The attached model does not converge. for control by carrying out a frequency analysis it emerges that the profile is not connected to the base plate. I can’t generate the correct contact. How can I fix it
Thank you and congratulations for the excellent work you are doing
Alex
link: https://we.tl/t-lvmtKu1TYI
Try using tie constraint with enabled adjustment and proper tolerance (distance between the surfaces in pair) first. Keep in mind that you have to take the shell thickness into account when defining the tolerance.
I tried to vary the value from 0.01 to 1 with step 0.1, then from 1 to 10 with step 1, but the error persists. where am i wrong?
I specify that the base plate (solid) has been drawn with the surface coinciding with the base of the steel plate (shell)
Error.zip (582.2 KB)
The tolerance defines the distance in the normal direction within witch the solver searches for the other surface in a pair. So it should be selected based on the actual separation between the surfaces (usually with a few additional millimeters just in case) and taking the shell thickness into account.
I don’t have access to a computer now so I can’t check your model but start by measuring the distance in the normal direction between the surfaces to be connected (using Query —> Distance). It would be good if you could share some screenshots as well.
the distance between the plate base and the solid surface is equal to zero.
Also see the zip file sent earlier
The “Error in add_sm_st: coefficient should be 0” message may suggest some overconstraint. Make sure that there are no multiple comstraints acting in the same regions (like rigid body and boundary condition, rigid body and tie and so on). Try supressing constraints until the error disappears.
The model you provided will not work. The load is working in a parallel direction to the contact (Hard) surface; thus, there is a static solution.
Changing the contact from Hard to Tied, the solution is obtained. The static step (1,1) gives a sensible solution where the stresses are transferred from the profile to the base, but the Frequency step result (2,1) is strange. I think there might be a problem with a tied contact, shells and frequency analysis.
Changing the contact tied to a tied constraint works for both steps.
Thanks for the replies; I tried according to the indications but the analysis does not converge.
The model foresees that the compound-1 element is welded to the plate1 and therefore the contact between the parts must be Hard, the plate1 is in contact with the plate2 with the possibility of detachment between the 2 plates as their connection is guaranteed by the presence of the bolts, unfortunately I can’t get the results.
The model converges if plate2 and its contacts with plate1 are dropped, but this is not the desired solution
Alessandro
If compound-1 is welded to plate1, you need to use the tie constraint or tied contact. The hard contact has a compressive resistance only and transversal resistance if friction is used. In case of tension, the contact transfers no forces. Since the weld transforms the force in both ways so must the connection.
For the connection between plate1 and plate2 you need a Hard contact if you want to see the separation between them.
A simple rule to remember is that you should use tie constraint or tied contact whenever you want the parts (their surfaces) to stay connected for the whole analysis, with no possibility of separation or sliding. It’s like unbreakable glued connection. Regular (by default hard) contact should be used only when you want to allow for the relative motion of surfaces (separation/sliding) and when you are interested in contact pressure in the interface between the parts.
I tried to follow the instructions given but the calculation fails. I attach images of the connections considered (some images are with exploded views)
Thanks for your patience
the frequency analysis shows that the contacts between Compound-1 and solid-1 are correct (there are no slips and detachments), but not the contact between solid-1 and solid-2 which has interpenetration
Contact won’t work properly in a frequency analysis - it can be only frozen but won’t detect interaction when there’s an initial gap. You would have to use tied contact or tie constraint for a frequency analysis.
In the tree you have “Solid part 2 to Solid part 1” tie constraint and “Plate 1 - Plate 2” contact pair. Aren’t they applied to the same surfaces and thus redundant ? Do you have any constraints applied to the same regions simultaneously ?
I tried it again with a Hard contact between the plates and a tied constraint between the compound and the top plate, and the analysis failed. The problem seems to be that on the top plate, the internal surfaces of the holes are fixed, and at the same time, the bottom edge of the holes is included in Hard contact. If I change the fixed support of the top plate to include only the top edges of the holes, the analysis works.
Good morning
the model sent represents a classic connection of a column of a building to the foundation and foresees a column with stiffening plates (compound-1), connection plate to the column (solid part-1) connected to each other with Tie contact; the plate (solid part-1) has holes (to simulate the presence of connection bolts to the foundation), the edge of the bolt holes have a Fixed type external contact. to correctly determine the force of the bolts, the foundation (solid part-2) was considered with a contact type Hard (which allows the possible detachment between solid part-1 and solid part-2) for the surfaces in contact between solid part-1 and solid part-2 .
The bottom surface of solid part-2 was constrained with a fixed contact. Surely there are two types of contact for the solid part-1 surface: a Tie between compound-1 solid part-1 and a fixed type for the edge of the bolt holes.
I also tried with another model where two distinct surfaces were considered to replace solid part-1 and solid part-2, assigning the indicated constraints, but the calculation does not converge.
I also tried to create a single compound that includes the square profile + the vertical stiffening plates + the horizontal plate (as a surface), to avoid creating contact between the edges of the square profile and the stiffening gussets with the horizontal plate. but the compound fails and no mesh is generated. I can’t figure out how I can overcome the problem.
Thanks for your availability
Agazzotti
There is a limitation to meshing the compound parts. There should be no edges splitting the surface that end in the middle of the surface or edges that do not split the surface into 2 separated faces.
Figure 1: Unsupported face configurations
The face configurations in Figure 1 must be split into two separate faces in order for the Netgen mesher to be able to mesh them properly.
Figure 2: Supported face configurations