Bolt Connector in Shear has very high Displacement

[Anonymous]

Hello All,

I posted an issue earlier regarding bolt connector displacement, and I wanted to revisit it for bolts in shear.  I made 2 test blocks with bolt holes and ran two analyses.  The first was using the Nastran Bolt Connector between the two blocks, where full fixed one end of the block and applied a 1000 lbf load perpendicular to the axis of the bolt.  The displacement of the blocks was 0.0220" .  This seems like a unrealistically large amount.  

I retried the same  analysis but made a part to represent the bolt,  and applied separation contacts except for the threaded section where it is bonded.  I applied the same 1000 lbf load and it only displaced 0.0002".

Is there a reason or an adjustable setting that the bolt connector is displacing so much compared to a physical part?

Regards,

Derek

[KubliJ]

Hi @Anonymous,

The simplified beam bolt is not actually making contact with the inside walls of the plate.  So the displacement and stress around the bolt hole on the plate will be inaccurate.  But the stresses of the bolt should be correct.  The shear stress should match the solid model.

Thanks,
James

[Anonymous]

Hello James,

Thank you for the reply.  Unfortunately my core issue is with the displacement.  I have an assembly where a circular bolt pattern is transferring torque from one plate to another (through shear load of the bolt).  I keep getting a singularity, which I believe is a result of the high displacement of the bolts.  The shear displacement for the simulated bolt connector was 100x the shear displacement of the physical bolt part.  

I tried this same test with the load in the direction of the bolts axis (pure tension) and the results between the connector and the physical part was very similar and matched my hand calculations.  Thus it seems like the tension displacement is accurate while the shear displacement is not.

I am wanting to know if this can be fixed or if there is a an adjustable setting that allows for the connectors rigidity in the shear direction to be increased. 

Regards,

Derek.

[John_Holtz]

Hi @Anonymous,

My guess is that the shear modulus is too low in the model with the beam elements used to simulate the bolt; hence, the large displacement in the shear direction.

When you write that you are getting a singularity,

• are you referring to the type that causes a high stress at some nodes? (That is not directly related to the displacements but more to the force transmitted through the nodes.) Maybe you need a finer mesh around the bolt hole so that there are more beam element "spokes" connecting the bolt shank to the model? 
• Or are you referring to the analysis will not solve because of a singularity in the stiffness matrix? (The matrix singularity is probably not caused by the beam elements. They should make the model more statically stable because it connects parts together rigidly.)

[Anonymous]

Hello John,

I believe that my assembly is statically stable because when I bond the two surfaces that are supposed to be bolted together, the analysis solves and give a reasonable result.  If I let the bolt connectors carry the torque, either I get Fatal Error E5004: Stiffness Matrix Singular or Non-Positive Definite or the solution complete with the bolts not transferring the torque to the next plate (the output plate gets no reaction torque and the input plate gets distorted).

Regards,

Derek

[John_Holtz]

Hi,

Without having either of your models (the bolt shear test model or the real model), the following is just a guess. But I think you are encountering two different issues which are probably unrelated:

1. The shear displacement in the beam elements is larger in the test model than expected (0.022 instead of 0.002). The solid bolt model and beam bolt model must be different, either because of material properties or because the setup is different (such as the contact).
2. A singularity error in the real model. The displacement on the order of 0.022 is not a large displacement that would cause the analysis to think there was a singularity. Did the analysis converge? Or did it fail to converge and the results that are shown are garbage?

I assume that your test model and real model are using separation contact between the two plates. Another test that you can perform (in either the test model or real model) is to use no separation contact in the model and let all of the load transfer through the bolts (either idealized as beam elements or as solid). These results should be similar and eliminate the complication of separation contact. If these results are vastly different, there is either a problem with the material properties or the cross-section of the beam.

I had a similar solid versus beam test model until Inventor crashed Thankfully I saved some images of the results. (My model dimensions and loads are completely different, so we cannot compare the displacement of my model to your model, but the comparison between solid and beam should be valid.)

Idealization for bolt	Derek’s model	John’s model
Solid	0.0002 displacement total	0.0022 displacement in shear direction
Beam	0.022	0.0026
Beam/Solid	110x	1.18x

This is the contact that I defined in my model which creates identical analyses between the model with the solid bolt and the model with the beam bolt:

• cap screw threaded into bottom plate (beam model)
• bonded contact between bolt threads and bottom plate (solid model)
• bonded contact between bolt head and plate (solid model)
• separation contact between face of plates (both models)
• no contact between the body of the bolt and the top plate.

John's bolt model

Now that I look at your images, I am not sure what type of bolt you are simulating (bolt and nut or cap screw) and whether you are using separation contact between the body of the bolt and the bolt hole. Even if you defined separation contact between the beam element bolt and the sides of the hole (and entered the appropriate "penetration offset"), the beam element is not going to make contact with the side of the hole because there are no nodes along the length of the beam element to come into contact with the hole. (This is what James was indicating in his reply.)

I was seeing a slight difference in my results with the beam element bolt depending on how I created the bolt, but the differences were a factor of 2 in the displacement, not a factor of 100:

• larger displacement if the bolt head was defined using the edge of the hole instead of a face that represented the washer/bolt head area. Fewer "spokes" to the surface of the plate allow more rotation of the beam element which increases the displacement.
• larger displacement if the bolt "Useful length" was blank instead of using a value of 0. This increases the length of the beam element which gives a larger displacement.

I still think that the material properties for the beam element bolt must be having some effect in your analysis. If you edit the .log file, are there any warnings about the material properties? (The end of the .log file has a nice summary of the warnings and errors in the analysis.)