I have completed a non linear dynamic analysis in FEMAP , with large displacements enabled. Having large displacements enabled was essential for the model to run correctly. I wish to extract the axial and shear forces from some beam elements. The beam elements represent bolts.
Using 'large displacements' has meant that the following results , amongst others, are not available:
3018..Beam EndA Pl1 Shear Force
3019..Beam EndA Pl2 Shear Force
3022..Beam EndA Axial Force
I'm guessing the orientation of the co-ordinate system for the respective element moves with it as the element displaces.
Does anyone know how I extract the resultant shear and axial forces? Direction is not essential.
I'm also trying to understand what the 'Pt1' means in the following item, I can't find anything in the FEMAP user guide. Can anyone explain?
3901..Nonlinear Beam EndA Pt1 Comb Stress
3901..Nonlinear Beam EndA Pt1 Comb Stress represents the combined stress due to axial and bending forces at "end A, location 1" in the beam cross section. When defining beam and bar properties, you can choose up to 4 locations on the cross section to calculate stresses. See the diagram below, Femap has standard or common extreme fiber locations preset for you, but you can edit these if desired.
The only element forces that are output for nonlinear transient are for CBUSH and CBUSH1D elements. CBUSH elements are not large displacement, so depending on how much rigid body motion your bolts have, they might be an acceptable choice instead of using CBEAM. You would just need to calculate the equivalent beam stiffness to input on the CBUSH.
CBUSH1D does account for large displacement, but it is a single DOF, and is not supported by Femap currently, so a lot more work to use it.
My best guess on why you no longer see your shear and axial forces is that maybe you didn't request Element Forces in the output request section of your analysis set. It shows up in one of my NL runs that requested element forces. As far as the bulk data file goes, in the Case Control section you should see FORCE(PLOT) = ALL, or print or a set number. If you use a bulk data file.
Regarding 'Pt1', this is the stress recovery point that is defined when you create your beam property. It's location is based on your orientation for the section. See the attached image.
Great, the 'Pt1' makes sense now. Will be useful for other analyses.
I'll give the CBEAM element a go. I'm modelling a sprocket drive braking a large drum. The CBUSH elements are simulating the link between the drum and the sprocket drives. The only part of the model that undergoes large displacement is the drum as it rotates. I'll however try the CBEAM elements for interest.
I have the 'Force' box enabled. Fembrackin describes how NL loads are produced as 'combined stress' values. So I should be able to extract the loads with some number crunching in Excel.
Thanks for clarification of the 'Pt1' values. Again, I'll manipulate these to extract the bolt loads.
They should also prove useful for future analyses.