Living hinge simulation

[thebigconsultant]

Here's another one for you!

I have been given a box that has a living hinge, designed in SolidWorks.

Similar to this, but with a more complex shape

Now the box is drawn in the open shape, in the orientation that it would be injection molded.

I need to make a drawing of the box closed. Sounds easy enough right??

Maybe not. I can think of 3 ways.
1. To cut the model in half, and then close manually.
- But this cant be done, as the living hinge is not a straight line as in the picture. It has a unusual design to achieve a positive 'snap' shut.
2. I can used the "Flex/Deform" tool.
- I have always struggled with this tool, and again, I dont expect that the curved 'living hinge' will like the twist or bend tool too much.
3. Using FEA to calculate a 'displacement'.
- I have SolidWorks Premium 2011. So this is a full version of Cosmos inside.
The problem is that when I used Cosmos, I am not too familiar with it, initial problems:-
a. The 'show displacement' always moved the lid about one inch... even when I changed the force applied to the lid... SO it seems that Cosmos initial or default settings only show limited and unrealistic displacement, or a fixed amount for false colour analysis or whatever reason.
b. When I increased the force above a certain threshold... and we are talking about a KG here, it asked me if I wanted to turn on "Large Displacement Mode". BINGO! (so it does limit displacement after all)
c. Large displacement initially failed to calculate. I think because I had already gone beyond the 1KG and the parts had probably contacted and 'mashed' into each other.
d. When I reloaded, the "Large Displacement" was not on, and I do not know how to set it.
e. I could really do with some tips on how to make a realistic closure of the part.

I think that the advantage of the FEA method is that it will cause the flexing that will be created with this unusual living hinge. This will flex the box somewhat, if I can get the displacement through applying a force and restrain correctly to the lid and main box.

Can anybody help or advise?

Kind regards, Bid

 

[Plamen]

Hi!

My personal opinion is that FEA may give where to go: East, West, North, South

I read the post twice i couldn't find any info about the material. I suggest it is an ordinary plastic box.

If so FORGET about designing the hinge with FEA. (i am not saying it does not work)

FEA will calculate only the initial state. After the hinge is in use the plastic behaves in a very, very different way than in the calculations.

There are a bunch of proven designs - ask Google.

Select your best suited design and buy a shampoo. Use your intuition.

CHOOSE the BEST material to use. (working environment and conditions, cycles of opening, sealing, etc)

One MAJOR think you have to consider is to avoid melt lines near the hinge AT ALL COSTS.

I just finished a product which is a ring that should be closed only once. Well - method 1 you gave (and a little experience) gave the result better than the customer has ever expected.

Of course when you already have the FEA - check your design. Never start with it.

 

[thebigconsultant]

Thanks.

I have finalised the design now, and I really want to know how to set the FEA in SW Premium to calculate a "large displacement" i.e. "Shutting the box".

Can i force the lid closed, and rather than using a force, and then view the displacement.

Or am I right to just keep adding force in a direction vector until it is shut properly, and back off, as it reaches the closed state.

Problems with the displacement are what i am struggling with, as SW seems to limit displacement as default, perhaps scaling it on purpose. I am sure it is doing this!!

 

[StuartKelly]

Hi.

Cosmos (as supplied with Solidworks Premium) is based on linear analysis theory which assumes small displacements. If you want to accurately simulate a full 180 hinge action you really need to use an explicit FEA solver like ABAQUS/Explicit or LS-Dyna, which is probably a bit over the top (these are mainly used for crash simulation, modelling rubber parts, etc).

I have never used Solidworks Simulation Premium, I believe it is still an implicit FEA solver but it claims to have some plastics & rubber capability which might work if you just want to predict shapes, not stresses. This is expensive too.

We have recently been designing a product with two different living hinges (see http://www.contactspod.com) and found there's no real alternative to having different (linked) CAD models for "closed" position and "as-moulded" position.

We have used 3D printing (Objet) to test how the as-moulded geometry will deform when closed.

 

[AndrewNew]

You don't necessarily need an explicit FE code to solve this problem - an implicit code will do fine. You do, however, need to be careful about how you set up your analysis and there are some tricky bits such as how to pick up the box closure, as you've already discovered. I'm not particularly familiar with SolidWorks Simulation/Cosmos but here are some tips which apply to FEA in general - you may need to interpret terminology according to your package.

