Modeling bolt connection with preloaded beam element

General Questions
1

Hi everybody,
it’s my first time here so i’d like, first, to say thank you to the people that are improving the software.
I’m planning to test this software in some jobs where i’m using Ansys (some simple structures). The future objective is to use PrePoMax in the early stage of the design and Ansys only for the final checks.
The software has almost all the needed features, the only thing that is missing is the design of bolt connections. I’m tryng to create the missing parts with the editor (Model → Edit Calculix Keyword) but I have some problems.
In Ansys I use spring elements with preload and Cylindrical Joint (it’s basically a rigid radial connection) to simulate the bolt connection.

01_mod
01_mod1688×904 155 KB

03B_mod
03B_mod1483×897 179 KB

In PrePoMax I’m plannig to use the beam element with preload instead of the spring (for the Cylindrical Joint I’ll think how to do later).
I created a model and changed the script using the file in this video as reference (https://www.youtube.com/watch?v=VA0eg0LWfWM&t=783s) but the analisys has some issue and I can’t find the problem.
Can someone help me? On the forum I saw that no one indicated the entire procedure to follow, which I would like to describe.
BoltConnectionDesign.pmx (849.9 KB)

1 Like
2

You should make sure that it works with beam elements without pre-tension first (pre-tension with beams in CalculiX is tricky as those elements are deleted internally). It seems that the model is underconstrained. Also, the beams are misplaced.

BoltConnectionDesign_mod.pmx (322.1 KB)

3

Something similar is used in the Nastran world for aircraft structures. The fasteners are modeled using springs/beams and it is connected to the mesh directly (or to the hole border) using interpolation elements. I would like to see this in PrePoMax in the future!

“Sealing” connection in Hypermesh:
image

Same for OptiStruct:
image

4

Good evening FEAnalyst,
I checked at first the correct position of the beams but I changed so many things tryng to solve this problem that it seams I made some mystakes with the nodes in the last try.
By the way even with the correct beams position the anlaysis is a failure.
In the different attempts I found that changing the reference nodes in the load:
*Cload
5678,1,80000
5679,1,80000

with, for example, existing nodes (I know that is not correct):
*Cload
678,1,80000
679,1,80000
I obtain some results (even if they are obviously incorrect).
Isn’t that strange?
Attached the PrePoMax with preload activated and Cload “wrongly” changed (if you insert the reference nodes you’ll see that the analysis is a failure).
BoltConnectionDesign_mod2.pmx (543.0 KB)

P.S.1: In Ansys with the same restrain the system is not underconstrained (but I added some other restrain, I’m more interested in find the problem with the pretension at the moment)
P.S.2: I watched all your videos on youtube, they are really well made

5

*CLOAD should be applied to the reference node of the pre-tension section. Maybe there’s an issue with the way those beam elements are attached to the solid model. CalculiX documentation suggests distributing coupling and equation constraints for that. There’s a simple example that you can try first:

