topic Re: Surface Contact of Bolts DO NOT WORK in Simulation Mechanical Forums (Read-Only)

Surface Contact of Bolts DO NOT WORK

Anonymous — Sun, 15 Feb 2015 10:20:52 GMT

Hello everyone,

I am experiencing hell during my analises of a structural steel connection. The thing I am trying to model and discover are the traction and shear loads of some anchor bolts.

The model is the following:

The blue part is a brick element concrete wall.

The orange part is a brick element steel plate.

The green parts are brick element anchor bolts.

The gray parts are shell element steel plates.

The loads are inputted onto the shell elements steel plates by the usage of rigid links.

The restraints are complete (all 6) and done around the concrete (as shown) and on the back as well.

The surface contacts I set are:

1- The back of the orange brick plate with the front of the blue concrete wall.

2- The holes of the orange plate with the cilindrical part of the anchor bolts

3- The front of the orange brick plate with the head of the anchor bolts.

The following pictures show the contacts between the bolts and the orange plate (I hit some surfaces for visualization purporses

Important Notes:

1- The CAD spacing between the concat parts are always 0.5mm

2- I checked they do not share elements and the mesh is well made.

3- I put some refinement for the surface of the holes of the orange part so that they would match the size of the bolts.

4- The bolts are aglutinated into the concrete wall part (they have no space and they share elements - bounded contact

----------------------------------------------

Check Model Results:

When I check the model, I get some warnings, but I think it is due to the rigid links for load application.

Autodesk (R) Simulation Nonlinear Analysis Decoder for AGSDB
2015.01.00.0013-W64/X64 12-May-2014
Copyright (c) 2014, Autodesk, Inc. All rights reserved.

Model [test.ds_data\1\ds] opened

Zapping NODES, ELEMENTS, NODECOND, and ELEMCOND tables ...
Start to make nonlinear analysis AGSDB model ...
Made 151886 node tables
Start to make nodal condition tables ...
Start to make element tables ...
Element Part(101): Brick element
Made 1471 element tables
Element Part(100): Beam element
Made 128 element tables
Element Part(54): Original Shell element
Made 117 element tables
Element Part(53): Original Shell element
Made 132 element tables
Element Part(52): Original Shell element
Made 117 element tables
Element Part(51): Original Shell element
Made 84 element tables
Element Part(50): Original Shell element
Made 84 element tables
Element Part(49): Original Shell element
Made 132 element tables
Element Part(48): Original Shell element
Made 117 element tables
Element Part(47): Original Shell element
Made 84 element tables
Element Part(46): Original Shell element
Made 84 element tables
Element Part(45): Original Shell element
Made 132 element tables
Element Part(44): Original Shell element
Made 448 element tables
Element Part(43): Original Shell element
Made 334 element tables
Element Part(42): Original Shell element
Made 448 element tables
Element Part(41): Original Shell element
Made 334 element tables
Element Part(40): Original Shell element
Made 448 element tables
Element Part(39): Original Shell element
Made 334 element tables
Element Part(38): Original Shell element
Made 448 element tables
Element Part(37): Original Shell element
Made 334 element tables
Element Part(36): Original Shell element
Made 238 element tables
Element Part(35): Original Shell element
Made 238 element tables
Element Part(34): Original Shell element
Made 105 element tables
Element Part(33): Original Shell element
Made 105 element tables
Element Part(32): Original Shell element
Made 238 element tables
Element Part(31): Original Shell element
Made 238 element tables
Element Part(30): Original Shell element
Made 133 element tables
Element Part(29): Original Shell element
Made 133 element tables
Element Part(28): Original Shell element
Made 314 element tables
Element Part(27): Original Shell element
Made 290 element tables
Element Part(26): Original Shell element
Made 36 element tables
Element Part(25): Original Shell element
Made 32 element tables
Element Part(24): Original Shell element
Made 284 element tables
Element Part(23): Original Shell element
Made 315 element tables
Element Part(22): Original Shell element
Made 160 element tables
Element Part(21): Original Shell element
Made 845 element tables
Element Part(20): Original Shell element
Made 255 element tables
Element Part(19): Original Shell element
Made 850 element tables
Element Part(18): Original Shell element
Made 247 element tables
Element Part(17): Original Shell element
Made 89 element tables
Element Part(16): Brick element
Made 1471 element tables
Element Part(15): Brick element
Made 1471 element tables
Element Part(14): Brick element
Made 1471 element tables
Element Part(13): Brick element
Made 1471 element tables
Element Part(12): Brick element
Made 1471 element tables
Element Part(10): Brick element
Made 1471 element tables
Element Part(9): Brick element
Made 1471 element tables
Element Part(8): Brick element
Made 1471 element tables
Element Part(7): Brick element
Made 1471 element tables
Element Part(6): Brick element
Made 1471 element tables
Element Part(5): Brick element
Made 1471 element tables
Element Part(4): Brick element
Made 1471 element tables
Element Part(3): Brick element
Made 1471 element tables
Element Part(2): Brick element
Made 247540 element tables
Element Part(1): Brick element
Made 32087 element tables
Made 55 element parts

2015/02/15-11:10:40
Model [test.ds_data\1\ds] done

Autodesk (R) Simulation Surface Contact Management
Version 2015.01.00.0013-W64/X64 12-May-2014
Copyright (c) 2014, Autodesk, Inc. All rights reserved.

