To get Grid Point Forces in your results you should request them in analysis options:
Then you get Applied/Reaction and Summed GP Forces for nodes (vectors 161-188):
And also GP forces on elements (element has results for each node, in my case I have only beams that's why I have C1 and C2 results - for 2 ends):
Nodal or elemental results you would like to get using API?
Elemental routine will be a bit more complex.
2) As you can see on screenshot above you can get gp forces using List - Query method.
Hope this helps.
Yarko, I have requested gridpoint forces to be printed (in the DAT file) for a specific nodes, I can see them listed in the F06 file but can't see them in Femap!
In "Select Post Proccessing Data" menu, the "161.. Total Summed GPForce" option is missing (as well as 168-188 options)!
Set 1 = 600100,600200,600300,600400,600500,600600,600121,6
ELFORCE(PRINT,PLOT) = 1
DISPLACEMENT(PRINT,PLOT) = ALL
SPCFORCES(PRINT,PLOT) = ALL
GPFORCE(PRINT,PLOT) = 1
Before you run analysis you need to request force balance forces and than you will see all vectors (see my first post).
Here is an example how to get applied GP forces for selected nodes (vectors 172 -T1, 173- T2 and 174 - T3). In my example Output Set ID is defined manually in line: Output1.setID =19.
Sub Main Dim App As femap.model Set App = feFemap() 'vectors for applied gp forces T1, T2, T3 Dim appliedGPForceX ,appliedGPForceY, appliedGPForceZ As Integer appliedGPForceX = 172 appliedGPForceY = 173 appliedGPForceZ = 174 'select nodes to display results Dim nodeSet As femap.Set Set nodeSet = App.feSet If nodeSet.Select(FT_NODE,True, "Select Nodes" ) = FE_CANCEL Then End Dim nodeIds As Variant Dim count As Long nodeSet.GetArray(count, nodeIds) Dim Output1 As femap.Output Set Output1 = App.feOutput 'use output set with Id = 19 Output1.setID =19 For i = 0 To count -1 Dim x As Double, y As Double, z As Double Output1.Get(appliedGPForceX) x = Output1.Value(nodeIds(i)) Output1.Get(appliedGPForceY) y = Output1.Value(nodeIds(i)) Output1.Get(appliedGPForceZ) z = Output1.Value(nodeIds(i)) App.feAppMessage(FCM_NORMAL, "Node ID = " & nodeIds(i) & " " & x & " " & y & " " & z) Next End Sub
For summed forces and constraint gp forces you should vector 172, 173, 174 on (162, 163, 164) or (182, 183, 184)
Can you please teach me how to include the load cases in the example module (I would like to be able to choose a specific LC)? Also how to include the R1, R2, & R3 values in the result?
Short question to understand what you need:
You would like to select load cases using dialog window (each time tool will ask to select Output Sets for which to show resutls)? Or it is fine to define Output Sets (Load Cases Resutls) IDs in code?
To be short: Do you want to select load cases with user interaction?
Tomorrow I can update this example to use R1, R2 and R3.