Compressible o-ring with CONTACT surfaces.

DaveStupple

Hello all, me again. I have done well, I think, to get this far without pestering you guys, but here goes...

I am trying to model the compression of a rubber o-ring in a slightly undersized groove. The attached models are revolved through 1deg, so are slightly wedged (p0ssibly an unnecessary compication, but ultimately I will do a bigger revolve for better visual impact). I think this allows me to get away with frictionless restraints.

I want to apply a force of around 30N, which I think will approximate atmospheric pressure. Up to 2N, applied slowly, the CONTACT conditions hold, but at a fraction over 2N the o-ring crashes though its base CONTACT (force.liml). If I blindly beef up K to 5000, The CONTACT holds but many elements fail (force2.liml). If I try K 2500, elements fail even before the o-ring hits the base CONTACT.

If I take away the force and just use a displacement over time of the nodes at the base of the window, the o-ring compresses fine. It seems to me that with the force applied, the o-ring suddenly squeezes into the groove, past the radii, then hurtles friction-free downwards, causing failure of the model. I tried some different friction values to make it a bit more controlled, but it was taking an age to converge, so I figured things were not right and abandoned - I can't spend that much time in the trial-and-error stage.

I will now try to engage the o-ring with the walls and base of the groove by using a timed displacement, which I know I can do. Once partially compressed,  I will try to introduce a timed force. I am not sure how I will time it, whether to introduce the force on the next time step after the last displacement, or whether to overlap them. Or would I be better off increasing the mesh resolution of the o-ring at this stage? Or are there some better settings that will allow the force only approach to work?

With rubber being incompressible (Poisson ratio close to 0.5), I am not sure how well this model copes (not well, I think) when there is nowhere to expand into under compression - presumably the modulus should increase at this stage, which this model does not have. I suspect this is why we have elements deforming. I made the elements of the o-ring longer in the vertical (y), which improved things, but I am at the stage now where input from you guys and girls could save me a lot of time and experimentation. 

Thanks for reading, please ask if any more info needed.

DaveStupple

Can't see how to edit the above, but it occurs to me now that my point about the model coping with non-compressibility and limited room to expand might be not right. The model copes OK and continues to compress/expand when only dislacement is used to compress the 0-ring, so it is likely to be the rate of change that is causing difficulties.

Sergio

Try with more increments and a displacement in place of load. And for Viton and other rubbers is better to use hyperelastic materials, now available on Mecway.

You can see some rubber examples made it with Mecway and CCX at

http://www.4pingenieria.com/en-us/goma/

Regards

Victor

I agree with your assessment that the force isn't resisted so the o-ring flies away. Friction might be difficult because it has to be high enough that it resists the applied force at every time step, especially during the transition from deformation to friction and as it's sliding down the groove where the force of friction might not be increasing much, even though the applied force is, so it might still fly away.

Using displacement instead of force should solve that problem. To turn off the displacement when changing to force, you may need a new *STEP section, which you'd have to enter by hand in CCX -> Custom step contents.

Instead of applying a force, can you just look at the reaction force and use that to find the point where the force is what you want? If summing them is too tricky, connect one of the constraints to a single node using *DISTRIBUTING COUPLING, *RIGID BODY, or bonded contact.

Use a hyperelastic material instead of linear because of the large strains. The linear material seems to be why some elements are collapsing - there's a phenomenon in FEA where linear material elements can be unstable in compression and they snap inside-out if you compress them too far. That only happens when you push them way beyond the strain where the linear model applies so it's not really a problem, but a sign that you're using the wrong material model.

It's also usually a good idea to turn on Analysis settings -> Automatic time stepping for both speed and convergence. With fixed time steps, it might jump past an important transition region so it's unable to solve the next state.

Frictionless support is fine on a tapered sector of an axisymetric model regardless of the size of the angle.

Attached is a model that solves and looks reasonable.

Sergio

Victor, on your formula for appling the displacement you took a displacement of 4.5mm, that is the actual separation betwen the rigid parts. but why at the end they don't finished completly closed?

I have made it with a table directly, ramping from 0 to 4.5 mm and get the final assembly fully closed

Victor

It's because the time steps only go up to 0.45 s but my formula has 4.5 mm displacement at 0.5 s.

Sergio

Thanks! Will you made something to plot .dat files in the future? Is very usefull for this kind of analysis.

Regards

Victor

Probably not. You can copy and paste from Mecway's table into Excel. How did you make your graph?

Sergio

As you say, Excel. But is a little bit akward the .dat format and a repetitive task. I don't remember now if there is another way of getting this data in a more clear way using TIME POINTS card.

