Discussion Forum

Hi Mathias,

There are some problems in your model.

1. The last node under Geometry is 'Form Union', so all parts are 'welded' together. This is the most fundamental reason for why your model is too stiff. The beam is more like fixed than simply supported. Change to 'Form Assembly'. Note that you have to re-define your contact pairs after this operation, since the splitting of boundaries in the model will change.

2. The two last Contact nodes do not have any selections. On the other hand, you could skip them, and keep only the first Contact node and select all contact pairs there as long as you use the same settings for them all.

3. In the contact pairs, you use the convex boundaries as 'Source'. This is correct and necessary as long as they are rigid, but for a flexible domain they should preferably be 'Destination'. You can switch with one mouse-click in the contact pair definition.

4. An analysis including friction should not be solved in a single load step, since the friction forces depend on the sliding, so it is history dependent.
- Add a parameter 'Load' under Global Definitions->Parameters
- Replace your load '9' by the parameter 'Load'
- Under Study1->Stationary->Study Extension, select Continuation. Then add Load as Continuation Parameter and use range(1,1,18) for parameter values.

5. In its initial configuration, your model is unstable. There are possible free rigid body translations and rotations now that the parts are no longer 'welded'. The simplest way of handling an initially unconnected contact model is to add weak springs. Add for example a Spring foundation at the domain level, and select the free floating domains. The spring constant can be made dependent on the load parameter, so that the spring is only used in the beginning of the simulation.

6. (Minor improvement) One Linear Elastic Material node is enough since you take the material data from the Material node.

7. (Minor improvement) On the two fixed supports, it is better to use Fixed constraint on the domain level than on the boundary. Then you will not need to solve for a lot of zeros in the internal of these domains.

8. Maybe the mesh on the rounded parts should be finer. It is usually difficult to make a contact model converge if the contacting boundary is very roughly 'faceted'.

9. You can speed up your analysis and get rid of most of the rigid body motions by employing the symmetries of the problem.

Regards,
Henrik

Hi Henrik,

Thank you very much for your extensive feedback!

I have implemented your suggestions. For simplifying the model I will try to simulate it without friction at first and then later when the model works implement your suggestions from point 4.

To point nr.1: in how far should I redefine my contact pairs?

To point nr: 5: I have implemented a spring foundation to achieve “weak springs”, but I am not certain if I configured it correctly. www.comsol.com/support/knowledgebase/1102/

When I am computing the results, the “segregated group 1” doesn´t converge. Could that be due to the wrong configuration of “weak springs”?

Best regards
Mathias

Hello Matthias,

would that be possible that you have used a linear small deformation analysis with fixed constraints at the edges in contact along z and y in the study you mention?
Just add a point fixed along x and y where you apply your force so that the problem is well posed.
The steel parts being much stiffer than the shell, you can remove them from your analysis at first.
If you do this kind of simplified numerical experiment, you get with a default mesh 2.46mm as deflexion at the center, which looks pretty close to what you expect. It goes to 2.49mm with a slightly more refined mesh. Without the added complexity related to contact modeling about which Henrik's comments are good to know.

Best regards,
Eric

You should have received the file.
I guess you could be very close in 2D as well. I mean that in that specific case (with no multiphysics, symmetries, linear analysis...) 3D does not really help to get a good approximate solution.
This is actually an interesting case where it is not a small job to reproduce this exact numerical experiment in the real world!
Note that you can extract a geometry from a work plane and start modeling immediately with 4.3b.
Last comment : Perhaps you would like to test the structural shells as well, and compare.

Good luck,
Eric