**
**   Structure: bolt-like structure.
**   Test objective: pre-tension force with beam element.
**
*NODE, NSET=Nall
       1,0.000000000000e+00,0.000000000000e+00,0.000000000000e+00
       2,0.000000000000e+00,1.000000000000e+00,0.000000000000e+00
       3,2.000000000000e-01,1.000000000000e+00,0.000000000000e+00
       4,2.000000000000e-01,0.000000000000e+00,0.000000000000e+00
       5,1.414213562373e-01,0.000000000000e+00,-1.414213562373e-01
       6,1.414213562373e-01,1.000000000000e+00,-1.414213562373e-01
       7,1.000000000000e+00,1.000000000000e+00,0.000000000000e+00
       8,1.000000000000e+00,0.000000000000e+00,0.000000000000e+00
       9,7.071067811865e-01,0.000000000000e+00,-7.071067811865e-01
      10,7.071067811865e-01,1.000000000000e+00,-7.071067811865e-01
      11,2.000000000000e-01,5.000000000000e-01,0.000000000000e+00
      12,1.847759065023e-01,0.000000000000e+00,-7.653668647302e-02
      13,1.414213562373e-01,5.000000000000e-01,-1.414213562373e-01
      14,1.847759065023e-01,1.000000000000e+00,-7.653668647302e-02
      15,6.000000000000e-01,1.000000000000e+00,0.000000000000e+00
      16,6.000000000000e-01,0.000000000000e+00,0.000000000000e+00
      17,4.242640687119e-01,0.000000000000e+00,-4.242640687119e-01
      18,4.242640687119e-01,1.000000000000e+00,-4.242640687119e-01
      19,1.000000000000e+00,5.000000000000e-01,0.000000000000e+00
      20,9.238795325113e-01,0.000000000000e+00,-3.826834323651e-01
      21,7.071067811865e-01,5.000000000000e-01,-7.071067811865e-01
      22,9.238795325113e-01,1.000000000000e+00,-3.826834323651e-01
      23,2.775557561563e-17,0.000000000000e+00,-2.000000000000e-01
      24,2.775557561563e-17,1.000000000000e+00,-2.000000000000e-01
      25,2.220446049250e-16,0.000000000000e+00,-1.000000000000e+00
      26,2.220446049250e-16,1.000000000000e+00,-1.000000000000e+00
      27,7.653668647302e-02,0.000000000000e+00,-1.847759065023e-01
      28,2.775557561563e-17,5.000000000000e-01,-2.000000000000e-01
      29,7.653668647302e-02,1.000000000000e+00,-1.847759065023e-01
      30,1.249000902703e-16,0.000000000000e+00,-6.000000000000e-01
      31,1.249000902703e-16,1.000000000000e+00,-6.000000000000e-01
      32,3.826834323651e-01,0.000000000000e+00,-9.238795325113e-01
      33,2.220446049250e-16,5.000000000000e-01,-1.000000000000e+00
      34,3.826834323651e-01,1.000000000000e+00,-9.238795325113e-01
      35,-1.414213562373e-01,0.000000000000e+00,-1.414213562373e-01
      36,-1.414213562373e-01,1.000000000000e+00,-1.414213562373e-01
      37,-7.071067811865e-01,0.000000000000e+00,-7.071067811865e-01
      38,-7.071067811865e-01,1.000000000000e+00,-7.071067811865e-01
      39,-7.653668647302e-02,0.000000000000e+00,-1.847759065023e-01
      40,-1.414213562373e-01,5.000000000000e-01,-1.414213562373e-01
      41,-7.653668647302e-02,1.000000000000e+00,-1.847759065023e-01
      42,-4.242640687119e-01,0.000000000000e+00,-4.242640687119e-01
      43,-4.242640687119e-01,1.000000000000e+00,-4.242640687119e-01
      44,-3.826834323651e-01,0.000000000000e+00,-9.238795325113e-01
      45,-7.071067811865e-01,5.000000000000e-01,-7.071067811865e-01
      46,-3.826834323651e-01,1.000000000000e+00,-9.238795325113e-01
      47,-2.000000000000e-01,0.000000000000e+00,-8.326672684689e-17
      48,-2.000000000000e-01,1.000000000000e+00,-8.326672684689e-17
      49,-1.000000000000e+00,0.000000000000e+00,-2.775557561563e-16
      50,-1.000000000000e+00,1.000000000000e+00,-2.775557561563e-16
      51,-1.847759065023e-01,0.000000000000e+00,-7.653668647302e-02
      52,-2.000000000000e-01,5.000000000000e-01,-8.326672684689e-17
      53,-1.847759065023e-01,1.000000000000e+00,-7.653668647302e-02
      54,-6.000000000000e-01,0.000000000000e+00,-1.804112415016e-16
      55,-6.000000000000e-01,1.000000000000e+00,-1.804112415016e-16
      56,-9.238795325113e-01,0.000000000000e+00,-3.826834323651e-01
      57,-1.000000000000e+00,5.000000000000e-01,-2.775557561563e-16
      58,-9.238795325113e-01,1.000000000000e+00,-3.826834323651e-01
      59,-1.414213562373e-01,0.000000000000e+00,1.414213562373e-01
      60,-1.414213562373e-01,1.000000000000e+00,1.414213562373e-01
      61,-7.071067811865e-01,0.000000000000e+00,7.071067811865e-01
      62,-7.071067811865e-01,1.000000000000e+00,7.071067811865e-01
      63,-1.847759065023e-01,0.000000000000e+00,7.653668647302e-02
      64,-1.414213562373e-01,5.000000000000e-01,1.414213562373e-01