DaveStupple

That's fantastic thanks Victor & Sergio. Lots for me to read up on and better understand, particularly setting the values for the hyperelastic models.

I will try to work with your model and bring the force in using tables. If this does not work I will try adding a STEP as you say, Victor. I will try to work out how to do this from the CCX manual, can you give me any pointers on where to start?

One more, how to access the reaction forces? I have noticed this in the tree before, but I can't see it now.

Thanks again, and for the link Sergio. 

D

DaveStupple

Oops, I see the forces there, plain to see...!

Sergio

Be aware that in my charts, I have made a mistake. I took yuour model and remove one element in thkcness (to speed up the calculus), so I work with 0,5 degrees. Then I multiply the load reaction by 360, but should be 720 to take in count the 0,5. Regards

DaveStupple

Trying to do the custom CCX step to 'switch off' the displacement when I bring in the force...

I copied the whole block of *BOUNDARY text and pasted in the custom step box, e.g.

*BOUNDARY,AMPLITUDE=A_67A728BC732D

4873,2,,1

*BOUNDARY,AMPLITUDE=A_67A728BC732D

4873,3,,9.540979117872E-17

*BOUNDARY,AMPLITUDE=A_67A728BC732D

4879,2,,1

I replaced the AMPLITUDE with OP=NEW then deleted the 1, except where the DoF was 3, in which case I deleted the whole section. So the above text would become:

*BOUNDARY,OP=NEW

4873,2,

*BOUNDARY,OP=NEW

4879,2,
This solved with no indicated error but did not have the intended effect. I will carry on trying to work it out. Any suggestions?
Thanks

Sergio

I don't understand why you try to mix loading by displacement and force. Using only displacement I was able to finish the assembly (fully close). Driving the movement by force is always more complicated than fixed displacement increments.

Can you share your new input file? Maybe is the OP=NEW, as far I remember it tells to release the prior dof of the nodes.

Sergio

Victor, for making the load/deflection plot I look for the values in a .dat files by means of Excel using custom filters to remove the blank lines and other stuff in the .dat file. Now I'm trying to get at list this values in Mecway by means of the table function.

Have made a rigid body to sumarize all the reaction force in the movil side in one node, and create a group of nodes for this node, but then I realize that node sets are not visible for the table function... can be this added in some future update?

Regards

Victor

You can use element or face selections instead.

Node selections is risky because for shells and beams it would depend on CCX always generating new nodes using the same numbering scheme. It'll also have to detect and cope with manually added OUTPUT=2D that will change the node numbering too.

Victor

DaveStupple, adding commands there just add them to the existing *STEP section. Define the displacement constraints in Mecway, then make a new *STEP section that has forces and no non-homogeneous displacements.

Here's how to define a 2nd *STEP section:

*END STEP

*STEP

... everything needed for the step

The first *END STEP ends the automatically generated step that would have the displacements in it. The *STEP starts a 2nd step where you can define force, and Mecway automatically adds a final *END STEP after that.

But I tend to agree with Sergio that this is probably more complicated than necessary if you can measure the force instead of specifying it.

DaveStupple

Victor, I did go back and re-read your original post more carefully and have been experimenting with a second step - not there yet, but feel I am close. 

I will certainly take a look at the force approach too. Will let you know.

Hi Sergio, the idea is to see whether the applied force will cause the two solid parts to meet, so an analysis with a varying force is the easiest to interpret. Ideally, I will apply an increasing force and see the two surfaces approach each other. I will do this for several rubber stiffness values. This will make more sense when I show the results to other people. But I will have go using displacement, and looking at the forces acting at the top interface. I will give this a bit more time, then share an inp file to let you know where I've got to.

Thanks both.

Sergio

How do you plan to represent the differen rubber sttiffnes? Viton data is not very common. Do you have measured data to correlationate?

DaveStupple

It is very difficult to find data. I am running three analyses with C10 values (0.17, 0.84, 1.7)  that represent Young's Modulus 1, 5 and 10 MPa, which I think is a reasonable range. I have no measured data, it would be useful to try to get this when the components are manufactured.

Do you have any data on the stiffness of Viton?

Sergio

Have nothing in Viton yet. I have contacted some rubber compound manufacturer here that could give me some samples to measure, but I'm not sure if they will have Viton, is a very specific compound. I will try to reactivate this issue during the week as I has to send a quotation for a related work to him. Yoy should try to make some correlations between some measured data and FEA before start to make your own model simulations, even you could look for some available data on the internet.

DaveStupple

I have not succeeded with the application of force after an initial displacement. I did not use OP=NEW, I just let the new STEP do this. It goes through the motions then returns a 'too many cutbacks' error, so it must be the fault of Theresa May and her Conservative government. I haven't looked at the results file yet. .inp file attached for your interest, but don't worry too much about it.

