Questions regarding efficient retrieval of Nodal Forces and applying displacements in MAPDL

[HazemEldahshan]

Hello,

I am trying to find an efficient way to retrieve the elemental nodal forces for the entire mesh directly from the MAPDL session “on the fly,” without having to write the results to an .rst file and retrieve them afterward. For large meshes, this additional I/O step becomes a significant bottleneck in my algorithm. Could you please let me know whether there is a way to access these forces directly from the MAPDL session without generating an .rst file?

I also have a second question regarding the application of prescribed displacements to the model’s degrees of freedom. Currently, I create a NumPy array containing the displacement values for all DOFs at every time step and then load it using the load_table function. Since my algorithm applies displacements to all nodes in the model many times, this operation is also becoming quite time-consuming and represents another bottleneck.

Could you please advise whether there is a more efficient way to apply these displacement constraints, or whether there are any recommended approaches for improving the performance of load_table in this situation?

Thank you in advance for your help.

Best regards,
Hazem

[germa89]

Regarding retrieval of the elemental nodal forces, I am not sure. I will leave it to @mikerife to comment.

With respect to the application of prescribed displacements, load_table() is intended for transferring a MAPDL table. Calling it repeatedly for a full mesh is expensive because each call creates/transfers a file and executes TREAD. A better approach is to transfer the complete displacement history once as an array or table, then let MAPDL apply it internally.

I hope it helps!

[HazemEldahshan]

In fact, the table content changes at each iteration in ly algorithm, so I need to update it regularly. One possible approach would be to develop a method that reads only the spatial and temporal modes, allowing ANSYS to reconstruct the complete displacement history directly within the solver, such that:

U(x,t) = Σ X(x)T(t)

This approach would significantly reduce the amount of data that needs to be read from the file and, consequently, improve the computational efficiency.

Would it be possible to implement this approach as an evolution within ANSYS?

Best regards,
Hazem

[germa89]

I would then open a service support ticket to ask for that feature. You can then post here their answers.

[nazeeh111]

This addresses the force-retrieval part of your question. It helps to distinguish the two outputs:

• MAPDL's NFORCE is a nodal sum of contributions from attached elements, not the per-element force at each element node. With all elements selected it usually cancels except at loads or constraints; contact elements are excluded unless you request BOTH. For element-by-element nodal forces, use PRESOL,F.
• For numeric bulk access, the documented PyMAPDL route is the results file: mapdl.result reads .rst through DPF or the PyMAPDL reader, and DPF exposes element_nodal_forces. There is no documented live bulk API for these POST1 result fields that bypasses .rst.

If the needed result is missing or the file is too large, request only element-nodal load output before solving:

mapdl.outres("NLOAD", "LAST")  # last substep of each load step

Use "ALL" instead if you need every substep. Then read the selected result sets in bulk with DPF instead of making one remote *GET,EFOR call per node. This specifically covers the force-output question; your maintainer's response about transferring the displacement table covers the separate loading bottleneck.