      65,-1.847759065023e-01,1.000000000000e+00,7.653668647302e-02
      66,-4.242640687119e-01,0.000000000000e+00,4.242640687119e-01
      67,-4.242640687119e-01,1.000000000000e+00,4.242640687119e-01
      68,-9.238795325113e-01,0.000000000000e+00,3.826834323651e-01
      69,-7.071067811865e-01,5.000000000000e-01,7.071067811865e-01
      70,-9.238795325113e-01,1.000000000000e+00,3.826834323651e-01
      71,-1.110223024625e-16,0.000000000000e+00,2.000000000000e-01
      72,-1.110223024625e-16,1.000000000000e+00,2.000000000000e-01
      73,-4.440892098501e-16,0.000000000000e+00,1.000000000000e+00
      74,-4.440892098501e-16,1.000000000000e+00,1.000000000000e+00
      75,-7.653668647302e-02,0.000000000000e+00,1.847759065023e-01
      76,-1.110223024625e-16,5.000000000000e-01,2.000000000000e-01
      77,-7.653668647302e-02,1.000000000000e+00,1.847759065023e-01
      78,-2.775557561563e-16,0.000000000000e+00,6.000000000000e-01
      79,-2.775557561563e-16,1.000000000000e+00,6.000000000000e-01
      80,-3.826834323651e-01,0.000000000000e+00,9.238795325113e-01
      81,-4.440892098501e-16,5.000000000000e-01,1.000000000000e+00
      82,-3.826834323651e-01,1.000000000000e+00,9.238795325113e-01
      83,1.414213562373e-01,0.000000000000e+00,1.414213562373e-01
      84,1.414213562373e-01,1.000000000000e+00,1.414213562373e-01
      85,7.071067811865e-01,0.000000000000e+00,7.071067811865e-01
      86,7.071067811865e-01,1.000000000000e+00,7.071067811865e-01
      87,7.653668647302e-02,0.000000000000e+00,1.847759065023e-01
      88,1.414213562373e-01,5.000000000000e-01,1.414213562373e-01
      89,7.653668647302e-02,1.000000000000e+00,1.847759065023e-01
      90,4.242640687119e-01,0.000000000000e+00,4.242640687119e-01
      91,4.242640687119e-01,1.000000000000e+00,4.242640687119e-01
      92,3.826834323651e-01,0.000000000000e+00,9.238795325113e-01
      93,7.071067811865e-01,5.000000000000e-01,7.071067811865e-01
      94,3.826834323651e-01,1.000000000000e+00,9.238795325113e-01
      95,1.847759065023e-01,0.000000000000e+00,7.653668647302e-02
      96,1.847759065023e-01,1.000000000000e+00,7.653668647302e-02
      97,9.238795325113e-01,0.000000000000e+00,3.826834323651e-01
      98,9.238795325113e-01,1.000000000000e+00,3.826834323651e-01
99,0.,0.,0.
100,0.,0.,0.
101,0.,0.,0.
*ELEMENT, TYPE=B31, ELSET=Ebeam
     1,      1,      2
*ELEMENT, TYPE=C3D20R, ELSET=Evol
     2,     3,     4,     5,     6,     7,     8,     9,    10,    11,    12,
          13,    14,    19,    20,    21,    22,    15,    16,    17,    18
     3,     6,     5,    23,    24,    10,     9,    25,    26,    13,    27,
          28,    29,    21,    32,    33,    34,    18,    17,    30,    31
     4,    24,    23,    35,    36,    26,    25,    37,    38,    28,    39,
          40,    41,    33,    44,    45,    46,    31,    30,    42,    43
     5,    36,    35,    47,    48,    38,    37,    49,    50,    40,    51,
          52,    53,    45,    56,    57,    58,    43,    42,    54,    55
     6,    48,    47,    59,    60,    50,    49,    61,    62,    52,    63,
          64,    65,    57,    68,    69,    70,    55,    54,    66,    67
     7,    60,    59,    71,    72,    62,    61,    73,    74,    64,    75,
          76,    77,    69,    80,    81,    82,    67,    66,    78,    79
     8,    72,    71,    83,    84,    74,    73,    85,    86,    76,    87,
          88,    89,    81,    92,    93,    94,    79,    78,    90,    91
     9,    84,    83,     4,     3,    86,    85,     8,     7,    88,    95,
          11,    96,    93,    97,    19,    98,    91,    90,    16,    15
*ELEMENT,TYPE=DCOUP3D,ELSET=Ecoup1
10,100
*ELEMENT,TYPE=DCOUP3D,ELSET=Ecoup2
11,101
*MATERIAL,NAME=EL
*ELASTIC
210000.,.3
*SOLID SECTION,ELSET=Evol,MATERIAL=EL
*BEAM SECTION,ELSET=Ebeam,MATERIAL=EL,SECTION=RECT
0.001,0.001
0.,0.,1.
*PRE-TENSION SECTION,ELEMENT=1,NODE=99
0.,1.,0.
*NSET,NSET=FIX
49,68,61,80,73,92,85,97,8,20,9,32,25,44,37,56
*NSET,NSET=Ncoup1
5,12,4,95,83,87,71,75,59,63,47,51,35,39,23,27
*NSET,NSET=Ncoup2
6,14,3,96,84,89,72,77,60,65,48,53,36,41,24,29
*BOUNDARY
FIX,1,3
*DISTRIBUTING COUPLING,ELSET=Ecoup1
Ncoup1,1.
*DISTRIBUTING COUPLING,ELSET=Ecoup2
Ncoup2,1.
*EQUATION
2
100,1,1.,1,1,-1.
2
100,2,1.,1,2,-1.
2
100,3,1.,1,3,-1.
*EQUATION
2
101,1,1.,2,1,-1.
2
101,2,1.,2,2,-1.
2
101,3,1.,2,3,-1.
*STEP
*STATIC
*CLOAD
99,1,1.
*NODE PRINT,NSET=Nall
U
*NODE PRINT,NSET=Ncoup1,TOTALS=YES
RF
*NODE PRINT,NSET=Ncoup2,TOTALS=YES
RF
*END STEP
6