You will need to turn large displacements on. This is because your displacements are, well, large! In FEA the term "large" refers to the size of the displacements relative to the size of the model, and displacements greater than about 1% of the characteristic dimensions of the model start to introduce non-linear geometric effects that are not accounted for in the small-displacement formulation that is used by default. If you recall your basic beam theory you might remember that similar caveats apply, for the same reasons (beam deflections must be small relative to the beam span for simple beam theory to apply).

Note that it is not really a question of "limiting displacements" - the small displacement formulation places no intrinsic limits on the size of the displacements - but I guess there is some "intelligence" built into the system that detects when non-linear geometric effects might become important which then triggers the question of "do you want to turn on large displacements". You can find a more complete description of these effects, and why SS might be showing you the large displacements message here http://www.kxcad.net/ansys/ANSYS/ansysh ... H2_11.html

To help you get somewhere with your current problem, as a first step I'd suggest you make sure you apply your "closing force" as a pressure on the top face of the box lid. This is because pressure loads "follow" the geometry of the box as it deforms (in technical terms, the pressures remain normal to the faces of the finite elements that form the lid), whereas force loads always act in the direction you specify initially. In my experience of CAD-integrated FEA systems, it is not always clear whether you are applying force or pressure loads to faces. For small displacement problems, the two will give pretty much identical results, but for large displacement problems the different behaviour can be very important.

I doubt that you will see significant inelastic deformation (I'm talking about plasticity and other non-linear materials effects here, separate from the large-displacement discussion above - my rather cursory understanding is that living hinges are designed to operate in the elastic regime, such as it is for polymers) so stick with an elastic material model for starters.

Also, when you are exploring and just trying to get the simulation method to work, use the coarsest mesh you can get away with, and use linear or "draft quality" elements (there's that "l" word again - it means something different in this context - don't worry about it!). If available, you could try using shell elements rather than solids, as your (thin wall) geometry is better suited to shells. This will keep your solution times to a minimum - you can worry about mesh convergence and results accuracy later.

One other thing, when you are checking your results, make sure that you have any "results scaling" set to 1. I can't remember how you do this in SS, but many packages have a habit of applying scale factors to displacements for display purposes to make them more "visible", which can be useful for visualisation but can also make you forget to check the numbers in your scale bar properly!

Finally, this kind of thing is what I do for a living, so if you get really stuck you could always give me a call!

 

[StuartKelly]

I agree with all Andrew's comments, just a few clarifications to add:

The "Large Displacement" flag in the standard linear version supplied within Solidworks Premium does not actually turn on full geometric non-linearity - to get this you need to upgrade to the non-linear version (part of Solidworks Simulation Premium).

In the linear version the "Large Displacement" flag applies the load gradually to improve the chances of reaching a solution when contact is present. I don't believe it will change the direction of the load as the part moves, but worth a try.

The Help files supplied within basic Solidworks Simulation cover the capability of the full Solidworks Simulation Premium, so reading the help files might suggest you have more options available than you actually do. The matrix of capabilities is shown here: http://www.solidworks.com/sw/products/1 ... U_HTML.htm

Some of the curved "bistable" type living hinges seen on shampoo bottles (e.g. Pantene Pro-V) depend on buckling of the plastic and probably some localised yielding.

 

[AndrewNew]

Stuart, your point about the bistable hinges is well taken. Local buckling could be one reason for the analysis failing in the manner described - when you get two (or more) possible equal-energy configurations in the model (like you do at the onset of buckling) you are likely to come across numerical problems. I'd be sceptical of the capacity of a CAD-integrated FE package to give you enough control of the numerics to overcome them to be honest - you might well need something more specialist (Ansys, Abaqus, Nastran and the like). Interested to see how the poster gets on!

 

[thebigconsultant]

Stuart, your point about the bistable hinges is well taken. Local buckling could be one reason for the analysis failing in the manner described - when you get two (or more) possible equal-energy configurations in the model (like you do at the onset of buckling) you are likely to come across numerical problems. I'd be sceptical of the capacity of a CAD-integrated FE package to give you enough control of the numerics to overcome them to be honest - you might well need something more specialist (Ansys, Abaqus, Nastran and the like). Interested to see how the poster gets on!

Well, you have certainly whet my appitite to find out!!