DaveStupple

Using just displacement, and calculating a C10 value of 1.68 to represent Young's modulus of 10MPa, I can solve but with a few distorted elements. When I do the same for 5MPa, it is too soft and the model fails horribly. From the 10MPa model, I summed the y forces from the nodes on the underside of the window (treating x and z as negligible), and converted these to pressure (applied to the whole window). I was also interested in the o-ring volume, so I excluded 5 failed elements from the selection and used the volume tool, making sure that I matched this up to the correct displacement (I ran the model with displacement = time to make this simpler).

In this example the available space in the groove is not filled. I will later try one that does. I don't think the neo-Hooke model increases the stiffness, is this correct? Would it be the case that this model will over-compress the material because it does not change the stiffness (and also no friction)?

DaveStupple

DaveStupple

Finer mesh in the o-ring failed catastrophically. Sergio makes a good point about the stiffness of Viton. I will try to get some physical tests sorted, but they are likely to be quite basic to start with. I do think the model is likely to over-estimate the compression because it may not properly reflect the material's increased resistance once deformed and compressed. And I think 10 MPa might be too soft. I've learned a lot about Mecway/CCX doing this.  

DaveStupple

Image did not attach...

DaveStupple

I have done this twice now, once with a 5.75 mm groove depth and again with 5 mm, in both cases the groove width (6.5 mm) is a little narrower than the o-ring (7 mm). With the deeper groove the window bottoms out and the o-ring does not quite fill the volume. 5 elements at the o-ring surface become distorted where contact is made with the external radii of the groove. I was concerned that the compression would be overestimated because the software does not increase the modulus of the material as it is compressed. When I ran the 5 mm groove, the compression looked reasonable: the o-ring totally fills the groove and starts to mushroom out at the top (with no distorted elements). Increasing the displacement beyond this point causes a catastrophic failure of the o-ring mesh. I think that demanding more displacement when a material that is nearly incompressible has nowhere to expand into causes the mesh failure. This is useful, if true, because the model is delivering non-sensical results in this situation rather than feasible but wrong solutions. In both cases, C10 is 1.67, and if I halve this to make the rubber softer, both meshes fail before the o-ring is seated.

Sergio

Have never look for the volume variation due to loading in rubber, as the mantra for hyperelastic materials is his incompressibility. Could it be that this change in volume is due to the colapse of some elements? Have you tried with reduced integration elements that has some formulation to reduce this colapse and hourglassing effects?

Regards 

DaveStupple

Hi Sergio, In the 5.75 mm model there were 5 collapsed elements, so I excluded these from the volume calculations. In the 5 mm model, there were no collapsed elements. I think the volume change is genuine. In the material properties, with D1 set to zero. the Poisson ratio is 0.4754, so this would allow a small amount of volume loss. I have just realised that if D1 is set to a very small value, e.g. 0.0000003 or smaller, this can be adjusted. When very small, e.g. 0.000000001, the Poissons ratio approaches 0.5. I will try with a Poisson ratio close to 0.5 to see if this minimizes the volume change. At larger D1 the Poisson ratio becomes negative. i have seen D1 defined as 2/bulk modulus, so with a bulk modulus close to infinity (incompressible), D1 would be very small, so this makes sense.

DaveStupple

With the 5.75 mm groove model, I switched on reduced integration. The model now solves without the minor element failures. Next, I left everything the same and just changed the D1 value to give different Poisson ratios. Poisson 0.4857 seems to be the cut-off between models that solve well and models that don't. At this value, there were minor element failures but still reached zero clearance without catastrophic failure. Below this value, the model solves with no distorted elements, above this value there is catastrophic failure before zero clearance is reached. There is no obvious relationship between Poisson ratio and either o-ring volume at failure, or clearance value at failure. For the runs that got to zero clearance with no failed elements, the final o-ring volume was larger for higher Poisson ratios.

DaveStupple

I took one of the models that showed an early mesh failure (i.e. shortly after the O-ring engages the walls of the groove, see image) and changed the O-ring mesh so that it was all hex20 elements (create>plate>circle, then revolve). It now solves without the early mesh failure, but does fail as the O-ring fills the groove (see image). This failure So the previous post doesn't hold true, as this model had a Poisson ratio of 0.4896. The two images show the ultimate displacement of each model just prior to catastrophic mesh failure. For the hex20 model, the failure probably comes when the displacement exceeds that allowed by the given Poisson ratio. The old model had a single node shared by the O-ring and the top component to prevent rotation. The new mesh does not have this.