## Preprocessing

Topics relate to geometry, meshing, and CAD

#### Multi step analysis : Activate/deactivate

• aozer
Subscriber
Hi there,nI am working on a static structural multistep analysis. In this analysis a boundary condition (nodal displacement-this is a center for rotation) deactivated in 13.step (before 13.step all steps active for this bc) and at the end then a new boundary condition (another nodal displacement-a new point for center ) activated in 13.step (before 13.step all steps deactivated for this bc) and continues to end. Is it true? I think this logic does not work for me. It works at the and of the 12. step. When enter the 13. step, analysis does not continue and stops due to element formulation. What can we do? Any idea. Thank you all.n
• aozer
Subscriber
I want to explain the problem a bit more: For examplenin first step : The part rotates with remote rotate command with respect to a center (the center created with nodal displacement)nin second step : The center changes to another coordinate (new center created with nodal displacement)nCan we do this with activate/deactiveate in multi step analysis?.n
• peteroznewman
Subscriber
nPlease reply with an image or sketch of the first point that acts as the center point and label the second point that is used in step 13 to be the new center. What is the overall goal of the analysis?nOne method I have used before is to have a Contact definition that bonds two parts together, but is Deactivated in the first step. Loads and Boundary conditions can support and move the two parts in step 1, then in step 2, the contact is activated, bonding the two parts together at their current location. Then further changes in the Loads and Boundary Conditions can take place in step 3.n
• aozer
Subscriber
Dear Peter, thank you for your reply. Attached a picture. The first bc A and B, they are togather center of rotation of component until at the end of the step 12. Then center changes to F in step 13 and 14. After, the center changes to G in steps 15, 16. And then in steps 17 and 18 the center becomes E and at the end of the step 18 it stops.nn
• peteroznewman
Subscriber
nIn the example below, during step 1, the body rotates about the gold star, carrying the green star with it.nWhen you deactivate the gold star BC, what are you using for the displacement on the green star at the beginning of step 2 since it was displaced in step 1?nThis is a knee replacement joint right? You could just let contact between the two parts dictate where the top part is and apply a minimal constraint to rotate the top part such as a Rotation about Y on a remote point (deformable) on the top, leaving all other DOF free, and use Gravity to apply a force in the -X direction to keep the faces in contact. Rotation about Y does not have to occur about a fixed axis. The axis is free to float because you leave all those constraints Free.n
• aozer
Subscriber
Hi Peter, thank you. nYes, you are right, it displaces, i use nodal displacement to fix green star as a new center.Is not is true. Or what can i do?nYour suggestion is good idea, i am working on knee replacement, but i could not achieve convergence. When i apply gravity the top part, does not rotate.I use remote displacement about Y and others free. The bottom part fixed at the bottom. What is problem?n
• peteroznewman
Subscriber
nOn the green star, are you using a command to fix that node at the current value? That is okay.nFor the model with the gravity and the remote displacement rotation about Y with all free, you have to use many substeps. What angle of rotation did you specify?nUnder Analysis Settings, turn Large Deflection On.nSet Auto Time Stepping On.nSet Initial and Minimum Substeps to 100 and Maximum Substeps to 1000.nClick on Solution Information Folder set the Newton-Raphson Residuals to 3.nSolve and if it fails to converge, reply with the Newton-Raphson Force Convergence Plot and the Newton Raphson Residual Force Plot.nThe corrective action could be smaller elements where the Residual is a maximum or change the contact settings.nUnder the Frictional Contact details, set the Normal Stiffness to Factor and enter 0.1n
• aozer
Subscriber
I use nodal displacement for lets say green star and fix x,y and z to zero, rotations free. After for example step 12, I want from upper part to rotate (according to my boundary conds and constraints) about another point (new center). I rotated upper part 90 degree about one center to end. I achieved convergence in this way. But problem is when I rotate it about one center it deforms elastically pointed (*) part so much. So, this unwanted. When it touch to (*) part as in reality, I want it to rotate about here where it touch.n n
• aozer
Subscriber
thank you so much. Your suggestion works. But we could not solve with activate/deactivate .n