Ah! ok… reading the “.inp” file I associated the *EQUATION at a sort of “rigid link” between the edge of the hole and the node of the beam so I didn’t added it (for that I have the constraints “BOLT-B-1-RIGID”, “BOLT-B-2-RIGID”,… ).

If it’s as you say, well, that is something so unfriendly that is basically unusable for my projects where I have at the minimum 10/15 bolts.

Without even the graphic visualization of the bolt and the preload for a check of the input data and, I suppose, the possibility to check the preload in the bolt after the analysis (as you said the bolt is deleted after the analysis).

My only hope is that mr. Matej will consider in the future to implement these two features (bolt with preload and cylindrical joint).

I’ll write something in the relative section.

Thankyou very much for the help.

7

You can still try with just the rigid body constraint, possibly using a very simple model like a single brick/cylinder or two such parts connected together. But it may not work properly and there are still the limitations of pre-tension with beam elements. So all in all, it might be best to just model the bolts as solids.

Those might be better as feature requests for CalculiX. Especially improved preloaded bolts. You could ask Guido (CalculiX) dev about it or post here: GitHub - Dhondtguido/CalculiX: This repository contains the source files of CalculiX, a three-dimensional Finite Element Program (www.calculix.de).

8

Thank you, that’s a great idea… I’ll do as you suggest…

good night

9

Side note, by using solid elements and connecting the bolt head to the shaft with tied contact, you can use the History output to get the summed up normal/shear loads + moments for the slave surface.

9
92068×732 102 KB

2 Likes
10

That’ really interesting Gunnar.
Can you please share the .pmx file?

11

Sure
BoltConnectionDesign_solid-bolt.pmx (352.3 KB)

It would be nice if you could run the same simulation with Ansys for comparing the results (I’m just interested in the beam forces + moments in the bolt head region) and how many iterations Ansys needs per time step (with default settings and similar mesh).

Thank you

12

Very interesting and stable. May I ask you why you define two rigid bodies with the same Ref ?. Is it a Prpomax limitation?

You could save the contact definition requesting the SOF SOM directly at the internal surface. I will try to do it with Prepomax. Calc_em proposed a workaround on the Calculix forum.

13

True this is just a habit and not necessary at all.

That’s definitely just as good, but i prefer to work with the gui only if possible and have all results available in prepomax.

Thanks for the tips.

14

Hello everyone!

I trying to prepare very simple model of bolt on two plates with pretension using beam (B31) element and Rigid Body constraint to simulate connection between edge of hole.

image
image596×783 105 KB

Unfortunately my model is still not working correctly and can’t convergence when I apply preload on bolt. Without preload and with additional force on side face in reference point the bolt simplification works fine.

