Hi Peter (@pborgens),
there are two types of contacts in SimScale:
Contact Constraints - These are linear relations for connecting bodies. Available types are bonded, sliding or cyclic symmetry.
Physical Contacts - These are non-linear relations for allowing separate bodies to interact with each other i.e transmit forces if and when they are in contact.
For some reason, which I don’t fully understand, using two physical contacts, on the same body, opposing each other, is proving to be problematic.
It turns out that this is only problematic for second order meshes. Where possible I always use second order meshs. However in this case a first order mesh is probably acceptable so long as it is sufficiently fine. At a minimum you should have at least three elements through any thickness, especially if the member is in bending. Three elements allows for tension, compression and a neutral axis.
I have added a first order simulation to my public project. In this case I have used four elements through the thickness of the spring.
Here are the results.
To create the force-displacement curve I used Excel. Here are the steps:
- In SimScale navigate to the Post Processor
- Expand the simulation of interest to show the Face Calculations
- Click on RY press (1) > Reaction Force. This is the force required to lift the press plate.
- At the top right hand corrner of the chart there is an icon for chart options. This gives the option to download the plot as an xls or csv file.
- Open the data in Excel (or equivenlent). You will need to multiply the force by two because it is a half model. You will need to convert the time to distance (1 sec = 2 mm).
The plot for the first order mesh looks like this:
It can be seen that the spring stiffness is a little higher with first order elements. This is to be expect because first order elements tend to be too stiff in bending. You will need to keep this in mind.
The forces are multiplied by two because we are using a half model. Half a spring requires only half the force to bend it a given distance.
To move forward this is what I suggest:
Use a first order mesh to optimize your design. Compare it to the results obtained from the original spring with a first order mesh.
As a final check create a second order mesh and simulate the last time step only (maximum displacement). Compare the results to those obtained from the original spring with a second order mesh. The second order mesh is only problematic with multiple time steps.
I would double check the dimesions of the current system. The stress seems too high. I would not be surprised if the spring is thinner than what has been modelled or the maximum displacement is less than 2 mm.
When you’re done please post back the results. I’m interested to see what you come up with.