Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Changing model in mid-simulation
Hi all,
I am currently working on a concrete beam model including bonded reinforcorments on the tension side of the beam.
Now I have the follwow challenge:
The use case is, for example, that a existing concrete beam shall be reinforced to carry loads that it was originally not designed for.
This means that the beam is already carrying an initial load (from its mass and the mass of other structures above it) during the application of the reinforcements. Therefore, when the reinforcement is bondet to the beam, the beam will under tension/compression but the reinforcement itself will be strain-free. The Reinforcement will only start to experience strain when the laod is increased past the initial load.
Does anyone have an idea if / how this can be implemented in mecway?
I have not had a deep look into it yet but my current ideas (maybe not good at all) are:
- Somehow activating a contact during simulation to "attach" the reinforcement at a certain time. I suppose the trouble here would be that the beam is already deflected while the reinforcement is not so contact pairs will not align properly
- attaching the reinforcement at the beginning but with a verly low stiffness material so that it wont have an effect. Then somehow changing / increasing the material properties of the reinforcement without having the current strain for the reinforment causing tension...
searching the internet I came across the *MODEL CHANGE keyword and these example input files:
https://www.feacluster.com/CalculiX/ccx_2.18/doc/ccx/node299.html
But so far, I can't get them to work. The last thing tried is to open a fresh MW instance and copy the example input deck into a custom model definition and adding the "dont generate step" option. When Then export from MW to CCX input file, the file looks like the example as far as I can tell. But when trying to solve, I get his error message
Google says the english version of that message is "KeyNotFoundException"
Can anyone help?
Thanks!
I am currently working on a concrete beam model including bonded reinforcorments on the tension side of the beam.
Now I have the follwow challenge:
The use case is, for example, that a existing concrete beam shall be reinforced to carry loads that it was originally not designed for.
This means that the beam is already carrying an initial load (from its mass and the mass of other structures above it) during the application of the reinforcements. Therefore, when the reinforcement is bondet to the beam, the beam will under tension/compression but the reinforcement itself will be strain-free. The Reinforcement will only start to experience strain when the laod is increased past the initial load.
Does anyone have an idea if / how this can be implemented in mecway?
I have not had a deep look into it yet but my current ideas (maybe not good at all) are:
- Somehow activating a contact during simulation to "attach" the reinforcement at a certain time. I suppose the trouble here would be that the beam is already deflected while the reinforcement is not so contact pairs will not align properly
- attaching the reinforcement at the beginning but with a verly low stiffness material so that it wont have an effect. Then somehow changing / increasing the material properties of the reinforcement without having the current strain for the reinforment causing tension...
searching the internet I came across the *MODEL CHANGE keyword and these example input files:
https://www.feacluster.com/CalculiX/ccx_2.18/doc/ccx/node299.html
But so far, I can't get them to work. The last thing tried is to open a fresh MW instance and copy the example input deck into a custom model definition and adding the "dont generate step" option. When Then export from MW to CCX input file, the file looks like the example as far as I can tell. But when trying to solve, I get his error message
Google says the english version of that message is "KeyNotFoundException"
Can anyone help?
Thanks!
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
*MODEL CHANGE cannot add anything to the model, unless it was there in the first place. so to add elements or contacts, they must be difined in the the model at first.
then they can be removed in an initial step and added back again later.
In my case, using the parameter MECHSTRAINTORESIDUAL turned out to be the better option as far as I can see. It removes strain from a set of elements so they become stress free. Then they do no longer have an effect on the model.
Im not sure why, but if have to use MECHSTRAINTORESIDUAL repeatedly to remove all stress. It seems that approximately 1/3 of the stress is still there after MECHSTRAINTORESIDUAL.
In the model are two beams. The top one without reinforcement.
0-1 sec: Apply load (eg. weight of beam and permanent installations)
1-2 sec: do nothing - stress in top beam is higher
2-3 sec: remove strain from reinforcement in 10 steps
3-4 sec: do nothing - stress in both beams are identical (reinforcement is stress free eg. "not there")
4-5 sec: increase (double) the load (eg operation loads added to weight)
5-6 sec: do nothing - stress in reinforcement builds up and the bottom beam shows lower stress levels
Next step will be to try this on a concrete beam with compression only material and rebars with nonlinear material properties.