**
** Heading +++++++++++++++++++++++++++++++++++++++++++++++++
**
*Heading
Hash: hOLqPOZO, Date: 06/10/2024, Unit system: MM_TON_S_C
**
** Nodes +++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Node
4096, 2.49998671E+001, 2.50000080E+001, 5.00011796E+000
4097, 2.49998671E+001, 2.50000080E+001, 5.00011796E+000
4098, 2.49998671E+001, 2.50000080E+001, 1.50001180E+001
4099, 2.49998671E+001, 2.50000080E+001, 1.50001180E+001
4100, 5.00000000E+001, 2.50000000E+001, 1.50000000E+001
4101, 5.00000000E+001, 2.50000000E+001, 1.50000000E+001
**
** Elements ++++++++++++++++++++++++++++++++++++++++++++++++
**
*Element, Type=C3D4, Elset=Solid_part-2
**
** Node sets +++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Element sets ++++++++++++++++++++++++++++++++++++++++++++
**
**
** Surfaces ++++++++++++++++++++++++++++++++++++++++++++++++
**
*Surface, Name=Surface-1, Type=Element
Internal-1_Surface-1_S4, S4
Internal-1_Surface-1_S1, S1
Internal-1_Surface-1_S3, S3
Internal-1_Surface-1_S2, S2
*Surface, Name=Surface-2, Type=Element
Internal-1_Surface-2_S4, S4
Internal-1_Surface-2_S1, S1
Internal-1_Surface-2_S3, S3
Internal-1_Surface-2_S2, S2
*Surface, Name=Internal_Selection-1_Contact_Pair-1_Master, Type=Element
Internal-1_Internal_Selection-1_Contact_Pair-1_Master_S1, S1
Internal-1_Internal_Selection-1_Contact_Pair-1_Master_S4, S4
Internal-1_Internal_Selection-1_Contact_Pair-1_Master_S2, S2
Internal-1_Internal_Selection-1_Contact_Pair-1_Master_S3, S3
*Surface, Name=Internal_Selection-1_Contact_Pair-1_Slave, Type=Element
Internal-1_Internal_Selection-1_Contact_Pair-1_Slave_S3, S3
Internal-1_Internal_Selection-1_Contact_Pair-1_Slave_S4, S4
Internal-1_Internal_Selection-1_Contact_Pair-1_Slave_S2, S2
Internal-1_Internal_Selection-1_Contact_Pair-1_Slave_S1, S1
*Surface, Name=Surface-3, Type=Element
Internal-1_Surface-3_S3, S3
Internal-1_Surface-3_S4, S4
Internal-1_Surface-3_S2, S2
Internal-1_Surface-3_S1, S1
**
** Physical constants ++++++++++++++++++++++++++++++++++++++
**
**
** Materials +++++++++++++++++++++++++++++++++++++++++++++++
**
*Material, Name=S355
*Density
7.8E-09
*Elastic
210000, 0.28
*Expansion, Zero=20
1.1E-05
*Conductivity
14
*Specific heat
440000000
**
** Sections ++++++++++++++++++++++++++++++++++++++++++++++++
**
*Solid section, Elset=Internal_Selection-1_Solid_Section-1, Material=S355
*ELEMENT,TYPE=B31,ELSET=B1
15769,4096,4098
*BEAM SECTION,MATERIAL=S355,ELSET=B1,SECTION=RECT
12.,12.
0,1,0
*Node
4102, 25., 25., 10.
*PRE-TENSION SECTION,ELEMENT=15769,NODE=4102
0.,0.,1.
**
** Pre-tension sections ++++++++++++++++++++++++++++++++++++
**
**
** Constraints +++++++++++++++++++++++++++++++++++++++++++++
**
*Rigid body, Nset=Node_Set-11, Ref node=4096, Rot node=4097
*Rigid body, Nset=Node_Set-21, Ref node=4098, Rot node=4099
*Rigid body, Nset=Internal-1_Surface-3, Ref node=4100, Rot node=4101
**
** Surface interactions ++++++++++++++++++++++++++++++++++++
**
*Surface interaction, Name=Surface_Interaction-1
*Surface behavior, Pressure-overclosure=Linear
1050000, 2.86
*Friction
0.1
**
** Contact pairs +++++++++++++++++++++++++++++++++++++++++++
**
*Contact pair, Interaction=Surface_Interaction-1, Type=Surface to surface
Internal_Selection-1_Contact_Pair-1_Slave, Internal_Selection-1_Contact_Pair-1_Master
**
** Amplitudes ++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Initial conditions ++++++++++++++++++++++++++++++++++++++
**
**
** Steps +++++++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Step-1 ++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Step, Nlgeom, Inc=50
*Static, Solver=PaStiX
0.01, 1, 1E-05, 1E+30
**
** Controls ++++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Output frequency ++++++++++++++++++++++++++++++++++++++++
**
*Output, Frequency=1
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
**
*Boundary, op=New
** Name: Fixed-1
*Boundary
Internal_Selection-1_Fixed-1, 1, 6, 0
** Name: Displacement_Rotation-1: Deactivated
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Cload, op=New
*Dload, op=New
** Name: Concentrated_Force-1: Deactivated
** Name: Pretension
*Cload
4102, 1, 1000
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
**
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
*Node file
RF, U
*El file
S, E, NOE
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step