Its like excitement that you can, then for my hopes to be dashed, then built up again reading this. You were initially hopeful that the solver built into SolidWorks Premium could do this (I think) and now I see backtracking?!?

Lets stick to our principles and arguments and give this a bash!

Hi.

Cosmos (as supplied with Solidworks Premium) is based on linear analysis theory which assumes small displacements. If you want to accurately simulate a full 180 hinge action you really need to use an explicit FEA solver like ABAQUS/Explicit or LS-Dyna, which is probably a bit over the top (these are mainly used for crash simulation, modelling rubber parts, etc).

I have never used Solidworks Simulation Premium, I believe it is still an implicit FEA solver but it claims to have some plastics & rubber capability which might work if you just want to predict shapes, not stresses. This is expensive too.

We have recently been designing a product with two different living hinges (see http://www.contactspod.com) and found there's no real alternative to having different (linked) CAD models for "closed" position and "as-moulded" position.

We have used 3D printing (Objet) to test how the as-moulded geometry will deform when closed.

Stuart, you are right. And thank you for the keen observations. By the way your ContactsPod looks excellent. I had a feeling that the only method available to me was to create two models. And the "flex deform" tool might approximate this, but not accurately. Unfortunately as the device I have does not have a straight living hinge, it is impossible for me to simply split the model and close it. My model should and will deform as it is closed. Elastically I hope!! But you are right, the FEA solver in the Premium product no doubt is not going to perform a plastic deformation, but I still think, as you say here, that deformation is not ruled out.. Even if it is a workaround, and maybe requires some tinkering?

Thank you for the notes on 'implicit ' and 'explicit'. This is something that i should learn more about! Interesting!

You don't necessarily need an explicit FE code to solve this problem - an implicit code will do fine. You do, however, need to be careful about how you set up your analysis and there are some tricky bits such as how to pick up the box closure, as you've already discovered. I'm not particularly familiar with SolidWorks Simulation/Cosmos but here are some tips which apply to FEA in general - you may need to interpret terminology according to your package.

Thanks Andrew. I realise that SolidWorks is a 'baby' package (well technically 'mid-range' CAD), compared to some of the big FEA. But the principles no doubt will be the same, but within limits of this solver I would imagine. What it does, it seems to do well, and the interface is very intuitive, so I think I should be able to follow advice and I'll tell you if the option is not there!

You will need to turn large displacements on.

This is what I guessed!!

This is because your displacements are, well, large! In FEA the term "large" refers to the size of the displacements relative to the size of the model, and displacements greater than about 1% of the characteristic dimensions of the model start to introduce non-linear geometric effects that are not accounted for in the small-displacement formulation that is used by default.

Yes, I did take a quick look and it was apparent that every force I put on there resulted in the same displacement. I cannot confirm yet if this is a limitation in this FEA modeller, or indeed just a setting or two. I suspect that it 'scales' to give useful and readable false colour chart results etc. But also, i mentioned that when I really cranked up the forces in the spirit of scientific discovery (also known as frustration), the software prompted me to 'turn on large displacement mode'. So credit to SolidWorks for making things easy, they do seem to add the dialog boxes that are most helpful and guiding etc.

You can find a more complete description of these effects, and why SS might be showing you the large displacements message here http://www.kxcad.net/ansys/ANSYS/ansysh ... H2_11.html

But much for me right now. But clearly, it looks at the parameters, and makes recommendations based on the type of simulation required. The solver still ran very quickly when large displacement was on, and I think also did several studies i.e. 25%, 50%, 75% etc etc, and probably plots a median movement I am guessing to ensure that it displaces in a predicable manner?

To help you get somewhere with your current problem, as a first step I'd suggest you make sure you apply your "closing force" as a pressure on the top face of the box lid. This is because pressure loads "follow" the geometry of the box as it deforms (in technical terms, the pressures remain normal to the faces of the finite elements that form the lid), whereas force loads always act in the direction you specify initially. In my experience of CAD-integrated FEA systems, it is not always clear whether you are applying force or pressure loads to faces. For small displacement problems, the two will give pretty much identical results, but for large displacement problems the different behaviour can be very important.

Thank you. This is an excellent tip, and I did not know this! I had used a 'force' set on a 'direction vector', and I was aware that at the lid rotated, the closing force would change. I was not aware that the 'pressure' setting worked in this way, and SolidWorks certainly contains that option! So I will try this when I get the chance!

