I trying to start small and build up to a slightly more complex study. For now, I’m analyzing a simple tube in PreProMax, and I got widely different results from hand-calcs.
PreProMax says: 0.006999728 Rad (~0.4 deg)
Hand Calcs says (13deg)[Torsion of a Thin-walled Open Tube | Online Calculator] EDIT: this is the wrong formula, leaving it here to keep the thread coherent)
The mesh is 1mm to 0.1mm, with the other settings remaining default.
I applied 500 N⋅mm to a rigid body from a reference point at one end, and made a fixed boundary condition on end-surface of the other end. Then I look at UR3 for the rotational displacement in the Z-axis.
What other information should I include here to ask for help?
If I upload the .pmx file to share, do I also need the .STEP file separately?
Where should I start looking for my problem?
I’d like to apply more force, but I expect I’ll need a non-linear study for more deflection. I need to learn more before I can do that.
Please share the .pmx file. No need for a separate .step file. You can upload it to some hosting website like WeTransfer, Google Drive or Dropbox and paste the link here.
The formulas are for open tube, I assume that your model accounts for that. It would be easier to start from a closed pipe. Formulas from Roark’s:
Rotations are nonlinear effects. Default iteration scheme may lead to error. Try to switch to automatic with a minimum of 10 increments for the whole period. Let us know if that fix your discrepancy.
As I suspected, your part doesn’t have a cutout so you should use the formulas for a closed pipe. I shared the ones from Roark’s above. I would also refine the mesh - it’s very coarse in your model.
You’re right - I’ve checked my math and discovered that I was using the wrong formulas. Thank you for straightening me out. It’s always nice to discover the FEA was right and the hand-math was wrong.
I’m starting with this shape/loading because I’m designing a part that will be a derivative of this. It will get various slots/holes/changes in wall thickness.
As deflections get larger, I’ll need to move to non-linear analysis, no?
I’m struggling with the details of how to do this, and what sources to trust.
My understanding is that we’re trying to put in more data points in the relevant region of the stress/strain curve. I assume the software does linear interpolation between them.
Stress up to yield is assumed to be linear, so we’d enter Yield-stress and 0? or 0.2%?
Then we need some additional points along the curve in the plastic region. Should I be grabbing these from a stress/strain curve?
I’m currently working with 316 Stainless Steel (1.4401 in some parts of the world). I found this curve from as figure 9 in this paper.
I tried to grab some values from first part of the graph
205 MPa, 0 mm/mm
310 MPa, 0.01 mm/mm <–QUESTIONable measurement!
675 MPa, 0.2 mm/mm
900 MPa, 0.44 mm/mm
Is there a more accepted method for acquiring / entering this data?
You can use a bilinear model (hardening recommended) like this, for instance:
Re ——- 0
Rm —— A
where Re is yield strength, Rm is tensile strength (UTS) and A is elongation at failure.
Or you can specify more data points to define a while nonlinear stress-strain curve (keeping in mind what I said at the beginning about the required stress and strain measures).
Between them - yes. But outside of the specified data, it assumes plateau (horizontal line). You should avoid this due to potential convergence issues - do the linear extrapolation manually by specifying higher stress-strain values as the last point.
Special attention to this @JKnight ! Some people may be familiar with Nastran in which some non-linear solutions use engineering stress and strain… In CCX we need to use the true ones. The results can be very different.
Thank you for clarifying. I believe I can use the curve in the top-half of the image I posted. I wish I had more of the data they used to create the graph.
