What does the script do?

Stress engineers routinely need total joint resultants — Fx, Fy, Fz, Mx, My, Mz — for fastener patterns, footprint joints, ring attachments, and similar load paths. The default Nastran way to get there is grid-point-force-balance plus a hand summation, which is fine for static runs but fragile for transient or frequency-response cases where you''d rather not post-process N CBUSH outputs at every step.

This tool takes the shortcut: it creates a probe node plus six MPC equations that map the relative displacements of every CBUSH in a selected joint pattern into the probe node''s six DOF. After the analysis runs, the probe node''s translations and rotations are the joint resultants. One node, six numbers, no post-processing pipeline.

The math falls out of F = k · x: each CBUSH stiffness k directly couples relative displacement to joint force, so a properly weighted MPC equation literally is the joint force.

How It Works

  1. Collect the selected CBUSH elements and their nodes; cache positions, stiffnesses, lengths, and CSYS orientation per element.
  2. Verify assumptions: all CBUSHes share a single output (nodal) CSYS and use a supported orientation form (CSYS-on-element or CSYS-on-property). Node-vector and orientation-vector forms are not supported.
  3. Calculate the probe location — either the stiffness-weighted centroid of the CBUSH pattern, or a user-picked point in the model.
  4. Create the probe node at the calculated location, using the joint''s shared nodal output CSYS so probed displacements line up with the MPC equation coefficients.
  5. Generate 6 MPC equations: translations Tx..z = sum over CBUSH [ki·(uA−uB)]; rotations Rx..z include direct rotational stiffness terms k4..6 plus moment-arm r × F contributions from the translational forces.
  6. Apply the chosen sign convention: positive = "force ON the joint" (default), or positive = "force REACTED BY the joint."

Why a probe node + MPC instead of feFGForceBalance?

FEMAP''s grid-point-force-balance gives you per-element CBUSH forces, and those can be hand-summed for one static load case. The MPC approach wins when:

  • Transient or frequency-response runs — you do not want to post-process N CBUSH outputs at every time step or every frequency line. With this tool, the probe node''s six output values are the joint resultants for free.
  • Random vibration / PSD / RMS — reading total joint RMS off one node is much cleaner than RSS-summing individual CBUSH RMS values (which is wrong anyway because CBUSHes within a joint are correlated).
  • Many joints in one run — one probe node per joint, all six DOF, side-by-side in the post-processor.
  • The joint has a non-trivial moment arm — the tool builds the lever arms automatically; you don''t have to keep track of which point you''re summing about.

Initial Option Descriptions

Probe (summation) location

  • Pattern Centroid (default) — stiffness-weighted centroid. Heavier-stiffness CBUSHes pull the probe node toward themselves; for a uniform-stiffness pattern this is the geometric centroid.
  • Select Location — the script prompts you to pick a point in the model after OK. Useful when you want forces summed at a bolt-head datum, ring center, or other physically-meaningful point.

Output sign convention

  • Force ON the Joint — positive = surrounding structure pushing into the joint. Useful for joint-capacity checks ("is the bolt seeing more than its rated load?").
  • Force REACTED BY the Joint — positive = joint pushing back on the surrounding structure. Useful for back-out checks ("is my doubler overloaded by the reaction?").

Lever-arm reference (per CBUSH) — new in v3.00

The legacy v1/v2 of this tool assumed every CBUSH was zero-length, so both end nodes were physically coincident and there was no ambiguity in the moment arm. v3.00 supports CBUSHes of any length, which means each element has two distinct end nodes and you have to pick a single reference point per element for the r × F moment assembly. The four options:

  • Midpoint (default) — lever arm taken from the element midpoint. Symmetric across the CBUSH; the natural choice when there''s no reason to prefer one end.
  • End A — lever arm taken from the first node. Use when one side is "structure" and the other side is "fastener head," and you want moments referenced to the structure side.
  • End B — mirror of End A.
  • Probe — lever arm taken from the probe node itself, applied to both end terms. Same convention as a textbook "moment about a point" calculation: every force projects through the same reference. Numerically equivalent to Midpoint for zero-length CBUSHes.

For zero-length CBUSHes all four options collapse to identical equations.

Prerequisites

  • A FEMAP model with an interface joint represented by a pattern of CBUSH elements (any length).
  • All CBUSHes use the same orientation CSYS (CSYS-on-element or CSYS-on-property). Node-vector and orientation-vector forms are not supported.
  • The connected nodes share a single nodal output (analysis) CSYS.
  • CBUSH stiffnesses defined on the property (PBUSH K1..K6). Frequency-dependent or load-dependent stiffness tables are not supported.

Workflow

  1. Open the model and confirm the CBUSH pattern is set up correctly.
  2. Run the script via FEMAP''s Custom Tools menu.
  3. In the dialog, pick the probe location, sign convention, and lever-arm reference.
  4. Select all CBUSHes that make up the joint pattern when prompted.
  5. If "Select Location" was chosen, pick the probe location in the model.
  6. The script reports the probe node ID and creates a constraint set named MPC Eqs — <sign> — <lever-ref>.
  7. Include the new constraint set in your analysis case.
  8. After the run, query the probe node''s translations and rotations — those are your total joint Fx/Fy/Fz and Mx/My/Mz.

 

Caveats and limitations

  • The MPC equations are written in the joint''s nodal output CSYS. If you change a node''s output CSYS later, the equations no longer match — rerun the tool.
  • If you change a CBUSH''s stiffness, the equations no longer match — rerun the tool.
  • For non-zero-length CBUSHes, the lever-arm reference is fixed at script-run time. If geometry changes, rerun the tool.
  • The probe node has 6 DOF and 6 equations — do not also SPC, load, or otherwise constrain the probe node, or the equations conflict with the user-applied constraint.
  • Solver-side: this is plain MPC, supported by Nastran, Simcenter Nastran, and Optistruct. No solver tweaks needed.

 

Licensed under the Apache License, Version 2.0. Modifications and contributions welcome via This email address is being protected from spambots. You need JavaScript enabled to view it..

Main Menu