Also, I can imagine that this would indeed be very useful for 'large displacement', and in this case may solve a multitude of evils.

I doubt that you will see significant inelastic deformation (I'm talking about plasticity and other non-linear materials effects here, separate from the large-displacement discussion above - my rather cursory understanding is that living hinges are designed to operate in the elastic regime, such as it is for polymers) so stick with an elastic material model for starters.

Well, I have very little experience. But I think that I am naturally limited to elastic deformation anyway, so this is a bonus. As the product "should" return to its original shape, then it stands to reason that elastic deformation is taking place. Amirite?

Also, when you are exploring and just trying to get the simulation method to work, use the coarsest mesh you can get away with, and use linear or "draft quality" elements (there's that "l" word again - it means something different in this context - don't worry about it!). If available, you could try using shell elements rather than solids, as your (thin wall) geometry is better suited to shells. This will keep your solution times to a minimum - you can worry about mesh convergence and results accuracy later.

I might try the thin wall geometry if I can. It certainly might help!

One other thing, when you are checking your results, make sure that you have any "results scaling" set to 1. I can't remember how you do this in SS, but many packages have a habit of applying scale factors to displacements for display purposes to make them more "visible", which can be useful for visualisation but can also make you forget to check the numbers in your scale bar properly!

Yup. I discovered this. The scaling was set to automatic, when I 1st ran the simulation. Seems to be default setting. I was in a rush, but I noticed with a bit of clicking, the scaling factor. But I must have pressed the wrong option, as it began to scale the lid only when I ramped it up (1:1 ratio being unsatisfactory) and the lid began to develop a bit of 'elephantitis', growing in size to a ridiculous shape etc.

I should probably try again, with the pressure set to the correct amount to displace (hopefully), and with some experimentation. And also set the scaling ratio from Automatic to 1:1

Finally, this kind of thing is what I do for a living, so if you get really stuck you could always give me a call!

Great. Thanks for this offer. This is interesting, but you cant beat experience.

I agree with all Andrew's comments, just a few clarifications to add:
The "Large Displacement" flag in the standard linear version supplied within Solidworks Premium does not actually turn on full geometric non-linearity - to get this you need to upgrade to the non-linear version (part of Solidworks
Simulation Premium). .

Can someone lend me £10,000 ?

In the linear version the "Large Displacement" flag applies the load gradually to improve the chances of reaching a solution when contact is present. I don't believe it will change the direction of the load as the part moves, but worth a try.

Thanks. I think that using pressure might help? Also, I noted that the solver does the FEA in increments on the Large Displacement setting also. So I have some hope still that it might solve? Only one way to find out!

- Well sadly, there are probably hundreds of ways to find out.. Such is the complexity of FEA. So I should rephrase. I have the skills only to try one way to find out. And find out I surely will, and if its a failure. I will return to share my misfortune.

Some of the curved "bistable" type living hinges seen on shampoo bottles (e.g. Pantene Pro-V) depend on buckling of the plastic and probably some localised yielding.

Yup. I had a very brief talk with a contact of mine at SolidWorks, and he said, quote "This is tricky stuff. The living hinge causes stability problems. Its the same as with shampoo bottles. {redacted} use simulia to do this".

But I would be happy with a perfect elastic deformation, and who knows. Would be a neat and simple trick if it works, and certainly repeatable and useful for other products. I'll tell you how I get on! Thanks again!

 

[maniacal_engineer]

do you need to model the hinge itself? can you just assume the hinge will behave as ... a hinge, and focus on the deformation of the rest of the box that gives you the snap action? If you break the hinge into several parallel pieces you could still get the snap and it would be a lot easier to analyse. Just some random thoughts, sorry if they are not really relevant

 

[thebigconsultant]

do you need to model the hinge itself? can you just assume the hinge will behave as ... a hinge, and focus on the deformation of the rest of the box that gives you the snap action? If you break the hinge into several parallel pieces you could still get the snap and it would be a lot easier to analyse. Just some random thoughts, sorry if they are not really relevant

Good idea.

Maybe 'splitting' the part, and then just FEA'ing a small part, for example the hinge, and then joining to other parts as an assembly. Of just running FEA on one part of the body is a solution.