Please see attached file in link below:

15

From the documentation on the *PRE-TENSION SECTION:

To this end the nodes of the beam element (e.g. representing a bolt) should be connected by linear equations or a *DISTRIBUTING COUPLING card to nodes of the structures to be held together.

So I would use the approach shown in this documentation example (also to avoid the issues with ROT NODE): Modeling bolt connection with preloaded beam element - #5 by FEAnalyst

And it seems to be working here:

Test Bolt B31_mod.pmx (6.4 MB)

16

Thanks for explanation! I have changed the model according to your tip but without this *EQUATION keyword and it is work fine I think.

In general I don’t understand this *EQUATION mechanism even after lecture of USER’S MANUAL. I know that it is merging the nodes or something similar but the command syntax is not clear for me.

Now I am trying to activate Concentrated_Force-1 on Reference_Point-3 to act shear on this connection but then model is not converagnance. It seems like the connection of bolt (simplified by the beam) is not acting in this direction.

Is it necessary to duplicate the nodes on the end of the beam merge those nodes with the exciting reference points and then model additional connection between those nodes and edge of the hole? How to handle this?

Test Bolt B31_v1.pmx (5.3 MB)

17

The *EQUATION constraint connects the nodal degrees of freedom (not the nodes themselves physically) with a user-defined relation. In the majority of cases (including the one discussed here), it’s used to make the degrees of freedom equal for 2 nodes so they can move together (even if they are not in the same position). Here it’s helpful because it lets you avoid the issues due to various limitations when trying to use the same nodes for beam and “spiders” connecting it to the rest of the model.

For some forms of loading and usage cases you may need more sophisticated approach. This one is highly simplified as the beam element is connected to the model only at the top and bottom surfaces, not along the whole shank. Moreover, the beam element is deleted internally and replaced with a special type of constraint when using the pre-tension section. So you can extract the results from it or apply other loads, for instance.

More common and versatile approach is to model the bolt as a simple solid part (cylinder or multiple cylinders). Then you can use pre-tension but also account for contact between the bolt and the plates when e.g. shearing the joint.

1 Like
18

Thank you for explanation. I have added *EQUATION to my model and it works fine.

Furthermore I have duplicate the reference points and the beam then connect those nodes with nodes set with is on the opposite side of hole. This operation leads model to convergence even with additional shear force on sidewall of the plate. Unfortunately this approach is far from ideal especially with bigger model because of quite complicated input method. The outcomes of stress are also not perfect in area of bolt but in general it is possible to extract the forces in the bolt and verify connection by code procedure. I am not sure if my approach to model this connection way is wrights here. It feels like for sure that is not the easiest way but is there is any other simplification of this kind of connection with beam as bolt?

Model bolts as solids is not what I prefers because it leeds model to be very heavy and hard to compute on my hardware. The idea of simplified bolt like in Inventor Nastran is very useful in some situations and it would be very nice to see this kind of features in some next versions of PrePoMax.

https://help.autodesk.com/view/NINCAD/2024/ENU/?guid=GUID-DE94AF96-28B9-40B0-AE30-5D19798A5D18

image
image1133×850 134 KB

My current model is linked below.

Test Bolt B31_v2.pmx (5.3 MB)

1 Like
19

One more improvement you could make right away would be to connect the “spider” to annular surface partition on each side instead of using just the edges of the hole.

In the book “Practical Finite Element Analysis for Mechanical Engineers” by D. Madier, you can find a nice summary of different approaches to bolt modelling in FEA.

1 Like