I prepared a simple static 2D (plane stress) analysis of a bimetallic strip subjected to temperature difference. It works in Abaqus but when I submit it in CalculiX the analysis terminates without error.
I have two input files showing this problem - one the same as in Abaqus with a single part having different materials in different regions and another one with two parts and contact between them (the mesh is also different):
Can you confirm this issue ? Do you know what can be causing it ?
¿Do you have the source problem statement data, geometry, BC, properties?.
The problem is referring to rotational DOFs in *BOUNDARY:
I found this by iteratively deleting groups of cards until it solved then adding them back to isolate the problematic one.
The geometry is very simple - two rectangles 120 mm long and 4 mm heigh (beams forming a bimetallic strip are 120x20x4 but depth of 20 mm is included as a section thickness in plane stress). Beams are connected with a tie constraint. One end of the layered beam is fixed (it’s a cantilever). The only load is predefined temperature of 80°C and I also had to add an initial temperature of 20°C in CalculiX (in Abaqus it’s not necessary). Material properties are as follows:
- copper (top layer): E=110000 MPa, ν=0.35, α=1.7E-05 1/°C, T_0=20°C
- steel (bottom layer): E=200000 MPa, ν=0.33, α=1.23E-05 1/°C, T_0=20°C
Thank you very much. I thought that the solver will handle this automatically but I forgot that in CalculiX it’s not necessarily the case (I had a similar problem with beam elements some time ago).
Now I just have to figure out how to increase the accuracy since the maximum deflection obtained in CalculiX is 0.4743 mm while the analytical solution for this case is 0.38 mm.
Increase the accuracy or confirm it! Sometimes it’s the hand calcs that have the error because they idealize too far - high slenderness assumption or, for example, or neglecting the Poisson effect.
That’s right, analytical calculations are often very simplified and it can be difficult to eliminate all the differences in the assumptions of the analysis and hand calcs.
Even in Abaqus I keep getting the deflection around 0.5 mm. Normally, I would suspect that the interface between the layers is modeled incorrectly but it must be bonded (no slipping) for this device to work so it shouldn’t be the case. Some time ago, I made a 3D thermo-mechanical analysis for this case and the results were similar (0.52 mm) so it’s not a matter of the simplified approach that I’m using now.
The assumption on the theoretical result (plain stress) is very strong. I would basically say that Plain stress and “fixed support” are incompatible BC if we consider Poisson Ratio . Note Victor is also pointing in that direction. Far from the supporting areas stresses could be ok but here you are looking at deflections. Any small deviation in the supporting area of a cantilever beam is amplified on the tip.
To get plain stress on two plates with different thermal expansion coefficient I would consider the thickness small compared with high. The largest the thickness, the further the Plain Stress assumption will be.
I have considered 1mm which is closer to satisfy a plain stress condition. If you go to 3D and 20mm, the plates are probably bending and tips going down more than the center of the strip.
I’m obtaining :
Maximum vertical displacement of beam at Top and Botom of beam:
CPS4: [ -0.357642, -0.350605 ] mm
CPS4R: [-0.376332 , -0.383329 ] mm
CPS8: [ -0.379072 , -0.372064 ] mm
CPS8R: [-0.371977 , -0.378983 ] mm
Maximum displacement of beam:
CPS4: [ 0.3732 ] mm
CPS4R: [ 0.3981 ] mm
CPS8: [ 0.3939 ] mm
CPS8R: [ 0.3938 ] mm
That’s right, thank you for pointing this out. I didn’t realize that it might be necessary to use unit thickness to obtain the results agreeing with the analytical solution.
So it seems that the deflection of 0.5 mm (obtained with actual thickness in plane stress and with 3D model) is more realistic but the one of 0.38 mm (obtained with unit thickness in plane stress) is more compatible with the plane stress assumption of the analytical solution. Do you agree with this ?
Well…,I would not say 0.5mm is more realistic. If you were right, one could be tempted to use always Plain Stress no matter what.
In this problem, thermal expansion and Poisson ratio are constraining the displacements in the transverse direction too as both plates are tied. It’s technically impossible to get Plain Stress.
We can use 1mm just to approach that assumption and validate but for the device design I think better 3D.