Engineering Tools

MPC Equation Creator

Engineering Tools — MPC Equation Creator (00228)

Availability: this tool ships in customer and super-user packages of Engineering Tools, not in the standard download. Contact the admins if it would help your workflow.

What this tool does

Turns a pattern of CBUSH elements — a bolted joint, a fastener row, an interface — into a single probe node whose six “displacements” are the total joint load: T1, T2, T3 = Fx, Fy, Fz and R1, R2, R3 = Mx, My, Mz about the probe.

It does this with six MPC equations, one per DOF. Each one ties the probe DOF to the CBUSH end displacements times the CBUSH stiffnesses, so the probe carries the force and moment that cross the joint and adds no stiffness of its own. The analysis is unchanged; you get one extra node to read.

When you want it

  • Frequency response and transient runs. You get one time history or FRF of the joint load straight from the solver, instead of post-processing every CBUSH force at every frequency or time step.
  • Interface loads. Get one resultant per joint, about a point you choose, ready for a margin check or a hand-off to the next analysis.
  • Checking a fastener pattern. The probe sums every CBUSH you pick, including several CBUSHes sharing a node (spider hubs, doubled fasteners).

How to use it

  1. Give the joint's CBUSHes an orientation from a coordinate system (on the element or the property), and give their nodes the same output coordinate system. The tool checks this and stops with a message if they differ.
  2. Open Custom Tools > Meshing > MPC Equation Creator.
  3. Choose the options (below) and click OK.
  4. Pick the CBUSH elements that make up the joint.
  5. If you chose a user-picked location, pick the probe point.
  6. The tool creates the probe node and a new constraint set holding six equations named Tx, Ty, Tz, Rx, Ry, Rz.
  7. Use that constraint set for constraint equations in your analysis set, next to your usual constraints, and request displacements on the probe node.

Options

Probe locationPattern stiffness centroid (each axis weighted by that axis's CBUSH stiffness, summed over every CBUSH on a node) or user-picked location. The moments are reported about this point.
Sign conventionForce ON the joint or force REACTED BY the joint — the same numbers with the opposite sign. With “on the joint” the probe reads the sum of the CBUSH element forces as Nastran reports them, K(uB − uA), so it follows your end A / end B ordering.
CBUSH spring locationMust match where the spring sits on your CBUSHes (the CBUSH S field): Midpoint, S = 0.5 (the Nastran default — use this unless you set S), End A, S = 0, End B, S = 1. For zero-length CBUSHes all three give the same answer.

How exact is it?

Tested against Simcenter Nastran with every option combination. The joints had zero-length and offset CBUSHes, with and without rotational stiffness, carrying a known force and moment. With the spring location set to match the CBUSHes, the probe reproduced the load that crosses the joint to within 0.01 lb, and the moment about the probe likewise.

Choosing the wrong spring location on offset CBUSHes is not a small error: on a 0.5 in offset it misstated the force by up to about 20% of the load in that test.

The math, briefly

  for each CBUSH, with ref = its spring point and every grid displacement projected
  to ref through that grid's rotation (u' = u + theta x (ref - grid)):

    F_bolt = k_t * (u_B' - u_A')                         (per axis, CSYS of the joint)
    M_bolt = k_r * (theta_B - theta_A) + (ref - probe) x F_bolt

  probe translations = s * sum F_bolt,   probe rotations = s * sum M_bolt
  s = +1 "force on the joint", -1 "reacted by the joint"

The rotation projection is what makes offset CBUSHes come out right: it matches the rigid offsets Nastran itself uses between the grids and the spring point.

Tips

  • CBUSHes with a zero stiffness term simply drop that term from the equations.
  • Every run makes a new probe node and constraint set, so you can have probes on several joints in one model. Put their equations in the constraint-equation set you analyse.
  • The probe is a plain grid with no stiffness. Do not constrain it, and do not connect it to anything.

Related tools