Model [test.ds_data\1\ds] opened for generating contact surfaces...
No general impact plane

Warning: Pressure point defined on element plane (EL#1 in EG#17)!

Warning: Pressure point defined on element plane (EL#1 in EG#18)!

Warning: Pressure point defined on element plane (EL#1 in EG#19)!

Warning: Pressure point defined on element plane (EL#1 in EG#20)!

Warning: Pressure point defined on element plane (EL#1 in EG#21)!

Warning: Pressure point defined on element plane (EL#1 in EG#22)!

Surface Set1: 7292 surfaces, 3893 surface nodes, EG=1, SID=15
Surface Set2: 6786 surfaces, 3539 surface nodes, EG=2, SID=19
Surface Set3: 96 surfaces, 60 surface nodes, EG=4, SID=4
Surface Set4: 116 surfaces, 72 surface nodes, EG=1, SID=13
Surface Set5: 96 surfaces, 60 surface nodes, EG=3, SID=4
Surface Set6: 116 surfaces, 72 surface nodes, EG=1, SID=14
Surface Set7: 96 surfaces, 60 surface nodes, EG=6, SID=4
Surface Set8: 116 surfaces, 72 surface nodes, EG=1, SID=11
Surface Set9: 96 surfaces, 60 surface nodes, EG=5, SID=4
Surface Set10: 116 surfaces, 72 surface nodes, EG=1, SID=12
Surface Set11: 96 surfaces, 60 surface nodes, EG=8, SID=4
Surface Set12: 116 surfaces, 72 surface nodes, EG=1, SID=9
Surface Set13: 96 surfaces, 60 surface nodes, EG=7, SID=4
Surface Set14: 116 surfaces, 72 surface nodes, EG=1, SID=10
Surface Set15: 96 surfaces, 60 surface nodes, EG=12, SID=4
Surface Set16: 116 surfaces, 72 surface nodes, EG=1, SID=7
Surface Set17: 96 surfaces, 60 surface nodes, EG=9, SID=4
Surface Set18: 116 surfaces, 72 surface nodes, EG=1, SID=8
Surface Set19: 97 surfaces, 62 surface nodes, EG=13, SID=4
Surface Set20: 116 surfaces, 72 surface nodes, EG=1, SID=5
Surface Set21: 96 surfaces, 60 surface nodes, EG=10, SID=4
Surface Set22: 116 surfaces, 72 surface nodes, EG=1, SID=6
Surface Set23: 96 surfaces, 60 surface nodes, EG=14, SID=4
Surface Set24: 116 surfaces, 72 surface nodes, EG=1, SID=3
Surface Set25: 96 surfaces, 60 surface nodes, EG=101, SID=4
Surface Set26: 116 surfaces, 72 surface nodes, EG=1, SID=4
Surface Set27: 100 surfaces, 66 surface nodes, EG=15, SID=4
Surface Set28: 116 surfaces, 72 surface nodes, EG=1, SID=2
Surface Set29: 96 surfaces, 60 surface nodes, EG=16, SID=4
Surface Set30: 116 surfaces, 72 surface nodes, EG=1, SID=1
Surface Set31: 30 surfaces, 30 surface nodes, EG=4, SID=3
Surface Set32: 8530 surfaces, 4512 surface nodes, EG=1, SID=20
Surface Set33: 30 surfaces, 30 surface nodes, EG=3, SID=3
Surface Set34: 30 surfaces, 30 surface nodes, EG=6, SID=3
Surface Set35: 30 surfaces, 30 surface nodes, EG=5, SID=3
Surface Set36: 30 surfaces, 30 surface nodes, EG=8, SID=3
Surface Set37: 30 surfaces, 30 surface nodes, EG=7, SID=3
Surface Set38: 30 surfaces, 30 surface nodes, EG=12, SID=3
Surface Set39: 30 surfaces, 30 surface nodes, EG=9, SID=3
Surface Set40: 30 surfaces, 30 surface nodes, EG=13, SID=3
Surface Set41: 30 surfaces, 30 surface nodes, EG=10, SID=3
Surface Set42: 30 surfaces, 30 surface nodes, EG=14, SID=3
Surface Set43: 30 surfaces, 30 surface nodes, EG=101, SID=3
Surface Set44: 30 surfaces, 30 surface nodes, EG=16, SID=3
Surface Set45: 30 surfaces, 30 surface nodes, EG=15, SID=3

2015/02/15-11:10:51
Model [test.ds_data\1\ds] closed

I don`t really know what the pressure points mean - since I did not define any pressure.

