally successful running, also because for the limitations described further above (no preloads, no non-isotropic materials in combination with elasto-plasticity, …). This was a real-world project, so no simple demo example. Unfortunately, all of these limitations still exist, and elasto-plasticity needs to be improved (I still have at least one open SPR for it).

 

The workaround in that project was to apply the fastener preload with help of a thermal load. The other option - using initial interference -  you also find described in my latest presentation about the finite friction contact model, see The New Contact with Finite Friction Feature in Creo Simulate 3.0 - Theory and Application (or the thread of your discussion “Finite friction blocks”), slides 81-83.

 

All these limitations make Simulate pretty uncomfortable and sometimes impossible to use, as soon as a problem becomes a bit more complex. There is a lot of work to do for PTC R&D to improve this situation. This means implementation of significant enhancements and robustness increases for a lot of nonlinear engine functionalities. From my experience with the code won the last two years, R&D already has to struggle hard just to fix many existing bugs (I opened around 100 Simulate SPR after I left PTC, half of it is still open), and you can see that there is not even one engine enhancement or even robustness increase planned in Creo 4.0. That’s why I wrote this long feedback chapter for PTC in the finite friction presentation. This all needs highest management attention from PTC side and significant invest is necessary to compensate the huge loss of brainpower with laying off the San Jose engine group in 2013.

 

Best,
Roland

 

346gnu
12-Amethyst
(To:rjakel)

Hello Roland,

What I could never understand is why, when at PTC, your (and others') work:

  • Was often branded 'PTC Internal Only'
  • Is still not available via the knowledge base

We all just end up reverse engineering or using other s/w.

Hey ho.

Charles

rjakel
4-Participant
(To:346gnu)

 

Hi Charles,

 

To be honest – I don’t know why this work has been branded as PTC internal only, I even did not recognize this when I worked for PTC, and I do not know who was responsible for this classification at PTC.

 

The presentations I wrote for PTC Global Services were always intended as public information for PTC users. They were supported by the old Simulate engine group in SJ: I got R&D info very helpful for understanding how to better apply the code. In this case, you usually find an acknowledgement at the end of the presentation (typically, Rich King, Tad Doxsee and Christos Katsis gave this support). We have always posted all these presentations in the archive of www.saxsim.de, where you still find them today. Even though I was working for Global Services in Germany, I sometimes started to write these presentations in English so that all users could benefit from them, not only the German ones. The old engine group itself used these presentations for their purposes, too: E.g. you find my presentation about Hyperelasticity from 2010 posted by Christos Katsis here in the PTCusercommunity.

 

When I prepared my latest presentation about finite friction during the last weeks, I started to search the internet for experiences other customers have with Creo Simulate, since I became pretty displeased the last two years about the quality state of the code after the engine group was laid off. There, I found the PTCusercommunity again which came a bit out of my mind. I recognized that users complained that these GSO presentations are not available. So I decided to create my own blog now (Rolos Simulate Sources) to make this info easier available to all at one certain place.

 

I hope this will limit now the effort necessary for doing reverse engineering…  😉

 

Best,

 

Roland

 

 

Hi Roland,

You're 'Rolos Simulate Sources' page is not avialable anymore.

Can you please make it available again?

I'm specifically interested in the plasticity presentation at the moment.

 

...and a big thanks for assistance with our customer issues these last few months!

 

regards,

Agnes Uijttewaal

Announcements
Top Tags