Bolt connectors in PrePoMax?

[inquisitive_engineer]

Greetings!

I want to simulate bolt connectors in a simple plate tension test. How to do this in prepomax?

[FEAnalyst]

There’s no such predefined feature but you could define a beam element (through keyword editor because beams are not supported in GUI yet) and connect it to the rest of the model via rigid body constraints:

Modeling bolt connection with preloaded beam element

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 …

Connect rigid constraints with beam

Hello everyone. When I create rigid constraints and want to connect them to beam (via keywords). Bolt connection (similar to RBE2 with beams). Every rigid constraint has two control nodes, for translation and rotation. Do I need to create two beams? One beam between transformation control nodes and second between rotation nodes? *Rigid body, Nset=Internal_Selection-1_Rigid_Body-1, Ref node=2017, Rot node=2018 *Rigid body, Nset=Internal_Selection-1_Rigid_Body-2, Ref node=2019, Rot node=2020 *…

[inquisitive_engineer]

Thank you! i will check this out

[Paul18fr]

Hi,

I’m currently testing another way using DCOUP3D elements to mimic Rbe3 behavior. In the following screenshots, contact surfaces have been defined between the screw heads and the plate, but also between the plates themselves => in other words, the plates are only maintained by the contact.

However i’m facing 2 issues when applying temperature:

• I cannot impose a thermal scheme as i would like (see this post))
• error comes when using DCOUP3D elements with the temperature: i’ve to figure out if it’s a limitation, or something else

*ERROR in envtemp:
 *****number of network equations is not equal to
  number of active degrees of freedom*****
  # of network equations =           18
  # of active degrees of freedom=          679

Anybody would have recognized the FEAnalyst model (tutorial)

Still investigating …

[ANYS]

HI Paul18fr
Is your model constrained in any way in the z direction?
Regards

EDITED: Try to define the DCOUP 3D element initial temperatures with custom cards. It might be a problem similar to the one with compresion only in thermal analisys.

Compresion Only Support + Initial Temperature Field

Hi, When trying to define a Compression only support in presence of a Temperature Field ccx stops with the following message: *ERROR in checktemp: no initial temperature defined in node 2089 Is it possible that the new gapuny nodes are waiting for the initial temperature to be assigned?.

[FEAnalyst]

@Paul18fr

• error comes when using DCOUP3D elements with the temperature: i’ve to figure out if it’s a limitation, or something else

*ERROR in envtemp:
 *****number of network equations is not equal to
  number of active degrees of freedom*****
  # of network equations =           18
  # of active degrees of freedom=          679

Strange, such errors should normally happen for 1D fluid elements: Hydraulic analysis with split and joint - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).

But I guess DCOUP3D elements are indeed the culprit here.

[Paul18fr]

@ANYS: on the screw only, but not the plates.
Hare the 2 slave nodes are free following Z

Note the current model is a test : model link
(link available only 24 hours from now)

[ANYS]

Thanks.
I wasn’t able to preload without fixing at least one point in preload direction as you. Not big deal here.

I have finished recently the performance check of a similar model. Not detailed stresses at threads or heads, just overall tensile at the bolt shank and Contact preload pressure. FEA result compared against analytical calculation (*). Very good results.
My goal is now to check the Bolt Preload Change Due to Temperature. I got a “simple” example with analitical solution and methodology if you are interested. It would be applicable to your model so you could check your aproach performance. I’m using the model described in here as reference:

Bolted Connections

(*) VDI 2230 methodology as described in the book “Introduction to the Design & Behavior of Bolted Joints” by John H. Bickford

[Paul18fr]

@ANYS

the Bolt Preload Change Due to Temperature

that’s i would like to do too, but i’m facing difficulties (see previous post); if you’ve a look to the thermal expansion of the materials, the one of the bolt is twice of the plates => the tightening should decrease accordingly.

[ANYS]

@Paul18fr

the tightening should decrease accordingly

Hi,

¿How do you Know?

[Paul18fr]

@ANYS

¿How do you Know?

In the current model, with an uniform temperature and a screw that expands more than the plates => obviously the tightening (force) decreases …

[ANYS]

@Paul18fr

=> obviously the tightening (force) decreases

That’s true if the system is free to expand. But,… you have fixed the bottom and the preload reference node. That space in beteeen is not expanding freely.

[Paul18fr]

you’re right for the current BCs

[ANYS]

Not easy subject. I’m strugling too. So much parameters for a single bolt,

. I think I now have them all. (Different book different names and letter)
.
I need to simplify. .
Tomorrow.