----------------------------------------------------------------------

Calculation:

Time Percent DT L Iter. Residual
0.00000000E+00 0.0000 0.050000 1 0 0.0000E+00
5.00000000E-02 5.0000 0.050000 1 1 1.0000E+00
5.00000000E-02 5.0000 0.050000 1 2 1.0000E+00
5.00000000E-02 5.0000 0.050000 1 3 1.0000E+00
5.00000000E-02 5.0000 0.050000 1 4 1.0000E+00
5.00000000E-02 5.0000 0.050000 1 5 5.0000E-03c
ERROR: Vector length = NaN Vector= NaN NaN
NaN
Possibly bad normal vector or guiding vector direction.
** Time step reduction due to: bad normal vector or guiding vector direction

I usually get this message.

--------------------------------------------------------------------

Final Resutls:

Somehow and for no reason, The contact does not happen on all bolts. The solver ignores some of the bolts - and this even happens on a slightly random fashion.

What is happening here? I already tried to make the mesh smaller, bigger, etc. The mesh seems to be of a reasonable size.

The weird thing is that if I change the mesh size, the bolts that do not get the contact change.

This is also true if I change the time steps for the calculation.

Any suggestions on what to do would be GREATLY appreciated.

Thanks a lot!

Re: Surface Contact of Bolts DO NOT WORK

AstroJohnPE — Mon, 16 Feb 2015 14:06:56 GMT

FYI: scudelari is performing a nonlinear analysis, possibly an MES (Mechanical Event Simulation), and therefore is using surface to surface contact.

The messages about the pressure point being defined in the plane of an element is a bit of a misnomer. It really means that the "Element Normal" coordinate defined in the Element Definition is in the plane of an element. The normal coordinate point determines which side of the shell element is the "top" and which is the "bottom". When the coordinate is in the plane of the element, the software cannot define the top and bottom. (Or maybe it randomly chooses which is the top and the bottom). See the page "Shell Elements" in the documentation, and the section "Control Orientation of Shell Elements" for a description of the element normal.

It is possible that the element normal is related to the error about the "bad normal vector". That error is related to the shell elements. I would suggest that you define the Element Normal coordinate for all of the shell parts so that the normal direction is consistent. Alternatively, use brick elements instead of shell element. I think shell elements are the most difficult element type to use in MES because of convergence.

The log file (.alg) lists all of the surface-to-surface contact pairs and the number of contact elements created. That list occurs after the list of "real" elements and just before the convergence information begins. That list of contact pairs might help to determine if a problem is occurring with elements getting created or not. The problem could be that elements are being created, but too few elements to resist the load that they need to transmit. So it is possible that the elements begin to transmit a load, have too much penetration, and then "stop working". You can look at the reaction forces to see if any contact occurs. Some things to try would be:

surface-to-surface contact comes in many varieties; namely, point-to-surface contact and surface-to-surface contact. Some definitions may work better in this model than others. (The differences affect how many contact elements are created between the two chosen surfaces). The page titled "Options" in the section "Surface-to-Surface Contacts" describes the differences between point-to-surface and surface-to-surface.
Change the contact stiffness and contact distance so that more force can develope in the contact elements.

If all else fails, create an archive of the model and attach it to a reply. Perhaps someone will have time to take a look and make suggestions. See the post "Create, Post, or Provide an Archive of your model".

Re: Surface Contact of Bolts DO NOT WORK

Anonymous — Tue, 17 Feb 2015 15:03:29 GMT

Hello Astrojohn,

Once again, you come for the rescue.

Indeed it is a Mechanical Event Simulation I am trying to accomplish.

I thank you very much for your help.

Forcing the definition of the Element normal solved the warnings - and also the "bad normal vector" error. Just for the sake of completeness, it was onyl concerning the shell parts that are in my model the long transversal ones. This is due to the fact that they lie on the ZX plane.

The contact was actually skipping the bolts due to the contact distance. More information may be found here:

http://help.autodesk.com/view/ASMECH/2015/ENU/?guid=GUID-489F3645-31BE-43D4-8992-6E8C181B38BA

The thing is that the hole was skipping the bolt on the first timestep and it was considered as never contacting.

I changed the value on the advanced tab to 5000mm (to force them to be verified at all times) and it did work.

Thanks a lot for your help, again, AstroJohn.

Re: Surface Contact of Bolts DO NOT WORK

Anonymous — Thu, 26 Feb 2015 14:43:11 GMT

AstroJohn, thank you for the information regarding pressure points. I've been getting those, but the pressure arrows applied on the shell elements look to be in the correct direction, and the analysis results seemed reasonable.

Scudelari, it looks like you may have shell elements interacting with brick elements. Did you get a chance to read the section regarding contacts between shell and brick elements,http://help.autodesk.com/cloudhelp/2015/ENU/SimMech/files/GUID-BFD9750D-ADD3-4C57-BA5A-3413C8AA5454.htm? There should be added features to the shell elements to transfer the forces through the different parts due to a difference in degrees of freedom.