{"id":403827,"date":"2025-01-07T03:56:57","date_gmt":"2025-01-07T03:56:57","guid":{"rendered":"https:\/\/innovationspace.ansys.com\/forum\/forums\/reply\/403827\/"},"modified":"2025-01-11T12:25:16","modified_gmt":"2025-01-11T12:25:16","slug":"403827","status":"publish","type":"reply","link":"https:\/\/innovationspace.ansys.com\/forum\/forums\/reply\/403827\/","title":{"rendered":"Reply To: How to extract running loads and moments from SHELL181 elements in workbench?"},"content":{"rendered":"

<p>Since I was in the Units of inches and lbf when I created the User Defined Result, that information was captured and can be seen in the Details window.<\/p><p><\/p><p>That means that if I change Units and solve in mm and N, SMISC values will change but the Details window becomes misleading.<\/p><p>Most output such as moment reaction probes, stress and deformation will respond to changes in Units by updating the output values approprately. For those outputs, it doesn’t matter what Units you solve in. That is not true for SMISC. The values do not update when you change Units. The SMISC values depend on what the Units were when you Solved. The best practice to avoid solving in different units than the User Defined Result details window shows is under Ansys Settings, Analysis Data Management, Solver Units, set that to Manual so you can select a specific unit system such as Bin for the Solver to use, independent of what the Units are set to in Mechanical for viewing results when you hit the Solve button. Then the SMISC output will alway be in the British inch (Bin) units.<\/p><p> In Ansys Help, Mechanical APDL, Element Reference, SHELL181 has Table 181.1 that says what the names mean.<\/p><p><\/p><p>Then Table 181.2 says what the SMISC number is to get that output.<\/p><p><\/p><p>The average moment is zero on the left (-x) edge where the transverse force is applied and is 10 in-lbf on the right (+x) edge. Half way along the length the average moment is 5 in-lbf.  You can see the SMISC4 output for elements are -4.5 in-lbf\/in on one side of the center and -5.5 in-lbf\/in on the other side of the center. [edited to add units which are per unit length, the model is 1 inch wide]<\/p><p>One confusing item is that SMISC4 is for M11, or moments about the X axis, but the large moment is about Global Y. It seems ACP(Pre) messes up the Element Orientation item that was imposed on the shell elements in Static Structural and Ansys warned me about that.<\/p><p><\/p><p>I don’t work with ACP(Pre) so I’m not sure how to resolve the confusion. Element Orientation worked correctly in other shell models I have done.<\/p><\/p>\n","protected":false},"template":"","class_list":["post-403827","reply","type-reply","status-publish","hentry"],"aioseo_notices":[],"aioseo_head":"\n\t\t\n\t\n\t\n\t\n\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t